if both individuals are feasible, the one with the best
 objective function value is chosen;

if both individuals are unfeasible, the one with the least
 violation of the constraints is preferred.



No penalty factor is required, since the
selection procedure only performs pairwise comparisons.


This technique has demonstrated to be successful [15],
especially in providing feasible solutions in highly constrained
problems. But as a drawback, the optimizer might focus in local
extrema too rapidly if the design space is scarcely populated, thus it
is strongly suggested to use as many as possible samples so that
multiple extrema (if they exist) are well represented. This method
always privileges feasible solutions and is generally more likely to
converge towards a feasible solution.


The main difficulty in handling constraints by using penalty methods
in EAs and more generally in classical optimization methods, is to
set appropriate values for the penalty parameters. Most of the time,
this requires the user to experiment with different values of
parameters. The Deb's constraint handling method is thus recommended
as it does not require any penalty parameter. With this technique,
infeasible solutions are penalized in a way so as to provide a search
direction towards the feasible region. 

For MINAMO in FINE™/Design3D, these options are available via the EA Settings tab in the Expert Mode. Four Constraint Handling Methods are available:



Tournament [default]

Static Penalty

Dynamic Penalty

Adaptive Penalty




FIGURE 3 Constraint Management Settings.

Mono-objective evolutionary
algorithms (EAs)


A genetic algorithm (GA) is a search
heuristic that mimics the process of natural evolution. Genetic
algorithms belong to the larger class of evolutionary algorithms
(EAs), which generate solutions to
optimization problems using techniques inspired by natural evolution,
such as inheritance, mutation, selection, and crossover. Genetic
algorithms were designed by Holland in the 70s, and improved and made
well known by Goldberg in the 80s [2]. Genetic
Algorithms are becoming more and more widely used in mechanical
and aerodynamic problems, e.g. preliminary design of turbines
[3], aerodynamic optimization using CFD [4]
[5] [6] [7]
[8], optimization of target pressure distributions for
inverse design methods [9] [10], multi-objective
aerodynamic shape optimization [11].



Genetic algorithms mimic natural behavior in terms of
biological evolution in order to reach the best possible solution to a
given problem. Weak individuals tend to die before reproducing, while
the stronger ones live longer and bear many offsprings, who often
inherit the qualities that enabled their parents to survive. 
A genetic algorithm is summarized as in FIGURE 1. 



An initial population is generated by randomly (or by using Design of
Experiments) selecting individuals in the whole design space. Then,
pairs of individuals are selected from this population based on their
objective function values. The performance of an individual is
measured by its fitness. Then, each pair of individuals undergoes a
reproduction mechanism to generate a new population in such a way that
fitter individuals will spread their genes with higher probability.
The children replace their parents. As this proceeds, inferior traits
in the pool die out due to lack of reproduction. At the same time,
strong traits tend to combine with other strong traits to produce
children who perform better.



The reproduction cycle is governed by genetic operators. Numerous
genetic operators have been proposed in the literature. Three of them
are used here, namely: selection, recombination, and mutation
operators. 


FIGURE 1 Evolutionary algorithm scheme.

The selection operator chooses two
 individuals from the population that will mate to generate an
 offspring. MINAMO implements different selection operators
 (tournament selection), which are probabilistically chosen along
 with a recombination operator as described below.


The recombination operators take
 two individuals selected by the selection operator and will be mated
 to generate an offspring, which tends to preserve the favorable
 characteristics of the parent individuals. A special attention is
 paid to the construction of the recombination algorithm so that it
 does not degrade the diversity of the population excessively. In
 MINAMO, selection and recombination operators are
 probabilistically chosen to form a pair of operators that are
 combined to generate an offspring.


Mutation introduces new genetic
 material into a heterogeneous population. The mutation operator
 implemented in MINAMO introduces a perturbation to each design
 parameter with a small probability. This genetic operator is a key
 feature for avoiding local optima traps.




An elitism mechanism is also adopted to ensure
the best individuals of the current population are not lost. By
default in MINAMO, the two best individuals are copied to the next
population. 


In MINAMO, a real number coding has been chosen because it allows
using an easy and compact form to represent an individual. In the rest
of this document, our real-coded genetic algorithm will be denoted by
Evolutionary Algorithm (EA). 

Evolutionary Algorithm options

For MINAMO in FINE™/Design3D, the EA-related options are available via the EA Settings tab.



FIGURE 2  
Standard Mode 

Number of Generations: This is the number of generations which will be processed by the EA on the
surrogate models. The number should be at least 50 [default = 100].

Population Size: This is the number of individuals present in a population during the EA
process on the surrogate models. It is suggested to set this number sufficiently large so that the EA can safely find the design update without a risk of missing a potential optimum point. The number should be at least 50 as a rule of thumb, and preferably as large as 200 [default = 400].

Mutation Probability: The mutation is a genetic operator used to maintain genetic diversity into the
population. It allows the algorithm to avoid local optima by preventing the population of individuals from becoming too similar to each other, thus slowing or even stopping the evolution. Typically, mutation is given a fairly low probability of occurrence. The default value for the mutation probability is 0.01 (probability of 1%).


Expert Mode

Elitism: Number of elites in the elitism mechanism [default = 2]

Tournament Order: Number of tournaments to select the individuals [default = 2]

Number of Parents: Number of parents selected for the reproduction process [default = 2]

Forced Elitism History: Number of best accurate evaluated point(s) included in the EA population. Warning, modifying this parameter drastically impacts the exploration ability of MINAMO. Not recommended to set > 1. Can not be set greater than Population Size [default = 0].

Constraint Handling Method: Type of constraint handling method [default = Tournament]. For more details about this option, please refer to the section Deb's constraint handling method.

Surrogate model assessment


In MINAMO, the reliability assessment of the surrogate models can be
performed through a leave-one-out cross validation. In order to
assess the reliability of the approximate model at each design
iteration, the correlation coefficientR is calculated 
by using the leave-one-out (LOO) cross-validation
technique. The LOO procedure is a way to estimate
the accuracy of a surrogate model without the need of an external
dataset for validation. The method uses a single sample point from the
original data set as the validation data, and the remaining sample
points as the training data. This is repeated such that each sample
point in the database is used once as the validation data. Finally,
one obtains a set of estimated outputs (with LOO) and one of real
outputs for each response. These output sets can be statistically
analyzed for error estimation. The correlation coefficient is computed
and given by:



where  and  denotes, respectively, the
real values and the predicted ones for the n sample points.  R
always takes a value between -1 and 1 and measures the degree to
which two variables are linearly related. A value of R=1.0 indicates
a perfect fit. During the optimization process, for each response, the
correlation coefficient is computed for the local model (which
corresponds to the model constructed based on the points inside the
trust region defined by the move limit strategy). After the DoE
creation, the user is encouraged to perform a LOO reliability
assessment and has a look not only to the
correlation coefficient value but also to the scatter of
points. Furthermore, the user is strongly encouraged to monitor the
LOO correlation coefficient during the optimization process. 


FIGURE 14 Plot of actual vs. predicted values.




In its basic form, the LOO procedure is often computationally
expensive because of the large number of times the training process is
repeated. To circumvent this, an efficient procedure proposed in
[19] has been implemented in MINAMO. This procedure is named
here by Efficient LOO (available for RBF, Tuned RBF and ordinary
Kriging).


The LOO tool is accessible through the post-processing tool (see Section 4.3.1)(see Section 2.3.7).

Surrogate modeling


The challenge of the surrogate modeling is to generate a surrogate
that is as good as possible, using as few expensive evaluations as
possible. Polynomial fitting surfaces are generally not well-suited
for high dimensional and highly multimodal problems. Several
non-linear data-fitting modeling techniques can be used to build the
surrogates, e.g. artificial neural networks, Radial Basis Functions
(RBF) networks, Kriging or support vector regression. Contrary to
polynomial response surface models, these techniques have the
advantage of decoupling the number of free parameters with respect to
the number of design parameters. Furthermore, they can describe
complex and multimodal landscapes. 



Data-fitting models : Interpolation/Regression

Radial Basis Function networks



In order to obtain a surrogate model which is both accurate and
computationally efficient for approximation in high dimensions, two
variants of the Radial Basis Functions (RBF) networks have been implemented in MINAMO: a
classical RBF model and a tuned RBF model. RBF are linear models
expressed as follows [18] :




where: 

y is the model defined as a linear combination of n radial
basis functions, 

's are the weights, 
h is called the hidden
unit function or the basis function, 

's and 's denote,
respectively, the centers and the widths of the basis functions,
σ is a parameter controlling the
smoothness of the interpolation.


The goal of the approximator is to find the weights  minimizing
the error between the real outputs and those predicted by the
model. While several basis functions exist, we will concentrate on the
two most popular ones, the multiquadric and the Gaussian basis
functions. The Gaussian function decreases monotonically with respect
to the distance from a central point and the multiquadric one
increases.






Name
Expression of 




Gaussian





Multiquadric










FIGURE 11 Types of RBF

The classical RBF model uses the multiquadric function with a fixed 
for all i. The tuned RBF model implements a tuning so
as the surrogate models are generated without the user has to prescribe the
type of basis function and hyper-parameter values. In the training, the technique uses a leave-one-out based heuristic to select
appropriately the radial basis function h (Gaussian or multiquadric) and to
adjust the parameters 's with respect to the experiment plan in
order to obtain a higher quality model. In the MINAMO's tuned RBF model construction,
two types of width parameter are considered: a fixed width for all basis
functions and a variable width for each basis function. Note that the tuned
RBF network training is more time consuming than the classical RBF one, but it
is still cheap compared to the high-fidelity model. The tuned RBFN is highly
recommended. These surrogates are available with mixed variables. 



Kriging

Another type of surrogate models has also been included in MINAMO:
the Kriging model:
 


where x is an m-dimensional vector (m design parameters). The global trend  approximates globally the design
space. 
There are two Kriging variants in MINAMO:

   Ordinary Kriging assumes a constant but unknown mean: 
 -->. This is the most commonly used type of Kriging. 
Universal
 Kriging considers a polynomial function as global trend. The second
term Z(x) of this equation for y(x), represents the local deviation from
the global trend and is expressed using a stochastic process with zero
mean and covariance






where

  is the process variance and 

 is the
correlation function:




where 
where is the -th element of the
correlation parameter denoted by  and . 
The
parameter  is essentially a width parameter that affects how far a
sample point's influence extends. The exponent  is a measure of the
smoothness of the function in coordinate direction k, with 
corresponding to smooth function and values near 1 corresponding to less
smoothness. We can choose to fit  and  for each dimension k. But, most of the time, the exponent  is set to 2 for all k. This
choice of correlation function is called the Gaussian correlation
 function. Another possible choice is the exponential correlation function ( for all k). The version where the 's are tuned as the  parameters is more expensive ( and
 are optimized via a EA).



Given a set of  sample points, and their
responses  evaluated by the accurate
high-fidelity model, the estimated model
prediction of the equation for y(x) is given by:




  
where: 


 is the current unknown point, 

 is the
estimate of the mean response value (defined below), 

 is the set of
regression function: . 

 is obtained by
evaluating  at each of the samples points.
 In the case of ordinary
Kriging, we have  and thus  is
a vector with all values set to one. 
The vector  is
the correlation vector of terms between the unknown point  and the
 known sample points
and  is the correlation matrix for all of the data points in ,






This matrix is symmetric, positive definite and the diagonal
consists of all ones because . 
Note that
the size of the Kriging correlation matrix depends only on the number
of samples considered and not on the number of design parameters. 

The unknown parameters to be estimated for constructing the Kriging
model is the vector of parameters , named , and the
vector of exponents , denoted by . Indeed, for given 
and , the generalized least-squares estimate of  is
given by





 
The best choice for the values of vectors  and  can be
obtained by maximizing the following likelihood function


,

over the domain  and , where





Once  and  are determined by maximizing the likelihood function,
the estimated model prediction  can be completely defined as ,  and
 are functions of  and . 

Maximizing the likelihood function is a multidimensional optimization problem. This
function is known to be multimodal hence global optimization
techniques might be preferable to solve this problem. One of the
possible strategies (used in MINAMO) is to use an evolutionary algorithm. It is 
important to note that no convergence is guaranteed with such evolutionary algorithms. 
As Kriging computation requires the resolution of a multidimensional and
multimodal optimization problem, it is obviously more costly than RBF network
fitting. As more points will be added to the database during the optimization
process, the computation time of the Kriging fitting could be increased
considerably. This is the reason why, in literature, Kriging is generally used
for problems with less than 10 to 20 design parameters.


For MINAMO in FINE™/Design3D, the surrogate-related options are available via the Surrogate Model Settings tab. Three types of surrogate models are available:



TunedRBFN [default]

RBFN

Kriging
                For Kriging, different options are available through the Expert Mode
 
Correlation TypeGaussian [default]
ExponentialOptimizedHP  and  are optimized 
  
Regression Type : 0 [default, Ordinary Kriging]  to choose the regression type (0,1,2)
 




FIGURE 12 
Surrogate Model Settings.

The Parallel Surrogate Construction option allows to activate the training of the surrogate models of the different responses in parallel (mutli-threading). This option is not activated by default. The Number of Threads option allows to define the number of threads to use for the parallelization of the training of surrogate models.



Classification

Support Vector Machines

Support Vector Machines (SVM) can be used in MINAMO to classify binary data such as feasible/ non-feasible domains, or 
computable/ uncomputable zones. SVM are built based on a training set of  samples:



where:


 
( design parameters) and

. 





FIGURE 13 
SVM principle. Black points are support vectors.
This figure represents one possible classification based on a given training set with a linear classifier.
The goal of SVM is to separate classes
by maximizing the margin (space between the 2 purple lines). In MINAMO, soft margins are used to accept some 
misclassified samples (outliers). The black points, located on the margin, are called support vectors. For each class 
(blue and red), one point is misclassified with regards to the classifier . 
The degree of allowed misclassified samples is driven by a global parameter .



The tradeoff between maximization of margins and minimization of misclassified samples is computed by an optimization algorithm.
The corresponding dual problem to solve is:





where  is a Karush-Kuhn-Tucker multiplier strictly positive if  is a support vector and  is a kernel function.
The mathematical form of a SVM classifier is:



 wherewhere  is the support vectors indices. In MINAMO, the dual problem is solved with a Sequential Minimal Optimization (SMO). SMO is a standard algorithm for solving the quadratic programming problem that arises during the training of SVM. 
Different types of kernel exist but only the Gaussian one is available in MINAMO for the moment: with .
In MINAMO, SVM classification models are used in infill criteria targeting feasibility 
(see Section 2.3.7) and to build success models of success flags (See Section 2.3.8).

Mono-objective surrogate-assisted EA optimizer

Nowadays, with the continuous increase in computing power, a
widespread practice in engineering is that of simulation-based design
optimization. Indeed, design of complex engineering systems, which is
synonymous with the use of accurate high-fidelity
simulation models (e.g. Computational
Fluid Dynamics (CFD) analysis or Finite Element Method (FEM)), has
become a reality. However, even with today's computational power, it
is rarely conceivable to thoroughly search the design space using the
high-fidelity simulations. Since optimization procedures are mandatory
to quickly provide optimal designs, an adequate and general answer to
optimization based on computationally expensive analysis lies in the
surface models. Indeed, since the computation of the objectives and
constraints can take hours on tens of processors (with CFD or FEM
models for instance), and as the number of function evaluations is
rather high with EAs (to fix ideas : often more than 500 times the
number of design parameters), it is of paramount importance to reduce
the number of calls to the expensive high-fidelity
simulation. Therefore, in order to speed up the optimization process
(and decrease the number of calls to the external function), the
evolutionary algorithm is strongly combined with surrogate models in an adaptive/online scheme.

Online SBO framework

Surrogate-Based Optimization (SBO)  essentially exploits surrogates or
approximations in lieu of the expensive analysis results to contain
the computational time within affordable limits
(see [16,17]), with occasional recourse to the
high-fidelity model. However, the performance of such methods is known to be
largely dependent on the following key elements: 


the underlying optimization algorithm(s),

the surrogate model(s), 

the training (design of experiments and infill criteria),

the surrogate model(s) management schemes.



An SBO design cycle consists of several major elements as shown in the following figure.
 
FIGURE 4 Online surrogate-based optimization framework.

It is worth underlining the major importance of the first step, namely
the problem definition and optimization specification, which includes,
for instance:

 the parameterization, 
the definition of the bounds, 
the
objectives 
and the constraints. 

In MINAMO, the penalty type "MAXIMIZE" and "MINIMIZE" can be applied to the objectives, and "UPPER_BOUNDS and "LOWER_BOUNDS" for the constraints.
			The penalty weight of each penalty can be computed following the same formula as the one used in the FINE™/Design3D optimization run mode (see Objective Function for more details).
			The reference value displayed in the GUI for each penalty corresponds to the value computed for the first valid sample generated in the database considered for the optimization.
The second step consists in building
an initial database by choosing a set of initial individuals in the
design space and conducting high-fidelity simulations (exact models)
at the selected sample points. This exercise is called the
Design of Experiments (DoE). Based
on this DoE, surrogate models are constructed in order to build an
analytical relationship between the design parameters and the
expensive simulation responses. This phase provides cheap responses to
be used by the optimizer. Using the surrogate models to evaluate the
objective and constraint functions, an optimization is then carried
out to identify the optimum, at least in the sense of the
surrogates. The accurate simulation is used to evaluate the real
objective function and constraint values for this optimum in order to
check the accuracy of the surrogates at the optimal solution. The new
simulation result (and possibly simulation results at other
points) is (are) added to the database which is therefore continuously
improved with new design points, leading to increasingly accurate
approximate models all along the design. This design loop is repeated
until the maximum number of design iterations specified by the user is
reached. Most of the time, this number of iterations is driven by the
CPU execution time of the high-fidelity simulation. 


Therefore, a design iteration consists of:



executing the EA on the surrogate model (and not on the accurate
one);

after the end of the EA process, computing the best solution
found by the optimizer thanks to the accurate model; 

adding a new set of samples including this new point to the
database in order to enrich the model and be able to construct a
better approximation. 



The periodic retraining of the surrogates ensures that the models
continue to be representative of the newly-defined search
regions. Generally, the quality of the model increases with the number
of design loops, since new points are added to the database.


According to how the model interacts with a simulation and the
optimizer, modeling approaches can be categorized as online or offline
approaches. A strength of our optimization strategy is its online
modeling framework opposed to an offline one,
depicted in the next figure. In an online approach, a
model is created and is adaptively improved during the course of the
optimization, while in an offline approach, the optimization
 is performed based on an a priori trained model.



FIGURE 5 Online vs. offline SBO scheme.

The importance of
the online feature of our strategy can be observed in the following figure. Indeed, a better solution can be
obtained with the online SBO procedure than with the offline one, in a
limited computational budget of 60 function evaluations of the
Rosenbrock function. 


FIGURE 6 
Convergence histories of online and offline SBO schemes on the
 Rosenbrock problem.

 Number of best evaluated point(s) included
 in the GA population.
Modifying this parameter drastically impacts the exploration ability of MINAMO. Not recommended
to set IncludeBests>1. Can not be set greater than PopulationSize.

Of course, an offline scheme is always possible in MINAMO by setting
the number of iterations to one, but an online scheme is strongly
recommended. For the offline SBO, the DoE contains 59 points,
the optimizer is run on the surrogate model built on this initial
sample set and the optimum found is validated with the true
function. Whereas for the online procedure, 10 points are put
in the initial database and then 50 design iterations of our
algorithm assisted by surrogates are performed. This variant is
clearly quicker in terms of convergence.

Optimization algorithms

The optimization problem considered through this manual is the
following:




where


 is the design parameter vector,

 f is the objective (it is also possible to have more than one
 objective),

  and  are inequality and equality constraints,


 and  are explicit bounds on the design parameters.



The design parameter vector  can be continuous, integer, discrete or categorical (only continuous and integer parameter are considered for the first integration of MINAMO in FINE™/Design3D).
As mentioned in the introduction, the main optimization algorithm of
MINAMO is based on evolutionary algorithm accelerated by the
use of surrogate models that speed up the convergence rate. The
surrogate models are successively refined as the optimization
progresses in order to converge to the final optimum. The use of
evolutionary algorithm offers mechanisms to avoid local minima and
therefore find innovative solutions. The main optimization algorithm
of MINAMO is therefore organized with the following 5 steps:



The first step consists in building a database using a design of
 experiments technique.

Then a surrogate model is built using the DoE points in order
 to construct an analytical relationship between the design
 parameters and the simulation responses.

Third, an optimization algorithm is used to find the optimum
 using surrogate models to evaluate the objective and
 constraints functions.  

Then the accurate simulation is used to evaluate and verify the
 real objective function and constraint values. This new simulation
 result is added to the database. The database is therefore always
 improved with new design points, leading to improved surrogate
 models. 

Go to Step 2 until the maximum number of optimization
 cycles specified by the user is reached.



For industrial applications, the computational cost of one
optimization iteration mainly depends on the cost of the simulation
employed. In general the cost for building the surrogate model and
running the evolutionary algorithm is reasonable, depending on the
number of training samples, the number of input and output variables
and the choice of the surrogate model, but this time is generally
relatively small compared to the evaluation time of the simulation chain.

AutoBlade™
AutoBlade™ is a 3D parametric blade modeler with an advanced fitting module to start designs either from scratch or from an existing geometry. To get started with the use of AutoBlade™ the links in the following paragraphs can be of good use.
Installation AutoBlade™
Consult the System requirements  prior to the Installation on the hardware of choice.
Alternatively AutoBlade™ can be installed and used as part of FINE™/Design3D.
What's New?
The release note: New Features in v13 details what is new in the latest release of AutoBlade™.
Getting Started with AutoBlade™
To get started with the use of AutoBlade™ the following material is available:
User Guide

Tutorials

New Features in v13
This document provides a description of the new capabilities and major improvements included in AutoBlade™ v13, as well as statements outlining main customer benefits and known limitations. 
The following is a detailed list of new capabilities and enhancements in AutoBlade™ v13:

All Products:
Flexlm based security ID updated to v18

Improve administration wizard

 
Finally, the following is a detailed list of existing capabilities and enhancements included in AutoBlade™ but still requiring additional calibration
List of existing BETA capabilities
            

New parametric template for turbocharger
Improvement in generation of solid sectors
Improved solid sector periodic face generation




Flexlm based security ID updated to v18 (All Products)
(New in AutoBlade™ v13.1)
        
(All Products)
AutoBlade™ requires FlexLM based license keys for execution. In AutoBlade™ v13, the security ID has been upgraded to v18, thus requiring the delivery of new license keys for execution.
Customer Benefits

None
Known Limitations

None


Improve administration wizard
(New in AutoBlade™ v13.1)
        
(All Products)
The user-friendliness of the license management and diagnostics of the administration wizard is improved:

License Management>Product (de)activation: Deactivate button to return all fulfillment and all servers on the machine.
License Management>Trusted storage: check-box to return a fulfillment and refresh button to refresh the fulfillment status if needed.
License Management>License server: control and display the status of the known servers and the list of all the features deserves by the selected server. 
Diagnostics: Support request button to generate a file containing the results from the checks performed.

 
Customer Benefits

More user-friendly tool to diagnose and manage licensing.
Known Limitations

None

TUTORIAL 1. Marine propeller - blade fitting

Introduction

Introduction

Preparation

Blade fitting

Create new AutoBlade™  project

Define the target model

Define the initial model

Pre-fitting

Fitting

Save the project


Introduction
Introduction
In order to re-design and optimize existing blades to reach better design goals, NUMECA has developed a unique integrated environment for the design and parametrization of three dimensional turbomachinery blades. 

This tutorial is particularly adapted to the parametrization of a marine propeller. It makes use of Autoblade™. This parametric model can be used in the framework of an optimization loop.
In this tutorial:

fit a target geomTurbo to create a parametric blade model within AutoBlade™.

Preparation

Copy the provided project "Tutorial_1" located in the archive AutoBlade-Tutorials to your working directory.
Start the NUMECA blade modeler for turbomachinery blades AutoBlade™ v13.1:
                                            
       
            For Linux systems, you can access AutoBlade™ with the following command line:autoblade -niversion 131 -printFor Windows systems, you can access AutoBlade™ from the Start menu going to \Programs\NUMECA software\Fine131\AutoBlade or \Programs\NUMECA software\AutoBlade131\AutoBlade.

The AutoBlade™  graphical user interface includes several sections that enable the simultaneous visualization of the designed or fitted blade geometry. Access to the main menu and controls is provided through a menu bar and a quick access pad (QAP), and is complemented  with a tool/ icon bar.


Blade fitting
In this tutorial, the target geometry provided by a geomTurbo of the marine propeller will be fitted and parametrized. The fitting process is an optimization process that consists of minimizing the distance between the parametric model and the target geometry (predefined geomTurbo). Several fitting steps may be needed during a blade fitting.


Create new AutoBlade™ project
1.  Click on the button Create a new project to create a new AutoBlade™  project. 


2. Select the button Start from scratch and click on the button Ok to confirm.


3. Select a directory and enter the project name <DTMB_fitting>, then click on the button Save to confirm.


Define the target model
In this section use the file "tutorial_1.geomTurbo" as provided in the "Tutorial_1" package.
In case the geometry is not yet available in .geomTurbo format, AutoGrid5™ should be used to build one, e.g. from a Parasolid file (see Marine propeller - from CAD to geomTurbo). 
4.  Click in the QAP on Target Settings to expand it, then click on the button  to specify a target geometry file.


5. Go to the directory where the target geometry (the .geomTurbo file) is available and select the geometry file "tutorial_1.geomTurbo". Click on Open. A warning appears informing that the loaded geometry is not sliced into sections. Click on ok.


6. In order to create the sections, click on the button  .
7. Enter <8> <Enter> for the Number of sections.
8. Enter the following value as Spanwise locations: <0.01 0.2 0.4 0.6 0.8 0.88 0.95 1> <Enter>. Click on Ok.


Define the initial model
9. Click on the button  in the tool bar to import a predefined template.
10. Click on the button  and select "marine propeller" in the list to import the predefined template, click on the button Ok to confirm.


Before the initialization and fitting processes take place, a starting model must be defined with topological settings that are well adapted to the target geometry. It is usually advised to load a template or an existing parametric model close to the target geometry. Then the user should review all design steps and modify the settings if necessary.
The marine propeller has been developed from the PPTC marine propeller featuring a rounded tip topology. More details in the AutoBlade™ User Guide.
11. Review all the design steps in the Model Editor in the QAP.


Click on Endwalls, under Hub endwall, change the Curve to Composite by using the button . Click on the Insert button to add an element and change both element types to LINE by using the button . Keep the settings under Shroud endwall. Click on the button Ok to confirm.




Click on Stream surfaces, unselect the Rounded tip and keep the others settings. Click on the button Ok to confirm.




Click on Main blade, under  Side curves, select blunt for the TE shape. Keep the others settings. Click on the button Ok to confirm.

Improper settings will result in poor fitted models. Check all the design steps to be sure:

use suitable topology,
use an adequate number of parameters.

A new pre-fitting is required each time the topology and/ or the number of parameters are modified.



Pre-fitting
12. Click on Fitting Control in the QAP to expand it, then click on the button Adapt model to start the pre-fitting process.



Once the target and initial models are defined, a pre-fitting process must be performed.
The pre-fitting process will:

Guess values for the parameters that define prescribed curves and laws (end walls, sweep laws, camber curves,...).
Find the best traces for planar, cylindrical and conical stream surfaces.
Change the amount of primary sections and their spanwise locations.
Freeze some parameters that are unlikely to improve the model in the fitting process.
Initialize the lower and upper bounds of the parameters of the geometrical model.

The pre-fitting process will not:

Make suitable choices for the topology definition.
Capture special shapes for edges (including sharp ends).
Check that the pressure and suction sides coincide with the legend of 2D views.

Pre-fitting remains an approximation and a fitting should always be executed afterward.

13. Click on Ok to confirm.


14. Click on Yes in the warning message dialog box to start the pre-fitting process.


15. After the pre-fitting process is finished, activate the button Show projection in Target Settings in the QAP to check the difference between the target geometry and the parametric geometry in the MERIDIONAL view and the B2B view.


16. The parametric hub settings are not adapted to fit the target hub. The control points of the line can be changed to match the relevant hub shape. In the MERIDIONAL view, left-click on the hub curve, control points will appear.


17. Left-click on the center control point as it turns red. In the keyboard area, enter the following coordinates <0.067091 0.03082 0> <Enter>.


18. Click on the button  in the tool bar and select "section 8" to compare the difference of the section 8 in the B2B view. Click on the button   to zoom in/ out the B2B view.


Fitting
19.  Click on the button Fit model in Fitting Control in the QAP to start the first fitting process.


20. Select the feature hub_curve from the Selected features and use the button  to remove it from the selection.


21. Click on the button Ok to confirm, then click on the button Yes to start a coarse fitting process.
The first fitting process is usually a coarse process because the topological settings could be wrong or bounds of some parameters are reached early. In such a case, a fine fitting process is useless.
22. After the fitting process is finished, click on the button   in Fitting Control in the QAP to access the fitting graph window.
23. Choose "M_RTHETA_SECTION" for Category and "SECTION_3_SPAN_39"  for Selection using the button  to compare the parametric geometry (fitted result) and the target geometry of the section 3.


24. Click on the button Close to close the fitting graph window.
25. Click on the button   in Fitting Control in the QAP to access the convergence graph window.
26. Select "10" for Fitting step and "S8_CAMBER_H2" for Graph to view the convergence history of the parameter S8_CAMBER_H2 in the fitting step 10.


27. Click on the button Close to close the convergence graph window.
28. Select the menu Analysis/Parametric report..., some free parameters are blocked.
The number of blocked free parameters should always be checked before launching the next fitting process. This number should be 0, so that the next fitting process is able to further improve the value of the parameters.
29. Click on the Free tab and keep the Show blocked free parameters only option active. The blocked parameters are listed including "S8_CAMBER_H2". 
30. Click on the button Close.
31. Select the menu View/Show parameter status to display the status in the parameter list window.
32. Select the menu Geometry/Parameter list... to check and modify the bounds and the current value of the parameters:

select "all" for Group using the button ,
write <CAMBER_H> for Filter,
As it was seen in Show blocked free parameters only list, some camber parameters are blocked. Increase the bounds to unblock them by clicking on Increase all. 
Click four times on that button, then click Apply and OK.



33. Click on the button Fit model in Fitting Control in the QAP. Keep the default settings and click on the button Ok to confirm, then click on the button Yes to start a second coarse fitting process.
34. Select the menu Analysis/Parametric report..., the invalid parameters is 0 and the free blocked parameters is 1 (the parameter "HUB_R3" under the Free tab is related to the control point that has been placed previously), click on the button Close.
35.  Click on the button Fit model in Fitting Control in the QAP to start the third fitting process.
36. Set the Accuracy to Fine, click on the button Ok to confirm, then click on the button Yes to start a fine fitting process.
37. After the fitting process is finished, click on the button   in Fitting Control in the QAP to access the fitting graph window.
38. Choose "M_RTHETA_SECTION" for the Category and "SECTION_1_SPAN_0"  for the Selection using the button , click once in the graph, move the cursor and click again to zoom in the blade section, compare the fitted geometry and the target geometry.
The radius at the leading edge or the trailing edge can be difficult to capture. The fitting can be improved by imposing the value of the radius manually.
The fitting process can be launched several times, until the fitted geometry is sufficiently close to the target geometry.
39. Click on the button Close to close the fitting graph window.
Save the project
40. Select the menu Geometry/Export options....
41. Click on the geomTurbo tab in the Export settings dialog box, click on the button Ok to confirm.


42.  Select the menu File/Save to save the project and the parametric model.

Tutorials


Where to Find the Files Used in the Tutorials?
 The appropriate files (and any other relevant files used in the tutorials) can be downloaded from the corresponding link: AutoBlade-Tutorials.
Conventions Used in the Tutorials
Several conventions are used in the tutorials to facilitate your learning process. 
Inputs required to execute the tutorials are most often restricted to the geometry definition.
The sequence of actions to be executed are described through a step-by-step approach, in the form of Arabic numbers.
Additional insight about some specific actions and/ or features is frequently added to illustrate the tutorial further. This information is proposed for the purpose of clarity and completeness, and should not be executed. It appears as a note with a light blue background.
Contact NUMECA local sales or support office for any question or information you may require. To allow NUMECA local sales or support office to help you out within the shortest delays, please provide a detailed description of the observed behavior and performed analysis.

System requirements

For proper installation and use of AutoBlade™ please consult the following sections detailing the system requirements for the applicable operating system.

Installation

Prior to the installation of AutoBlade™ it is important to consult first the System requirements.
This installation note concerns AutoBlade™ as a standalone product.
It is not necessary to install AutoBlade™ separately if it was already installed as part of FINE™/Turbo with FINE™/Design3D.

Topology & Parameters
The nine steps illustrated in FIGURE 1 are detailed in the next sections. All steps are accessed using the graphical menu in the left area introduced earlier (Model Editor subpad).
All menus feature embedded diagrams that permit to understand the physical significance of the related parameters. The naming of the parameters is defined for all topological choices and allows to identify them in the Parameter list.


FIGURE 1 The nine generation steps

Fitting Settings


FIGURE 3 Settings controlling the fitting process
Fitting Features
A complete fitting is achieved with default settings. For convenience, AutoBlade™ allows the user to select the features involved in the fitting process by selecting their order and the number of times the fitting process has to be applied.
Here are some examples.

If the endwalls are defined by parameterless curves, they do not need fitting.
If the endwalls need fitting while hub to shroud interpolated stream surfaces are applied, the sections cannot be finely fitted in the first fitting run, since the endwalls are usually not sufficiently improved after the first step. In such a case, it is advised to fit the endwalls only, by means of two or three fitting processes. Then, in a new computation, the fitting can be applied on the stacking laws and sections.

Each feature in the list corresponds to one step of the fitting process except for the primary_sections feature that will lead to several steps function of the number of sections and blades.
When a Non-Axisymmetric Hub/Shroud is defined, additional features non_axisymmetric_hub and non_axisymmetric_shroud are available for the fitting process. The number of steps equals the number of cuts, including the start and end cuts.
Optimization Settings
Several algorithms are accessible for the fitting process and it is even possible to combine them or customize their settings. 
However, the genetic algorithm gives the best results and the three default modes Coarse, Medium and Fine are sufficient in practise (FIGURE 3). All those modes use a genetic algorithm and share the same settings, except the number of iterations. They correspond respectively to a number of reproduction cycles of 25, 50 and 100. This really means that a Fine process is twice slower as a Medium process which is twice slower as a Coarse process.
User-Defined mode is not covered in this manual and should not be enabled. Default settings Coarse, Medium and Fine are sufficient even for an advanced user.

Topological Compatibility Issues
Selecting a planar radial stream surface prevents some stacking point options and the center of gravity stacking point does not allow the use of splitter blades. These are some examples of the compatibility restrictions in the definition of the topology. Since the topology dialogs act as ordered steps in the design process, the stream surface choice affects settings for meridional and tangential location, but also the construction plane for the camber curve and all subsequent choices.
It is not easy to understand all restrictions about the topological settings, especially for a new user. The goal of this section is to help selecting the right settings for your project. In addition, importing a template close to your final design could minimize the time required to achieve the project.
TABLE 10, "Compatibility table for topological settings" suggests a summary of the compatibility for the main topological choices.
Axial Pumps, Compressors & Turbines
The default model or the two first templates are a good starting point for an axial project. The first template is a compressor model, the second one a turbine model.
The Wind Turbines are treated in the next section.
Stream Surfaces
Usual construction planes for the camber curve are (Z,Y) and (m,R*θ) planes. In the first case, planar axial stream surfaces are mandatory and in the second case, the best choice is cylindrical stream surfaces. If the machine is not strictly axial, conical or hub to shroud interpolation surfaces can be helpful too, provided the traces remain close to a R cst line in the area of definition of the blade.
Blade Meridional & Tangential Locations
Leading and trailing edge stacking points are compatible with all topological settings. This is not the case of the other stacking points, which could be unavailable or prevent the selection of subsequent settings.
        
The options centre of gravity, maximum thickness, centre of channel, on camber and on chord are restricted to dimensional planes (Z,Y) and (m,R*θ) and therefore only available for axial turbomachinery.
Currently, those special stacking points do not allow splitter blades. Maximum thickness and centre of channel are not available for hub to shroud interpolation stream surfaces. Centre of channel is not compatible with conical stream surfaces.
Choosing leading or trailing edge stacking allows more freedom in subsequent choices (edge traces, camber construction plane, optional splitters,...) and are always available
The sweep law is always available and edge traces are compatible with leading and trailing edge stacking points only.
2D Blade Sections
Planar stream surfaces impose (Z,Y) as construction plane for the camber curve. Revolved stream surfaces should use (m,R*θ) construction plane.
A reference length is needed when a sweep stacking law has been selected and should always be an axial length DZ: other lengths are meaningless with planar or cylindrical stream surfaces.
Both construction modes independent suction & pressure sides and camber & thickness are always available for (Z,Y) and (m,R*θ) construction planes.
DM and DZ reference lengths have the same effect for pure axial cases.
Optional Splitters
The splitters menu is available when leading or trailing edge stacking is selected in the meridional location menu. Most settings are shared with the main blade topology (construction mode and edge shape) but the amount and values of the parameters are specific.
Technological Effects
Edge filing is available for blunt trailing edges in single blade cases only. Blade cutoff is always available.
Radial Pumps, Compressors & Turbines
Several template models are available for radial machines:

a centrifugal compressor model,
a centrifugal compressor with a single splitter blade,
a pure radial diffuser.

Stream Surfaces
Usual construction planes for the camber curve are (m,β) and (,θ) planes, whereas only conical and hub to shroud interpolation stream surfaces are usually applied.
Blade Meridional & Tangential Locations
Leading and trailing edge stacking points are compatible with all topological settings while all other points are simply not available.
        
The sweep law and edge traces are always available but the traces are usually preferred.
2D Blade Sections
Assuming conical or interpolated stream surfaces have been selected, the construction of the blade section is limited to a few choices:

Common construction planes for the camber curve in radial cases are (m,β) and (,θ) planes.
A reference length is needed when a sweep stacking law has been selected and the designer can choose among axial length DZ, radial length DR and meridional length DM. In pure radial cases, an axial length DZ is not suitable, but not forbidden in AutoBlade™
Only camber & thickness construction mode is compatible with common construction planes introduced above.

Optional Splitters
Splitter blades are always available.
Technological Effects
Edge filing is available for blunt trailing edges in single blade cases only. Blade cutoff is always available.
Wind Turbines
To design a wind turbines, the easiest way is to start form the provided template.
Stream Surfaces
Planar axial stream surfaces is the preferred choice. Cylindrical surfaces is an alternate choice.
Blade Meridional & Tangential Locations
All stacking points are available, with three usual options: center of gravity, on camber or on chord. Those options are required when using rounded tip topology.
Edges traces are not compatible with very high staggered blades near the tip section (near or exceeding 90 degrees). Therefore, a sweep law is advised because crossing edges are allowed in the meridional view.
2D Blade Sections
Both construction modes are allowed, but thickness addition is the usual choice. The construction plane is (Z,Y) or as a second choice (m,Rθ).
Optional Splitters
Not applicable
Technological Effects
Not applicable
Marine Propeller
To design a marine propeller, the easiest way is to start from the provided marine propeller template available in the Geometry/Import parametric model... menu. 
The template for marine propeller is the PPTC VP1304 with rounded tip topology.
Stream Surfaces
Cylindrical surfaces is the preferred choice. Conical and Planar axial stream surfaces are alternate choices.
Blade Meridional & Tangential Locations
All stacking points are available, with three usual options: center of gravity, on camber or on chord. 
Leading edge or Trailing edge are also convenient. But those stacking point are not compatible with rounded tip topology.
2D Blade Sections
For the main blade, the reference length True Chord Based is preferable.
For the side curves, both construction modes are allowed, but thickness addition is the usual choice.
Optional Splitters
Not applicable
Technological Effects
Not applicable
Flank-Milled Compressor & Ruled Blades
This section describes the definition of ruled blades in general, where the ruling direction can be controlled with precise CAD output of the side surfaces.
Stream Surfaces
All surfaces are available, interpolated stream surfaces being the most usual choice for centrifugal cases.
Blade Meridional & Tangential Locations
Leading edge, trailing edge, on camber and on chord options are available. Other stacking points are unavailable because the profile cannot be built directly in the construction plane.
Edges traces and sweep law are both allowed.
2D Blade Sections
Thickness addition is the only construction mode available. Double blunt is mandatory for late elliptical rounding, with or without cutoff.
Optional Splitters
Splitter blades are always available.
Technological Effects
The compatible effects are the generalized cutoff (linear and spline options), the 	late elliptical rounding (only for double blunt case) and the 	non axi-symmetric endwalls.
TABLE 10 Compatibility table for topological settings

Geometry Analysis 
The Geometry Analysis icon of the model editor, in the left area of the main interface, grants access to the geometry analysis tool.
This tool generates plots showing the distribution used to generate the samples in Optional quantities notebook (Sampling). This menu can be left open for monitoring purposes while editing the topology and parameters and updates automatically after each change.


FIGURE 106 Geometry analysis tool
Up to 8 geometry analysis windows are allowed simultaneously.
When the window is re-sized, the aspect ratio cannot be preserved.
Selectors
Five selectors are available to control the distribution. The selectors control the Quantity, Blade, Section, Abscissa and Cut , respectively. The selectors Quantity and Abscissa are always available and control respectively the choices of ordinate and abscissa. The selectors Blade and Section  are available for some distributions and control the choices of blade and primary section. If the quantity is plotting a cut value, the Cut coordinate choice can be selected. The next table details the usage of the selectors.
TABLE 14 Selectors for distributions






Selector
Usage
Values





Quantity


Controls the ordinate of the graph.
All values are always available, except Channel width that applies to single blade cases only.



endwall angle
endwall curvature
section thickness
mean line theta
mean line metallic angle
mean line curvature
mean line beta star
mean line epsilon
side curves metallic angle
side curves curvature
epsilon axial cut
camber curve metal angle
camber curve curvature
channel width
draft angle
spanwise chord length and its meridional projection
spanwise meanline angles (stagger, LE metal and TE metal)
spanwise solidity and its meridional solidity
spanwise leading and/or trailing edge radius
spanwise Z coordinate profiles for leading edge, trailing edge and gravity center
spanwise R coordinate profiles for leading edge, trailing edge and gravity center
spanwise theta coordinate profiles for leading edge, trailing edge and gravity center
spanwise thickness min/max values
spanwise thickness cut value
spanwise throat width





Abscissa


Controls the abscissa of the graph.
Up to four choices are available according to the selected quantity.



curve length
fraction of the curve length (used for sampling)
m coordinate

 coordinate





Blade


Thickness, mean line and side curves distributions require the selection of a blade when at least one splitter is defined.



main blade
splitter 1
splitter 2
...





Section


Thickness, mean line, side curves and channel width distributions require the selection of a primary section when a splitter is defined.


number of the primary section




Cut


Spanwise thickness cut value requires the cut coordinate where the profile is built.



Z coordinate
R coordinate
curve length
fraction of the curve length





In the tool bar, an optional selector curvature Clipping allows to control the clipping of the ordinate in curvature graphs (endwalls, side curves and mean line). This option limits the default zoom and the fit operation when the values have a large range of variation.
Another special selector axial Cut value allows to set the Z coordinate at which the mean line is cut for analysis of the special epsilon angle. The minimum and maximum cuts are automatically updated according to the bounding box of the mean lines.
All active sections (either primary and parametric sections or discretized sections) are used for sampling.
Viewing Commands & Options
The graph can be zoomed in by means of the left mouse button. Just click once to define the first corner, then move the pointer and click again to defined the second corner. The aspect ratio is not constrained in distributions.
It is possible to highlight one or more curves by selecting their legend text (FIGURE 107). This operation is achieved by means of the middle mouse button. Clicking a selected item removes it from the selection.


FIGURE 107 Highlighting a curve is achieved by means of a middle click over the legend
A few other operations are available in the contextual menu. This menu appears when the right mouse button is pressed over the graphics area. The following commands are listed and activated:
TABLE 15 Optional commands - contextual menu






Zoom back


Reverts the last zoom operation




Fit view


Fits the view (default zoom)




Show/hide legend


Shows or hides the legend. This option is active until the session is closed.




Show/hide crosshairs


Shows or hides the crosshairs. This option is active until the session is closed.




Show/hide grid


Shows or hides the background grid. This option is active until the session is closed.




The icon  is used to lock specific user-defined ranges for abscissa and ordinate. This special flag is inactive by default. If it is activated by clicking the locker icon, the current zoom ranges are preserved until the user explicitly changes the zoom or deactivates the option. The zoom ranges are also saved in the project if the locker is activated, so that the user can retrieve the zoom when saving and reopening a project.
Export
Graphs can be exported to text and postscript files thanks to the commands Save and Print from the tool bar.

First Time Use
Basic Installation
When using AutoBlade™ for the first time it is important to verify that AutoBlade™ is properly installed according to the installation note. The installation note provided with the installation software should be read carefully and the following points are specifically important:

Hardware and operating system requirements should be verified to see whether the chosen machine is supported.
Installation of AutoBlade™ according to the described procedure in a directory chosen by the user and referenced in the installation note as 'NUMECA_INSTALLATION_DIRECTORY'.
A license should be requested that allows for the use of AutoBlade™ and the desired component and modules (see Required Licenses for all available licenses). The license should be installed according to the described procedure in the installation note.
Each user willing to use AutoBlade™ or any other NUMECA software must perform a user configuration as described in the installation note.

When these points are checked the software can be started as described in the installation note or the How to start AutoBlade™ section of this user manual.

Main Blade
Once their stacking point and extent is defined, the primary blade sections can be constructed and placed on the stream surfaces.
In AutoBlade™, the splitter blades are optional and their definition is always relative to the main blade. Therefore, splitter blades are covered in a separate menu (Optional Splitters).
Any blade section is built from a camber curve in a prescribed 2D construction plane. According to the stream surface type, the designer can choose between several construction planes and curve types. AutoBlade™ then provides two distinct methods for the construction of the full blade contour:

Suction side and pressure side mode: independent suction and pressure sides are constructed from the camber line using Bezier curves. In general, this method is used for axial turbine and axial compressor blades.
Camber and thickness mode: a thickness distribution is applied along the camber curve from leading edge to trailing edge. This method is very common in centrifugal turbomachinery design.

It is also possible to specify blunt leading and trailing edges.

Tool Stack
In each view, a permanent tool allows the selection and highlighting (meridional view) or the picking of the controls (other views). Zoom, dynamic viewing and others are all tools that mask the permanent tools in the active view, recognized by its red border.
When one or more tools are started in turn, the latest grabs all events and suspends the previous one. This means that the tools are stacked and must be quit in turn to return to the original permanent tool.
For instance, the selection tool is permanent in the meridional view. Selecting an highlighted curve starts the edition tool for that curve and no more selection is possible until left clicking a unhighlighted area of the view. If the zoom area tool is then started, the edition tool is also suspended. This means three tools are stacked and zoom area is the only active tool. In order to return to the default selection tool, the zoom tool has to be stopped by a right click. Then the edition tool must be stopped by a left click.
Aborting a specific tool
Specific edition tools are stopped by means of a left click in a unhighlighted area of the corresponding view.
Zoom area and dynamic viewing tools are stopped by means of right click.
Aborting all tools
To prevent bad operations in tools, applying changes in the model editor from the left area of the main interface stops all non permanent tools in the views. Generally speaking, all model and file operations automatically abort the tools.

View Layout & Graphs
Multi view is the default mode. In this mode, four graphs showing different views of the blade appear in the main area. The blade is defined by means of the hub and shroud contours, a series of so-called primary sections and by stacking laws. All these features can be observed in the different views. TABLE 4 summarizes the properties and numbering of the views.
TABLE 4 Available views






Viewport


Content






View 1 (upper left)


Meridional view in (Z,R) plane with

hub and shroud curves,
stream lines of the defining sections,
edge traces,
reference stacking point and stacking sweep curve (when available)





View 2 (bottom left)


Camber curve in its construction plane. The curve belongs to the current selections of blade and primary section.
No curve appears if the selected splitter blade inherits the main camber curve.




View 3 (bottom right)


According to the construction mode,

Suction and pressure sides in the chosen construction plane (independent SS & PS section mode)
half thickness distribution versus camber length (camber & thickness 2D section mode)

for the selected blade and primary section.




View 4 (upper right)



Blade-to-blade view,
Sweep curve in (z,span) plane (when active),
Lean curve in (span,θ) plane,
3D view with optional hub, shroud and blade repetition





When a stacking sweep law is active, the 3D stacking curve is shown in orange color in the 3D view.
The user can quickly switch between single view and multiple views:

double-clicking in a subview activates full view for that subview,
double-clicking the full view restores the multiple views (alternate key: escape),
right-click in a sub/full view and select the menu Single/multiple view from the context menu entry.

Export geometry
The menu Geometry/Export geometry... allows the user to output the coordinates of the selected curve.


The user should select one curve type first. Depending on the selected curve, the user may be able to select the coordinate system and the location of the curve (blade index and section index) for output. Then, clicking on the button Save will opens a file chooser and prompts for a location where to save the selected curve with default extension ".dat".
The format of the .dat file is as follows:

The first line is a comment line indicating the coordinate system.
The second line defines the number of the discrete points.
The next lines list the data of each point.

Method 'along channel'
The method described above is generally not suitable for turbines because the perturbed surface is then generated from profiles far from parallel and too high perturbations appear near the suction side of the main blade (FIGURE 80).
To allow non-axisymmetric endwalls in case of turbines, an alternate method consists in building the cuts along virtual stream lines created as shown in FIGURE 84. The cuts may extend outside the blade channel, but then the start and end cuts must be identical to ensure C0 continuity. G1 continuity can be enforced by mean of special boundary conditions in the generation of the loft patch.


FIGURE 84 Cuts are defined along the blade channel
If the perturbation is limited to the blade channel, the start and end cuts may be independent, enabling free boundaries (Limit perturbed surface to blade channel option in FIGURE 87).
The guide curves are defined as circle arcs at constant value of m and C0 continuity is automatically ensured if the start and end heights of each perturbation are managed by the algorithm (FIGURE 85). G1 continuity is optional. In the case of Bezier curves, G1 continuity will freeze two additional heights (h1 and h5).


FIGURE 85 Perturbation law for 'along' method
In 'cut along' method, cuts defined with a spline law only accept identical boundary conditions for start and end. This limitation does not apply to Bezier laws.
This new construction is especially suitable for axial turbines and fans, but not for centrifugal compressors or impellers where the first method provides far better results. An example of the 3D construction of loft profiles and guide curves is depicted in FIGURE 86.


FIGURE 86 The complete perturbed surface for 'along' method

Settings Dialog
When activating Define non-axisymmetric hub/shroud surface in the corresponding pages, a list of new entries are provided to the user to control the settings.


FIGURE 87 Non-axisymmetric hub/shroud settings
The positive direction corresponds by default to the left side of the hub or shroud curve direction.
The repetition option by default, set to 1, duplicates one time the non-axisymmetric patches in both θ directions. This option is useful for the exportation to AutoGrid™.
In both 'cut across' and 'cut along' methods, a check button Imprint cuts on surface can be activated to enforce cuts as internal edges on the non axisymmetrical patch in the Parasolid model
The option Imprint cuts on surface is responsible for a higher amount of faces and may significantly slow down the build and analysis of the non axisymmetrical surfaces. Therefore, it is advised to disable this option in an optimization.
The angular tolerance allows to avoid any gap between repeated patches in ".geomTurbo" file.

GeomTurbo 3.7
This format is deprecated and only allows a single splitter blade. Not all specifications of the format are supported in the fitting module: external data or merged blade cannot be treated correctly.
The major supported keywords are listed in TABLE 1.
TABLE 1 Supported geomTurbo blocks






Keyword


Usage






HUB


starts the definition of the hub curve




SHROUD


starts the definition of the shroud curve




PRESSURE


starts the definition of the pressure side curves. A single curve for each section follows.




SUCTION


starts the definition of the suction side curves. A single curve for each section follows.




PRESSURE_SPLITTER


starts the definition of the pressure side curves for the splitter blade. A single curve for each section follows.




SUCTION_SPLITTER


starts the definition of the suction side curves for the splitter blade. A single curve for each section follows.




The next paragraphs explain the header content, the choice of coordinates and how to add each section. A last paragraph describes additional keywords that have been introduced specifically for AutoBlade™. Example Fitting Target Geometry contains sample target geometry files that can be used as a reference.
Further details about the original geomTurbo format 3.7 and keywords can be found in the AutoGrid™ 4 User Manual.
".geomTurbo" format is not case sensitive, so all keywords can be written in lower or upper case letters or even as a mix of both styles.
Header
The header contains a line defining the format and its version and a few optional values that apply to the geometry.
GEOMETRY TURBO VERSION 3.7
geometric_tolerance					1e-06
blade_expansion_factor_hub					0.03
blade_expansion_factor_shroud					0.03
blade_merging					0
units					1
number_of_blades					36
The blade repetition in the tangential direction is specified after the NUMBER_OF_BLADES keyword as an integer value.
GEOMETRIC_TOLERANCE, BLADE_EXPANSION_FACTOR_HUB, BLADE_MERGING and BLADE_EXPANSION_FACTOR_SHROUD are not currently used in AutoBlade™.
Curve Data Formats
Curves must be defined as a set of data points. External files are not supported. It is not possible to use IGG™ curve formats or linked data files.
Curves are defined by 2 or 3 coordinates and follow a simple rule: a symbolic coordinate system is defined, followed by the amount of points defining the curve and the list of data points.
Example:
# a meridional curve
ZR
3
1.2		2.3
1.3		2.4
1.4		2.5
The list of points contains one data point per line and the coordinates are space separated. The next table lists all supported formats according to the curve type.
TABLE 2 Curve data formats






Curve type


Supported formats






hub and shroud


XYZ, XZY, YXZ, YZX, ZXY, ZYX, ZR, RZ




side curve


XYZ, XZY, YXZ, YZX, ZXY, ZYX, ZRTH, ZTHR, RTHZ, RZTH, THZR, THRZ




where X, Y and Z stand for the cartesian coordinates and Z, R and TH for the cylindrical coordinates. Angle TH is expressed in radians.




A "space" can be a combination of several space or tab characters.
Hub & Shroud Curves
Endwall curves are usually defined first, but this is not a requirement. A ZR format is preferred however. Data points must be ordered from inlet to outlet.
AutoBlade™ is not accepting hub and shroud defined as ZR curve along partly Z-axis (R=0), ZR curve crossing Z-axis or ZR curve defined with negative radius.
Pressure & Suction Side Curves
Suction and pressure side curves are defined separately, under SUCTION and PRESSURE keywords. The next keyword is always SECTIONAL followed by the number of sections and the definition of the curves.
Example:
suction
SECTIONAL
+3
# section 1
XYZ
51
0.17669		-0.0208609		0.000351471
0.176693		-0.0208955		0.000391449
...
0.186772		0.0144109		0.0429921
0.186768		0.0144296		0.0429756
# section 2
XYZ
51
0.217127		-0.0231681		0.00303258
0.217124		-0.0231913		0.00306532
...
0.217501		0.0200831		0.0381821
0.2175		0.0200963		0.0381687
# section 3
XYZ
51
0.251068		-0.0250123		0.00642899
0.25106		-0.0250273		0.00645487
...
0.243571		0.0233406		0.0341187
0.243573		0.0233511		0.034108
AutoBlade™ assumes that all sections are ordered from hub to shroud (increasing span parameter). and curves must be defined from leading to trailing edge.
It is very important to carefully define the starting and ending points of the side curves:

If the leading edge is rounded, both side curves should begin with the same point coordinates for any given section.
If the trailing edge is rounded, both side curves should end with the same point coordinates for any given section.
The chosen edge point at a rounded edge must divide the section almost symmetrically in that region. Although this is straightforward with thin blades, corrections may be required in some cases.

It is important to point out that good fitting results may depend on the choice of suitable edge points.
The BLADE keyword which in AutoGrid™ permits to enter a full blade contour as one single curve is not supported since AutoBlade™ needs both leading and trailing edge points.
AutoBlade™ assumes that the suction side is located above pressure side when plotted against an increasing θ angle.
Further details about the original geomTurbo format 3.7 and keywords can be found in the AutoGrid™ 4 User Manual.
Splitter Blade
In addition to the main blade, the ".geomTurbo" format permits to define one single optional splitter blade. The splitter blade, if it exists, must be defined on the same sections as the main blade.
Splitter side curves are defined exactly in the same way as for the main blade: SUCTION_SPLITTER and PRESSURE_SPLITTER keywords replace respectively SUCTION and PRESSURE.
AutoBlade™ requires that the splitter blade is located below the main blade (when plotted against increasing θ). An additional argument ROTATE followed by a floating point value may be added just after the main keyword. This represents a rotation angle (in radians) to be applied on the splitter side. 
Example:
SUCTION_SPLITTER rotate -0.785398
SECTIONAL
+2
...
PRESSURE_SPLITTER rotate -0.785398
SECTIONAL
+2
...
Topologies including multiple splitters cannot be fitted in the current version of the software. This is a direct consequence of the limitation in the ".geomTurbo" format.
ROTATE argument is not part of the specifications of the ".geomTurbo" format and is optional.

Visual Check & Parameters Manual Correction
Once initialized, the parametric model should be a rough approximation of the target geometry. In some cases, the results are quite close, but it depends on the topological choices, the overall number of parameters and the shape of the target geometry. This is why a visual comparison between the target and the initialized model is necessary before a fitting process is launched.
Visual Check
Comparison is achieved by means of the menu Analysis / Fitting graphs.
A progress meter appears as soon as the page is opened and a quick process begins: the sections of the target geometry are projected to the stream surfaces of the initial model. This operation takes a few seconds.
It is important to check the meridional view as well as each section in the conformal (RAHMAN Md Asfiqur, θ) plane.

Endwall curves are usually well initialized. The most critical setting is the number of parameters in use, especially if hub to shroud interpolated surfaces are used. It may be necessary to increase the amount of points.
When a sweep law is used, the endpoints of the traces may drift away if special stacking points CC or MT are used. The fitting process will improve this without any manual change.
Thick blades with bent camber curves may be poorly initialized (a failure message is usually generated in that case).
Leading and trailing edge radii must be precise in all rounded cases. If not, a manual correction is necessary (ill formed circular arcs in target or sharp edges).
The wedge angle parameters could need correction when construction curves are active for suction and pressure sides.
If the model defines a splitter blade with a refined camber curve, the refinement parameters are never modified in the initialization process and both values and bounds could be too large.

Topological settings of the model usually do not need further checking if the results are good after correction of the above issues.
The suction side curve must be the suction side curve from an aerodynamic point of view and the pressure side curve must be the pressure side curve from an aerodynamic point of view. This can be checked by activating the markers in the legend of the section graph. If the target suction side is not the aerodynamic suction side, the target geomTurbo file needs a correction! Please refer to sections 4-2.1 and 4-2.2 for details about the manipulation of the side curves.
Parameter Bounds Check
The starting model has been altered by the initialization process and the parameters should be carefully checked before a fitting process.
The Parameters list button (on the Icon bar) or the Geometry/Parameter list menu opens a new window. This window allows to easily check the value and the bounds of the parameters. If the bounds are not visible, remember to check the View/Show parameter bounds option. Endwalls and Others groups may be skipped. In all other groups, the value of the parameters should be free to move with very few exceptions and the ranges must be large enough.
In addition, a parametric report aiming the description of the total number of parameters can be opened with the Parametric report button (on the Model Editor subpad) or the menu Analysis / Parameter report.
2D blade sections

If the camber curve is of Bezier type defined by a custom amount of equally spaced heights, the ranges need to be large, at least 20 percent of the highest value in both directions, for all parameters. A narrow range will indeed limit the results of the fitting if one of the bound is reached!
When the trailing edge is rounded and circular (independent construction curves or B-spline thickness), the corresponding radius can be frozen by means of the Reset command (contextual menu). The estimate of the initialization process is usually precise and cannot be improved by the fitting process.
When available, the half wedge angle parameter at leading edge is large when the blade is thick, so the range needs to be large also. Angles are given in degrees. The range at trailing edge is usually large enough.

Meridional and tangential locations
The range and value of the angular parameters are usually suitable.

Graphical Interactions
This section covers the graphical controls and actions.

Sampling
These sampled values are extracted from available distributions (see Geometry Analysis). For each distribution, responses are computed versus a normalized length and thus, user input values are kept between 0.0 and 1.0. Up to fifteen values can be generated for each distribution. All sample locations are automatically rounded to the nearest percentage value and duplicate values are discarded.
For the optional quantities, the camber curve and the mean line are considered with their three global coordinates (X,Y,Z). This allows AutoBlade™ to use the same formulas whatever the topology (i.e. axial or radial).
In order to allow the user to input values between 0.0 and 1.0, AutoBlade™ uses the length of the camber line as normalization factor. In such fashion, the 0.0 station would comprise the leading edge point of the camber line and the 1.0 station represents the trailing edge. Other points between 0.0 and 1.0 have their coordinates extracted according to the percentage of the total camber length they are located at. The total length of a curve can be calculated as:






where  is the number of points describing the curve [0,1,2,…,]. Therefore, a point j located at the global coordinate () would have the following as normalized coordinate:



In AutoBlade™, the user can check the total length of the camber line through the Analysis/Optional quantities... menu. In the Optional quantities window, the user selects the Camber length under the Scalar values tab. Then when clicking on the Apply button and on the Camber length, the value is displayed and represents the result of the equation (3-16a). When the number of Camber coordinates is selected under the Sampling tab (e.g. 4), the user is in fact selecting the value of  in the equations (3-16a) and (3-16b). In that case, by inputting 0 0.33 0.67 1, the user is specifying the normalized coordinates at which he desires to extract the coordinates of sampling points (in this case at 0%, 33%, 67% and 100% of the total camber line length).
 
TABLE 11 summarizes the sampling capabilities in AutoBlade™. A detailed description of every distribution follows.
TABLE 11 Sampling summary







Quantity


Input value


Response






hub angle


length fraction of the hub curve


angle of the hub curve (in degrees)




shroud angle


length fraction of the shroud curve


angle of the shroud curve (in degrees)




hub curvature


length fraction of the hub curve


signed curvature of the hub curve




shroud curvature


length fraction of the shroud curve


signed curvature of the shroud curve




thickness


length fraction of the blade section mean line


thickness computed in X,Y,Z coordinates at input location




metallic angle


length fraction of the suction or pressure side


angle on SS or PS computed in (,θ) plane. The unit is degree




curvature


length fraction of the suction or pressure side


signed curvature of suction or pressure side computed in (m, R*θ) plane




channel width


length fraction of the mean fluid line


width of the channel seen perpendicularly to the mean fluid line in (,θ) plane




camber metallic angle


length fraction of the camber curve


angle of camber curve in (,θ) plane. The unit is degree




camber curvature


length fraction of the camber curve


angle of camber curve in (m, R*θ) plane. The unit is degree




mean line metallic angle


length fraction of the blade section mean line


angle of mean line in (,θ) plane. The unit is degree




mean line curvature


length fraction of the blade section mean line


signed curvature of mean line in (m, R*θ) plane. The unit is degree




draft angle


length fraction of the suction or pressure side


draft angle (in degree)




Endwall Angle
The angle of the hub or shroud curve is measured in degrees in the meridional plane (Z,R).






Quantity


Examples






HUB_ANGLE_U??


HUB_ANGLE_U33 stands for angle value at 33 percent of the hub curve length.




SHROUD_ANGLE_U??


SHROUD_ANGLE_U75 stands for angle value at 75 percent of the shroud curve length.




Endwall Curvature
The signed curvature of the hub or shroud curve is measured in the meridional plane (Z,R).






Quantity


Examples






HUB_CURV_U??


HUB_CURV_U33 stands for signed curvature value at 33 percent of the hub curve length.




SHROUD_CURV_U??


SHROUD_CURV_U75 stands for signed curvature value at 75 percent of the shroud curve length.




Thickness
Thickness is defined as the blade width measured in the perpendicular direction along the blade section mean line (FIGURE 94). Mean line and thickness are both computed in spatial coordinates (X,Y,Z) for any primary blade section. Therefore, thickness distribution and sampling are always available.


FIGURE 94 Thickness computation






Quantity


Examples






S?_(SPLIT?_)THICK_U??


S1_THICK_U33 stands for thickness value at 33 percent of the mean line length for main blade section 1.
S2_SPLIT1_THICK_U60 stands for thickness value at 60 percent of the mean line length for the second section of the first splitter blade.




Side Metallic Angle
Metallic angle is available for both sides of any primary blade section. It is computed in (,θ) conformal plane and the calculated angles are given in degrees. Samples always apply on both sides.






Quantity


Examples






S?_(SPLIT?_)SS_METALANG_U??
S?_(SPLIT?_)PS_METALANG_U??


S1_SS_METALANG_U33 stands for metallic angle value at 33 percent of the suction side length for main blade section 1.
S2_SPLIT1_PS_METALANG_U60 stands for metallic angle value at 60 percent of the pressure side length for the second section of the first splitter blade.




Side Curvature
Curvature is available for both sides of any primary blade section. It is computed in (m,R*θ) plane and always applies on both sides.






Quantity


Examples






S?_(SPLIT?_)SS_CURV_U??
S?_(SPLIT?_)PS_CURV_U??


S1_SS_CURV_U33 stands for signed curvature value at 33 percent of the suction side length for main blade section 1.
S2_SPLIT1_PS_CURV_U60 stands for signed curvature value at 60 percent of the pressure side length for the second section of the first splitter blade.




The local curvature radius is obtained by inverting the curvature value.
Channel Width
For each primary section, the channel width is computed along a mean fluid line, built in the (,θ) conformal plane, between the suction side of the main blade and the pressure side of the adjacent blade. The channel path is defined as the mean fluid line portion that really "sees" consecutive blades. On FIGURE 95, locations s=0 and s=1 limit the channel path.
The width is then measured in spatial coordinates along the channel path and plotted versus its length fraction "s". The channel width is available for all primary sections in single blade cases only.


FIGURE 95 Channel width computation






Quantity


Examples






S?_CHANNEL_U??


S1_CHANNEL_U33 stands for channel width value at 33 percent of the fluid path length for section 1.




Mean Line Metallic Angle & Curvature
The mean line is the line located mid-way between suction and pressure sides. This line is built in (,θ) conformal plane where the metallic angle is computed. The curvature is processed in (m,Rθ) plane.






Quantity


Examples






S?_(SPLIT?_)ML_METALANG_U??


S1_ML_METALANG_U50 stands for metallic angle value at 50 percent of the mean line length for main blade section 1.




S?_(SPLIT?_)ML_CURV_U??


S2_SPLIT1_ML_CURV_U80 stands for signed curvature value at 80 percent of the mean line length for the second section of the first splitter blade.




Camber Metallic Angle & Curvature
The camber differs from the mean line when suction and pressure sides are built independently (with side curves method or asymmetric thickness addition).






Quantity


Examples






S?_(SPLIT?_)CAMBER_METALANG_U??


S1_CAMBER_METALANG_U50 stands for metallic angle value at 50 percent of the camber curve length for main blade section 1.




S?_(SPLIT?_)CAMBER_CURV_U??


S2_CAMBER_CURV_U80 stands for signed curvature value at 80 percent of the camber curve length for main blade section 2.




Beta Star
Angle βstar (expressed in degrees) is defined by relation (3-17a) and applies to either camber or mean line of each section.









Quantity


Examples






S?_(SPLIT?_)CAMBER_BETASTAR_U??


S1_CAMBER_BETASTAR_U50 stands for βstar angle value at 50 percent of the camber curve length for main blade section 1.




S?_(SPLIT?_)ML_BETASTAR_U??


S2_ML_BETASTAR_U80 stands for βstar angle value at 80 percent of the mean line curve length for main blade section 2.




Epsilon
Angle ε is defined by relation (3-17b) and applies to either camber or mean line of each section.
The value is expressed in degrees.









Quantity


Examples






S?_(SPLIT?_)CAMBER_EPSILON_U??


S1_CAMBER_EPSILON_U50 stands for ε angle value at 50 percent of the camber curve length for main blade section 1.




S?_(SPLIT?_)ML_EPSILON_U??


S2_ML_EPSILON_U80 stands for ε angle value at 80 percent of the mean line curve length for main blade section 2.

Fitting Results Check
At the end of the fitting process, the solution can be checked by checking the menu File/Fitting graphs.
After projection of the target curves on the fitted solution, the comparison graphs show the remaining differences between the projected target geometry and the fitted model. Overall improvements should be noticed on all graphs. If not, users should care about the following potential limitations:

After a fitting run, some bounds of parameters could have been reached and may prevent good fitting results as explained in the Visual Check & Parameters Manual Correction.
If the number of parameters defining a curve is low, the resulting curves will not be able to give very good results. An increase of the number of parameters will probably improve the fitted model, but could lead to a significant increase of the complexity (for optimization purposes).

Additional problems and possible solutions are described in the Fitting Problems section.

Meridional View
Edition of the meridional view is different from other views. Controls are never visible by default to avoid garbage on the screen, since many curves are drawn in the same graph: hub and shroud curves, sweep trace, edge traces and stream surfaces.
Generally speaking, curves appearing in the foreground color highlight if they can be edited and a selection is first needed to access its controls. Only a single selection of curve is possible, so the previous curve must be unselected to go on with selection.
Hub & Shroud Curves


FIGURE 38 Hub selection in meridional view
To edit hub or shroud curve, the curve has to be selected first, so that its controls are activated. This is done by a simple left click over the highlighted curve (FIGURE 38 left): the controls of the curve appear and the nodes can be edited as described above (FIGURE 38, right).
To leave the curve, another left click is required, outside the drawing of the curve and its controls.
When hub to shroud interpolation methods are selected, the user can control interactively the start and end of the reference stream surfaces for hub and shroud curves by left-clicking on it.


FIGURE 39 Modify start/end of reference stream surfaces
Stacking Reference Point
When a sweep law is available, its representation appears in the meridional view, but can only be edited in the sweep view (upper right viewport). Its reference point Z_STACKING_SWEEP or R_STACKING_SWEEP is however editable in the upper left view, but only appears when highlighted (FIGURE 40).


FIGURE 40 Reference stacking point highlighting
The reference point can move along the hub curve but does not exist when edge traces are selected in Stacking laws menu.
Edge Traces & Edge Points
Edge traces are always visible in the meridional view, but cannot be edited if the stacking sweep law is active (see previous paragraph). If selectable, left-clicking the trace shows its controls, as depicted in the left picture of FIGURE 41. The right picture shows that the four edge points can be edited just like the reference stacking sweep law, as explained above.


FIGURE 41 Edition of edge traces and end points
Selection of Section
Left-clicking the stream trace in the meridional view allows to display the corresponding section in lower views. This graphical selection acts as a replacement for the section selector from the main tool bar.
Contextual Menu
Right-clicking in the meridional view opens a popup menu that allows to edit endwalls (Edit hub/shroud) or to reverse them (Reverse hub/shroud). 



FIGURE 42 Popup menu for endwalls
Furthermore, when the meridional control is defined by means of leading and trailing edges location or/and when the rulings is activated, the menu allows respectively to edit the leading and/or trailing edge, or/and to edit the rulings settings for the main blade and the main blade ruling links.


FIGURE 43 Popup menu for leading/trailing and rulings

Camber & Thickness Construction Mode
The use of a thickness distribution in order to construct the pressure and suction sides from the camber line is mainly used in the fields of centrifugal turbines, compressors and pumps.
The thickness distribution is constructed by means of a Bezier or a B-spline curve. The ordinate values of the generated curve are exact half thickness values that are applied to the camber curve on its both sides to obtain suction and pressure side curves.


FIGURE 55 Thickness addition mode
Two different thickness distributions can be applied on the sides of the camber curve. The Symmetric option enables or disables the pressure side specific thickness distribution. The curve type is however common to both distributions (FIGURE 56).
If the camber curve has been defined between edge traces or by means of the meridional chord, the thickness distribution can be defined along the camber curve (S coordinate) or the meridional chord (m coordinate). If the camber is defined by the chord length, the thickness distribution can only be defined along the camber curve (the meridional chord could become negative).
The camber and thickness construction mode is compatible with all camber construction planes contrary to the independent suction and pressure sides mode (see Topological Compatibility Issues).
Using a thickness distribution defined along the meridional curve does not preserve the value of the radius at edges. Therefore, the general definition along the camber curve is preferred.
In case of axial machines, (Z,Y) and (m,R*θ) construction planes preserve distances. The length of the camber curve is straightforward and the blade section can be entirely constructed in these planes. This is unfortunately not so easy for the conformal (m,β) and (,θ) planes because they don't preserve the distances, so the length of the camber curve is not known until the curve is projected on the stream surface. For those planes, the construction of the blade section is still allowed in two steps:

First, the camber curve is constructed in (m,β) or (,θ) plane and is then projected on the stream surface, where the length of the camber curve can be computed.
Second, the thickness distribution is generated and applied along the projected camber curve, directly on the stream surface.



FIGURE 56 Settings for camber and thickness mode
The thickness distribution can be built from three different methods (FIGURE 56). Their definitions and related options are covered in the next pages:

a single high order Bezier curve,
a B-spline curve with optional ending circular arcs,
a parameterless user-defined law.

In addition to the number of parameters, a points Distribution control (uniform, geometric or twice_geometric) allows to alter the concentration of points which - by default - is uniform along the definition axis. A stretching factor larger than one results in a higher concentration towards the leading edge while a lower value moves that concentration towards the trailing edge when the geometric distribution is selected.
Bezier curve


FIGURE 57 Relation between the number of parameters and the degree of the corresponding Bezier curve
Leading and trailing edges can be either rounded or blunt. According to these choices, the number of control points used by the curve can differ from the amount of parameters specified in the interface. The examples in FIGURE 57 assume a Bezier curve with 4 parameters:

In the blunt case, a single control point is used at the edge, so that the number of user specified parameters equals the number of control points.
In the rounded case, three control points are needed at the edge to maintain both prescribed radius and perpendicularity to the abscissa axis.

A general formula for the number of control point n can be presented in the form
n = 2 x number of rounded edges + number of user parameters
The parameters menu keeps trace of the parameters names as HALF_THICKNESS_P(j) variables except when a rounded edge is involved, where the notation LE_RADIUS and TE_RADIUS are used.
Rounded edge construction
The method applied for the rounded edge radius computation uses the equation below where a is the first control segment length and b is the distance between the third control point and the first control segment. In the present case, this expression is simplified thanks to the assumption that a equals the prescribed radius value (FIGURE 58). Parameter b is then the only unknown in the equation and can be easily computed. The height of the third control point is fixed by convention to the same radius value and, although it controls the curve locally, has no influence on the curvature radius at the edge point.

 
becomes

 
when a=R


FIGURE 58 Rounded edge radius construction (leading edge case)
.






Parameter


Description






S(i)_HALF_THICKNESS_P(j)


half thickness parameter (j) for blade section (i)




S(i)_RADIUS_LE


prescribed curvature radius at leading edge for section (i)
This value replaces S(i)_HALF_THICKNESS_P0 in rounded case




S(i)_RADIUS_TE


prescribed curvature radius at trailing edge for section (i)
This value replaces S(i)_HALF_THICKNESS_P(n) in rounded case




When an independent thickness distribution is applied on the pressure side, parameter names contain an additional string 'PS' and become S(i)_PS_HALF_THICKNESS_P(j), S(i)_PS_RADIUS_LE and S(i)_PS_RADIUS_TE.




B-Spline curve with optional circular ends
A B-Spline curve does not offer the same properties in terms of continuity, and therefore it is usually exclusively used in blunt cases. It is however possible to add an optional circular arc at one or both ends and to make the corresponding edges rounded. Continuity is then ensured up to the first derivative.
The relationship between amounts of parameters and nodes is straightforward when a blunt is used at both ends. When a circle arc is added at one end, the end node of the B-Spline curve is not controlled directly and the corresponding parameter HALF_THICKNESS_P(j) is replaced by two parameters RADIUS and HALF_WEDGE_ANGLE. All four combinations of blunt and rounded edges are shown in FIGURE 59 in the general case.


FIGURE 59 Rounded and blunt distributions based on a B-Spline curve
Besides those general cases, wedge angle parameters disappear when fewer parameters are set, resulting in the following two distributions:

Linear case, when only two parameters exist and whatever edge options are selected (the top picture in FIGURE 60 shows the rounded edge case).
Constant case, when a single parameter exist (the bottom picture in FIGURE 60 shows the rounded edge case).



FIGURE 60 Linear and constant thickness cases
In those two special situations, the edge angle parameter is automatically constrained. Therefore, there are no combinations of three and four parameters!






Parameter


Description






S(i)_HALF_THICKNESS_P(j)


half thickness parameter (j) for blade section (i)




S(i)_LE_RADIUS


prescribed curvature radius at leading edge for section (i)
This value replaces S(i)_HALF_THICKNESS_P0 in rounded case




S(i)_TE_RADIUS


prescribed curvature radius at trailing edge for section (i)
This value replaces S(i)_HALF_THICKNESS_P(n) in rounded case




S(i)_LE_HALF_WEDGE_ANGLE


leading edge half wedge angle when at least one of the edges is rounded
This parameter does not exist in a constant or linear thickness distribution or when both edges are blunt




S(i)_TE_HALF_WEDGE_ANGLE


trailing edge half wedge angle when at least one of the  edges is rounded
This parameter does not exist in a constant or linear thick ness distribution or when both edges are blunt




When an independent thickness distribution is applied on the pressure side, parameter names contain an additional string 'PS' and become S(i)_PS_HALF_THICKNESS_P(j), S(i)_PS_LE_RADIUS, S(i)_PS_TE_RADIUS, S(i)_PS_LE_HALF_WEDGE_ANGLE and S(i)_PS_TE_HALF_WEDGE_ANGLE.




Half wedge angles do not exist in a blunt-blunt configuration. Bessel end conditions are applied instead.
Because of the need for the additional parameters for the half wedge angles some numbers of parameters (3 and 4) are not allowed in the interface.
User-defined law
Three types of user-defined laws are available:
1) Data file
If the thickness law is available as an external data file, it can be imported as a user-defined law in the parametric model. This law is then free of parameters and, once applied, can be edited in the graphics area.
File format
As for user-defined endwalls, the distribution is defined in a simple text format, as illustrated in the example below.
# comments
59			(amount of defining points)
0.0	0.0
0.01	0.125		('s' abscissa and half-thickness value)
0.03	0.25
...
0.97	1.23
0.99	1.24
1.0	1.245
The first input number is the amount of provided points. Then, each line defines a single point by means of the following coordinates:

the first coordinate is the fraction of the camber curve length at which the thickness is defined (real fractional length ranging from 0.0 to 1.0),
the second coordinate is the prescribed half-thickness, that may be given as a fraction of the camber length (NACA style) or a real measurement of the half-thickness.

A comment may be added anywhere provided that it starts the line with '#' character.
To provide easier input, two special keywords STARTING_ABSCISSA and ENDING_ABSCISSA are allowed either at start or end of the file to transform starting and ending values for the abscissa of the distribution. For instance, the two instructions below tell AutoBlade™ that the abscissa 50.0 should be considered as 0.0 and abscissa 100.0 as 1.0. A linear transformation is defined by these two parameters and applied to all provided abscissa values.
starting_abscissa		50.0
ending_abscissa		100.0
Once read, the thickness file is stored in the parametric model and the file may be deleted. This allows to manage the model as a whole.
All provided points generate a spline law for smooth interpolation of half-thickness values, especially near ends.
File options and input
Two selectors allow to define a distribution for each side (if asymmetric) and primary section. The following controls allow to tune the selected distribution (FIGURE 61):

The option Include points as parameters allows to include all reference points as regular parameters for the fitting or the optimization. This means that the law can be initialized and even altered by the fitting process!
The option Number of nodes is used to specify the number of the points in the inputted file. If the number of the defining points has been defined in the inputted file, the option Number of nodes will be neglected.
The option Dimensional abscissa specifies either if the abscissa must be considered as the values read (checked) or if the provided abscissa must be scaled by the length of the camber curve (unchecked).
The option Dimensional height specifies either if the half-thickness must be considered as the values read (checked) or if the provided law must be scaled by the length of the camber curve (unchecked). Default is dimensionless thickness (unchecked state) that corresponds to the NACA style definition.
The option Abscissa factor allows to scale the abscissa by means of the optional floating point value (on the right side).
The option Height factor allows to scale the ordinate of the prescribed half-thickness by means of the optional floating point value (on the right side). This option is useful to define a scaled thickness from hub to shroud, while reusing the same thickness file, or to adapt a reference law.



FIGURE 61 User-defined thickness law and options
The user-defined thickness can be only inputted by Right-clicking in the SIDES view, as shown in FIGURE 43.


FIGURE 62 Input use-defined thickness
In the Init curve from file dialog, the user can enter the path ended by a hit on the <Enter> key or click the button on the right and use a classic file chooser. By default, no file is active and the value in the field is none. Once selected, the file is parsed and checked: if the color of the field is changed to red, this means that the file does not comply with the format specification described above!
When no valid thickness file is selected, a default thickness law is applied when Ok is clicked.
If the camber curve is modified, the final thickness is also changed when it is defined in NACA style (unchecked Dimensional height). User-defined thickness is not constant in that case and this must be pointed out for optimization projects!
Optional rounding
When the thickness is not defined at edges or if the edge is assumed blunt, the resulting section will be treated as a blunt. It is possible to define a rounded edge from the thickness file; but this is not advised because the quality of the edge shape highly depends on the amount of defining points.
In rounded cases, AutoBlade™ provides additional options under the areas Leading edge and Trailing edge. These boxes do not appear until the thickness file is selected, because the default values of these fields are set according to the content of the thickness file.

The default option leaves the thickness law unchanged (FROM_FILE option)
Automatic elliptical rounding (ELLIPTICAL option) defines an elliptic arc to close the edge and ensures C1 continuity with the prescribed law (continuity of the tangent). This is the preferred option for the leading edge, but this method does not provide control of the starting curvature radius (FIGURE 63).
The circular rounding (deprecated CIRCULAR option) allows to define a circular edge linked to the prescribed law by a linear segment starting from a relative location (round at field) on the abscissa axis. This method is convenient for the trailing edge, with a precise curvature radius, but C1 continuity is not provided (FIGURE 64).
The circular rounding with tangency (CIRCULAR_TGT option) tries to find a location where the linear segment can be connected to the prescribed law with a marginal error on the continuity of the tangency (FIGURE 65). This option is preferred to the previous one and behaves the same way when no suitable location can be found, thanks to the relative location value in round at field.



FIGURE 63 Automatic elliptical rounding at prescribed 's' location


FIGURE 64 Circular rounding with linear segment at prescribed 's' location


FIGURE 65 Circular rounding with linear segment and C1 continuity
The existence of a solution for the CIRCULAR_TGT option highly depends on the external law and the prescribed radius. The search ranges in s relative location are [0,0.5] for the leading edge and [0.5,1] for the trailing edge: if no location that satisfies the C1 continuity can be found, an error is generated and the CIRCULAR rounding is applied.
2) Expression
The thickness can be defined by a mathematical expression involving a single parameter 's' for each blade, each section and each side. In order to simplify the user input, this expression can use an existing function with an arbitrary amount of arguments. The thickness is evaluated after all parametric dependencies are solved and evaluated. Therefore, the value of all existing parameters is already available as input.
For the thickness law, a variable must be reserved for the reduced abscissa and is assumed to be 's' by default. All other symbols must be constants, existing parameters or other functions.


FIGURE 66 User-defined expression
It is allowed that the expression does not contain the abscissa 's'. In this case, the expression is a constant.
3) NACA45
A built-in definition for NACA thickness laws (NACA 4 and 5 digits) has been introduced as a user-defined thickness, since this law is common to the original NACA 4 and 5 digits and often used in blade definitions. 
The reduced thickness for NACA 4 and 5 digits is given by:



where tmax is the maximum relative thickness (in percent) and x is the reduced abscissa variables (defined over [0,1]). 


FIGURE 67 User-defined NACA45
NACA is a blunt thickness, so one of the existing rounding options should be used to round the distribution at the training edge.
There is no difference between NACA 4 and 5 digits for the thickness definition.
4) Parameters
If the user selects the user-defined laws, some parameters are added in the Parameter list menu when

an optional height factor is selected,
an optional rounding option is applied.

Those parameters are especially useful for fitting purposes.






Parameter


Description






S(i)_HEIGHT_FACTOR


optional height factor in user-defined thickness law for blade section (i)




S(i)_LE_RADIUS


prescribed curvature radius at leading edge for section (i)
This parameter only applies when the special rounding option CIRCULAR or CIRCULAR_TGT is selected at the leading edge




S(i)_TE_RADIUS


prescribed curvature radius at trailing edge for section (i)
This parameter only applies when the special rounding option CIRCULAR or CIRCULAR_TGT is selected at the trailing edge




S(i)_LE_START


starting s abscissa of optional rounding at leading edge for section (i)
This parameter applies when a rounding option is selected and effectively used with CIRCULAR and CIRCULAR_TGT options




S(i)_TE_START


starting s abscissa of optional rounding at trailing edge for section (i)
This parameter applies when a rounding option is selected and effectively used with CIRCULAR and CIRCULAR_TGT options




When an independent thickness distribution is applied on the pressure side, parameter names contain an additional string 'PS'




Since the CIRCULAR_TGT rounding option is very sensitive to the distribution of the tangent in the spline law, the graphical edition of the control points in the thickness view can lead to a flickering effect.

GeomTurbo 5.3
This format is the preferred target input, at least for multiple splitter fitting projects, but may require AutoGrid™ software if used as output of AutoBlade™.
The ".geomTurbo" file format 5.3 is structured in three main blocks: the header, the channel and the definition of the rows. Following is a example of a geomTurbo file structure for a turbomachinery with three blade rows respectively named impeller, diffuser and return channel.
GEOMETRY TURBO
VERSION 5.3
NI_BEGIN CHANNEL
...
NI_END   CHANNEL 
NI_BEGIN nirow
NAME impeller
...
NI_END nirow
NI_BEGIN nirow
  NAME diffuseur
...
NI_END nirow
NI_BEGIN nirow
NAME return channel
...
NI_END nirow
AutoBlade™ does not support all options of the format, especially the following features:

gap curves at hub and shroud,
bulbs and nozzles,
IGG™ data and CAD data (Parasolid™ format) except for non-axisymetric hub and/or shroud.

Further details about the original geomTurbo format 5.3 and keywords can be found in the AutoGrid™ User Manual.
Channel Format
The channel format contains the definition of the turbomachinery meridional contours (hub and shroud). It is defined by two types of curves:

The basic curves defined by a set of points
The channel curves defined as a composite of basic curves.

NI_BEGIN CHANNEL 
 NI_BEGIN basic_curve
  NAME curve_1
  ...
 NI_END   basic_curve
 NI_BEGIN basic_curve
  NAME curve_2
  ...
 NI_END   basic_curve
 NI_BEGIN channel_curve hub    
  NAME hub
...
   NI_END   channel_curve hub    
 NI_BEGIN channel_curve shroud 
  NAME shroud
  ...
 NI_END   channel_curve shroud 
 NI_END   CHANNEL 
The ".geomTurbo" file must contain two channel curves named respectively hub and shroud. In addition, AutoBlade™ does not currently support channels defined as composite of several basic curves.
AutoBlade™ is not accepting hub and shroud defined as ZR curve along partly Z-axis (R=0), ZR curve crossing Z-axis or ZR curve defined with negative radius.
Basic Curves
The basic curve format is used to defined a curve and project it in the meridional space (z,r). The curve is defined at least by

a name,
a coordinate type,
the number of defining points,
the list of points coordinates

 NI_BEGIN basic_curve
  NAME curve_1
  DISCRETISATION 10
  NI_BEGIN zrcurve
   ZR 
   28
   -0.0425   0.256692
   -0.0312928   0.25656
...
    NI_END zrcurve
 NI_END   basic_curve
The coordinate types are identified by the following keywords: ZR, XYZ, RTHZ, ZRTH, THRZ, RZTH,... where X,Y and Z are the 3 Cartesian coordinates and R,TH and Z are the 3 cylindrical coordinates.
The discretization value and optional interpolation type are not used by AutoBlade™.
Channel Curves
The channel curves are used to define the hub and the shroud. A channel curve is a composite of defined basic curves. It is defined by a name and vertices. The vertex should be an absolute vertex or belong to a basic curves and is defined by its parametric location (normalized arc length).
 NI_BEGIN channel_curve hub    
  NAME hub
VERTEX ABS_P 0 0 0
  VERTEX curve_1 0
  VERTEX curve_1 1
 NI_END   channel_curve hub    
 NI_BEGIN channel_curve shroud 
  NAME shroud
  VERTEX curve_2 0
  VERTEX curve_2 1
 NI_END   channel_curve shroud 
The fitting module uses a single discretized curve. This means that a complex composite curve that shows several discontinuities in AutoGrid5 will be converted to a single linearly interpolated curve that does not strictly preserve the vertices.
Row Format
The row format contains the geometry definition of a complete row. It is defined by a row name, a row type, a periodicity and the definition of the main blade and possibly one or more splitter blades.
NI_BEGIN nirow
  NAME impeller
  TYPE normal
PERIODICITY 36
UNITS 1
NI_BEGIN NIBlade
  NAME main Blade
...
NI_END NIBlade
NI_BEGIN NIBlade
  NAME splitter 1
...
NI_END NIBlade
...
NI_END nirow
Row Periodicity
The periodicity defines the number of main blades in the row. 
Units
The units keyword is never used by the software. However, it is preserved in export when the model has been initialized on a target that contains the keyword. Otherwise, it is not exported to the geomTurbo output!
AutoBlade™ allows a global scaling factor in the Steerings page and is completely unrelated to the units keyword.
Blade Definition
The blade(s) and possibly the splitter(s) are defined by a name and two surfaces defining the pressure and the suction side. The surfaces are identified by the keywords pressure and suction:
NI_BEGIN NIBlade
  NAME main Blade
NI_BEGIN nibladegeometry
TYPE GEOMTURBO
suction
...
pressure
...
NI_END nibladegeometry
NI_END NIBlade
The pressure side and the suction side are defined by a set of cross sections of the blade at several spanwise location. Each section is defined by a set of points:
suction
SECTIONAL
13
#   section 1
XYZ
100
0.17669 -0.0208609 0.000351471
0.176691 -0.0208788 0.000370063
...
#   section 2
XYZ
100
0.17669 -0.0208609 0.000351471
0.176691 -0.0208788 0.000370063
...
The coordinate types of each sections are identified by the following keywords: ZR, XYZ, RTHZ, ZRTH, THRZ, RZTH,... where X,Y and Z are the 3 Cartesian coordinates and R, TH and Z are the 3 cylindrical coordinates.
A few optional keywords are supported after the suction and pressure keywords. Further details about the keywords can be found in the AutoGrid™ User Manual.

File Menu
This menu contains the usual commands for the file management and session settings.

Some entries may appear greyed out, meaning they cannot be activated in this context. This typically occurs when

no model is loaded in the interface (Save and Save As entries are not available),

AutoBlade™ is accessed as a tool from Design3D interface (only Save and Preferences entries are available).


New
This menu creates a new AutoBlade™ project. A small dialog pops up when activating File/New or clicking the corresponding icon in the main toolbar, as shown in FIGURE 3. 


FIGURE 3 Create a new project
This allows the user to start from scratch or create a new project from an existing parametric model. The Ok button is greyed until a valid parametric file has been selected. When Ok is clicked, a file browser is opened (in both cases) to select a new file name for the project.
White spaces should be avoided in the file name.
Open
There are two ways to open an existing project file:
Use File / Open menu
This menu opens an existing AutoBlade™ project. The user can open a project file (*.abp) directly. As an alternate solution, the filter in the file browser can be changed to parametric file (*.par). In the latter case, AutoBlade first tries to locate the corresponding project file (same path and name) and loads it or select the parametric file as starting model and calls a second file browser for the new project name (acts as File/New with starting model).
Select File From the List of Files in File Menu
The File menu lists the names of the five most recent projects that have already been opened. Clicking on a project name from this menu will open it. When clicking on a project name in the File menu, AutoBlade first prompts for save if the current project is modified.
When a project file from the saved list is not physically present on disk at startup, it is deleted from the list.
Save 
The File/Save menu stores the project on disk.
Save As
The File/Save as menu is used to store the current AutoBlade™ project to a new location.
Properties
Description
The tab Description allows the user to add customized information in the project.


Parasolid
Under the tab Parasolid, the user can applies an internal scaling factor and activate the solid model.


The Internal scaling factor for Parasolid is used to keep the range of data within suitable limits internally. This scale factor has no visual impact on the data in the views and is independent of the Edit/Scale command or the target geometry scale factor.
The scaling factor is automatically adapted in the following cases if the bounding box extent is smaller than 0.01 or larger than 100.0:

at import or read a parametric model coming from a previous version,
at adaptation step on a target geometry (fitting module).

The user can also activate this scaling and change the scaling factor.
By default, sheet models are generated for all models, which are used for 3D view and CAD surfaces output. The button Solid model allows the user to build solid body for the designed blade in addition to the sheet models and check it in the 3D view. 
The following limitations apply to the solid model:

the solid model is not compatible with ruled blades using late rounding option.
when the solid model is active, the bottom and tip closure surfaces are not defined as part of revolved surfaces.
Both sheet and solid models require more time for update, especially when many sections and many points are involved in curves. In Design3D, the update has significant impact in the optimization phase when using the ANN (as the ANN needs updated quantities as input, the parametric model is updated for each sample)

Report
The tab Report shows the general parametric information.


Preferences
The menu File/Preferences opens the Preferences dialog that gives access to some project specific and global settings.
Session page


Amount of undo/redo is used to specify the maximum number of the undo/redo steps. When the limit is achieved, the oldest editions are deleted, but the persistent steps are kept with a higher priority than volatile steps.
Parasolid tolerance is used to set the tolerance to treat Parasolid geometry.
The button create backup files (.bak) is used to make a backup of the existing project file and the data directory at saving.
Curves page
Different styles and colors are used to draw and highlight the graphical items in the main interface of AutoBlade™. Most curves appear in foreground color, but the graphical representation of their control polygon, nodes and angular parameters are drawn in a different color. If an item can be picked, monitored or selected, its color changes according to the imposed color selected in the Curvestab from the File/Preferences menu by left-clicking on the color.


FIGURE 4 Curves color control
Display page
Furthermore, the background and foreground colors are controlled in the Display tab from the File/Preferences menu.


FIGURE 5 Background/foreground colors control
Quit
Select the menu File/Quit to quit the interface.

Rulings (for flank-milled blade only)
When activating Activate rulings, the ruling direction for flank-milled blades (i.e. centrifugal impellers) can be controlled, by means of simple sampling of the two camber curves and an interactive definition of the links between those samples in the meridional view. The resulting geometry is built with Parasolid™.


FIGURE 16 Ruling control for flank-milled blades
The ruling directions are straight links between samples defined on the two cambers. This treatment requires the definition of the cambers, but not the side curves, that will be built just after. For clarity and ease of management, exactly two primary sections are required and no parametric sections are allowed for controlled ruling.
Imprint directions on side surfaces allows to visualize the ruling directions on the 3D model.        
In the Configuration of the stream surfaces dialog box, links can be quickly reset. For instance, it is possible to select 50 samples and generate 9 links between the two cambers, just by activating Reset rulings. By default, the ruling consists in a uniform sampling in (m,R*θ) over the two primary camber curves and links between some of these samples. The user can also apply a clustering (uniform-geometric) in case of a rounded edge. The clustering will apply an uniformly distributed samples near the middle of the camber traces and a geometric progression near the edges. The Global ratio is defined as the edge spacing over the central spacing between the samples.
Clustering is only applied in the vicinity of a rounded edge. If the edge is blunt, an uniform spacing is automatically applied.
 After generating the links, the leading and trailing edges are fixed links but any intermediate link can be added or deleted when right-clicking in the meridional view and selecting Edit rulings settings for main blade.


FIGURE 17 Ruling settings

Reset links and samples  allows to modify the number of nodes and links. 
Modify sampling allows to modify the sampling and update the previous links to start and end on the closest samples.
Refine sampling allows to insert intermediate samples by changing the Number of internal samples without losing the previous sampling. 

The nodes and links are visualized in the meridional view when right-clicking in the view and selecting Edit main blade ruling links . The link nodes can be picked and can be set to another node by left-clicking.


FIGURE 18 Ruling links interactive control

Fitting Control subpad
This subpad, Fitting Control,  in the left area - grants access to control the fitting process (FIGURE 30). Some associated commands can be found under the Analysis menu whereas others are only accessible through this subpad.
Before starting the fitting process, the designer needs to change the topological settings and parameters of the current model. All operations on the current model are allowed, except new, open, save and save as.


FIGURE 30 Fitting Control subpad
Adapt model
The button Adapt model allows to launch the initialization process on the current model (the one displayed in graphical interface), see Setup Initial Model and Initialization Process for more detail.
Fit model
The button Fit model allows to launch the fitting process and the settings of the optimization algorithms. Details about this step is covered in the Fitting Process section.
Generate report
The button Generate report is used to export the parameters of the fitting process to a file. The following data will be included in the exported report:

general information (number of the blades and number of the sections),
fitting features that are fitted,
parametric report with all the parameters and their values,
error report of the fitting features between the target and the fitted model,
analysis data.

Fitting graphs



This button provides a graphical comparison of the current design and the projected target curves. It is very useful to verify the model after an initialization or a fitting process. 
The comparison always applies between the current design and the projected target curves. If the button is disabled, a new projection is required.
The Fitting graphs page is not accessible until the initialization process has been finished.
Two entries allows the selection of a graph containing:

the endwall curves,
the meridional and tangential edge traces,
the sweep and lean laws,
the side curves of a primary section.

Sections can be compared in the following planes. Some of them could be meaningless according to the machinery type:







(, θ)


(m,Rθ)


(Z,Rθ)




(R,Rθ)


(Z,R)


(Z,Y)




(X,Y)


 


 




By default, the comparison of the sections in the different viewing planes involve the stacking laws. If selecting the button Unstacked view, the stacking laws will not be applied in order to allow an easier check of the error in shape.


FIGURE 31 The fitting graphs comparison page
Fitting log file



This button allows to access the log file of the fitting steps.


Fitting Convergence



This button allows to visualize the convergence of the fitting steps as well as the evolution of each free parameter within its bounds.

Modules Menu

This menu allows to switch to other products integrated into the FINE™ interface. Currently, FINE™/Turbo and Design3D are the only options.
If a model is opened and modified, AutoBlade™ always prompts for save before the effective switch to the selected module.

Graphical and Exported Outputs
The construction of the surfaces is treated in Parasolid™ format.
Export of the non-axisymmetric surfaces is allowed in both geomTurbo 5.3 and IGES formats.
The non-axisymmetric surfaces can be activated in the 3D view, but are not shown as default. Their display is either limited to a single blade occurrence or repeated just like blades.

Export parametric model
The menu Geometry/Export parametric model... opens a file chooser and prompts for a location where to save the parametric model with default extension ".par".

Meridional Location
AutoBlade™ provides two methods to define the location of the blade sections in the meridional view. They are the sweep law curve and the leading and trailing edge traces.
Sweep Law Curve
This method consists in defining a stacking curve in the meridional view that will extend from hub reference trace (span value 0.0) to shroud reference trace (span value 1.0). AutoBlade™ is then able to align the selected stacking point of the 2D sections along this sweep curve.


FIGURE 24 Sweep law menu
The curve is not constructed directly in the (Z,R) plane, but in a non dimensional construction (z,span) plane (FIGURE 25). The following formula is applied to compute the stacking locations in the (Z,R) plane, ZRef being the origin of the sweep curve (Origin) on the hub or on the shroud reference trace (Z_stacking_sweep in the list of parameters). The major interest of this transformation is that angles are preserved.





FIGURE 25 Stacking sweep law definition
When a span parameter value lies outside of the interval [0,1], a linear extrapolation is applied and continuity is assured up to the first order (C1, continuity of the first derivative with respect to the span parameter).
Five curve types can be used to achieve the sweep law:
Line
A line is advantageous when the stacking is straight or linear: in optimization, this law involves a single angular parameter β (FIGURE 26, left) and ensures a perfect linear stacking if more than two primary sections are defined.
Second order Bezier curve (3 control points)
This simple law is a second order Bezier curve defined by three control points respectively at span 0.0, 0.5 and 1.0. The three user defined parameters are axial reference position at hub ZRef, angles β1 and β2. In our example (FIGURE 26, center), angle β1 is negative and angle β2 is positive.
Composite Bezier - line - Bezier curve
The alternative is a composite Bezier-line-Bezier curve. The Bezier curves are second order curves joined together with a straight line segment. The first control polygon is defined by parameters C1, P1 and angle α1, the second by (C2,P2,α3) and line angle α2 is common to both to assure C1 continuity (FIGURE 26, right).


FIGURE 26 Available sweep laws
All angles are measured clockwise from a line at constant z.






Parameter


Description






Z_STACKING_SWEEP


Z value for the stacking point on stream surface at span = 0 (close to hub) or span = 1 (close to shroud)




Line:




SWEEP_BETA


angle β of the line (in degrees)




Second order Bezier curve (3 control points):




SWEEP_BETA1


angle β1 of the Bezier curve at span = 0 (in degrees)




SWEEP_BETA2


angle β2 of the Bezier curve at span = 1 (in degrees)




Bezier-line-Bezier composite curve:




SWEEP_ALPHA1


angle α1 of the first Bezier curve at span = 0 (in degrees)




SWEEP_C1


spanwise extent of the first Bezier curve




SWEEP_P1


fractional factor defining the second control point location of the first Bezier curve




SWEEP_ALPHA2


angle α2 of the linear segment (in degrees)




SWEEP_ALPHA3


angle α3 of the second Bezier curve at span = 1 (in degrees)




SWEEP_C2


spanwise extent of the second Bezier curve




SWEEP_P2


fractional factor defining the second control point location of the second Bezier curve




Bezier & B-spline curve defined by an arbitrary amount of nodes
Wind turbines are defined by more complicated shapes and controlling their stacking requires a larger amount of sections. In release AutoBlade™ 2.1, the more general stacking law is a composite Bezier-line-Bezier curve that allows a perfect stacking (sweep and lean) for 5 to 7 sections. This is clearly insufficient for wind turbines blades, where 10 to 15 primary and parametric sections may be necessary for good control of shape and stacking. Therefore, a new and more general stacking law has been added.
The proposed law is either a Bezier or a B-spline curve defined by an arbitrary amount of nodes along the span (Number of parameters).


FIGURE 27 Stacking Law: Meridional location control
To simplify the optimization, only the Z or θ coordinate is parametric (Hi), the nodes being by default equally spaced along the span (left picture in FIGURE 28). In addition, this distribution can be stretched along the span by means of a geometric or twice_geometric progression where the ratio are defined (first/second common ratio).


FIGURE 28 Sweep law ruled by a geometric progression (left picture) and all the distribution types available (right pictures) 
The geometric progression (left picture in FIGURE 28) will always lead to an asymmetrical distribution of the points while the twice_geometric may lead to a symmetrical distribution when imposing the same stretching factor (first/second common ratio).
Leading & Trailing Edges Traces
Edge traces fully constrain both the meridional location and the extent of the blade sections. Edge traces need two end points and the curve is built directly in the meridional plane (Z,R). This method does not make use of the stacking point because the traces completely define the blade sections in the meridional view.
The end points of each trace are defined using either a coordinate - Z or R - on hub and shroud curve or a non dimensional location measured along the endwalls.


FIGURE 29 Leading and trailing edges traces menu.






Parameter


Description






End points defined by coordinates:




Z_LE_HUB / R_LE_HUB


Z or R starting coordinate for leading edge on hub trace




Z_LE_SHROUD / R_LE_SHROUD


Z or R starting coordinate for leading edge on shroud trace




Z_TE_HUB / R_TE_HUB


Z or R starting coordinate for trailing edge on hub trace




Z_TE_SHROUD / R_TE_SHROUD


Z or R starting coordinate for trailing edge on shroud trace




End points defined by a fractional length along the endwall curve:




S_LE_HUB


end point location along hub curve for leading edge




S_LE_SHROUD


end point location along shroud curve for leading edge




S_TE_HUB


end point location along hub curve for trailing edge




S_TE_SHROUD


end point location along shroud curve for trailing edge




Five laws are available to define each trace. Traces are extrapolated linearly when spanwise locations below 0.0 or above 1.0 are requested or when reference traces differ from endwall contours.
Parameterless line
A linear trace free of parameters can be selected as the simplest law FIGURE 30 (top picture). This is the default.
Second order Bezier curve (symmetric)
Leading and trailing edge traces are defined by means of a second order Bezier curve controlled by three points. User input is simplified by the assumption that both control segments have the same length and therefore, only one additional angular parameter βLE or βTE is necessary.
On FIGURE 30 (bottom left  picture), βLE is defined as the angle between:

the segment joining the intersection points of the edge trace with hub and shroud curves,
the first control segment of the edge trace.

This angle is measured clockwise and a similar definition applies for the trailing edge curve.
Third order Bezier curve
The above law is indeed very simple and does not comply with all topologies.This second curve is controlled by four points and allows more freedom, especially when the trace is not symmetric. It requires four additional parameters, as depicted in the bottom right picture of FIGURE 29.


FIGURE 30 Meridional blade passage definition using edges traces






Parameter


Description






Second order Bezier curve:




LE_MERIDIONAL_BETA


angle βLE controlling the leading edge trace (in degrees)




TE_MERIDIONAL_BETA


angle βTE controlling the trailing edge trace (in degrees)




Third order Bezier curve:




LE_MERIDIONAL_BETA1


angle β1 controlling the LE control segment near hub




LE_MERIDIONAL_C1


projected fractional length of LE control segment near hub




LE_MERIDIONAL_BETA2


angle β2 controlling the LE control segment near shroud




LE_MERIDIONAL_C2


projected fractional length of LE control segment near shroud




TE_MERIDIONAL_BETA1


angle β1 controlling the TE control segment near hub




TE_MERIDIONAL_C1


projected fractional length of TE control segment near hub




TE_MERIDIONAL_BETA2


angle β2 controlling the TE control segment near shroud




TE_MERIDIONAL_C2


projected fractional length of TE control segment near shroud




Bezier & B-spline curve defined by an arbitrary amount of nodes
The proposed law is either a Bezier or a B-spline curve defined by an arbitrary amount of nodes along the span (Number of parameters).  


FIGURE 31 Stacking Law: Meridional location control
In addition, this distribution can be altered by means of a geometric or twice_geometric progression  where the ratio are defined (first/second common ratio).

Model Editor subpad
This menu - the subpad Model Editor in the left area - grants access to the governing topological settings of the blade definition as well as some quantities and distributions (FIGURE 27). All associated commands can alternatively be found under the Geometry and Analysis menu.


FIGURE 27 Model Editor subpad
Nine Design Steps
Nine successive design steps can be outlined (fully described in the AutoBlade™ Modeller chapter) and make up the first part of the menu:

definition of the curve type used to shape the endwall contours,
selection of the stream surfaces type, spanwise type and location of the 2D sections,
definition of the stacking point, sweep and lean laws,
definition of the topology for the main blade: selection of the construction plane, camber curve type, construction of the suction and pressure sides and settings for the edges,
definition of the topology for the optional splitter blades: number of additional blades, optional camber refinement and settings of the side curves,
optional technological effects,
definition of the non-axisymmetric hub surface,
definition of the non-axisymmetric shroud surface.
definition of the solid geometry such as the axisymmetric wheel and shroud components in the RZ frame.

These nine menus - activated by the green buttons - can be seen as successive steps that need to be performed in order to build the model. The features are however dependent, which explains why it is not possible to edit two of them at the same time. For example, changes in endwall curves can affect stream surfaces and a change in the stream surface type will alter the definition of the blades. On the contrary, changes in the definition of a section cannot modify the endwall curves.
FIGURE 28 illustrates the behavior of the menu when the Stacking laws button is clicked.


FIGURE 28 Opening a topology menu excludes others
The Parameter list menu cannot be opened when a topology step is edited. On the contrary, Optional quantities, Geometry analysis and Parametric report tools are allowed and updated automatically.
Error Messages
When an error or a potential problem is detected in the update of the model, AutoBlade™ will report failures and warnings in the message list. The graphical menu will be updated accordingly and the color of the failing step is changed to red. Subsequent steps are frozen and appear in gray color to indicate that the corresponding parts of the model are also incorrect. In such a case, quantities are not updated.
For instance, if the meridional location of the edge traces fails for some reason, the graphical menu will appear exactly as in FIGURE 29. The dedicated message window can be opened to get further information about the error (see the Show messages section for details about the Message window).


FIGURE 29 The graphical menu is updated when an error occurs
Optional Quantities



This menu allows the computation of geometrical quantities such as blade thickness and moments of inertia for every section. All values and samples are affected by the changes of the parameters and topologies in the menus described above. The Optional Quantities section is devoted to the available quantities, their definition and how they are computed.
When topology settings or parameters are changed while the menu is opened, the quantities are automatically updated.
Geometry Analysis



The Geometry analysis tool consists in graphs showing distributions of useful properties like endwall curvature, side metal angle or section thickness. Please consult the Geometry Analysis section for more details.
When topology settings or parameters are changed while the menu is opened, the distributions are automatically updated.
Parametric Report



The Parametric report consists in the description of the total number of parameter and the free, frozen and dependent parameters in order to ease the parameters and their dependencies analysis (see the Parametric Report section for more details).

Export solid sector geometry
The menu Geometry/Export solid sector geometry... opens a file chooser and prompts for a location where to save the merged blade and solid body in parasolid format, see Solid Body for more details.
The exported solid sector geometry may be a single sector or the full 360 degree body, depending on the Repetition option in the menu View / 3D view options under the tab Geometry.


FIGURE 14 Examples of exported solid sector geometry

Introduction
What is AutoBlade™?
AutoBlade™ has been developed in the context of a wider product able to provide to the user a complete and very efficient environment for the design of turbomachinery blades. AutoBlade™ includes two modules: modeller and fitting.
The blade modeller is an advanced geometry modeller for three-dimensional turbomachinary blades. 
The blade fitting is a unique and general purpose module which allows to import blade geometries and determine parameter values that best fit the provided geometry.
AutoBlade™ is integrated into the NUMECA CFD package FINE™/Turbo and benefits from the expertise accumulated with the design algorithms available in this complete design environment. AutoBlade™ is also available as an edition and monitoring tool inside the FINE™/Design3D module.
Features
AutoBlade™ can define various types of axial, radial or mixed flow turbomachinary blades that can be rotating or stationary. AutoBlade™ has been extensively tested on a wide range of applications:

compressors (axial or radial),
turbines (axial or radial),
fans,
pumps,
inducers,
blowers,
turbochargers,
return channels.

Project Management
To manage complete blade designs, AutoBlade™ integrates the concept of project. A new file management is used to handle and store the project and history of the changes (FIGURE 1).


FIGURE 1 Project management
In AutoBlade™, each interactive edition is stored in a memory stack for undo and redo operations. In addition, some operations can be marked as persistent and saved to disk. These persistent models are saved in a subdirectory and referenced in the project file. When reloading the project, these steps are retrieved and automatically fill the undo stack.
An AutoBlade™ project involves the parametric file, the target geometry file (for fitting) and some persistent state files:

.abp file: the project file,
.par file: the current parametric model,
.geomTurbo and .geomTurbo.xmt_txt files: the target geometry file. When the turbomachine is specified using CAD import (more details in AutoGrid™ User Manual), the file ".geomTurbo.xmt_txt" is used in addition of the ".geomTurbo" file and should not be removed.
a directory "project_name" with the persistent states and related files. 

model####.abm: the design step,
overlay####.abm: the inserted overlay,
model####.his: the fitting convergence history file for the design step model####.abm,
model####.fit: the fitting log file for the design step model####.abm.




FIGURE 2 Project structure on disk
Some special characters with accents, such as ü, ë and ê et al., are not allowed in the path and project names.

Preparing Target Geometry
The geometry to "import" must be defined in the ".geomTurbo" format before any fitting project can begin.
A ".geomTurbo" file contains the curves defining the hub, the shroud and the sections of the three-dimensional blades. This is an ASCII formatted file beginning with a specific header. Inside it, any line starting with character '#' is treated as a command and is therefore ignored.
Each section starts with a reserved keyword. Currently, AutoBlade™ supports usual keywords in both versions 3.7 and 5.3 of the format.
geomTurbo 5.3 (AutoGrid™ 5) is now the preferred format for AutoBlade™, but geomTurbo 3.7 is still supported for backward compatibility. Users of AutoGrid™ 4 will prefer the old format.

Import 
This menu allows:

to import a geometry file previously designed under AutoBlade™. Clicking the Import a parametric file button will launch a browser dialog to select an existing parametric file.
to create a new project from a template. Design is easier if a template similar to the desired geometry is first loaded. The template can be loaded by selecting the appropriate item under the Import a parametric template box.



FIGURE 7 Import menu
A general rule to ensure a quick design is to first load a template similar to the anticipated final configuration. Then topological choices can be fixed and eventually the values of the corresponding parameters are modified.
When a parametric file is selected in the menu, the template name is reset to "NONE" and when a template is chosen, the file name is reset to "none". This behavior prevents ambiguous choices, since those two options exclude each other.
It is possible to define an existing parametric model as a template. To do so, the existing parametric file must be copied in the directory:
<NUMECA_INSTALLATION_DIRECTORY>/fine#/COMMON/templates/ (on LINUX)
<NUMECA_INSTALLATION_DIRECTORY>\fine#\bin\templates\ (on Windows)
or
<NUMECA_INSTALLATION_DIRECTORY>/autoblade#/COMMON/templates/ (on LINUX)
<NUMECA_INSTALLATION_DIRECTORY>\autoblade#\bin\templates\ (on Windows)
Then the new template will appear under the Import a parametric template box.

Non-Axisymmetric Hub/Shroud
The following descriptions assume the definition of the hub surface, but all topics are directly applicable to shroud surface as well.

Selection Notebook
The first panel in Optional quantities menu is a selection notebook. Clicking on the tabs grants user access to three different categories of quantities. For each quantity, description and naming conventions are given in the three next paragraphs. If necessary, the computation method is also described shortly.

Export as '.geomTurbo'
The menu Geometry/Export as geomTurbo... opens a file chooser and prompts for a location where to save the geomTurbo export with default extension ".geomTurbo".

In stand-alone mode, the Save operation does not export the geomTurbo output automatically. On the contrary, each parametric model is saved with its geomTurbo export in a FINE™/Design3D project!

User Guide

Welcome to the AutoBlade™ User's Guide, a presentation of NUMECA's 3D parametric blade modeler.

Optional Splitters
Splitters are added to the main blade to guide the flow when the channel becomes wider, in radial turbomachinery. In AutoBlade™, splitters are compatible with both construction modes and all camber construction planes. Up to ten splitters can be added.
As a workaround, the splitter model can be used to model the tandem row configuration.
Splitters are built using the main blade camber curve with an optional refinement and their locations are relative to the main blade position and defined by means of few simple non dimensional parameters.
Suction and pressure sides are built according to the same method as the main blade: camber curve type, construction mode and edge types are all inherited form the main blade selections. Nevertheless, the number and values of the parameters are specific. In camber and thickness mode the thickness distribution is optionally asymmetric.
The Splitter blades menu consists in three pages:

the General properties page controls the number of additional blades (FIGURE 69),
the Camber curve page allows to alter the camber curve,
the Sides definition page defines the number of parameters controlling the suction and pressure side curves or thickness law



FIGURE 69 Splitter blades menu
Some topological choices may prevent the use of splitters, for example the stacking points in the centre of gravity.
Quick Method: Inherited Camber Curve
The simplest way to define splitters is to reuse the same blade camber line by selecting "None" in the Camber Curve section: the camber line of the main blade is simply rotated and truncated with respect to parameters MLE and MTE. Those two parameters are non dimensional factors used to limit the main camber extend in the meridional plane for splitter blades (FIGURE 70).
MLE parameter value represents a fraction of the main blade camber measured along the abscissa construction axis and starting from the main blade leading edge point. The value 0.0 corresponds to the main blade leading edge location, the value 1.0 to the main blade trailing edge location. The splitter leading edge location along the abscissa axis is obtained by formula below, where XLE(splitter) is the edge coordinate of the splitter blade along the abscissa construction axis and XLE and XTE are the edge locations of the main blade along the same axis.
One can establish a similar relation for the trailing edge location of the splitter thanks to parameter MTE. A zero value imposes that the m-coordinate of the splitter trailing edge point equals the one of the main blade trailing edge.






Once the splitter camber is defined, suction and pressure sides are constructed by means of the same method as for the main blade.


FIGURE 70 Splitter leading and trailing edges locations
AutoBlade™ accepts values in the range [-3,4] for MLE and MTE parameters. Outside regular bounds 0.0 and 1.0, the main camber curve is extrapolated linearly to allow the splitter blade to include upstream and downstream extensions.
If the criterion (MLE + MTE > 0.99) is reached, the value of MTE will be reset to 0.99-MLE automatically.
Camber Curve Refinement
It is also possible to perturb the initial camber curve portion defined above by a refinement curve. This perturbation is enabled by selecting the Camber Curve Refinement option.
FIGURE 71 shows the refinement process: first, the main camber curve is processed in its construction plane. A refinement Bezier curve is then generated with the help of by default equally spaced height parameters CAMBER_H(j) between the splitter limits defined by MLE and MTE parameters. The stretching factor allows the user to adapt this last space, it can evolve from 1 for uniform intervals to a factor bigger/lower than 1 that will result in increasing/decreasing intervals from leading MLE to trailing edge MTE. Finally, the ordinate values of both main camber and refinement curves are summed and the resulting camber is ready for side curves construction.
The refinement curve always uses dimensional heights.


FIGURE 71 Splitter camber curve refinement
Resizing & Moving Splitter Limits
Changing parameters MLE and MTE allows the splitter blade camber to be moved and resized in the meridional direction, as explained in the previous section Quick Method: Inherited Camber Curve.
An additional parameter DELTA_THETA controls the blade tangential location if the splitter blade needs to be moved away from its default central location, corresponding to the value of zero. The following expression is the formula computed by AutoBlade™ to rotate the splitter blades from initial the main blade camber line, where j stands for the splitter index, ABT for the number of blade types and NB for the amount of angular repetitions.



In single splitter case, when DELTA_THETA is given -1.0 value, the splitter blade camber is not rotated at all and when this value is changed to +1.0, splitter camber is rotated of a quantity , which is the spacing between the main blades. Therefore valid values are near zero, somewhere in the interval [-1.0,1.0].
Splitter location and extend are thus relative to the main camber curve and fully expressed through the use of three non dimensional parameters MLE, MTE and DELTA_THETA. It is important to notice that the stacking point defined for the main blade does not influence the splitters location.
The following figure shows a typical radial compressor with a single splitter blade (upper left). The next two pictures show the influence of parameter DELTA_THETA (upper right and lower left) while the latest shows how splitter blades extend can be modified with parameters MLE and MTE (lower right).


FIGURE 72 Example of compressor with splitter blade (upper left) and some effects in parameters changes
Summary table
TABLE 9 contains a list of all splitter parameters. Some of them are construction mode specific and may not be available in other construction modes.
TABLE 9 Parameters for splitter blades






Parameter


Description






S(i)_SPLIT(k)_MLE


leading edge fractional location parameter for splitter (k) on section (i). -0.5 < MLE < 1.5




S(i)_SPLIT(k)_MTE


trailing edge fractional location parameter for splitter (k) on section (i). -0.5 < MTE < 1.5




S(i)_SPLIT(k)_DELTA_THETA


rotation parameter for section (i) of splitter (k). Centred leading edge position is ensured by a zero value.




S(i)_SPLIT(k)_CAMBER_H(j)


optional refined camber height (j) for splitter (k) on section (i).




S(i)_SPLIT(k)_HALF_THICKNESS_P(j)


half thickness value (j) for splitter (k) on section (i) - camber & thickness mode only




S(i)_SPLIT(k)_TSS(j)
S(i)_SPLIT(k)_TPS(j)


suction and pressure side offsets (j) for splitter (k) on section (i) - suction & pressure sides mode only




S(i)_SPLIT(k)_RADIUS_LE


prescribed curvature radius at leading edge for section (i) of splitter (k) - rounded case




S(i)_SPLIT(k)_RADIUS_TE


prescribed curvature radius at trailing edge for section (i) of splitter (k) - rounded case




S(i)_SPLIT(k)_TE_WEDGE_ANGLE


prescribed wedge angle at trailing edge for section (i) of splitter (k) - suction & pressure sides mode only




Additional parameters for side curves with end line - applies for SS and PS




S(i)_SPLIT(k)_SS_LE_WEDGE_ANGLE


prescribed wedge angle δle for suction side curve, on section (i) of splitter (k) (in degrees)




S(i)_SPLIT(k)_SS_REAR_SHAPE


prescribed fractional offset  for suction side curve, on section (i) of splitter (k)




S(i)_SPLIT(k)_SS_END_LINE


prescribed fractional length  of the ending line for suction side curve, on section (i) of splitter (k)

Export as VDA-FS
The menu Geometry/Export as VDA-FS... opens a file chooser and prompts for a location where to save the blade curves in VDA-FS format.
When exporting the ruling directions to VDA-FS with late roundings and/or cutoff, the ruling directions defining the initial blade surface before applying late roundings and/or cutoff are exported. These directions do not match the final blade surfaces because the final blade is not  ruled after applying late roundings and/or cutoff.
When exporting to the VDA-FS format, all curves are exported and the data is written as sets of points. The name of the exported curves are following the name conventions below (where # is the index of the blade/splitters and ??? is the index of the directions):







Component


Description


Name






Hub


Hub curve


HUB




Shroud


Shroud curve


SHROUD




Hub gap


Hub gap curve (possibly multiple blades)

Mean line on gap surface (revolved gap surface)

Suction curve on gap surface

Pressure curve on gap surface


B#HGAP

B#HGAPML

B#HGAPSS

B#HGAPPS




Shroud gap



Tip gap curve (possibly multiple blades)

Mean line on gap surface (revolved gap surface)

Suction curve on gap surface

Pressure curve on gap surface



B#SGAP

B#SGAPML

B#SGAPSS

B#SGAPPS




Blade rulings


Ruling directions as a set of 4 aligned points if extended (reduced to 2 points otherwise)
:
Suction side directions (numbered from LE to TE)

Pressure side directions (numbered from LE to TE)


B#RSS???

B#RPS???




Blade sections


Suction and pressure side curves, for each blade:
Hub camber curve
Shroud camber curve
Hub suction curve
Shroud suction curve
Hub pressure curve
Shroud pressure curve


B#CB0001
B#CB0002
B#SS0001
B#SS0002
B#PS0001
B#PS0002

Tools Menu
Distance
Tools/Distance is useful to measure the distance between two points. When measuring the distance, the distance tool dialog box will appear, showing the distances computed along principal directions between the two points:


FIGURE 22 Distance tool dialog box
After selecting the menu Tools/Distance, the following prompt appears, asking to enter the first point:
Enter first point
Once the first point is entered, a second prompt appears, asking to enter the second point:
Enter second point
Attraction features are available, allowing automatic attraction to control points, end points, parametric cures and discrete curves. Once a distance is calculated, another distance can be measured by selecting other points.
To quit this tool, press <Esc> or the right mouse button.

AutoBlade™ Modeller

This chapter describes AutoBlade™ Modeller, the advanced and interactive NUMECA geometry modeller for three-dimensional turbomachinary blades. It can define various types of axial, radial or mixed flow turbomachinary blades that can be rotating or stationary. AutoBlade™  allows:

two design modes for generating the 2D section profiles: independent suction and pressure sides or camber and thickness addition,
multiple splitter blades (single for the fitting module),
various types of stream surfaces (planar, cylindrical, conical or arbitrary),
multiple choices for the blade stacking point, tangential lean and meridional sweep,
rounded and blunt edges,
special technological effects (edge filing and arbitrary blade cutoff),
non-axisymmetric hub/shroud surface,
solid geometry such as the axisymmetric wheel and shroud components in the RZ frame.

AutoBlade™ also provides a powerful geometry analysis tool able to monitor distributions from the model:

hub and shroud angle and curvature,
section thickness,
suction, pressure metallic angle and curvature,
various angles and curvature of camber and mean lines,
section channel width.

In addition, many useful quantities can be extracted from the model and the above graphs:

samples for angle and curvature of hub, shroud, suction, pressure and mean line curves,
samples and maximum value for thickness,
solidity, meridional chord, chord and stagger angle,
minimum channel width and throat area,
unguided turning angle,
moment of inertia and area of the 2D sections,
leading edge wedge angle,
leading and trailing edges coordinates.

Export Options
The Geometry/Export options... menu contains various settings controlling the exportation of the parametric blade sections in both ".geomTurbo" and CAD formats.
Common Settings


FIGURE 8 Common Settings
By default, primary and parametric blade sections are assumed for export. Primary blade sections are fully defined by parameters. Parametric sections are only defined to capture the imposed stacking laws. At all spanwise positions where a parametric section has been placed, the parameters are interpolated from the primary sections and used to create an additional blade section. See Stream Surfaces Spanwise Location for more detail on primary and parametric sections. 
In general, this default selection to export the primary and parametric sections is recommended. However, a drawback of the parametric sections is that the interpolation of the parameters can lead to non physical values such as a negative leading edge radius. Therefore, it is possible to use discretized sections to export an arbitrary amount of sections to the ".geomTurbo" file.
Discretized sections are quite similar to parametric sections apart from the fact that they are obtained through an interpolation of the blade geometry in point coordinates instead of the parameters. This has the advantage that the geometrical interpolation between realistic blade sections always leads to realistic full blade shapes. At least two different spanwise locations must be entered in the Spanwise locations field. Span values 0.0 and 1.0 make up the default minimal set.
Discretized sections are obtained by interpolation of point coordinates from both primary and parametric sections curves with respect to the span. Interpolation type controls the way discretized sections are computed from primary and parametric sections. Cubic spline is the default choice, but a linear law is always applied in case an extrapolation is required (see FIGURE 22). The Discretized sections are not allowed if the rounded tip topology is used.
TABLE 2 Exported sections






Output blade sections


Action






Primary & parametric sections


all primary and parametric sections are exported




User defined discretized sections


only discretized sections are exported




The output should at least contain two sections.
The amount of discretized sections should be greater than the amount of parametric and primary sections in order to tightly capture the design intent in the geometry file. For instance, if three primary sections are defined at span values 0.05, 0.5 and 0.95 but only two discretized sections are interpolated at span values 0.0 and 1.0, the exported geomTurbo file will not contain the non linear spanwise evolution of the blade shape. Choosing three or more discretized sections can solve this problem if span values are chosen with equal spacing along the spanwise direction.
Discretized sections are quite similar to parametric sections apart from the fact that they are obtained through a regular XYZ interpolation of the blade geometry in point coordinates instead of the parameters.
To improve interpolation for high staggered blade as centrifugal impeller, an option allows to export interpolated sections built from the reduced meridional coordinate of the camber curve and based on cylindrical coordinates R,θ,Z.
The approach is not directly accessible from templates or in models built from scratch in AutoBlade™ GUI. The keyword "ALLOW_ZRTHETA" must be added manually at the end of the section "SECONDARY_SECTIONS" of the parametric ".par" file to access the Z,R,θ interpolation approach in AutoBlade™ GUI as presented in the dialog box below.


FIGURE 9 Export Z,R,θ interpolated sections
        
When using the Z,R,θ interpolation approach, a distribution is prepared for the reduced meridional coordinate 'm', in [0,1] range, 0 corresponding to the leading edge, 1 to the trailing edge. This distribution allows clustering in both leading and trailing edge areas and shows a central region with constant intervals (Number of constant intervals). Three different distributions are available and their default settings are listed in the following table.
TABLE 3 Distribution settings when Z,R,θ interpolation approach








 


GUG
Geometric-Uniform-Geometric



GU
Geometric-Uniform



UG
Uniform-Geometric







Number of points for curves


201

201
201


Number of constant intervals
100
100
100


Total ratio

200
(10 if Blunt/Blunt)

200
200



Application


Rounded/Rounded
Blunt/Blunt

Rounded/Blunt
Blunt/Rounded



For each spanwise value i and each point j in [0,1] range, the camber coordinates and the local thickness are recomputed.
R(i,j) = Rhub(j) + span(i) x (Rshroud(j) - Rhub(j))
θ(i,j) = θhub(j) + span(i) x (θshroud(j) - θhub(j))
Z(i,j) = Zhub(j) + span(i) x (Zshroud(j) - Zhub(j))
X(i,j) = R(i,J) x cos(θ(i,j))
Y(i,j) = R(i,J) x sin(θ(i,j))
TSS(i,j) = TSShub(j) + span(i)^A x (TSSshroud(j) – TSShub(j))
TPS(i,j) = TPShub(j) + span(i)^A x (TPSshroud(j) – TPShub(j))
The exponent A is by default set to 1.0 but allows additional control over the thickness by changing the value in the range [1e-6,1e6].
The Z,R,θ interpolation approach is restricted to the following settings:

interpolated stream surfaces,
(m,β) and (m',θ) construction planes,
thickness addition mode, excluding flank-milled options (rulings and late rounding),
blades defined by exactly two primary sections and no parametric section.

geomTurbo Settings


FIGURE 10 geomTurbo Settings
This AutoBlade™ output format, carrying a "geomTurbo" extension, is used as input by the mesh generator AutoGrid5™.
The names of the blades can be altered and saved by means of the field Blade and Name. The option Stick edges is used to fit leading and trailing edges of pressure and suction sides along the spanwise direction when the leading and/or trailing edge are very curved (i.e. twisted blade).
The outputted geometry can be Full or Partial, which is controlled by the option Content. 
The option Enforce CAD output allows the user to output the CAD surfaces to the .geomTurbo file, instead of the surfaces defined by coordinates. Please note that some options specific to sections are not available when this CAD is active, such as the expansion factors.
The Curve format selector allows one among two systems of units for export: XYZ format that uses cartesian coordinates (X,Y,Z) or ZRTH format that uses cylindrical coordinates (Z,R,θ). The axis conventions are explained in the Axis Conventions section. 
A Scaling factor option allows a direct scaling of the geometry. This option is independent of the geomTurbo 'units' keyword and applies to any point or curve.
The option Enforce ruled surfaces allows, when two sections are exported, to force strict compliance of the side curves. This option adds the special keyword 'uniform_parametrization' at the end of the format field for suction and pressure side curves.
The option Exchange sides allows to exchange the pressure and suction sides of the blade to respectively suction and pressure sides.
The option Reverse theta orientation allows to reverse the theta orientation of the blade.
The option Apply a rotation allows to rotate the selected blade around a user-defined axis. The axis and anchor point fields expect three floating point coordinates while the angle value is given in degrees.


FIGURE 11 Apply blade rotation parameters
To use the exported geomTurbo file in AutoGrid5™, it is essential that the blade definition intersects the hub and the shroud. Therefore it may be necessary to export a sections at, for example, span values -0.05 and 1.05.
The scaling factor only applies to geomTurbo.
 CAD Settings


FIGURE 12 CAD Settings
CAD export can be customized independently of the 3D view settings. The main and splitters blades are exported by default.  
The units of the IGES file can be imposed by the user (Length unit). As for the "geomTurbo" export, you can apply a rotation for both Parasolid and IGES files.
VDA-FS Settings


FIGURE 13 VDA-FS Settings
When exporting to the VDA-FS format, the ruling directions are exported by default for ruled blades. Deselecting the button include ruling directions will cancel the ruling direction export.
The ruling directions are used as reference to generate the side surface by means of the Parasolid library. Usually a dozen of links are sufficient for that purpose. If needed, the user can also refine the ruling directions during the export. Clicking on the radio button refine ruling directions will activate the refinement during the export. The number of directions are used to define the number of sampled directions on each blade side. The ratio at rounded edge is the ratio between max spacing and min spacing in the U-direction. In addition, the directions can be extended outside the channel as a percentage [0,0.499] of the distance between the hub and the shroud.

Next Fitting Runs
After a first run, the fitted model is shown in the graphical view as the current model. The users should follow the procedure described below.

Open the list of parameters and check the bounds of the free parameters. The range should be modified when the corresponding parameter appears in yellow color, so that the next fitting run is able to further improve the value of the parameter. If no bounds are reached in free parameters, no changes are mandatory, but sometimes, it seems appropriate to reduce some very wide ranges.
If no bounds were enlarged or moved, a finer fitting can be launched: select a coarse or a medium fitting and click the Ok button. If some bounds were too tight and have been corrected accordingly, stick with a coarse fitting setting.

The above procedure can be followed several times, until the fitted solution is close enough to the target geometry. This model can then be used as initial model for database generation or optimization or simply used as company template in AutoBlade™.

Geometry Menu
Most of the options available in this menu are also available as accelerated buttons (top button bar) or as side buttons (left tool box). This menu consists in four groups of commands:

GeomTurbo 3.7 Example
The following file complies with geomTurbo 3.7 format and can be used within both AutoGrid™ 4 and 5.
GEOMETRY TURBO VERSION 3.7
geometric_tolerance		1E-06
blade_expansion_factor_hub		0.03
blade_expansion_factor_shroud		0.03
blade_merging		+0
number_of_blades		36
HUB
ZR
+28
-0.0425	0.17526	
-0.0307086	0.17526	
-0.0243586	0.175412	
-0.0180086	0.175717	
-0.0116586	0.176022	
-0.0026416	0.177394	
0.001016	0.178054	
0.007366	0.179578	
0.013716	0.181229	
0.020066	0.182982	
0.0264414	0.184404	
0.0327914	0.185674	
0.0391414	0.186741	
0.045212	0.187681	
0.0515366	0.188671	
0.0578866	0.189484	
0.0642366	0.190297	
0.0705866	0.19111	
0.0769366	0.19177	
0.0832866	0.192354	
0.0896366	0.192938	
0.0959866	0.193294	
0.102337	0.19365	
0.108687	0.193904	
0.115037	0.194056	
0.121387	0.194208	
0.126467	0.194335	
0.135	0.194335	
SHROUD
ZR
+28
-0.0425	0.256692	
-0.0312928	0.256565	
-0.0249428	0.256388	
-0.0185928	0.256083	
-0.0122428	0.255626	
-0.0058928	0.254864	
0.0004572	0.253746	
0.0068072	0.252222	
0.0131572	0.250495	
0.0195072	0.248717	
0.0258572	0.246888	
0.0322072	0.245161	
0.0385572	0.243738	
0.0449072	0.242672	
0.0512572	0.242062	
0.0576072	0.241732	
0.0639572	0.241452	
0.0703072	0.241097	
0.0766572	0.240665	
0.0830072	0.240182	
0.0893572	0.239827	
0.0957072	0.23942	
0.102057	0.23876	
0.108407	0.238354	
0.114757	0.237998	
0.121107	0.237642	
0.126187	0.23749	
0.135	0.237363	
SUCTION
SECTIONAL
3
# section 1
XYZ
+106
0.17669	-0.0208609	0.000351471	
0.176689	-0.0208418	0.000335267	
0.176689	-0.0208217	0.000321196	
0.176689	-0.0208002	0.000308953	
0.17669	-0.0207763	0.000298336	
0.176691	-0.0207475	0.000289117	
0.176697	-0.0206839	0.000281091	
0.176706	-0.0206206	0.000289117	
0.176711	-0.0205922	0.000298336	
0.176716	-0.0205687	0.000308953	
0.176721	-0.0205471	0.000321196	
0.176726	-0.0205228	0.000335267	
0.176733	-0.0204953	0.000351471	
0.17674	-0.0204633	0.000370063	
0.176748	-0.0204267	0.000391449	
0.176758	-0.0203848	0.000415985	
0.176769	-0.0203366	0.000444127	
0.176781	-0.0202815	0.000476459	
0.176796	-0.0202181	0.000513517	
0.176812	-0.0201457	0.000555958	
0.176831	-0.0200631	0.00060447	
0.176853	-0.019969	0.000659739	
0.176877	-0.0198621	0.000722525	
0.176905	-0.0197415	0.000793617	
0.176936	-0.0196056	0.000873903	
0.176971	-0.0194527	0.000964298	
0.17701	-0.0192817	0.00106579	
0.177054	-0.0190908	0.00117948	
0.177103	-0.0188783	0.00130655	
0.177155	-0.0186552	0.00144058	
0.177212	-0.0184092	0.00158921	
0.177275	-0.0181384	0.00175377	
0.177345	-0.0178413	0.00193573	
0.177422	-0.0175159	0.00213666	
0.177506	-0.0171605	0.00235832	
0.177598	-0.016773	0.00260258	
0.177705	-0.0163289	0.00288604	
0.177823	-0.0158442	0.00319969	
0.177952	-0.0153146	0.00354699	
0.178094	-0.0147345	0.00393199	
0.178251	-0.0140965	0.00435963	
0.178424	-0.0133911	0.00483594	
0.178615	-0.0126084	0.00536792	
0.178825	-0.0117457	0.00595929	
0.179062	-0.0107612	0.00664244	
0.179316	-0.00969826	0.00739387	
0.179585	-0.0085647	0.00822069	
0.179869	-0.00738629	0.00913027	
0.18017	-0.00617709	0.0101307	
0.180494	-0.00486988	0.0112305	
0.180846	-0.00336678	0.0124389	
0.181227	-0.00172503	0.0137656	
0.181642	-6.61359E-05	0.0152216	
0.182088	0.00153746	0.0168217	
0.182558	0.00312748	0.0185841	
0.183029	0.00477259	0.0205313	
0.183445	0.00627275	0.0224897	
0.183825	0.00759274	0.0244556	
0.184151	0.0087059	0.0262459	
0.184444	0.00960719	0.0278742	
0.184706	0.010364	0.0293552	
0.184939	0.011008	0.0307027	
0.185145	0.0115486	0.0319291	
0.185325	0.0120016	0.0330455	
0.185484	0.0123811	0.0340617	
0.185624	0.0126985	0.0349864	
0.185748	0.0129647	0.0358278	
0.185859	0.0131903	0.0365931	
0.185959	0.0133835	0.0372892	
0.186044	0.013542	0.0378917	
0.186121	0.0136777	0.0384335	
0.186189	0.0137936	0.0389184	
0.186249	0.0138931	0.0393534	
0.186304	0.0139787	0.0397448	
0.186353	0.0140526	0.0400976	
0.186397	0.0141164	0.0404159	
0.186437	0.0141716	0.0407034	
0.186472	0.0142172	0.0409509	
0.186504	0.0142572	0.0411753	
0.186532	0.0142921	0.0413786	
0.186558	0.0143228	0.0415626	
0.186582	0.0143498	0.0417289	
0.186603	0.0143736	0.0418791	
0.186622	0.0143946	0.0420144	
0.18664	0.0144131	0.0421361	
0.186656	0.0144304	0.0422513	
0.186671	0.0144455	0.0423542	
0.186684	0.0144588	0.0424458	
0.186695	0.0144705	0.0425271	
0.186706	0.0144808	0.0425992	
0.186715	0.0144898	0.0426628	
0.186723	0.0144977	0.0427188	
0.18673	0.0145044	0.042768	
0.186736	0.0145054	0.0428111	
0.186743	0.0145001	0.0428487	
0.186748	0.0144906	0.0428815	
0.186754	0.0144782	0.0429101	
0.186759	0.0144635	0.042935	
0.186763	0.0144472	0.0429567	
0.186768	0.0144296	0.0429756	
0.186772	0.0144109	0.0429921	
0.186776	0.014391	0.0430064	
0.186779	0.0143695	0.0430189	
0.186783	0.0143456	0.0430297	
0.186786	0.0143166	0.0430392	
0.186793	0.0142511	0.0430476	
# section 2
XYZ
+102
0.217127	-0.0231681	0.00303258	
0.217128	-0.0231547	0.00301933	
0.21713	-0.0231404	0.0030078	
0.217132	-0.0231247	0.00299778	
0.217134	-0.0231074	0.00298909	
0.217136	-0.0230861	0.00298156	
0.217141	-0.0230388	0.00297498	
0.217146	-0.0229917	0.00298156	
0.217148	-0.0229704	0.00298909	
0.21715	-0.0229528	0.00299778	
0.217152	-0.0229354	0.0030078	
0.217154	-0.0229154	0.00301933	
0.217156	-0.0228924	0.00303258	
0.217159	-0.0228659	0.00304783	
0.217162	-0.0228354	0.00306532	
0.217165	-0.0228007	0.0030854	
0.217169	-0.0227605	0.00310845	
0.217174	-0.0227146	0.00313489	
0.217179	-0.022662	0.00316527	
0.217185	-0.0226016	0.00320002	
0.217192	-0.0225327	0.00323976	
0.217199	-0.0224543	0.00328503	
0.217208	-0.0223652	0.00333647	
0.217218	-0.0222641	0.00339477	
0.217229	-0.0221502	0.00346057	
0.217241	-0.022022	0.00353471	
0.217255	-0.0218781	0.00361798	
0.217271	-0.0217172	0.00371129	
0.217289	-0.0215374	0.0038156	
0.217307	-0.021348	0.00392571	
0.217327	-0.0211382	0.00404787	
0.217349	-0.0209063	0.00418319	
0.217374	-0.0206503	0.0043329	
0.217401	-0.0203681	0.00449835	
0.217431	-0.0200576	0.00468094	
0.217463	-0.0197164	0.00488234	
0.2175	-0.0193216	0.00511623	
0.21754	-0.0188862	0.00537524	
0.217584	-0.0184058	0.00566229	
0.217632	-0.0178749	0.00598079	
0.217685	-0.0172871	0.00633486	
0.217741	-0.0166341	0.00672957	
0.217803	-0.0159073	0.00717072	
0.217869	-0.0151029	0.00766143	
0.217941	-0.0141796	0.0082285	
0.218016	-0.0131724	0.00885233	
0.218091	-0.0120731	0.00953855	
0.218167	-0.0108711	0.0102934	
0.218242	-0.00955873	0.0111238	
0.218317	-0.00813882	0.0120372	
0.21839	-0.00660734	0.0130419	
0.218461	-0.004933	0.0141469	
0.218531	-0.00310057	0.0153623	
0.218592	-0.00112156	0.0166992	
0.218634	0.00100507	0.01817	
0.218643	0.00323621	0.0197883	
0.218611	0.00530518	0.0214069	
0.21855	0.00721804	0.0230256	
0.218477	0.00884761	0.0244972	
0.218404	0.0102505	0.025835	
0.218331	0.0114683	0.0270512	
0.218261	0.0125242	0.0281569	
0.218193	0.01344	0.029162	
0.218127	0.0142372	0.0300757	
0.218065	0.0149369	0.0309063	
0.218006	0.0155568	0.0316614	
0.217951	0.0161082	0.0323478	
0.2179	0.0165992	0.0329718	
0.217853	0.0170364	0.0335391	
0.217813	0.0174069	0.03403	
0.217777	0.0177328	0.0344713	
0.217744	0.0180183	0.0348661	
0.217715	0.0182695	0.0352203	
0.21769	0.018492	0.0355389	
0.217667	0.0186901	0.0358261	
0.217646	0.0188671	0.0360852	
0.217628	0.0190257	0.0363191	
0.217612	0.0191614	0.0365206	
0.217598	0.0192839	0.0367032	
0.217585	0.0193943	0.0368687	
0.217573	0.019494	0.0370185	
0.217563	0.0195838	0.0371539	
0.217553	0.0196647	0.0372761	
0.217545	0.0197374	0.0373862	
0.217537	0.0198026	0.0374853	
0.21753	0.0198643	0.0375791	
0.217524	0.0199193	0.0376628	
0.217518	0.0199682	0.0377374	
0.217513	0.0200116	0.0378036	
0.217509	0.0200499	0.0378623	
0.217505	0.0200838	0.037914	
0.217501	0.0201136	0.0379596	
0.217499	0.0201321	0.0379997	
0.217498	0.0201394	0.0380347	
0.217497	0.0201398	0.0380654	
0.217497	0.0201358	0.0380921	
0.217498	0.0201287	0.0381153	
0.217498	0.0201194	0.0381356	
0.217499	0.0201085	0.0381533	
0.2175	0.0200963	0.0381687	
0.217501	0.0200831	0.0381821	
0.217502	0.0200688	0.0381938	
# section 3
XYZ
+101
0.251068	-0.0250123	0.00642899	
0.251071	-0.0250032	0.0064185	
0.251075	-0.0249931	0.00640938	
0.251078	-0.0249818	0.00640146	
0.251081	-0.0249691	0.00639458	
0.251084	-0.0249534	0.00638863	
0.251089	-0.024918	0.00638343	
0.251091	-0.0248824	0.00638863	
0.251091	-0.0248664	0.00639458	
0.251091	-0.0248518	0.00640146	
0.251091	-0.024835	0.00640938	
0.25109	-0.0248157	0.0064185	
0.25109	-0.0247935	0.00642899	
0.251089	-0.024768	0.00644106	
0.251088	-0.0247387	0.00645487	
0.251087	-0.0247051	0.00647077	
0.251086	-0.0246665	0.00648901	
0.251085	-0.0246222	0.00650991	
0.251084	-0.0245715	0.00653394	
0.251082	-0.0245134	0.00656142	
0.251081	-0.024447	0.00659284	
0.251078	-0.0243714	0.00662865	
0.251076	-0.0242856	0.00666932	
0.251073	-0.0241885	0.00671539	
0.25107	-0.0240789	0.00676743	
0.251067	-0.0239556	0.00682603	
0.251062	-0.0238174	0.00689184	
0.251058	-0.0236627	0.00696557	
0.251052	-0.0234903	0.00704804	
0.251046	-0.0233086	0.00713503	
0.251039	-0.0231077	0.00723155	
0.251031	-0.0228858	0.00733848	
0.251021	-0.0226413	0.00745676	
0.251011	-0.0223724	0.00758744	
0.250998	-0.0220769	0.00773168	
0.250984	-0.0217526	0.0078907	
0.250967	-0.0213778	0.00807538	
0.250947	-0.0209644	0.00827987	
0.250924	-0.0205076	0.00850645	
0.250897	-0.020001	0.0087578	
0.250865	-0.019437	0.00903716	
0.250829	-0.0188064	0.00934853	
0.250786	-0.0180988	0.00969644	
0.250736	-0.017309	0.0100834	
0.250674	-0.0163931	0.0105304	
0.250603	-0.0153838	0.011022	
0.250519	-0.0142764	0.0115627	
0.250421	-0.0130649	0.0121573	
0.250305	-0.0117371	0.0128113	
0.25017	-0.0102766	0.0135307	
0.250011	-0.00867329	0.0143219	
0.249824	-0.00692007	0.0151922	
0.249603	-0.00500169	0.0161493	
0.249342	-0.00287863	0.0172017	
0.249032	-0.000511463	0.0183589	
0.248663	0.00199586	0.019631	
0.248266	0.00448552	0.0209022	
0.247834	0.00725954	0.0221728	
0.24743	0.00934753	0.0233276	
0.247053	0.0111107	0.0243776	
0.246703	0.0126726	0.0253325	
0.246382	0.0140067	0.0262008	
0.246088	0.0151793	0.0269907	
0.245819	0.0162116	0.0277093	
0.245576	0.0170985	0.0283629	
0.245357	0.017861	0.0289576	
0.24516	0.018529	0.0294987	
0.244981	0.0191217	0.029991	
0.24482	0.0196488	0.0304389	
0.244681	0.0200948	0.0308267	
0.244557	0.0204871	0.0311756	
0.244447	0.0208312	0.0314879	
0.244349	0.0211346	0.0317683	
0.244262	0.0214037	0.0320206	
0.244183	0.0216433	0.0322481	
0.244112	0.0218572	0.0324535	
0.244049	0.0220488	0.032639	
0.243995	0.0222126	0.0327988	
0.243946	0.0223602	0.0329438	
0.243901	0.0224933	0.0330751	
0.243861	0.0226131	0.033194	
0.243825	0.0227211	0.0333015	
0.243792	0.0228182	0.0333986	
0.243763	0.0229055	0.033486	
0.243737	0.0229838	0.0335648	
0.243712	0.0230577	0.0336393	
0.24369	0.0231236	0.0337059	
0.24367	0.0231822	0.0337651	
0.243653	0.0232341	0.0338177	
0.243637	0.02328	0.0338644	
0.243624	0.0233206	0.0339055	
0.243612	0.0233555	0.0339418	
0.243602	0.0233746	0.0339736	
0.243595	0.0233824	0.0340015	
0.243589	0.0233839	0.0340258	
0.243584	0.0233814	0.0340471	
0.24358	0.0233762	0.0340656	
0.243577	0.0233691	0.0340817	
0.243575	0.0233606	0.0340958	
0.243573	0.0233511	0.034108	
0.243571	0.0233406	0.0341187	
PRESSURE
SECTIONAL
3
# section 1
XYZ
+94
0.17669	-0.0208609	0.000351471	
0.176691	-0.0208788	0.000370063	
0.176693	-0.0208955	0.000391449	
0.176696	-0.0209107	0.000415985	
0.1767	-0.0209239	0.000444127	
0.176705	-0.0209342	0.000476459	
0.176712	-0.0209405	0.000513517	
0.17672	-0.0209406	0.000555958	
0.17673	-0.0209316	0.00060447	
0.176744	-0.0209076	0.000659739	
0.176763	-0.0208557	0.000722525	
0.176785	-0.0207848	0.000793617	
0.17681	-0.0207048	0.000873903	
0.176839	-0.0206148	0.000964298	
0.176871	-0.0205139	0.00106579	
0.176908	-0.0204007	0.00117948	
0.176949	-0.0202743	0.00130655	
0.176992	-0.0201412	0.00144058	
0.17704	-0.0199936	0.00158921	
0.177094	-0.0198303	0.00175377	
0.177154	-0.01965	0.00193573	
0.17722	-0.019451	0.00213666	
0.177293	-0.019232	0.00235832	
0.177375	-0.0189909	0.00260258	
0.17747	-0.0187116	0.00288604	
0.177576	-0.018403	0.00319969	
0.177694	-0.0180618	0.00354699	
0.177825	-0.0176839	0.00393199	
0.177972	-0.0172643	0.00435963	
0.178136	-0.0167966	0.00483594	
0.178319	-0.0162734	0.00536792	
0.178522	-0.0156898	0.00595929	
0.178756	-0.0150119	0.00664244	
0.179011	-0.0142601	0.00739387	
0.179287	-0.0134251	0.00822069	
0.179586	-0.0124979	0.00913027	
0.179911	-0.0114742	0.0101307	
0.180262	-0.0103699	0.0112305	
0.180643	-0.00920084	0.0124389	
0.181063	-0.00789994	0.0137656	
0.181529	-0.00639667	0.0152216	
0.182033	-0.00472947	0.0168217	
0.18256	-0.00298793	0.0185841	
0.183087	-0.00118232	0.0205313	
0.183552	0.000569893	0.0224897	
0.183968	0.00223894	0.0244556	
0.184319	0.0036897	0.0262459	
0.184627	0.00494096	0.0278742	
0.184899	0.00601565	0.0293552	
0.185136	0.00695767	0.0307027	
0.185341	0.00779946	0.0319291	
0.185517	0.00854382	0.0330455	
0.185669	0.00919753	0.0340617	
0.185801	0.00977275	0.0349864	
0.185916	0.0102805	0.0358278	
0.186018	0.0107304	0.0365931	
0.186108	0.0111305	0.0372892	
0.186184	0.0114699	0.0378917	
0.186251	0.0117696	0.0384335	
0.186311	0.0120332	0.0389184	
0.186363	0.0122659	0.0393534	
0.186411	0.012472	0.0397448	
0.186453	0.0126551	0.0400976	
0.186491	0.012818	0.0404159	
0.186525	0.0129631	0.0407034	
0.186555	0.0130865	0.0409509	
0.186582	0.0131972	0.0411753	
0.186606	0.0132966	0.0413786	
0.186628	0.0133858	0.0415626	
0.186648	0.0134658	0.0417289	
0.186666	0.0135375	0.0418791	
0.186682	0.0136018	0.0420144	
0.186696	0.0136594	0.0421361	
0.18671	0.0137137	0.0422513	
0.186722	0.0137619	0.0423542	
0.186733	0.0138048	0.0424458	
0.186743	0.0138428	0.0425271	
0.186752	0.0138763	0.0425992	
0.186759	0.0139059	0.0426628	
0.186766	0.0139318	0.0427188	
0.186772	0.0139546	0.042768	
0.186777	0.0139745	0.0428111	
0.186781	0.013992	0.0428487	
0.186785	0.0140071	0.0428815	
0.186789	0.0140209	0.0429101	
0.186791	0.0140361	0.042935	
0.186794	0.0140529	0.0429567	
0.186795	0.0140709	0.0429756	
0.186796	0.0140901	0.0429921	
0.186797	0.0141103	0.0430064	
0.186797	0.0141321	0.0430189	
0.186797	0.0141562	0.0430297	
0.186796	0.0141855	0.0430392	
0.186793	0.0142511	0.0430476	
# section 2
XYZ
+98
0.217127	-0.0231681	0.00303258	
0.217125	-0.0231803	0.00304783	
0.217124	-0.0231913	0.00306532	
0.217123	-0.0232009	0.0030854	
0.217122	-0.0232082	0.00310845	
0.217121	-0.0232125	0.00313489	
0.217121	-0.0232125	0.00316527	
0.217121	-0.0232059	0.00320002	
0.217123	-0.0231888	0.00323976	
0.217126	-0.0231503	0.00328503	
0.217133	-0.0230862	0.00333647	
0.21714	-0.0230134	0.00339477	
0.217148	-0.022931	0.00346057	
0.217157	-0.022838	0.00353471	
0.217168	-0.0227337	0.00361798	
0.217179	-0.0226166	0.00371129	
0.217192	-0.0224854	0.0038156	
0.217206	-0.0223466	0.00392571	
0.217222	-0.0221925	0.00404787	
0.217239	-0.0220214	0.00418319	
0.217259	-0.0218315	0.0043329	
0.21728	-0.0216212	0.00449835	
0.217304	-0.0213882	0.00468094	
0.21733	-0.0211304	0.00488234	
0.21736	-0.02083	0.00511623	
0.217394	-0.0204962	0.00537524	
0.217432	-0.0201254	0.00566229	
0.217473	-0.0197138	0.00598079	
0.217519	-0.019257	0.00633486	
0.217569	-0.0187499	0.00672957	
0.217625	-0.0181856	0.00717072	
0.217685	-0.017559	0.00766143	
0.217752	-0.0168328	0.0082285	
0.217824	-0.0160287	0.00885233	
0.2179	-0.0151392	0.00953855	
0.217978	-0.0141596	0.0102934	
0.21806	-0.0130814	0.0111238	
0.218145	-0.0118857	0.0120372	
0.218234	-0.0105593	0.0130419	
0.218327	-0.0091119	0.0141469	
0.218423	-0.00752169	0.0153623	
0.218519	-0.00574169	0.0166992	
0.218603	-0.00379413	0.01817	
0.21866	-0.00166115	0.0197883	
0.218675	0.00048992	0.0214069	
0.218653	0.00260323	0.0230256	
0.218611	0.00445339	0.0244972	
0.218559	0.00610324	0.025835	
0.2185	0.00758562	0.0270512	
0.218438	0.00889941	0.0281569	
0.218374	0.0100659	0.029162	
0.218309	0.0111166	0.0300757	
0.218243	0.0120647	0.0309063	
0.218178	0.0129181	0.0316614	
0.218117	0.0136848	0.0323478	
0.218058	0.0143722	0.0329718	
0.218004	0.0149886	0.0335391	
0.217956	0.0155155	0.03403	
0.217912	0.0159844	0.0344713	
0.217872	0.0164004	0.0348661	
0.217836	0.0167711	0.0352203	
0.217803	0.0171032	0.0355389	
0.217774	0.0174016	0.0358261	
0.217747	0.0176705	0.0360852	
0.217722	0.0179132	0.0363191	
0.217701	0.0181223	0.0365206	
0.217682	0.0183118	0.0367032	
0.217664	0.0184836	0.0368687	
0.217648	0.0186392	0.0370185	
0.217634	0.0187799	0.0371539	
0.217621	0.0189069	0.0372761	
0.217609	0.0190214	0.0373862	
0.217598	0.0191244	0.0374853	
0.217588	0.019222	0.0375791	
0.217579	0.0193091	0.0376628	
0.217571	0.0193867	0.0377374	
0.217564	0.0194556	0.0378036	
0.217557	0.0195167	0.0378623	
0.217552	0.0195705	0.037914	
0.217547	0.019618	0.0379596	
0.217542	0.0196597	0.0379997	
0.217538	0.0196962	0.0380347	
0.217535	0.0197281	0.0380654	
0.217532	0.0197559	0.0380921	
0.21753	0.0197801	0.0381153	
0.217527	0.0198012	0.0381356	
0.217525	0.0198196	0.0381533	
0.217524	0.0198357	0.0381687	
0.217522	0.0198498	0.0381821	
0.217521	0.019864	0.0381938	
0.217519	0.0198796	0.0382039	
0.217518	0.019897	0.0382127	
0.217516	0.0199183	0.0382205	
0.217511	0.0199664	0.0382273	
0.217507	0.0200146	0.0382205	
0.217505	0.0200358	0.0382127	
0.217503	0.0200533	0.0382039	
0.217502	0.0200688	0.0381938	
# section 3
XYZ
+99
0.251068	-0.0250123	0.00642899	
0.251064	-0.0250204	0.00644106	
0.25106	-0.0250273	0.00645487	
0.251055	-0.0250325	0.00647077	
0.25105	-0.0250354	0.00648901	
0.251044	-0.0250351	0.00650991	
0.251039	-0.02503	0.00653394	
0.251033	-0.0250168	0.00656142	
0.251027	-0.0249876	0.00659284	
0.251024	-0.0249273	0.00662865	
0.25102	-0.0248566	0.00666932	
0.251016	-0.0247766	0.00671539	
0.251011	-0.0246862	0.00676743	
0.251006	-0.0245844	0.00682603	
0.251	-0.02447	0.00689184	
0.250993	-0.0243419	0.00696557	
0.250985	-0.0241987	0.00704804	
0.250976	-0.0240475	0.00713503	
0.250967	-0.0238797	0.00723155	
0.250956	-0.0236939	0.00733848	
0.250944	-0.0234884	0.00745676	
0.25093	-0.0232613	0.00758744	
0.250915	-0.0230106	0.00773168	
0.250897	-0.0227341	0.0078907	
0.250877	-0.0224127	0.00807538	
0.250853	-0.0220564	0.00827987	
0.250827	-0.0216606	0.00850645	
0.250796	-0.0212198	0.0087578	
0.250762	-0.0207276	0.00903716	
0.250722	-0.0201762	0.00934853	
0.250676	-0.0195583	0.00969644	
0.250623	-0.018872	0.0100834	
0.250558	-0.0180832	0.0105304	
0.250484	-0.0172167	0.011022	
0.250399	-0.0162526	0.0115627	
0.250302	-0.0151755	0.0121573	
0.250189	-0.0139956	0.0128113	
0.250058	-0.0127184	0.0135307	
0.249907	-0.0112921	0.0143219	
0.249732	-0.00968576	0.0151922	
0.249527	-0.0079398	0.0161493	
0.249286	-0.00599318	0.0172017	
0.249003	-0.00381508	0.0183589	
0.248667	-0.00141637	0.019631	
0.248305	0.000973856	0.0209022	
0.247918	0.0033137	0.0221728	
0.247544	0.00554123	0.0233276	
0.247186	0.00761649	0.0243776	
0.24685	0.00937261	0.0253325	
0.246542	0.0108178	0.0262008	
0.246255	0.0121657	0.0269907	
0.245987	0.0134319	0.0277093	
0.24574	0.0145632	0.0283629	
0.245514	0.0155557	0.0289576	
0.24531	0.0164269	0.0294987	
0.245124	0.0171942	0.029991	
0.244956	0.0178748	0.0304389	
0.24481	0.0184539	0.0308267	
0.24468	0.0189687	0.0311756	
0.244563	0.0194255	0.0314879	
0.244458	0.0198325	0.0317683	
0.244364	0.0201964	0.0320206	
0.24428	0.0205228	0.0322481	
0.244203	0.020816	0.0324535	
0.244135	0.0210798	0.032639	
0.244076	0.0213062	0.0327988	
0.244022	0.0215111	0.0329438	
0.243973	0.0216963	0.0330751	
0.243929	0.0218636	0.033194	
0.24389	0.0220145	0.0333015	
0.243854	0.0221506	0.0333986	
0.243822	0.0222731	0.033486	
0.243793	0.0223832	0.0335648	
0.243765	0.0224874	0.0336393	
0.243741	0.0225803	0.0337059	
0.243719	0.0226629	0.0337651	
0.2437	0.0227363	0.0338177	
0.243682	0.0228012	0.0338644	
0.243667	0.0228585	0.0339055	
0.243654	0.022909	0.0339418	
0.243642	0.0229533	0.0339736	
0.243632	0.0229921	0.0340015	
0.243623	0.0230259	0.0340258	
0.243615	0.0230555	0.0340471	
0.243609	0.0230812	0.0340656	
0.243603	0.0231036	0.0340817	
0.243597	0.0231231	0.0340958	
0.243593	0.0231402	0.034108	
0.243589	0.023155	0.0341187	
0.243586	0.0231679	0.034128	
0.243583	0.0231799	0.034136	
0.24358	0.0231934	0.0341431	
0.243577	0.02321	0.0341492	
0.243572	0.023248	0.0341546	
0.243569	0.0232861	0.0341492	
0.243569	0.0233031	0.0341431	
0.243569	0.0233169	0.034136	
0.24357	0.0233293	0.034128	
0.243571	0.0233406	0.0341187

Suction & Pressure Sides Construction Mode - throat-based
The throat based model is inspired from the Pritchard's eleven parameter model (Prichard LJ, 1985, "An eleven parameter axial turbine airfoil geometry model", ASME Paper 85-GT-219), but will reuse some angles and curves from the existing topologies for construction curves. This method is dedicated to axial turbines and is enabled through the Construction curves option.
The throat based model is defined as follows:

The camber curve is defined as a simple Bezier curve. It can be defined with absolute inlet and outlet angles β1 and β2, or defined by the relative definition (δ1 and δ2). Please note however that the stagger angle γ is not allowed to reach +/- 90 degrees for proper behavior.
The leading edge radius definition is included in the suction and pressure side curves with control of the start radius.
The pressure side curve is defined as in construction curve with end line (regular), with a linear part of zero length. This definition has the advantage to allow an angular control near leading edge. Order of pressure side Bezier curve is at least four (5 control points) without TPS parameters.
The suction side is defined from two Bezier curves. The leading edge part is at least of order four (when no TSS parameters are available) and the trailing edge part is defined from a third order Bezier curve (four control points) and is fully automatic once angles are defined. The throat location in the blade-to-blade view passes through the center of the trailing edge circle.



FIGURE 54 Definition of the side curves for throat based model
TABLE 7 Parameter definition of the throat based model






Parameters


Description




span


Spanwise location of the section




NB


Number of blades









Axial chord




γ


Stagger angle. , where Ct is the tangential chord




ζ


Deviation angle




β1


Inlet blade angle




εin


Inlet half wedge angle




RLE


Leading edge radius




RTE


Trailing edge radius




β2


Exit blade angle




o


Throat width




The model does not ensure that the effective throat is located at the prescribed location if users try to design a supersonic blade.
TABLE 8 2D blade profile definition (throat based model)






Setting


Description






number of intermediate control points


number of intermediate offsets to add between leading and trailing edges in the pressure side and between leading edge and throat location in the suction side - amounts may differ for suction and pressure sides.




stretching factor


ratio of two successive offset gaps on the camber curve - values may differ for suction and pressure sides




Parameter


Description




S(i)_LE_RADIUS


prescribed leading edge curvature radius RLE for section(i)




S(i)_TE_RADIUS


prescribed trailing edge radius RTE for section(i)




S(i)_TE_WEDGE_ANGLE


prescribed wedge angle δte for section(i) (in degrees)




S(i)_THROAT_WIDTH


prescribed throat width




S(i)_DEV_ANGLE


prescribed deviation angle




S(i)_SS_LE_WEDGE_ANGLE
S(i)_PS_LE_WEDGE_ANGLE


prescribed wedge angle εin for the side curve of section(i) (in degrees)




S(i)_PS_REAR_SHAPE


prescribed fractional offset  for the side curve of section(i)




S(i)_PS_END_LINE


prescribed fractional length  of the ending line for the side curve of section(i)




S(i)_TSS_(j)


intermediate offset TSS(j) for suction side curve of section (i)




S(i)_TPS_(k)


intermediate offset TPS(k) for pressure side curve of section (i)

Initialization Process
Once a valid target file has been imported in the Target settings subpad, an initialization of the model is possible through the button Adapt model (Adapt model). This operation will guess suitable values for all or some of the following features:

hub curve,
shroud curve,
the meridional stacking law,
the tangential stacking law,
main camber curves,
main side curves,
splitter camber curves,
splitter side curves,
non axisymmetrical hub,
non axisymmetrical shroud.

This quick operation will also prepare the minimum and maximum bounds of the parameters, so that a fitting process can be launched with minimum user input.


FIGURE 2 Initialization options
Two initialization methods are available: RESET and IMPROVE. These methods allow to either reset the selected features or improve them. In the IMPROVE case, the initialization only alters the feature if the new guess improves the comparison.
Clicking the Ok button will start the initialization process. When launching the initialization process, the model is stored as a persistent step in the undo stack.
It is important to choose the most suitable topological settings before the initialization: improper settings will result in poor initial and fitted models. If the initialization process provides a very rough result, it is probable that some topological choices need to be changed or the amount of parameters is insufficient.
Some parameters are always reset by the initialization process, even when all features are unselected and the chosen method is improve. This is the case for the parameters controlling the stream surfaces, the location of the splitters and the meridional reference position.
What it does?
The initialization process is responsible for the following tasks:

generate suitable parameters for all curves and laws (hub, shroud, sweep and lean laws, camber curves, side curves or thickness distributions, several lengths and locations). Values and bounds are guessed.
find the best traces for planar, cylindrical and conical stream surfaces.
change the amount of primary sections and their spanwise locations. Each target section is considered as a primary section in the initialized and fitted models.
freeze some parameters that are unlikely to improve the model in the fitting process.

What it does not do?
The initialization process is unable

to correct poor topology choices or suggest more suitable solutions,
to adapt the reference values of the parameters,
to guess some parameters like filing lengths and thicknesses
to capture some edge shapes like a sharp end,
to provide a precise model, very close to the target geometry.

When a setting is changed, for instance a curve type or its amount of defining parameters, a new initialization is required for best results. This is however unnecessary when a blunt type or filing option is changed.

Tangential Position
The lean curve types are very close to those (five types) introduced in the Meridional Location section for the sweep law. The tangential law defines θ as a function of the span parameter value. This coordinate system has been chosen because a purely radial law is easily defined by setting the angular parameters to 0.
The lean law is defined between 0.0 and 1.0 but linear extrapolation is allowed for other span values.
Usually, sections can be rotated by means of the parameter BLADE_ROTATION and the lean law has its origin at θ=0 (left picture in FIGURE 32). There is an exception however: when planar axial stream surfaces are used, the lean law requires an additional degree of freedom because the sections do not rely on axi-symmetric surfaces (right picture in FIGURE 32).
Therefore, an additional angular parameter LEAN_OFFSET is added to the lean law parameters when planar axial stream surfaces are defined (FIGURE 33).
The computed angle θ is plotted in radians, not in degrees. This is an exception.


FIGURE 32 BLADE_ROTATION parameter allows the rotation of the model


FIGURE 33 Three of available lean laws, defined in (span,θ) plane with special offset






Parameter


Description






LEAN_OFFSET


special offset angle for the lean law applied to planar axial stream surfaces (in radians)




Line:

 



LEAN_BETA


angle β of the line (in degrees)




Second order Bezier curve (3 control points):




LEAN_BETA1


angle β1 of the Bezier curve at span = 0 (in degrees)




LEAN_BETA2


angle β2 of the Bezier curve at span = 1 (in degrees)




Bezier-line-Bezier composite curve:




LEAN_ALPHA1


angle α1 of the first Bezier curve at span = 0 (in degrees)




LEAN_C1


spanwise extent of the first Bezier curve




LEAN_P1


fractional factor defining the second control point location of the first Bezier curve




LEAN_ALPHA2


angle α2 of the linear segment (in degrees)




LEAN_ALPHA3


angle α3 of the second Bezier curve at span = 1 (in degrees)




LEAN_C2


spanwise extent of the second Bezier curve




LEAN_P2


fractional factor defining the second control point location of the second Bezier curve

Space of Definition
The domain of definition is an area built in (m',θ) plane. First, the mean line of the main blade at hub section is computed (upper dotted black curve on FIGURE 79). This line is the first side limit of the domain inside the blade channel, the second side limit being defined by its vertical translation of value Δθ = -2*PI / NB.


FIGURE 79 Space of definition
The extent of the domain is always limited at inlet and outlet and by the mean line of the main blade and its translated repetition. The inlet and outlet parts (Inlet/Outlet extension in FIGURE 87) are built from either a line segment tangent to the mean line of the blade at the edge point or a smooth Bezier curve ending horizontally at the other end (red curves). Aside this construction choice, the extensions are fully automatic. This definition has a clear advantage: the perturbation may occur over a space covering the whole hub surface once repeated, since a 2*PI extent is travelled in θ direction.
For the definition of the non axisymmetric hub, the preferred configuration is interpolated stream surfaces with the first primary section at span location 0. Other stream surfaces are allowed, but may cause discontinuities if the perturbed surface ends outside the blade section. The reference hub mean line is always built for span 0, by interpolation if it is not defined in the list of primary sections.

Blade Meridional & Tangential Locations
It is common, in the turbomachinery community, to define the position of the 2D blade section on a stream surface with respect to a reference point - the stacking point. This point is first defined on the 2D blade section, then positioned on the corresponding stream surface in the meridional and tangential directions based on two independent stacking law definitions.


FIGURE 23 Stacking point choice in the Locations menu
The menu consists in three pages that define:

the stacking point, defined on the 2D blade sections.
the meridional location law, defined in the (Z,R) plane, which can be either a sweep law curve that defines the meridional trace of the stacking point or leading and trailing edges traces that define the meridional limits of the leading and trailing edges of the blade section.
the tangential location law for the stacking point, defined using a lean law curve. This curve is built in the (span,θ) plane.

Optional splitters are positioned relative to the main blade. Therefore, the meridional and tangential location menu affects the main blade sections only.

Scalar Values
This page contains switches to select geometrical data computed for each blade section, except throat section area which is a global property. Some scalar quantities - namely minimum channel width, unguided turning angle and throat section area - are not available when one or more splitter blades are defined.


FIGURE 96 Scalar values option tab
Draft angle extrema
Defines the extrema of the draft angle for casting process.






Quantity


Examples






DRAFT_ANGLE_MIN


the minimum draft angle




DRAFT_ANGLE_MEAN


the averaged draft angle




DRAFT_ANGLE_MAX


the maximum draft angle




Camber & Mean Line Length
The lengths of the camber curve and mean line are built in spatial coordinates, not in a peculiar construction plane.






Quantity


Examples






S?_(SPLIT?_)CAMBER_LEN


S1_CAMBER_LEN stands for the length of the main camber curve on section 1




S?_(SPLIT?_)ML_LEN


S1_CAMBER_LEN stands for the length of the mean line in section 1 of the main blade




Special Camber Properties
Several camber quantities are available for all sections and illustrated in the few next figures (figures  3.3.2-96 to  3.3.2-98).
Meridional chord, chord and stagger angle
The meridional chord is defined as the difference in m coordinate between leading and trailing edge. In pure axial cases, this length is then the real axial chord.
The stagger angle is the angle measured in (,θ) conformal plane between the edge points. This angle is equivalent to the one measured in (m,Rθ) plane for pure axial cases.
To ensure proper values, the chord is defined as the ratio of the meridional length to the cosine of the stagger angle. In pure axial cases, this definition of the chord produces the same value as the distance between edge points in the dimensional (m,Rθ) plane.





FIGURE 97 Chord, meridional chord and stagger angle
Maximum NACA height
This quantity simply extracts the maximum height measured relatively to the chord in (m,Rθ) plane and only has meaning in pure axial or nearly axial cases. Its location as a fraction of the chord is also provided, as the next figure clearly explains.


FIGURE 98 Maximum camber height (NACA style definition)
Solidity
The last camber related quantity is the solidity and its alternative meridional definition. As for the maximum NACA height, this special value is built from (m,Rθ) plane and loses all interest in radial configurations! It is defined as the ratio of the chord to the average distance between the camber lines of the main blade and the next occurrence of the blade.
The meridional solidity is defined relative to the meridional chord instead of the chord.
        


FIGURE 99 Section solidity
Solidity is defined for the main blade only!






Quantity


Examples






S?_(SPLIT?_)CHORD


S1_CHORD stands for the chord of the main camber curve of section 1




S?_(SPLIT?_)AXIALCHORD


S1_AXIALCHORD stands for meridional chord of the main camber curve of section 1




S?_(SPLIT?_)STAGGERANG


S1_STAGGERANG stands for stagger angle of the main camber curve of section 1




S?_(SPLIT?_)NACAH_MAX


S1_NACAH_MAX stands for the maximum height of the camber in section 1 of the main blade, relative to the chord
S1_NACAH_MAX_U is the fractional location of this maximum along the chord for the same section




S?_SOLIDITY


S1_SOLIDITY stands for the solidity of the main camber curve on section 1




S?_AXIALSOLIDITY


S1_AXIALSOLIDITY stands for the meridional solidity of the main camber curve on section 1




Thickness Extrema
Maximum value: thickness distribution is examined and the highest value found is reported as maximum. Maximum thickness value always exists and is reported with its corresponding location along the blade section mean line as a fraction of the length in the range [0,1].
Minimum value: thickness distribution is examined. Each time a local thickness minimum is found, it is retained if lower than the previous one. This minimum value is thus a global optimum in the mathematical sense, not simply the smallest value in the distribution. For instance, starting and ending zero thicknesses are not taken into account as minima in rounded cases. Location along the blade section mean line is also available.
The minimum value does not always exist since it is a mathematical optimum. When not found, a "none" string is reported in the list for both value and location. This does not apply for the maximum thickness value.






Quantity


Examples






S?_(SPLIT?_)THICK_MIN_U
S?_(SPLIT?_)THICK_MIN


S1_THICK_MIN_U stands for thickness minimum location along the mean line of main blade section 1. It is expressed as a fraction length in the range [0,1] except when no minimum value is found.
S2_SPLIT1_THICK_MIN is the name given to the minimum thickness value for the second section of the first splitter blade.




S?_(SPLIT?_)THICK_MAX_U
S?_(SPLIT?_)THICK_MAX


S1_THICK_MAX_U stands for thickness maximum location along the mean line of main blade section 1. It is expressed as a fraction length in the range [0,1].
S2_SPLIT1_THICK_MAX is the name given to the maximum thickness value for the second section of the first splitter blade.




Minimum Channel Width
The Channel width distribution is examined and the smallest value found is reported as minimum. This value is not available in splitter cases. Please note the corresponding location along the fluid path is not available. Unit is of dimension [L].






Quantity


Examples






S?_CHANNEL_MIN


S1_CHANNEL_MIN stands for the minimum channel width value along the fluid path for main blade section 1.






FIGURE 100 Channel width and minimum value (axial turbine)
Unguided Turning Angle
Unguided turning angle is defined as the angle between two lines starting from the suction side point where the minimum channel width is located:

the first line is perpendicular to the channel width
the second line passes through the junction point between suction side and trailing edge circle in rounded edge case or the end of the suction side curve in blunt case.

This value is computed in (,θ) plane as shown in FIGURE 101 for an axial turbine with a rounded trailing edge


FIGURE 101 Unguided turning angle (axial turbine)
Since it is based on channel width computation, this quantity is available in single blade type only. Angles are given in degrees.






Quantity


Examples






S?_UNGUIDEDTURNANG_U
S?_UNGUIDEDTURNANG


S1_UNGUIDEDTURNANG_U stands for the unguided turning angle location on suction side for main blade section 1. It is expressed as a fraction length in the range [0,1].
S1_UNGUIDEDTURNANG stands for the unguided turning angle value for main blade section 1.




Throat Area
Two types of throat area estimates are available:

estimate of spatial throat surface area or "3D throat"
estimate of projected throat surface area in the (X,Y) plane

This quantity is not available in splitter cases. Unit is of dimension [L²].






Quantity


Examples






THROAT
THROAT2D


Throat section area estimate computed in spatial coordinates
Throat section area estimate projected on (X,Y) plane




Wedge Angle
Wedge angle is defined at leading edge as the angle slope difference, in the (,θ) plane, between a position on suction side and a position on pressure side. Those positions are length fractions of suction and pressure sides in the range [0.01,0.15]. 5 percent is the default value.






Quantity


Examples






S?_(SPLIT?_)WEDGEANG


S1_WEDGEANG stands for the wedge angle value at leading edge of main blade section 1.
S2_SPLIT1_WEDGEANG stands for the wedge angle value at leading edge of first splitter blade section 2.




Section Area
Section area estimate is computed in (Z,R*θ) plane as the polygonal area limited by the discretized suction and pressure side curves. If θ is small, this corresponds to a projected area in (Z,Y) plane.
A very good accuracy is reached by AutoBlade™ using this simple scheme.
This quantity is available for every section and blade type. Unit is of dimension [L²].






Quantity


Examples






S?_(SPLIT?_)AREA


S1_AREA stands for the section area estimate of main blade section 1.
S2_SPLIT1_AREA stands for the section area estimate of the first splitter blade section 2.




Flexional Inertia
An estimation of the flexional inertia is computed in (Z,R*θ) plane as 2D section inertia for every primary section and three values are generated:

minimum moment of flexional inertia,
maximum moment of flexional inertia,
angle in degree between the minimum moment direction and Z axis direction.

Moments unit is of dimension [L4] and values are always related to the center of gravity of the section in (Z,R*θ) plane.
The flexional inertia is computed with respect to all possible rotation axes in this plane through the center of gravity of the section. For one specific rotation axis the flexional inertia or moment of inertia is defined by I = ∫ m r² where "m" is the mass or area of the section and "r" is the perpendicular distance to the rotation axis.
The flexional inertia of the section with respect to all possible axes can be described as a tensor. The eigenvalues of this tensor provide the minimum and maximum value of flexional inertia and the eigenvectors provide the corresponding rotation axes. The angle as indicated in  Flexional inertia - angle defines the angle between the z-direction and the rotation axis of the minimum flexional inertia.


FIGURE 102 Flexional inertia - angle
It is important to note that the flexional inertia in (Z,R*θ) plane is only correct for planar construction surfaces of the sections. For e.g. conical surfaces it is not correct because the value of the radius is not constant for the section. As a solution the (Z,R*θ) plane is kept for processing of the area, flexional inertia and torsional inertia, but the section is reprojected on the ‘closest’ cylinder for each section. This closest cylinder is the one that passes through the mid-point of the 3D line segment joining the leading to trailing edge.






Quantity


Examples






S?_(SPLIT?_)IMIN
S?_(SPLIT?_)IMAX
S?_(SPLIT?_)IMINANG


S1_IMIN stands for the section minimum moment of flexional inertia for main blade section 1.
S1_IMAX stands for the section maximum moment of flexional inertia for main blade section 1.
S1_IMINANG stands for the angle between minimum moment of flexional inertia direction and Z axis direction for main blade section 1.




Torsional Inertia
An estimation is computed, either in (Z,R*θ) plane or in X,Y,Z coordinates, for every section. The torsional moment of inertia is evaluated thanks to the approximate formula for thin profiles.
Moments unit is of dimension [L4].

 where 
with t being the local thickness measured perpendicularly to the mean line, U the length of the mean line and A the section area (see FIGURE 103).


FIGURE 103 Torsional inertia - mean line integration
The (Z,R*θ) case is similar to a computation in (Z,Y) plane as soon as θ is near zero for the whole section and planar or cylindrical stream surfaces are chosen. Suction and pressure side curves are considered in spatial cartesian coordinates.
The above formula is an approximation that loses its accuracy for thick blade sections.






Quantity


Examples






S?_(SPLIT?_)JT
S?_(SPLIT?_)JT2D


S1_JT stands for the moment of torsional inertia value for main blade section 1, computed in spatial coordinates
S2_SPLIT1_JT2D stands for the moment of torsional inertia value for section 2 of the first splitter blade, computed in (Z,R*θ) plane

Export parameters
The menu Geometry/Export parameters... opens a file chooser and prompts for a location where to save the whole list of the parameters with default extension ".param". All the parameters defining the current model are exported. Each line in the .param file defines one parameter with the name, the expression (if defined) and the value of the parameter.

Surface Setup
The designer can choose between planar, cylindrical, conical and hub to shroud interpolation surfaces. All surfaces except planar type are obtained by revolution of a trace around the Z axis.
According to the chosen type, one or more settings among X, Z, R and α are prompted for the reference traces near hub and shroud. Those reference curves are defined respectively as the spanwise locations "0" and "1".
According to the chosen stream surface type, several construction planes for the blade sections will be available. (Z,Y), (m,R*θ), (m,β) and (,θ) planes properties are described in Camber Curve Definition.
Cascade topology and rounded tip configuration can be managed in the section Special options.
X, Z, R and α values are not parameters but static data. Their value is not accessible in the Parameters menu and are not allowed to vary within an optimization.
Planar Axial Surfaces
Planar stream surfaces allow the 2D blade sections to be defined in the (Z,Y) plane. This plane is located at a constant height X above the axis of rotation. Therefore, a value of X is required to define the height for both hub and shroud. This is useful for axial turbomachinery.






Parameter


Description






REF_TRACE_HUB_R


height of the reference stream plane trace at hub




REF_TRACE_TIP_R


height of the reference stream plane trace at shroud






FIGURE 10 Planar stream surfaces traces definition
Planar Radial Surfaces
Pure radial surfaces can be defined as planes parallel to (X,Y). The usual construction planes are then (,θ) and (m,β).
A Z value is required to define the reference traces at hub and shroud.
The streamwise orientation can be changed by means of the switch Orientation from the menu. However, the default value is usually correct when the endwalls have been defined from inlet to outlet.






Parameter


Description






REF_TRACE_HUB_Z


coordinate of the reference stream plane trace at hub




REF_TRACE_TIP_Z


coordinate of the reference stream plane trace at shroud






FIGURE 11 Radial stream traces
Cylindrical Surfaces
Cylindrical stream surfaces allow the 2D blade sections to be defined in the (m,R*θ) and (,θ) planes. The reference surfaces are defined at a constant radius R with respect to the axis of rotation at hub and shroud. This is a useful option for axial turbomachinery.
The streamwise orientation can be changed by means of the switch Orientation from the menu. However, the default value is usually correct when the endwalls have been defined from inlet to outlet.






Parameter


Description






REF_TRACE_HUB_R


R coordinate of the hub reference stream cylinder trace




REF_TRACE_TIP_R


R coordinate of the tip reference stream cylinder trace




Conical Surfaces
Conical stream surfaces allow the 2D blade sections to be defined in the (m,R*θ), (m,β) and (,θ) planes. A reference point (Z,R) and the half cone angle are needed for each of the two reference traces. The Z axis is the axis of revolution. The half cone angle, α, can be positive (hub case in FIGURE 12) or negative (shroud case in FIGURE 12).


FIGURE 12 Conical stream surfaces traces definition






Parameter


Description






REF_TRACE_HUB_Z


Z coordinate of the reference point for span = 0




REF_TRACE_HUB_R


R coordinate of the reference point for span = 0




REF_TRACE_HUB_ALPHA


half cone angle (in degrees) for conical surface for span = 0




REF_TRACE_TIP_Z


Z coordinate of the reference point for span = 1




REF_TRACE_TIP_R


R coordinate of the reference point for span = 1




REF_TRACE_TIP_ALPHA


half cone angle (in degrees) for conical surface for span = 1




Linear Interpolation Surfaces
This case does not require user input since the two reference stream surface traces at spanwise locations 0 and 1 are respectively the hub and the shroud endwall curves (FIGURE 13). This is the quickest and most convenient choice since the surfaces update automatically after an endwall curve adjustment. This type of stream surface is compatible with (m,R*θ), (m,β) and (,θ) construction planes, but do not allow all stacking options (see Blade Meridional & Tangential Locations). Hub to shroud direct interpolation is compatible with both axial and radial turbomachinery. Usually, this option is the typical choice for radial turbomachinery. This option is not appropriate for two-dimensional blades defined by means of one single primary section.


FIGURE 13 Stream surfaces traces definition by linear interpolation
Custom Interpolation
The custom interpolation allows the user to define the stream surface traces based on an interpolation grid with a control on the grid points, the initial hub/ shroud distribution and the smoothing. This type of stream surface has the same restriction as the linear interpolation approach. 






Setting


Description






Hub/Shroud BC


when smoothing active, either the grid points are fixed on hub and/ or shroud (fixed mode) or they are allowed to move on the hub and/or shroud curve (on curve mode)




Curvature weight


the grid point distribution from uniform (0) to curvature (100)




Precision


the number of grid points along the hub and the shroud




Smoothing


the number of smoothing steps




Weight factor


when smoothing active, the higher the weight factor is, the more freedom is given to the grid points movement






FIGURE 14 Stream surfaces traces definition by custom interpolation
The grid used to build the stream surface traces is displayed with the View/Show stream grid menu.


Special options
Cascade topology
The button Cascade topology allows to activate the construction mode for cascade topology. The cascade mode is only available for blades defined on planar axial surfaces in (Z,Y) construction plane. Splitters are also supported. 
The menu Geometry/Export as geomTurbo is limited to geomTurbo 5.3 format in cascade mode.
Non axisymmetric hub / shroud are not available.
Hub and shroud curves must be defined with positive radius: the Z axis cannot be taken as hub curve.
In cascade mode, a new parameter 'CASCADE_PITCH' is used to control the distance between blades (pitch). The parameter 'BLADE_ROTATION' is disabled. The parameter 'NB' will be the number of repetitions for 3D view and CAD export. Blades are repeated with translation along Y axis instead of rotation around Z axis.






Parameter


Description






CASCADE_PITCH


Pitch value for the cascade periodicity




Rounded tip configuration
The rounded tip configuration is entirely controlled from the stream surfaces menu. The method consists in performing a single loft with a degenerate profile at tip (point).
The inputs parameters are:
		

A single span value for the degenerate tip section. This information is used with the stacking and lean laws to automatically define the exact 3D tip point location. This value is parametric, as regular span values for primary sections,
Two clamp factors corresponding to the reference magnitudes (two scalar values), a main for the long direction, a secondary for the short direction,
The number of intermediate imprints on each side (single integer), with a minimum of 0, leading to two vectors (one at leading edge, one at the trailing edge).



FIGURE 15 Rounded tip settings
The feature is applicable under the following restrictions:
        	Only available for axial machines without splitters (axial planar, cylindrical and conical stream surfaces only);Partial and double blunts are not supported;Leading edge and trailing edge stacking points are not suitable. Meridional edge traces can also not be used  (sweep and lean only);	Not compatible with ruled surfaces;	Not compatible with discretized sections (only primary and parametric sections are allowed);	Not compatible with native geomTurbo format. The fitting cannot retrieve the tip point position if edge curves are not defined. Also, only CAD output (Parasolid) is possible as export format for the geomTurbo data;The tip point location is not fitted. It is a user input.

Inlet & Outlet Offsets
Inlet and outlet extensions can be built with an optional signed offset (above or below the revolved hub). Offsets are controlled by two additional parameters and may be applied even if no parameters exist in the perturbed area, whatever the chosen method.






Parameter


Description






HUB_INLET_OFFSET
SHROUD_INLET_OFFSET	


Offset value from hub/shroud revolved surface for construction of the inlet patch, as a 3D distance




HUB_OUTLET_OFFSET
SHROUD_OUTLET_OFFSET	


Offset value from hub/shroud revolved surface for construction of the outlet patch, as a 3D distance

Blade-to-blade view options
The blade-to-blade view (upper right viewport) can be customized by means of the View/b2b view options command (FIGURE 24). The construction plane selected for the camber curve definition is assumed as default, but the designer can select any of the planes listed in TABLE 5.
The blade-to-blade settings are saved to the parametric file and retained. However, an import operation alters those properties.


FIGURE 24 Preferences for the blade-to-blade view
TABLE 5 Available viewing planes







(Z,Y)


(m,Rθ)


(R,Rθ)




(Z,Rθ)


(, θ)


(X,Y)




The option Repeat main blade allows to repeat the blade section in the blade to blade view and should be deactivated when dealing with wind turbines.
The option Show all primary sections allows to stack all primary sections instead of just the current one. If the view is not in stacked mode, the blade-to-blade view is fitted when selecting another section with the selector of a stream trace in the meridional view. If the view is in stacked mode, the blade-to-blade view will be preserved.
The stacking point of each section is added to the blade-to-blade view. The checked option Relatively to stacking point will translate all primary sections so that their stacking point is placed on the stacking point of the current section.
In stacked mode, the current primary section appears with the regular color while curves and stacking points from other sections appear in an alternate color, based on a gradient from two reference colors at span values 0.0 and 1.0. The two reference colors can be modified on the View/b2b view options/Appearance tab. Two colors are defined for spanwise locations at hub (0.0) and shroud (1.0). The color of each section is interpolated from R, G and B channels. These settings are saved to the preference file and are persistent on disk.

Summary Table
All quantities and samples are available whatever the topology choices, except the following options.
TABLE 13 Quantities availability







Quantity


Single blade cases


Splitters cases






Channel width


available


not available




Minimum channel width


available


not available




Unguided turning angle


available


not available




Throat section area


informational only


not available

Technological Effects


FIGURE 73 Technological effects menu
This menu grants access to a set of technological effects that are applied on the final blade shape. The five available features - Hub and shroud gaps, edge rounding, trailing edge filing, blade cutoff and section recut - are applied at the end of the design process, after the construction of the blade sides and edges.
Hub and shroud gaps
This operation allows the user to define a hub and/or shroud gaps, which can be exported to AutoGrid5™ for mesh generation, or exported as a curve. The gap can be defined for the main blade and the splitter independently. After defining the gap, the gap curve appears in the MERIDIONAL view.
The gap curves cannot be exported when exporting the geometry as rulings (the menu Export rulings ).


Three gap types are provided:

None: No gap is defined (default)
Constant: A simple gap is defined with a constant width from the leading edge to the trailing edge. In this case, a single constant width needs to be defined.
Linear: A gap is defined from two width values at leading and trailing edge points. The gap is changing in a linear way in the streamwise direction. In this case, two width parameters at the leading edge and the trailing edge need to be defined.

The button Reset is used to set the gap value to a suitable default value corresponding to 5 percent height of the average edge length (mean value of LE and TE edge lengths).
The Curve extension is used to control the extension of the gap curve before the leading edge location and after the trailing edge location. This factor can be set to any value in range [0.0,0.5], (default value 0.1). It is not advised to set extension to zero if the gap curve itself is exported as a curve. Please note that extensions also follow the offset law.
The gap curve is build from the channel curve as an offset curve with linear or constant value. In case of linear offset, the two values are imposed from the intersection points between the channel curve and the leading / trailing edge curves. This may lead an invalid gap curve if the local radius of curvature of the channel curve is lower than the offset value.
The gap width parameters are non-negative and have a unique naming following the simple rule below, where [] is optional fields and {} mentions special strings listed in the next table.
[SPLIT{INDEX}]{ENDWALL}_[{POSITION}]_GAP_WIDTH






Special fields

 





INDEX


index of the splitter blade, starting from 1




ENDWALL


HUB or SHROUD




POSITION


LE or TE




For example,
			the constant tip gap width parameter on the main blade is named 'SHROUD_GAP_WIDTH'.
		The tip gap width at leading edge of the splitter blade is named 'SPLIT1_SHROUD_LE_GAP_WIDTH'.
Edge Rounding
After applying the edge rounding, the ruled blade surface will be not ruled anymore.
This operation allows to apply internal, external and cutback rounding with elliptical arc, based on a prescribed ratio b/a.


FIGURE 74 Edge rounding options

The internal roundingallows to close the leading/trailing edge with an elliptical arc that is passing through the starting/ending point of the camber curve.
The external rounding allows to close the leading/trailing edge with an elliptical arc that has its center at the starting/ending point of the camber curve.
The cutback rounding allows to close the leading/trailing edge with an elliptical arc that is tangent to the meridional location of the starting/ending point of the camber curve.

The edge rounding is restricted for use with (m,β) or (,θ) construction plane, flank-milled blades, symmetrical thickness addition mode and presence of blunt both at leading/trailing edge.
Trailing Edge Filing
Practically, this operation is achieved with simple tools directly on the manufactured blade and consists in material removal on one of the sides near the trailing edge.
Two lengths are needed on each blade section for that purpose and the designer may select either suction or pressure side or both (see FIGURE 75). To simplify user input, length and thickness distributions are built from one, two or more values of the span parameter.




FIGURE 75 Edge filing length and thickness (suction & pressure sides)
In the simplest case, if Number of parameters is 1, constant length and thickness are applied on all blade sections, so only two parameters FILING_LENGTH_SPAN_0 and FILING_THICK_SPAN_0 need user input. If Number of parameters is 2, length and thickness are required at spanwise locations 0.0 and 1.0. and blade sections values are interpolated or extrapolated linearly from those reference values. If three or more parameters are set up, a spline interpolation is applied and spanwise reference values are free.






Parameter


Description






FILING_LENGTH_SPAN_(i)


Trailing edge filing reference length at i percent of the span




FILING_THICK_SPAN_(i)


Trailing edge filing reference thickness at i percent of the span




When deactivating Straight filing option, the removal of material is applied in a direction normal to the camber curve in (m',θ) plane. The removed thickness is linearly interpolated between "t" for trailing edge and 0 at location "s" along the side curve (FIGURE 76).


FIGURE 76 Straight filing option
When imposing edge filing on both sides of the blade (see FIGURE 75), the removed thickness can be symmetric or not. In the latter option (both_asymmetric), the non-axisymmetry is controlled by a new parameter FILING_SS_FRACTION_SPAN_(i) defined in the range [0,1].
Edge filing does not apply to rounded edges.
Please note that filing length and thickness parameters are measured in Cartesian coordinates X,Y and Z and not in the blade section construction plane.
Blade Cutoff
This option comes from the need for manufacturers to use the same blade design for multiple pumps or compressors. To some extend, design and manufacturing costs can be reduced if an entire family of low- to mid-range turbomachines share the same blades. For instance, blade design is carried out for the most powerful machine of a pump family. Other designs are dimensionally identical except that blades are shorter. This can be achieved simply by cutting the blades near the trailing edge, reducing the head of the pump. Companies have to manufacture a one-size component for the whole family, eventually leading to a reduction of the costs.


FIGURE 77 Example of radial cutoff: blades are cut to achieve a whole family of compressors sharing the same design and dimensions
The blade cutoff option has been developed to be applied at leading or trailing edge in radial and axial cases. This operation preserves the axi-symmetric characteristic of the machinery and is therefore applied in (Z,R) plane.
Spline Cutoff (flank-milled blades)
When working with flank-milled blades, the cutoff can be performed using a meridional spline curve.



The recut is applied to the camber, not the side curves. This means that a 'normal' blunt can be obtained while the linear cutoff produces a tangential blunt.
The recut can be applied with optional extension of the camber curve. This allows the success of the operation on the whole edge even in case of limited recut and avoid discontinuities in the recut area. If late rounding is applied to a discontinuous edge, the model will not be considered as valid.
If, in case of inexistent or insufficient extension in cutoff operation, no intersection is found with one of the camber curves, the model is considered as invalid.
The spline is defined by 2D nodes in a full parametric way. All related parameters are accessed in the Others tab of the Parameters list.







Parameter


Description






LE_CUTOFF_Z(i)
TE_CUTOFF_Z(i)


Axial location of the node i




LE_CUTOFF_R(i)
TE_CUTOFF_R(i)


Radial location of the node i




After applying the cutoff, the user can manually edit the parameters in the Parameters list, or directly edit the spline in the Meridional view. Right-clicking on the Meridonal view and selecting Edit main blade LE/TE cutoff curve will activate the edit mode. The control points of the selected spline will be shown in green points. Each control point can be moved by left-clicking on it. Right-clicking will quit the edit mode.


This operation makes sense on turbomachines with blunt edges. Complete design can be achieved in AutoBlade™ before enabling the cutoff as the very last operation.
If both edge filing and cutoff are applied, filing is applied first.
Section Recut
The effect allows to re-cut the blade sections. One or more spanwise locations are defined for reference and, for each location, a cutting distance is defined in the parametric form. 
For instance, when a cutting distance is defined between the hub and the shroud (span locations 0 and 1), this distance is linearly interpolated or extrapolated for any intermediate location. When more locations are defined for reference, the interpolation uses a spline and is constant in the special case of a single reference location.


FIGURE 78 Sectional cut-off of the blade
All primary and parametric sections are built in the usual way. If discretized sections are required, they are processed before the treatment. Then, all sections are cut at the prescribed 3D distance from the trailing edge using the interpolated value from parameters TE_CUT_LENGTH_SPAN_0 and TE_CUT_LENGTH_SPAN_100 at the prescribed spanwise value.
A switch controls the way this length is input, either as a fraction of the 3D camber or as an absolute length. In case of fraction, the name CUT_LENGTH is replaced by CUT_S.
When a cut value is null or negative, the section is left untouched and no warning or error is generated (the model is assumed valid).

Optional Quantities 
AutoBlade™ provides the ability to compute data such as thickness extrema, moments of inertia and channel width.
Two major interests justify the computation of a quantity:

Monitoring purposes: optional geometrical quantities can be checked at any time in AutoBlade™ interface, even while editing the model.

Constraints: any quantity selected in AutoBlade™ interface can be constrained in the optimization process loop of FINE™/Design3D as part of the objective function (see FINE™/Desing3D User Manual).

Menu Overview


FIGURE 92 Optional quantities menu (selection panel)
Clicking the Optional quantities interface button opens a window with two panels:

a Selection notebook: contains sampling and properties switches to select the desired quantities (see Selection Notebook). Three tabs containing different types of data are available (FIGURE 92).
a Monitor list: contains a double list with the quantity type on the left and corresponding values on the right. The choice panel shows two columns. In the first one, quantity types that were selected through the notebook are listed and, in the second one, the corresponding quantity names are listed with their value. All quantity names conform to a naming convention explained in the next paragraph. Each time a quantity is selected in the notebook, the left list shows one or more new entries (FIGURE 93).

Selecting an item in the left list will refresh the content of the right list, but this is not sufficient to update the values. In particular, newly added quantities are not computed immediately. To update all quantities, please click the Apply button and check the values: they should now appear correct in the right list.
The left Choice  list allows multiple selection by means of the <Shift> and <Ctrl> modifiers. The selection is reset once the window is closed.


FIGURE 93 Optional quantities menu (monitor panel)
The two boxed panel Selection and Monitor can be collapsed and restored by a left click on the corresponding large blue button. This is useful to monitor changes while editing the model since the menu takes less space on the desktop.
Naming Conventions
Every quantity depends on one or several blade sections. Some of them are side or edge specific. In order to allow easy distinction and ensure consistency between menus, a naming convention has been established. Conventions in the formula below are described shortly and will be particularized for each quantity type.
(S?_)(SPLIT?_)(PREFIX_)QUANTITY_(SUFFIX)
where ’?’ stands for a digit and ’(...)’ describes an optional field





Field
                    
Description
                    





S?_


Section prefix
This prefix applies for section specific quantities. An integer is used to define the section number, ranging from 1 to the total amount of primary sections.
S1_ defines a quantity relative to the first primary blade section
S1S3_ is a special notation for a quantity difference between sections 1 and 3.




SPLIT?_


Splitter prefix
This prefix applies for splitter specific quantities. Numbering begins at 1 for the first splitter.
SPLIT1_ defines a quantity relative to the first splitter blade.




PREFIX_


Quantity prefix
This prefix applies for quantities that depend on a side or an edge.
LE and TE mean leading and trailing edges,
SS and PS apply for suction and pressure side respectively.




QUANTITY_


Quantity name
This is the quantity base name. The chosen string is as short as possible while long enough to allow easy understanding.
For instance, THICK stands for "thickness" and WEDGEANG stands for "wedge angle".




SUFFIX_


Quantity suffix
This suffix is chosen among three types:

extrema suffixes MIN_ and MAX_ for maximum and minimum values,
sampling suffixes U??_ for samples,
special MIN_U and MAX_U suffixes for extrema locations.

For instance, THICK_MAX, THICK_U34 and THICK_MAX_U stand respectively for maximum thickness value, thickness value at 34 percent of the length and length fraction corresponding to the maximum thickness value.

Camber Curve Definition
The camber curve is constructed in a dimensional plane using either the given reference length or meridional extent. It is then applied on the stream surfaces with the help of a transformation to meet the stacking point requirement.


FIGURE 35 Camber curve definition
The camber curve must be a pure function of the construction abscissa. It is not possible to build camber curves like the ones shown in FIGURE 36. If such a case occurs, AutoBlade™ may apply a correction to any inadequate parameter value or bound set by the user. A warning or an error message is generated to point out the problem.


FIGURE 36 Invalid camber curves
TABLE 4 Camber curve types


Meridional Chord Based Cambers
Bezier curve defined by n control points
The n control points are by default equally spaced in the abscissa interval (Z, m or  coordinate), the first point being placed at origin (0,0). The user can adjust the number of parameters from 1 to any higher integer and change the distribution of the points (uniform, geometric and twice_geometric) by imposing the stretching factor  (first/second common ratio). 
When selecting the geometric distribution, imposing a ratio from 1 (for uniform intervals) to a factor bigger/lower than 1 will result in increasing/decreasing intervals from leading to trailing edge (asymmetrical points distribution). 
The simplest case 1 corresponds to a linear segment (2 control points). The formula linking the number of control points to the number of parameters appearing in the interface is, taking into account that the first control point is always located at the origin,
number of control points = number of parameters S(i)_CAMBER_H(j) + 1
Thanks to the simplified way to manage control points, only (n-1) ordinates S(i)_CAMBER_H(j) must be specified in the parameters menu (FIGURE 37, left). Values can be negative. This curve is not compatible with the (m,β) construction plane.
Cubic B-spline curve defined by n control points
The spline case is very similar to the Bezier case explained above, except that the curve passes through the given points instead of being controlled by them (FIGURE 37, right).


FIGURE 37 Bezier & B-spline curves defined by equally spaced nodes






Parameter


Description






S(i)_CAMBER_H(j)


construction ordinate (j) for the camber curve of section (i)




Bezier using angles γ, β1 and β2
A simple second order Bezier curve can be used to define the camber line (FIGURE 38). The first control point coincides with the leading edge at the origin and the last one with the trailing edge. The relative position of the two edges is defined by the stagger angle γ. A third control point is constructed from leading and trailing edges using respectively angles β1 and β2. All angles are measured in degrees from the abscissa direction.
This method is not compatible with the (m,β) construction plane.






Parameter


Description






SN(i)_STAGGER_ANGLE


the stagger angle γ (in degrees) for the camber curve of section (i)




S(i)_CAMBER_BETA1


inlet metal angle β1 (in degrees) for camber curve in section (i)




S(i)_CAMBER_BETA2


outlet metal angle β2 (in degrees) for camber curve in section (i)






FIGURE 38 Definition of the camber curve
The second order Bezier curve type calls for an additional comment: the stagger angle value is accepted only if it lies between CAMBER_BETA1 and CAMBER_BETA2  values. This condition is necessary to ensure the existence of a control polygon for the curve. This simple curve type cannot show an inflexion point either (reversal of the sign in curvature values).
Integrated Bezier & B-spline curves
The special construction plane (m,β) requires a non zero starting angle and introduces its own curves. the β distribution is defined by a similar curve to the one described above: it is built from nodes equally spaced along the abscissa axis in the form of a Bezier or a B-spline curve.
Abscissa is the non dimensional interval [0,1] and can be interpreted as the length fraction of the camber curve. The ordinate is the prescribed β angle expressed in degrees (FIGURE 39). The camber curve is obtained by integration of this angle distribution on the stream surface according to equation below.



Those curves are reserved to (m,β) construction plane.


FIGURE 39 Bezier distribution for an integrated camber curve.
Circle arc
A circle arc can be used to define the camber line. The arc is defined by start and end angles β1 and β2. This option is only available in axial planes (Z,Y) and (m,R*θ).
True chord based cambers
For True chord based profiles, four new curve types replace the usual curves in (Z,Y), (m,R*θ) and (,θ) planes as summarized in TABLE 7.
Simple Bezier curve
The simplest curve defined by a second Bezier curve is reused in a slightly different parametrization. The stagger angle is kept, with an increased range [-180.0,180.0]. The two relative angles δ1 and δ2 respectively replace the absolute metal angles β1 and β2 (FIGURE 40). The edge angles are still limited to 90 degrees, but the signs of δ1 and δ2 are always opposite. This property ensures that no invalid topology may be generated in optimization if the bounds of the δ1 are positive while those of δ2 are negative.


FIGURE 40 The classic second order Bezier curve defined based on meridional chord (left) and its new definition based on true chord (right)
Bezier & B-spline curves where nodes equally spaced along the chord
The two types of curve use similar height parameters as with meridional chord. There are two major differences:

 	the last height parameter is dropped (curve end),
 	the stagger angle is added to ensure the proper orientation of the camber curve.



FIGURE 41 Bezier curve defined by heights at uniformly spaced abscissa based on meridional chord (left) and its new definition based on true chord (right)
Circle arc
A circle arc can be used to define the camber line. The arc is defined by start and end angles δ1 and δ2. This option is only available in axial planes (Z,Y) and (m,R*θ).
User-defined Camber Curve
The user-defined camber distribution is defined form a dimensionless abscissa, in the [0,1] range, whatever the construction plane. In case of (Z,Y), (m,Rθ) and (,θ) planes, the starting point should be (0,0). In case of (m,β) plane, the ordinate is free.
User defined camber curve is not compatible with parametric sections.
Data file
If the camber distribution law is available as an external data file, it can be imported as a user-defined law in the parametric model. 


FIGURE 42 User-defined data file
The following controls allow to set the selected distribution:

The option Include points as parameters allows to include all reference points as regular parameters for the fitting or the optimization. This means that the law can be initialized and even altered by the fitting process!
The option Dimensional height specifies either if the ordinate must be considered as the values read (checked) or if the provided law must be scaled by the length of the camber curve (unchecked).
The option Height factor allows to scale the ordinate of the prescribed camber curve by means of the optional floating point value (on the right side).

The user-defined camber distribution law can be defined in a simple text format, as illustrated in the example below.
# comments
101			(amount of defining points)
0.0	0.0
0.01	0.01598
...
0.99	2.457
1.0	2.469
The first input number is the amount of provided points. Then, each line defines a single point. A comment may be added anywhere provided that it starts the line with '#' character.
The abscissa should be increasing and cover the [0,1] range exactly in order to produce a valid camber curve or wrap angle distribution. If the range is not fully covered, a warning is generated and the distribution is internally adapted to match the starting and ending values.


FIGURE 43 Input user-defined camber distribution
The user-defined camber distribution can be only inputted by Right-clicking in the CAMBER view, as shown in FIGURE 43.
In the Init curve from file dialog, The user can enter the path ended by a hit on the <Enter> key or click the button on the right and use a classic file chooser. By default, no file is active and the value in the field is none. Once selected, the file is parsed and checked: if the color of the field is changed to red, this means that the file does not comply with the format specification described above! 
If the button Apply to all sections is checked, the inputted user-defined camber distribution will be applied to all sections.
Expression
The camber curve can be defined by a mathematical expression involving a single parameter 's' for each blade. In order to simplify the user input, this expression can use an existing function with an arbitrary amount of arguments. For example, a user-defined expression is used in FIGURE 44, where NACA4_CAMBER() is the user-defined function; s is a dimensionalized abscissa along the chord and ranges from 0 to 1; M1 and P1 is the user-defined optional parameters.


FIGURE 44 User-defined expression
A valid formula should always produce a zero ordinate for a zero abscissa except for the wrap angle distribution. If the camber is defined using the chord, the ordinate should also be zero for abscissa 1.0. If the law does not comply to these rules, it is internally altered to enforce the conditions.

AutoBlade™ Fitting


The AutoBlade™  Fitting allows the designer to create a parametric blade model close to a given customer geometry defined by point coordinates. In this way, it can be seen as a functionality used to import a blade geometry into the AutoBlade™ or FINE™/Design3D environment.
When a turbomachinery model has not been created under AutoBlade™, it is not possible to import it directly as a simple and almost instantaneous operation. Instead, the following procedure is required to obtain an AutoBlade™ model close enough to the target design:

First, the data from the CAD software must be converted to the geomTurbo format described in the next sections. The resulting file is the target geometry.
An initial model will then be generated from a quick analysis of the target geometry. Some choices in topology and parameters are necessary at this stage and a range of values will be estimated for each parameter by means of a process called initialization. The resulting parametric design is referred to as the initial model.
At last, an iterative process is launched to search the multidimensional space of valid parameters and to find a better subset of values for the defining parameters. This process, called fitting, is the time consuming part and may require two or three runs to achieve a satisfying model. The resulting model is called the fitted solution and will be considered as a conversion of the target geometry into an AutoBlade™ parametric blade model.

In AutoBlade™, only one fitting process can be launched in a single project.
The fitting module is a kind of optimization tool and is integrated in AutoBlade™ starting from version 8.9. FIGURE 1 shows the fitting interface. The following pads or menu are dedicated to the fittings module:

The subpad Target Settings in the left area - allows to access the target settings for the fitting project, see also Target Settings subpad for more details.
The subpad Fitting Control in the left area - allows to control the fitting process, see also Fitting Control subpad for more details.
The submenus under the menu Analysis - allows to analyze the fitting result, see also Analysis Menu for more details.

The fitting module requires a special license feature.


FIGURE 1 The fitting interface
In the following sections, a step by step guide to the fitting process will be given.

GeomTurbo 5.3 Example
The following file complies with geomTurbo 5.3 format and can be used within AutoGrid™ 5.
GEOMETRY TURBO
VERSION 5.3
TOLERANCE                                          1E-06
 
NI_BEGIN CHANNEL
  NI_BEGIN basic_curve
    NAME		hub
    DISCRETISATION	10
    NI_BEGIN zrcurve
      ZR
      +28
      -0.0425	0.17526	
      -0.0307086	0.17526	
      -0.0243586	0.175412	
      -0.0180086	0.175717	
      -0.0116586	0.176022	
      -0.0026416	0.177394	
      0.001016	0.178054	
      0.007366	0.179578	
      0.013716	0.181229	
      0.020066	0.182982	
      0.0264414	0.184404	
      0.0327914	0.185674	
      0.0391414	0.186741	
      0.045212	0.187681	
      0.0515366	0.188671	
      0.0578866	0.189484	
      0.0642366	0.190297	
      0.0705866	0.19111	
      0.0769366	0.19177	
      0.0832866	0.192354	
      0.0896366	0.192938	
      0.0959866	0.193294	
      0.102337	0.19365	
      0.108687	0.193904	
      0.115037	0.194056	
      0.121387	0.194208	
      0.126467	0.194335	
      0.135	0.194335	
    NI_END   zrcurve
  NI_END   basic_curve
  NI_BEGIN basic_curve
    NAME		shroud
    DISCRETISATION	10
    NI_BEGIN zrcurve
      ZR
      +28
      -0.0425	0.256692	
      -0.0312928	0.256565	
      -0.0249428	0.256388	
      -0.0185928	0.256083	
      -0.0122428	0.255626	
      -0.0058928	0.254864	
      0.0004572	0.253746	
      0.0068072	0.252222	
      0.0131572	0.250495	
      0.0195072	0.248717	
      0.0258572	0.246888	
      0.0322072	0.245161	
      0.0385572	0.243738	
      0.0449072	0.242672	
      0.0512572	0.242062	
      0.0576072	0.241732	
      0.0639572	0.241452	
      0.0703072	0.241097	
      0.0766572	0.240665	
      0.0830072	0.240182	
      0.0893572	0.239827	
      0.0957072	0.23942	
      0.102057	0.23876	
      0.108407	0.238354	
      0.114757	0.237998	
      0.121107	0.237642	
      0.126187	0.23749	
      0.135	0.237363	
    NI_END   zrcurve
  NI_END   basic_curve
  NI_BEGIN channel_curve hub
    NAME		hub
    VERTEX		hub	0
    VERTEX		hub	1
  NI_END   channel_curve hub
  NI_BEGIN channel_curve shroud
    NAME		shroud
    VERTEX		shroud	0
    VERTEX		shroud	1
  NI_END   channel_curve shroud
NI_END   CHANNEL

NI_BEGIN NIROW
  NAME		row 1
  TYPE		normal
  PERIODICITY		36
  NI_BEGIN NIBLADE
    NAME		Main Blade
    NI_BEGIN NIBLADEGEOMETRY
      TYPE			GEOMTURBO
      GEOMETRY_MODIFIED	0
      GEOMETRY TURBO VERSION 5
      blade_expansion_factor_hub			0.03
      blade_expansion_factor_shroud			0.03
      intersection_npts			10
      intersection_control			0
      number_of_blades			36
      suction
      SECTIONAL
      3
      # section 1
      XYZ
      +106
      0.17669	-0.0208609	0.000351471	
      0.176689	-0.0208418	0.000335267	
      0.176689	-0.0208217	0.000321196	
      0.176689	-0.0208002	0.000308953	
      0.17669	-0.0207763	0.000298336	
      0.176691	-0.0207475	0.000289117	
      0.176697	-0.0206839	0.000281091	
      0.176706	-0.0206206	0.000289117	
      0.176711	-0.0205922	0.000298336	
      0.176716	-0.0205687	0.000308953	
      0.176721	-0.0205471	0.000321196	
      0.176726	-0.0205228	0.000335267	
      0.176733	-0.0204953	0.000351471	
      0.17674	-0.0204633	0.000370063	
      0.176748	-0.0204267	0.000391449	
      0.176758	-0.0203848	0.000415985	
      0.176769	-0.0203366	0.000444127	
      0.176781	-0.0202815	0.000476459	
      0.176796	-0.0202181	0.000513517	
      0.176812	-0.0201457	0.000555958	
      0.176831	-0.0200631	0.00060447	
      0.176853	-0.019969	0.000659739	
      0.176877	-0.0198621	0.000722525	
      0.176905	-0.0197415	0.000793617	
      0.176936	-0.0196056	0.000873903	
      0.176971	-0.0194527	0.000964298	
      0.17701	-0.0192817	0.00106579	
      0.177054	-0.0190908	0.00117948	
      0.177103	-0.0188783	0.00130655	
      0.177155	-0.0186552	0.00144058	
      0.177212	-0.0184092	0.00158921	
      0.177275	-0.0181384	0.00175377	
      0.177345	-0.0178413	0.00193573	
      0.177422	-0.0175159	0.00213666	
      0.177506	-0.0171605	0.00235832	
      0.177598	-0.016773	0.00260258	
      0.177705	-0.0163289	0.00288604	
      0.177823	-0.0158442	0.00319969	
      0.177952	-0.0153146	0.00354699	
      0.178094	-0.0147345	0.00393199	
      0.178251	-0.0140965	0.00435963	
      0.178424	-0.0133911	0.00483594	
      0.178615	-0.0126084	0.00536792	
      0.178825	-0.0117457	0.00595929	
      0.179062	-0.0107612	0.00664244	
      0.179316	-0.00969826	0.00739387	
      0.179585	-0.0085647	0.00822069	
      0.179869	-0.00738629	0.00913027	
      0.18017	-0.00617709	0.0101307	
      0.180494	-0.00486988	0.0112305	
      0.180846	-0.00336678	0.0124389	
      0.181227	-0.00172503	0.0137656	
      0.181642	-6.61359E-05	0.0152216	
      0.182088	0.00153746	0.0168217	
      0.182558	0.00312748	0.0185841	
      0.183029	0.00477259	0.0205313	
      0.183445	0.00627275	0.0224897	
      0.183825	0.00759274	0.0244556	
      0.184151	0.0087059	0.0262459	
      0.184444	0.00960719	0.0278742	
      0.184706	0.010364	0.0293552	
      0.184939	0.011008	0.0307027	
      0.185145	0.0115486	0.0319291	
      0.185325	0.0120016	0.0330455	
      0.185484	0.0123811	0.0340617	
      0.185624	0.0126985	0.0349864	
      0.185748	0.0129647	0.0358278	
      0.185859	0.0131903	0.0365931	
      0.185959	0.0133835	0.0372892	
      0.186044	0.013542	0.0378917	
      0.186121	0.0136777	0.0384335	
      0.186189	0.0137936	0.0389184	
      0.186249	0.0138931	0.0393534	
      0.186304	0.0139787	0.0397448	
      0.186353	0.0140526	0.0400976	
      0.186397	0.0141164	0.0404159	
      0.186437	0.0141716	0.0407034	
      0.186472	0.0142172	0.0409509	
      0.186504	0.0142572	0.0411753	
      0.186532	0.0142921	0.0413786	
      0.186558	0.0143228	0.0415626	
      0.186582	0.0143498	0.0417289	
      0.186603	0.0143736	0.0418791	
      0.186622	0.0143946	0.0420144	
      0.18664	0.0144131	0.0421361	
      0.186656	0.0144304	0.0422513	
      0.186671	0.0144455	0.0423542	
      0.186684	0.0144588	0.0424458	
      0.186695	0.0144705	0.0425271	
      0.186706	0.0144808	0.0425992	
      0.186715	0.0144898	0.0426628	
      0.186723	0.0144977	0.0427188	
      0.18673	0.0145044	0.042768	
      0.186736	0.0145054	0.0428111	
      0.186743	0.0145001	0.0428487	
      0.186748	0.0144906	0.0428815	
      0.186754	0.0144782	0.0429101	
      0.186759	0.0144635	0.042935	
      0.186763	0.0144472	0.0429567	
      0.186768	0.0144296	0.0429756	
      0.186772	0.0144109	0.0429921	
      0.186776	0.014391	0.0430064	
      0.186779	0.0143695	0.0430189	
      0.186783	0.0143456	0.0430297	
      0.186786	0.0143166	0.0430392	
      0.186793	0.0142511	0.0430476	
      # section 2
      XYZ
      +102
      0.217127	-0.0231681	0.00303258	
      0.217128	-0.0231547	0.00301933	
      0.21713	-0.0231404	0.0030078	
      0.217132	-0.0231247	0.00299778	
      0.217134	-0.0231074	0.00298909	
      0.217136	-0.0230861	0.00298156	
      0.217141	-0.0230388	0.00297498	
      0.217146	-0.0229917	0.00298156	
      0.217148	-0.0229704	0.00298909	
      0.21715	-0.0229528	0.00299778	
      0.217152	-0.0229354	0.0030078	
      0.217154	-0.0229154	0.00301933	
      0.217156	-0.0228924	0.00303258	
      0.217159	-0.0228659	0.00304783	
      0.217162	-0.0228354	0.00306532	
      0.217165	-0.0228007	0.0030854	
      0.217169	-0.0227605	0.00310845	
      0.217174	-0.0227146	0.00313489	
      0.217179	-0.022662	0.00316527	
      0.217185	-0.0226016	0.00320002	
      0.217192	-0.0225327	0.00323976	
      0.217199	-0.0224543	0.00328503	
      0.217208	-0.0223652	0.00333647	
      0.217218	-0.0222641	0.00339477	
      0.217229	-0.0221502	0.00346057	
      0.217241	-0.022022	0.00353471	
      0.217255	-0.0218781	0.00361798	
      0.217271	-0.0217172	0.00371129	
      0.217289	-0.0215374	0.0038156	
      0.217307	-0.021348	0.00392571	
      0.217327	-0.0211382	0.00404787	
      0.217349	-0.0209063	0.00418319	
      0.217374	-0.0206503	0.0043329	
      0.217401	-0.0203681	0.00449835	
      0.217431	-0.0200576	0.00468094	
      0.217463	-0.0197164	0.00488234	
      0.2175	-0.0193216	0.00511623	
      0.21754	-0.0188862	0.00537524	
      0.217584	-0.0184058	0.00566229	
      0.217632	-0.0178749	0.00598079	
      0.217685	-0.0172871	0.00633486	
      0.217741	-0.0166341	0.00672957	
      0.217803	-0.0159073	0.00717072	
      0.217869	-0.0151029	0.00766143	
      0.217941	-0.0141796	0.0082285	
      0.218016	-0.0131724	0.00885233	
      0.218091	-0.0120731	0.00953855	
      0.218167	-0.0108711	0.0102934	
      0.218242	-0.00955873	0.0111238	
      0.218317	-0.00813882	0.0120372	
      0.21839	-0.00660734	0.0130419	
      0.218461	-0.004933	0.0141469	
      0.218531	-0.00310057	0.0153623	
      0.218592	-0.00112156	0.0166992	
      0.218634	0.00100507	0.01817	
      0.218643	0.00323621	0.0197883	
      0.218611	0.00530518	0.0214069	
      0.21855	0.00721804	0.0230256	
      0.218477	0.00884761	0.0244972	
      0.218404	0.0102505	0.025835	
      0.218331	0.0114683	0.0270512	
      0.218261	0.0125242	0.0281569	
      0.218193	0.01344	0.029162	
      0.218127	0.0142372	0.0300757	
      0.218065	0.0149369	0.0309063	
      0.218006	0.0155568	0.0316614	
      0.217951	0.0161082	0.0323478	
      0.2179	0.0165992	0.0329718	
      0.217853	0.0170364	0.0335391	
      0.217813	0.0174069	0.03403	
      0.217777	0.0177328	0.0344713	
      0.217744	0.0180183	0.0348661	
      0.217715	0.0182695	0.0352203	
      0.21769	0.018492	0.0355389	
      0.217667	0.0186901	0.0358261	
      0.217646	0.0188671	0.0360852	
      0.217628	0.0190257	0.0363191	
      0.217612	0.0191614	0.0365206	
      0.217598	0.0192839	0.0367032	
      0.217585	0.0193943	0.0368687	
      0.217573	0.019494	0.0370185	
      0.217563	0.0195838	0.0371539	
      0.217553	0.0196647	0.0372761	
      0.217545	0.0197374	0.0373862	
      0.217537	0.0198026	0.0374853	
      0.21753	0.0198643	0.0375791	
      0.217524	0.0199193	0.0376628	
      0.217518	0.0199682	0.0377374	
      0.217513	0.0200116	0.0378036	
      0.217509	0.0200499	0.0378623	
      0.217505	0.0200838	0.037914	
      0.217501	0.0201136	0.0379596	
      0.217499	0.0201321	0.0379997	
      0.217498	0.0201394	0.0380347	
      0.217497	0.0201398	0.0380654	
      0.217497	0.0201358	0.0380921	
      0.217498	0.0201287	0.0381153	
      0.217498	0.0201194	0.0381356	
      0.217499	0.0201085	0.0381533	
      0.2175	0.0200963	0.0381687	
      0.217501	0.0200831	0.0381821	
      0.217502	0.0200688	0.0381938	
      # section 3
      XYZ
      +101
      0.251068	-0.0250123	0.00642899	
      0.251071	-0.0250032	0.0064185	
      0.251075	-0.0249931	0.00640938	
      0.251078	-0.0249818	0.00640146	
      0.251081	-0.0249691	0.00639458	
      0.251084	-0.0249534	0.00638863	
      0.251089	-0.024918	0.00638343	
      0.251091	-0.0248824	0.00638863	
      0.251091	-0.0248664	0.00639458	
      0.251091	-0.0248518	0.00640146	
      0.251091	-0.024835	0.00640938	
      0.25109	-0.0248157	0.0064185	
      0.25109	-0.0247935	0.00642899	
      0.251089	-0.024768	0.00644106	
      0.251088	-0.0247387	0.00645487	
      0.251087	-0.0247051	0.00647077	
      0.251086	-0.0246665	0.00648901	
      0.251085	-0.0246222	0.00650991	
      0.251084	-0.0245715	0.00653394	
      0.251082	-0.0245134	0.00656142	
      0.251081	-0.024447	0.00659284	
      0.251078	-0.0243714	0.00662865	
      0.251076	-0.0242856	0.00666932	
      0.251073	-0.0241885	0.00671539	
      0.25107	-0.0240789	0.00676743	
      0.251067	-0.0239556	0.00682603	
      0.251062	-0.0238174	0.00689184	
      0.251058	-0.0236627	0.00696557	
      0.251052	-0.0234903	0.00704804	
      0.251046	-0.0233086	0.00713503	
      0.251039	-0.0231077	0.00723155	
      0.251031	-0.0228858	0.00733848	
      0.251021	-0.0226413	0.00745676	
      0.251011	-0.0223724	0.00758744	
      0.250998	-0.0220769	0.00773168	
      0.250984	-0.0217526	0.0078907	
      0.250967	-0.0213778	0.00807538	
      0.250947	-0.0209644	0.00827987	
      0.250924	-0.0205076	0.00850645	
      0.250897	-0.020001	0.0087578	
      0.250865	-0.019437	0.00903716	
      0.250829	-0.0188064	0.00934853	
      0.250786	-0.0180988	0.00969644	
      0.250736	-0.017309	0.0100834	
      0.250674	-0.0163931	0.0105304	
      0.250603	-0.0153838	0.011022	
      0.250519	-0.0142764	0.0115627	
      0.250421	-0.0130649	0.0121573	
      0.250305	-0.0117371	0.0128113	
      0.25017	-0.0102766	0.0135307	
      0.250011	-0.00867329	0.0143219	
      0.249824	-0.00692007	0.0151922	
      0.249603	-0.00500169	0.0161493	
      0.249342	-0.00287863	0.0172017	
      0.249032	-0.000511463	0.0183589	
      0.248663	0.00199586	0.019631	
      0.248266	0.00448552	0.0209022	
      0.247834	0.00725954	0.0221728	
      0.24743	0.00934753	0.0233276	
      0.247053	0.0111107	0.0243776	
      0.246703	0.0126726	0.0253325	
      0.246382	0.0140067	0.0262008	
      0.246088	0.0151793	0.0269907	
      0.245819	0.0162116	0.0277093	
      0.245576	0.0170985	0.0283629	
      0.245357	0.017861	0.0289576	
      0.24516	0.018529	0.0294987	
      0.244981	0.0191217	0.029991	
      0.24482	0.0196488	0.0304389	
      0.244681	0.0200948	0.0308267	
      0.244557	0.0204871	0.0311756	
      0.244447	0.0208312	0.0314879	
      0.244349	0.0211346	0.0317683	
      0.244262	0.0214037	0.0320206	
      0.244183	0.0216433	0.0322481	
      0.244112	0.0218572	0.0324535	
      0.244049	0.0220488	0.032639	
      0.243995	0.0222126	0.0327988	
      0.243946	0.0223602	0.0329438	
      0.243901	0.0224933	0.0330751	
      0.243861	0.0226131	0.033194	
      0.243825	0.0227211	0.0333015	
      0.243792	0.0228182	0.0333986	
      0.243763	0.0229055	0.033486	
      0.243737	0.0229838	0.0335648	
      0.243712	0.0230577	0.0336393	
      0.24369	0.0231236	0.0337059	
      0.24367	0.0231822	0.0337651	
      0.243653	0.0232341	0.0338177	
      0.243637	0.02328	0.0338644	
      0.243624	0.0233206	0.0339055	
      0.243612	0.0233555	0.0339418	
      0.243602	0.0233746	0.0339736	
      0.243595	0.0233824	0.0340015	
      0.243589	0.0233839	0.0340258	
      0.243584	0.0233814	0.0340471	
      0.24358	0.0233762	0.0340656	
      0.243577	0.0233691	0.0340817	
      0.243575	0.0233606	0.0340958	
      0.243573	0.0233511	0.034108	
      0.243571	0.0233406	0.0341187	
      pressure
      SECTIONAL
      3
      # section 1
      XYZ
      +94
      0.17669	-0.0208609	0.000351471	
      0.176691	-0.0208788	0.000370063	
      0.176693	-0.0208955	0.000391449	
      0.176696	-0.0209107	0.000415985	
      0.1767	-0.0209239	0.000444127	
      0.176705	-0.0209342	0.000476459	
      0.176712	-0.0209405	0.000513517	
      0.17672	-0.0209406	0.000555958	
      0.17673	-0.0209316	0.00060447	
      0.176744	-0.0209076	0.000659739	
      0.176763	-0.0208557	0.000722525	
      0.176785	-0.0207848	0.000793617	
      0.17681	-0.0207048	0.000873903	
      0.176839	-0.0206148	0.000964298	
      0.176871	-0.0205139	0.00106579	
      0.176908	-0.0204007	0.00117948	
      0.176949	-0.0202743	0.00130655	
      0.176992	-0.0201412	0.00144058	
      0.17704	-0.0199936	0.00158921	
      0.177094	-0.0198303	0.00175377	
      0.177154	-0.01965	0.00193573	
      0.17722	-0.019451	0.00213666	
      0.177293	-0.019232	0.00235832	
      0.177375	-0.0189909	0.00260258	
      0.17747	-0.0187116	0.00288604	
      0.177576	-0.018403	0.00319969	
      0.177694	-0.0180618	0.00354699	
      0.177825	-0.0176839	0.00393199	
      0.177972	-0.0172643	0.00435963	
      0.178136	-0.0167966	0.00483594	
      0.178319	-0.0162734	0.00536792	
      0.178522	-0.0156898	0.00595929	
      0.178756	-0.0150119	0.00664244	
      0.179011	-0.0142601	0.00739387	
      0.179287	-0.0134251	0.00822069	
      0.179586	-0.0124979	0.00913027	
      0.179911	-0.0114742	0.0101307	
      0.180262	-0.0103699	0.0112305	
      0.180643	-0.00920084	0.0124389	
      0.181063	-0.00789994	0.0137656	
      0.181529	-0.00639667	0.0152216	
      0.182033	-0.00472947	0.0168217	
      0.18256	-0.00298793	0.0185841	
      0.183087	-0.00118232	0.0205313	
      0.183552	0.000569893	0.0224897	
      0.183968	0.00223894	0.0244556	
      0.184319	0.0036897	0.0262459	
      0.184627	0.00494096	0.0278742	
      0.184899	0.00601565	0.0293552	
      0.185136	0.00695767	0.0307027	
      0.185341	0.00779946	0.0319291	
      0.185517	0.00854382	0.0330455	
      0.185669	0.00919753	0.0340617	
      0.185801	0.00977275	0.0349864	
      0.185916	0.0102805	0.0358278	
      0.186018	0.0107304	0.0365931	
      0.186108	0.0111305	0.0372892	
      0.186184	0.0114699	0.0378917	
      0.186251	0.0117696	0.0384335	
      0.186311	0.0120332	0.0389184	
      0.186363	0.0122659	0.0393534	
      0.186411	0.012472	0.0397448	
      0.186453	0.0126551	0.0400976	
      0.186491	0.012818	0.0404159	
      0.186525	0.0129631	0.0407034	
      0.186555	0.0130865	0.0409509	
      0.186582	0.0131972	0.0411753	
      0.186606	0.0132966	0.0413786	
      0.186628	0.0133858	0.0415626	
      0.186648	0.0134658	0.0417289	
      0.186666	0.0135375	0.0418791	
      0.186682	0.0136018	0.0420144	
      0.186696	0.0136594	0.0421361	
      0.18671	0.0137137	0.0422513	
      0.186722	0.0137619	0.0423542	
      0.186733	0.0138048	0.0424458	
      0.186743	0.0138428	0.0425271	
      0.186752	0.0138763	0.0425992	
      0.186759	0.0139059	0.0426628	
      0.186766	0.0139318	0.0427188	
      0.186772	0.0139546	0.042768	
      0.186777	0.0139745	0.0428111	
      0.186781	0.013992	0.0428487	
      0.186785	0.0140071	0.0428815	
      0.186789	0.0140209	0.0429101	
      0.186791	0.0140361	0.042935	
      0.186794	0.0140529	0.0429567	
      0.186795	0.0140709	0.0429756	
      0.186796	0.0140901	0.0429921	
      0.186797	0.0141103	0.0430064	
      0.186797	0.0141321	0.0430189	
      0.186797	0.0141562	0.0430297	
      0.186796	0.0141855	0.0430392	
      0.186793	0.0142511	0.0430476	
      # section 2
      XYZ
      +98
      0.217127	-0.0231681	0.00303258	
      0.217125	-0.0231803	0.00304783	
      0.217124	-0.0231913	0.00306532	
      0.217123	-0.0232009	0.0030854	
      0.217122	-0.0232082	0.00310845	
      0.217121	-0.0232125	0.00313489	
      0.217121	-0.0232125	0.00316527	
      0.217121	-0.0232059	0.00320002	
      0.217123	-0.0231888	0.00323976	
      0.217126	-0.0231503	0.00328503	
      0.217133	-0.0230862	0.00333647	
      0.21714	-0.0230134	0.00339477	
      0.217148	-0.022931	0.00346057	
      0.217157	-0.022838	0.00353471	
      0.217168	-0.0227337	0.00361798	
      0.217179	-0.0226166	0.00371129	
      0.217192	-0.0224854	0.0038156	
      0.217206	-0.0223466	0.00392571	
      0.217222	-0.0221925	0.00404787	
      0.217239	-0.0220214	0.00418319	
      0.217259	-0.0218315	0.0043329	
      0.21728	-0.0216212	0.00449835	
      0.217304	-0.0213882	0.00468094	
      0.21733	-0.0211304	0.00488234	
      0.21736	-0.02083	0.00511623	
      0.217394	-0.0204962	0.00537524	
      0.217432	-0.0201254	0.00566229	
      0.217473	-0.0197138	0.00598079	
      0.217519	-0.019257	0.00633486	
      0.217569	-0.0187499	0.00672957	
      0.217625	-0.0181856	0.00717072	
      0.217685	-0.017559	0.00766143	
      0.217752	-0.0168328	0.0082285	
      0.217824	-0.0160287	0.00885233	
      0.2179	-0.0151392	0.00953855	
      0.217978	-0.0141596	0.0102934	
      0.21806	-0.0130814	0.0111238	
      0.218145	-0.0118857	0.0120372	
      0.218234	-0.0105593	0.0130419	
      0.218327	-0.0091119	0.0141469	
      0.218423	-0.00752169	0.0153623	
      0.218519	-0.00574169	0.0166992	
      0.218603	-0.00379413	0.01817	
      0.21866	-0.00166115	0.0197883	
      0.218675	0.00048992	0.0214069	
      0.218653	0.00260323	0.0230256	
      0.218611	0.00445339	0.0244972	
      0.218559	0.00610324	0.025835	
      0.2185	0.00758562	0.0270512	
      0.218438	0.00889941	0.0281569	
      0.218374	0.0100659	0.029162	
      0.218309	0.0111166	0.0300757	
      0.218243	0.0120647	0.0309063	
      0.218178	0.0129181	0.0316614	
      0.218117	0.0136848	0.0323478	
      0.218058	0.0143722	0.0329718	
      0.218004	0.0149886	0.0335391	
      0.217956	0.0155155	0.03403	
      0.217912	0.0159844	0.0344713	
      0.217872	0.0164004	0.0348661	
      0.217836	0.0167711	0.0352203	
      0.217803	0.0171032	0.0355389	
      0.217774	0.0174016	0.0358261	
      0.217747	0.0176705	0.0360852	
      0.217722	0.0179132	0.0363191	
      0.217701	0.0181223	0.0365206	
      0.217682	0.0183118	0.0367032	
      0.217664	0.0184836	0.0368687	
      0.217648	0.0186392	0.0370185	
      0.217634	0.0187799	0.0371539	
      0.217621	0.0189069	0.0372761	
      0.217609	0.0190214	0.0373862	
      0.217598	0.0191244	0.0374853	
      0.217588	0.019222	0.0375791	
      0.217579	0.0193091	0.0376628	
      0.217571	0.0193867	0.0377374	
      0.217564	0.0194556	0.0378036	
      0.217557	0.0195167	0.0378623	
      0.217552	0.0195705	0.037914	
      0.217547	0.019618	0.0379596	
      0.217542	0.0196597	0.0379997	
      0.217538	0.0196962	0.0380347	
      0.217535	0.0197281	0.0380654	
      0.217532	0.0197559	0.0380921	
      0.21753	0.0197801	0.0381153	
      0.217527	0.0198012	0.0381356	
      0.217525	0.0198196	0.0381533	
      0.217524	0.0198357	0.0381687	
      0.217522	0.0198498	0.0381821	
      0.217521	0.019864	0.0381938	
      0.217519	0.0198796	0.0382039	
      0.217518	0.019897	0.0382127	
      0.217516	0.0199183	0.0382205	
      0.217511	0.0199664	0.0382273	
      0.217507	0.0200146	0.0382205	
      0.217505	0.0200358	0.0382127	
      0.217503	0.0200533	0.0382039	
      0.217502	0.0200688	0.0381938	
      # section 3
      XYZ
      +99
      0.251068	-0.0250123	0.00642899	
      0.251064	-0.0250204	0.00644106	
      0.25106	-0.0250273	0.00645487	
      0.251055	-0.0250325	0.00647077	
      0.25105	-0.0250354	0.00648901	
      0.251044	-0.0250351	0.00650991	
      0.251039	-0.02503	0.00653394	
      0.251033	-0.0250168	0.00656142	
      0.251027	-0.0249876	0.00659284	
      0.251024	-0.0249273	0.00662865	
      0.25102	-0.0248566	0.00666932	
      0.251016	-0.0247766	0.00671539	
      0.251011	-0.0246862	0.00676743	
      0.251006	-0.0245844	0.00682603	
      0.251	-0.02447	0.00689184	
      0.250993	-0.0243419	0.00696557	
      0.250985	-0.0241987	0.00704804	
      0.250976	-0.0240475	0.00713503	
      0.250967	-0.0238797	0.00723155	
      0.250956	-0.0236939	0.00733848	
      0.250944	-0.0234884	0.00745676	
      0.25093	-0.0232613	0.00758744	
      0.250915	-0.0230106	0.00773168	
      0.250897	-0.0227341	0.0078907	
      0.250877	-0.0224127	0.00807538	
      0.250853	-0.0220564	0.00827987	
      0.250827	-0.0216606	0.00850645	
      0.250796	-0.0212198	0.0087578	
      0.250762	-0.0207276	0.00903716	
      0.250722	-0.0201762	0.00934853	
      0.250676	-0.0195583	0.00969644	
      0.250623	-0.018872	0.0100834	
      0.250558	-0.0180832	0.0105304	
      0.250484	-0.0172167	0.011022	
      0.250399	-0.0162526	0.0115627	
      0.250302	-0.0151755	0.0121573	
      0.250189	-0.0139956	0.0128113	
      0.250058	-0.0127184	0.0135307	
      0.249907	-0.0112921	0.0143219	
      0.249732	-0.00968576	0.0151922	
      0.249527	-0.0079398	0.0161493	
      0.249286	-0.00599318	0.0172017	
      0.249003	-0.00381508	0.0183589	
      0.248667	-0.00141637	0.019631	
      0.248305	0.000973856	0.0209022	
      0.247918	0.0033137	0.0221728	
      0.247544	0.00554123	0.0233276	
      0.247186	0.00761649	0.0243776	
      0.24685	0.00937261	0.0253325	
      0.246542	0.0108178	0.0262008	
      0.246255	0.0121657	0.0269907	
      0.245987	0.0134319	0.0277093	
      0.24574	0.0145632	0.0283629	
      0.245514	0.0155557	0.0289576	
      0.24531	0.0164269	0.0294987	
      0.245124	0.0171942	0.029991	
      0.244956	0.0178748	0.0304389	
      0.24481	0.0184539	0.0308267	
      0.24468	0.0189687	0.0311756	
      0.244563	0.0194255	0.0314879	
      0.244458	0.0198325	0.0317683	
      0.244364	0.0201964	0.0320206	
      0.24428	0.0205228	0.0322481	
      0.244203	0.020816	0.0324535	
      0.244135	0.0210798	0.032639	
      0.244076	0.0213062	0.0327988	
      0.244022	0.0215111	0.0329438	
      0.243973	0.0216963	0.0330751	
      0.243929	0.0218636	0.033194	
      0.24389	0.0220145	0.0333015	
      0.243854	0.0221506	0.0333986	
      0.243822	0.0222731	0.033486	
      0.243793	0.0223832	0.0335648	
      0.243765	0.0224874	0.0336393	
      0.243741	0.0225803	0.0337059	
      0.243719	0.0226629	0.0337651	
      0.2437	0.0227363	0.0338177	
      0.243682	0.0228012	0.0338644	
      0.243667	0.0228585	0.0339055	
      0.243654	0.022909	0.0339418	
      0.243642	0.0229533	0.0339736	
      0.243632	0.0229921	0.0340015	
      0.243623	0.0230259	0.0340258	
      0.243615	0.0230555	0.0340471	
      0.243609	0.0230812	0.0340656	
      0.243603	0.0231036	0.0340817	
      0.243597	0.0231231	0.0340958	
      0.243593	0.0231402	0.034108	
      0.243589	0.023155	0.0341187	
      0.243586	0.0231679	0.034128	
      0.243583	0.0231799	0.034136	
      0.24358	0.0231934	0.0341431	
      0.243577	0.02321	0.0341492	
      0.243572	0.023248	0.0341546	
      0.243569	0.0232861	0.0341492	
      0.243569	0.0233031	0.0341431	
      0.243569	0.0233169	0.034136	
      0.24357	0.0233293	0.034128	
      0.243571	0.0233406	0.0341187	
    NI_END   NIBLADEGEOMETRY
  NI_END   NIBLADE
NI_END   NIROW
NI_END GEOMTURBO
 
NI_BEGIN GEOMETRY
NI_END   GEOMETRY

Icon Bar


FIGURE 23 Interface buttons
The icon bar (FIGURE 23) is a collection of accelerators. This means that all buttons allow quick access to dialog boxes or operations that are already available in the menu bar.

The first three buttons (1) allow quick access to the usual file management operations.
The next four accelerators (2) control the undo and redo stacks.
The next group of buttons (3) are shortcuts to some of the geometry commands.
The view management group consists of two selectors (4), which allows to change blade and section in views.

File management buttons










New file


Accelerator to File\New
Creates a new parametric model on disk







Open file


Accelerator for File\Open
Opens an existing parametric model from disk







Save file


Accelerator for File\Save
Saves the current parametric model to disk




Edition buttons










Undo change


Accelerator for Edit\Undo
Undoes the latest change or undoes the selected change







Redo change


Accelerator for Edit\Redo
Redoes the last undone change or redoes the selected undone change







Name of current step


Show the name of the current design step







Checked button


If the button is checked, the current design step will be saved in the project




Geometry buttons










Import model


Accelerator for Geometry\Import
Opens the import model dialog (see Import section)







Parameter list


Accelerator for Geometry\Parameterlist
Opens the full list of parameters defining the current model (see Parameter List)







AutoBlade™ messages


Accelerator for Analysis\Showmessages
Opens or restores the message dialog (see Show messages)




View management buttons










Blade selector


Selector for the blade choice when one or more splitters are defined. This only affects the lower views (camber curve, side curves and thickness laws)







Section selector


Selector for the primary section choice. This changes the lower views and the blade-to-blade view

Quick Access Pad
The Quick Access Pad is located in the left part of the GUI. It contains icons and more evolved options providing a fast access to the more used functions of AutoBlade™. Some of these functions are only accessible through the Quick Access Pad whereas others are also accessible through the menu bar, so that their description will be referenced to these menus.
The pad is divided into three subpads, each of which can be toggled by a simple mouse left-click:

Target Settings
Model Editor
Fitting Control

All the commands and options accessible with these subpads are described in detail in this section. The three subpads are composed of pages containing buttons, icons, input areas. The icons perform specific function related to the subpad and the page. Each page can also be toggled by a simple mouse left-click.
The subpads Target Settings and Fitting Control only appear in the interface when the fittings license feature is detected.

Suction & Pressure Side Curves
This section allows the user to define the pressure and suction sides of the main blade. AutoBlade™ assumes that the suction side is located above the pressure side when plotted against an increasing θ angle.


FIGURE 45 Construction modes for side curves
These topological choices are described in the following order:

independent suction and pressure sides (legacy - default),
independent suction and pressure sides (regular),
independent suction and pressure sides (throat-based),
thickness addition (symmetric or not).

Suction & Pressure Sides Construction Mode - legacy
Both suction and pressure sides are constructed in the form of a high degree Bezier curve with respect to the camber curve. Special treatments are performed to shape the leading and trailing edges. This method is dedicated to axial turbines and axial compressors and is enabled through the Construction curves option.
This construction mode is neither compatible with (m,β) nor (,θ) planes, where angles are involved. This limitation comes from the need for the side curves to be entirely defined in a dimensional construction plane.


FIGURE 46 Topology menu for independent suction and pressure sides mode
The side curves are defined by a Bezier curve starting at the previously defined leading edge and ending just before the trailing edge. The trailing edge is shaped with a circular arc in the rounded case.
The construction of the suction side is depicted in FIGURE 47. The location of the Bezier control points is determined as follows, in a rounded trailing edge case. Pressure side and blunt edge cases will then be discussed.


FIGURE 47 Definition of the suction side curve

First, intermediate construction points are defined on the camber curve. The camber curve is divided into a fixed number of intervals which can be of equal or variable length using a stretching factor.
From each of these intermediate control points, a fractional length TSS(j) is added perpendicularly to the camber curve. This defines the position of the Bezier control points for the side curve. Each TSS(j) is defined as a fraction relatively to chord length instead of meridional chord (conversion is ensured for full backward compatibility with AutoBlade™ 2.1).
A special treatment is performed at the leading edge. The first Bezier control point coincides with the leading edge point and the position of the second control point is determined by the following two conditions:

the suction side curve must start perpendicularly to the camber line,
the curvature radius RLE must be matched at the leading edge.


FIGURE 48 Construction of leading and trailing edges (rounded case). 11 control points and 7 user defined parameters are used.
Taking into account the well known properties of Bezier curves, the locations of the first two control points are constrained as follows (FIGURE 48):
The first condition imposes that the second control point lies along a line perpendicular to the camber curve at leading edge point.
The second condition fixes the first control segment length as:



where RLE is the imposed curvature radius, n the amount of control points (n=11 in our example) and b the distance between the point defined by TSS(1) and the first control segment. In this formula, only the radius RLE is user defined since n and b depend on the chosen number of intermediate control points and the stretching factor.

A special treatment is also performed at the trailing edge. To obtain the proper rounded shape (case of FIGURE 48), two parameters are imposed by the designer: radius RTE and wedge angle δte. The locations of the last two control points Cn-1 and Cn are constrained to meet both continuity and the prescribed curve angle, just before the ending arc:

The end point is common to Bezier curve and circle arc to ensure continuity of order 0.
Building the last control segment tilted by half the wedge angle δte over the camber curve and tangent to the circle ensures the right ending angle and the first derivative continuity. The previous control point is thus defined as the intersection between the perpendicular line from point 8 in our example and the last control segment direction.


In order to determine the amount of control points n, a simple relation can be established, where the number of intermediate control points can be any integer greater or equal to zero:
n = 4 + number of intermediate control points
Our example (FIGURE 47) shows the curve obtained for order 10 (n=11) using 7 intermediate control points and a stretching factor of 1.1. Ten parameters are needed: the fractional offsets TSS(1) to TSS(7), the curvature radii RLE and RTE and the prescribed wedge angle δte.
This method allows the generation of suction and pressure sides that are highly continuous in the leading edge region. The use of Bezier curves avoids pressure discontinuities along the blade walls that could lead to boundary layer distortion or even separation. This is the reason why a circle or an ellipse is not used to shape the leading edge. A circular arc for instance cannot ensure the continuity of the high derivatives at its junction point with the Bezier curve, although the latter offers continuity up to the derivative (n-1). This remark is not critical at trailing edge where a circular arc is used.
TABLE 5 summarizes the settings and parameters defining the side curves.
TABLE 5 2D blade profile definition (rounded case)






Setting


Description






number of intermediate control points


amount of intermediate offsets to add between leading and trailing edges - amounts may differ for suction and pressure sides.




stretching factor


ratio of two successive offset gaps from leading edge to trailing edge along the camber curve - values may differ for suction and pressure sides. A stretching factor of 1 will give uniform intervals while a factor bigger than 1 will result in increasing intervals from leading to trailing edge




Parameter


Description




S(i)_LE_RADIUS


prescribed leading edge curvature radius RLE




S(i)_TE_RADIUS


prescribed trailing edge radius RTE




S(i)_TE_WEDGE_ANGLE


prescribed wedge angle δte




S(i)_TSS_(j)


Suction side intermediate offset TSS(j) for section (i)




S(i)_TPS_(k)


Pressure side intermediate offset TPS(k) for section (i)




Pressure side curve
Pressure side definition shares the same three parameters RLE, RTE and δte with suction side but all other settings or parameters - amount of intermediate control points, stretching factor and fractional offsets TPS(k) - are specific and may be different from the suction side.


FIGURE 49 Definition of the side curves (view 4)
Blunt cases
If a blunt trailing edge is requested, the Bezier curve is computed the same way, but no circular arc is built. Two types of blunts are available (FIGURE 50):

the normal blunt (FIGURE 50, left) is obtained by applying the RTE parameter perpendicularly to the camber curve as an offset, so the location of the last control point differs slightly from the rounded case.
the constant m' blunt (FIGURE 50, right) is obtained from the normal blunt case above. The side is then truncated or extended linearly so that the ending  value for the side is the same as the trailing edge point. If the construction plane is (,θ), the endpoints of the side curves and the camber curve obviously share the same abscissa.

The number of intermediate control points expression is still applicable for a blunt trailing edge.


FIGURE 50 Normal (left) and tangential (right) blunt cases - sections are here plotted in (, θ) construction plane

Required Licenses
The AutoBlade™ modeller module requires the AutoBlade™ license. That allows to create a parametric representation of a 3D turbomachinery blade starting from a template or an already existing parametric representation.
The AutoBlade™ Fitting module requires the AutoBlade™ Fitting license. That allows to create a parametric representation of a 3D turbomachinery blade from a points representation (in geomTurbo format).
The AutoBlade™ solid body module requires the AutoBlade™ solid domain license. That allows to create a Solid Body.
The run mode selection list in FINE™/Design3D environment displays only the run modes for which a license is available.

Stacking Point
Seven choices are available for the stacking point: leading edge (LE), trailing edge (TE), centre of gravity (CG), maximum thickness (MT), centre of channel (CC), on camber (CA) and on chord (CH) as depicted in FIGURE 23.
The centre of gravity is computed as the geometrical centre of the blade section in its construction plane (see Camber Curve Definition for details on this plane).
Point of maximum thickness is the point on the blade section mean line for which the maximum thickness is found. The mean line can be defined as the average curve dividing the blade section in such a way that the distances from one of its point to suction and pressure sides in the perpendicular direction are the same.
The centre of channel is the point, halfway between two successive blades, where the minimum channel width is achieved. For further details about the channel computation see also Sampling. This stacking point is only meaningful for axial machines.
A relative position of the stacking point is specified when defined on camber or on chord.
Centre of gravity, maximum thickness and centre of channel should be selected for axial or nearly axial machines only.
When the leading edge or trailing edge is blunt, the stacking point is the mean point of the side edge points.

Overlays
Optional overlays allow the display of one or more saved states of the model in the graphical views. This option allows comparison of the current state of the model with one or more reference states.


FIGURE 44 Overlay in the camber view
To quick insert the current state of the model as an overlay, select the menu View/Quick insert overlay. The state is immediately added to all views in a different color, but will only appear when the model is edited since the two states are initially identical. All views are affected, but the 3D view only shows a single instance of the wireframe model for each blade.
FIGURE 44 illustrates the comparison of the camber curve with a previous state that appears in another color. It is possible to add up to five states in the graphical interface. 
Overlays are persistent in a parametric model. This means that overlays are linked to a state saved on disk and available after reload of the project. Overlays can be removed  all at once by the menu  View/Remove all overlays.
The menu View/Overlay manager... provides advanced control of overlays. With the overlay manager, the user can add the current model as an overlay, or add a parametric model from file as an overlay. The new overlay can be added before or after the selected overlay. A name (Overlay name)can also be specified for the added overlay. Click on the button Insert will add a new overlay in the list shown in the following figure.
For each added overlay, the user may edit its color shown in the graphical interface by left-clicking on the color. The user can also remove the overlay by clicking on the button Remove next to the name of the overlay.

Import parameters
The menu Geometry/Import parameters allows to import a parameter file with default extension ".param" and modifies the parameters defining the current model. Each line in the .param file defines one parameter with the name and the expression (or the value) of the parameter. The user can make this .param file manually or modify the exported .param file, see Export parameters section. For example, importing the following file will set the parameter HUB_Z1 = -0.03 and set the parameter SHROUD_R2= "SHROUD_R1" (expression).


All the lines in the .param file starting with # will be considered as comment lines.

Meridional Contours
Both hub and shroud endwalls are assumed to be axisymmetric surfaces, so the corresponding surfaces can be defined by two curves in the (Z,R) plane, where Z and R are the axial and radial directions respectively. The meridional contours always appear in the upper left view.
Each meridional contour can be defined using seven different methods to allow the designer as much control as possible (FIGURE 2):

B-spline,
Bezier,
Line-Bezier-Line,
Line-Spline-Line,
User-defined,
composite,
Bezier 4.



FIGURE 2 Endwalls definition menu
A single curve definition is used to define the complete streamwise extent of each contour, except for the composite curve, that allow the use of an arbitrary amount of elements linked to each other with optional tangency constraints.
B-spline curve


FIGURE 3 B-spline curve
This method uses a B-spline curve defined by n nodes. The main difference with Bezier curves is that the resulting curve is a piecewise continuous interpolation of the defining points: the curve passes through all prescribed points and offers continuity up to the second derivative. This curve type is especially useful in the case the user wishes the contour to pass through one or more known coordinates, but the resulting curve exhibits less smoothness than its Bezier counterpart.






Parameter


Description






HUB_Z(i)


Z coordinate of the (i)th node of hub curve




HUB_R(i)


R coordinate of the (i)th node of hub curve




SHROUD_Z(i)


Z coordinate of the (i)th node of shroud curve




SHROUD_R(i)


R coordinate of the (i)th node of shroud curve




Bezier curve


FIGURE 4 Bezier curve
A Bezier curve defined by n control points only passes through its first and last control points. Among other properties, its first derivative at both ends is the direction of the first and last control polygon segments. This produces a smooth curve well defined at ends, but provides the user with indirect control through the use of the intermediate control points.






Parameter


Description






HUB_Z(i)


Z coordinate of the (i)th control point from hub curve




HUB_R(i)


R coordinate of the (i)th control point from hub curve




SHROUD_Z(i)


Z coordinate of the (i)th control point from shroud curve




SHROUD_R(i)


R coordinate of the (i)th control point from shroud curve




Composite line-Bezier-line curve


FIGURE 5 Composite Line-Bezier-Line curve
This curve offers the same properties as a Bezier curve plus optional straight line segments at one or both ends. Both end points are defined in the usual way and at least six additional parameters completes the curve description: the direction and length of the optional end segment at both ends and the length of the first and last control segments of the Bezier curve.






Parameter (hub curve)


Description






HUB_Z1


Z coordinate of the first endpoint




HUB_R1


R coordinate of the first endpoint




HUB_Z2


Z coordinate of the second endpoint




HUB_R2


R coordinate of the second endpoint




HUB_BETA1


angle of the starting segment above Z axis (in degree)




HUB_BETA2


angle of the ending segment above Z axis (in degree)




HUB_L1


length of the starting straight line segment




HUB_L2


length of the ending straight line segment




HUB_D1


length of the starting straight line segment




HUB_D2


length of the ending straight line segment




HUB_ADD_Z(i)


Z coordinate of the (i)th additional node of the Bezier part




HUB_ADD_R(i)


R coordinate of the (i)th additional node of the Bezier part




Similar parameters exist for the shroud endwall




The default curve requires thus ten parameters and provides a third order Bezier curve. If required, additional control points can be added at the cost of two additional parameters per control point.
Composite line-Spline-line curve


FIGURE 6 Line-Spline-Line curve
This curve offers the same properties as a B-spline curve plus optional straight line segments at one or both ends. Both end points are defined in the usual way and at least four additional parameters completes the curve description: the direction and length of the optional end segment at both ends and the length of the first and last control segments of the B-spline curve.






Parameter (hub curve)


Description






HUB_Z1


Z coordinate of the first endpoint




HUB_R1


R coordinate of the first endpoint




HUB_Z2


Z coordinate of the second endpoint




HUB_R2


R coordinate of the second endpoint




HUB_BETA1


angle of the starting segment above Z axis (in degree)




HUB_BETA2


angle of the ending segment above Z axis (in degree)




HUB_L1


length of the starting straight line segment




HUB_L2


length of the ending straight line segment




HUB_ADD_Z(i)


Z coordinate of the (i)th additional node of the Bezier part




HUB_ADD_R(i)


R coordinate of the (i)th additional node of the Bezier part




Similar parameters exist for the shroud endwall




The default curve requires thus eight parameters and provides a third order B-spline curve. If required, additional control points can be added at the cost of two additional parameters per control point.
User-defined curve
A special type allowing a curve free of parameters can be selected. It requires a list of points in the meridional plane and an interpolation law. The endwall is thus a linear or spline interpolated curve passing through user-defined points.
A dialog box allows the designer to enter the nodes using a simple text formatted file carrying a ".dat" extension. At least two nodes must exist and the content must comply with the following format. Points are numbered from inlet to outlet.
TABLE 1 File format for a parameterless endwall curve





Rules
Sample





n (unsigned integer, number of points)
Z1 R1 (two space separated floating point numbers)
...
Zn Rn


5
0.0 0.15
0.05 0.15
0.1 0.14
0.15 0.13
0.2 0.13




Although the curve is parameterless (no parameters appear in the Parameter list), it can be edited like any other curve in the meridional view.
Once the file has been read, it may be deleted since all data is saved in the parametric file.
Composite curve
For complex contours, a special composite curve can be defined with an arbitrary amount of elements of different types. Those elements are linked to each other to ensure continuity. Optionally, they can be constrained to fulfil the continuity of the tangency.


FIGURE 7 Composite hub curve
Any of the following curves can be added and removed in any order:

a Bezier curve defined by n control points,
a B-spline curve defined by n nodes,
a C-spline curve defined by n nodes,
a linear segment,
a user-defined curve.
a circular arc

Buttons Add and Insert allow to respectively add an element at the end and the beginning of the list. An existing element may also be split.
The slope continuity is not ensured for composite curve.
Selecting an element then allows to modify its settings like the type, the amount of parameters (Bezier and spline elements) or the related external data file (user-defined element), as illustrated in FIGURE 7.
Tangency constraint is also possible at start or end of an element for most types, but is undefined between a linear and a user-defined elements. Checking a tangency constraint will automatically increase the amount of nodes (spline curves) or control points (Bezier curves) as needed.
Each element, once selected, can be edited in the Curve parameters area of the menu (bottom area in FIGURE 7).






Parameter


Description






HUB_Z(i)


Z coordinate of the (i)th node of hub curve




HUB_R(i)


R coordinate of the (i)th node of hub curve




SHROUD_Z(i)


Z coordinate of the (i)th node of shroud curve




SHROUD_R(i)


R coordinate of the (i)th node of shroud curve




In the interface, the composite curve can be edited as a whole: any control point or node can be picked and moved.
Third order Bezier curve


FIGURE 8 Bezier 4 curve
This 3rd order degree Bezier curve is controlled by eight parameters, namely positions at both ends, length and angular direction of the first and last control segments. These parameters define the location of the four nodes controlling the curve.






Parameter (hub curve)


Description






HUB_Z1


Z coordinate of the first endpoint




HUB_R1


R coordinate of the first endpoint




HUB_ALPHA1


angle of the first control segment above Z axis (in degree)




HUB_L1


length of the first control segment




HUB_Z2


Z coordinate of the second endpoint




HUB_R2


R coordinate of the second endpoint




HUB_ALPHA2


angle of the last control segment above Z axis (in degree)




HUB_L2


length of the last control segment




Similar parameters exist for the shroud endwall

View Menu
Six groups of commands are offered:

the selection for the upper right view: Blade 2 blade view, Sweep law, Lean law or 3D model. Alternative buttons exist in the main button bar (see View Layout & Graphs for details).
customize layout of AutoBlad™. When designing a blade, the user may open few geometry analysis windows to monitor the status of the designed blade. These layout settings can be exported to a file. When creating a new design, the user may import the saved layout to retrieve all the settings.
Import layout ..., allows to import a layout file from a previously saved layout. The user may copy the saved layout to Installation_path\autoblade(Undefined variable: Versions.turboVersinoCmd)\bin\templates (on Windows) or Installation_path/autoblade(Undefined variable: Versions.turboVersinoCmd)/COMMON/templates/ (on Linux) and use it as a template.


Some layout settings might be incompatible with the current model, such as the section or blade number. AutoBlade™ will update the choices to the closest valid possibility if any, but no warning or errors are generated.
Export layout, allows to export the current layout to a specified file.
the management, insertion and removal of optional overlays allowing the comparison of several states of the model being edited (see Overlays for details).
the properties for Blade-to-blade view options and 3D view options.
Save screen shot: allow to save a capture of the active views. The pictures are saved in png format. If the four views are active (multiple view), all four views are saved to disk in separate files. If a single view is active (full view), only that view is exported.
The command Save screen shot is only available in interactive mode.
The saved pictures do not show labels for view and the name of axis.


Show stream grid: allow to show the grid in meridional view when the stream surfaces type "Hub to shroud custom interpolation" is used. Show parameter bounds, scale, expressions and type: the command enables or disables the bounds, scale, expression and type of the parameters in all menus.

Method 'across channel'
If the internal limits of the extensions are the start and end of the blade channel, the domain is defined by three areas where the middle part is always located in the blade passage. Those limits are approximate segments stretched between the mean lines and entering into the blade sections.
The first method builds cuts in the blade channel area only (see FIGURE 80). The start and end cuts are located by the designer and become the links between the inlet, outlet and perturbed channel areas. Additional cuts can be defined in arbitrary amount between those two limits.


FIGURE 80 Cuts are defined across the blade channel
By default, the cuts are perpendicular to the channel line. But a special angular deviation can be applied for each cut as an additional parameter. All angular deviations are measured in degree from the normal direction along the mean channel line. In case of intersection between cuts, the generation of the patch will fail, and AutoBlade™ will issue a message.


FIGURE 81 Cuts are defined across the blade channel






Parameter


Description






HUB_CUT(i)_ANG_DEV
                        
HUB_START_ANG_DEV
HUB_END_ANG_DEV
                        


Angular deviations of the cut i in the 'cut across' method.
                        




Internal Cuts
For every internal cut, a perturbation law is defined by mean of a Bezier curve or a cubic spline controlled by height parameters. This law is then defined in (S,h) plane where S stands for the natural parameter of the cut in (m',θ) plane and h is the dimensional height of the perturbation (FIGURE 82).


FIGURE 82 Perturbation law for 'across' method
No continuity constraint is necessary as long as the resulting endwall completely intersects the blade because the discontinuity has no effect on the mesh generated from a geomTurbo output.
The number of parameters is free and an optional stretching factor allows to concentrate more control points near one end.
Start & End Cuts
The first and last cuts can be freely placed in the blade channel, but are parameterless in order to reach at least C0 continuity. 
Final Surface
The final perturbed patch is a loft surface passing through the perturbed cuts (loft profiles) and two guide curves defined by splines from start to end cuts. The loft profiles are generated from the cuts on the revolved hub by addition of the perturbation heights defined earlier.


FIGURE 83 The complete perturbed surface for 'across' method
The perturbations are applied in the normal direction to the revolved hub (radial direction for a cylindrical reference hub).
G1 continuity can be enforced with inlet and outlet patches by means of clamped ends conditions on spline guides. Therefore, this continuity is only strictly ensured at ends of the start and end cuts.






Parameter


Description






HUB_CUT(i)_H(j)
                        
SHROUD_CUT(i)_H(j)
                        


Height value of control point j of the cut i, as a 3D distance

Fitting Problems
The fitted solution is globally improved, but some edge radii got worse
The fitting process is a global optimization, which tries to minimize the error of the shape for every section. Since the trailing edge is often a small detail when compared to a whole section, the fitting process may find a set of values for parameters that allow a better error estimate for the section and for which the quality of the shape is decreased.
Edge radii are usually precisely estimated by the initialization process. Therefore, freezing the corresponding parameters will ensure a satisfying edge shape (especially the trailing edge).
The initialized model is not very close to the target geometry

If an error has been generated, this means that some topology settings are probably not suitable or the amount of defining parameters is insufficient.
If no error is generated, then the solution monitor should provide some clues about what went wrong (see Visual Check for examples).

The fitting process cannot improve the solution and the value of parameters do not change any more
If some bounds are reached, moving these bounds should allow further fitting.
If no critical bound is reached, the model may converge to a solution not close enough because the topology settings are not optimal. Adding some more parameters in the definition of the curves should help, but could significantly increase the complexity of the model. In such situations, switching to another camber curve type or construction mode may allow better results (see Setup Initial Model for advice).

Export as Parasolid
The menu Geometry/Export as Parasolid...  opens a file chooser and prompts for a location where to save the blade geometry in Parasolid format as independent sheet bodies.
If a solid body is requested, the user can check the Solid model option under the Parasolid tab in the File/Properties... menu. The blades will be exported as closed volumes instead of open sheets.

Stream Surfaces & Spanwise Location
This second step menu defines the stream surface type, the rulings and the spanwise location of their traces in the meridional plane (FIGURE 9). The primary sections are defined on these stream surfaces which should therefore be defined before the blade sections.


FIGURE 9 Setup of the stream surfaces

Stream Surfaces Spanwise Location
Two types of parametric blade sections are available and can be used simultaneously: primary and parametric 2D sections. For each section, a supporting stream surface is defined by interpolation or extrapolation of the reference traces defined above.
Number and spanwise position of both types of sections can be input by the user. Spanwise locations usually range from 0.0 (hub) to 1.0 (shroud), but values between -0.5 to 1.5 are accepted by the modeller.


FIGURE 21 The spanwise location of the stream surfaces
Primary Sections
Primary sections are the defining 2D sections of the blades. All primary sections within a given project are described by the same set of parameters such as a camber stagger angle, a prescribed thickness distribution, leading edge radius, etc. These sections share common topological settings but the values of the involved parameters vary independently from one section to another. 
Parametric Sections
Parametric sections are computed by interpolation or extrapolation of the primary sections parameters. All parameter values are automatically generated with the help of the span parameter and values of the corresponding parameter for the primary sections. Interpolation laws are explained in the next paragraph. The purpose of the parametric sections is to refine the output data transferred to the mesh generator. This is for instance essential in case an optimization of the stacking laws is performed whereas the blade shape is defined by means of a limited number of primary sections.
Parametric sections are optional, except when only one primary section is defined. In this particular case, a constant extrapolation applies for all section specific parameters.
The use of parametric sections can lead to invalid blades in optimization projects. It is generally a good idea to discard them (or to use polyline instead of spline interpolation) when parameters are allowed to vary over a large range, because some unrealistic values of the parameters (such as negative leading edge radius) may result from the interpolation process!
Parameter Interpolation
Each primary blade section is defined by a set of parameters. The value of every parameters on every primary sections is defined by user input, but the value of the corresponding parameter on any parametric section is interpolated. The preferred interpolation type is selected by means of the two buttons:

Polyline

Cubic spline


FIGURE 22 assumes that four primary sections are defined at spanwise locations {0, 0.3, 0.7, 1} and two parametric sections at spanwise locations {0.5, 1.2}. If the parameter is the stagger angle for instance, the angular value of this parameter is precisely defined for each primary section and the value of the stagger angle can be seen as a function of the spanwise location. Therefore, a spline (or a polyline) can be built through the points (span value, parameter value) from every spanwise location of the set. The value of the stagger angle of the first parametric section is interpolated from this curve: to the given value 0.5 of the span parameter corresponds one value of the stagger angle.


FIGURE 22 Interpolation laws (cubic spline and polyline)
According to the number of primary sections, interpolation laws behave differently:

if only one primary section is defined, all parametric sections will have identical defining parameters whatever interpolation type is selected: this is the constant interpolation case.
if only two primary sections are defined, values are interpolated with the help of a linear law whatever interpolation type is selected. Extrapolation is also linear.
if three or more primary sections are used, interpolation differs according to the type selected. Extrapolation is always linear below 0 and above span 1, so that the interpolation curve remains continuous up to the first derivative at span 0 and 1. This case is depicted in FIGURE 22.

At least two primary sections are usually required. A special case with one primary and one parametric section exists to allow constant blade profiles.
Spanwise location differences among primary and parametric sections should be more than the built-in tolerance or AutoBlade™ will discard duplicate values automatically. The smallest valid difference between two span values is 0.01.
As explained in the Export Options, discretized sections are direct interpolations of point coordinates from primary and parametric sections. Hence those sections do not need a supporting surface.

Views
Stream surfaces are shown in the meridional view (upper left viewport) for primary sections only, but are defined for parametric sections too. The location of the parametric sections can be noticed in the 3D View of the blade.

Graphical User Interface

This chapter describes the AutoBlade™ interface, a powerful and interactive interface for three-dimensional turbomachinary blade designs. The AutoBlade™ interface offering

interactive control of the parameters defining the model (point drag and keyboard input),
full undo/redo capability on operations,
multiple overlays to compare the edited geometry to one or previous states,
advanced error reporting

In the following sections, the items in the interface are described in more detail.
Axis Conventions
Axis names and conventions are summarized in this section.
The XYZ axis system is positively oriented such that the rotation axis of the machinery is the Z-axis (FIGURE 1). The azimuthal angle θ is measured from the positive X axis and expressed in radians.


FIGURE 1 Axes and conventions in AutoBlade™
The meridional plane (Z,R) for the definition of hub, shroud and traces of the stream surfaces corresponds to (Z,X) plane. The meridional length m of endwall curves and traces is often used as abscissa for the location and the construction of the blade sections (see Meridional Location).
The tangential plane is (X,Y), but (span,θ) plane is used for the tangential stacking (see Tangential Position).
TABLE 1 Axis conventions and special coordinates






Name


Description






X


vertical radial direction (θ=0)




Y


horizontal radial direction (θ=π/2)




Z


axial direction




z


non dimensional axial length computed as (Z-ZRef)/(Rshroud(ZRef)-Rhub(ZRef)) where ZRef is the axial reference location for the blade sections




R


radius




r


non dimensional radius computed as (R-RRef)/(Zshroud(RRef)-Zhub(RRef)) where RRef is the reference radius for the meridional location of the blade sections




                        θ
                    

tangential angle measured from the positive X axis (in radians)




m


distance measured along a curve in the meridional (Z,R) plane and defined as the integral of 




m' or 


integral of  ()




span


spanwise location parameter - expressed as a fraction of the local distance between reference stream surface traces in the meridional (Z,R) plane




Units
No unit system is currently implemented inside AutoBlade™. In particular, no information about units is saved in the ".geomTurbo" file. Consistency is thus the ruling word. All angles in AutoBlade™ are measured in degrees unless differently stated.
There are however some exceptions:

Some lengths are normalized. This is the case of parameters like TSS(j) and TPS(k) (see FIGURE 38).
The angle θ is expressed in radians in the lean law graph and in the section view plane (view 3).

If AutoBlade™ is coupled with NUMECA flow solver, it is strongly recommended to express lengths in meters.
Leading and trailing edge radii are currently limited to values greater than 1e-6. A similar limit exists for the camber length.

Menu Bar
The menu bar of AutoBlade™ consists in 6 entries File, Edit, Geometry, Analysis, View and Modules (only available if AutoBlade™ is started from FINE™ GUI):



FIGURE 2 Menu bar

Special functions
The menu Geometry/Special functions allows the user to define his own functions. The user can specify a name (always in uppercase), the number of arguments and the corresponding formula using all previously defined functions, including existing user-defined functions.


FIGURE 19 User-defined functions editor

Analysis Menu
Most of the options available in this menu are also available as accelerated buttons (top button bar) or as side buttons (left tool box). This menu consists in three groups of commands:
Optional quantities
The menu Analysis / Optional quantities controls the computation of optional quantities and distributions depending on the geometric model. These options are detailed in the Optional Quantities section. 
Geometry analysis
The menu Analysis / Geometry analysis allows to access a geometry analysis tool, see Geometry Analysis for more details.
Parametric report
The menu Analysis / Parametric report aims at the description of the total number of parameter and the free, frozen and dependent parameters in order to ease the parameters and their dependencies analysis, see Parametric Report for more details.
Fitting graphs
The menu Analysis / Fitting graphs allows to access the graphical comparison analysis tool, see Fitting graphs for more details.
Fitting log file
The menu Analysis / Fitting log file allows to monitor the log file of the fitting process, see Fitting log file for more details.
Fitting convergence
The menu Analysis / Fitting convergence allows to monitor the convergence history of the fitting process, see Fitting Convergence for more details.
Fitting report
The menu Analysis / Fitting report allows to save all the parameters of the fitting process, the fitted model and the analysis results to a file, see Generate report for more details.
Fitting report hub / shroud
After an initialization or a fitting process, the menu Analysis / Fitting report hub or Fitting report shroud allows to compute the differences of the non axisymmetrical surfaces between the target and the fitted model. The distances are computed on directions built over a customized range with uniform sampling in both m and θ directions. All directions start from the rotation axis and are perpendicular to the revolved hub surface. For instance, in case of a cylindrical reference hub, the directions are all radial.


The choice for definition of the domain is one of the following:

full channel (automatic range in both m and θ directions, for full coverage),
partial channel (automatic θ range and user-defined m range),
user-defined square domain with custom ranges in both m and θ directions.

The sampling is always uniform, but the number of samples for each coordinate is free (maximum 500).


The processing may be long according to the number of samples and the results will be presented as statistics in the interface. When no intersection is found for a direction, the sample is dropped without error.
The statistical data consists in arithmetic and quadratic means and the standard deviation as well as minimum and maximum errors.
Further results are available by saving the report to file for further processing or archive purposes.

If the menu Report / Save summary is selected, the data contained is exported as well as an histogram to check the distribution of the error.
If the menu Report / Save all data is selected, an additional block containing all samples is exported.

Show messages 
A graphical console reflects all useful warning and error messages generated by AutoBlade™. It consists in a simple menu and a read-only text area (see FIGURE 21).
If the message list is full of old messages, the history can be cleared using the View/Clear command.


FIGURE 21 AutoBlade™ Message window
Three kinds of messages are issued:
Success
A success message is usually an update status after a topology or parameter change. It simply confirms that an operation is free of errors.
Warning
A warning is generated either when there is a potential risk of failure or when a correction has been automatically applied by AutoBlade™ to ensure compatibility.
This is the case when a parametric file from a previous release is loaded and converted or when a change in a step of the blade construction is incompatible with a setting from another step.
Error
When AutoBlade™ cannot update the model or needs to correct a value of some parameter, an error is generated.

In Design3D mode, errors prevent the complete saving of the project: the geomTurbo file is not updated until problems are solved.

Parameter List
The parameter list is accessible through the menu item Geometry/Parameter list or the corresponding button in the main tool bar.
This menu allows the designer to access the whole list of parameters defining the current model. Most parameters can be read and changed interactively in the graphical views. Furthermore, by clicking in the Expression entries (FIGURE 15), additional mathematical expressions allow some parameters to be defined as a function of one or more other parameters and help reduce the space of independent parameters. So this menu is especially useful for the advanced user who will be able to quickly modify several parameters. There are a few exceptions however that make this list necessary:


The bounds of the parameters can be checked and changed in the list. To show them, simply activate the option View/Show parameter bounds. This topic is useful in Design3D mode only.
The scale of the parameters can be checked in the list. To show it, simply activate the option View/Show parameter scale. This topic is useful in Design3D mode only.
The expression of the parameters can be checked and changed in the list. To show it, simply activate the option View/Show parameter expressions.
Some parameters do not appear in the graphics area. For instance, meridional chord parameters, edge radii in construction curves mode or the blade repetition number are only available in the Parameter list or in the topology menus.



FIGURE 15 Parameters menu
All parameters are listed in specific pages and depend on the chosen topological settings. The names of the parameters are listed in section of the AutoBlade™ Modeller chapter after the corresponding topology setting. To find information about a precise parameter name, please look for the parameter keyword in the index located at the end of this manual.
For a fast design process, it is suggested that all topological settings are fixed before editing their corresponding parametric values.
All the parameters have a double precision with about 16 decimal digits.
The next few paragraphs explain the additional functions available in any grid of parameters.
Expression - Dependency of Parameters
When checking the small button in front of an Expression entry, the corresponding parameter can be controlled by a mathematical expression in such a way that its value is defined as a function of one or more other parameters.
This new ability offers several advantages:

	design changes are easier since fewer parameters need to be changed,
	optimization is faster thanks to a reduced space of search (reduced amount of free parameters),
geometrical constraints are easier to express avoiding the definition of complex penalties in the objective function.

With the above features, AutoBlade™ will be able to support complex parametric dependencies, where a reduced list of independent parameters can be built. All dependent parameters are internally evaluated, so that the whole model can be built from this limited subset of independent parameters. This may help decrease the dimension of the parametric space in optimization and achieving special topological goals like

constant or incremental chord length for all primary sections,
identical radius at trailing edge,
symmetric thickness at both edges.

Enabling / Disabling Expression
When the Expression field is unchecked, the bounds are unlocked and may be edited.


When an expression is entered and activated, the value field becomes read-only and shows the last known evaluation of the expression.


The check button activates or deactivates each expression, allowing the designer to disable the expression and restore it later.This is especially useful in fitting projects.
User defined Parameters


FIGURE 16 User defined parameters
Additional parameters can be introduced under the group user(FIGURE 16) and can serve as reference for the dependencies. For instance, a reference length can be defined and used as factor in expressions for some dependent lengths in the model.
Here is an example using user defined parameters. Assuming that , , , and the user wants to define , the user can define an additional optional parameter X and make P2 dependent on P1, P3 and X:






In this case, P2 will follow X but is automatically bounded by P1 and P3.
Editing Expression
The expression editor (FIGURE 17) is invoked by right-clicking over the Expression field. The full lists of variables (parameters), constants, operators and functions allow the designer to enter and edit complex dependencies.
The parser is able to recognize the operators, grouping symbols and functions, but also numerical data (floating point) and names of variables.


FIGURE 17 Expression editor window
Expressions allow the following operators and functions:

	Arithmetic: +, -, *, /,^
Unary operators: +, -
Unary functions: abs, sin, cos, tan, sinh, cosh, tanh, asin, acos, atan, sqrt, log, log10, exp, round, trunc
Two arguments functions: atan2
Three arguments function: switch
Multiple arguments functions: min, max
Logical operators: &&, ||
Comparison operators: <, <=, >, >=,==,!= 
User-defined Functions


The precedence of the operators occurs in the following order of decreasing priority: 

	grouping parentheses and functions,
exponent ^,
	* and / ,
	+ and -.

Grouping symbols '(' and ')' are allowed to constrain associativity and precedence or to separate the arguments of a function from the rest of the expression. In case of multiple arguments, the comma is mandatory as separator.
Cyclic dependencies are not supported. For instance, the following system is not accepted by the solver of constraints because B is function of C but C is also a function of B:
A=1.0
B=D-C
C=A+B
D=2.0
User-defined Functions
The user interface allows the user to define special functions, see the Special functions section for more detail.
Export Parameters
The button Export group (at the bottom of the grid) allows to save on disk the group of parameters appearing in the corresponding window. A dialog box then prompts for a text file name.
Simple Use of Parameter Grid
Basic edition
To change a parameter value in the grid, simply edit the field to reflect the new value.
There is no need to key in <Return> or <Enter>: the model will not be updated unless Ok or Apply button is clicked.
If a value is set to an incorrect value, it will be corrected and a message will be issued. For instance, a radius cannot be negative, so a default epsilon will replace the wrong value.
Select, Copy, Paste
Some basic editing commands are provided to allow copy and paste of parameters. The simple example below shows how to copy values from a parameter to one or several other parameters.

To copy a parameter, place the mouse pointer over the label of the target parameter and right-click. Release the mouse over the Copy option to store the parameter to the internal memory.
Select the labels of the parameters to overwrite by means of the left mouse button and the <Ctrl> or <Shift> modifiers if necessary. All selected parameters will appear on a blue background for an easy check.
To paste the copied value to each parameter of the selection, simply right-click over any label and release the button over the Paste option.

Control of Parameters Bounds
In Fitting, Database Generation and Optimization modules, the value of the defining parameters is allowed to move within a user-defined range, limited by a lower and an upper bound. Those additional fields can be monitored in the grid of parameters by means of the option Geometry/Show bounds from the menu bar. When active, this option adds new fields and commands to the grids, as depicted in FIGURE 15.
The new fields are:

lower bound: the minimum allowed value for the parameter,
upper bound: the maximum allowed value for the parameter,
reference: a special value used as increment when moving the bounds.

Copy and Paste options behave exactly as explained above and include all four fields. 
Moving Bounds of Single Parameter or Selection
Bounds can be set manually, just like the value, but the variation range of specific parameters can also be enlarged or shrunk at once by right-clicking on the selected parameters.
The commands on the contextual menu apply to only the selected parameters.
The commands on the panel apply to all the listed parameters. If a filter is used, the commands will apply to the filtered parameters.


FIGURE 18 Commands for edition of a selection of parameters
New commands can be applied to the selection from the contextual menu:

Reset bounds: sets lower and upper bounds to the value of the parameter (freezes the value of the parameter),
Increase bounds: moves lower and upper bounds away from the value by a quantity equal to the reference value,
Decrease bounds: tightens both bounds by a quantity equal to the reference value.
Shift by a constant: shift lower and upper bounds by a specified constant.
Scale by a constant: scale the lower and upper bounds by a specified constant.

According to the location of the value with respect to its range of variation, the label of the parameter can appear in one among five colors:

black: the value is free to move in both directions within the specified range and does not reach any of its bounds,
yellow: the value is free to move in the specified range, but one of its bounds is reached,
orange: the value is frozen because its range has a zero length (both bounds are set to the value) or is ruled by an expression,
red: the current value is outside its allowed bounds. A correction is required.
pink: one of the field does not contain valid numeric input. If applied, the wrong field recovers the previous value.

Finally, three new commands also appear at the bottom of each parameter group to allow a quick control of the ranges of variation of all parameters at once.
Parameters should never appear in red color. This means the range of the involved parameter is wrong, possibly due to a typing error. This is not important in stand-alone mode.
Monitor parameter status
In Fitting, Database Generation and Optimization modules, the value of the defining parameters is allowed to move within a user-defined range, limited by a lower and an upper bound. 
Those additional fields can be monitored in the grid of parameters by means of the option View/Show parameter scale from the menu bar. When active, this option adds new field on the right side of the parameter list, as depicted in FIGURE 15.
According to the location of the value with respect to its range of variation, the label of the parameter can appear in one among colors:

green: the value is free to move in both directions within the specified range and does not reach any of its bounds,
yellow: the value is free to move in the specified range, but one of its bounds is reached,
orange: the value is frozen because its range has a zero length (both bounds are set to the value) or is ruled by an expression,
red: the current value is outside its allowed bounds. A correction is required.

Furthermore, a cursor shows the relative location of the parameter value compared to its bounds.

Target Settings subpad
This menu - the subpad Target Settings in the left area - grants access to the target settings for the fitting project. All these functions are only accessible through this subpad.


FIGURE 25 Target Settings subpad
Link target geometry



A geomTurbo file can be linked to the current project through the button . For more detail on how to prepare a target geomTurbo file, please refer to the Preparing Target Geometry section.
Remove target geometry



The button  allows to remove the geomTurbo file linked to the current project.
Build target sections from CAD geometry



If the geomTurbo file uses CAD import (more details in AutoGrid™ User Manual), the geomTurbo file can be linked to the current project, but requires a specific treatment to obtain sections before the initialization and fitting processes can be launched. The button  can be used to build the target sections from the CAD geometry. The operation alters the target file and archives the original target. 


FIGURE 26 Build blade sections from CAD surfaces
The Build tolerance is the precision used when building the sheet bodies of the CAD blades. The Sewing tolerance is the tolerance applied when sewing the CAD faces together. The default value of the sewing tolerance assumes an suitable scale (order of magnitude of the bounding box is at least 0.1 and at most 100) and good precision of the data.
These two tolerances can be modified when AutoBlade™ fails to generate blade sections from CAD surfaces. In such a case, a generic message is issued:
"Failed to build some sections. Please check error messages and retry"
Additional messages can be found in the log file. The two next messages are examples where those settings should be modified. However, the operation may fail later by producing strange or incomplete shapes for side curves, without any failure message.
"Failed to build the suction/pressure sheets for blade"
"Failed to sew the suction/pressure sheets for blade"
Generally speaking, the build tolerance should be increased in the first case and the sewing tolerance should be increased in the second case. When increased, it is advised to keep the smallest possible value for build tolerance. The sewing tolerance should never be larger than the smallest edge length in the CAD surfaces.
The option correct position of side curves allows to automatically correct the orientation of the target sections. This option is applied by default when building the sections.
Restore original CAD geometry



The button  allows to restore the original CAD target.
The operations Build sections from CAD  and restore CAD  directly change the target files stored on disk.
Edge point relocation



Edge points of the leading or trailing edge on the target can be altered for each section through the button , if the corresponding edge is rounded. The blade index refers to the blade number in the fitted row. It can be different from 1 in case of splitter blades.


The location is relative to the original position and expressed as a fraction of the profile length. It is positive in the counter-clockwise sense, negative in the other sense. If the check box all sections is selected, the relocation of the edge points will be applied for all sections. Edge point relocation affects the geometry loaded in memory, but does not alter the target geometry file.
Project target geometry on model stream surfaces



The button  allows to project the target curves on the stream surfaces of the parametric model. 
Other settings and target viewing
The option Row to fit allows to select the target row to fit (if several rows are defined). And an optional Scaling factor can be applied on the target geometry. 
The sampling of the target side curves and intermediate projection paths can be controlled for more precision (if increased) or to improve speed (if decreased) of the projection/fitting processes. 
In addition, the options Exchange sides  and Reverse orientation  allow respectively to set the suction side above the pressure side and to reverse the azimuthal orientation when necessary.
Both the target geometry and the projected target curves can be shown in the graphical view for comparison with the fitted geometry, which is controlled by the buttons Show target and Show projection, respectively. Two special colors can be reserved for the target geometry and the projected target curves in the graphical interface: orange for the target curves and surfaces, yellow for the projected target curves. These default colors can be changed in the menu File / Preferences.
Currently, three views can show the target curves and surfaces:

the meridional view for endwall curves (target and projected target),
the 3D view for blade surfaces (target only) or section curves (target and projected target). The 3D view shows target surfaces if the target is a CAD geometry. After building of the section curves, the resulting target curves are shown instead. The target data is shown without transformation except in those two cases:

if the scaling factor is set, the target geometry appears scaled,
in case of planar stream surfaces, the target blade is rotated to approximately match the alignment with plane (Z,Y).

the blade-to-blade view for curves (projected target only).

Spanwise Locations
Spanwise locations of the stream surfaces traces are controlled by the means of the span parameter. In the cylindrical case (FIGURE 19), two radius values are necessary to define the reference stream surface traces, one near the hub (Rhub) and another near the shroud (Rtip). Those two radii represent respectively the spanwise locations "0" and "1" and are usually chosen to mimic the hub and shroud curves.


FIGURE 19 The span parameter applied on cylindrical stream surfaces
As soon as the two reference surfaces are defined, any intermediate stream surface is obtained by interpolation of the reference traces radii using the span parameter, which is defined as a normalized location between the trace at hub (0.0) and the trace at tip (1.0).
For linear interpolation surfaces, intermediate stream surfaces are built using interpolation of points from start to end, as shown in FIGURE 20. The linear formula  is a generalization of the interpolation law for points in the meridional (Z,R) plane. This law is actually applicable to every stream surface type.





FIGURE 20 Application of the span parameter for interpolation of the stream surfaces
There is no direct link between endwall curves and planar, cylindrical or conical stream surfaces, so that none of the defining X, Z, R and α change after an endwall curve adjustment. On the contrary, hub to shroud interpolation surfaces are linked to the endwall curves and are updated automatically.

Viewing Control Buttons
The graphics layout use IGG™ toolbar for view all manipulations. The buttons appearing below the views can be used to control the view:
View selector



The view selector allows to cycle through view layouts. The icon changes slightly and indicates the selection corresponding to the next action. The cycle order is full upper left view, full bottom left view, full bottom right view, full upper right view and four views layout.
X, Y, and Z projections



Press the left mouse button to project the view on an X, Y or Z constant plane. If the same button is pressed more than one time, the horizontal axis sense changes at each press.
Coordinate axes



The coordinate axis button acts as a toggle to display the coordinate axis on the view.

A left click enables/disables the reference axes
A middle click enables/disables axes ticks
A right click has no effect in AutoBlade™.

Scrolling



This button is used to translate the contents of the view within the plane of the graphics window in the direction specified by the user. The following functions can be performed with the mouse buttons:

Left: press and drag the left mouse button to indicate the translation direction. The translation is proportional to the mouse displacement. Release the button when finished. The translation magnitude is automatically calculated by measuring the distance between the initial clicked point and the current position of the cursor.
Middle: press and drag the middle mouse button to indicate the translation direction. The translation is continuous in the indicated direction. Release the button when finished. The translation speed is automatically calculated by measuring the distance between the initial clicked point and the current position of the cursor.

3D viewing



This button allows to perform viewing operations directly in the graphics area. Allowed operations are 3D rotation, scrolling and zooming.
After having selected the option with the left mouse button, move the mouse to the active view, then:

Press and drag the left mouse button to perform a 3D rotation.
Press and drag the middle mouse button to perform a translation.
Press and drag the middle mouse button, while holding the <Shift> key, to perform a zoom.
To select the centre of rotation, hold the <Shift> key and press the left mouse button on a vertex of a curve or a surface. The view is immediately centred on the clicked entity which will act as the centre of rotation. Dragging the mouse will rotate the model.

To quit the option, right-click the button.
A <Shift> and left-click allow to select the centre of rotation in the 3D view if and only if show edges option is activated in the 3D view options dialog. Otherwise, the action is identical to a left-click.
Rotate about x, y or z axis



The rotation buttons are used to rotate graphical objects on the view around the X, Y or Z axis. The rotations are always performed around the centre of the view. The following functions can be performed with the mouse buttons:

Left: press and drag the left mouse button to the left or to the right. A clockwise or counter-clockwise rotation will be performed, proportional to the mouse displacement. Release the button when finished.
Middle: press and drag the middle mouse button to the left or to the right. A continuous rotation will be performed, clockwise or counter-clockwise. Release the button when finished.

Zoom in/out



This button is used for zooming operations. Zooming is always performed around the centre of the view. The following functions can be performed with the mouse buttons:

Left: press and drag the left mouse button to the left or to the right. A zoom in - zoom out will be performed, proportional to the mouse displacement. Release the button when finished.
Middle: press and drag the middle mouse button to the left or to the right. A continuous zoom in - zoom out will be performed. Release the button when finished.

Region zoom



This button allows to specify a rectangular area of the active view that will be fitted to the view dimensions. After having selected the button:

press and drag the left mouse button to select the rectangular region,
release the button to perform the zoom operation.

These operations can be repeated several times to perform more zooming.
Press the right mouse button to quit the option.
Fit view



The fit button is used to fit the content of the view to the view limits without changing the current orientation of the camera (which can be interpreted as the user's eyes).
Restore view



The restore button is used to fit the content of the view and to give a default orientation to the camera.

Getting Started

Welcome to the AutoBlade™ User manual - a presentation of the NUMECA parametric blade modeller for turbomachinery blades. This chapter presents the basic concepts of the AutoBlade™ and shows how to get started with the program by describing:

3D view options
The 3D view is customized in the menu opened by the command View/3D view options.
The 3D view settings are stored in the parametric file. Therefore, the model retains the settings when it is reopened, but importing a parametric model or template alters those settings.
Geometry
The tab Geometry is used to select the contents that will be shown in the view and choose the display mode. By default, the main blade and the optional splitters are drawn as single instances. Hub surface, shroud surface and repetition can also be activated as well as the defining section curves. Curves can be turned on or off, as well as shading and wireframe. The settings apply to all objects in the view. 


In case of cascade topology, the buttons Revolved hub surface and Revolved shroud surface are renamed as Reference hub surface and Reference shroud surface, respectively
Appearance
In this tab, the color of both edge and shading can be imposed by the user by left-clicking on the color proposed by default.
The view is automatically updated after any change but this operation is slower when more objects are displayed. Hub, shroud and repetition should be disabled for better performance during edition. A coarse quality settings might slightly improve the refresh speed.


Surface analysis


The tab Surface analysis allows the user to display the surface curvature and the derivatives of x, y, and z in the u and v parametric directions in the 3D view. Before starting the surface analysis, the user must select the surfaces first in the tab Geometry / Geometry options / Surface analysis, see Geometry Options for more details. If no surfaces are selected for analysis, the tab Surface analysis in the 3D view settings window will be disabled.
The option Display surface analysis contour is used to view the quantity contours for all selected surfaces. The option Display surface analysis mesh is used to view the surface analysis mesh.   The displayed quantity can be selected in the pull down menu Quantity. By default, the colormap range is set to its minimum/maximum values. This colormap range may be specified manually. The button Default sets the colormap to the full range of the chosen quantity. The Update button allows the user to update the contour plot without closing the 3D view settings pop-up. This button only updates the contour drawing, and is many times faster than updating the full 3D view.
Currently, the following quantities are available for selection.
TABLE 6 Surface analysis quantities





Quantity
Description





Curvature


Maximum of the absolute value of the two principal curvatures. The principal curvature is defined as , where r is the radius of the osculating circle.




dx_du


1st partial derivative of x relative to the surface parameter u




dy_du


1st partial derivative of y relative to the surface parameter u




dz_du


1st partial derivative of z relative to the surface parameter u




dx_dv


1st partial derivative of x relative to the surface parameter v




dy_dv


1st partial derivative of y relative to the surface parameter v




dz_dv


1st partial derivative of z relative to the surface parameter v




dx_duu


2st partial derivative of x relative to the surface parameter u




dy_duu


2st partial derivative of y relative to the surface parameter u




dz_duu


2st partial derivative of z relative to the surface parameter u




dx_dvv


2st partial derivative of x relative to the surface parameter v




dy_dvv


2st partial derivative of y relative to the surface parameter v




dz_dvv


2st partial derivative of z relative to the surface parameter v




The quantities are computed based on the Parasolid faces. The u and v directions are not assumed to be aligned streamwise, spanwise, etc.

Optimization Algorithms for AutoBlade™ Fitting

In AutoBlade™ Fitting, four types of optimization algorithms are available: genetic algorithm, simulated annealing, gradient and random walk.:


FIGURE 1 AutoBlade™ Fitting algorithms

Random Walk  
From the best sample found in the database, the algorithm steps from the original point to another point in a random way. If the sample found is better than the original point, the algorithm goes to this point. Otherwise, another direction is tried. After a number of unsuccessful attempts, the perturbation amplitude is reduced.
Gradient Method
This method is based on the computation of the gradient of the global objective function with respect to all the design parameters. Then a small step in the direction opposed to the gradient is performed. This process is repeated a number of times and usually ends when a stable optimum has been found.
Genetic Algorithm: Default Algorithm
This algorithm mimics natural behavior in terms of biological evolution in order to reach the best possible solution to a given problem. An initial population is generated and pairs of individuals are selected from this population based on their performances. Weak individuals tend to die before reproducing while stronger ones live longer.


FIGURE 2 Genetic algorithm parameters

Population Size: number of individuals generated at each step of the reproduction process.
Number of Reproduction Cycles: determines how many times the population will reproduce.
At each generation, the individuals are classified according their performances (from the best to the worse). That allows to select the x best ones to generate the next population:
Truncation Rate: number of samples which are selected to reproduce; the default number is 20 that means only the 20 best samples are used to create a new sample in the next generation. It is advised not to exceed half of the population size.
Elitism: number of individuals that are directly transmitted to the next generation without any change; by default, this value is 1, that means the next generation will contain the best individual of the current population. It is advised not to exceed half of the Truncation rate.
Extrapolation Range: determines between which values the parameters of the child will be found. If it is set to 0 (default value), the interval of variation will be delimited by the parameters of the parents. If not, the interval of variation will be bigger: it is useful only if the parents are too close to explore a new field of variation.

Then, the user has to define the amplitude of mutation. If set to 0, there is no mutation: the parameters of the child will be a mixing with the parameters of the parents. If not, the parameters will be taken in the interval defined with the Extrapolation range and excluding the parameters of the parents. Higher the amplitude of mutation is, more distant the parameters of the child will be compared to the ones of the parents. Two parameters define the mutation:

Search Interval: fixed amplitude of mutation. 
Precision Coefficient: coefficient which determines the fluctuation of the mutation

The amplitude of mutation is proportional to the product Search Interval*2-αPrecision Coefficient with α generated randomly. So, if Search interval is set to 0, there is no mutation (default case) and the higher the value of Precision Coefficient is, the lower the mutation amplitude will be.  It is advised to keep the default values of these two parameters.
Simulated Annealing


FIGURE 3 Simulated Annealing algorithm parameters
This algorithm is based on the analogy of the simulation of the annealing of solids. The algorithm is similar to the random walk method but has a more sophisticated method to decrease amplitude of the random perturbation steps.

Initial temperature: initial temperature of the algorithm
Final temperature: temperature at the end of the algorithm.
Temperature Reduction factor: coefficient by which the current temperature is multiplied to give the temperature of the next step. The number of iterations could be deduced using the following formula: 

(Tini-Tend)/Tred.

Number of steps: Number of steps performed before the temperature reduction.
Minimum error: parameter that fixes the convergence level of optimization (10-Minimum error). If the algorithm reaches the final temperature or the convergence level specified, the algorithm will stop.

AutoBlade™ Fitting allows combining these algorithms by selecting the number of optimization algorithms (FIGURE 1 (1)). The processing order of the algorithms is given with the active optimization algorithm (FIGURE 1 (2)). In particular, a genetic algorithm can be applied and then a gradient method to better refine the final optimum shape.

Setup Initial Model
Before the initialization and fitting processes take place, a starting model must be defined with topological settings that are well adapted to the target geometry. It is usually advised to load a template close to the type of machinery to be fitted, especially to satisfy:

the number of blade types (with or without splitter blade),
the machinery type (axial or radial)

Then, the designer should review all design steps and check for settings and amounts of defining parameters. The few next topics can be seen as quick guidelines. Further details about topological choices and compatibility are available in the section Topological Compatibility Issues.
When an optimization based on the fitted model is planned, the key point is to use as few sections as possible (from 2 to 5) and the simplest laws to define the curves. Additional sections will increase the total number of parameters and the fitting process will be much more time consuming. When ready, a starting model without splitter blade should contain between 50 and 100 parameters.
More parameters can be defined if the goal is simply to 'import' an existing geometry for a standalone use of AutoBlade™ on the fitted model. More parameters mean possibly slower convergence of the fitting process, but also finer results.
Endwall Curves
Bezier and B-spline curves defined by up to 10 nodes are generally good choices for most designs, except in some specific cases:

when the endwall curve is nearly linear at one or both ends, a composite line-Bezier-line is preferred. A B-spline curve type is typically the worst choice and should be discarded.
when no optimization is planned on endwalls, a parameterless curve may be a suitable. The data points from the target geometry file should be used here.

Stream Surfaces
This critical choice depend on the way sections are defined in the target geometry file.

Axial turbomachinery are usually defined on cylindrical or conical stream surfaces. In case of pure axial geometry, a planar section is another common choice.
Radial turbomachinery should rely on hub to shroud interpolated stream surfaces or planar radial surfaces.

Stacking Point
Leading or trailing edge stacking is the most efficient choice, but many rotating geometries use the centre of gravity. This choice is usually dictated by mechanical considerations.
Meridional Location

Radial compressors and turbines use edge traces
A stacking law is suitable in most axial cases (stacking on Z coordinate) or pure radial cases (stacking on R coordinate).

Sections Construction Mode
A single thickness distribution is the most compatible choice and is usually preferred for radial machinery and thin blades.
Construction curves is a good choice for axial machinery and thick blades, but it is not compatible with all camber constructions planes.
Effects
Effects are not handled by the initialization process and are not compatible with the fitting process. Therefore, effects should be disabled in any fitting project. If an effect is active, a warning is generated within the interface as soon as one of the processes is being launched.
Expressions
The initialization process does not support dependencies and automatically disables any active expression in the model before trying to guess suitable values for the parameters.
Expressions allow complex dependencies between the defining parameters and are generally not compatible with the fitting algorithms. Therefore, it is highly advisable to disable all expressions before launching the fitting process.
Some dependencies are safe in the fitting process. As soon as all parameters linked by expressions are included in the same steps, they are almost always compatible with the fitting process. For instance, linking several parameters from a single curve always produce valid results. On the contrary, linking several parameters from one section to another will probably produce very bad results since linked parameters are involved in separate fitting steps!

First Run
Two to three runs are usually sufficient to achieve a good result in single blade cases. The first run is usually a coarse process because the topological settings could be wrong or bounds of some parameters reached early. In such a case, a longer process useless.
Clicking the Ok button will start the fitting process. When launching a fitting process, each step is specified in the status bar. The resulting model at the end of the process is set as persistent. The convergence history and log file are saved on disk.
An Abort operation button appears on top of the interface to allow abort of the process. If clicked, the current step is not interrupted, but all next steps are skipped and the message is changed to "ABORTING – please wait".
Fitting Steps
The first two fitting steps optimize the endwall curves (optional) as well as the meridional and tangential locations of the edge traces (optional). Then, the parameters defining the sections are optimized for each single section and each blade. The formula below gives the number of steps required for a complete fitting run, whatever the amount of reproduction cycles (Coarse, Medium or Fine).
nb(steps) = 2 + nb(primary sections) x nb(blade types)
Processing Speed
The completion time required for a single step is highly dependent on the geometry involved in the step.

The first step is very quick because it involves the hub and shroud curves only.
The second step fits the stacking laws. This is quick if a sweep law is applied, but a full processing of the sections is required in case of edge traces.
The next steps involve each section of each blade. For a given blade, the processing time is equal for all sections. The completion of such a step is usually slightly slower than the two first steps.

On average, the processing time is therefore proportional to the number of blades, but the use of edge traces may also significantly slow down the process.
Typically, a coarse fitting on a simple case defined by one blade and 5 sections takes less than a minute if a sweep law is active.

Leading & Trailing Edges
This menu collects optional settings for leading and trailing edges that are available for the selected construction modes. Please consult the Suction & Pressure Side Curves section for explanations on how requested edges are constructed.


FIGURE 68 Leading & trailing edges options menu
For both edges, up to three edge types are available:

Rounded: this is the default selection.
Blunt:


Regular: edges are cut perpendicularly to the camber curve in the chosen construction plane.
Constant dmr: edges are cut at camber edge point  value, whatever the construction plane.
Constant theta: edges are cut at camber edge point θ value, whatever the construction plane.


In independent suction and pressure sides mode, leading edge is always rounded, but a blunt trailing edge is possible. In that case, no ending circle arc is built.
If a user-defined thickness law is applied, the edges are explicitly defined by the law or the specific rounding options. This menu is therefore not applicable in that case!

Elliptical:


The internal rounding allows to close the leading/trailing edge with an elliptical arc that is passing through the starting/ending point of the camber curve.
The external rounding allows to close the leading/trailing edge with an elliptical arc that has its center at the starting/ending point of the camber curve.
The cutback rounding allows to close the leading/trailing edge with an elliptical arc that is tangent to the meridional location of the starting/ending point of the camber curve.






            Elliptical rounding and edge position choices present the following limitations:

Supports symmetric thickness addition only.
Discretized sections are not well supported. Interpolation can possibly generate bad profiles.
External and cutback positions are not available for splitter blades.
Currently no support in the fitting module (mainly because the rounding is not built in the parametric curve).
Not available when the Center of Gravity selected as stacking point.

Monitoring of Controls
Any angle, control point, node or length can be monitored in the status bar. This happens when the mouse pointer is close or over the graphical representation of the control, as soon as it is highlighted (the color changes from green to red).
Angular Parameters
Angles are easily recognized thanks to their two reference lines, their circular arc and their symbolic name. A small triangle to one end of the arc indicates the direction of the angle and is used to pick or highlight the angular control.
For instance (FIGURE 32), the stagger parameter can be highlighted in the lower left view by moving the mouse pointer over the control triangle (1). The color changes to red and a message indicates an optional edition of the angle in the bottom of the viewing area (2). The status bar indicates that the control is parameter S1_CAMBER_GAMMA with current value 40.0 degrees (3).


FIGURE 32 Highlighting and monitoring of an angular parameter
Nodes & Control Points
Nodes and control points are drawn as simple green points and may appear differently according to the control, curve and view they belong to. Three different cases can be encountered, as illustrated in FIGURE 33 on the default model.

In the first case (upper left), the node on hub curve is controlled by two parameters HUB_Z2 and HUB_R2 that fully defines its location in the meridional plane.
In the second case (upper right), the control point of the suction side curve is defined by a single parameter S1_TSS_2. Therefore, it cannot freely move in the plane and is constrained to remain on a line perpendicular to the camber curve.

In the third case (bottom), no parameter is linked to the control point, but can indirectly change angular parameters named B1 and B2 of the camber curve. The 2D coordinates of the control point in the construction plane appear in the status bar.


FIGURE 33 Three kinds of nodes and control points
Lengths
Length and fraction parameters are symbolized by a hollow point and a short name in the view. This kind of parameter appears in some endwall curves (left picture in FIGURE 34), stacking laws or edge traces (right picture in FIGURE 34). Those controls are specialized control points that either define a length or a fraction of a reference length. Those points can move in only one direction!


FIGURE 34 Length parameter on hub curve (left) and edge trace (right)
End line parameter for side curves is a length, but its symbolic representation differs from the one introduced above for more readability. A triangle control replaces the circular marker and its label.
Radius
A radius parameter is symbolized by a circle arc of the prescribed size, its centre point and a label R. It is highlighted when the mouse pointer is near the centre point (FIGURE 35).
If the involved curve is a real circle however, the symbolic arc is not drawn (case of B-spline half-thickness).


FIGURE 35 Radius parameter in a half-thickness law (Bezier)

How To Use This Manual
Outline
This manual consists of three distinct parts:

Getting Started and Graphical User Interface: introduction and description of the interface,
AutoBlade™ Modeller, 
AutoBlade™ Fitting.

At first time use of AutoBlade™ it is recommended to read this first chapter carefully and certainly sections First Time Use to Required Licenses of this chapter. The Graphical User Interface chapter gives a general overview of the AutoBlade™ interface and the way to manage a project. The AutoBlade™ Modeller chapter presents the NUMECA parametric blade modeller for turbomachinery blades. It describes all the geometrical functionalities available in AutoBlade™. The AutoBlade™ Fitting chapter presents the fitting module which allows to import an existing blade geometry and convert it to the AutoBlade™ format.
Conventions
Some conventions are used to ease information access throughout this guide:

Commands to type are in italics.
Keys to press are in italics and surrounded by <> (e.g.: press <Ctrl>).
Names of menu, sub-menu items and names of buttons in dialog boxes are in bold.
Numbered sentences are steps to follow to complete a task. Sentences that follow a step and are preceded with a dot (•) are substeps; they describe in detail how to accomplish the step.

Blue text in a blue box indicates an important note

Export rulings
The menu Geometry/Export rulings...  opens a file chooser and prompts for a location where to save the geometry with default extension ".rln" for flank-milled designs.
The .rln file includes the following parts:
Rulings and rounding
Rulings
Ruling directions are defined independently for each blade.
Each ruling direction is defined by its two ending points in 3D coordinates (X, Y, Z, R and θ) on hub and tip sections. This original definition is based on the 3D camber curves.
For each ruling direction, two additional links are defined for suction and pressure sides. These links are directly built from the original camber ruling directions on the side curves by thickness addition.
The suction and pressure links belong to the original ruled surfaces and do not take the effects like blade cutoff or late elliptical rounding into account.
Optional elliptical rounding & cutoff
Blade cutoff
When blade cutoff is applied, the following data is written to the .rln file
CUTOFF_DATA
Then for leading edge cutoff:
CUT_LOCATIONS_FOR_LE
HUB_LOCATION_Z [floating point value]
HUB_LOCATION_R [floating point value]
SHROUD_LOCATION_Z [floating point value]
SHROUD_LOCATION_R [floating point value]
And/or for trailing edge cutoff:
CUT_LOCATIONS_FOR_TE
HUB_LOCATION_Z [floating point value]
HUB_LOCATION_R [floating point value]
SHROUD_LOCATION_Z [floating point value]
SHROUD_LOCATION_R [floating point value]
Elliptical rounding
When late elliptical rounding is applied, the topology and b/a ratios are included in the output. This section is announced by the line:
LATE_ELLIPTICAL_ROUNDING
Then, for rounding at the leading edge for hub section as an example:
HUB_LE_RADIUS_RATIO [floating point value]
HUB_LE_ROUNDING [rounding topology]
where [rounding topology] stands for one of the three identifiers:

EXTERNAL for external rounding (adds material to the section),
INTERNAL for internal rounding (preserves the original edge point),
CUTBACK for special cutback option (enforces the minimum or maximum meridional location of the blade section)

If no elliptical rounding is applied on the edge of the section, a single line is written:
HUB_LE_ROUNDING NONE

When elliptical rounding is not active at all, the next line is written:
BUILT_IN_ROUNDING

Camber and thickness
For each section, the hub and tip camber curves are written to the file with their original internal sampling. The output consists in the following fields:

the cylindrical coordinates Z, R and θ,
the wrap angle β,
the meridional coordinate m,
the reduced meridional coordinate m/m*, where m/m*=(m-mStart)/(mEnd-mStart), mStart and mEnd are the start and end points of the camber curve, respectively.
the local thickness value (on the stream surface).

The local thickness value is the thickness measured on the stream surface and not as a 3D distance.
θ angle is given in radians.
β angle is given in degrees.
Final side curves
The final side curves (suction and pressure sides) are written for hub and tip sections in coordinates X, Y, Z, R, θ, m and m'.
This output corresponds to the final side curves, after blade cutoff and elliptical rounding if applied.

Geometry Options
Curves
This tab Geometry options / Curves allows to control the discretized curves in cases where the default precision is insufficient.
By clicking the small button in front of the curve name, the user can change the default sampling value. 


FIGURE 20 Curve sampling dialog
The following table is a summary of the sampling rules for the different curves.







Curves


Default value of samples


Description






Hub/Shroud


100


This is the default sampling for endwall curves except when a composite is defined.




Camber


100


For all camber types.




Suction side


110


For all suction side curves and regular thickness laws. This sampling is additive with trailing edge circle sample in case of construction curves.




Pressure side


110


For all pressure side curves and regular thickness laws. This sampling is additive with trailing edge circle sample in case of construction curves.




Half trailing edge circle


10


Only for the trailing edge circle when the construction curves are active. In practice, the final suction/pressure sampling is increased by this value minus one.




Thickness formula


130


Internal sampling of the mathematical thickness laws. This value is not applied to file input where the sampling is dependent of the data file.




Gap curve


50


Internal sampling of the hub/shroud gap curves.




Defaults for endwalls
For regular parametric curves, the default value is 100.
For composite curves, each element has an automatic number of points depending on the type (2 for linear segments) and the number of nodes. Therefore, the total number of points is variable. In addition, the export to geomTurbo differs according to the version: each element is exported as a basic curve with its own sampling in version 5.3, but as a single curve with the default number of points in version 3.7. However, if the composite curve contains at least one linear segment, it is exported as a single polyline with automatic refinement when the older format applies.
When interpolated stream surfaces are used with shortening (inlet/outlet locations), the composite curve is always exported as a single curve with the default sampling and the vertex mapping is taken into account to shorten the curve in version 5.3 (replaced by a shortened curve in version 3.7).
User-defined sampling for endwalls
The curve is always exported as a single curve with the prescribed number of points, whatever the type of the curve (including composite) and this is true for all geomTurbo outputs.
Checks
As described in Error Messages, when an error or a potential problem is detected in the update of the model, Autoblade™ will report failures and warnings in the message list. However, Autoblade™ may give a failure message for a good model in some special cases. The user can avoid this kind of error message by means of cancelling the check for the geometry. 


The option Check endwall curves allows to check the hub/shroud curves. 
The option Check thickness laws allows to check the thickness laws. 
The option Check 2D sections allows to check the blade passage.
The option Check CAD model allows to check the 3D Parasolid model.
The option Check min draft angle allows to check the minimum draft angle. The draft angle is used in manufacture of blades with the casting process in order to make sure that a ruled blade is removable relatively to one direction.
The option Check min draft angle can be accessed only when the blade is defined by 2 primary sections.
The option Check min draft angle is not available for splitters.
The draft angle is defined by two sections. In order to process the minimum draft angle, the head section is compared to the foot section. For each sample point on the head section (pressure side and suction side, respectively), starting from the leading edge to the trailing edge, the interiority is checked. The draw direction is assumed oriented from foot to head.



If a head point is interior to the foot profile, the closest point of the foot section in the projected plane is searched. Then the draft angle is processed in 3D coordinates. In this case, the draft angle is positive.
If the head point is exterior, the draw angle is assumed negative. Please note that if the draw direction is contradictory with blade orientation, interiority is reversed and the sign of the resulting draw angle as well.

Surface analysis
This tab Geometry options / Surface analysis allows users to select surfaces, where users can analyze the principal face curvature and the derivatives of x, y, and z in the u and v parametric directions.


Three surfaces are available for selection: the non-axisymmetric hub, the non-axisymmetric shroud, and the blade. By default, no surfaces are selected for analysis.
The number of Boundary points is used to set the number of discrete boundary points. A 2D mesh will be created in the uv coordinate system based on the imposed number of boundary points. If necessary, the user may increase or decrease the resolution of the surface mesh.
After enabling the surface, the curvature and the derivatives of x, y, and z can be analized in the Blade-to-blade view, see 3D view options for more details.

Solid Body

The solid body module allows the user to create one or multiple solid geometries in AutoBlade™, and thus allows the user to perform multidisciplinary optimization in FINE™/Design3D. The solid body is defined as one or more axisymmetrically defined bodies merged and optionally blended with the AutoBlade™ solid blade geometry.
The solid body module can be activated by selecting the selection box Activate solid body modeling. Then the interface defining the solid body can be accessed. The window configuring solid geometries contains two tabs, one for the definition of the axisymmetric geometry with composite curves in the Meridional view (Axisymmetric geometry definition), and one for other advanced settings (Advanced settings).


Define solid body
The left panel of the tab Axisymmetric geometry definition contains a list of the solid bodies in the model. The name of each solid body may be changed by double-clicking on the entry in the list.    The button Delete selected solid body allows to remove the selected solid body from the list. The button Sketch new solid body opens a tool allowing the user to sketch a new solid body profile in the Meridional view. The right panel contains a list of the composite curve elements for each solid body. For the existing composite curve elements, the curve type and the number of control points may be modified. The existing elements may also be deleted and new elements may be inserted in the composite curve.


FIGURE 88 Axisymmetric geometry definition
To add a new solid body, click on the button Sketch new solid body. Then, the meridional view will be switched to interactive edit mode, as shown in FIGURE 89. Left-clicking in the meridional view will add a new control point. Right-clicking in the meridional view will draw a line or bspline by using the new control points, depending on the number of the new control points. If no new control points are added, right-clicking will exit the edit mode (or use the key <q>). After exiting the edit mode, the new body will be added in the solid body list. A valid solid body will be displayed as a shaded region.
For an existing solid body, if the user selects the definition profile of the solid body in the meridional view, the control points will be highlighted and may be interactively moved. Once moved, the underlying R and Z parameters are automatically updated.


FIGURE 89 Interactive edit mode in the Meridional view
Each axisymmetric solid body is defined by a single composite curve in the RZ frame and the corresponding hub/shroud curve. The single composite curve in the RZ frame should intersect its associated endwall curve exactly twice, and must not be self-intersecting. FIGURE 90 shows the examples with correct solid body definition (A) and wrong solid body definition (B/C/D). 


FIGURE 90 Centrifugal compressor solid body setup (A - Valid geometry, B/C/D - Invalid geometry)
The merging of the blade and hub/shroud solid bodies requires a clean intersection of the bodies.  The spanwise locations of the blade sections may influence the success of the merge, particularly if sections are spaced such that  [ 0 < spanwise location < 1 ].
The parameters defining the control points are as follows:






Parameter


Description






#_SOLID_R(i)


defines the R coordinate of the ith control point in the solid body named as #




#_SOLID_Z(i)


defines the Z coordinate of the ith control point in the solid body named as #




Advanced settings
The tab Advanced settings contains options related to the setup of the blend parameters and expert setting used to tune the periodic sector symmetry creation.


FIGURE 91 Advanced settings of the solid body
By default, the blend function is disabled. The user may activate this function by selecting the selection box Activate blend parameters. Then a blend will be created between the blade and the solid body. AutoBlade™ supports both constant radius and constant width blending. If the option Extend blend to blunt faces is selected, the blend will be extended to the blunt faces at leading/trailing edge of the blade.
The parameters defining the blend are as follows:






Parameter


Description






MAIN_HUB_BLEND_RADIUS
or
MAIN_SHROUD_BLEND_RADIUS


defines the blend radius of the main blade for constant radius blend




SPLIT(i)_HUB_BLEND_RADIUS
or
SPLIT(i)_SHROUD_BLEND_RADIUS


defines the blend radius of the ith splitter blade for constant radius blend




MAIN_HUB_BLEND_WIDTH
or
MAIN_SHROUD_BLEND_WIDTH


defines the blend radius of the main blade for constant width blend




SPLIT(i)_HUB_BLEND_WIDTH
or
SPLIT(i)_SHROUD_BLEND_WIDTH


defines the blend radius of the ith splitter blade for constant width blend




To minimize the size of the solid geometry and the structural analysis mesh, it is prudent to represent the solid geometry as a sector model. A sheet body is used to extract the sector geometry from the 360 degree spun bodies. A separate set of cut sheets is generated for each solid body, with the meanline curves of the main and splitter blades at the associated endwall used as a guide. The cut sheet is generated by projecting a series of wire bodies from R=0 through a reference curve to the maximum radius of the solid body. The reference curve passes through the meanline curves of the main and splitter blades, with additional segments to facilitate the transition between the main and splitter blades. Additional wires are created at axial locations upstream and downstream of the solid body. A sheet body is lofted through this array of wires, yielding a series of sheet bodies. The sheet is then duplicated and rotated by one full passage angle.
The solid sector geometry can be exported.
For most axial and radial configurations the method above works well. With some radial configurations lofting the cut sheet through the full extent of the reference curve has been shown to create undesirable or invalid geometry. In this case, the following settings can be used:

Reference curve range: specifies the range of the reference curve to be used when lofting the cut sheets.
Sector positioning, main blade: modifies the tangential positioning of the main blade segment of the reference curve. 
Sector positioning, splitter blade: modifies the tangential positioning of the splitter blade segment of the reference curve. 
Transition factor: modifies the segments between the splitter and main blades. 
The surfaces of the merged solid geometry are named as follows:
The solid body surfaces inherit their names from the RZ profile used to define the geometry, along with suffixes specifying additional information:
<Solid_body_name> + "_" + <segment_name> 
<Solid_body_name> + "_Endwall"
<Solid_body_name> + "_Periodic_" + <face_number> + "_side1"/"_side2"
For example:
Test_Endwall
Test_Curve_1
Test_Periodic_2_Side2
Surfaces originating from the blade bodies inherit their names from the preexisting blade body names. For example:
"MAIN_PRESSURE_F1"
"MAIN_SUCTION_F1"
"SPLIT1_PRESSURE_F1"
Surfaces resulting from the blend operations are built to indicate the associated blade and endwall. For example:
"MAIN_HUB_Blend_0"
"MAIN_HUB_Blend_1"
"SPLIT1_SHROUD_Blend_0"

Suction & Pressure Sides Construction Mode - regular
In the method described above, the suitable values of the involved parameters TSS(j) and TPS(k) are not easy to estimate, especially the offsets near the leading and the trailing edges.
For instance, a low value of TSS(1) could generate a bad leading edge shape as shown in FIGURE 51, where the curvature radius reaches a low local minimum just after the leading edge point. This case can be avoided if the value of TSS(1) is larger than the length of control segment  (FIGURE 51). Since the latter value depends on formula for the first control segment length, the user cannot guess when a given TSS value is suitable or not.


FIGURE 51 Bad leading edge shape
A similar problem can occur near trailing edge.
A new set of parameters is provided to help the designer achieving valid topologies in an easier way. This method is activated by pressing the button With end line in the Suction & Pressure Sides section. In comparison with the classic construction mode, three intermediate parameters are defined, one near the leading edge and two near the trailing edge, as shown in FIGURE 52.


FIGURE 52 Definition of the suction curve with an ending line (for 9 control points or 2 intermediate control points)
The three following changes have been introduced for both suction and pressure sides. It is here explained in the suction side context and a rounded trailing edge is assumed.

The first TSS parameter from the original method is replaced by an angle δle to ensure a better control of the side curve near the leading edge (FIGURE 53, left). The control point C3 is defined as the intersection between the prescribed direction issued from C2 and the line parallel to the first control segment and passing through construction point 1. Angle δle should always be positive and, thus, its lower bound is straightforward.
The (n-1) TSS parameter is replaced by a fractional offset  measured from the last control segment direction  so the control point moves away from the camber curve when it is positive and moves closer when it is negative. The definition of the fractional offset is similar to the definition of the TSS parameters, but it starts from the last control segment direction instead of the camber curve.


FIGURE 53 Leading edge (left) and trailing edge (right)
The suction side curve is optionally ended by a line segment. Continuity up to the first derivative is ensured at both ends of that segment, at the junctions with the Bezier curve and the circle arc. Length  is expressed as a fraction of the camber curve length in its construction plane.

TABLE 6 2D blade profile definition (rounded case with end line)






Setting


Description






number of intermediate control points


number of intermediate offsets to add between leading and trailing edges - amounts may differ for suction and pressure sides.




stretching factor


ratio of two successive offset gaps on the camber curve - values may differ for suction and pressure sides




Parameter


Description




S(i)_LE_RADIUS


prescribed leading edge curvature radius RLE for section(i)




S(i)_TE_RADIUS


prescribed trailing edge radius RTE for section(i)




S(i)_TE_WEDGE_ANGLE


prescribed wedge angle δte for section(i) (in degrees)




S(i)_SS_LE_WEDGE_ANGLE
S(i)_PS_LE_WEDGE_ANGLE


prescribed wedge angle δle for the side curve of section(i) (in degrees)




S(i)_SS_REAR_SHAPE
S(i)_PS_REAR_SHAPE


prescribed fractional offset  for the side curve of section(i)




S(i)_SS_END_LINE
S(i)_PS_END_LINE


prescribed fractional length  of the ending line for the side curve of section(i)




S(i)_TSS_(j)


intermediate offset TSS(j) for suction side curve of section (i)




S(i)_TPS_(k)


intermediate offset TPS(k) for pressure side curve of section (i)




The number of control points n here becomes:
n = 6 + number of intermediate control points

Parametric Report 
The last icon of the model editor, in the left area of the main interface, grants access to a parametric report aiming the description of the total number of parameters.


The tolerances blocking tolerance and blocking epsilon allow to determine in the Free page the free parameters that can be considered as blocked when one of the bounds is reached.

Construction Plane


FIGURE 34 Reference length & Construction plane
Reference length
When a sweep law is defined, the modeler can not evaluate the meridional blade passage simply by stacking the blade sections on the sweep curve because the blade section length is unknown.
According to the stream surface type, up to three camber length types are possible:

Z: an axial length DZ is a common choice in axial turbomachinery (planar and cylindrical stream surfaces).
R: a radial extend DR is useful in centrifugal turbomachinery (hub to shroud linear interpolation and conical stream surfaces).
m: a meridional DM length. This is the safest choice since the parameter m always increases along the stream surface traces. On the contrary, Z and R coordinates do not always increase from inlet to outlet.

The meridional length is not interfaced graphically and can be modified either in the Stacking laws menu or in the Parameter list window.






Parameter


Description






S(i)_DZ_prim


(i)th section length along Z axis for blade length type 'DZ'




S(i)_DR_prim


(i)th section length along R axis for blade length type 'DR'




S(i)_DM_prim


(i)th section length along m axis for blade length type 'DM'




When the meridional location is defined using edges traces, no reference length is available. The meridional length DM is not available for axial stream surfaces since DZ and DM values are equal.
If the modeller does not succeed in applying a DZ or DR length, please make sure your reference lengths are not too close to zero or out of the machine reference dimension. If this does not solve the problem, try a DM length.
Furthermore, the user can select either meridional chord or true chord. This choice enables the merge of the new method (true chord) with the classic coordinate choice previously available in the Meridional location page under the Stacking laws menu within AutoBlade™ 2.1.
In the page Construction plane, True chord is unavailable:

when Leading and trailing edges traces are selected, where the meridional chord is assumed and automatically managed (usually for radial blades), 
when planar radial stream surfaces are selected, since the chord has no meaning.

When the Meridional chord method is selected, the available construction planes are simply the same as in release 2.1. When True chord is selected, the construction planes are identical, except that (m,β) is never accessible since it is not compatible with the definition of a chord.
The list of available construction planes compatible with the True chord option is summarized below and depends on the stream surface type and the stacking point choice.
TABLE 2 Compatibility table for sweep law option and true chord based profiles


Since (Z,Y) and (m,Rθ) planes are dimensional, the chord can be built directly from its length, so these planes are the preferred choices for axial blades.
For enlarged compatibility, (,θ) plane will be available, but the chord length has no direct meaning with these coordinates. However, in pure axial cases with cylindrical stream surfaces for instance, the true chord is simply the prescribed length in (,θ) multiplied by the radius of the cylinder.
Construction plane
Up to four construction plane options are available for the definition of the camber curve and their properties are briefly explained in the following table.
TABLE 3 Construction planes for camber curve






Plane


Description






(Z, Y)


The camber curve is directly built in planar coordinates (Z,Y) and translated on the stream surface.




(m, R*θ)


The camber curve is built in (m, R*θ) plane and is then applied on the stream surface. It is often preferred for axial turbomachinery, where distances are preserved.




(m, β)


β is the prescribed angle, expressed in degrees, for the camber curve in (, θ) plane. The distribution of β is generated, then integrated to obtain θ. The latter angle is stored on the stream surface.




(, θ)


The camber curve is built in the (, θ) plane and translated on the stream surface. This is an angle conservative plane often preferred for radial turbomachinery.




The (Z,Y) plane is specific to axial planar stream surfaces while (m,R*θ), (m,β) and (,θ) planes are compatible with revolved stream surfaces.
For axial topologies dimensional planes (Z,Y) or (m, R*θ) are often preferred while radial blades are usually described using either (m, β) or (, θ) plane.
When previous settings do not allow a construction plane for some reason, the choice is disabled in the interface. Please refer to Topological Compatibility Issues for further details.
When conical or interpolated stream surfaces are active, AutoBlade™ is not aware of the exact type of machinery (axial, centrifugal,...). Users are therefore not prevented from choosing (m,R*θ) with a radial topology, while the (m,R*θ) plane only preserves distances when the radius R can be assumed constant over the whole section.
In such a case, the prescribed thickness is not preserved in thickness addition mode and edge radii are not preserved in suction and pressure side mode.
The good practice with radial topologies is therefore to define the camber curve either in (m, β) or (, θ) together with a thickness addition.

Dialogs & Windows
In AutoBlade™, most menus appearing as separated or top level windows carry two buttons:

OK: applies the changes entered in the menu and closes the dialog box. An update of the blade model is applied accordingly.
Cancel: leaves the menu without saving changes. If Apply has been clicked, only the changes brought after this last operation are discarded.

Sometimes, a third button Apply also appears to apply the changes without leaving the dialog. This option is useful to reflect the changes and to continue within the menu, in the Parameter list for instance.
Confirmation dialogs have two buttons Ok and Cancel.
Information windows only have a Close or Ok button.
Closing the dialog box using the platform specific way to close a window is similar to a click on the Cancel button. This applies to all menus and dialogs inside AutoBlade™.

How to start AutoBlade™
In order to run AutoBlade™, the following command should be executed:

On Linux platforms type: 
autoblade# -print <Enter> 
where # is the version number to be used (131).
On Windows click on the AutoBlade icon in Start/Programs/NUMECA Software/Fine# or Start/Programs/NUMECA Software/AutoBlade#. Alternatively AutoBlade™ can be launched from a dos shell by typing: 
<NUMECA_INSTALLATION_DIRECTORY>\fine#\bin64\autobladex86_64 

or
<NUMECA_INSTALLATION_DIRECTORY>\autoblade#\bin64\autobladex86_64 

where NUMECA_INSTALLATION_DIRECTORY is the installation directory chosen by the user and # is the number corresponding to the version to be used.
Press the first button from the main tool bar or select item File/New from the main menu. A small dialog pops up. This allows the user to start from scratch or create a new project from an existing parametric model. If the user selects Start from an existing model, the button Ok is grayed until a valid parametric file has been selected.



FIGURE 3 File/New dialog
When the button Ok is clicked, a file chooser dialog opens. Select a folder under Directories field, then type a name in the Files field and click Ok.
White spaces should be avoided in the file name.


FIGURE 4 Model creation dialog box
A default blade model appears in the four views layout as shown in figure below.


FIGURE 5 AutoBlade™ interface
To start working in AutoBlade™ as a standalone modeller from the FINE™/Turbo interface, the following steps should be followed:

Launch the FINE™/Turbo interface. Please refer to the FINE™/Turbo User Manual for further details on how to start the FINE™/Turbo interface.
Once FINE™/Turbo interface is started, a Project Selection window appears. Press Cancel to close this dialog and get full control over the main window.




FIGURE 6 Project selection window

Select Modules/AutoBlade item from the main menu bar. A confirmation dialog opens with the message This will start AutoBlade module. Press Ok to continue.



FIGURE 7 FINE™ interface

Press the first button from the main tool bar or select item File/New from the main menu. A file chooser dialog opens. Select a folder under Directories field, then type a name in the Files field and click Ok.

Edges Control


FIGURE 104 Edge control options tab
Coordinates
Edge coordinates Z, R or θ can be exported as quantities to the optimization process for both leading and trailing edges. In blunt cases, the arithmetic average of leading and trailing edges end points is returned.
It is also possible to know coordinate differences from section to section as described in TABLE 12, where Ci is the related coordinate for section i. Please note these differences can be positive or negative. For n sections (n>2), n differences or "delta" values are computed from which the last one is the sum of the (n-1) first ones.
TABLE 12 Coordinates differences






Number of sections


Returned delta values






0, 1


not applicable




2


1: C1 - C2




3


3: C1 - C2, C2 - C3, C1 - C3




4


4: C1 - C2, C2 - C3, C3 - C4, C1 - C4




...


...




n


n: C1 - C2, C2 - C3, ... Cn-1 - Cn, C1 - Cn










Quantity


Examples






S?_(SPLIT?_)LE_Z, S?_(SPLIT?_)LE_R, S?_(SPLIT?_)LE_THETA, S?_(SPLIT?_)TE_Z, S?_(SPLIT?_)TE_R, S?_(SPLIT?_)TE_THETA
S?S?_(SPLIT?_)LE_DZ, S?S?_(SPLIT?_)LE_DR, S?S?_(SPLIT?_)LE_DTHETA, S?S?_(SPLIT?_)TE_DZ, S?S?_(SPLIT?_)TE_DR, S?S?_(SPLIT?_)TE_DTHETA


S1_LE_Z stands for the Z coordinate of leading edge point for section 1 of the main blade.
S2_SPLIT1_TE_R stands for the R coordinate of trailing edge point for section 2 of the first splitter blade.
S1S2_LE_DZ stands for the Z coordinate difference of leading edge points for sections 1 and 2 of the main blade.
S1S3_SPLIT1_TE_R stands for the R coordinate difference of trailing edge points for sections 1 and 3 of the first splitter blade.




Fitting Lines
The searching for the best straight line approximating the main blade edge traces can be obtained through AutoBlade™. A fitting line is computed in (span, Z), (span, R) or (span, θ) plane from the edge coordinates according to the generic form:

,
so three values are generated, namely constants a, b and the approximate error. Angular coefficient a is returned in the form of an angle with respect to the ordinate direction, as shown in the next figure.


FIGURE 105 The best fitting line construction
A fitting line is computed from edge coordinates of the primary sections only. The use of this option is facilitated if all the span values are nearly uniformly spaced and extreme sections at hub and shroud are typically included. For instance, a (0.0, 0.20, 0.40, 0.60, 0.80 0.99) span list will give meaningful parameters and (0.0, 1.0) will given an error free fitting line.
This quantity is available for the main blade only, with or without splitters. The angle ANG is provided in degrees and the ERROR is of dimension [L].






Quantity


Examples






LE_BESTLINEZ_ANG, LE_BESTLINER_ANG, LE_BESTLINETHETA_ANG, TE_BESTLINEZ_ANG, TE_BESTLINER_ANG, TE_BESTLINETHETA_ANG
LE_BESTLINEZ_ERROR, LE_BESTLINER_ERROR, LE_BESTLINETHETA_ERROR, TE_BESTLINEZ_ERROR, TE_BESTLINER_ERROR, TE_BESTLINETHETA_ERROR


LE_BESTLINEZ_ANG is the best fitting line angle for the main blade leading edge in (span,Z) plane. Its value is expressed in degrees.
TE_BESTLINER_ERROR is the best fitting line error for the main blade trailing edge in (span,R) plane.

Export as IGES
The menu Geometry/Export as IGES... opens a file chooser and prompts for a location where to save the IGES export with default extension ".igs".

Example Fitting Target Geometry

This section contains two sample target files for the fitting module. As explained in the Preparing Target Geometry section, support for the geomTurbo format is partial under AutoBlade™.
The axial compressor template in AutoBlade™ is the fitted model of a simplified geometry file describing the NASA Rotor 37. The two corresponding geomTurbo files below can be used for practise in a first fitting project of an axial compressor. The first sample is a geomTurbo version 3.7 while the second is compliant with version 5.3 of the format.
The two target files define exactly the same geometry with hub and shroud in (Z,R) plane as well as three sections respectively at hub, mid-span and tip. Sections are defined on conical surfaces in Cartesian coordinates X, Y and Z.

Edition of Control
Once highlighted, any control can be edited by means of the mouse: simply left-click the highlighted symbols, then move the mouse pointer over the view. At each move, the control is moved and the value of the corresponding parameters is updated in the status bar. If the control is part of a curve definition, the curve is also updated in real time.
To accept a new location for the control, it is possible to use the mouse for rough values or the keyboard for precise values of corresponding parameters.
Mouse Input


FIGURE 36 Mouse input allows rough values for parameters (right)
Once the control has been moved to a suitable location or the value is close to the one expected, left-clicking a second time ends the edition of the control and the model is fully updated.
Highlighting the control again monitors the new value for the parameter (FIGURE 36), but the entered value is rough. Therefore, this method is especially useful for pre-design, when the shape of the blade need to be modified quickly.
Keyboard Input
Once the control has been clicked for edition, a precise numeric input may be keyed as new value for the parameter. For instance, if the value -7.0 is wanted for parameter S1_CAMBER_BETA1, simply type the following sequence in the main interface:
- 7 <Enter>
The keys are grabbed and transferred to the special keyboard input area just above the status bar (FIGURE 37, left). The edition of the control ends on <Enter> and the model is updated accordingly. Highlighting the control again allows the check of the new value (FIGURE 37, right).


FIGURE 37 Keyboard input for single parameter
Special Keyboard Input
When two parameters are involved in a single control, keyboard input is still possible, but two numeric values are required, separated by a space, before the <Enter> key is entered.
For instance, the following sequence allows to impose (-0.04, 0.51) coordinates for hub point:
- . 0 5	0.51	<Enter>
Bounds & Limits for Parameters
All parameters have a validity range. A radius is always positive and some angles cannot exceed -[90, 90] range. At edition time, the new value is compared to those limits and invalid values are automatically replaced by the closest limit (keyboard input).
In other constraints exist, the validity range can be reduced. This is the case for β1 value in the camber curve, for which the value must comply with [γ,90] range.

Minimum and maximum bounds are less critical values used when AutoBlade™ is run from FINE™/Design3D module that define the allowed range for the value of a parameter. If a value is changed in the interface, with mouse or keyboard, the bounds are automatically adapted so that the new value lies within the allowed range.
For instance, if β1 has minimum and maximum bounds of respectively 0.0 and 10.0, setting the value to -7.0 in the interface moves the minimum bound to -7.0 and the new allowed range is then [-7.0, 10.0].

Edit Menu
This menu contains the Undo and Redo commands that allow to respectively revert and recover changes to the parametric model.
Furthermore, the Scale command allows to scale the parametric model.


FIGURE 6 Scale parametric model

Fitting Process
Once the parameters of the initialized model have been checked and their bounds corrected, a fitting process can be launched through the button Fitting model (Fitting Control subpad) to get a solution closer to the target geometry.
The fitting process uses an optimization algorithm (typically a genetic algorithm) combined to an estimate of the error between the current model and the target geometry. To achieve a solution that minimizes this error criterion, the process is split into successive steps which consist in local optimizations that involve only a subset of the parameters defining the machine. 
For each step, a subset of active parameters is extracted and an initial population is generated with random values of the active parameters inside their allowed range. An iterative process begins in which a new population is generated from the best representative of the previous population.

Model Topology
The topology has been split into nine distinct steps: Endwalls, Stream surfaces, Stacking laws, Main blade, Splitter blades, Effects, Non axi hub, Non axi shroud and Solid domain. The available topologies are explained in the Model Editor subpad and the AutoBlade™ Modeller chapter in more detail.

Batch Mode
Linux
Under Linux, the executable is located under the directory "Installation_path/autoblade131/LINUX/autoblade/" (when AutoBlade™ is installed as standalone product) or "Installation_path/fine131/LINUX/autoblade/" (when full FINE™/Turbo package is installed). 
The executable can then be launched in batch mode respectively with the following command:
autoblade131 -batch -print
will launch AutoBlade™ v13.1 executable in batch mode and print all messages to the standard output. 
Windows
Under Windows, the executable is located under the directory "Installation_path\autoblade131\bin64\"  (when AutoBlade™ is installed as standalone product) or "Installation_path\fine131\bin64\" (when full FINE™/Turbo package is installed).
The executable can then be launched in batch mode respectively with the following command:
C:\NUMECA_SOFTWARE\autoblade131\bin64\autobladex86_64.exe -batch
or
C:\NUMECA_SOFTWARE\fine131\bin64\autobladex86_64.exe -batch
There is no need for the "-print" flag under Microsoft Windows. However, in order to see messages, it is advised to open a DOS shell (Command prompt) to launch the executable instead of the Run dialog under the Start menu.
Usual Flags
If no valid flag is added, an error message is printed by AutoBlade™ executable as well as a list of commonly used options.
Parametric model (.par) input
The flag "-par" is mandatory to activate AutoBlade™ support in batch mode. It must be followed by the path to the parametric file to read and acts as input. The parametric file is provided with relative or absolute path. For instance,
> autoblade131 -par /home/usr/blade.par -batch
will use model '/home/usr/blade.par' as input while
> autoblade131 -par blade.par -batch
will use model 'blade.par' from the current directory.
If no other AutoBlade™ flag is supplied, the return value of the executable allows to test the validity of the input model. In case of bad parametric format or problem in the generated model, value different from 0 is returned. If the model is valid, 0 is returned.
Parametric model (.par) output
It is possible to upgrade an older parametric file to the latest format by means of the "-opar" flag, followed by the path to the output file.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -opar blade_new.par -batch -batch
Geometric model (.geomTurbo) input
The flag "-geom" is mandatory to open a given ".geomTurbo" file (geomTurbo 3.7 or geomTurbo 5.3) in AutoBlade™. It must be followed by the path to the ".geomTurbo" file to read and acts as input. The ".geomTurbo" file is provided with relative or absolute path.
> autoblade -geom /home/usr/blade.geomTurbo -batch
Geometric model (.geomTurbo) output
A geomTurbo file can be generated from the input parametric or geometric model and saved to disk by means of the "-ogeom" flag
This flag requires an input parametric or geometric file and is additive to "-par" or "-geom" flag.
Example:
> autoblade131 -par blade.par -ogeom blade.geomTurbo -batch
The version number of the output geomTurbo format is stored in the parametric file and can be either 3.7 or 5.3. If a specific format is required, the flag "-ogeom" can be replaced by "-ogeom4" for geomTurbo 3.7 or "-ogeom5" for geomTurbo 5.3.
> autoblade131 -par blade.par -ogeom4 blade_AG4.geomTurbo -batch
> autoblade131 -par blade.par -ogeom5 blade_AG5.geomTurbo -batch
Parasolid output
A parasolid file can be generated from the input parametric model and saved to disk by means of the "-oparasolid" flag.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -oparasolid blade.x_t -batch
Solid sector geometry output
A merged blade and solid body can be outputted in parasolid format by means of the "-osectorparasolid" flag. For more information of solid body, see Solid Body.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -osectorparasolid blade.x_t -batch
IGES output
An IGES file can be generated from the input parametric model and saved to disk by means of the "-oiges" flag.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -oiges blade.igs -batch
Rulings Output
A rulings data file can be generated from the input parametric model (when Activate rulings active) and saved to disk by means of the "-orulings" flag.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -orulings blade.dat -batch
TRAF outputs
TRAF format files can be generated in a specified folder "traf-folder" from the input parametric or geometric model and saved to disk by means of the "-otraf" flag.
This flag requires an input parametric or geometric file and is additive to "-par" or "-geom" flag.
Example:
> autoblade131 -par blade_org.par -otraf traf-folder -batch
Parameters input
The flag "-iparam" can be used to import a list of parameters that will replace the parameters of the current model. It must be followed by the absolute path to the parameter file.
> autoblade131 -iparam /home/usr/blade.param -batch
Here is an example of a parameter file:
SWEEP_BETA1	5
SWEEP_BETA2	-2.5
LEAN_BETA2	2.5
LEAN_BETA1	-5
For each line, the name of the parameter should be written followed by its value.
Parameters Output
The flag "-oparam" can be used to output all active parameters to a file. It must be followed by the absolute path to the parameter file.
> autoblade131 -oparam /home/usr/blade.param -batch
This flag requires an input parametric or geometric file and is additive to "-par" or "-geom" flag.
Example:
> autoblade131 -par blade.par -oparam blade.param -batch

CONTENTS
CHAPTER 1. GETTING STARTED
Introduction
1.1
1.2 How To Use This Manual
1.3 First Time Use
1.4 How to start AutoBlade™
1.5 Required Licenses
CHAPTER 2. GRAPHICAL USER INTERFACE
2.1 Menu Bar
2.1.1
2.1.2
2.1.3 Geometry Menu
File Menu
Edit Menu
Import
Import parameters
A.
B.
C. Export Options
D. Export parametric model
E. Export as '.geomTurbo'
F. Export as IGES
G. Export as Parasolid
H. Export solid sector geometry
I. Export as VDA-FS
J. Export rulings
K. Export parameters
L. Export geometry
M. Model Topology
N. Parameter List
O. Special functions
P. Geometry Options
2.1.4 Analysis Menu
2.1.5 View Menu
2.1.6
Tools Menu
2.1.7 Modules Menu
Icon Bar
2.2
2.3 Dialogs & Windows
2.4 View Layout & Graphs
2.4.1
2.4.2
Blade-to-blade view options
3D view options
2.5 Viewing Control Buttons
2.6 Quick Access Pad
Target Settings subpad
2.6.1
2.6.2 Model Editor subpad
2.6.3
Fitting Control subpad
2.7 Graphical Interactions
2.7.1 Monitoring of Controls
AutoBlade™ 13.1 User Guide
14
18
18
24
24
24
26
26
33
34
34
34
34
35
36
39
39
40
40
48
49
53
56
58
58
59
60
61
62
63
66
69
70
74
78
Edition of Control
2.7.2
2.7.3 Meridional View
2.7.4
Tool Stack
2.7.5 Overlays
2.8 Batch Mode
CHAPTER 3. AUTOBLADE™ MODELLER
3.1 Topology & Parameters
3.1.1 Meridional Contours
3.1.2
Stream Surfaces & Spanwise Location
A. Surface Setup
B. Rulings (for flank-milled blade only)
C. Spanwise Locations
D. Stream Surfaces Spanwise Location
E. Views
Blade Meridional & Tangential Locations
A. Stacking Point
B. Meridional Location
C. Tangential Position
3.1.3
3.1.4 Main Blade
A. Construction Plane
B. Camber Curve Definition
C. Suction & Pressure Side Curves
D. Leading & Trailing Edges
3.1.5 Optional Splitters
3.1.6
Technological Effects
3.1.7 Non-Axisymmetric Hub/Shroud
A. Space of Definition
B. Method 'across channel'
C. Method 'along channel'
D.
E. Graphical and Exported Outputs
F. Settings Dialog
Solid Body
Topological Compatibility Issues
Inlet & Outlet Offsets
3.1.8
3.1.9
3.2 Optional Quantities
3.2.1
3.2.2
Selection Notebook
A. Sampling
B. Scalar Values
C. Edges Control
Summary Table
3.3 Geometry Analysis
3.4 Parametric Report
CHAPTER 4. AUTOBLADE™ FITTING
4.1 Preparing Target Geometry
AutoBlade™ 13.1 User Guide
85
88
92
92
94
100
101
109
110
117
120
121
124
125
126
126
135
137
138
141
149
177
179
185
194
194
195
199
201
201
201
203
209
214
217
218
224
236
238
239
CHAPTER 1.
GETTING STARTED
Welcome to the AutoBlade™ User manual - a presentation of the NUMECA parametric blade modeller
for turbomachinery blades. This chapter presents the basic concepts of the AutoBlade™ and shows how
to get started with the program by describing:
In this section
1.1 Introduction
1.2 How To Use This Manual
1.3 First Time Use
1.4 How to start AutoBlade™
1.5 Required Licenses
14
1.1
INTRODUCTION
What is AutoBlade™?
AutoBlade™ has been developed in the context of a wider product able to provide to the user a
complete and very efficient environment for the design of turbomachinery blades. AutoBlade™
includes two modules: modeller and fitting.
The blade modeller is an advanced geometry modeller for three-dimensional turbomachinary
blades.
The blade fitting is a unique and general purpose module which allows to import blade geometries
and determine parameter values that best fit the provided geometry.
AutoBlade™ is integrated into the NUMECA CFD package FINE™/Turbo and benefits from
the expertise accumulated with the design algorithms available in this complete design
environment. AutoBlade™ is also available as an edition and monitoring tool
inside the
FINE™/Design3D module.
Features
AutoBlade™ can define various types of axial, radial or mixed flow turbomachinary blades that
can be rotating or stationary. AutoBlade™ has been extensively tested on a wide range of
applications:
l compressors (axial or radial),
l turbines (axial or radial),
l fans,
l pumps,
l inducers,
l blowers,
l turbochargers,
l return channels.
Project Management
To manage complete blade designs, AutoBlade™ integrates the concept of project. A new file
management is used to handle and store the project and history of the changes (FIGURE 1.1).
FIGURE 1.1
Project management
In AutoBlade™, each interactive edition is stored in a memory stack for undo and redo
operations. In addition, some operations can be marked as persistent and saved to disk. These
persistent models are saved in a subdirectory and referenced in the project file. When reloading
the project, these steps are retrieved and automatically fill the undo stack.
An AutoBlade™ project involves the parametric file, the target geometry file (for fitting) and
some persistent state files:
l .abp file: the project file,
l .par file: the current parametric model,
l .geomTurbo and .geomTurbo.xmt_txt files: the target geometry file. When the turbomachine
the file
is specified using CAD import (more details in AutoGrid™ User Manual),
".geomTurbo.xmt_ txt" is used in addition of the ".geomTurbo" file and should not be
removed.
l a directory "project_name" with the persistent states and related files.
l model####.abm: the design step,
l overlay####.abm: the inserted overlay,
l model####.his: the fitting convergence history file for the design step model####.abm,
l model####.fit: the fitting log file for the design step model####.abm.
FIGURE 1.2
Project structure on disk
Some special characters with accents, such as ü, ë and ê et al., are not allowed in the path and project
names.
1.2
HOW TO USE THIS MANUAL
Outline
This manual consists of three distinct parts:
l Getting Started and Graphical User Interface: introduction and description of the interface,
l AutoBlade™ Modeller,
l AutoBlade™ Fitting.
At first time use of AutoBlade™ it is recommended to read this first chapter carefully and
certainly sections First Time Use to Required Licenses of this chapter. The Graphical User
Interface chapter gives a general overview of the AutoBlade™ interface and the way to manage a
project. The AutoBlade™ Modeller chapter presents the NUMECA parametric blade modeller
for
functionalities available in
AutoBlade™. The AutoBlade™ Fitting chapter presents the fitting module which allows to
import an existing blade geometry and convert it to the AutoBlade™ format.
turbomachinery blades.
It describes all
the geometrical
Conventions
Some conventions are used to ease information access throughout this guide:
l Commands to type are in italics.
l Keys to press are in italics and surrounded by <> (e.g.: press <Ctrl>).
l Names of menu, sub-menu items and names of buttons in dialog boxes are in bold.
l Numbered sentences are steps to follow to complete a task. Sentences that follow a step and
are preceded with a dot (•) are substeps; they describe in detail how to accomplish the step.
Blue text in a blue box indicates an important note
1.3
FIRST TIME USE
Basic Installation
When using AutoBlade™ for the first time it is important to verify that AutoBlade™ is properly
installed according to the installation note. The installation note provided with the installation
software should be read carefully and the following points are specifically important:
l Hardware and operating system requirements should be verified to see whether the chosen
machine is supported.
l Installation of AutoBlade™ according to the described procedure in a directory chosen by the
user and referenced in the installation note as 'NUMECA_INSTALLATION_DIRECTORY'.
l A license should be requested that allows for the use of AutoBlade™ and the desired
component and modules . The license should
be installed according to the described procedure in the installation note.
l Each user willing to use AutoBlade™ or any other NUMECA software must perform a user
configuration as described in the installation note.
When these points are checked the software can be started as described in the installation note or
the How to start AutoBlade™ section of this user manual.
1.4
HOW TO START AUTOBLADE™
In order to run AutoBlade™, the following command should be executed:
1. On Linux platforms type:
autoblade# -print <Enter>
where # is the version number to be used (131).
2. On Windows click on the AutoBlade icon in Start/Programs/NUMECA Software/Fine# or
Start/Programs/NUMECA Software/AutoBlade# . Alternatively AutoBlade™ can be
launched from a dos shell by typing:
<NUMECA_INSTALLATION_DIRECTORY>\fine#\bin64\autobladex86_64
or
<NUMECA_INSTALLATION_DIRECTORY>\autoblade#\bin64\autobladex86_64
where NUMECA_INSTALLATION_DIRECTORY is the installation directory chosen by
the user and # is the number corresponding to the version to be used.
3. Press the first button from the main tool bar or select item File/New from the main menu. A
small dialog pops up. This allows the user to start from scratch or create a new project from an
existing parametric model. If the user selects Start from an existing model, the button Ok is
grayed until a valid parametric file has been selected.
FIGURE 1.3
File/New dialog
When the button Ok is clicked, a file chooser dialog opens. Select a folder under Directories
field, then type a name in the Files field and click Ok.
White spaces should be avoided in the file name.
FIGURE 1.4
Model creation dialog box
A default blade model appears in the four views layout as shown in figure below.
FIGURE 1.5
AutoBlade™ interface
To start working in AutoBlade™ as a standalone modeller from the FINE™/Turbo interface, the
following steps should be followed:
l Launch the FINE™/Turbo interface. Please refer to the FINE™/Turbo User Manual for
further details on how to start the FINE™/Turbo interface.
l Once FINE™/Turbo interface is started, a Project Selection window appears. Press Cancel to
close this dialog and get full control over the main window.
FIGURE 1.6
Project selection window
l Select Modules/AutoBlade item from the main menu bar. A confirmation dialog opens with
the message This will start AutoBlade module. Press Ok to continue.
FIGURE 1.7
FINE™ interface
l Press the first button from the main tool bar or select item File/New from the main menu. A
file chooser dialog opens. Select a folder under Directories field, then type a name in the Files
field and click Ok.
1.5
REQUIRED LICENSES
The AutoBlade™ modeller module requires the AutoBlade™ license. That allows to create a
parametric representation of a 3D turbomachinery blade starting from a template or an already
existing parametric representation.
The AutoBlade™ Fitting module requires the AutoBlade™ Fitting license. That allows to create
a parametric representation of a 3D turbomachinery blade from a points representation (in
geomTurbo format).
The AutoBlade™ solid body module requires the AutoBlade™ solid domain license. That
allows to create a Solid Body.
The run mode selection list in FINE™/Design3D environment displays only the run modes for
which a license is available.
CHAPTER 2.
GRAPHICAL USER INTERFACE
This chapter describes the AutoBlade™ interface, a powerful and interactive interface for three-
dimensional turbomachinary blade designs. The AutoBlade™ interface offering
l interactive control of the parameters defining the model (point drag and keyboard input),
l full undo/redo capability on operations,
l multiple overlays to compare the edited geometry to one or previous states,
l advanced error reporting
In the following sections, the items in the interface are described in more detail.
Axis Conventions
Axis names and conventions are summarized in this section.
The XYZ axis system is positively oriented such that the rotation axis of the machinery is the Z-axis
(FIGURE 2.1). The azimuthal angle θ is measured from the positive X axis and expressed in radians.
FIGURE 2.1
Axes and conventions in AutoBlade™
The meridional plane (Z,R) for the definition of hub, shroud and traces of the stream surfaces
corresponds to (Z,X) plane. The meridional length m of endwall curves and traces is often used as
abscissa for the location and the construction of the blade sections .
The tangential plane is (X,Y), but (span,θ) plane is used for the tangential stacking .
TABLE 2.1 Axis conventions and special coordinates
Name Description
vertical radial direction (θ=0)
horizontal radial direction (θ=π/2)
axial direction
non dimensional axial length computed as (Z-ZRef)/(Rshroud(ZRef)-Rhub(ZRef)) where ZRef is
the axial reference location for the blade sections
radius
non dimensional radius computed as (R-RRef)/(Zshroud(RRef)-Zhub(RRef)) where RRef is the
reference radius for the meridional location of the blade sections
tangential angle measured from the positive X axis (in radians)
distance measured along a curve in the meridional (Z,R) plane and defined as the integral of
m' or
integral of
(
)
span
spanwise location parameter - expressed as a fraction of the local distance between reference
stream surface traces in the meridional (Z,R) plane
Units
No unit system is currently implemented inside AutoBlade™. In particular, no information about units
is saved in the ".geomTurbo" file. Consistency is thus the ruling word. All angles in AutoBlade™ are
measured in degrees unless differently stated.
There are however some exceptions:
1. Some lengths are normalized. This is the case of parameters like TSS(j) and TPS(k) .
2. The angle θ is expressed in radians in the lean law graph and in the section view plane (view 3).
2.1
MENU BAR
The menu bar of AutoBlade™ consists in 6 entries File, Edit, Geometry, Analysis, View and
Modules (only available if AutoBlade™ is started from FINE™ GUI):
FIGURE 2.2
Menu bar
2.1.1
File Menu
This menu contains the usual commands for the file management and session settings.
Some entries may appear greyed out, meaning they cannot be activated in this context. This typically
occurs when
l no model is loaded in the interface (Save and Save As entries are not available),
l AutoBlade™ is accessed as a tool from Design3D interface (only Save and Preferences entries
are available).
New
This menu creates a new AutoBlade™ project. A small dialog pops up when activating File/New
or clicking the corresponding icon in the main toolbar, as shown in FIGURE 2.3.
FIGURE 2.3
Create a new project
This allows the user to start from scratch or create a new project from an existing parametric
model. The Ok button is greyed until a valid parametric file has been selected. When Ok is
clicked, a file browser is opened (in both cases) to select a new file name for the project.
White spaces should be avoided in the file name.
Open
There are two ways to open an existing project file:
Use File / Open menu
This menu opens an existing AutoBlade™ project. The user can open a project file (*.abp)
directly. As an alternate solution, the filter in the file browser can be changed to parametric file
(*.par). In the latter case, AutoBlade first tries to locate the corresponding project file (same path
and name) and loads it or select the parametric file as starting model and calls a second file
browser for the new project name (acts as File/New with starting model).
Select File From the List of Files in File Menu
The File menu lists the names of the five most recent projects that have already been opened.
Clicking on a project name from this menu will open it. When clicking on a project name in the
File menu, AutoBlade first prompts for save if the current project is modified.
When a project file from the saved list is not physically present on disk at startup, it is deleted from
the list.
Save
The File/Save menu stores the project on disk.
Save As
The File/Save as menu is used to store the current AutoBlade™ project to a new location.
Properties
Description
The tab Description allows the user to add customized information in the project.
Parasolid
Under the tab Parasolid, the user can applies an internal scaling factor and activate the solid
model.
The Internal scaling factor for Parasolid is used to keep the range of data within suitable limits
internally. This scale factor has no visual impact on the data in the views and is independent of the
Edit/Scale command or the target geometry scale factor.
The scaling factor is automatically adapted in the following cases if the bounding box extent is
smaller than 0.01 or larger than 100.0:
l at import or read a parametric model coming from a previous version,
l at adaptation step on a target geometry (fitting module).
The user can also activate this scaling and change the scaling factor.
By default, sheet models are generated for all models, which are used for 3D view and CAD
surfaces output. The button Solid model allows the user to build solid body for the designed blade
in addition to the sheet models and check it in the 3D view.
The following limitations apply to the solid model:
l the solid model is not compatible with ruled blades using late rounding option.
l when the solid model is active, the bottom and tip closure surfaces are not defined as part of
revolved surfaces.
l Both sheet and solid models require more time for update, especially when many sections and
many points are involved in curves. In Design3D, the update has significant impact in the
optimization phase when using the ANN (as the ANN needs updated quantities as input, the
parametric model is updated for each sample)
Report
The tab Report shows the general parametric information.
Preferences
The menu File /Preferences opens the Preferences dialog that gives access to some project
specific and global settings.
Session page
Amount of undo/redo is used to specify the maximum number of the undo/redo steps. When the
limit is achieved, the oldest editions are deleted, but the persistent steps are kept with a higher
priority than volatile steps.
Parasolid tolerance is used to set the tolerance to treat Parasolid geometry.
The button create backup files (.bak) is used to make a backup of the existing project file and the
data directory at saving.
Curves page
Different styles and colors are used to draw and highlight the graphical items in the main interface
of AutoBlade™. Most curves appear in foreground color, but the graphical representation of their
control polygon, nodes and angular parameters are drawn in a different color. If an item can be
picked, monitored or selected, its color changes according to the imposed color selected in the
Curvestab from the File/Preferences menu by left-clicking on the color.
FIGURE 2.4
Curves color control
Display page
Furthermore, the background and foreground colors are controlled in the Display tab from the
File/Preferences menu.
FIGURE 2.5
Background/foreground colors control
Quit
Select the menu File/Quit to quit the interface.
2.1.2
Edit Menu
This menu contains the Undo and Redo commands that allow to respectively revert and recover
changes to the parametric model.
Furthermore, the Scale command allows to scale the parametric model.
FIGURE 2.6
Scale parametric model
2.1.3
Geometry Menu
Most of the options available in this menu are also available as accelerated buttons (top button
bar) or as side buttons (left tool box). This menu consists in four groups of commands:
A.
Import
This menu allows:
l to import a geometry file previously designed under AutoBlade™. Clicking the Import a
parametric file button will launch a browser dialog to select an existing parametric file.
l to create a new project from a template. Design is easier if a template similar to the desired
geometry is first loaded. The template can be loaded by selecting the appropriate item under
the Import a parametric template box.
FIGURE 2.7
Import menu
A general rule to ensure a quick design is to first load a template similar to the anticipated final
configuration. Then topological choices can be fixed and eventually the values of the corresponding
parameters are modified.
When a parametric file is selected in the menu, the template name is reset to "NONE" and when a
template is chosen, the file name is reset to "none". This behavior prevents ambiguous choices, since
those two options exclude each other.
It is possible to define an existing parametric model as a template. To do so, the existing
parametric file must be copied in the directory:
<NUMECA_INSTALLATION_DIRECTORY>/fine#/COMMON/templates/ (on LINUX)
<NUMECA_INSTALLATION_DIRECTORY>\fine#\bin\templates\ (on Windows)
or
<NUMECA_INSTALLATION_DIRECTORY>/autoblade#/COMMON/templates/ (on LINUX)
<NUMECA_INSTALLATION_DIRECTORY>\autoblade#\bin\templates\ (on Windows)
Then the new template will appear under the Import a parametric template box.
B.
Import parameters
The menu Geometry/Import parameters allows to import a parameter file with default
extension ".param" and modifies the parameters defining the current model. Each line in the
.param file defines one parameter with the name and the expression (or the value) of the
parameter. The user can make this .param file manually or modify the exported .param file, see
Export parameters section. For example, importing the following file will set the parameter HUB_
Z1 = -0.03 and set the parameter SHROUD_R2= "SHROUD_R1" (expression).
All the lines in the .param file starting with # will be considered as comment lines.
C. Export Options
The Geometry/Export options... menu contains various settings controlling the exportation of
the parametric blade sections in both ".geomTurbo" and CAD formats.
Common Settings
FIGURE 2.8
Common Settings
By default, primary and parametric blade sections are assumed for export. Primary blade sections
are fully defined by parameters. Parametric sections are only defined to capture the imposed
stacking laws. At all spanwise positions where a parametric section has been placed,
the
parameters are interpolated from the primary sections and used to create an additional blade
section. See Stream Surfaces Spanwise Location for more detail on primary and parametric
sections.
In general, this default selection to export the primary and parametric sections is recommended.
However, a drawback of the parametric sections is that the interpolation of the parameters can
lead to non physical values such as a negative leading edge radius. Therefore, it is possible to use
discretized sections to export an arbitrary amount of sections to the ".geomTurbo" file.
Discretized sections are quite similar to parametric sections apart from the fact that they are
obtained through an interpolation of the blade geometry in point coordinates instead of the
parameters. This has the advantage that the geometrical interpolation between realistic blade
sections always leads to realistic full blade shapes. At least two different spanwise locations must
be entered in the Spanwise locations field. Span values 0.0 and 1.0 make up the default minimal
set.
Discretized sections are obtained by interpolation of point coordinates from both primary and
parametric sections curves with respect to the span. Interpolation type controls the way
discretized sections are computed from primary and parametric sections. Cubic spline is the
default choice, but a linear law is always applied in case an extrapolation is required . The Discretized sections are not allowed if the rounded tip topology is used.
TABLE 2.2 Exported sections
Output blade sections
Action
Primary & parametric sections
all primary and parametric sections are exported
User defined discretized sections
only discretized sections are exported
The output should at least contain two sections.
The amount of discretized sections should be greater than the amount of parametric and primary
sections in order to tightly capture the design intent in the geometry file. For instance, if three
primary sections are defined at span values 0.05, 0.5 and 0.95 but only two discretized sections are
interpolated at span values 0.0 and 1.0, the exported geomTurbo file will not contain the non linear
spanwise evolution of the blade shape. Choosing three or more discretized sections can solve this
problem if span values are chosen with equal spacing along the spanwise direction.
Discretized sections are quite similar to parametric sections apart from the fact that they are
obtained through a regular XYZ interpolation of the blade geometry in point coordinates instead
of the parameters.
To improve interpolation for high staggered blade as centrifugal impeller, an option allows to
export interpolated sections built from the reduced meridional coordinate of the camber curve and
based on cylindrical coordinates R,θ,Z.
The approach is not directly accessible from templates or in models built from scratch in
AutoBlade™ GUI. The keyword "ALLOW_ZRTHETA" must be added manually at the end of
the section "SECONDARY_ SECTIONS" of the parametric ".par" file to access the Z,R,θ
interpolation approach in AutoBlade™ GUI as presented in the dialog box below.
FIGURE 2.9
Export Z,R,θ interpolated sections
When using the Z,R,θ interpolation approach, a distribution is prepared for the reduced
meridional coordinate 'm', in [0,1] range, 0 corresponding to the leading edge, 1 to the trailing
edge. This distribution allows clustering in both leading and trailing edge areas and shows a
central region with constant
intervals ( Number of constant intervals ). Three different
distributions are available and their default settings are listed in the following table.
TABLE 2.3 Distribution settings when Z,R,θ interpolation approach
GUG
GU
UG
Geometric-Uniform-Geometric
Geometric-Uniform
Uniform-Geometric
Number of points for curves
Number of constant intervals
Total ratio
201
100
200
(10 if Blunt/Blunt)
201
100
200
201
100
200
Application
Rounded/Rounded
Rounded/Blunt
Blunt/Rounded
Blunt/Blunt
For each spanwise value i and each point j in [0,1] range, the camber coordinates and the local
thickness are recomputed.
R(i,j) = Rhub(j) + span(i) x (Rshroud(j) - Rhub(j))
θ(i,j) = θhub(j) + span(i) x (θshroud(j) - θhub(j))
Z(i,j) = Zhub(j) + span(i) x (Zshroud(j) - Zhub(j))
X(i,j) = R(i,J) x cos(θ(i,j))
Y(i,j) = R(i,J) x sin(θ(i,j))
TSS(i,j) = TSShub(j) + span(i)^A x (TSSshroud(j) – TSShub(j))
TPS(i,j) = TPShub(j) + span(i)^A x (TPSshroud(j) – TPShub(j))
The exponent A is by default set to 1.0 but allows additional control over the thickness by
changing the value in the range [1e-6,1e6].
The Z,R,θ interpolation approach is restricted to the following settings:
l interpolated stream surfaces,
l (m,β) and (m',θ) construction planes,
l thickness addition mode, excluding flank-milled options (rulings and late rounding),
l blades defined by exactly two primary sections and no parametric section.
geomTurbo Settings
FIGURE 2.10
geomTurbo Settings
This AutoBlade™ output format, carrying a "geomTurbo" extension, is used as input by the mesh
generator AutoGrid5™.
The names of the blades can be altered and saved by means of the field Blade and Name. The
option Stick edges is used to fit leading and trailing edges of pressure and suction sides along the
spanwise direction when the leading and/or trailing edge are very curved (i.e. twisted blade).
The outputted geometry can be Full or Partial, which is controlled by the option Content.
The option Enforce CAD output allows the user to output the CAD surfaces to the .geomTurbo
file, instead of the surfaces defined by coordinates. Please note that some options specific to
sections are not available when this CAD is active, such as the expansion factors.
The Curve format selector allows one among two systems of units for export: XYZ format that
uses cartesian coordinates (X,Y,Z) or ZRTH format that uses cylindrical coordinates (Z,R,θ). The
axis conventions are explained in the Axis Conventions section.
A Scaling factor option allows a direct scaling of the geometry. This option is independent of the
geomTurbo 'units' keyword and applies to any point or curve.
The option Enforce ruled surfaces allows, when two sections are exported, to force strict
compliance of the side curves. This option adds the special keyword 'uniform_parametrization' at
the end of the format field for suction and pressure side curves.
The option Exchange sides allows to exchange the pressure and suction sides of the blade to
respectively suction and pressure sides.
The option Reverse theta orientation allows to reverse the theta orientation of the blade.
The option Apply a rotation allows to rotate the selected blade around a user-defined axis. The
axis and anchor point fields expect three floating point coordinates while the angle value is given
in degrees.
FIGURE 2.11
Apply blade rotation parameters
To use the exported geomTurbo file in AutoGrid5™, it is essential that the blade definition intersects
the hub and the shroud. Therefore it may be necessary to export a sections at, for example, span
values -0.05 and 1.05.
The scaling factor only applies to geomTurbo.
CAD Settings
FIGURE 2.12
CAD Settings
CAD export can be customized independently of the 3D view settings. The main and splitters
blades are exported by default.
The units of the IGES file can be imposed by the user (Length unit). As for the "geomTurbo"
export, you can apply a rotation for both Parasolid and IGES files.
VDA-FS Settings
FIGURE 2.13
VDA-FS Settings
When exporting to the VDA-FS format, the ruling directions are exported by default for ruled
blades. Deselecting the button include ruling directions will cancel the ruling direction export.
The ruling directions are used as reference to generate the side surface by means of the Parasolid
library. Usually a dozen of links are sufficient for that purpose. If needed, the user can also refine
the ruling directions during the export. Clicking on the radio button refine ruling directions will
activate the refinement during the export. The number of directions are used to define the number
of sampled directions on each blade side. The ratio at rounded edge is the ratio between max
spacing and min spacing in the U-direction. In addition, the directions can be extended outside the
channel as a percentage [0,0.499] of the distance between the hub and the shroud.
D. Export parametric model
The menu Geometry/Export parametric model... opens a file chooser and prompts for a
location where to save the parametric model with default extension ".par".
E. Export as '.geomTurbo'
The menu Geometry/Export as geomTurbo... opens a file chooser and prompts for a location
where to save the geomTurbo export with default extension ".geomTurbo".
In stand-alone mode, the Save operation does not export the geomTurbo output automatically. On the
contrary, each parametric model is saved with its geomTurbo export in a FINE™/Design3D project!
F. Export as IGES
The menu Geometry/Export as IGES... opens a file chooser and prompts for a location where to
save the IGES export with default extension ".igs".
G. Export as Parasolid
The menu Geometry/Export as Parasolid... opens a file chooser and prompts for a location
where to save the blade geometry in Parasolid format as independent sheet bodies.
If a solid body is requested, the user can check the Solid model option under the Parasolid tab in
the File/Properties... menu. The blades will be exported as closed volumes instead of open
sheets.
H. Export solid sector geometry
The menu Geometry/Export solid sector geometry... opens a file chooser and prompts for a
location where to save the merged blade and solid body in parasolid format, see Solid Body for
more details.
The exported solid sector geometry may be a single sector or the full 360 degree body, depending
on the Repetition option in the menu View / 3D view options under the tab Geometry.
FIGURE 2.14
Examples of exported solid sector geometry
I.
Export as VDA-FS
The menu Geometry/Export as VDA-FS... opens a file chooser and prompts for a location
where to save the blade curves in VDA-FS format.
When exporting the ruling directions to VDA-FS with late roundings and/or cutoff, the ruling
directions defining the initial blade surface before applying late roundings and/or cutoff are
exported. These directions do not match the final blade surfaces because the final blade is not
ruled after applying late roundings and/or cutoff.
When exporting to the VDA-FS format, all curves are exported and the data is written as sets of
points. The name of the exported curves are following the name conventions below (where # is
the index of the blade/splitters and ??? is the index of the directions):
Component Description
Hub
Hub curve
Shroud
Shroud curve
Hub gap
Hub gap curve (possibly multiple blades)
Mean line on gap surface (revolved gap surface)
Suction curve on gap surface
Pressure curve on gap surface
Name
HUB
SHROUD
B#HGAP
B#HGAPML
B#HGAPSS
B#HGAPPS
Component Description
Shroud gap
Tip gap curve (possibly multiple blades)
Mean line on gap surface (revolved gap surface)
Suction curve on gap surface
Pressure curve on gap surface
Name
B#SGAP
B#SGAPML
B#SGAPSS
B#SGAPPS
Blade rulings Ruling directions as a set of 4 aligned points if extended (reduced to 2
B#RSS???
Blade
sections
points otherwise) :
Suction side directions (numbered from LE to TE)
Pressure side directions (numbered from LE to TE)
Suction and pressure side curves, for each blade:
Hub camber curve
Shroud camber curve
Hub suction curve
Shroud suction curve
Hub pressure curve
Shroud pressure curve
B#RPS???
B#CB0001
B#CB0002
B#SS0001
B#SS0002
B#PS0001
B#PS0002
J. Export rulings
The menu Geometry/Export rulings... opens a file chooser and prompts for a location where to
save the geometry with default extension ".rln" for flank-milled designs.
The .rln file includes the following parts:
Rulings and rounding
Rulings
Ruling directions are defined independently for each blade.
Each ruling direction is defined by its two ending points in 3D coordinates (X, Y, Z, R and θ) on
hub and tip sections. This original definition is based on the 3D camber curves.
For each ruling direction, two additional links are defined for suction and pressure sides. These
links are directly built from the original camber ruling directions on the side curves by thickness
addition.
The suction and pressure links belong to the original ruled surfaces and do not take the effects like
blade cutoff or late elliptical rounding into account.
Optional elliptical rounding & cutoff
Blade cutoff
When blade cutoff is applied, the following data is written to the .rln file
CUTOFF_DATA
Then for leading edge cutoff:
CUT_LOCATIONS_FOR_LE
HUB_LOCATION_Z [floating point value]
HUB_LOCATION_R [floating point value]
SHROUD_LOCATION_Z [floating point value]
SHROUD_LOCATION_R [floating point value]
And/or for trailing edge cutoff:
CUT_LOCATIONS_FOR_TE
HUB_LOCATION_Z [floating point value]
HUB_LOCATION_R [floating point value]
SHROUD_LOCATION_Z [floating point value]
SHROUD_LOCATION_R [floating point value]
Elliptical rounding
When late elliptical rounding is applied, the topology and b/a ratios are included in the output.
This section is announced by the line:
LATE_ELLIPTICAL_ROUNDING
Then, for rounding at the leading edge for hub section as an example:
HUB_LE_RADIUS_RATIO [floating point value]
HUB_LE_ROUNDING [rounding topology]
where [rounding topology] stands for one of the three identifiers:
l EXTERNAL for external rounding (adds material to the section),
l INTERNAL for internal rounding (preserves the original edge point),
l CUTBACK for special cutback option (enforces the minimum or maximum meridional
location of the blade section)
If no elliptical rounding is applied on the edge of the section, a single line is written:
HUB_LE_ROUNDING NONE
When elliptical rounding is not active at all, the next line is written:
BUILT_IN_ROUNDING
Camber and thickness
For each section, the hub and tip camber curves are written to the file with their original internal
sampling. The output consists in the following fields:
l the cylindrical coordinates Z, R and θ,
l the wrap angle β,
l the meridional coordinate m,
l the reduced meridional coordinate m/m*, where m/m*=(m-mStart)/(mEnd-mStart), mStart and mEnd
are the start and end points of the camber curve, respectively.
l the local thickness value (on the stream surface).
The local thickness value is the thickness measured on the stream surface and not as a 3D distance.
θ angle is given in radians.
β angle is given in degrees.
Final side curves
The final side curves (suction and pressure sides) are written for hub and tip sections in
coordinates X, Y, Z, R, θ, m and m'.
This output corresponds to the final side curves, after blade cutoff and elliptical rounding if
applied.
K. Export parameters
The menu Geometry/Export parameters... opens a file chooser and prompts for a location
where to save the whole list of the parameters with default extension ".param". All the parameters
defining the current model are exported. Each line in the .param file defines one parameter with
the name, the expression (if defined) and the value of the parameter.
L. Export geometry
The menu Geometry/Export geometry... allows the user to output the coordinates of the selected
curve.
The user should select one curve type first. Depending on the selected curve, the user may be able
to select the coordinate system and the location of the curve (blade index and section index) for
output. Then, clicking on the button Save will opens a file chooser and prompts for a location
where to save the selected curve with default extension ".dat".
The format of the .dat file is as follows:
l The first line is a comment line indicating the coordinate system.
l The second line defines the number of the discrete points.
l The next lines list the data of each point.
M. Model Topology
The topology has been split into nine distinct steps: Endwalls, Stream surfaces, Stacking laws,
Main blade, Splitter blades, Effects, Non axi hub, Non axi shroud and Solid domain. The
available topologies are explained in the Model Editor subpad and the AutoBlade™ Modeller
chapter in more detail.
N. Parameter List
The parameter list
corresponding button in the main tool bar.
is accessible through the menu item Geometry/Parameter list or the
This menu allows the designer to access the whole list of parameters defining the current model.
Most parameters can be read and changed interactively in the graphical views. Furthermore, by
clicking in the Expression entries (FIGURE 2.15), additional mathematical expressions allow
some parameters to be defined as a function of one or more other parameters and help reduce the
space of independent parameters. So this menu is especially useful for the advanced user who will
be able to quickly modify several parameters. There are a few exceptions however that make this
list necessary:
l The bounds of the parameters can be checked and changed in the list. To show them, simply
activate the option View/Show parameter bounds. This topic is useful in Design3D mode
only.
l The scale of the parameters can be checked in the list. To show it, simply activate the option
View/Show parameter scale. This topic is useful in Design3D mode only.
l The expression of the parameters can be checked and changed in the list. To show it, simply
activate the option View/Show parameter expressions.
l Some parameters do not appear in the graphics area. For instance, meridional chord
parameters, edge radii in construction curves mode or the blade repetition number are only
available in the Parameter list or in the topology menus.
FIGURE 2.15
Parameters menu
All parameters are listed in specific pages and depend on the chosen topological settings. The
names of the parameters are listed in section of the AutoBlade™ Modeller chapter after the
corresponding topology setting. To find information about a precise parameter name, please look
for the parameter keyword in the index located at the end of this manual.
For a fast design process, it is suggested that all topological settings are fixed before editing their
corresponding parametric values.
All the parameters have a double precision with about 16 decimal digits.
The next few paragraphs explain the additional functions available in any grid of parameters.
Expression - Dependency of Parameters
When checking the small button in front of an Expression entry, the corresponding parameter can
be controlled by a mathematical expression in such a way that its value is defined as a function of
one or more other parameters.
This new ability offers several advantages:
l design changes are easier since fewer parameters need to be changed,
l optimization is faster thanks to a reduced space of search (reduced amount of free parameters),
l geometrical constraints are easier to express avoiding the definition of complex penalties in the
objective function.
With the above features, AutoBlade™ will be able to support complex parametric dependencies,
where a reduced list of independent parameters can be built. All dependent parameters are
internally evaluated, so that the whole model can be built from this limited subset of independent
parameters. This may help decrease the dimension of the parametric space in optimization and
achieving special topological goals like
l constant or incremental chord length for all primary sections,
l identical radius at trailing edge,
l symmetric thickness at both edges.
Enabling / Disabling Expression
When the Expression field is unchecked, the bounds are unlocked and may be edited.
When an expression is entered and activated, the value field becomes read-only and shows the
last known evaluation of the expression.
The check button activates or deactivates each expression, allowing the designer to disable the
expression and restore it later.This is especially useful in fitting projects.
User defined Parameters
FIGURE 2.16
User defined parameters
Additional parameters can be introduced under the group user(FIGURE 2.16) and can serve as
reference for the dependencies. For instance, a reference length can be defined and used as factor
in expressions for some dependent lengths in the model.
Here is an example using user defined parameters. Assuming that
,
,
, and the user wants to define
, the user can define an additional
optional parameter X and make P2 dependent on P1, P3 and X:
In this case, P2 will follow X but is automatically bounded by P1 and P3.
Editing Expression
The expression editor (FIGURE 2.17) is invoked by right-clicking over the Expression field. The
full lists of variables (parameters), constants, operators and functions allow the designer to enter
and edit complex dependencies.
The parser is able to recognize the operators, grouping symbols and functions, but also numerical
data (floating point) and names of variables.
FIGURE 2.17
Expression editor window
Expressions allow the following operators and functions:
l Arithmetic: +, -, *, /,^
l Unary operators: +, -
l Unary functions: abs, sin, cos, tan, sinh, cosh, tanh, asin, acos, atan, sqrt, log, log10, exp,
round, trunc
l Two arguments functions: atan2
l Three arguments function: switch
l Multiple arguments functions: min, max
l Logical operators: &&, ||
l Comparison operators: <, <=, >, >=,==,!=
l User-defined Functions
The precedence of the operators occurs in the following order of decreasing priority:
1. grouping parentheses and functions,
2. exponent ^,
3. * and / ,
4. + and -.
Grouping symbols '(' and ')' are allowed to constrain associativity and precedence or to separate
the arguments of a function from the rest of the expression. In case of multiple arguments, the
comma is mandatory as separator.
Cyclic dependencies are not supported. For instance, the following system is not accepted by the
solver of constraints because B is function of C but C is also a function of B:
A=1.0
B=D-C
C=A+B
D=2.0
User-defined Functions
The user interface allows the user to define special functions, see the Special functions section for
more detail.
Export Parameters
The button Export group (at the bottom of the grid) allows to save on disk the group of
parameters appearing in the corresponding window. A dialog box then prompts for a text file
name.
Simple Use of Parameter Grid
Basic edition
To change a parameter value in the grid, simply edit the field to reflect the new value.
There is no need to key in <Return> or <Enter>: the model will not be updated unless Ok or
Apply button is clicked.
If a value is set to an incorrect value, it will be corrected and a message will be issued. For instance, a
radius cannot be negative, so a default epsilon will replace the wrong value.
Select, Copy, Paste
Some basic editing commands are provided to allow copy and paste of parameters. The simple
example below shows how to copy values from a parameter to one or several other parameters.
1. To copy a parameter, place the mouse pointer over the label of the target parameter and right-
click. Release the mouse over the Copy option to store the parameter to the internal memory.
2. Select the labels of the parameters to overwrite by means of the left mouse button and the
< Ctrl> or < Shift> modifiers if necessary. All selected parameters will appear on a blue
background for an easy check.
3. To paste the copied value to each parameter of the selection, simply right-click over any label
and release the button over the Paste option.
Control of Parameters Bounds
In Fitting, Database Generation and Optimization modules, the value of the defining parameters is
allowed to move within a user-defined range, limited by a lower and an upper bound. Those
the option
additional fields can be monitored in the grid of parameters by means of
Geometry/Show bounds from the menu bar. When active, this option adds new fields and
commands to the grids, as depicted in FIGURE 2.15.
The new fields are:
l lower bound: the minimum allowed value for the parameter,
l upper bound: the maximum allowed value for the parameter,
l reference: a special value used as increment when moving the bounds.
Copy and Paste options behave exactly as explained above and include all four fields.
Moving Bounds of Single Parameter or Selection
Bounds can be set manually, just like the value, but the variation range of specific parameters can
also be enlarged or shrunk at once by right-clicking on the selected parameters.
The commands on the contextual menu apply to only the selected parameters.
The commands on the panel apply to all the listed parameters. If a filter is used, the commands will
apply to the filtered parameters.
FIGURE 2.18
Commands for edition of a selection of parameters
New commands can be applied to the selection from the contextual menu:
l Reset bounds: sets lower and upper bounds to the value of the parameter (freezes the value of
the parameter),
l Increase bounds: moves lower and upper bounds away from the value by a quantity equal to
the reference value,
l Decrease bounds: tightens both bounds by a quantity equal to the reference value.
l Shift by a constant: shift lower and upper bounds by a specified constant.
l Scale by a constant: scale the lower and upper bounds by a specified constant.
According to the location of the value with respect to its range of variation, the label of the
parameter can appear in one among five colors:
l black: the value is free to move in both directions within the specified range and does not
reach any of its bounds,
l yellow: the value is free to move in the specified range, but one of its bounds is reached,
l orange: the value is frozen because its range has a zero length (both bounds are set to the
value) or is ruled by an expression,
l red: the current value is outside its allowed bounds. A correction is required.
l pink: one of the field does not contain valid numeric input. If applied, the wrong field recovers
the previous value.
Finally, three new commands also appear at the bottom of each parameter group to allow a quick
control of the ranges of variation of all parameters at once.
Parameters should never appear in red color. This means the range of the involved parameter is
wrong, possibly due to a typing error. This is not important in stand-alone mode.
Monitor parameter status
In Fitting, Database Generation and Optimization modules, the value of the defining parameters is
allowed to move within a user-defined range, limited by a lower and an upper bound.
Those additional fields can be monitored in the grid of parameters by means of the option
View/Show parameter scale from the menu bar. When active, this option adds new field on the
right side of the parameter list, as depicted in FIGURE 2.15.
According to the location of the value with respect to its range of variation, the label of the
parameter can appear in one among colors:
l green: the value is free to move in both directions within the specified range and does not
reach any of its bounds,
l yellow: the value is free to move in the specified range, but one of its bounds is reached,
l orange: the value is frozen because its range has a zero length (both bounds are set to the
value) or is ruled by an expression,
l red: the current value is outside its allowed bounds. A correction is required.
Furthermore, a cursor shows the relative location of the parameter value compared to its bounds.
O. Special functions
The menu Geometry/Special functions allows the user to define his own functions. The user can
specify a name (always in uppercase), the number of arguments and the corresponding formula
using all previously defined functions, including existing user-defined functions.
FIGURE 2.19
User-defined functions editor
P. Geometry Options
Curves
This tab Geometry options / Curves allows to control the discretized curves in cases where the
default precision is insufficient.
By clicking the small button in front of the curve name, the user can change the default sampling
value.
FIGURE 2.20
Curve sampling dialog
The following table is a summary of the sampling rules for the different curves.
Curves
Default
value of
samples
Description
Hub/Shroud 100
Camber
Suction
side
100
110
This is the default sampling for endwall curves except when a composite is
defined.
For all camber types.
For all suction side curves and regular thickness laws. This sampling is
additive with trailing edge circle sample in case of construction curves.
Curves
Default
value of
samples
Description
Pressure
side
Half
trailing
edge circle
Thickness
formula
110
10
130
For all pressure side curves and regular thickness laws. This sampling is
additive with trailing edge circle sample in case of construction curves.
Only for the trailing edge circle when the construction curves are active. In
practice, the final suction/pressure sampling is increased by this value minus
one.
Internal sampling of the mathematical thickness laws. This value is not
applied to file input where the sampling is dependent of the data file.
Gap curve
50
Internal sampling of the hub/shroud gap curves.
Defaults for endwalls
For regular parametric curves, the default value is 100.
For composite curves, each element has an automatic number of points depending on the type (2
for linear segments) and the number of nodes. Therefore, the total number of points is variable. In
addition, the export to geomTurbo differs according to the version: each element is exported as a
basic curve with its own sampling in version 5.3, but as a single curve with the default number of
points in version 3.7. However, if the composite curve contains at least one linear segment, it is
exported as a single polyline with automatic refinement when the older format applies.
When interpolated stream surfaces are used with shortening (inlet/outlet locations), the composite
curve is always exported as a single curve with the default sampling and the vertex mapping is
taken into account to shorten the curve in version 5.3 (replaced by a shortened curve in version
3.7).
User-defined sampling for endwalls
The curve is always exported as a single curve with the prescribed number of points, whatever the
type of the curve (including composite) and this is true for all geomTurbo outputs.
Checks
As described in Error Messages, when an error or a potential problem is detected in the update of
the model, Autoblade™ will report failures and warnings in the message list. However,
Autoblade™ may give a failure message for a good model in some special cases. The user can
avoid this kind of error message by means of cancelling the check for the geometry.
The option Check endwall curves allows to check the hub/shroud curves.
The option Check thickness laws allows to check the thickness laws.
The option Check 2D sections allows to check the blade passage.
The option Check CAD model allows to check the 3D Parasolid model.
The option Check min draft angle allows to check the minimum draft angle. The draft angle is
used in manufacture of blades with the casting process in order to make sure that a ruled blade is
removable relatively to one direction.
The option Check min draft angle can be accessed only when the blade is defined by 2 primary
sections.
The option Check min draft angle is not available for splitters.
The draft angle is defined by two sections. In order to process the minimum draft angle, the head
section is compared to the foot section. For each sample point on the head section (pressure side
and suction side, respectively), starting from the leading edge to the trailing edge, the interiority is
checked. The draw direction is assumed oriented from foot to head.
l If a head point is interior to the foot profile, the closest point of the foot section in the projected
plane is searched. Then the draft angle is processed in 3D coordinates. In this case, the draft
angle is positive.
l If the head point is exterior, the draw angle is assumed negative. Please note that if the draw
direction is contradictory with blade orientation, interiority is reversed and the sign of the
resulting draw angle as well.
Surface analysis
This tab Geometry options / Surface analysis allows users to select surfaces, where users can
analyze the principal face curvature and the derivatives of x, y, and z in the u and v parametric
directions.
Three surfaces are available for selection: the non- axisymmetric hub, the non- axisymmetric
shroud, and the blade. By default, no surfaces are selected for analysis.
The number of Boundary points is used to set the number of discrete boundary points. A 2D
mesh will be created in the uv coordinate system based on the imposed number of boundary
points. If necessary, the user may increase or decrease the resolution of the surface mesh.
After enabling the surface, the curvature and the derivatives of x, y, and z can be analized in the
Blade-to-blade view, see 3D view options for more details.
2.1.4
Analysis Menu
Most of the options available in this menu are also available as accelerated buttons (top button
bar) or as side buttons (left tool box). This menu consists in three groups of commands:
Optional quantities
The menu Analysis / Optional quantities controls the computation of optional quantities and
distributions depending on the geometric model. These options are detailed in the Optional
Quantities section.
Geometry analysis
The menu Analysis / Geometry analysis allows to access a geometry analysis tool, see Geometry
Analysis for more details.
Parametric report
The menu Analysis / Parametric report aims at the description of the total number of parameter
and the free, frozen and dependent parameters in order to ease the parameters and their
dependencies analysis, see Parametric Report for more details.
Fitting graphs
The menu Analysis / Fitting graphs allows to access the graphical comparison analysis tool, see
Fitting graphs for more details.
Fitting log file
The menu Analysis / Fitting log file allows to monitor the log file of the fitting process, see
Fitting log file for more details.
Fitting convergence
The menu Analysis / Fitting convergence allows to monitor the convergence history of the
fitting process, see Fitting Convergence for more details.
Fitting report
The menu Analysis / Fitting report allows to save all the parameters of the fitting process, the
fitted model and the analysis results to a file, see Generate report for more details.
Fitting report hub / shroud
After an initialization or a fitting process, the menu Analysis / Fitting report hub or Fitting
report shroud allows to compute the differences of the non axisymmetrical surfaces between the
target and the fitted model. The distances are computed on directions built over a customized
range with uniform sampling in both m and θ directions. All directions start from the rotation axis
and are perpendicular to the revolved hub surface. For instance, in case of a cylindrical reference
hub, the directions are all radial.
The choice for definition of the domain is one of the following:
l full channel (automatic range in both m and θ directions, for full coverage),
l partial channel (automatic θ range and user-defined m range),
l user-defined square domain with custom ranges in both m and θ directions.
The sampling is always uniform, but the number of samples for each coordinate is free (maximum
500).
The processing may be long according to the number of samples and the results will be presented
as statistics in the interface. When no intersection is found for a direction, the sample is dropped
without error.
The statistical data consists in arithmetic and quadratic means and the standard deviation as well
as minimum and maximum errors.
Further results are available by saving the report to file for further processing or archive purposes.
1. If the menu Report / Save summary is selected, the data contained is exported as well as an
histogram to check the distribution of the error.
2. If the menu Report / Save all data is selected, an additional block containing all samples is
exported.
Show messages
A graphical console reflects all useful warning and error messages generated by AutoBlade™. It
consists in a simple menu and a read-only text area .
If the message list is full of old messages, the history can be cleared using the View/Clear
command.
FIGURE 2.21
AutoBlade™ Message window
Three kinds of messages are issued:
Success
A success message is usually an update status after a topology or parameter change. It simply
confirms that an operation is free of errors.
Warning
A warning is generated either when there is a potential risk of failure or when a correction has
been automatically applied by AutoBlade™ to ensure compatibility.
This is the case when a parametric file from a previous release is loaded and converted or when a
change in a step of the blade construction is incompatible with a setting from another step.
Error
When AutoBlade™ cannot update the model or needs to correct a value of some parameter, an
error is generated.
In Design3D mode, errors prevent the complete saving of the project: the geomTurbo file is not
updated until problems are solved.
2.1.5
View Menu
Six groups of commands are offered:
l the selection for the upper right view: Blade 2 blade view, Sweep law, Lean law or 3D
model. Alternative buttons exist in the main button bar .
l customize layout of AutoBlad™. When designing a blade, the user may open few geometry
analysis windows to monitor the status of the designed blade. These layout settings can be
exported to a file. When creating a new design, the user may import the saved layout to
retrieve all the settings.
the
saved
Import layout ..., allows to import a layout file from a previously saved layout. The user may
variable
copy
Versions.turboVersinoCmd]]]\bin\templates (on Windows) or
Installation_ path/autoblade
[[[Undefined variable Versions.turboVersinoCmd]]]/COMMON/templates/ (on Linux) and
use it as a template.
Installation_ path\autoblade [[[Undefined
layout
to
Some layout settings might be incompatible with the current model, such as the section or
blade number. AutoBlade™ will update the choices to the closest valid possibility if any,
but no warning or errors are generated.
Export layout, allows to export the current layout to a specified file.
l the management, insertion and removal of optional overlays allowing the comparison of
several states of the model being edited .
l the properties for Blade-to-blade view options and 3D view options.
l Save screen shot: allow to save a capture of the active views. The pictures are saved in png
format. If the four views are active (multiple view), all four views are saved to disk in separate
files. If a single view is active (full view), only that view is exported.
The command Save screen shot is only available in interactive mode.
The saved pictures do not show labels for view and the name of axis.
l Show stream grid: allow to show the grid in meridional view when the stream surfaces type
"Hub to shroud custom interpolation" is used. Show parameter bounds, scale, expressions
and type: the command enables or disables the bounds, scale, expression and type of the
parameters in all menus.
2.1.6
Tools Menu
Distance
Tools/Distance is useful to measure the distance between two points. When measuring the
distance, the distance tool dialog box will appear, showing the distances computed along principal
directions between the two points:
FIGURE 2.22
Distance tool dialog box
After selecting the menu Tools/Distance, the following prompt appears, asking to enter the first
point:
Enter first point
Once the first point is entered, a second prompt appears, asking to enter the second point:
Enter second point
Attraction features are available, allowing automatic attraction to control points, end points,
parametric cures and discrete curves. Once a distance is calculated, another distance can be
measured by selecting other points.
To quit this tool, press <Esc> or the right mouse button.
2.1.7 Modules Menu
This menu allows to switch to other products integrated into the FINE™ interface. Currently,
FINE™/Turbo and Design3D are the only options.
If a model is opened and modified, AutoBlade™ always prompts for save before the effective
switch to the selected module.
2.2
ICON BAR
FIGURE 2.23
Interface buttons
The icon bar (FIGURE 2.23) is a collection of accelerators. This means that all buttons allow
quick access to dialog boxes or operations that are already available in the menu bar.
l The first three buttons (1) allow quick access to the usual file management operations.
l The next four accelerators (2) control the undo and redo stacks.
l The next group of buttons (3) are shortcuts to some of the geometry commands.
l The view management group consists of two selectors (4), which allows to change blade and
section in views.
File management buttons
New file
Accelerator to File\New
Creates a new parametric model on disk
Open file
Accelerator for File\Open
Opens an existing parametric model from disk
Save file
Accelerator for File\Save
Saves the current parametric model to disk
Edition buttons
Undo change
Accelerator for Edit\Undo
Undoes the latest change or undoes the selected change
Redo change
Accelerator for Edit\Redo
Redoes the last undone change or redoes the selected
undone change
Show the name of the current design step
Name of
current step
Checked
button
If the button is checked, the current design step will be
saved in the project
Geometry buttons
Import model
Accelerator for Geometry\Import
Opens the import model dialog 
Parameter list
Accelerator for Geometry\Parameterlist
Opens the full list of parameters defining the current model 
AutoBlade™
messages
Accelerator for Analysis\Showmessages
Opens or restores the message dialog 
View management buttons
Blade
selector
Selector for the blade choice when one or more splitters are defined.
This only affects the lower views (camber curve, side curves and
thickness laws)
Section
selector
Selector for the primary section choice. This changes the lower views
and the blade-to-blade view
2.3
DIALOGS & WINDOWS
In AutoBlade™, most menus appearing as separated or top level windows carry two buttons:
l OK: applies the changes entered in the menu and closes the dialog box. An update of the blade
model is applied accordingly.
l Cancel: leaves the menu without saving changes. If Apply has been clicked, only the changes
brought after this last operation are discarded.
Sometimes, a third button Apply also appears to apply the changes without leaving the dialog.
This option is useful to reflect the changes and to continue within the menu, in the Parameter list
for instance.
Confirmation dialogs have two buttons Ok and Cancel.
Information windows only have a Close or Ok button.
Closing the dialog box using the platform specific way to close a window is similar to a click on the
Cancel button. This applies to all menus and dialogs inside AutoBlade™.
2.4
VIEW LAYOUT & GRAPHS
Multi view is the default mode. In this mode, four graphs showing different views of the blade
appear in the main area. The blade is defined by means of the hub and shroud contours, a series of
so-called primary sections and by stacking laws. All these features can be observed in the
different views. TABLE 2.4 summarizes the properties and numbering of the views.
TABLE 2.4 Available views
Viewport
Content
View 1 (upper
left)
Meridional view in (Z,R) plane with
l hub and shroud curves,
l stream lines of the defining sections,
l edge traces,
l reference stacking point and stacking sweep curve (when available)
View 2 (bottom
left)
Camber curve in its construction plane. The curve belongs to the current selections of
blade and primary section.
No curve appears if the selected splitter blade inherits the main camber curve.
View 3 (bottom
right)
According to the construction mode,
l Suction and pressure sides in the chosen construction plane (independent SS & PS
section mode)
l half thickness distribution versus camber length (camber & thickness 2D section
View 4 (upper
right)
mode)
for the selected blade and primary section.
l Blade-to-blade view,
l Sweep curve in (z,span) plane (when active),
l Lean curve in (span,θ) plane,
l 3D view with optional hub, shroud and blade repetition
When a stacking sweep law is active, the 3D stacking curve is shown in orange color in the 3D view.
The user can quickly switch between single view and multiple views:
l double-clicking in a subview activates full view for that subview,
l double-clicking the full view restores the multiple views (alternate key: escape),
l right-click in a sub/full view and select the menu Single/multiple view from the context menu
entry.
2.4.1
Blade-to-blade view options
The blade-to-blade view (upper right viewport) can be customized by means of the View/b2b
view options command (FIGURE 2.24). The construction plane selected for the camber curve
definition is assumed as default, but the designer can select any of the planes listed in TABLE
2.5.
The blade-to-blade settings are saved to the parametric file and retained. However, an import
operation alters those properties.
FIGURE 2.24
Preferences for the blade-to-blade view
TABLE 2.5 Available viewing planes
(Z,Y)
(Z,Rθ)
(m,Rθ)
(
, θ)
(R,Rθ)
(X,Y)
The option Repeat main blade allows to repeat the blade section in the blade to blade view and
should be deactivated when dealing with wind turbines.
The option Show all primary sections allows to stack all primary sections instead of just the
current one. If the view is not in stacked mode, the blade-to-blade view is fitted when selecting
another section with the selector of a stream trace in the meridional view. If the view is in stacked
mode, the blade-to-blade view will be preserved.
The stacking point of each section is added to the blade-to-blade view. The checked option
Relatively to stacking point will translate all primary sections so that their stacking point is placed
on the stacking point of the current section.
In stacked mode, the current primary section appears with the regular color while curves and
stacking points from other sections appear in an alternate color, based on a gradient from two
reference colors at span values 0.0 and 1.0. The two reference colors can be modified on the
View/b2b view options/Appearance tab. Two colors are defined for spanwise locations at hub
(0.0) and shroud (1.0). The color of each section is interpolated from R, G and B channels. These
settings are saved to the preference file and are persistent on disk.
2.4.2
3D view options
The 3D view is customized in the menu opened by the command View/3D view options.
The 3D view settings are stored in the parametric file. Therefore, the model retains the settings
when it is reopened, but importing a parametric model or template alters those settings.
Geometry
The tab Geometry is used to select the contents that will be shown in the view and choose the
display mode. By default, the main blade and the optional splitters are drawn as single instances.
Hub surface, shroud surface and repetition can also be activated as well as the defining section
curves. Curves can be turned on or off, as well as shading and wireframe. The settings apply to all
objects in the view.
In case of cascade topology, the buttons Revolved hub surface and Revolved shroud surface are
renamed as Reference hub surface and Reference shroud surface, respectively
Appearance
In this tab, the color of both edge and shading can be imposed by the user by left-clicking on the
color proposed by default.
The view is automatically updated after any change but this operation is slower when more
objects are displayed. Hub, shroud and repetition should be disabled for better performance
during edition. A coarse quality settings might slightly improve the refresh speed.
Surface analysis
The tab Surface analysis allows the user to display the surface curvature and the derivatives of x,
y, and z in the u and v parametric directions in the 3D view. Before starting the surface analysis,
the user must select the surfaces first in the tab Geometry / Geometry options / Surface
analysis, see Geometry Options for more details. If no surfaces are selected for analysis, the tab
Surface analysis in the 3D view settings window will be disabled.
The option Display surface analysis contour is used to view the quantity contours for all
selected surfaces. The option Display surface analysis mesh is used to view the surface analysis
mesh. The displayed quantity can be selected in the pull down menu Quantity. By default, the
colormap range is set to its minimum/maximum values. This colormap range may be specified
manually. The button Default sets the colormap to the full range of the chosen quantity. The
Update button allows the user to update the contour plot without closing the 3D view settings
pop-up. This button only updates the contour drawing, and is many times faster than updating the
full 3D view.
Currently, the following quantities are available for selection.
TABLE 2.6 Surface analysis quantities
Quantity Description
Curvature Maximum of the absolute value of the two principal curvatures. The principal curvature is
, where r is the radius of the osculating circle.
defined as
Quantity Description
dx_du
dy_du
dz_du
dx_dv
dy_dv
dz_dv
1st partial derivative of x relative to the surface parameter u
1st partial derivative of y relative to the surface parameter u
1st partial derivative of z relative to the surface parameter u
1st partial derivative of x relative to the surface parameter v
1st partial derivative of y relative to the surface parameter v
1st partial derivative of z relative to the surface parameter v
dx_duu
2st partial derivative of x relative to the surface parameter u
dy_duu
2st partial derivative of y relative to the surface parameter u
dz_duu
2st partial derivative of z relative to the surface parameter u
dx_dvv
2st partial derivative of x relative to the surface parameter v
dy_dvv
2st partial derivative of y relative to the surface parameter v
dz_dvv
2st partial derivative of z relative to the surface parameter v
The quantities are computed based on the Parasolid faces. The u and v directions are not assumed to
be aligned streamwise, spanwise, etc.
2.5
VIEWING CONTROL BUTTONS
The graphics layout use IGG™ toolbar for view all manipulations. The buttons appearing below
the views can be used to control the view:
View selector
The view selector allows to cycle through view layouts. The icon changes slightly and indicates
the selection corresponding to the next action. The cycle order is full upper left view, full bottom
left view, full bottom right view, full upper right view and four views layout.
X, Y, and Z projections
Press the left mouse button to project the view on an X, Y or Z constant plane. If the same button
is pressed more than one time, the horizontal axis sense changes at each press.
Coordinate axes
The coordinate axis button acts as a toggle to display the coordinate axis on the view.
l A left click enables/disables the reference axes
l A middle click enables/disables axes ticks
l A right click has no effect in AutoBlade™.
Scrolling
This button is used to translate the contents of the view within the plane of the graphics window
in the direction specified by the user. The following functions can be performed with the mouse
buttons:
l Left: press and drag the left mouse button to indicate the translation direction. The translation is
proportional to the mouse displacement. Release the button when finished. The translation
magnitude is automatically calculated by measuring the distance between the initial clicked
point and the current position of the cursor.
l Middle: press and drag the middle mouse button to indicate the translation direction. The
translation is continuous in the indicated direction. Release the button when finished. The
translation speed is automatically calculated by measuring the distance between the initial
clicked point and the current position of the cursor.
3D viewing
This button allows to perform viewing operations directly in the graphics area. Allowed
operations are 3D rotation, scrolling and zooming.
After having selected the option with the left mouse button, move the mouse to the active view,
then:
l Press and drag the left mouse button to perform a 3D rotation.
l Press and drag the middle mouse button to perform a translation.
l Press and drag the middle mouse button, while holding the <Shift> key, to perform a zoom.
l To select the centre of rotation, hold the <Shift> key and press the left mouse button on a
vertex of a curve or a surface. The view is immediately centred on the clicked entity which
will act as the centre of rotation. Dragging the mouse will rotate the model.
To quit the option, right-click the button.
A <Shift> and left-click allow to select the centre of rotation in the 3D view if and only if show
edges option is activated in the 3D view options dialog. Otherwise, the action is identical to a left-
click.
Rotate about x, y or z axis
The rotation buttons are used to rotate graphical objects on the view around the X, Y or Z axis.
The rotations are always performed around the centre of the view. The following functions can be
performed with the mouse buttons:
l Left: press and drag the left mouse button to the left or to the right. A clockwise or counter-
clockwise rotation will be performed, proportional to the mouse displacement. Release the
button when finished.
l Middle: press and drag the middle mouse button to the left or to the right. A continuous
rotation will be performed, clockwise or counter-clockwise. Release the button when finished.
Zoom in/out
This button is used for zooming operations. Zooming is always performed around the centre of
the view. The following functions can be performed with the mouse buttons:
l Left: press and drag the left mouse button to the left or to the right. A zoom in - zoom out will
be performed, proportional to the mouse displacement. Release the button when finished.
l Middle: press and drag the middle mouse button to the left or to the right. A continuous zoom
in - zoom out will be performed. Release the button when finished.
Region zoom
This button allows to specify a rectangular area of the active view that will be fitted to the view
dimensions. After having selected the button:
l press and drag the left mouse button to select the rectangular region,
l release the button to perform the zoom operation.
These operations can be repeated several times to perform more zooming.
Press the right mouse button to quit the option.
Fit view
The fit button is used to fit the content of the view to the view limits without changing the current
orientation of the camera (which can be interpreted as the user's eyes).
Restore view
The restore button is used to fit the content of the view and to give a default orientation to the
camera.
2.6 QUICK ACCESS PAD
The Quick Access Pad is located in the left part of the GUI. It contains icons and more evolved
options providing a fast access to the more used functions of AutoBlade™. Some of these
functions are only accessible through the Quick Access Pad whereas others are also accessible
through the menu bar, so that their description will be referenced to these menus.
The pad is divided into three subpads, each of which can be toggled by a simple mouse left-click:
l Target Settings
l Model Editor
l Fitting Control
All the commands and options accessible with these subpads are described in detail in this section.
The three subpads are composed of pages containing buttons, icons, input areas. The icons
perform specific function related to the subpad and the page. Each page can also be toggled by a
simple mouse left-click.
The subpads Target Settings and Fitting Control only appear in the interface when the fittings
license feature is detected.
2.6.1
Target Settings subpad
This menu - the subpad Target Settings in the left area - grants access to the target settings for the
fitting project. All these functions are only accessible through this subpad.
FIGURE 2.25
Target Settings subpad
Link target geometry
A geomTurbo file can be linked to the current project through the button
how to prepare a target geomTurbo file, please refer to the Preparing Target Geometry section.
. For more detail on
Remove target geometry
The button
allows to remove the geomTurbo file linked to the current project.
Build target sections from CAD geometry
If the geomTurbo file uses CAD import (more details in AutoGrid™ User Manual),
the
geomTurbo file can be linked to the current project, but requires a specific treatment to obtain
can be
sections before the initialization and fitting processes can be launched. The button
used to build the target sections from the CAD geometry. The operation alters the target file and
archives the original target.
FIGURE 2.26
Build blade sections from CAD surfaces
The Build tolerance is the precision used when building the sheet bodies of the CAD blades.
The Sewing tolerance is the tolerance applied when sewing the CAD faces together. The default
value of the sewing tolerance assumes an suitable scale (order of magnitude of the bounding box
is at least 0.1 and at most 100) and good precision of the data.
These two tolerances can be modified when AutoBlade™ fails to generate blade sections from
CAD surfaces. In such a case, a generic message is issued:
"Failed to build some sections. Please check error messages and retry"
Additional messages can be found in the log file. The two next messages are examples where
those settings should be modified. However, the operation may fail later by producing strange or
incomplete shapes for side curves, without any failure message.
"Failed to build the suction/pressure sheets for blade"
"Failed to sew the suction/pressure sheets for blade"
Generally speaking, the build tolerance should be increased in the first case and the sewing
tolerance should be increased in the second case. When increased, it is advised to keep the
smallest possible value for build tolerance. The sewing tolerance should never be larger than the
smallest edge length in the CAD surfaces.
The option correct position of side curves allows to automatically correct the orientation of the
target sections. This option is applied by default when building the sections.
Restore original CAD geometry
The button
allows to restore the original CAD target.
The operations Build sections from CAD
stored on disk.
and restore CAD
directly change the target files
Edge point relocation
Edge points of the leading or trailing edge on the target can be altered for each section through the
button
the fitted row. It can be different from 1 in case of splitter blades.
, if the corresponding edge is rounded. The blade index refers to the blade number in
The location is relative to the original position and expressed as a fraction of the profile length. It
is positive in the counter-clockwise sense, negative in the other sense. If the check box all sections
is selected, the relocation of the edge points will be applied for all sections. Edge point relocation
affects the geometry loaded in memory, but does not alter the target geometry file.
Project target geometry on model stream surfaces
The button
allows to project the target curves on the stream surfaces of the parametric model.
Other settings and target viewing
The option Row to fit allows to select the target row to fit (if several rows are defined). And an
optional Scaling factor can be applied on the target geometry.
The sampling of the target side curves and intermediate projection paths can be controlled for
more precision (if increased) or to improve speed (if decreased) of the projection/fitting processes.
In addition, the options Exchange sides and Reverse orientation allow respectively to set the
suction side above the pressure side and to reverse the azimuthal orientation when necessary.
Both the target geometry and the projected target curves can be shown in the graphical view for
comparison with the fitted geometry, which is controlled by the buttons Show target and Show
projection , respectively. Two special colors can be reserved for the target geometry and the
projected target curves in the graphical interface: orange for the target curves and surfaces, yellow
for the projected target curves. These default colors can be changed in the menu File /
Preferences.
Currently, three views can show the target curves and surfaces:
l the meridional view for endwall curves (target and projected target),
l the 3D view for blade surfaces (target only) or section curves (target and projected target). The
3D view shows target surfaces if the target is a CAD geometry. After building of the section
curves, the resulting target curves are shown instead. The target data is shown without
transformation except in those two cases:
l if the scaling factor is set, the target geometry appears scaled,
l in case of planar stream surfaces, the target blade is rotated to approximately match the
alignment with plane (Z,Y).
l the blade-to-blade view for curves (projected target only).
2.6.2 Model Editor subpad
This menu - the subpad Model Editor in the left area - grants access to the governing topological
settings of the blade definition as well as some quantities and distributions (FIGURE 2.27). All
associated commands can alternatively be found under the Geometry and Analysis menu.
FIGURE 2.27
Model Editor subpad
Nine Design Steps
Nine successive design steps can be outlined (fully described in the AutoBlade™ Modeller
chapter) and make up the first part of the menu:
1. definition of the curve type used to shape the endwall contours,
2. selection of the stream surfaces type, spanwise type and location of the 2D sections,
3. definition of the stacking point, sweep and lean laws,
4. definition of the topology for the main blade: selection of the construction plane, camber curve
type, construction of the suction and pressure sides and settings for the edges,
5. definition of the topology for the optional splitter blades: number of additional blades, optional
camber refinement and settings of the side curves,
6. optional technological effects,
7. definition of the non-axisymmetric hub surface,
8. definition of the non-axisymmetric shroud surface.
9. definition of the solid geometry such as the axisymmetric wheel and shroud components in the
RZ frame.
These nine menus - activated by the green buttons - can be seen as successive steps that need to
be performed in order to build the model. The features are however dependent, which explains
why it is not possible to edit two of them at the same time. For example, changes in endwall
curves can affect stream surfaces and a change in the stream surface type will alter the definition
of the blades. On the contrary, changes in the definition of a section cannot modify the endwall
curves.
FIGURE 2.28 illustrates the behavior of the menu when the Stacking laws button is clicked.
FIGURE 2.28
Opening a topology menu excludes others
The Parameter list menu cannot be opened when a topology step is edited. On the contrary,
Optional quantities, Geometry analysis and Parametric report tools are allowed and updated
automatically.
Error Messages
When an error or a potential problem is detected in the update of the model, AutoBlade™ will
report failures and warnings in the message list. The graphical menu will be updated accordingly
and the color of the failing step is changed to red. Subsequent steps are frozen and appear in gray
color to indicate that the corresponding parts of the model are also incorrect. In such a case,
quantities are not updated.
For instance, if the meridional location of the edge traces fails for some reason, the graphical
menu will appear exactly as in FIGURE 2.29. The dedicated message window can be opened to
get further information about the error .
FIGURE 2.29
The graphical menu is updated when an error occurs
Optional Quantities
This menu allows the computation of geometrical quantities such as blade thickness and moments
of inertia for every section. All values and samples are affected by the changes of the parameters
and topologies in the menus described above. The Optional Quantities section is devoted to the
available quantities, their definition and how they are computed.
When topology settings or parameters are changed while the menu is opened, the quantities are
automatically updated.
Geometry Analysis
The Geometry analysis tool consists in graphs showing distributions of useful properties like
endwall curvature, side metal angle or section thickness. Please consult the Geometry Analysis
section for more details.
When topology settings or parameters are changed while the menu is opened, the distributions are
automatically updated.
Parametric Report
The Parametric report consists in the description of the total number of parameter and the free,
frozen and dependent parameters in order to ease the parameters and their dependencies analysis
.
2.6.3
Fitting Control subpad
This subpad, Fitting Control, in the left area - grants access to control the fitting process
(FIGURE 2.30). Some associated commands can be found under the Analysis menu whereas
others are only accessible through this subpad.
Before starting the fitting process, the designer needs to change the topological settings and
parameters of the current model. All operations on the current model are allowed, except new,
open, save and save as.
FIGURE 2.30
Fitting Control subpad
Adapt model
The button Adapt model allows to launch the initialization process on the current model (the one
displayed in graphical interface), see Setup Initial Model and Initialization Process for more detail.
Fit model
The button Fit model allows to launch the fitting process and the settings of the optimization
algorithms. Details about this step is covered in the Fitting Process section.
Generate report
The button Generate report is used to export the parameters of the fitting process to a file. The
following data will be included in the exported report:
l general information (number of the blades and number of the sections),
l fitting features that are fitted,
l parametric report with all the parameters and their values,
l error report of the fitting features between the target and the fitted model,
l analysis data.
Fitting graphs
This button provides a graphical comparison of the current design and the projected target curves.
It is very useful to verify the model after an initialization or a fitting process.
The comparison always applies between the current design and the projected target curves. If the
button is disabled, a new projection is required.
The Fitting graphs page is not accessible until the initialization process has been finished.
Two entries allows the selection of a graph containing:
l the endwall curves,
l the meridional and tangential edge traces,
l the sweep and lean laws,
l the side curves of a primary section.
Sections can be compared in the following planes. Some of them could be meaningless according
to the machinery type:
(
, θ)
(R,Rθ)
(X,Y)
(m,Rθ)
(Z,R)
(Z,Rθ)
(Z,Y)
By default, the comparison of the sections in the different viewing planes involve the stacking
laws. If selecting the button Unstacked view, the stacking laws will not be applied in order to
allow an easier check of the error in shape.
FIGURE 2.31
The fitting graphs comparison page
Fitting log file
This button allows to access the log file of the fitting steps.
Fitting Convergence
This button allows to visualize the convergence of the fitting steps as well as the evolution of each
free parameter within its bounds.
2.7
GRAPHICAL INTERACTIONS
This section covers the graphical controls and actions.
2.7.1 Monitoring of Controls
Any angle, control point, node or length can be monitored in the status bar. This happens when
the mouse pointer is close or over the graphical representation of the control, as soon as it is
highlighted (the color changes from green to red).
Angular Parameters
Angles are easily recognized thanks to their two reference lines, their circular arc and their
symbolic name. A small triangle to one end of the arc indicates the direction of the angle and is
used to pick or highlight the angular control.
For instance (FIGURE 2.32), the stagger parameter can be highlighted in the lower left view by
moving the mouse pointer over the control triangle (1). The color changes to red and a message
indicates an optional edition of the angle in the bottom of the viewing area (2). The status bar
indicates that the control is parameter S1_CAMBER_GAMMA with current value 40.0 degrees
(3).
FIGURE 2.32
Highlighting and monitoring of an angular parameter
Nodes & Control Points
Nodes and control points are drawn as simple green points and may appear differently according
to the control, curve and view they belong to. Three different cases can be encountered, as
illustrated in FIGURE 2.33 on the default model.
l In the first case (upper left), the node on hub curve is controlled by two parameters HUB_Z2
and HUB_R2 that fully defines its location in the meridional plane.
l In the second case (upper right), the control point of the suction side curve is defined by a
single parameter S1_TSS_2. Therefore, it cannot freely move in the plane and is constrained to
remain on a line perpendicular to the camber curve.
In the third case (bottom), no parameter is linked to the control point, but can indirectly change
angular parameters named B1 and B2 of the camber curve. The 2D coordinates of the control
point in the construction plane appear in the status bar.
FIGURE 2.33
Three kinds of nodes and control points
Lengths
Length and fraction parameters are symbolized by a hollow point and a short name in the view.
This kind of parameter appears in some endwall curves (left picture in FIGURE 2.34), stacking
laws or edge traces (right picture in FIGURE 2.34). Those controls are specialized control points
that either define a length or a fraction of a reference length. Those points can move in only one
direction!
FIGURE 2.34
Length parameter on hub curve (left) and edge trace (right)
End line parameter for side curves is a length, but its symbolic representation differs from the one
introduced above for more readability. A triangle control replaces the circular marker and its label.
Radius
A radius parameter is symbolized by a circle arc of the prescribed size, its centre point and a label
R. It is highlighted when the mouse pointer is near the centre point (FIGURE 2.35).
If the involved curve is a real circle however, the symbolic arc is not drawn (case of B-spline half-
thickness).
FIGURE 2.35
Radius parameter in a half-thickness law (Bezier)
2.7.2
Edition of Control
Once highlighted, any control can be edited by means of the mouse: simply left- click the
highlighted symbols, then move the mouse pointer over the view. At each move, the control is
moved and the value of the corresponding parameters is updated in the status bar. If the control is
part of a curve definition, the curve is also updated in real time.
To accept a new location for the control, it is possible to use the mouse for rough values or the
keyboard for precise values of corresponding parameters.
Mouse Input
FIGURE 2.36
Mouse input allows rough values for parameters (right)
Once the control has been moved to a suitable location or the value is close to the one expected,
left-clicking a second time ends the edition of the control and the model is fully updated.
Highlighting the control again monitors the new value for the parameter (FIGURE 2.36), but the
entered value is rough. Therefore, this method is especially useful for pre-design, when the shape
of the blade need to be modified quickly.
Keyboard Input
Once the control has been clicked for edition, a precise numeric input may be keyed as new value
for the parameter. For instance, if the value -7.0 is wanted for parameter S1_CAMBER_BETA1,
simply type the following sequence in the main interface:
- 7 <Enter>
The keys are grabbed and transferred to the special keyboard input area just above the status bar
(FIGURE 2.37, left). The edition of the control ends on <Enter> and the model is updated
accordingly. Highlighting the control again allows the check of the new value (FIGURE 2.37,
right).
FIGURE 2.37
Keyboard input for single parameter
Special Keyboard Input
When two parameters are involved in a single control, keyboard input is still possible, but two
numeric values are required, separated by a space, before the <Enter> key is entered.
For instance, the following sequence allows to impose (-0.04, 0.51) coordinates for hub point:
- . 0 5 0.51 <Enter>
Bounds & Limits for Parameters
All parameters have a validity range. A radius is always positive and some angles cannot exceed -
[90, 90] range. At edition time, the new value is compared to those limits and invalid values are
automatically replaced by the closest limit (keyboard input).
In other constraints exist, the validity range can be reduced. This is the case for β1 value in the
camber curve, for which the value must comply with [γ,90] range.
Minimum and maximum bounds are less critical values used when AutoBlade™ is run from
FINE™/Design3D module that define the allowed range for the value of a parameter. If a value is
changed in the interface, with mouse or keyboard, the bounds are automatically adapted so that
the new value lies within the allowed range.
For instance, if β1 has minimum and maximum bounds of respectively 0.0 and 10.0, setting the
value to -7.0 in the interface moves the minimum bound to -7.0 and the new allowed range is then
[-7.0, 10.0].
2.7.3 Meridional View
Edition of the meridional view is different from other views. Controls are never visible by default
to avoid garbage on the screen, since many curves are drawn in the same graph: hub and shroud
curves, sweep trace, edge traces and stream surfaces.
Generally speaking, curves appearing in the foreground color highlight if they can be edited and a
selection is first needed to access its controls. Only a single selection of curve is possible, so the
previous curve must be unselected to go on with selection.
Hub & Shroud Curves
FIGURE 2.38
Hub selection in meridional view
To edit hub or shroud curve, the curve has to be selected first, so that its controls are activated.
This is done by a simple left click over the highlighted curve (FIGURE 2.38 left): the controls of
the curve appear and the nodes can be edited as described above (FIGURE 2.38, right).
To leave the curve, another left click is required, outside the drawing of the curve and its controls.
When hub to shroud interpolation methods are selected, the user can control interactively the start and
end of the reference stream surfaces for hub and shroud curves by left-clicking on it.
FIGURE 2.39
Modify start/end of reference stream surfaces
Stacking Reference Point
When a sweep law is available, its representation appears in the meridional view, but can only be
edited in the sweep view (upper right viewport). Its reference point Z_STACKING_SWEEP or R_
STACKING_ SWEEP is however editable in the upper left view, but only appears when
highlighted (FIGURE 2.40).
FIGURE 2.40
Reference stacking point highlighting
The reference point can move along the hub curve but does not exist when edge traces are
selected in Stacking laws menu.
Edge Traces & Edge Points
Edge traces are always visible in the meridional view, but cannot be edited if the stacking sweep
law is active . If selectable, left-clicking the trace shows its controls, as
depicted in the left picture of FIGURE 2.41. The right picture shows that the four edge points can
be edited just like the reference stacking sweep law, as explained above.
FIGURE 2.41
Edition of edge traces and end points
Selection of Section
Left-clicking the stream trace in the meridional view allows to display the corresponding section
in lower views. This graphical selection acts as a replacement for the section selector from the
main tool bar.
Contextual Menu
Right-clicking in the meridional view opens a popup menu that allows to edit endwalls (Edit
hub/shroud) or to reverse them (Reverse hub/shroud).
FIGURE 2.42
Popup menu for endwalls
Furthermore, when the meridional control is defined by means of leading and trailing edges
location or/and when the rulings is activated, the menu allows respectively to edit the leading
and/or trailing edge, or/and to edit the rulings settings for the main blade and the main blade ruling
links.
FIGURE 2.43
Popup menu for leading/trailing and rulings
2.7.4
Tool Stack
In each view, a permanent tool allows the selection and highlighting (meridional view) or the
picking of the controls (other views). Zoom, dynamic viewing and others are all tools that mask
the permanent tools in the active view, recognized by its red border.
When one or more tools are started in turn, the latest grabs all events and suspends the previous
one. This means that the tools are stacked and must be quit in turn to return to the original
permanent tool.
For instance, the selection tool is permanent in the meridional view. Selecting an highlighted
curve starts the edition tool for that curve and no more selection is possible until left clicking a
unhighlighted area of the view. If the zoom area tool is then started, the edition tool is also
suspended. This means three tools are stacked and zoom area is the only active tool. In order to
return to the default selection tool, the zoom tool has to be stopped by a right click. Then the
edition tool must be stopped by a left click.
Aborting a specific tool
Specific edition tools are stopped by means of a left click in a unhighlighted area of the
corresponding view.
Zoom area and dynamic viewing tools are stopped by means of right click.
Aborting all tools
To prevent bad operations in tools, applying changes in the model editor from the left area of the
main interface stops all non permanent tools in the views. Generally speaking, all model and file
operations automatically abort the tools.
2.7.5
Overlays
Optional overlays allow the display of one or more saved states of the model in the graphical
views. This option allows comparison of the current state of the model with one or more reference
states.
FIGURE 2.44
Overlay in the camber view
To quick insert the current state of the model as an overlay, select the menu View/Quick insert
overlay. The state is immediately added to all views in a different color, but will only appear
when the model is edited since the two states are initially identical. All views are affected, but the
3D view only shows a single instance of the wireframe model for each blade.
FIGURE 2.44 illustrates the comparison of the camber curve with a previous state that appears in
another color. It is possible to add up to five states in the graphical interface.
Overlays are persistent in a parametric model. This means that overlays are linked to a state saved
on disk and available after reload of the project. Overlays can be removed all at once by the menu
View/Remove all overlays.
The menu View/Overlay manager... provides advanced control of overlays. With the overlay
manager, the user can add the current model as an overlay, or add a parametric model from file
as an overlay. The new overlay can be added before or after the selected overlay. A name
(Overlay name)can also be specified for the added overlay. Click on the button Insert will add a
new overlay in the list shown in the following figure.
For each added overlay, the user may edit its color shown in the graphical interface by left-
clicking on the color. The user can also remove the overlay by clicking on the button Remove
next to the name of the overlay.
2.8
BATCH MODE
Linux
Linux,
" Installation_
located
Under
path/autoblade131/LINUX/autoblade/" (when AutoBlade™ is installed as standalone product) or
"Installation_path/fine131/LINUX/autoblade/" (when full FINE™/Turbo package is installed).
executable
directory
under
the
the
is
The executable can then be launched in batch mode respectively with the following command:
autoblade131 -batch -print
will launch AutoBlade™ v13.1 executable in batch mode and print all messages to the standard
output.
Windows
Under Windows,
path\autoblade131\bin64\ "
"Installation_path\fine131\bin64\" (when full FINE™/Turbo package is installed).
is
(when AutoBlade™ is
under
installed as
executable
located
directory
" Installation_
standalone product) or
the
the
The executable can then be launched in batch mode respectively with the following command:
C:\NUMECA_SOFTWARE\autoblade131\bin64\autobladex86_64.exe -batch
or
C:\NUMECA_SOFTWARE\fine131\bin64\autobladex86_64.exe -batch
There is no need for the "-print" flag under Microsoft Windows. However, in order to see messages,
it is advised to open a DOS shell (Command prompt) to launch the executable instead of the Run
dialog under the Start menu.
Usual Flags
If no valid flag is added, an error message is printed by AutoBlade™ executable as well as a list
of commonly used options.
Parametric model (.par) input
The flag "-par" is mandatory to activate AutoBlade™ support in batch mode. It must be followed
by the path to the parametric file to read and acts as input. The parametric file is provided with
relative or absolute path. For instance,
> autoblade131 -par /home/usr/blade.par -batch
will use model '/home/usr/blade.par' as input while
> autoblade131 -par blade.par -batch
will use model 'blade.par' from the current directory.
If no other AutoBlade™ flag is supplied, the return value of the executable allows to test the
validity of the input model. In case of bad parametric format or problem in the generated model,
value different from 0 is returned. If the model is valid, 0 is returned.
Parametric model (.par) output
It is possible to upgrade an older parametric file to the latest format by means of the "-opar" flag,
followed by the path to the output file.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -opar blade_new.par -batch -batch
Geometric model (.geomTurbo) input
The flag " - geom " is mandatory to open a given ".geomTurbo" file (geomTurbo 3.7 or
geomTurbo 5.3) in AutoBlade™. It must be followed by the path to the ".geomTurbo" file to
read and acts as input. The ".geomTurbo" file is provided with relative or absolute path.
> autoblade -geom /home/usr/blade.geomTurbo -batch
Geometric model (.geomTurbo) output
A geomTurbo file can be generated from the input parametric or geometric model and saved to
disk by means of the "-ogeom" flag
This flag requires an input parametric or geometric file and is additive to "-par" or "-geom" flag.
Example:
> autoblade131 -par blade.par -ogeom blade.geomTurbo -batch
The version number of the output geomTurbo format is stored in the parametric file and can be
either 3.7 or 5.3. If a specific format is required, the flag "-ogeom" can be replaced by "-ogeom4"
for geomTurbo 3.7 or "-ogeom5" for geomTurbo 5.3.
> autoblade131 -par blade.par -ogeom4 blade_AG4.geomTurbo -batch
> autoblade131 -par blade.par -ogeom5 blade_AG5.geomTurbo -batch
Parasolid output
A parasolid file can be generated from the input parametric model and saved to disk by means of
the "-oparasolid" flag.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -oparasolid blade.x_t -batch
Solid sector geometry output
A merged blade and solid body can be outputted in parasolid format by means of the " -
osectorparasolid" flag. For more information of solid body, see Solid Body.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -osectorparasolid blade.x_t -batch
IGES output
An IGES file can be generated from the input parametric model and saved to disk by means of the
"-oiges" flag.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -oiges blade.igs -batch
Rulings Output
A rulings data file can be generated from the input parametric model (when Activate rulings
active) and saved to disk by means of the "-orulings" flag.
This flag requires an input parametric file and is additive to "-par" flag.
Example:
> autoblade131 -par blade_org.par -orulings blade.dat -batch
TRAF outputs
TRAF format files can be generated in a specified folder "traf-folder" from the input parametric or
geometric model and saved to disk by means of the "-otraf" flag.
This flag requires an input parametric or geometric file and is additive to "-par" or "-geom" flag.
Example:
> autoblade131 -par blade_org.par -otraf traf-folder -batch
Parameters input
The flag "-iparam" can be used to import a list of parameters that will replace the parameters of
the current model. It must be followed by the absolute path to the parameter file.
> autoblade131 -iparam /home/usr/blade.param -batch
Here is an example of a parameter file:
SWEEP_BETA1 5
SWEEP_BETA2 -2.5
LEAN_BETA2 2.5
LEAN_BETA1 -5
For each line, the name of the parameter should be written followed by its value.
Parameters Output
The flag "-oparam" can be used to output all active parameters to a file. It must be followed by
the absolute path to the parameter file.
> autoblade131 -oparam /home/usr/blade.param -batch
This flag requires an input parametric or geometric file and is additive to "-par" or "-geom" flag.
Example:
> autoblade131 -par blade.par -oparam blade.param -batch
CHAPTER 3.
AUTOBLADE™ MODELLER
This chapter describes AutoBlade™ Modeller,
the advanced and interactive NUMECA geometry
modeller for three-dimensional turbomachinary blades. It can define various types of axial, radial or
mixed flow turbomachinary blades that can be rotating or stationary. AutoBlade™ allows:
l two design modes for generating the 2D section profiles: independent suction and pressure sides or
camber and thickness addition,
l multiple splitter blades (single for the fitting module),
l various types of stream surfaces (planar, cylindrical, conical or arbitrary),
l multiple choices for the blade stacking point, tangential lean and meridional sweep,
l rounded and blunt edges,
l special technological effects (edge filing and arbitrary blade cutoff),
l non-axisymmetric hub/shroud surface,
l solid geometry such as the axisymmetric wheel and shroud components in the RZ frame.
AutoBlade™ also provides a powerful geometry analysis tool able to monitor distributions from the
model:
l hub and shroud angle and curvature,
l section thickness,
l suction, pressure metallic angle and curvature,
l various angles and curvature of camber and mean lines,
l section channel width.
In addition, many useful quantities can be extracted from the model and the above graphs:
l samples for angle and curvature of hub, shroud, suction, pressure and mean line curves,
l samples and maximum value for thickness,
l solidity, meridional chord, chord and stagger angle,
l minimum channel width and throat area,
l unguided turning angle,
l moment of inertia and area of the 2D sections,
l leading edge wedge angle,
l leading and trailing edges coordinates.
In this section
3.1 Topology & Parameters
3.2 Optional Quantities
3.3 Geometry Analysis
3.4 Parametric Report
100
214
239
244
3.1
TOPOLOGY & PARAMETERS
The nine steps illustrated in FIGURE 3.1 are detailed in the next sections. All steps are accessed
using the graphical menu in the left area introduced earlier (Model Editor subpad).
All menus feature embedded diagrams that permit to understand the physical significance of the
related parameters. The naming of the parameters is defined for all topological choices and allows
to identify them in the Parameter list.
FIGURE 3.1
The nine generation steps
3.1.1 Meridional Contours
Both hub and shroud endwalls are assumed to be axisymmetric surfaces, so the corresponding
surfaces can be defined by two curves in the (Z,R) plane, where Z and R are the axial and radial
directions respectively. The meridional contours always appear in the upper left view.
Each meridional contour can be defined using seven different methods to allow the designer as
much control as possible (FIGURE 3.2):
l B-spline,
l Bezier,
l Line-Bezier-Line,
l Line-Spline-Line,
l User-defined,
l composite,
l Bezier 4.
FIGURE 3.2
Endwalls definition menu
A single curve definition is used to define the complete streamwise extent of each contour, except
for the composite curve, that allow the use of an arbitrary amount of elements linked to each other
with optional tangency constraints.
B-spline curve
FIGURE 3.3
B-spline curve
This method uses a B-spline curve defined by n nodes. The main difference with Bezier curves is
that the resulting curve is a piecewise continuous interpolation of the defining points: the curve
passes through all prescribed points and offers continuity up to the second derivative. This curve
type is especially useful in the case the user wishes the contour to pass through one or more
known coordinates, but the resulting curve exhibits less smoothness than its Bezier counterpart.
Description
Z coordinate of the (i)th node of hub curve
R coordinate of the (i)th node of hub curve
Z coordinate of the (i)th node of shroud curve
R coordinate of the (i)th node of shroud curve
Parameter
HUB_Z(i)
HUB_R(i)
SHROUD_Z(i)
SHROUD_R(i)
Bezier curve
FIGURE 3.4
Bezier curve
A Bezier curve defined by n control points only passes through its first and last control points.
Among other properties, its first derivative at both ends is the direction of the first and last control
polygon segments. This produces a smooth curve well defined at ends, but provides the user with
indirect control through the use of the intermediate control points.
Parameter
Description
HUB_Z(i)
HUB_R(i)
Z coordinate of the (i)th control point from hub curve
R coordinate of the (i)th control point from hub curve
SHROUD_Z(i)
Z coordinate of the (i)th control point from shroud curve
SHROUD_R(i)
R coordinate of the (i)th control point from shroud curve
Composite line-Bezier-line curve
FIGURE 3.5
Composite Line-Bezier-Line curve
This curve offers the same properties as a Bezier curve plus optional straight line segments at one
or both ends. Both end points are defined in the usual way and at least six additional parameters
completes the curve description: the direction and length of the optional end segment at both ends
and the length of the first and last control segments of the Bezier curve.
Parameter (hub curve)
Description
HUB_Z1
HUB_R1
HUB_Z2
HUB_R2
Z coordinate of the first endpoint
R coordinate of the first endpoint
Z coordinate of the second endpoint
R coordinate of the second endpoint
HUB_BETA1
angle of the starting segment above Z axis (in degree)
Parameter (hub curve)
Description
HUB_BETA2
angle of the ending segment above Z axis (in degree)
HUB_L1
HUB_L2
HUB_D1
HUB_D2
length of the starting straight line segment
length of the ending straight line segment
length of the starting straight line segment
length of the ending straight line segment
HUB_ADD_Z(i)
HUB_ADD_R(i)
Z coordinate of the (i)th additional node of the Bezier part
R coordinate of the (i)th additional node of the Bezier part
Similar parameters exist for the shroud endwall
The default curve requires thus ten parameters and provides a third order Bezier curve. If
required, additional control points can be added at the cost of two additional parameters per
control point.
Composite line-Spline-line curve
FIGURE 3.6
Line-Spline-Line curve
This curve offers the same properties as a B-spline curve plus optional straight line segments at
one or both ends. Both end points are defined in the usual way and at least four additional
parameters completes the curve description: the direction and length of the optional end segment
at both ends and the length of the first and last control segments of the B-spline curve.
Parameter (hub curve)
Description
HUB_Z1
HUB_R1
HUB_Z2
HUB_R2
HUB_BETA1
HUB_BETA2
HUB_L1
HUB_L2
HUB_ADD_Z(i)
HUB_ADD_R(i)
Z coordinate of the first endpoint
R coordinate of the first endpoint
Z coordinate of the second endpoint
R coordinate of the second endpoint
angle of the starting segment above Z axis (in degree)
angle of the ending segment above Z axis (in degree)
length of the starting straight line segment
length of the ending straight line segment
Z coordinate of the (i)th additional node of the Bezier part
R coordinate of the (i)th additional node of the Bezier part
Similar parameters exist for the shroud endwall
The default curve requires thus eight parameters and provides a third order B-spline curve. If
required, additional control points can be added at the cost of two additional parameters per
control point.
User-defined curve
A special type allowing a curve free of parameters can be selected. It requires a list of points in the
meridional plane and an interpolation law. The endwall is thus a linear or spline interpolated curve
passing through user-defined points.
A dialog box allows the designer to enter the nodes using a simple text formatted file carrying a
".dat" extension. At least two nodes must exist and the content must comply with the following
format. Points are numbered from inlet to outlet.
TABLE 3.1 File format for a parameterless endwall curve
Rules
n (unsigned integer, number of points)
Z1 R1 (two space separated floating point numbers)
...
Zn Rn
Sample
0.0 0.15
0.05 0.15
0.1 0.14
0.15 0.13
0.2 0.13
Although the curve is parameterless (no parameters appear in the Parameter list), it can be edited
like any other curve in the meridional view.
Once the file has been read, it may be deleted since all data is saved in the parametric file.
Composite curve
For complex contours, a special composite curve can be defined with an arbitrary amount of
elements of different types. Those elements are linked to each other to ensure continuity.
Optionally, they can be constrained to fulfil the continuity of the tangency.
FIGURE 3.7
Composite hub curve
Any of the following curves can be added and removed in any order:
l a Bezier curve defined by n control points,
l a B-spline curve defined by n nodes,
l a C-spline curve defined by n nodes,
l a linear segment,
l a user-defined curve.
l a circular arc
Buttons Add and Insert allow to respectively add an element at the end and the beginning of the
list. An existing element may also be split.
The slope continuity is not ensured for composite curve.
Selecting an element then allows to modify its settings like the type, the amount of parameters
(Bezier and spline elements) or the related external data file (user-defined element), as illustrated
in FIGURE 3.7.
Tangency constraint is also possible at start or end of an element for most types, but is undefined
between a linear and a user-defined elements. Checking a tangency constraint will automatically
increase the amount of nodes (spline curves) or control points (Bezier curves) as needed.
Each element, once selected, can be edited in the Curve parameters area of the menu (bottom
area in FIGURE 3.7).
Parameter
HUB_Z(i)
HUB_R(i)
SHROUD_Z(i)
SHROUD_R(i)
Description
Z coordinate of the (i)th node of hub curve
R coordinate of the (i)th node of hub curve
Z coordinate of the (i)th node of shroud curve
R coordinate of the (i)th node of shroud curve
In the interface, the composite curve can be edited as a whole: any control point or node can be
picked and moved.
Third order Bezier curve
FIGURE 3.8
Bezier 4 curve
This 3rd order degree Bezier curve is controlled by eight parameters, namely positions at both
ends, length and angular direction of the first and last control segments. These parameters define
the location of the four nodes controlling the curve.
Parameter (hub curve)
Description
HUB_Z1
HUB_R1
Z coordinate of the first endpoint
R coordinate of the first endpoint
HUB_ALPHA1
angle of the first control segment above Z axis (in degree)
Parameter (hub curve)
Description
HUB_L1
HUB_Z2
HUB_R2
length of the first control segment
Z coordinate of the second endpoint
R coordinate of the second endpoint
HUB_ALPHA2
angle of the last control segment above Z axis (in degree)
HUB_L2
length of the last control segment
Similar parameters exist for the shroud endwall
3.1.2
Stream Surfaces & Spanwise Location
This second step menu defines the stream surface type, the rulings and the spanwise location of
their traces in the meridional plane (FIGURE 3.9). The primary sections are defined on these
stream surfaces which should therefore be defined before the blade sections.
FIGURE 3.9
Setup of the stream surfaces
A. Surface Setup
The designer can choose between planar, cylindrical, conical and hub to shroud interpolation
surfaces. All surfaces except planar type are obtained by revolution of a trace around the Z axis.
According to the chosen type, one or more settings among X, Z, R and α are prompted for the
reference traces near hub and shroud. Those reference curves are defined respectively as the
spanwise locations "0" and "1".
According to the chosen stream surface type, several construction planes for the blade sections
,θ) planes properties are described in Camber
will be available. (Z,Y), (m,R*θ), (m,β) and (
Curve Definition.
Cascade topology and rounded tip configuration can be managed in the section Special options.
X, Z, R and α values are not parameters but static data. Their value is not accessible in the
Parameters menu and are not allowed to vary within an optimization.
Planar Axial Surfaces
Planar stream surfaces allow the 2D blade sections to be defined in the (Z,Y) plane. This plane is
located at a constant height X above the axis of rotation. Therefore, a value of X is required to
define the height for both hub and shroud. This is useful for axial turbomachinery.
Parameter
Description
REF_TRACE_HUB_R
height of the reference stream plane trace at hub
REF_TRACE_TIP_R
height of the reference stream plane trace at shroud
FIGURE 3.10
Planar stream surfaces traces definition
Planar Radial Surfaces
Pure radial surfaces can be defined as planes parallel to (X,Y). The usual construction planes are
then (
,θ) and (m,β).
A Z value is required to define the reference traces at hub and shroud.
The streamwise orientation can be changed by means of the switch Orientation from the menu.
However, the default value is usually correct when the endwalls have been defined from inlet to
outlet.
Parameter
Description
REF_TRACE_HUB_Z
coordinate of the reference stream plane trace at hub
REF_TRACE_TIP_Z
coordinate of the reference stream plane trace at shroud
FIGURE 3.11
Radial stream traces
Cylindrical Surfaces
Cylindrical stream surfaces allow the 2D blade sections to be defined in the (m,R*θ) and (
,θ) planes. The reference surfaces are defined at a constant radius R with respect to the axis of
rotation at hub and shroud. This is a useful option for axial turbomachinery.
The streamwise orientation can be changed by means of the switch Orientation from the menu.
However, the default value is usually correct when the endwalls have been defined from inlet to
outlet.
Parameter
Description
REF_TRACE_HUB_R
R coordinate of the hub reference stream cylinder trace
REF_TRACE_TIP_R
R coordinate of the tip reference stream cylinder trace
Conical Surfaces
Conical stream surfaces allow the 2D blade sections to be defined in the (m,R*θ), (m,β) and (
,θ) planes. A reference point (Z,R) and the half cone angle are needed for each of the two
reference traces. The Z axis is the axis of revolution. The half cone angle, α, can be positive (hub
case in FIGURE 3.12) or negative (shroud case in FIGURE 3.12).
FIGURE 3.12
Conical stream surfaces traces definition
Parameter
Description
REF_TRACE_HUB_Z
Z coordinate of the reference point for span = 0
REF_TRACE_HUB_R
R coordinate of the reference point for span = 0
REF_TRACE_HUB_ALPHA
half cone angle (in degrees) for conical surface for span = 0
REF_TRACE_TIP_Z
Z coordinate of the reference point for span = 1
REF_TRACE_TIP_R
R coordinate of the reference point for span = 1
REF_TRACE_TIP_ALPHA
half cone angle (in degrees) for conical surface for span = 1
Linear Interpolation Surfaces
This case does not require user input since the two reference stream surface traces at spanwise
locations 0 and 1 are respectively the hub and the shroud endwall curves (FIGURE 3.13). This is
the quickest and most convenient choice since the surfaces update automatically after an endwall
,θ)
curve adjustment. This type of stream surface is compatible with (m,R*θ), (m,β) and (
construction planes, but do not allow all stacking options . Hub to shroud direct
interpolation is compatible with both axial and radial
turbomachinery. Usually, this option is the typical choice for radial turbomachinery. This option is
not appropriate for two-dimensional blades defined by means of one single primary section.
FIGURE 3.13
Stream surfaces traces definition by linear interpolation
Custom Interpolation
The custom interpolation allows the user to define the stream surface traces based on an
interpolation grid with a control on the grid points, the initial hub/ shroud distribution and the
smoothing. This type of stream surface has the same restriction as the linear interpolation
approach.
Setting
Description
Hub/Shroud
BC
when smoothing active, either the grid points are fixed on hub and/ or shroud (fixed mode)
or they are allowed to move on the hub and/or shroud curve (on curve mode)
Curvature
weight
the grid point distribution from uniform (0) to curvature (100)
Precision
the number of grid points along the hub and the shroud
Smoothing
the number of smoothing steps
Weight
factor
when smoothing active, the higher the weight factor is, the more freedom is given to the
grid points movement
FIGURE 3.14
Stream surfaces traces definition by custom interpolation
The grid used to build the stream surface traces is displayed with the View/Show stream grid
menu.
Special options
Cascade topology
The button Cascade topology allows to activate the construction mode for cascade topology. The
cascade mode is only available for blades defined on planar axial surfaces in (Z,Y) construction
plane. Splitters are also supported.
The menu Geometry/Export as geomTurbo is limited to geomTurbo 5.3 format in cascade mode.
Non axisymmetric hub / shroud are not available.
Hub and shroud curves must be defined with positive radius: the Z axis cannot be taken as hub curve.
In cascade mode, a new parameter 'CASCADE_PITCH' is used to control the distance between
blades (pitch). The parameter 'BLADE_ROTATION' is disabled. The parameter 'NB' will be the
number of repetitions for 3D view and CAD export. Blades are repeated with translation along Y
axis instead of rotation around Z axis.
Parameter
Description
CASCADE_PITCH
Pitch value for the cascade periodicity
Rounded tip configuration
The rounded tip configuration is entirely controlled from the stream surfaces menu. The method
consists in performing a single loft with a degenerate profile at tip (point).
The inputs parameters are:
l A single span value for the degenerate tip section. This information is used with the stacking
and lean laws to automatically define the exact 3D tip point location. This value is parametric,
as regular span values for primary sections,
l Two clamp factors corresponding to the reference magnitudes (two scalar values), a main for
the long direction, a secondary for the short direction,
l The number of intermediate imprints on each side (single integer), with a minimum of 0,
leading to two vectors (one at leading edge, one at the trailing edge).
FIGURE 3.15
Rounded tip settings
The feature is applicable under the following restrictions:
l Only available for axial machines without splitters (axial planar, cylindrical and conical stream
surfaces only);
l Partial and double blunts are not supported;
l Leading edge and trailing edge stacking points are not suitable. Meridional edge traces can also
not be used (sweep and lean only);
l Not compatible with ruled surfaces;
l Not compatible with discretized sections (only primary and parametric sections are allowed);
l Not compatible with native geomTurbo format. The fitting cannot retrieve the tip point position if
edge curves are not defined. Also, only CAD output (Parasolid) is possible as export format for
the geomTurbo data;
l The tip point location is not fitted. It is a user input.
B. Rulings (for flank-milled blade only)
When activating Activate rulings, the ruling direction for flank-milled blades (i.e. centrifugal
impellers) can be controlled, by means of simple sampling of the two camber curves and an
interactive definition of the links between those samples in the meridional view. The resulting
geometry is built with Parasolid™.
FIGURE 3.16
Ruling control for flank-milled blades
The ruling directions are straight links between samples defined on the two cambers. This
treatment requires the definition of the cambers, but not the side curves, that will be built just after.
For clarity and ease of management, exactly two primary sections are required and no parametric
sections are allowed for controlled ruling.
Imprint directions on side surfaces allows to visualize the ruling directions on the 3D model.
In the Configuration of the stream surfaces dialog box, links can be quickly reset. For instance,
it is possible to select 50 samples and generate 9 links between the two cambers, just by activating
Reset rulings. By default, the ruling consists in a uniform sampling in (m,R*θ) over the two
primary camber curves and links between some of these samples. The user can also apply a
clustering (uniform-geometric) in case of a rounded edge. The clustering will apply an uniformly
distributed samples near the middle of the camber traces and a geometric progression near the
edges. The Global ratio is defined as the edge spacing over the central spacing between the
samples.
Clustering is only applied in the vicinity of a rounded edge. If the edge is blunt, an uniform spacing is
automatically applied.
After generating the links, the leading and trailing edges are fixed links but any intermediate link
can be added or deleted when right-clicking in the meridional view and selecting Edit rulings
settings for main blade.
FIGURE 3.17
Ruling settings
l Reset links and samples allows to modify the number of nodes and links.
l Modify sampling allows to modify the sampling and update the previous links to start and end
on the closest samples.
l Refine sampling allows to insert intermediate samples by changing the Number of internal
samples without losing the previous sampling.
The nodes and links are visualized in the meridional view when right-clicking in the view and
selecting Edit main blade ruling links . The link nodes can be picked and can be set to another
node by left-clicking.
FIGURE 3.18
Ruling links interactive control
C. Spanwise Locations
Spanwise locations of the stream surfaces traces are controlled by the means of the span
parameter. In the cylindrical case (FIGURE 3.19), two radius values are necessary to define the
reference stream surface traces, one near the hub (Rhub) and another near the shroud (Rtip). Those
two radii represent respectively the spanwise locations "0" and "1" and are usually chosen to
mimic the hub and shroud curves.
FIGURE 3.19
The span parameter applied on cylindrical stream surfaces
As soon as the two reference surfaces are defined, any intermediate stream surface is obtained by
interpolation of the reference traces radii using the span parameter, which is defined as a
normalized location between the trace at hub (0.0) and the trace at tip (1.0).
For linear interpolation surfaces, intermediate stream surfaces are built using interpolation of
points from start to end, as shown in FIGURE 3.20. The linear formula is a generalization of the
interpolation law for points in the meridional (Z,R) plane. This law is actually applicable to every
stream surface type.
FIGURE 3.20
Application of the span parameter for interpolation of the stream surfaces
There is no direct link between endwall curves and planar, cylindrical or conical stream surfaces, so
that none of the defining X, Z, R and α change after an endwall curve adjustment. On the contrary,
hub to shroud interpolation surfaces are linked to the endwall curves and are updated automatically.
D. Stream Surfaces Spanwise Location
Two types of parametric blade sections are available and can be used simultaneously: primary and
parametric 2D sections. For each section, a supporting stream surface is defined by interpolation
or extrapolation of the reference traces defined above.
Number and spanwise position of both types of sections can be input by the user. Spanwise
locations usually range from 0.0 (hub) to 1.0 (shroud), but values between -0.5 to 1.5 are accepted
by the modeller.
FIGURE 3.21
The spanwise location of the stream surfaces
Primary Sections
Primary sections are the defining 2D sections of the blades. All primary sections within a given
project are described by the same set of parameters such as a camber stagger angle, a prescribed
thickness distribution, leading edge radius, etc. These sections share common topological settings
but the values of the involved parameters vary independently from one section to another.
Parametric Sections
Parametric sections are computed by interpolation or extrapolation of the primary sections
parameters. All parameter values are automatically generated with the help of the span parameter
and values of the corresponding parameter for the primary sections. Interpolation laws are
explained in the next paragraph. The purpose of the parametric sections is to refine the output data
transferred to the mesh generator. This is for instance essential in case an optimization of the
stacking laws is performed whereas the blade shape is defined by means of a limited number of
primary sections.
Parametric sections are optional, except when only one primary section is defined. In this particular
case, a constant extrapolation applies for all section specific parameters.
The use of parametric sections can lead to invalid blades in optimization projects. It is generally a
good idea to discard them (or to use polyline instead of spline interpolation) when parameters are
allowed to vary over a large range, because some unrealistic values of the parameters (such as
negative leading edge radius) may result from the interpolation process!
Parameter Interpolation
Each primary blade section is defined by a set of parameters. The value of every parameters on
every primary sections is defined by user input, but the value of the corresponding parameter on
any parametric section is interpolated. The preferred interpolation type is selected by means of the
two buttons:
l Polyline
l Cubic spline
FIGURE 3.22 assumes that four primary sections are defined at spanwise locations {0, 0.3, 0.7,
1} and two parametric sections at spanwise locations {0.5, 1.2}. If the parameter is the stagger
angle for instance, the angular value of this parameter is precisely defined for each primary section
and the value of the stagger angle can be seen as a function of the spanwise location. Therefore, a
spline (or a polyline) can be built through the points (span value, parameter value) from every
spanwise location of the set. The value of the stagger angle of the first parametric section is
interpolated from this curve: to the given value 0.5 of the span parameter corresponds one value
of the stagger angle.
FIGURE 3.22
Interpolation laws (cubic spline and polyline)
According to the number of primary sections, interpolation laws behave differently:
l if only one primary section is defined, all parametric sections will have identical defining
parameters whatever interpolation type is selected: this is the constant interpolation case.
l if only two primary sections are defined, values are interpolated with the help of a linear law
whatever interpolation type is selected. Extrapolation is also linear.
l if three or more primary sections are used, interpolation differs according to the type
selected. Extrapolation is always linear below 0 and above span 1, so that the interpolation
curve remains continuous up to the first derivative at span 0 and 1. This case is depicted in
FIGURE 3.22.
least
At
parametric section exists to allow constant blade profiles.
two primary sections are usually required. A special case with one primary and one
Spanwise location differences among primary and parametric sections should be more than the built-
in tolerance or AutoBlade™ will discard duplicate values automatically. The smallest valid difference
between two span values is 0.01.
As explained in the Export Options , discretized sections are direct
interpolations of point
coordinates from primary and parametric sections. Hence those sections do not need a supporting
surface.
E. Views
Stream surfaces are shown in the meridional view (upper left viewport) for primary sections only,
but are defined for parametric sections too. The location of the parametric sections can be noticed
in the 3D View of the blade.
3.1.3
Blade Meridional & Tangential Locations
It is common, in the turbomachinery community, to define the position of the 2D blade section on
a stream surface with respect to a reference point - the stacking point. This point is first defined
on the 2D blade section, then positioned on the corresponding stream surface in the meridional
and tangential directions based on two independent stacking law definitions.
FIGURE 3.23
Stacking point choice in the Locations menu
The menu consists in three pages that define:
1.
2.
the stacking point, defined on the 2D blade sections.
the meridional location law, defined in the (Z,R) plane, which can be either a sweep law
curve that defines the meridional trace of the stacking point or leading and trailing edges
traces that define the meridional limits of the leading and trailing edges of the blade section.
3.
the tangential location law for the stacking point, defined using a lean law curve. This curve is
built in the (span,θ) plane.
Optional splitters are positioned relative to the main blade. Therefore, the meridional and tangential
location menu affects the main blade sections only.
A. Stacking Point
Seven choices are available for the stacking point: leading edge (LE), trailing edge (TE), centre
of gravity (CG), maximum thickness (MT), centre of channel (CC), on camber (CA) and on
chord (CH) as depicted in FIGURE 3.23.
The centre of gravity is computed as the geometrical centre of the blade section in its
construction plane .
Point of maximum thickness is the point on the blade section mean line for which the maximum
thickness is found. The mean line can be defined as the average curve dividing the blade section
in such a way that the distances from one of its point to suction and pressure sides in the
perpendicular direction are the same.
The centre of channel is the point, halfway between two successive blades, where the minimum
channel width is achieved. For further details about the channel computation see also "Sampling"
(p. 218). This stacking point is only meaningful for axial machines.
A relative position of the stacking point is specified when defined on camber or on chord.
Centre of gravity, maximum thickness and centre of channel should be selected for axial or
nearly axial machines only.
When the leading edge or trailing edge is blunt, the stacking point is the mean point of the side edge
points.
B. Meridional Location
AutoBlade™ provides two methods to define the location of the blade sections in the meridional
view. They are the sweep law curve and the leading and trailing edge traces.
Sweep Law Curve
This method consists in defining a stacking curve in the meridional view that will extend from
hub reference trace (span value 0.0) to shroud reference trace (span value 1.0). AutoBlade™ is
then able to align the selected stacking point of the 2D sections along this sweep curve.
FIGURE 3.24
Sweep law menu
The curve is not constructed directly in the (Z,R) plane, but in a non dimensional construction
(z,span) plane ( FIGURE 3.25 ). The following formula is applied to compute the stacking
locations in the (Z,R) plane, ZRef being the origin of the sweep curve (Origin) on the hub or on
the shroud reference trace (Z_stacking_sweep in the list of parameters). The major interest of this
transformation is that angles are preserved.
FIGURE 3.25
Stacking sweep law definition
When a span parameter value lies outside of the interval [0,1], a linear extrapolation is applied and
continuity is assured up to the first order (C1, continuity of the first derivative with respect to the
span parameter).
Five curve types can be used to achieve the sweep law:
Line
A line is advantageous when the stacking is straight or linear: in optimization, this law involves a
single angular parameter β (FIGURE 3.26, left) and ensures a perfect linear stacking if more than
two primary sections are defined.
Second order Bezier curve (3 control points)
This simple law is a second order Bezier curve defined by three control points respectively at span
0.0, 0.5 and 1.0. The three user defined parameters are axial reference position at hub ZRef, angles
β1 and β2. In our example (FIGURE 3.26, center), angle β1 is negative and angle β2 is positive.
Composite Bezier - line - Bezier curve
The alternative is a composite Bezier-line-Bezier curve. The Bezier curves are second order
curves joined together with a straight line segment. The first control polygon is defined by
parameters C1, P1 and angle α1, the second by (C2,P2,α3) and line angle α2 is common to both to
assure C1 continuity (FIGURE 3.26, right).
FIGURE 3.26
Available sweep laws
All angles are measured clockwise from a line at constant z.
Parameter
Description
Z_STACKING_
SWEEP
Line:
Z value for the stacking point on stream surface at span = 0 (close to hub) or
span = 1 (close to shroud)
SWEEP_BETA
angle β of the line (in degrees)
Second order Bezier curve (3 control points):
SWEEP_BETA1
angle β1 of the Bezier curve at span = 0 (in degrees)
SWEEP_BETA2
angle β2 of the Bezier curve at span = 1 (in degrees)
Bezier-line-Bezier composite curve:
SWEEP_ALPHA1 angle α1 of the first Bezier curve at span = 0 (in degrees)
SWEEP_C1
spanwise extent of the first Bezier curve
SWEEP_P1
fractional factor defining the second control point location of the first Bezier curve
SWEEP_ALPHA2 angle α2 of the linear segment (in degrees)
SWEEP_ALPHA3 angle α3 of the second Bezier curve at span = 1 (in degrees)
Parameter
Description
SWEEP_C2
spanwise extent of the second Bezier curve
SWEEP_P2
fractional factor defining the second control point location of the second Bezier
curve
Bezier & B-spline curve defined by an arbitrary amount of nodes
Wind turbines are defined by more complicated shapes and controlling their stacking requires a
larger amount of sections. In release AutoBlade™ 2.1, the more general stacking law is a
composite Bezier-line-Bezier curve that allows a perfect stacking (sweep and lean) for 5 to 7
sections. This is clearly insufficient for wind turbines blades, where 10 to 15 primary and
parametric sections may be necessary for good control of shape and stacking. Therefore, a new
and more general stacking law has been added.
The proposed law is either a Bezier or a B-spline curve defined by an arbitrary amount of nodes
along the span (Number of parameters).
FIGURE 3.27
Stacking Law: Meridional location control
To simplify the optimization, only the Z or θ coordinate is parametric (Hi), the nodes being by
default equally spaced along the span (left picture in FIGURE 3.28). In addition, this distribution
can be stretched along the span by means of a geometric or twice_geometric progression where
the ratio are defined (first/second common ratio).
FIGURE 3.28
Sweep law ruled by a geometric progression (left picture) and all the distribution types available
(right pictures)
The geometric progression (left picture in FIGURE 3.28) will always lead to an asymmetrical
distribution of the points while the twice_geometric may lead to a symmetrical distribution when
imposing the same stretching factor (first/second common ratio).
Leading & Trailing Edges Traces
Edge traces fully constrain both the meridional location and the extent of the blade sections. Edge
traces need two end points and the curve is built directly in the meridional plane (Z,R). This
method does not make use of the stacking point because the traces completely define the blade
sections in the meridional view.
The end points of each trace are defined using either a coordinate - Z or R - on hub and shroud
curve or a non dimensional location measured along the endwalls.
FIGURE 3.29
Leading and trailing edges traces menu.
Parameter
Description
End points defined by coordinates:
Z_LE_HUB / R_LE_HUB
Z or R starting coordinate for leading edge on hub trace
Z_LE_SHROUD / R_LE_SHROUD
Z or R starting coordinate for leading edge on shroud trace
Z_TE_HUB / R_TE_HUB
Z or R starting coordinate for trailing edge on hub trace
Z_TE_SHROUD / R_TE_SHROUD
Z or R starting coordinate for trailing edge on shroud trace
End points defined by a fractional length along the endwall curve:
S_LE_HUB
S_LE_SHROUD
S_TE_HUB
S_TE_SHROUD
end point location along hub curve for leading edge
end point location along shroud curve for leading edge
end point location along hub curve for trailing edge
end point location along shroud curve for trailing edge
Five laws are available to define each trace. Traces are extrapolated linearly when spanwise
locations below 0.0 or above 1.0 are requested or when reference traces differ from endwall
contours.
Parameterless line
A linear trace free of parameters can be selected as the simplest law FIGURE 3.30 (top picture).
This is the default.
Second order Bezier curve (symmetric)
Leading and trailing edge traces are defined by means of a second order Bezier curve controlled
by three points. User input is simplified by the assumption that both control segments have the
same length and therefore, only one additional angular parameter βLE or βTE is necessary.
On FIGURE 3.30 (bottom left picture), βLE is defined as the angle between:
1.
the segment joining the intersection points of the edge trace with hub and shroud curves,
2.
the first control segment of the edge trace.
This angle is measured clockwise and a similar definition applies for the trailing edge curve.
Third order Bezier curve
The above law is indeed very simple and does not comply with all topologies.This second curve
is controlled by four points and allows more freedom, especially when the trace is not symmetric.
It requires four additional parameters, as depicted in the bottom right picture of FIGURE 3.29.
FIGURE 3.30
Meridional blade passage definition using edges traces
Parameter
Description
Second order Bezier curve:
Parameter
Description
LE_MERIDIONAL_BETA
angle βLE controlling the leading edge trace (in degrees)
TE_MERIDIONAL_BETA
angle βTE controlling the trailing edge trace (in degrees)
Third order Bezier curve:
LE_MERIDIONAL_BETA1
angle β1 controlling the LE control segment near hub
LE_MERIDIONAL_C1
projected fractional length of LE control segment near hub
LE_MERIDIONAL_BETA2
angle β2 controlling the LE control segment near shroud
LE_MERIDIONAL_C2
projected fractional length of LE control segment near shroud
TE_MERIDIONAL_BETA1
angle β1 controlling the TE control segment near hub
TE_MERIDIONAL_C1
projected fractional length of TE control segment near hub
TE_MERIDIONAL_BETA2
angle β2 controlling the TE control segment near shroud
TE_MERIDIONAL_C2
projected fractional length of TE control segment near shroud
Bezier & B-spline curve defined by an arbitrary amount of nodes
The proposed law is either a Bezier or a B-spline curve defined by an arbitrary amount of nodes
along the span (Number of parameters).
FIGURE 3.31
Stacking Law: Meridional location control
In addition,
progression where the ratio are defined (first/second common ratio).
this distribution can be altered by means of a geometric or twice_ geometric
C. Tangential Position
The lean curve types are very close to those (five types) introduced in the Meridional Location
section for the sweep law. The tangential law defines θ as a function of the span parameter value.
This coordinate system has been chosen because a purely radial law is easily defined by setting
the angular parameters to 0.
The lean law is defined between 0.0 and 1.0 but linear extrapolation is allowed for other span
values.
Usually, sections can be rotated by means of the parameter BLADE_ROTATION and the lean law
has its origin at θ=0 (left picture in FIGURE 3.32). There is an exception however: when planar
axial stream surfaces are used, the lean law requires an additional degree of freedom because the
sections do not rely on axi-symmetric surfaces (right picture in FIGURE 3.32).
Therefore, an additional angular parameter LEAN_OFFSET is added to the lean law parameters
when planar axial stream surfaces are defined (FIGURE 3.33).
The computed angle θ is plotted in radians, not in degrees. This is an exception.
FIGURE 3.32
BLADE_ROTATION parameter allows the rotation of the model
FIGURE 3.33
Three of available lean laws, defined in (span,θ) plane with special offset
Parameter
Description
LEAN_OFFSET
special offset angle for the lean law applied to planar axial stream surfaces (in
radians)
Line:
LEAN_BETA
angle β of the line (in degrees)
Second order Bezier curve (3 control points):
LEAN_BETA1
angle β1 of the Bezier curve at span = 0 (in degrees)
LEAN_BETA2
angle β2 of the Bezier curve at span = 1 (in degrees)
Bezier-line-Bezier composite curve:
LEAN_ALPHA1
angle α1 of the first Bezier curve at span = 0 (in degrees)
LEAN_C1
LEAN_P1
spanwise extent of the first Bezier curve
fractional factor defining the second control point location of the first Bezier
curve
LEAN_ALPHA2
angle α2 of the linear segment (in degrees)
LEAN_ALPHA3
angle α3 of the second Bezier curve at span = 1 (in degrees)
LEAN_C2
LEAN_P2
spanwise extent of the second Bezier curve
fractional factor defining the second control point location of the second Bezier
curve
3.1.4 Main Blade
Once their stacking point and extent is defined, the primary blade sections can be constructed and
placed on the stream surfaces.
In AutoBlade™, the splitter blades are optional and their definition is always relative to the main
blade. Therefore, splitter blades are covered in a separate menu (Optional Splitters).
Any blade section is built from a camber curve in a prescribed 2D construction plane. According
to the stream surface type, the designer can choose between several construction planes and curve
types. AutoBlade™ then provides two distinct methods for the construction of the full blade
contour:
l Suction side and pressure side mode: independent suction and pressure sides are constructed
from the camber line using Bezier curves. In general, this method is used for axial turbine and
axial compressor blades.
l Camber and thickness mode: a thickness distribution is applied along the camber curve from
leading edge to trailing edge. This method is very common in centrifugal turbomachinery
design.
It is also possible to specify blunt leading and trailing edges.
A. Construction Plane
FIGURE 3.34
Reference length & Construction plane
Reference length
When a sweep law is defined, the modeler can not evaluate the meridional blade passage simply
by stacking the blade sections on the sweep curve because the blade section length is unknown.
According to the stream surface type, up to three camber length types are possible:
l Z: an axial length DZ is a common choice in axial turbomachinery (planar and cylindrical
stream surfaces).
l R: a radial extend DR is useful
in centrifugal
turbomachinery (hub to shroud linear
interpolation and conical stream surfaces).
l m: a meridional DM length. This is the safest choice since the parameter m always increases
along the stream surface traces. On the contrary, Z and R coordinates do not always increase
from inlet to outlet.
The meridional length is not interfaced graphically and can be modified either in the Stacking
laws menu or in the Parameter list window.
Parameter
Description
S(i)_DZ_prim
(i)th section length along Z axis for blade length type 'DZ'
S(i)_DR_prim
(i)th section length along R axis for blade length type 'DR'
S(i)_DM_prim
(i)th section length along m axis for blade length type 'DM'
When the meridional location is defined using edges traces, no reference length is available. The
meridional length DM is not available for axial stream surfaces since DZ and DM values are equal.
If the modeller does not succeed in applying a DZ or DR length, please make sure your reference
lengths are not too close to zero or out of the machine reference dimension. If this does not solve the
problem, try a DM length.
Furthermore, the user can select either meridional chord or true chord. This choice enables the
merge of the new method (true chord) with the classic coordinate choice previously available in
the Meridional location page under the Stacking laws menu within AutoBlade™ 2.1.
In the page Construction plane, True chord is unavailable:
l when Leading and trailing edges traces are selected, where the meridional chord is assumed
and automatically managed (usually for radial blades),
l when planar radial stream surfaces are selected, since the chord has no meaning.
When the Meridional chord method is selected, the available construction planes are simply the
same as in release 2.1. When True chord is selected, the construction planes are identical, except
that (m,β) is never accessible since it is not compatible with the definition of a chord.
The list of available construction planes compatible with the True chord option is summarized
below and depends on the stream surface type and the stacking point choice.
TABLE 3.2 Compatibility table for sweep law option and true chord based profiles
Since (Z,Y) and (m,Rθ) planes are dimensional, the chord can be built directly from its length, so
these planes are the preferred choices for axial blades.
For enlarged compatibility, (
,θ) plane will be available, but the chord length has no direct
meaning with these coordinates. However, in pure axial cases with cylindrical stream surfaces for
,θ) multiplied by the radius of the
instance, the true chord is simply the prescribed length in (
cylinder.
Construction plane
Up to four construction plane options are available for the definition of the camber curve and their
properties are briefly explained in the following table.
TABLE 3.3 Construction planes for camber curve
Plane Description
(Z,
Y)
The camber curve is directly built in planar coordinates (Z,Y) and translated on the stream
surface.
(m,
R*θ)
The camber curve is built in (m, R*θ) plane and is then applied on the stream surface. It is often
preferred for axial turbomachinery, where distances are preserved.
(m, β) β is the prescribed angle, expressed in degrees, for the camber curve in (
, θ) plane. The
distribution of β is generated, then integrated to obtain θ. The latter angle is stored on the stream
surface.
(
The camber curve is built in the (
, θ) plane and translated on the stream surface. This is an
angle conservative plane often preferred for radial turbomachinery.
, θ)
The (Z,Y) plane is specific to axial planar stream surfaces while (m,R*θ), (m,β) and (
,θ)
planes are compatible with revolved stream surfaces.
For axial topologies dimensional planes (Z,Y) or (m, R*θ) are often preferred while radial blades
are usually described using either (m, β) or (
, θ) plane.
When previous settings do not allow a construction plane for some reason, the choice is disabled
in the interface. Please refer to Topological Compatibility Issues for further details.
When conical or interpolated stream surfaces are active, AutoBlade™ is not aware of the exact type
of machinery (axial, centrifugal,...). Users are therefore not prevented from choosing (m,R*θ) with a
radial topology, while the (m,R*θ) plane only preserves distances when the radius R can be assumed
constant over the whole section.
In such a case, the prescribed thickness is not preserved in thickness addition mode and edge radii
are not preserved in suction and pressure side mode.
The good practice with radial topologies is therefore to define the camber curve either in (m, β) or
(
, θ) together with a thickness addition.
B. Camber Curve Definition
The camber curve is constructed in a dimensional plane using either the given reference length or
meridional extent. It is then applied on the stream surfaces with the help of a transformation to
meet the stacking point requirement.
FIGURE 3.35
Camber curve definition
The camber curve must be a pure function of the construction abscissa. It is not possible to build
camber curves like the ones shown in FIGURE 3.36. If such a case occurs, AutoBlade™ may
apply a correction to any inadequate parameter value or bound set by the user. A warning or an
error message is generated to point out the problem.
FIGURE 3.36
Invalid camber curves
TABLE 3.4 Camber curve types
Meridional Chord Based Cambers
Bezier curve defined by n control points
The n control points are by default equally spaced in the abscissa interval (Z, m or
coordinate), the first point being placed at origin (0,0). The user can adjust the number of
parameters from 1 to any higher integer and change the distribution of the points (uniform,
geometric and twice_geometric) by imposing the stretching factor (first/second common ratio).
When selecting the geometric distribution, imposing a ratio from 1 (for uniform intervals) to a
factor bigger/lower than 1 will result in increasing/decreasing intervals from leading to trailing
edge (asymmetrical points distribution).
The simplest case 1 corresponds to a linear segment (2 control points). The formula linking the
number of control points to the number of parameters appearing in the interface is, taking into
account that the first control point is always located at the origin,
number of control points = number of parameters S(i)_CAMBER_H(j) + 1
Thanks to the simplified way to manage control points, only (n-1) ordinates S(i)_CAMBER_H(j)
must be specified in the parameters menu (FIGURE 3.37, left). Values can be negative. This
curve is not compatible with the (m,β) construction plane.
Cubic B-spline curve defined by n control points
The spline case is very similar to the Bezier case explained above, except that the curve passes
through the given points instead of being controlled by them (FIGURE 3.37, right).
FIGURE 3.37
Bezier & B-spline curves defined by equally spaced nodes
Parameter
Description
S(i)_CAMBER_H(j)
construction ordinate (j) for the camber curve of section (i)
Bezier using angles γ, β1 and β2
A simple second order Bezier curve can be used to define the camber line (FIGURE 3.38). The
first control point coincides with the leading edge at the origin and the last one with the trailing
edge. The relative position of the two edges is defined by the stagger angle γ. A third control
point is constructed from leading and trailing edges using respectively angles β1 and β2 . All
angles are measured in degrees from the abscissa direction.
This method is not compatible with the (m,β) construction plane.
Parameter
Description
SN(i)_STAGGER_ANGLE
the stagger angle γ (in degrees) for the camber curve of section (i)
S(i)_CAMBER_BETA1
inlet metal angle β1 (in degrees) for camber curve in section (i)
S(i)_CAMBER_BETA2
outlet metal angle β2 (in degrees) for camber curve in section (i)
FIGURE 3.38
Definition of the camber curve
The second order Bezier curve type calls for an additional comment: the stagger angle value is
accepted only if it lies between CAMBER_BETA1 and CAMBER_BETA2 values. This condition is
necessary to ensure the existence of a control polygon for the curve. This simple curve type cannot
show an inflexion point either (reversal of the sign in curvature values).
Integrated Bezier & B-spline curves
The special construction plane (m,β) requires a non zero starting angle and introduces its own
curves. the β distribution is defined by a similar curve to the one described above: it is built from
nodes equally spaced along the abscissa axis in the form of a Bezier or a B-spline curve.
Abscissa is the non dimensional interval [0,1] and can be interpreted as the length fraction of the
camber curve. The ordinate is the prescribed β angle expressed in degrees (FIGURE 3.39). The
camber curve is obtained by integration of this angle distribution on the stream surface according
to equation below.
Those curves are reserved to (m,β) construction plane.
FIGURE 3.39
Bezier distribution for an integrated camber curve.
Circle arc
A circle arc can be used to define the camber line. The arc is defined by start and end angles β1
and β2. This option is only available in axial planes (Z,Y) and (m,R*θ).
True chord based cambers
For True chord based profiles, four new curve types replace the usual curves in (Z,Y), (m,R*θ)
and (
,θ) planes as summarized in TABLE 3.7.
Simple Bezier curve
The simplest curve defined by a second Bezier curve is reused in a slightly different
parametrization. The stagger angle is kept, with an increased range [-180.0,180.0]. The two
relative angles δ1 and δ2 respectively replace the absolute metal angles β1 and β2 (FIGURE
3.40). The edge angles are still limited to 90 degrees, but the signs of δ1 and δ2 are always
opposite. This property ensures that no invalid topology may be generated in optimization if the
bounds of the δ1 are positive while those of δ2 are negative.
FIGURE 3.40
The classic second order Bezier curve defined based on meridional chord (left) and its new
definition based on true chord (right)
Bezier & B-spline curves where nodes equally spaced along the chord
The two types of curve use similar height parameters as with meridional chord. There are two
major differences:
l the last height parameter is dropped (curve end),
l the stagger angle is added to ensure the proper orientation of the camber curve.
FIGURE 3.41
Bezier curve defined by heights at uniformly spaced abscissa based on meridional chord (left) and
its new definition based on true chord (right)
Circle arc
A circle arc can be used to define the camber line. The arc is defined by start and end angles δ1
and δ2. This option is only available in axial planes (Z,Y) and (m,R*θ).
User-defined Camber Curve
The user-defined camber distribution is defined form a dimensionless abscissa, in the [0,1] range,
,θ) planes, the starting point
whatever the construction plane. In case of (Z,Y), (m,Rθ) and (
should be (0,0). In case of (m,β) plane, the ordinate is free.
User defined camber curve is not compatible with parametric sections.
Data file
If the camber distribution law is available as an external data file, it can be imported as a user-
defined law in the parametric model.
FIGURE 3.42
User-defined data file
The following controls allow to set the selected distribution:
1. The option Include points as parameters allows to include all reference points as regular
parameters for the fitting or the optimization. This means that the law can be initialized and
even altered by the fitting process!
2. The option Dimensional height specifies either if the ordinate must be considered as the
values read (checked) or if the provided law must be scaled by the length of the camber curve
(unchecked).
3. The option Height factor allows to scale the ordinate of the prescribed camber curve by
means of the optional floating point value (on the right side).
The user-defined camber distribution law can be defined in a simple text format, as illustrated in
the example below.
# comments
101 (amount of defining points)
0.0 0.0
0.01 0.01598
...
0.99 2.457
1.0 2.469
The first input number is the amount of provided points. Then, each line defines a single point. A
comment may be added anywhere provided that it starts the line with '#' character.
The abscissa should be increasing and cover the [0,1] range exactly in order to produce a valid
camber curve or wrap angle distribution. If the range is not fully covered, a warning is generated
and the distribution is internally adapted to match the starting and ending values.
FIGURE 3.43
Input user-defined camber distribution
The user-defined camber distribution can be only inputted by Right-clicking in the CAMBER
view, as shown in FIGURE 3.43.
In the Init curve from file dialog, The user can enter the path ended by a hit on the <Enter> key or
click the button on the right and use a classic file chooser. By default, no file is active and the
value in the field is none. Once selected, the file is parsed and checked: if the color of the field is
changed to red, this means that the file does not comply with the format specification described
above!
If the button Apply to all sections is checked, the inputted user-defined camber distribution will be
applied to all sections.
Expression
The camber curve can be defined by a mathematical expression involving a single parameter 's'
for each blade. In order to simplify the user input, this expression can use an existing function
with an arbitrary amount of arguments. For example, a user- defined expression is used in
FIGURE 3.44, where NACA4_CAMBER() is the user-defined function; s is a dimensionalized
abscissa along the chord and ranges from 0 to 1; M1 and P1 is the user- defined optional
parameters.
FIGURE 3.44
User-defined expression
A valid formula should always produce a zero ordinate for a zero abscissa except for the wrap angle
distribution. If the camber is defined using the chord, the ordinate should also be zero for abscissa 1.0.
If the law does not comply to these rules, it is internally altered to enforce the conditions.
C. Suction & Pressure Side Curves
This section allows the user to define the pressure and suction sides of the main blade.
AutoBlade™ assumes that the suction side is located above the pressure side when plotted against
an increasing θ angle.
FIGURE 3.45
Construction modes for side curves
These topological choices are described in the following order:
l independent suction and pressure sides (legacy - default),
l independent suction and pressure sides (regular),
l independent suction and pressure sides (throat-based),
l thickness addition (symmetric or not).
Suction & Pressure Sides Construction Mode - legacy
Both suction and pressure sides are constructed in the form of a high degree Bezier curve with
respect to the camber curve. Special treatments are performed to shape the leading and trailing
edges. This method is dedicated to axial turbines and axial compressors and is enabled through
the Construction curves option.
This construction mode is neither compatible with (m,β) nor (
,θ) planes, where angles are
involved. This limitation comes from the need for the side curves to be entirely defined in a
dimensional construction plane.
FIGURE 3.46
Topology menu for independent suction and pressure sides mode
The side curves are defined by a Bezier curve starting at the previously defined leading edge and
ending just before the trailing edge. The trailing edge is shaped with a circular arc in the rounded
case.
The construction of the suction side is depicted in FIGURE 3.47. The location of the Bezier
control points is determined as follows, in a rounded trailing edge case. Pressure side and blunt
edge cases will then be discussed.
FIGURE 3.47
Definition of the suction side curve
1. First, intermediate construction points are defined on the camber curve. The camber curve is
divided into a fixed number of intervals which can be of equal or variable length using a
stretching factor.
2. From each of these intermediate control points, a fractional
length TSS (j) is added
perpendicularly to the camber curve. This defines the position of the Bezier control points for
the side curve. Each TSS (j) is defined as a fraction relatively to chord length instead of
meridional chord (conversion is ensured for full backward compatibility with AutoBlade™
2.1).
3. A special treatment is performed at the leading edge. The first Bezier control point coincides
with the leading edge point and the position of the second control point is determined by the
following two conditions:
l the suction side curve must start perpendicularly to the camber line,
l the curvature radius RLE must be matched at the leading edge.
FIGURE 3.48
Construction of leading and trailing edges (rounded case). 11 control points and 7 user
defined parameters are used.
Taking into account the well known properties of Bezier curves, the locations of the first
two control points are constrained as follows (FIGURE 3.48):
l The first condition imposes that the second control point lies along a line perpendicular to
the camber curve at leading edge point.
l The second condition fixes the first control segment length as:
where RLE is the imposed curvature radius, n the amount of control points (n=11 in our
example) and b the distance between the point defined by TSS(1) and the first control
segment. In this formula, only the radius RLE is user defined since n and b depend on the
chosen number of intermediate control points and the stretching factor.
4. A special treatment is also performed at the trailing edge. To obtain the proper rounded shape
(case of FIGURE 3.48), two parameters are imposed by the designer: radius RTE and wedge
angle δte. The locations of the last two control points Cn-1 and Cn are constrained to meet both
continuity and the prescribed curve angle, just before the ending arc:
l The end point is common to Bezier curve and circle arc to ensure continuity of order 0.
l Building the last control segment tilted by half the wedge angle δte over the camber curve
and tangent to the circle ensures the right ending angle and the first derivative continuity.
The previous control point is thus defined as the intersection between the perpendicular line
from point 8 in our example and the last control segment direction.
In order to determine the amount of control points n, a simple relation can be established, where
the number of intermediate control points can be any integer greater or equal to zero:
n = 4 + number of intermediate control points
Our example (FIGURE 3.47) shows the curve obtained for order 10 (n=11) using 7 intermediate
control points and a stretching factor of 1.1. Ten parameters are needed: the fractional offsets TSS
(1) to TSS(7), the curvature radii RLE and RTE and the prescribed wedge angle δte.
This method allows the generation of suction and pressure sides that are highly continuous in the
leading edge region. The use of Bezier curves avoids pressure discontinuities along the blade walls
that could lead to boundary layer distortion or even separation. This is the reason why a circle or an
ellipse is not used to shape the leading edge. A circular arc for instance cannot ensure the continuity
of the high derivatives at its junction point with the Bezier curve, although the latter offers continuity
up to the derivative (n-1). This remark is not critical at trailing edge where a circular arc is used.
TABLE 3.5 summarizes the settings and parameters defining the side curves.
TABLE 3.5 2D blade profile definition (rounded case)
Setting
Description
amount of intermediate offsets to add between leading and trailing edges - amounts may
differ for suction and pressure sides.
number of
intermediate
control
points
Setting
Description
stretching
factor
ratio of two successive offset gaps from leading edge to trailing edge along the camber
curve - values may differ for suction and pressure sides. A stretching factor of 1 will give
uniform intervals while a factor bigger than 1 will result in increasing intervals from
leading to trailing edge
Parameter
Description
S(i)_LE_
RADIUS
S(i)_TE_
RADIUS
S(i)_TE_
WEDGE_
ANGLE
S(i)_TSS_
(j)
S(i)_TPS_
(k)
prescribed leading edge curvature radius RLE
prescribed trailing edge radius RTE
prescribed wedge angle δte
Suction side intermediate offset TSS(j) for section (i)
Pressure side intermediate offset TPS(k) for section (i)
Pressure side curve
Pressure side definition shares the same three parameters RLE, RTE and δte with suction side but
all other settings or parameters - amount of intermediate control points, stretching factor and
fractional offsets TPS(k) - are specific and may be different from the suction side.
FIGURE 3.49
Definition of the side curves (view 4)
Blunt cases
If a blunt trailing edge is requested, the Bezier curve is computed the same way, but no circular
arc is built. Two types of blunts are available (FIGURE 3.50):
l the normal blunt ( FIGURE 3.50 ,
left) is obtained by applying the R TE parameter
perpendicularly to the camber curve as an offset, so the location of the last control point differs
slightly from the rounded case.
l the constant m' blunt (FIGURE 3.50, right) is obtained from the normal blunt case above.
value for the side is
The side is then truncated or extended linearly so that the ending
the same as the trailing edge point. If the construction plane is (
,θ), the endpoints of the
side curves and the camber curve obviously share the same abscissa.
The number of intermediate control points expression is still applicable for a blunt trailing edge.
Normal (left) and tangential (right) blunt cases - sections are here plotted in (
, θ)
FIGURE 3.50
construction plane
Suction & Pressure Sides Construction Mode - regular
In the method described above, the suitable values of the involved parameters TSS(j) and TPS(k)
are not easy to estimate, especially the offsets near the leading and the trailing edges.
For instance, a low value of TSS (1) could generate a bad leading edge shape as shown in
FIGURE 3.51, where the curvature radius reaches a low local minimum just after the leading
edge point. This case can be avoided if the value of TSS(1) is larger than the length of control
segment
segment length, the user cannot guess when a given TSS value is suitable or not.
(FIGURE 3.51). Since the latter value depends on formula for the first control
FIGURE 3.51
Bad leading edge shape
A similar problem can occur near trailing edge.
A new set of parameters is provided to help the designer achieving valid topologies in an easier
way. This method is activated by pressing the button With end line in the Suction & Pressure
Sides section. In comparison with the classic construction mode, three intermediate parameters are
defined, one near the leading edge and two near the trailing edge, as shown in FIGURE 3.52.
FIGURE 3.52
Definition of the suction curve with an ending line (for 9 control points or 2 intermediate control
points)
The three following changes have been introduced for both suction and pressure sides. It is here
explained in the suction side context and a rounded trailing edge is assumed.
1. The first TSS parameter from the original method is replaced by an angle δle to ensure a better
control of the side curve near the leading edge (FIGURE 3.53, left). The control point C3 is
defined as the intersection between the prescribed direction issued from C2 and the line parallel
to the first control segment and passing through construction point 1. Angle δle should always
be positive and, thus, its lower bound is straightforward.
2. The (n-1) TSS parameter is replaced by a fractional offset
measured from the last control
segment direction
so the control point moves away from the camber curve when it is
positive and moves closer when it is negative. The definition of the fractional offset is similar
to the definition of the TSS parameters, but it starts from the last control segment direction
instead of the camber curve.
FIGURE 3.53
Leading edge (left) and trailing edge (right)
3. The suction side curve is optionally ended by a line segment. Continuity up to the first
derivative is ensured at both ends of that segment, at the junctions with the Bezier curve and
the circle arc. Length
is expressed as a fraction of the camber curve length in its construction
plane.
TABLE 3.6 2D blade profile definition (rounded case with end line)
Setting
Description
number of intermediate
control points
number of intermediate offsets to add between leading and trailing edges -
amounts may differ for suction and pressure sides.
stretching factor
ratio of two successive offset gaps on the camber curve - values may differ for
suction and pressure sides
Parameter
Description
S(i)_LE_RADIUS
prescribed leading edge curvature radius RLE for section(i)
S(i)_TE_RADIUS
prescribed trailing edge radius RTE for section(i)
S(i)_TE_WEDGE_
ANGLE
S(i)_SS_LE_
WEDGE_ANGLE
S(i)_PS_LE_
WEDGE_ANGLE
S(i)_SS_REAR_
SHAPE
S(i)_PS_REAR_
SHAPE
S(i)_SS_END_LINE
S(i)_PS_END_LINE
prescribed wedge angle δte for section(i) (in degrees)
prescribed wedge angle δle for the side curve of section(i) (in degrees)
prescribed fractional offset
for the side curve of section(i)
prescribed fractional length
of the ending line for the side curve of section(i)
S(i)_TSS_(j)
intermediate offset TSS(j) for suction side curve of section (i)
S(i)_TPS_(k)
intermediate offset TPS(k) for pressure side curve of section (i)
The number of control points n here becomes:
n = 6 + number of intermediate control points
Suction & Pressure Sides Construction Mode - throat-based
The throat based model is inspired from the Pritchard's eleven parameter model (Prichard LJ,
1985, "An eleven parameter axial turbine airfoil geometry model", ASME Paper 85-GT-219), but
will reuse some angles and curves from the existing topologies for construction curves. This
method is dedicated to axial turbines and is enabled through the Construction curves option.
The throat based model is defined as follows:
1. The camber curve is defined as a simple Bezier curve. It can be defined with absolute inlet and
outlet angles β1 and β2, or defined by the relative definition (δ1 and δ2). Please note however
that the stagger angle γ is not allowed to reach +/- 90 degrees for proper behavior.
2. The leading edge radius definition is included in the suction and pressure side curves with
control of the start radius.
3. The pressure side curve is defined as in construction curve with end line (regular), with a linear
part of zero length. This definition has the advantage to allow an angular control near leading
edge. Order of pressure side Bezier curve is at least four (5 control points) without TPS
parameters.
4. The suction side is defined from two Bezier curves. The leading edge part is at least of order
four (when no TSS parameters are available) and the trailing edge part is defined from a third
order Bezier curve (four control points) and is fully automatic once angles are defined. The
throat location in the blade-to-blade view passes through the center of the trailing edge circle.
FIGURE 3.54
Definition of the side curves for throat based model
TABLE 3.7 Parameter definition of the throat based model
Parameters
Description
span
NB
β1
εin
RLE
RTE
Spanwise location of the section
, where Ct is the tangential chord
Number of blades
Axial chord
Stagger angle.
Deviation angle
Inlet blade angle
Inlet half wedge angle
Leading edge radius
Trailing edge radius
β2
Exit blade angle
Throat width
The model does not ensure that the effective throat is located at the prescribed location if users try to
design a supersonic blade.
TABLE 3.8 2D blade profile definition (throat based model)
Setting
Description
number of
intermediate
control points
number of intermediate offsets to add between leading and trailing edges in the pressure
side and between leading edge and throat location in the suction side - amounts may
differ for suction and pressure sides.
stretching
factor
ratio of two successive offset gaps on the camber curve - values may differ for suction
and pressure sides
Parameter
Description
S(i)_LE_
RADIUS
S(i)_TE_
RADIUS
S(i)_TE_
WEDGE_
ANGLE
S(i)_
THROAT_
WIDTH
S(i)_DEV_
ANGLE
S(i)_SS_LE_
WEDGE_
ANGLE
S(i)_PS_LE_
WEDGE_
ANGLE
S(i)_PS_
REAR_
SHAPE
prescribed leading edge curvature radius RLE for section(i)
prescribed trailing edge radius RTE for section(i)
prescribed wedge angle δte for section(i) (in degrees)
prescribed throat width
prescribed deviation angle
prescribed wedge angle εin for the side curve of section(i) (in degrees)
prescribed fractional offset
for the side curve of section(i)
Setting
Description
S(i)_PS_
END_LINE
prescribed fractional length
of the ending line for the side curve of section(i)
S(i)_TSS_(j)
intermediate offset TSS(j) for suction side curve of section (i)
S(i)_TPS_(k)
intermediate offset TPS(k) for pressure side curve of section (i)
Camber & Thickness Construction Mode
The use of a thickness distribution in order to construct the pressure and suction sides from the
camber line is mainly used in the fields of centrifugal turbines, compressors and pumps.
The thickness distribution is constructed by means of a Bezier or a B-spline curve. The ordinate
values of the generated curve are exact half thickness values that are applied to the camber curve
on its both sides to obtain suction and pressure side curves.
FIGURE 3.55
Thickness addition mode
Two different thickness distributions can be applied on the sides of the camber curve. The
Symmetric option enables or disables the pressure side specific thickness distribution. The curve
type is however common to both distributions (FIGURE 3.56).
If the camber curve has been defined between edge traces or by means of the meridional chord,
the thickness distribution can be defined along the camber curve (S coordinate) or the meridional
chord (m coordinate). If the camber is defined by the chord length, the thickness distribution can
only be defined along the camber curve (the meridional chord could become negative).
The camber and thickness construction mode is compatible with all camber construction planes
contrary to the independent suction and pressure sides mode .
Using a thickness distribution defined along the meridional curve does not preserve the value of the
radius at edges. Therefore, the general definition along the camber curve is preferred.
In case of axial machines, (Z,Y) and (m,R*θ) construction planes preserve distances. The length of the
camber curve is straightforward and the blade section can be entirely constructed in these planes. This
,θ) planes because they don't preserve
is unfortunately not so easy for the conformal (m,β) and (
the distances, so the length of the camber curve is not known until the curve is projected on the
stream surface. For those planes, the construction of the blade section is still allowed in two steps:
1. First, the camber curve is constructed in (m,β) or (
,θ) plane and is then projected on the
stream surface, where the length of the camber curve can be computed.
2. Second, the thickness distribution is generated and applied along the projected camber curve,
directly on the stream surface.
FIGURE 3.56
Settings for camber and thickness mode
The thickness distribution can be built from three different methods (FIGURE 3.56 ). Their
definitions and related options are covered in the next pages:
l a single high order Bezier curve,
l a B-spline curve with optional ending circular arcs,
l a parameterless user-defined law.
In addition to the number of parameters, a points Distribution control (uniform, geometric or
twice_geometric) allows to alter the concentration of points which - by default - is uniform along
the definition axis. A stretching factor larger than one results in a higher concentration towards the
leading edge while a lower value moves that concentration towards the trailing edge when the
geometric distribution is selected.
Bezier curve
FIGURE 3.57
Relation between the number of parameters and the degree of the corresponding Bezier curve
Leading and trailing edges can be either rounded or blunt. According to these choices, the number
of control points used by the curve can differ from the amount of parameters specified in the
interface. The examples in FIGURE 3.57 assume a Bezier curve with 4 parameters:
l In the blunt case, a single control point is used at the edge, so that the number of user
specified parameters equals the number of control points.
l In the rounded case, three control points are needed at the edge to maintain both prescribed
radius and perpendicularity to the abscissa axis.
A general formula for the number of control point n can be presented in the form
n = 2 x number of rounded edges + number of user parameters
The parameters menu keeps trace of the parameters names as HALF_THICKNESS_P(j) variables
except when a rounded edge is involved, where the notation LE_RADIUS and TE_RADIUS are
used.
Rounded edge construction
The method applied for the rounded edge radius computation uses the equation below where a is
the first control segment length and b is the distance between the third control point and the first
control segment. In the present case, this expression is simplified thanks to the assumption that a
equals the prescribed radius value (FIGURE 3.58). Parameter b is then the only unknown in the
equation and can be easily computed. The height of the third control point is fixed by convention
to the same radius value and, although it controls the curve locally, has no influence on the
curvature radius at the edge point.
becomes
when a=R
FIGURE 3.58
Rounded edge radius construction (leading edge case)
.
Parameter
Description
S(i)_HALF_THICKNESS_P(j)
half thickness parameter (j) for blade section (i)
Parameter
S(i)_RADIUS_LE
S(i)_RADIUS_TE
Description
prescribed curvature radius at leading edge for
section (i)
This value replaces S(i)_HALF_THICKNESS_
P0 in rounded case
prescribed curvature radius at trailing edge for
section (i)
This value replaces S(i)_HALF_THICKNESS_P
(n) in rounded case
When an independent thickness distribution is applied on the pressure side, parameter names
contain an additional string 'PS' and become S(i)_PS_HALF_THICKNESS_P(j), S(i)_PS_
RADIUS_LE and S(i)_PS_RADIUS_TE.
B-Spline curve with optional circular ends
A B-Spline curve does not offer the same properties in terms of continuity, and therefore it is
usually exclusively used in blunt cases. It is however possible to add an optional circular arc at
one or both ends and to make the corresponding edges rounded. Continuity is then ensured up to
the first derivative.
The relationship between amounts of parameters and nodes is straightforward when a blunt is
used at both ends. When a circle arc is added at one end, the end node of the B-Spline curve is
not controlled directly and the corresponding parameter HALF_THICKNESS_P(j) is replaced by
two parameters RADIUS and HALF_ WEDGE_ ANGLE . All four combinations of blunt and
rounded edges are shown in FIGURE 3.59 in the general case.
FIGURE 3.59
Rounded and blunt distributions based on a B-Spline curve
Besides those general cases, wedge angle parameters disappear when fewer parameters are set,
resulting in the following two distributions:
l Linear case, when only two parameters exist and whatever edge options are selected (the top
picture in FIGURE 3.60 shows the rounded edge case).
l Constant case, when a single parameter exist (the bottom picture in FIGURE 3.60 shows the
rounded edge case).
FIGURE 3.60
Linear and constant thickness cases
In those two special situations, the edge angle parameter is automatically constrained. Therefore,
there are no combinations of three and four parameters!
Parameter
Description
S(i)_HALF_THICKNESS_P(j)
half thickness parameter (j) for blade section (i)
S(i)_LE_RADIUS
S(i)_TE_RADIUS
S(i)_LE_HALF_WEDGE_ANGLE
prescribed curvature radius at leading edge for
section (i)
This value replaces S(i)_HALF_THICKNESS_
P0 in rounded case
prescribed curvature radius at trailing edge for
section (i)
This value replaces S(i)_HALF_THICKNESS_P
(n) in rounded case
leading edge half wedge angle when at least one of
the edges is rounded
This parameter does not exist in a constant or
linear thickness distribution or when both
edges are blunt
Parameter
Description
S(i)_TE_HALF_WEDGE_ANGLE
trailing edge half wedge angle when at least one of
the edges is rounded
This parameter does not exist in a constant or
linear thick ness distribution or when both
edges are blunt
When an independent thickness distribution is applied on the pressure side, parameter names
contain an additional string 'PS' and become S(i)_PS_HALF_THICKNESS_P(j), S(i)_PS_LE_
RADIUS, S(i)_PS_TE_RADIUS, S(i)_PS_LE_HALF_WEDGE_ANGLE and S(i)_PS_TE_
HALF_WEDGE_ANGLE.
Half wedge angles do not exist in a blunt- blunt configuration. Bessel end conditions are applied
instead.
Because of the need for the additional parameters for the half wedge angles some numbers of
parameters (3 and 4) are not allowed in the interface.
User-defined law
Three types of user-defined laws are available:
1) Data file
If the thickness law is available as an external data file, it can be imported as a user-defined law in
the parametric model. This law is then free of parameters and, once applied, can be edited in the
graphics area.
File format
As for user-defined endwalls, the distribution is defined in a simple text format, as illustrated in
the example below.
# comments
59 (amount of defining points)
0.0 0.0
0.01 0.125 ('s' abscissa and half-thickness value)
0.03 0.25
...
0.97 1.23
0.99 1.24
1.0 1.245
The first input number is the amount of provided points. Then, each line defines a single point by
means of the following coordinates:
l the first coordinate is the fraction of the camber curve length at which the thickness is
defined (real fractional length ranging from 0.0 to 1.0),
l the second coordinate is the prescribed half-thickness, that may be given as a fraction of the
camber length (NACA style) or a real measurement of the half-thickness.
A comment may be added anywhere provided that it starts the line with '#' character.
To provide easier input, two special keywords STARTING_ABSCISSA and ENDING_ABSCISSA
are allowed either at start or end of the file to transform starting and ending values for the abscissa
of the distribution. For instance, the two instructions below tell AutoBlade™ that the abscissa
50.0 should be considered as 0.0 and abscissa 100.0 as 1.0. A linear transformation is defined by
these two parameters and applied to all provided abscissa values.
starting_abscissa 50.0
ending_abscissa 100.0
Once read, the thickness file is stored in the parametric model and the file may be deleted. This
allows to manage the model as a whole.
All provided points generate a spline law for smooth interpolation of half-thickness values,
especially near ends.
File options and input
Two selectors allow to define a distribution for each side (if asymmetric) and primary section. The
following controls allow to tune the selected distribution (FIGURE 3.61):
1. The option Include points as parameters allows to include all reference points as regular
parameters for the fitting or the optimization. This means that the law can be initialized and
even altered by the fitting process!
2. The option Number of nodes is used to specify the number of the points in the inputted file. If
the number of the defining points has been defined in the inputted file, the option Number of
nodes will be neglected.
3. The option Dimensional abscissa specifies either if the abscissa must be considered as the
values read (checked) or if the provided abscissa must be scaled by the length of the camber
curve (unchecked).
4. The option Dimensional height specifies either if the half-thickness must be considered as the
values read (checked) or if the provided law must be scaled by the length of the camber curve
(unchecked). Default is dimensionless thickness (unchecked state) that corresponds to the
NACA style definition.
5. The option Abscissa factor allows to scale the abscissa by means of the optional floating point
value (on the right side).
6. The option Height factor allows to scale the ordinate of the prescribed half-thickness by
means of the optional floating point value (on the right side). This option is useful to define a
scaled thickness from hub to shroud, while reusing the same thickness file, or to adapt a
reference law.
FIGURE 3.61
User-defined thickness law and options
The user-defined thickness can be only inputted by Right-clicking in the SIDES view, as shown
in FIGURE 3.43.
FIGURE 3.62
Input use-defined thickness
In the Init curve from file dialog, the user can enter the path ended by a hit on the <Enter> key or
click the button on the right and use a classic file chooser. By default, no file is active and the
value in the field is none. Once selected, the file is parsed and checked: if the color of the field is
changed to red, this means that the file does not comply with the format specification described
above!
When no valid thickness file is selected, a default thickness law is applied when Ok is clicked.
If the camber curve is modified, the final thickness is also changed when it is defined in NACA style
(unchecked Dimensional height). User-defined thickness is not constant in that case and this
must be pointed out for optimization projects!
Optional rounding
When the thickness is not defined at edges or if the edge is assumed blunt, the resulting section
will be treated as a blunt. It is possible to define a rounded edge from the thickness file; but this is
not advised because the quality of the edge shape highly depends on the amount of defining
points.
In rounded cases, AutoBlade™ provides additional options under the areas Leading edge and
Trailing edge. These boxes do not appear until the thickness file is selected, because the default
values of these fields are set according to the content of the thickness file.
1. The default option leaves the thickness law unchanged (FROM_FILE option)
2. Automatic elliptical rounding (ELLIPTICAL option) defines an elliptic arc to close the edge
and ensures C 1 continuity with the prescribed law (continuity of the tangent). This is the
preferred option for the leading edge, but this method does not provide control of the starting
curvature radius (FIGURE 3.63).
3. The circular rounding (deprecated CIRCULAR option) allows to define a circular edge
linked to the prescribed law by a linear segment starting from a relative location (round at
field) on the abscissa axis. This method is convenient for the trailing edge, with a precise
curvature radius, but C1 continuity is not provided (FIGURE 3.64).
4. The circular rounding with tangency (CIRCULAR_TGT option) tries to find a location
where the linear segment can be connected to the prescribed law with a marginal error on the
continuity of the tangency (FIGURE 3.65). This option is preferred to the previous one and
behaves the same way when no suitable location can be found, thanks to the relative location
value in round at field.
FIGURE 3.63
Automatic elliptical rounding at prescribed 's' location
FIGURE 3.64
Circular rounding with linear segment at prescribed 's' location
FIGURE 3.65
Circular rounding with linear segment and C1 continuity
The existence of a solution for the CIRCULAR_TGT option highly depends on the external law
and the prescribed radius. The search ranges in s relative location are [0,0.5] for the leading edge
and [0.5,1] for the trailing edge: if no location that satisfies the C1 continuity can be found, an
error is generated and the CIRCULAR rounding is applied.
2) Expression
The thickness can be defined by a mathematical expression involving a single parameter 's' for
each blade, each section and each side. In order to simplify the user input, this expression can use
an existing function with an arbitrary amount of arguments. The thickness is evaluated after all
parametric dependencies are solved and evaluated. Therefore, the value of all existing parameters
is already available as input.
For the thickness law, a variable must be reserved for the reduced abscissa and is assumed to be 's'
by default. All other symbols must be constants, existing parameters or other functions.
FIGURE 3.66
User-defined expression
It is allowed that the expression does not contain the abscissa 's'. In this case, the expression is a
constant.
3) NACA45
A built-in definition for NACA thickness laws (NACA 4 and 5 digits) has been introduced as a
user-defined thickness, since this law is common to the original NACA 4 and 5 digits and often
used in blade definitions.
The reduced thickness for NACA 4 and 5 digits is given by:
where tmax is the maximum relative thickness (in percent) and x is the reduced abscissa variables
(defined over [0,1]).
FIGURE 3.67
User-defined NACA45
NACA is a blunt thickness, so one of the existing rounding options should be used to round the
distribution at the training edge.
There is no difference between NACA 4 and 5 digits for the thickness definition.
4) Parameters
If the user selects the user-defined laws, some parameters are added in the Parameter list menu
when
l an optional height factor is selected,
l an optional rounding option is applied.
Those parameters are especially useful for fitting purposes.
Parameter
Description
S(i)_HEIGHT_FACTOR
optional height factor in user-defined thickness law for blade section
(i)
Parameter
Description
S(i)_LE_RADIUS
prescribed curvature radius at leading edge for section (i)
This parameter only applies when the special rounding option
CIRCULAR or CIRCULAR_TGT is selected at the leading
edge
S(i)_TE_RADIUS
prescribed curvature radius at trailing edge for section (i)
This parameter only applies when the special rounding option
CIRCULAR or CIRCULAR_TGT is selected at the trailing
edge
S(i)_LE_START
starting s abscissa of optional rounding at leading edge for section (i)
This parameter applies when a rounding option is selected and
effectively used with CIRCULAR and CIRCULAR_TGT
options
S(i)_TE_START
starting s abscissa of optional rounding at trailing edge for section (i)
This parameter applies when a rounding option is selected and
effectively used with CIRCULAR and CIRCULAR_TGT
options
When an independent thickness distribution is applied on the pressure side, parameter names
contain an additional string 'PS'
Since the CIRCULAR_TGT rounding option is very sensitive to the distribution of the tangent in the
spline law, the graphical edition of the control points in the thickness view can lead to a flickering
effect.
D. Leading & Trailing Edges
This menu collects optional settings for leading and trailing edges that are available for the
selected construction modes. Please consult the Suction & Pressure Side Curves section for
explanations on how requested edges are constructed.
FIGURE 3.68
Leading & trailing edges options menu
For both edges, up to three edge types are available:
l Rounded: this is the default selection.
l Blunt:
l Regular: edges are cut perpendicularly to the camber curve in the chosen construction
plane.
l Constant dmr: edges are cut at camber edge point
value, whatever the construction
plane.
l Constant theta: edges are cut at camber edge point θ value, whatever the construction
plane.
In independent suction and pressure sides mode, leading edge is always rounded, but a blunt
trailing edge is possible. In that case, no ending circle arc is built.
If a user-defined thickness law is applied, the edges are explicitly defined by the law or the
specific rounding options. This menu is therefore not applicable in that case!
l Elliptical:
l The internal rounding allows to close the leading/trailing edge with an elliptical arc that is
passing through the starting/ending point of the camber curve.
l The external rounding allows to close the leading/trailing edge with an elliptical arc that
has its center at the starting/ending point of the camber curve.
l The cutback rounding allows to close the leading/trailing edge with an elliptical arc that is
tangent to the meridional location of the starting/ending point of the camber curve.
Elliptical rounding and edge position choices present the following limitations:
l Supports symmetric thickness addition only.
l Discretized sections are not well supported. Interpolation can possibly generate bad profiles.
l External and cutback positions are not available for splitter blades.
l Currently no support in the fitting module (mainly because the rounding is not built in the
parametric curve).
l Not available when the Center of Gravity selected as stacking point.
3.1.5
Optional Splitters
Splitters are added to the main blade to guide the flow when the channel becomes wider, in radial
turbomachinery. In AutoBlade™, splitters are compatible with both construction modes and all
camber construction planes. Up to ten splitters can be added.
As a workaround, the splitter model can be used to model the tandem row configuration.
Splitters are built using the main blade camber curve with an optional refinement and their
locations are relative to the main blade position and defined by means of few simple non
dimensional parameters.
Suction and pressure sides are built according to the same method as the main blade: camber
curve type, construction mode and edge types are all inherited form the main blade selections.
Nevertheless, the number and values of the parameters are specific. In camber and thickness mode
the thickness distribution is optionally asymmetric.
The Splitter blades menu consists in three pages:
l the General properties page controls the number of additional blades (FIGURE 3.69),
l the Camber curve page allows to alter the camber curve,
l the Sides definition page defines the number of parameters controlling the suction and
pressure side curves or thickness law
FIGURE 3.69
Splitter blades menu
Some topological choices may prevent the use of splitters, for example the stacking points in the
centre of gravity.
Quick Method: Inherited Camber Curve
The simplest way to define splitters is to reuse the same blade camber line by selecting "None" in
the Camber Curve section: the camber line of the main blade is simply rotated and truncated
with respect to parameters MLE and MTE. Those two parameters are non dimensional factors
used to limit the main camber extend in the meridional plane for splitter blades (FIGURE 3.70).
MLE parameter value represents a fraction of the main blade camber measured along the abscissa
construction axis and starting from the main blade leading edge point. The value 0.0 corresponds
to the main blade leading edge location, the value 1.0 to the main blade trailing edge location. The
splitter leading edge location along the abscissa axis is obtained by formula below, where XLE
(splitter) is the edge coordinate of the splitter blade along the abscissa construction axis and XLE
and XTE are the edge locations of the main blade along the same axis.
One can establish a similar relation for the trailing edge location of the splitter thanks to parameter
MTE. A zero value imposes that the m-coordinate of the splitter trailing edge point equals the one
of the main blade trailing edge.
Once the splitter camber is defined, suction and pressure sides are constructed by means of the
same method as for the main blade.
FIGURE 3.70
Splitter leading and trailing edges locations
AutoBlade™ accepts values in the range [-3,4] for MLE and MTE parameters. Outside regular bounds
0.0 and 1.0, the main camber curve is extrapolated linearly to allow the splitter blade to include
upstream and downstream extensions.
If the criterion ( MLE + MTE > 0.99) is reached, the value of MTE will be reset to 0.99- MLE
automatically.
Camber Curve Refinement
It is also possible to perturb the initial camber curve portion defined above by a refinement curve.
This perturbation is enabled by selecting the Camber Curve Refinement option.
FIGURE 3.71 shows the refinement process: first, the main camber curve is processed in its
construction plane. A refinement Bezier curve is then generated with the help of by default
equally spaced height parameters CAMBER_H(j) between the splitter limits defined by MLE and
MTE parameters. The stretching factor allows the user to adapt this last space, it can evolve from
1 for uniform intervals to a factor bigger/lower than 1 that will result in increasing/decreasing
intervals from leading MLE to trailing edge MTE . Finally, the ordinate values of both main
camber and refinement curves are summed and the resulting camber is ready for side curves
construction.
The refinement curve always uses dimensional heights.
FIGURE 3.71
Splitter camber curve refinement
Resizing & Moving Splitter Limits
Changing parameters MLE and MTE allows the splitter blade camber to be moved and resized in
the meridional direction, as explained in the previous section Quick Method: Inherited Camber
Curve.
An additional parameter DELTA_ THETA controls the blade tangential location if the splitter
blade needs to be moved away from its default central location, corresponding to the value of
zero. The following expression is the formula computed by AutoBlade™ to rotate the splitter
blades from initial the main blade camber line, where j stands for the splitter index, ABT for the
number of blade types and NB for the amount of angular repetitions.
In single splitter case, when DELTA_THETA is given -1.0 value, the splitter blade camber is not
,
rotated at all and when this value is changed to +1.0, splitter camber is rotated of a quantity
which is the spacing between the main blades. Therefore valid values are near zero, somewhere in
the interval [-1.0,1.0].
Splitter location and extend are thus relative to the main camber curve and fully expressed through
the use of three non dimensional parameters MLE, MTE and DELTA_THETA. It is important to
notice that the stacking point defined for the main blade does not influence the splitters location.
The following figure shows a typical radial compressor with a single splitter blade (upper left).
The next two pictures show the influence of parameter DELTA_THETA (upper right and lower
left) while the latest shows how splitter blades extend can be modified with parameters MLE and
MTE (lower right).
FIGURE 3.72
Example of compressor with splitter blade (upper left) and some effects in parameters changes
Summary table
TABLE 3.9 contains a list of all splitter parameters. Some of them are construction mode specific
and may not be available in other construction modes.
TABLE 3.9 Parameters for splitter blades
Parameter
Description
S(i)_SPLIT(k)_MLE
S(i)_SPLIT(k)_MTE
leading edge fractional location parameter for splitter (k) on section (i). -
0.5 < MLE < 1.5
trailing edge fractional location parameter for splitter (k) on section (i). -
0.5 < MTE < 1.5
S(i)_SPLIT(k)_DELTA_
THETA
rotation parameter for section (i) of splitter (k). Centred leading edge
position is ensured by a zero value.
S(i)_SPLIT(k)_CAMBER_H
(j)
optional refined camber height (j) for splitter (k) on section (i).
S(i)_SPLIT(k)_HALF_
THICKNESS_P(j)
half thickness value (j) for splitter (k) on section (i) - camber & thickness
mode only
S(i)_SPLIT(k)_TSS(j)
S(i)_SPLIT(k)_TPS(j)
suction and pressure side offsets (j) for splitter (k) on section (i) -
suction & pressure sides mode only
S(i)_SPLIT(k)_RADIUS_LE prescribed curvature radius at leading edge for section (i) of splitter (k) -
rounded case
S(i)_SPLIT(k)_RADIUS_TE prescribed curvature radius at trailing edge for section (i) of splitter (k) -
rounded case
S(i)_SPLIT(k)_TE_
WEDGE_ANGLE
prescribed wedge angle at trailing edge for section (i) of splitter (k) -
suction & pressure sides mode only
Additional parameters for side curves with end line - applies for SS and PS
S(i)_SPLIT(k)_SS_LE_
WEDGE_ANGLE
prescribed wedge angle δle for suction side curve, on section (i) of
splitter (k) (in degrees)
S(i)_SPLIT(k)_SS_REAR_
SHAPE
prescribed fractional offset
splitter (k)
S(i)_SPLIT(k)_SS_END_
LINE
prescribed fractional length
on section (i) of splitter (k)
for suction side curve, on section (i) of
of the ending line for suction side curve,
3.1.6
Technological Effects
FIGURE 3.73
Technological effects menu
This menu grants access to a set of technological effects that are applied on the final blade shape.
The five available features - Hub and shroud gaps, edge rounding, trailing edge filing, blade
cutoff and section recut - are applied at the end of the design process, after the construction of
the blade sides and edges.
Hub and shroud gaps
This operation allows the user to define a hub and/or shroud gaps, which can be exported to
AutoGrid5™ for mesh generation, or exported as a curve. The gap can be defined for the main
blade and the splitter independently. After defining the gap, the gap curve appears in the
MERIDIONAL view.
The gap curves cannot be exported when exporting the geometry as rulings (the menu Export
rulings ).
Three gap types are provided:
l None: No gap is defined (default)
l Constant: A simple gap is defined with a constant width from the leading edge to the trailing
edge. In this case, a single constant width needs to be defined.
l Linear: A gap is defined from two width values at leading and trailing edge points. The gap is
changing in a linear way in the streamwise direction. In this case, two width parameters at the
leading edge and the trailing edge need to be defined.
The button Reset is used to set the gap value to a suitable default value corresponding to 5
percent height of the average edge length (mean value of LE and TE edge lengths).
The Curve extension is used to control the extension of the gap curve before the leading edge
location and after the trailing edge location. This factor can be set to any value in range [0.0,0.5],
(default value 0.1). It is not advised to set extension to zero if the gap curve itself is exported as a
curve. Please note that extensions also follow the offset law.
The gap curve is build from the channel curve as an offset curve with linear or constant value. In case
of linear offset, the two values are imposed from the intersection points between the channel curve
and the leading / trailing edge curves. This may lead an invalid gap curve if the local radius of
curvature of the channel curve is lower than the offset value.
The gap width parameters are non-negative and have a unique naming following the simple rule
below, where [] is optional fields and {} mentions special strings listed in the next table.
[SPLIT{INDEX}]{ENDWALL}_[{POSITION}]_GAP_WIDTH
Special fields
INDEX
ENDWALL
POSITION
index of the splitter blade, starting from 1
HUB or SHROUD
LE or TE
For example, the constant tip gap width parameter on the main blade is named 'SHROUD_GAP_
WIDTH'. The tip gap width at leading edge of the splitter blade is named 'SPLIT1_SHROUD_
LE_GAP_WIDTH'.
Edge Rounding
After applying the edge rounding, the ruled blade surface will be not ruled anymore.
This operation allows to apply internal, external and cutback rounding with elliptical arc, based on
a prescribed ratio b/a.
FIGURE 3.74
Edge rounding options
l The internal roundingallows to close the leading/trailing edge with an elliptical arc that is
passing through the starting/ending point of the camber curve.
l The external rounding allows to close the leading/trailing edge with an elliptical arc that has
its center at the starting/ending point of the camber curve.
l The cutback rounding allows to close the leading/trailing edge with an elliptical arc that is
tangent to the meridional location of the starting/ending point of the camber curve.
The edge rounding is restricted for use with (m,β) or (
,θ) construction plane, flank-milled
blades, symmetrical thickness addition mode and presence of blunt both at leading/trailing edge.
Trailing Edge Filing
Practically, this operation is achieved with simple tools directly on the manufactured blade and
consists in material removal on one of the sides near the trailing edge.
Two lengths are needed on each blade section for that purpose and the designer may select either
suction or pressure side or both . To simplify user input, length and thickness
distributions are built from one, two or more values of the span parameter.
FIGURE 3.75
Edge filing length and thickness (suction & pressure sides)
In the simplest case, if Number of parameters is 1, constant length and thickness are applied on
all blade sections, so only two parameters FILING_LENGTH_SPAN_0 and FILING_THICK_
SPAN_0 need user input. If Number of parameters is 2, length and thickness are required at
spanwise locations 0.0 and 1.0. and blade sections values are interpolated or extrapolated linearly
from those reference values. If three or more parameters are set up, a spline interpolation is
applied and spanwise reference values are free.
Parameter
Description
FILING_LENGTH_SPAN_(i)
Trailing edge filing reference length at i percent of the span
FILING_THICK_SPAN_(i)
Trailing edge filing reference thickness at i percent of the span
When deactivating Straight filing option, the removal of material is applied in a direction normal
to the camber curve in (m',θ) plane. The removed thickness is linearly interpolated between "t" for
trailing edge and 0 at location "s" along the side curve (FIGURE 3.76).
FIGURE 3.76
Straight filing option
When imposing edge filing on both sides of the blade , the removed thickness
can be symmetric or not. In the latter option ( both_ asymmetric ), the non- axisymmetry is
controlled by a new parameter FILING_SS_FRACTION_SPAN_(i) defined in the range [0,1].
Edge filing does not apply to rounded edges.
Please note that filing length and thickness parameters are measured in Cartesian coordinates X,Y and
Z and not in the blade section construction plane.
Blade Cutoff
This option comes from the need for manufacturers to use the same blade design for multiple
pumps or compressors. To some extend, design and manufacturing costs can be reduced if an
entire family of low- to mid-range turbomachines share the same blades. For instance, blade
design is carried out for the most powerful machine of a pump family. Other designs are
dimensionally identical except that blades are shorter. This can be achieved simply by cutting the
blades near the trailing edge, reducing the head of the pump. Companies have to manufacture a
one-size component for the whole family, eventually leading to a reduction of the costs.
FIGURE 3.77
Example of radial cutoff: blades are cut to achieve a whole family of compressors sharing the
same design and dimensions
The blade cutoff option has been developed to be applied at leading or trailing edge in radial and
axial cases. This operation preserves the axi-symmetric characteristic of the machinery and is
therefore applied in (Z,R) plane.
Spline Cutoff (flank-milled blades)
When working with flank-milled blades, the cutoff can be performed using a meridional spline
curve.
1. The recut is applied to the camber, not the side curves. This means that a 'normal' blunt can be
obtained while the linear cutoff produces a tangential blunt.
2. The recut can be applied with optional extension of the camber curve. This allows the success
of the operation on the whole edge even in case of limited recut and avoid discontinuities in
the recut area. If late rounding is applied to a discontinuous edge, the model will not be
considered as valid.
3. If, in case of inexistent or insufficient extension in cutoff operation, no intersection is found
with one of the camber curves, the model is considered as invalid.
4. The spline is defined by 2D nodes in a full parametric way. All related parameters are accessed
in the Others tab of the Parameters list.
Parameter
LE_CUTOFF_Z(i)
TE_CUTOFF_Z(i)
LE_CUTOFF_R(i)
TE_CUTOFF_R(i)
Description
Axial location of the node i
Radial location of the node i
After applying the cutoff, the user can manually edit the parameters in the Parameters list, or
directly edit the spline in the Meridional view. Right-clicking on the Meridonal view and
selecting Edit main blade LE/TE cutoff curve will activate the edit mode. The control points of
the selected spline will be shown in green points. Each control point can be moved by left-
clicking on it. Right-clicking will quit the edit mode.
This operation makes sense on turbomachines with blunt edges. Complete design can be achieved in
AutoBlade™ before enabling the cutoff as the very last operation.
If both edge filing and cutoff are applied, filing is applied first.
Section Recut
The effect allows to re-cut the blade sections. One or more spanwise locations are defined for
reference and, for each location, a cutting distance is defined in the parametric form.
For instance, when a cutting distance is defined between the hub and the shroud (span locations 0
and 1), this distance is linearly interpolated or extrapolated for any intermediate location. When
more locations are defined for reference, the interpolation uses a spline and is constant in the
special case of a single reference location.
FIGURE 3.78
Sectional cut-off of the blade
All primary and parametric sections are built in the usual way. If discretized sections are required,
they are processed before the treatment. Then, all sections are cut at the prescribed 3D distance
from the trailing edge using the interpolated value from parameters TE_CUT_LENGTH_SPAN_0
and TE_CUT_LENGTH_SPAN_100 at the prescribed spanwise value.
A switch controls the way this length is input, either as a fraction of the 3D camber or as an
absolute length. In case of fraction, the name CUT_LENGTH is replaced by CUT_S.
When a cut value is null or negative, the section is left untouched and no warning or error is
generated (the model is assumed valid).
3.1.7
Non-Axisymmetric Hub/Shroud
The following descriptions assume the definition of the hub surface, but all topics are directly
applicable to shroud surface as well.
A. Space of Definition
The domain of definition is an area built in (m',θ) plane. First, the mean line of the main blade at
hub section is computed (upper dotted black curve on FIGURE 3.79). This line is the first side
limit of the domain inside the blade channel, the second side limit being defined by its vertical
translation of value Δθ = -2*PI / NB.
FIGURE 3.79
Space of definition
The extent of the domain is always limited at inlet and outlet and by the mean line of the main
blade and its translated repetition. The inlet and outlet parts (Inlet/Outlet extension in FIGURE
3.87) are built from either a line segment tangent to the mean line of the blade at the edge point or
a smooth Bezier curve ending horizontally at the other end (red curves). Aside this construction
choice, the extensions are fully automatic. This definition has a clear advantage: the perturbation
may occur over a space covering the whole hub surface once repeated, since a 2*PI extent is
travelled in θ direction.
For the definition of the non axisymmetric hub, the preferred configuration is interpolated stream
surfaces with the first primary section at span location 0. Other stream surfaces are allowed, but may
cause discontinuities if the perturbed surface ends outside the blade section. The reference hub mean
line is always built for span 0, by interpolation if it is not defined in the list of primary sections.
B. Method 'across channel'
If the internal limits of the extensions are the start and end of the blade channel, the domain is
defined by three areas where the middle part is always located in the blade passage. Those limits
are approximate segments stretched between the mean lines and entering into the blade sections.
The first method builds cuts in the blade channel area only . The start and end
cuts are located by the designer and become the links between the inlet, outlet and perturbed
channel areas. Additional cuts can be defined in arbitrary amount between those two limits.
FIGURE 3.80
Cuts are defined across the blade channel
By default, the cuts are perpendicular to the channel line. But a special angular deviation can be
applied for each cut as an additional parameter. All angular deviations are measured in degree
from the normal direction along the mean channel line. In case of intersection between cuts, the
generation of the patch will fail, and AutoBlade™ will issue a message.
FIGURE 3.81
Cuts are defined across the blade channel
Parameter
Description
HUB_CUT(i)_ANG_DEV
Angular deviations of the cut i in the 'cut across' method.
HUB_START_ANG_DEV
HUB_END_ANG_DEV
Internal Cuts
For every internal cut, a perturbation law is defined by mean of a Bezier curve or a cubic spline
controlled by height parameters. This law is then defined in (S,h) plane where S stands for the
natural parameter of the cut in (m',θ) plane and h is the dimensional height of the perturbation
(FIGURE 3.82).
FIGURE 3.82
Perturbation law for 'across' method
No continuity constraint is necessary as long as the resulting endwall completely intersects the
blade because the discontinuity has no effect on the mesh generated from a geomTurbo output.
The number of parameters is free and an optional stretching factor allows to concentrate more
control points near one end.
Start & End Cuts
The first and last cuts can be freely placed in the blade channel, but are parameterless in order to
reach at least C0 continuity.
Final Surface
The final perturbed patch is a loft surface passing through the perturbed cuts (loft profiles) and
two guide curves defined by splines from start to end cuts. The loft profiles are generated from the
cuts on the revolved hub by addition of the perturbation heights defined earlier.
FIGURE 3.83
The complete perturbed surface for 'across' method
The perturbations are applied in the normal direction to the revolved hub (radial direction for a
cylindrical reference hub).
G1 continuity can be enforced with inlet and outlet patches by means of clamped ends conditions
on spline guides. Therefore, this continuity is only strictly ensured at ends of the start and end
cuts.
Parameter
Description
HUB_CUT(i)_H(j)
Height value of control point j of the cut i, as a 3D distance
SHROUD_CUT(i)_H(j)
C. Method 'along channel'
The method described above is generally not suitable for turbines because the perturbed surface is
then generated from profiles far from parallel and too high perturbations appear near the suction
side of the main blade (FIGURE 3.80).
To allow non-axisymmetric endwalls in case of turbines, an alternate method consists in building
the cuts along virtual stream lines created as shown in FIGURE 3.84. The cuts may extend
outside the blade channel, but then the start and end cuts must be identical to ensure C0
continuity. G1 continuity can be enforced by mean of special boundary conditions in the
generation of the loft patch.
FIGURE 3.84
Cuts are defined along the blade channel
If the perturbation is limited to the blade channel, the start and end cuts may be independent,
enabling free boundaries (Limit perturbed surface to blade channel option in FIGURE 3.87).
The guide curves are defined as circle arcs at constant value of m and C0 continuity is
automatically ensured if the start and end heights of each perturbation are managed by the
algorithm (FIGURE 3.85). G1 continuity is optional. In the case of Bezier curves, G1 continuity
will freeze two additional heights (h1 and h5).
FIGURE 3.85
Perturbation law for 'along' method
In 'cut along' method, cuts defined with a spline law only accept identical boundary conditions for
start and end. This limitation does not apply to Bezier laws.
This new construction is especially suitable for axial turbines and fans, but not for centrifugal
compressors or impellers where the first method provides far better results. An example of the 3D
construction of loft profiles and guide curves is depicted in FIGURE 3.86.
FIGURE 3.86
The complete perturbed surface for 'along' method
D.
Inlet & Outlet Offsets
Inlet and outlet extensions can be built with an optional signed offset (above or below the
revolved hub). Offsets are controlled by two additional parameters and may be applied even if no
parameters exist in the perturbed area, whatever the chosen method.
Parameter
Description
HUB_INLET_OFFSET
SHROUD_INLET_
OFFSET
Offset value from hub/shroud revolved surface for construction of the inlet
patch, as a 3D distance
HUB_OUTLET_
OFFSET
Offset value from hub/shroud revolved surface for construction of the outlet
patch, as a 3D distance
SHROUD_OUTLET_
OFFSET
E. Graphical and Exported Outputs
The construction of the surfaces is treated in Parasolid™ format.
Export of the non-axisymmetric surfaces is allowed in both geomTurbo 5.3 and IGES formats.
The non-axisymmetric surfaces can be activated in the 3D view, but are not shown as default.
Their display is either limited to a single blade occurrence or repeated just like blades.
F. Settings Dialog
When activating Define non-axisymmetric hub/shroud surface in the corresponding pages, a
list of new entries are provided to the user to control the settings.
FIGURE 3.87
Non-axisymmetric hub/shroud settings
The positive direction corresponds by default to the left side of the hub or shroud curve
direction.
The repetition option by default, set to 1, duplicates one time the non-axisymmetric patches in
both θ directions. This option is useful for the exportation to AutoGrid™.
In both 'cut across' and 'cut along' methods, a check button Imprint cuts on surface can be
activated to enforce cuts as internal edges on the non axisymmetrical patch in the Parasolid model
The option Imprint cuts on surface is responsible for a higher amount of faces and may
significantly slow down the build and analysis of the non axisymmetrical surfaces. Therefore, it is
advised to disable this option in an optimization.
The angular tolerance allows to avoid any gap between repeated patches in ".geomTurbo" file.
3.1.8
Solid Body
The solid body module allows the user to create one or multiple solid geometries in AutoBlade™,
and thus allows the user to perform multidisciplinary optimization in FINE™/Design3D. The
solid body is defined as one or more axisymmetrically defined bodies merged and optionally
blended with the AutoBlade™ solid blade geometry.
The solid body module can be activated by selecting the selection box Activate solid body
modeling. Then the interface defining the solid body can be accessed. The window configuring
solid geometries contains two tabs, one for the definition of the axisymmetric geometry with
composite curves in the Meridional view (Axisymmetric geometry definition), and one for other
advanced settings (Advanced settings).
Define solid body
The left panel of the tab Axisymmetric geometry definition contains a list of the solid bodies in
the model. The name of each solid body may be changed by double-clicking on the entry in the
list. The button Delete selected solid body allows to remove the selected solid body from the list.
The button Sketch new solid body opens a tool allowing the user to sketch a new solid body
profile in the Meridional view. The right panel contains a list of the composite curve elements for
each solid body. For the existing composite curve elements, the curve type and the number of
control points may be modified. The existing elements may also be deleted and new elements may
be inserted in the composite curve.
FIGURE 3.88
Axisymmetric geometry definition
To add a new solid body, click on the button Sketch new solid body. Then, the meridional view
will be switched to interactive edit mode, as shown in FIGURE 3.89 . Left-clicking in the
meridional view will add a new control point. Right-clicking in the meridional view will draw a
line or bspline by using the new control points, depending on the number of the new control
points. If no new control points are added, right-clicking will exit the edit mode (or use the key
<q>). After exiting the edit mode, the new body will be added in the solid body list. A valid solid
body will be displayed as a shaded region.
For an existing solid body, if the user selects the definition profile of the solid body in the
meridional view, the control points will be highlighted and may be interactively moved. Once
moved, the underlying R and Z parameters are automatically updated.
FIGURE 3.89
Interactive edit mode in the Meridional view
Each axisymmetric solid body is defined by a single composite curve in the RZ frame and the
corresponding hub/shroud curve. The single composite curve in the RZ frame should intersect its
associated endwall curve exactly twice, and must not be self-intersecting. FIGURE 3.90 shows
the examples with correct solid body definition (A) and wrong solid body definition (B/C/D).
FIGURE 3.90
Centrifugal compressor solid body setup (A - Valid geometry, B/C/D - Invalid geometry)
The merging of the blade and hub/shroud solid bodies requires a clean intersection of the bodies. The
spanwise locations of the blade sections may influence the success of the merge, particularly if
sections are spaced such that [ 0 < spanwise location < 1 ].
The parameters defining the control points are as follows:
Parameter
Description
#_SOLID_R(i)
defines the R coordinate of the ith control point in the solid body named as #
#_SOLID_Z(i)
defines the Z coordinate of the ith control point in the solid body named as #
Advanced settings
The tab Advanced settings contains options related to the setup of the blend parameters and
expert setting used to tune the periodic sector symmetry creation.
FIGURE 3.91
Advanced settings of the solid body
By default, the blend function is disabled. The user may activate this function by selecting the
selection box Activate blend parameters. Then a blend will be created between the blade and the
solid body. AutoBlade™ supports both constant radius and constant width blending. If the option
Extend blend to blunt faces is selected, the blend will be extended to the blunt faces at
leading/trailing edge of the blade.
The parameters defining the blend are as follows:
Parameter
Description
MAIN_HUB_BLEND_RADIUS
or
MAIN_SHROUD_BLEND_
RADIUS
SPLIT(i)_HUB_BLEND_RADIUS
or
SPLIT(i)_SHROUD_BLEND_
RADIUS
MAIN_HUB_BLEND_WIDTH
or
MAIN_SHROUD_BLEND_WIDTH
SPLIT(i)_HUB_BLEND_WIDTH
or
SPLIT(i)_SHROUD_BLEND_
WIDTH
defines the blend radius of the main blade for constant radius
blend
defines the blend radius of the ith splitter blade for constant radius
blend
defines the blend radius of the main blade for constant width
blend
defines the blend radius of the ith splitter blade for constant width
blend
To minimize the size of the solid geometry and the structural analysis mesh, it is prudent to
represent the solid geometry as a sector model. A sheet body is used to extract the sector geometry
from the 360 degree spun bodies. A separate set of cut sheets is generated for each solid body,
with the meanline curves of the main and splitter blades at the associated endwall used as a guide.
The cut sheet is generated by projecting a series of wire bodies from R=0 through a reference
curve to the maximum radius of the solid body. The reference curve passes through the meanline
curves of the main and splitter blades, with additional segments to facilitate the transition between
the main and splitter blades. Additional wires are created at axial locations upstream and
downstream of the solid body. A sheet body is lofted through this array of wires, yielding a series
of sheet bodies. The sheet is then duplicated and rotated by one full passage angle.
The solid sector geometry can be exported.
For most axial and radial configurations the method above works well. With some radial
configurations lofting the cut sheet through the full extent of the reference curve has been shown
to create undesirable or invalid geometry. In this case, the following settings can be used:
l Reference curve range: specifies the range of the reference curve to be used when lofting the
cut sheets.
l Sector positioning, main blade: modifies the tangential positioning of the main blade segment
of the reference curve.
l Sector positioning, splitter blade: modifies the tangential positioning of the splitter blade
segment of the reference curve.
l Transition factor: modifies the segments between the splitter and main blades.
The surfaces of the merged solid geometry are named as follows:
l The solid body surfaces inherit their names from the RZ profile used to define the geometry,
along with suffixes specifying additional information:
<Solid_body_name> + "_" + <segment_name>
<Solid_body_name> + "_Endwall"
<Solid_body_name> + "_Periodic_" + <face_number> + "_side1"/"_side2"
For example:
Test_Endwall
Test_Curve_1
Test_Periodic_2_Side2
l Surfaces originating from the blade bodies inherit their names from the preexisting blade body
names. For example:
"MAIN_PRESSURE_F1"
"MAIN_SUCTION_F1"
"SPLIT1_PRESSURE_F1"
l Surfaces resulting from the blend operations are built to indicate the associated blade and
endwall. For example:
"MAIN_HUB_Blend_0"
"MAIN_HUB_Blend_1"
"SPLIT1_SHROUD_Blend_0"
3.1.9
Topological Compatibility Issues
Selecting a planar radial stream surface prevents some stacking point options and the center of
gravity stacking point does not allow the use of splitter blades. These are some examples of the
compatibility restrictions in the definition of the topology. Since the topology dialogs act as
ordered steps in the design process, the stream surface choice affects settings for meridional and
tangential location, but also the construction plane for the camber curve and all subsequent
choices.
It is not easy to understand all restrictions about the topological settings, especially for a new user.
The goal of this section is to help selecting the right settings for your project. In addition,
importing a template close to your final design could minimize the time required to achieve the
project.
TABLE 3.10, "Compatibility table for topological settings" suggests a summary of the compatibility
for the main topological choices.
Axial Pumps, Compressors & Turbines
The default model or the two first templates are a good starting point for an axial project. The first
template is a compressor model, the second one a turbine model.
The Wind Turbines are treated in the next section.
Stream Surfaces
Usual construction planes for the camber curve are (Z,Y) and (m,R*θ) planes. In the first case,
planar axial stream surfaces are mandatory and in the second case,
the best choice is
cylindrical stream surfaces . If the machine is not strictly axial, conical or hub to shroud
interpolation surfaces can be helpful too, provided the traces remain close to a R cst line in the
area of definition of the blade.
Blade Meridional & Tangential Locations
Leading and trailing edge stacking points are compatible with all topological settings. This is not
the case of the other stacking points, which could be unavailable or prevent the selection of
subsequent settings.
The options centre of gravity, maximum thickness, centre of channel, on camber and on
chord are restricted to dimensional planes (Z,Y) and (m,R*θ) and therefore only available for
axial turbomachinery.
Currently, those special stacking points do not allow splitter blades. Maximum thickness and
centre of channel are not available for hub to shroud interpolation stream surfaces. Centre of
channel is not compatible with conical stream surfaces.
Choosing leading or trailing edge stacking allows more freedom in subsequent choices (edge traces,
camber construction plane, optional splitters,...) and are always available
The sweep law is always available and edge traces are compatible with leading and trailing edge
stacking points only.
2D Blade Sections
Planar stream surfaces impose (Z,Y) as construction plane for the camber curve. Revolved stream
surfaces should use (m,R*θ) construction plane.
A reference length is needed when a sweep stacking law has been selected and should always
be an axial length DZ: other lengths are meaningless with planar or cylindrical stream surfaces.
Both construction modes independent suction & pressure sides and camber & thickness are
always available for (Z,Y) and (m,R*θ) construction planes.
DM and DZ reference lengths have the same effect for pure axial cases.
Optional Splitters
The splitters menu is available when leading or trailing edge stacking is selected in the meridional
location menu. Most settings are shared with the main blade topology (construction mode and
edge shape) but the amount and values of the parameters are specific.
Technological Effects
Edge filing is available for blunt trailing edges in single blade cases only. Blade cutoff is always
available.
Radial Pumps, Compressors & Turbines
Several template models are available for radial machines:
l a centrifugal compressor model,
l a centrifugal compressor with a single splitter blade,
l a pure radial diffuser.
Stream Surfaces
Usual construction planes for the camber curve are (m,β) and (
,θ) planes, whereas only
conical and hub to shroud interpolation stream surfaces are usually applied.
Blade Meridional & Tangential Locations
Leading and trailing edge stacking points are compatible with all topological settings while all
other points are simply not available.
The sweep law and edge traces are always available but the traces are usually preferred.
2D Blade Sections
Assuming conical or interpolated stream surfaces have been selected, the construction of the blade
section is limited to a few choices:
1. Common construction planes for the camber curve in radial cases are (m,β) and (
,θ)
planes.
2. A reference length is needed when a sweep stacking law has been selected and the designer
can choose among axial length DZ, radial length DR and meridional length DM. In pure radial
cases, an axial length DZ is not suitable, but not forbidden in AutoBlade™
3. Only camber & thickness construction mode is compatible with common construction planes
introduced above.
Optional Splitters
Splitter blades are always available.
Technological Effects
Edge filing is available for blunt trailing edges in single blade cases only. Blade cutoff is always
available.
Wind Turbines
To design a wind turbines, the easiest way is to start form the provided template.
Stream Surfaces
Planar axial stream surfaces is the preferred choice. Cylindrical surfaces is an alternate choice.
Blade Meridional & Tangential Locations
All stacking points are available, with three usual options: center of gravity, on camber or on
chord. Those options are required when using rounded tip topology.
Edges traces are not compatible with very high staggered blades near the tip section (near or
exceeding 90 degrees). Therefore, a sweep law is advised because crossing edges are allowed in
the meridional view.
2D Blade Sections
Both construction modes are allowed, but thickness addition is the usual choice. The construction
plane is (Z,Y) or as a second choice (m,Rθ).
Optional Splitters
Not applicable
Technological Effects
Not applicable
Marine Propeller
To design a marine propeller, the easiest way is to start from the provided marine propeller
template available in the Geometry/Import parametric model... menu.
The template for marine propeller is the PPTC VP1304 with rounded tip topology.
Stream Surfaces
Cylindrical surfaces is the preferred choice. Conical and Planar axial stream surfaces are
alternate choices.
Blade Meridional & Tangential Locations
All stacking points are available, with three usual options: center of gravity, on camber or on
chord.
Leading edge or Trailing edge are also convenient. But those stacking point are not compatible
with rounded tip topology.
2D Blade Sections
For the main blade, the reference length True Chord Based is preferable.
For the side curves, both construction modes are allowed, but thickness addition is the usual
choice.
Optional Splitters
Not applicable
Technological Effects
Not applicable
Flank-Milled Compressor & Ruled Blades
This section describes the definition of ruled blades in general, where the ruling direction can be
controlled with precise CAD output of the side surfaces.
Stream Surfaces
All surfaces are available,
centrifugal cases.
interpolated stream surfaces being the most usual choice for
Blade Meridional & Tangential Locations
Leading edge, trailing edge, on camber and on chord options are available. Other stacking
points are unavailable because the profile cannot be built directly in the construction plane.
Edges traces and sweep law are both allowed.
2D Blade Sections
Thickness addition is the only construction mode available. Double blunt is mandatory for late
elliptical rounding, with or without cutoff.
Optional Splitters
Splitter blades are always available.
Technological Effects
The compatible effects are the generalized cutoff (linear and spline options), the late elliptical
rounding (only for double blunt case) and the non axi-symmetric endwalls.
TABLE 3.10 Compatibility table for topological settings
3.2
OPTIONAL QUANTITIES
AutoBlade™ provides the ability to compute data such as thickness extrema, moments of inertia
and channel width.
Two major interests justify the computation of a quantity:
l Monitoring purposes : optional geometrical quantities can be checked at any time in
AutoBlade™ interface, even while editing the model.
l Constraints : any quantity selected in AutoBlade™ interface can be constrained in the
optimization process loop of FINE™/Design3D as part of the objective function .
Menu Overview
FIGURE 3.92
Optional quantities menu (selection panel)
Clicking the Optional quantities interface button opens a window with two panels:
1. a Selection notebook : contains sampling and properties switches to select the desired
quantities . Three tabs containing different types of data are available
(FIGURE 3.92).
2. a Monitor list: contains a double list with the quantity type on the left and corresponding
values on the right. The choice panel shows two columns. In the first one, quantity types that
were selected through the notebook are listed and, in the second one, the corresponding
quantity names are listed with their value. All quantity names conform to a naming convention
explained in the next paragraph. Each time a quantity is selected in the notebook, the left list
shows one or more new entries (FIGURE 3.93).
Selecting an item in the left list will refresh the content of the right list, but this is not sufficient to
update the values. In particular, newly added quantities are not computed immediately. To update
all quantities, please click the Apply button and check the values: they should now appear correct
in the right list.
The left Choice list allows multiple selection by means of the <Shift> and <Ctrl> modifiers. The
selection is reset once the window is closed.
FIGURE 3.93
Optional quantities menu (monitor panel)
The two boxed panel Selection and Monitor can be collapsed and restored by a left click on the
corresponding large blue button. This is useful to monitor changes while editing the model since the
menu takes less space on the desktop.
Naming Conventions
Every quantity depends on one or several blade sections. Some of them are side or edge specific.
In order to allow easy distinction and ensure consistency between menus, a naming convention
has been established. Conventions in the formula below are described shortly and will be
particularized for each quantity type.
(S?_)(SPLIT?_)(PREFIX_)QUANTITY_(SUFFIX)
where ’?’ stands for a digit and ’(...)’ describes an optional field
Field
S?_
Description
Section prefix
This prefix applies for section specific quantities. An integer is used to define the section
number, ranging from 1 to the total amount of primary sections.
S1_ defines a quantity relative to the first primary blade section
S1S3_ is a special notation for a quantity difference between sections 1 and 3.
SPLIT?_
Splitter prefix
This prefix applies for splitter specific quantities. Numbering begins at 1 for the first
splitter.
SPLIT1_ defines a quantity relative to the first splitter blade.
PREFIX_
Quantity prefix
This prefix applies for quantities that depend on a side or an edge.
LE and TE mean leading and trailing edges,
SS and PS apply for suction and pressure side respectively.
QUANTITY_ Quantity name
This is the quantity base name. The chosen string is as short as possible while long
enough to allow easy understanding.
For instance, THICK stands for "thickness" and WEDGEANG stands for "wedge angle".
SUFFIX_
Quantity suffix
This suffix is chosen among three types:
l extrema suffixes MIN_ and MAX_ for maximum and minimum values,
l sampling suffixes U??_ for samples,
l special MIN_U and MAX_U suffixes for extrema locations.
For instance, THICK_MAX, THICK_U34 and THICK_MAX_U stand respectively for
maximum thickness value, thickness value at 34 percent of the length and length fraction
corresponding to the maximum thickness value.
3.2.1
Selection Notebook
The first panel in Optional quantities menu is a selection notebook. Clicking on the tabs grants
user access to three different categories of quantities. For each quantity, description and naming
conventions are given in the three next paragraphs. If necessary, the computation method is also
described shortly.
A. Sampling
These sampled values are extracted from available distributions . For
each distribution, responses are computed versus a normalized length and thus, user input values
are kept between 0.0 and 1.0. Up to fifteen values can be generated for each distribution. All
sample locations are automatically rounded to the nearest percentage value and duplicate values
are discarded.
For the optional quantities, the camber curve and the mean line are considered with their three
global coordinates (X,Y,Z). This allows AutoBlade™ to use the same formulas whatever the
topology (i.e. axial or radial).
In order to allow the user to input values between 0.0 and 1.0, AutoBlade™ uses the length of the
camber line as normalization factor. In such fashion, the 0.0 station would comprise the leading
edge point of the camber line and the 1.0 station represents the trailing edge. Other points between
0.0 and 1.0 have their coordinates extracted according to the percentage of the total camber length
they are located at. The total length of a curve can be calculated as:
where
at the global coordinate (
is the number of points describing the curve [0,1,2,…,
]. Therefore, a point j located
) would have the following as normalized coordinate:
length of
the camber
the user can check the total
In AutoBlade™,
line through the
Analysis/Optional quantities... menu. In the Optional quantities window, the user selects the
Camber length under the Scalar values tab. Then when clicking on the Apply button and on
the Camber length, the value is displayed and represents the result of the equation (3-16a). When
the number of Camber coordinates is selected under the Sampling tab (e.g. 4), the user is in fact
in the equations (3-16a) and (3-16b). In that case, by inputting 0 0.33
selecting the value of
0.67 1 , the user is specifying the normalized coordinates at which he desires to extract the
coordinates of sampling points (in this case at 0%, 33%, 67% and 100% of the total camber line
length).
TABLE 3.11 summarizes the sampling capabilities in AutoBlade™. A detailed description of
every distribution follows.
TABLE 3.11 Sampling summary
Quantity
Input value
Response
hub angle
length fraction of the hub
curve
shroud angle
length fraction of the shroud
curve
hub curvature
length fraction of the hub
curve
angle of the hub curve (in degrees)
angle of the shroud curve (in degrees)
signed curvature of the hub curve
shroud
curvature
thickness
length fraction of the shroud
curve
signed curvature of the shroud curve
length fraction of the blade
section mean line
thickness computed in X,Y,Z coordinates at input
location
metallic angle
length fraction of the suction
or pressure side
angle on SS or PS computed in (
,θ) plane. The
unit is degree
curvature
length fraction of the suction
or pressure side
signed curvature of suction or pressure side computed
in (m, R*θ) plane
channel width
length fraction of the mean
fluid line
width of the channel seen perpendicularly to the mean
fluid line in (
,θ) plane
camber metallic
angle
length fraction of the camber
curve
angle of camber curve in (
,θ) plane. The unit is
degree
camber
curvature
length fraction of the camber
curve
angle of camber curve in (m, R*θ) plane. The unit is
degree
mean line
metallic angle
length fraction of the blade
section mean line
angle of mean line in (
,θ) plane. The unit is
degree
mean line
curvature
draft angle
length fraction of the blade
section mean line
signed curvature of mean line in (m, R*θ) plane. The
unit is degree
length fraction of the suction
or pressure side
draft angle (in degree)
Endwall Angle
The angle of the hub or shroud curve is measured in degrees in the meridional plane (Z,R).
Quantity
HUB_ANGLE_U??
SHROUD_ANGLE_U??
Endwall Curvature
Examples
HUB_ANGLE_U33 stands for angle value at 33 percent of the
hub curve length.
SHROUD_ANGLE_U75 stands for angle value at 75 percent of
the shroud curve length.
The signed curvature of the hub or shroud curve is measured in the meridional plane (Z,R).
Quantity
HUB_CURV_U??
SHROUD_CURV_U??
Thickness
Examples
HUB_CURV_U33 stands for signed curvature value at 33
percent of the hub curve length.
SHROUD_CURV_U75 stands for signed curvature value at 75
percent of the shroud curve length.
Thickness is defined as the blade width measured in the perpendicular direction along the blade
section mean line ( FIGURE 3.94 ). Mean line and thickness are both computed in spatial
coordinates (X,Y,Z) for any primary blade section. Therefore, thickness distribution and sampling
are always available.
FIGURE 3.94
Thickness computation
Quantity
Examples
S?_(SPLIT?_)THICK_U??
S1_THICK_U33 stands for thickness value at 33 percent of the
mean line length for main blade section 1.
S2_SPLIT1_THICK_U60 stands for thickness value at 60
percent of the mean line length for the second section of the first
splitter blade.
Side Metallic Angle
Metallic angle is available for both sides of any primary blade section. It is computed in (
,θ)
conformal plane and the calculated angles are given in degrees. Samples always apply on both
sides.
Quantity
Examples
S?_(SPLIT?_)SS_METALANG_U??
S?_(SPLIT?_)PS_METALANG_U??
S1_SS_METALANG_U33 stands for metallic angle value at 33
percent of the suction side length for main blade section 1.
S2_SPLIT1_PS_METALANG_U60 stands for metallic angle
value at 60 percent of the pressure side length for the second
section of the first splitter blade.
Side Curvature
Curvature is available for both sides of any primary blade section. It is computed in (m,R*θ) plane
and always applies on both sides.
Quantity
Examples
S?_(SPLIT?_)SS_CURV_U??
S?_(SPLIT?_)PS_CURV_U??
S1_SS_CURV_U33 stands for signed curvature value at 33
percent of the suction side length for main blade section 1.
S2_SPLIT1_PS_CURV_U60 stands for signed curvature value
at 60 percent of the pressure side length for the second section of
the first splitter blade.
The local curvature radius is obtained by inverting the curvature value.
Channel Width
For each primary section, the channel width is computed along a mean fluid line, built in the (
,θ) conformal plane, between the suction side of the main blade and the pressure side of the
adjacent blade. The channel path is defined as the mean fluid line portion that really "sees"
consecutive blades. On FIGURE 3.95, locations s=0 and s=1 limit the channel path.
The width is then measured in spatial coordinates along the channel path and plotted versus its
length fraction "s". The channel width is available for all primary sections in single blade cases
only.
FIGURE 3.95
Channel width computation
Quantity
S?_CHANNEL_U??
Examples
S1_CHANNEL_U33 stands for channel width value at 33
percent of the fluid path length for section 1.
Mean Line Metallic Angle & Curvature
The mean line is the line located mid-way between suction and pressure sides. This line is built in
,θ) conformal plane where the metallic angle is computed. The curvature is processed in
(
(m,Rθ) plane.
Quantity
S?_(SPLIT?_)ML_METALANG_U??
S?_(SPLIT?_)ML_CURV_U??
Examples
S1_ML_METALANG_U50 stands for metallic angle
value at 50 percent of the mean line length for main blade
section 1.
S2_SPLIT1_ML_CURV_U80 stands for signed curvature
value at 80 percent of the mean line length for the second
section of the first splitter blade.
Camber Metallic Angle & Curvature
The camber differs from the mean line when suction and pressure sides are built independently
(with side curves method or asymmetric thickness addition).
Quantity
Examples
S?_(SPLIT?_)CAMBER_METALANG_U??
S?_(SPLIT?_)CAMBER_CURV_U??
S1_CAMBER_METALANG_U50 stands for metallic
angle value at 50 percent of the camber curve length for
main blade section 1.
S2_CAMBER_CURV_U80 stands for signed curvature
value at 80 percent of the camber curve length for main
blade section 2.
Beta Star
Angle βstar (expressed in degrees) is defined by relation (3-17a) and applies to either camber or
mean line of each section.
Quantity
Examples
S?_(SPLIT?_)CAMBER_BETASTAR_U?? S1_CAMBER_BETASTAR_U50 stands for βstar angle
value at 50 percent of the camber curve length for main
blade section 1.
S?_(SPLIT?_)ML_BETASTAR_U??
S2_ML_BETASTAR_U80 stands for βstar angle value at
80 percent of the mean line curve length for main blade
section 2.
Epsilon
Angle ε is defined by relation (3-17b) and applies to either camber or mean line of each section.
The value is expressed in degrees.
Quantity
Examples
S?_(SPLIT?_)CAMBER_EPSILON_U??
S?_(SPLIT?_)ML_EPSILON_U??
S1_CAMBER_EPSILON_U50 stands for ε angle value at
50 percent of the camber curve length for main blade
section 1.
S2_ML_EPSILON_U80 stands for ε angle value at 80
percent of the mean line curve length for main blade
section 2.
B. Scalar Values
This page contains switches to select geometrical data computed for each blade section, except
throat section area which is a global property. Some scalar quantities - namely minimum
channel width, unguided turning angle and throat section area - are not available when one
or more splitter blades are defined.
FIGURE 3.96
Scalar values option tab
Draft angle extrema
Defines the extrema of the draft angle for casting process.
Quantity
Examples
DRAFT_ANGLE_MIN
the minimum draft angle
DRAFT_ANGLE_MEAN
the averaged draft angle
DRAFT_ANGLE_MAX
the maximum draft angle
Camber & Mean Line Length
The lengths of the camber curve and mean line are built in spatial coordinates, not in a peculiar
construction plane.
Quantity
Examples
S?_(SPLIT?_)CAMBER_LEN
S1_CAMBER_LEN stands for the length of the main camber
curve on section 1
S?_(SPLIT?_)ML_LEN
S1_CAMBER_LEN stands for the length of the mean line in
section 1 of the main blade
Special Camber Properties
Several camber quantities are available for all sections and illustrated in the few next figures
(figures 3.3.2-96 to 3.3.2-98).
Meridional chord, chord and stagger angle
The meridional chord is defined as the difference in m coordinate between leading and trailing
edge. In pure axial cases, this length is then the real axial chord.
The stagger angle is the angle measured in (
,θ) conformal plane between the edge points.
This angle is equivalent to the one measured in (m,Rθ) plane for pure axial cases.
To ensure proper values, the chord is defined as the ratio of the meridional length to the cosine of
the stagger angle. In pure axial cases, this definition of the chord produces the same value as the
distance between edge points in the dimensional (m,Rθ) plane.
FIGURE 3.97
Chord, meridional chord and stagger angle
Maximum NACA height
This quantity simply extracts the maximum height measured relatively to the chord in (m,Rθ)
plane and only has meaning in pure axial or nearly axial cases. Its location as a fraction of the
chord is also provided, as the next figure clearly explains.
FIGURE 3.98
Maximum camber height (NACA style definition)
Solidity
The last camber related quantity is the solidity and its alternative meridional definition. As for the
maximum NACA height, this special value is built from (m,Rθ) plane and loses all interest in
radial configurations! It is defined as the ratio of the chord to the average distance between the
camber lines of the main blade and the next occurrence of the blade.
The meridional solidity is defined relative to the meridional chord instead of the chord.
FIGURE 3.99
Section solidity
Solidity is defined for the main blade only!
Quantity
Examples
S?_(SPLIT?_)CHORD
S1_CHORD stands for the chord of the main camber curve of
section 1
S?_(SPLIT?_)AXIALCHORD
S1_AXIALCHORD stands for meridional chord of the main
camber curve of section 1
S?_(SPLIT?_)STAGGERANG
S1_STAGGERANG stands for stagger angle of the main camber
curve of section 1
Quantity
Examples
S?_(SPLIT?_)NACAH_MAX
S1_NACAH_MAX stands for the maximum height of the
camber in section 1 of the main blade, relative to the chord
S1_NACAH_MAX_U is the fractional location of this maximum
along the chord for the same section
S1_SOLIDITY stands for the solidity of the main camber curve
on section 1
S1_AXIALSOLIDITY stands for the meridional solidity of the
main camber curve on section 1
S?_SOLIDITY
S?_AXIALSOLIDITY
Thickness Extrema
Maximum value: thickness distribution is examined and the highest value found is reported as
maximum. Maximum thickness value always exists and is reported with its corresponding
location along the blade section mean line as a fraction of the length in the range [0,1].
Minimum value: thickness distribution is examined. Each time a local thickness minimum is
found, it is retained if lower than the previous one. This minimum value is thus a global optimum
in the mathematical sense, not simply the smallest value in the distribution. For instance, starting
and ending zero thicknesses are not taken into account as minima in rounded cases. Location
along the blade section mean line is also available.
The minimum value does not always exist since it is a mathematical optimum. When not found, a
"none" string is reported in the list for both value and location. This does not apply for the maximum
thickness value.
Quantity
Examples
S?_(SPLIT?_)THICK_MIN_U
S?_(SPLIT?_)THICK_MIN
S?_(SPLIT?_)THICK_MAX_U
S?_(SPLIT?_)THICK_MAX
S1_THICK_MIN_U stands for thickness minimum location
along the mean line of main blade section 1. It is expressed as a
fraction length in the range [0,1] except when no minimum value
is found.
S2_SPLIT1_THICK_MIN is the name given to the minimum
thickness value for the second section of the first splitter blade.
S1_THICK_MAX_U stands for thickness maximum location
along the mean line of main blade section 1. It is expressed as a
fraction length in the range [0,1].
S2_SPLIT1_THICK_MAX is the name given to the maximum
thickness value for the second section of the first splitter blade.
Minimum Channel Width
The Channel width distribution is examined and the smallest value found is reported as
minimum. This value is not available in splitter cases. Please note the corresponding location
along the fluid path is not available. Unit is of dimension [L].
Quantity
Examples
S?_CHANNEL_MIN
S1_CHANNEL_MIN stands for the minimum channel width
value along the fluid path for main blade section 1.
FIGURE 3.100
Channel width and minimum value (axial turbine)
Unguided Turning Angle
Unguided turning angle is defined as the angle between two lines starting from the suction side
point where the minimum channel width is located:
l the first line is perpendicular to the channel width
l the second line passes through the junction point between suction side and trailing edge circle
in rounded edge case or the end of the suction side curve in blunt case.
This value is computed in (
,θ) plane as shown in FIGURE 3.101 for an axial turbine with a
rounded trailing edge
FIGURE 3.101
Unguided turning angle (axial turbine)
Since it is based on channel width computation, this quantity is available in single blade type only.
Angles are given in degrees.
Quantity
Examples
S?_UNGUIDEDTURNANG_U
S?_UNGUIDEDTURNANG
S1_UNGUIDEDTURNANG_U stands for the unguided turning
angle location on suction side for main blade section 1. It is
expressed as a fraction length in the range [0,1].
S1_UNGUIDEDTURNANG stands for the unguided turning
angle value for main blade section 1.
Throat Area
Two types of throat area estimates are available:
l estimate of spatial throat surface area or "3D throat"
l estimate of projected throat surface area in the (X,Y) plane
This quantity is not available in splitter cases. Unit is of dimension [L²].
Quantity
THROAT
THROAT2D
Wedge Angle
Examples
Throat section area estimate computed in spatial coordinates
Throat section area estimate projected on (X,Y) plane
Wedge angle is defined at leading edge as the angle slope difference, in the (
,θ) plane,
between a position on suction side and a position on pressure side. Those positions are length
fractions of suction and pressure sides in the range [0.01,0.15]. 5 percent is the default value.
Quantity
Examples
S?_(SPLIT?_)WEDGEANG
S1_WEDGEANG stands for the wedge angle value at leading
edge of main blade section 1.
S2_SPLIT1_WEDGEANG stands for the wedge angle value at
leading edge of first splitter blade section 2.
Section Area
Section area estimate is computed in (Z,R*θ) plane as the polygonal area limited by the
discretized suction and pressure side curves. If θ is small, this corresponds to a projected area in
(Z,Y) plane.
A very good accuracy is reached by AutoBlade™ using this simple scheme.
This quantity is available for every section and blade type. Unit is of dimension [L²].
Quantity
Examples
S?_(SPLIT?_)AREA
Flexional Inertia
S1_AREA stands for the section area estimate of main blade
section 1.
S2_SPLIT1_AREA stands for the section area estimate of the
first splitter blade section 2.
An estimation of the flexional inertia is computed in (Z,R*θ) plane as 2D section inertia for every
primary section and three values are generated:
1. minimum moment of flexional inertia,
2. maximum moment of flexional inertia,
3. angle in degree between the minimum moment direction and Z axis direction.
Moments unit is of dimension [L4] and values are always related to the center of gravity of the
section in (Z,R*θ) plane.
The flexional inertia is computed with respect to all possible rotation axes in this plane through the
center of gravity of the section. For one specific rotation axis the flexional inertia or moment of
inertia is defined by I = ∫ m r² where "m" is the mass or area of the section and "r" is the
perpendicular distance to the rotation axis.
The flexional inertia of the section with respect to all possible axes can be described as a tensor.
The eigenvalues of this tensor provide the minimum and maximum value of flexional inertia and
the eigenvectors provide the corresponding rotation axes. The angle as indicated in "Flexional
inertia - angle" (p. 234) defines the angle between the z-direction and the rotation axis of the
minimum flexional inertia.
FIGURE 3.102
Flexional inertia - angle
It is important to note that the flexional inertia in (Z,R*θ) plane is only correct for planar
construction surfaces of the sections. For e.g. conical surfaces it is not correct because the value of
the radius is not constant for the section. As a solution the (Z,R*θ) plane is kept for processing of
the area, flexional inertia and torsional inertia, but the section is reprojected on the ‘closest’
cylinder for each section. This closest cylinder is the one that passes through the mid-point of the
3D line segment joining the leading to trailing edge.
Quantity
Examples
S?_(SPLIT?_)IMIN
S?_(SPLIT?_)IMAX
S?_(SPLIT?_)IMINANG
Torsional Inertia
S1_IMIN stands for the section minimum moment of flexional
inertia for main blade section 1.
S1_IMAX stands for the section maximum moment of flexional
inertia for main blade section 1.
S1_IMINANG stands for the angle between minimum moment
of flexional inertia direction and Z axis direction for main blade
section 1.
An estimation is computed, either in (Z,R*θ) plane or in X,Y,Z coordinates, for every section.
The torsional moment of inertia is evaluated thanks to the approximate formula for thin profiles.
Moments unit is of dimension [L4].
where
with t being the local thickness measured perpendicularly to the mean line, U the length of the
mean line and A the section area .
FIGURE 3.103
Torsional inertia - mean line integration
The (Z,R*θ) case is similar to a computation in (Z,Y) plane as soon as θ is near zero for the
whole section and planar or cylindrical stream surfaces are chosen. Suction and pressure side
curves are considered in spatial cartesian coordinates.
The above formula is an approximation that loses its accuracy for thick blade sections.
Quantity
S?_(SPLIT?_)JT
S?_(SPLIT?_)JT2D
Examples
S1_JT stands for the moment of torsional inertia value for main
blade section 1, computed in spatial coordinates
S2_SPLIT1_JT2D stands for the moment of torsional inertia
value for section 2 of the first splitter blade, computed in
(Z,R*θ) plane
C. Edges Control
FIGURE 3.104
Edge control options tab
Coordinates
Edge coordinates Z, R or θ can be exported as quantities to the optimization process for both
leading and trailing edges. In blunt cases, the arithmetic average of leading and trailing edges end
points is returned.
It is also possible to know coordinate differences from section to section as described in TABLE
3.12, where Ci is the related coordinate for section i. Please note these differences can be positive
or negative. For n sections (n>2), n differences or "delta" values are computed from which the last
one is the sum of the (n-1) first ones.
TABLE 3.12 Coordinates differences
Number of sections
Returned delta values
0, 1
...
not applicable
1: C1 - C2
3: C1 - C2, C2 - C3, C1 - C3
4: C1 - C2, C2 - C3, C3 - C4, C1 - C4
...
n: C1 - C2, C2 - C3, ... Cn-1 - Cn, C1 - Cn
Quantity
Examples
S1_LE_Z stands for the Z coordinate of leading edge point for
section 1 of the main blade.
S2_SPLIT1_TE_R stands for the R coordinate of trailing edge
point for section 2 of the first splitter blade.
S1S2_LE_DZ stands for the Z coordinate difference of leading
edge points for sections 1 and 2 of the main blade.
S1S3_SPLIT1_TE_R stands for the R coordinate difference of
trailing edge points for sections 1 and 3 of the first splitter blade.
S?_(SPLIT?_)LE_Z,
S?_(SPLIT?_)LE_R,
S?_(SPLIT?_)LE_THETA,
S?_(SPLIT?_)TE_Z,
S?_(SPLIT?_)TE_R,
S?_(SPLIT?_)TE_THETA
S?S?_(SPLIT?_)LE_DZ,
S?S?_(SPLIT?_)LE_DR,
S?S?_(SPLIT?_)LE_DTHETA,
S?S?_(SPLIT?_)TE_DZ,
S?S?_(SPLIT?_)TE_DR,
S?S?_(SPLIT?_)TE_DTHETA
Fitting Lines
The searching for the best straight line approximating the main blade edge traces can be obtained
through AutoBlade™. A fitting line is computed in (span, Z), (span, R) or (span, θ) plane from
the edge coordinates according to the generic form:
,
so three values are generated, namely constants a , b and the approximate error. Angular
coefficient a is returned in the form of an angle with respect to the ordinate direction, as shown in
the next figure.
FIGURE 3.105
The best fitting line construction
A fitting line is computed from edge coordinates of the primary sections only. The use of this
option is facilitated if all the span values are nearly uniformly spaced and extreme sections at hub
and shroud are typically included. For instance, a (0.0, 0.20, 0.40, 0.60, 0.80 0.99) span list will
give meaningful parameters and (0.0, 1.0) will given an error free fitting line.
This quantity is available for the main blade only, with or without splitters. The angle ANG is
provided in degrees and the ERROR is of dimension [L].
Quantity
Examples
LE_BESTLINEZ_ANG is the best fitting line angle for the main
blade leading edge in (span,Z) plane. Its value is expressed in
degrees.
TE_BESTLINER_ERROR is the best fitting line error for the
main blade trailing edge in (span,R) plane.
LE_BESTLINEZ_ANG,
LE_BESTLINER_ANG,
LE_BESTLINETHETA_ANG,
TE_BESTLINEZ_ANG,
TE_BESTLINER_ANG,
TE_BESTLINETHETA_ANG
LE_BESTLINEZ_ERROR,
LE_BESTLINER_ERROR,
LE_BESTLINETHETA_ERROR,
TE_BESTLINEZ_ERROR,
TE_BESTLINER_ERROR,
TE_BESTLINETHETA_ERROR
3.2.2
Summary Table
All quantities and samples are available whatever the topology choices, except the following
options.
TABLE 3.13 Quantities availability
Quantity
Channel width
Minimum channel width
Unguided turning angle
Throat section area
Single blade cases
Splitters cases
available
available
available
informational only
not available
not available
not available
not available
3.3
GEOMETRY ANALYSIS
The Geometry Analysis icon of the model editor, in the left area of the main interface, grants
access to the geometry analysis tool.
This tool generates plots showing the distribution used to generate the samples in Optional
quantities notebook (Sampling). This menu can be left open for monitoring purposes while editing
the topology and parameters and updates automatically after each change.
FIGURE 3.106
Geometry analysis tool
Up to 8 geometry analysis windows are allowed simultaneously.
When the window is re-sized, the aspect ratio cannot be preserved.
Selectors
Five selectors are available to control the distribution. The selectors control the Quantity, Blade,
Section , Abscissa and Cut , respectively. The selectors Quantity and Abscissa are always
available and control respectively the choices of ordinate and abscissa. The selectors Blade and
Section are available for some distributions and control the choices of blade and primary section.
If the quantity is plotting a cut value, the Cut coordinate choice can be selected. The next table
details the usage of the selectors.
TABLE 3.14 Selectors for distributions
Selector
Usage
Values
Quantity
Controls the ordinate of the
graph.
All values are always available,
except Channel width that
applies to single blade cases
only.
l endwall angle
l endwall curvature
l section thickness
l mean line theta
l mean line metallic angle
l mean line curvature
l mean line beta star
l mean line epsilon
l side curves metallic angle
l side curves curvature
l epsilon axial cut
l camber curve metal angle
l camber curve curvature
l channel width
l draft angle
l spanwise chord length and its meridional projection
l spanwise meanline angles (stagger, LE metal and
TE metal)
l spanwise solidity and its meridional solidity
l spanwise leading and/or trailing edge radius
l spanwise Z coordinate profiles for leading edge,
trailing edge and gravity center
l spanwise R coordinate profiles for leading edge,
trailing edge and gravity center
l spanwise theta coordinate profiles for leading edge,
trailing edge and gravity center
l spanwise thickness min/max values
l spanwise thickness cut value
l spanwise throat width
Selector
Usage
Abscissa
Controls the abscissa of the
graph.
Values
l curve length
l fraction of the curve length (used for sampling)
Blade
Section
Cut
Up to four choices are available
according to the selected
quantity.
l m coordinate
coordinate
Thickness, mean line and side
curves distributions require the
selection of a blade when at
least one splitter is defined.
l main blade
l splitter 1
l splitter 2
l ...
Thickness, mean line, side
curves and channel width
distributions require the
selection of a primary section
when a splitter is defined.
Spanwise thickness cut value
requires the cut coordinate
where the profile is built.
number of the primary section
l Z coordinate
l R coordinate
l curve length
l fraction of the curve length
In the tool bar, an optional selector curvature Clipping allows to control the clipping of the
ordinate in curvature graphs (endwalls, side curves and mean line). This option limits the default
zoom and the fit operation when the values have a large range of variation.
Another special selector axial Cut value allows to set the Z coordinate at which the mean line is
cut for analysis of the special epsilon angle. The minimum and maximum cuts are automatically
updated according to the bounding box of the mean lines.
All active sections (either primary and parametric sections or discretized sections) are used for
sampling.
Viewing Commands & Options
The graph can be zoomed in by means of the left mouse button. Just click once to define the first
corner, then move the pointer and click again to defined the second corner. The aspect ratio is not
constrained in distributions.
It is possible to highlight one or more curves by selecting their legend text (FIGURE 3.107). This
operation is achieved by means of the middle mouse button. Clicking a selected item removes it
from the selection.
FIGURE 3.107
Highlighting a curve is achieved by means of a middle click over the legend
A few other operations are available in the contextual menu. This menu appears when the right
mouse button is pressed over the graphics area. The following commands are listed and activated:
TABLE 3.15 Optional commands - contextual menu
Zoom back
Reverts the last zoom operation
Fit view
Fits the view (default zoom)
Show/hide legend
Shows or hides the legend. This option is active until the session is closed.
Show/hide
crosshairs
Shows or hides the crosshairs. This option is active until the session is closed.
Show/hide grid
Shows or hides the background grid. This option is active until the session is
closed.
is used to lock specific user-defined ranges for abscissa and ordinate. This special
The icon
flag is inactive by default. If it is activated by clicking the locker icon, the current zoom ranges are
preserved until the user explicitly changes the zoom or deactivates the option. The zoom ranges
are also saved in the project if the locker is activated, so that the user can retrieve the zoom when
saving and reopening a project.
Export
Graphs can be exported to text and postscript files thanks to the commands Save and Print from
the tool bar.
3.4
PARAMETRIC REPORT
The last icon of the model editor, in the left area of the main interface, grants access to a
parametric report aiming the description of the total number of parameters.
The tolerances blocking tolerance and blocking epsilon allow to determine in the Free page the
free parameters that can be considered as blocked when one of the bounds is reached.
CHAPTER 4.
AUTOBLADE™ FITTING
The AutoBlade™ Fitting allows the designer to create a parametric blade model close to a given
customer geometry defined by point coordinates. In this way, it can be seen as a functionality used to
import a blade geometry into the AutoBlade™ or FINE™/Design3D environment.
When a turbomachinery model has not been created under AutoBlade™, it is not possible to import it
directly as a simple and almost instantaneous operation. Instead, the following procedure is required to
obtain an AutoBlade™ model close enough to the target design:
1. First, the data from the CAD software must be converted to the geomTurbo format described in
the next sections. The resulting file is the target geometry.
2. An initial model will then be generated from a quick analysis of the target geometry. Some choices
in topology and parameters are necessary at this stage and a range of values will be estimated for
each parameter by means of a process called initialization. The resulting parametric design is
referred to as the initial model.
3. At last, an iterative process is launched to search the multidimensional space of valid parameters
and to find a better subset of values for the defining parameters. This process, called fitting, is the
time consuming part and may require two or three runs to achieve a satisfying model. The resulting
model is called the fitted solution and will be considered as a conversion of the target geometry
into an AutoBlade™ parametric blade model.
In AutoBlade™, only one fitting process can be launched in a single project.
The fitting module is a kind of optimization tool and is integrated in AutoBlade™ starting from
version 8.9. FIGURE 4.1 shows the fitting interface. The following pads or menu are dedicated to the
fittings module:
l The subpad Target Settings in the left area - allows to access the target settings for the fitting
project, see also Target Settings subpad for more details.
l The subpad Fitting Control in the left area - allows to control the fitting process, see also Fitting
Control subpad for more details.
l The submenus under the menu Analysis - allows to analyze the fitting result, see also Analysis
Menu for more details.
The fitting module requires a special license feature.
FIGURE 4.1
The fitting interface
In the following sections, a step by step guide to the fitting process will be given.
In this section
4.1 Preparing Target Geometry
4.2 Setup Initial Model
4.3 Initialization Process
4.4 Visual Check & Parameters Manual Correction
4.5 Fitting Process
4.6 Fitting Problems
248
258
260
263
265
270
4.1
PREPARING TARGET GEOMETRY
The geometry to "import" must be defined in the ".geomTurbo" format before any fitting project
can begin.
A ".geomTurbo" file contains the curves defining the hub, the shroud and the sections of the
three-dimensional blades. This is an ASCII formatted file beginning with a specific header. Inside
it, any line starting with character '#' is treated as a command and is therefore ignored.
Each section starts with a reserved keyword. Currently, AutoBlade™ supports usual keywords in
both versions 3.7 and 5.3 of the format.
geomTurbo 5.3 (AutoGrid™ 5) is now the preferred format for AutoBlade™, but geomTurbo 3.7
is still supported for backward compatibility. Users of AutoGrid™ 4 will prefer the old format.
4.1.1
GeomTurbo 3.7
This format is deprecated and only allows a single splitter blade. Not all specifications of the
format are supported in the fitting module: external data or merged blade cannot be treated
correctly.
The major supported keywords are listed in TABLE 4.1.
TABLE 4.1 Supported geomTurbo blocks
Keyword
Usage
HUB
starts the definition of the hub curve
SHROUD
starts the definition of the shroud curve
PRESSURE
SUCTION
PRESSURE_
SPLITTER
SUCTION_
SPLITTER
starts the definition of the pressure side curves. A single curve for each section
follows.
starts the definition of the suction side curves. A single curve for each section
follows.
starts the definition of the pressure side curves for the splitter blade. A single curve
for each section follows.
starts the definition of the suction side curves for the splitter blade. A single curve
for each section follows.
The next paragraphs explain the header content, the choice of coordinates and how to add each
section. A last paragraph describes additional keywords that have been introduced specifically for
AutoBlade™. Example Fitting Target Geometry contains sample target geometry files that can be
used as a reference.
Further details about the original geomTurbo format 3.7 and keywords can be found in the
AutoGrid™ 4 User Manual.
".geomTurbo" format is not case sensitive, so all keywords can be written in lower or upper case
letters or even as a mix of both styles.
Header
The header contains a line defining the format and its version and a few optional values that apply
to the geometry.
GEOMETRY TURBO VERSION 3.7
geometric_tolerance 1e-06
blade_expansion_factor_hub 0.03
blade_expansion_factor_shroud 0.03
blade_merging 0
units 1
number_of_blades 36
The blade repetition in the tangential direction is specified after the NUMBER_OF_BLADES
keyword as an integer value.
GEOMETRIC_TOLERANCE, BLADE_EXPANSION_FACTOR_HUB, BLADE_MERGING and
BLADE_EXPANSION_FACTOR_SHROUD are not currently used in AutoBlade™.
Curve Data Formats
Curves must be defined as a set of data points. External files are not supported. It is not possible to
use IGG™ curve formats or linked data files.
Curves are defined by 2 or 3 coordinates and follow a simple rule: a symbolic coordinate system
is defined, followed by the amount of points defining the curve and the list of data points.
Example:
# a meridional curve
ZR
1.2 2.3
1.3 2.4
1.4 2.5
The list of points contains one data point per line and the coordinates are space separated. The
next table lists all supported formats according to the curve type.
TABLE 4.2 Curve data formats
Curve type
hub and shroud
side curve
Supported formats
XYZ, XZY, YXZ, YZX, ZXY, ZYX, ZR, RZ
XYZ, XZY, YXZ, YZX, ZXY, ZYX, ZRTH, ZTHR,
RTHZ, RZTH, THZR, THRZ
where X, Y and Z stand for the cartesian coordinates and Z, R and TH for the cylindrical
coordinates. Angle TH is expressed in radians.
A "space" can be a combination of several space or tab characters.
Hub & Shroud Curves
Endwall curves are usually defined first, but this is not a requirement. A ZR format is preferred
however. Data points must be ordered from inlet to outlet.
AutoBlade™ is not accepting hub and shroud defined as ZR curve along partly Z- axis (R=0), ZR
curve crossing Z-axis or ZR curve defined with negative radius.
Pressure & Suction Side Curves
Suction and pressure side curves are defined separately, under SUCTION and PRESSURE
keywords. The next keyword is always SECTIONAL followed by the number of sections and
the definition of the curves.
Example:
suction
SECTIONAL
+3
# section 1
XYZ
51
0.17669 -0.0208609 0.000351471
0.176693 -0.0208955 0.000391449
...
0.186772 0.0144109 0.0429921
0.186768 0.0144296 0.0429756
# section 2
XYZ
51
0.217127 -0.0231681 0.00303258
0.217124 -0.0231913 0.00306532
...
0.217501 0.0200831 0.0381821
0.2175 0.0200963 0.0381687
# section 3
XYZ
51
0.251068 -0.0250123 0.00642899
0.25106 -0.0250273 0.00645487
...
0.243571 0.0233406 0.0341187
0.243573 0.0233511 0.034108
AutoBlade™ assumes that all sections are ordered from hub to shroud (increasing span
parameter). and curves must be defined from leading to trailing edge.
It is very important to carefully define the starting and ending points of the side curves:
l If the leading edge is rounded, both side curves should begin with the same point coordinates
for any given section.
l If the trailing edge is rounded, both side curves should end with the same point coordinates
for any given section.
l The chosen edge point at a rounded edge must divide the section almost symmetrically in
that region. Although this is straightforward with thin blades, corrections may be required in
some cases.
It is important to point out that good fitting results may depend on the choice of suitable edge
points.
The BLADE keyword which in AutoGrid™ permits to enter a full blade contour as one single curve
is not supported since AutoBlade™ needs both leading and trailing edge points.
AutoBlade™ assumes that the suction side is located above pressure side when plotted against an
increasing θ angle.
Further details about
AutoGrid™ 4 User Manual.
the original geomTurbo format 3.7 and keywords can be found in the
Splitter Blade
In addition to the main blade, the ".geomTurbo" format permits to define one single optional
splitter blade. The splitter blade, if it exists, must be defined on the same sections as the main
blade.
Splitter side curves are defined exactly in the same way as for the main blade: SUCTION_
SPLITTER and PRESSURE_ SPLITTER keywords
replace respectively SUCTION and
PRESSURE.
AutoBlade™ requires that the splitter blade is located below the main blade (when plotted against
increasing θ). An additional argument ROTATE followed by a floating point value may be added
just after the main keyword. This represents a rotation angle (in radians) to be applied on the
splitter side.
Example:
SUCTION_SPLITTER rotate -0.785398
SECTIONAL
+2
...
PRESSURE_SPLITTER rotate -0.785398
SECTIONAL
+2
...
Topologies including multiple splitters cannot be fitted in the current version of the software. This is
a direct consequence of the limitation in the ".geomTurbo" format.
ROTATE argument is not part of the specifications of the ".geomTurbo" format and is optional.
4.1.2
GeomTurbo 5.3
This format is the preferred target input, at least for multiple splitter fitting projects, but may
require AutoGrid™ software if used as output of AutoBlade™.
The ".geomTurbo" file format 5.3 is structured in three main blocks: the header, the channel and
the definition of the rows. Following is a example of a geomTurbo file structure for a
turbomachinery with three blade rows respectively named impeller, diffuser and return channel.
GEOMETRY TURBO
VERSION 5.3
NI_BEGIN CHANNEL
...
NI_END CHANNEL
NI_BEGIN nirow
NAME impeller
...
NI_END nirow
NI_BEGIN nirow
NAME diffuseur
...
NI_END nirow
NI_BEGIN nirow
NAME return channel
...
NI_END nirow
AutoBlade™ does not support all options of the format, especially the following features:
l gap curves at hub and shroud,
l bulbs and nozzles,
l IGG™ data and CAD data (Parasolid™ format) except for non- axisymetric hub and/or
shroud.
Further details about the original geomTurbo format 5.3 and keywords can be found in the
AutoGrid™ User Manual.
Channel Format
The channel format contains the definition of the turbomachinery meridional contours (hub and
shroud). It is defined by two types of curves:
l The basic curves defined by a set of points
l The channel curves defined as a composite of basic curves.
NI_BEGIN CHANNEL
NI_BEGIN basic_curve
NAME curve_1
...
NI_END basic_curve
NI_BEGIN basic_curve
NAME curve_2
...
NI_END basic_curve
NI_BEGIN channel_curve hub
NAME hub
...
NI_END channel_curve hub
NI_BEGIN channel_curve shroud
NAME shroud
...
NI_END channel_curve shroud
NI_END CHANNEL
The ".geomTurbo" file must contain two channel curves named respectively hub and shroud. In
addition, AutoBlade™ does not currently support channels defined as composite of several basic
curves.
AutoBlade™ is not accepting hub and shroud defined as ZR curve along partly Z- axis (R=0), ZR
curve crossing Z-axis or ZR curve defined with negative radius.
Basic Curves
The basic curve format is used to defined a curve and project it in the meridional space (z,r). The
curve is defined at least by
l a name,
l a coordinate type,
l the number of defining points,
l the list of points coordinates
NI_BEGIN basic_curve
NAME curve_1
DISCRETISATION 10
NI_BEGIN zrcurve
ZR
28
-0.0425 0.256692
-0.0312928 0.25656
...
NI_END zrcurve
NI_END basic_curve
The coordinate types are identified by the following keywords: ZR, XYZ, RTHZ, ZRTH, THRZ,
RZTH,... where X,Y and Z are the 3 Cartesian coordinates and R,TH and Z are the 3 cylindrical
coordinates.
The discretization value and optional interpolation type are not used by AutoBlade™.
Channel Curves
The channel curves are used to define the hub and the shroud. A channel curve is a composite of
defined basic curves. It is defined by a name and vertices. The vertex should be an absolute vertex
or belong to a basic curves and is defined by its parametric location (normalized arc length).
NI_BEGIN channel_curve hub
NAME hub
VERTEX ABS_P 0 0 0
VERTEX curve_1 0
VERTEX curve_1 1
NI_END channel_curve hub
NI_BEGIN channel_curve shroud
NAME shroud
VERTEX curve_2 0
VERTEX curve_2 1
NI_END channel_curve shroud
The fitting module uses a single discretized curve. This means that a complex composite curve that
shows several discontinuities in AutoGrid5 will be converted to a single linearly interpolated curve
that does not strictly preserve the vertices.
Row Format
The row format contains the geometry definition of a complete row. It is defined by a row name,
a row type, a periodicity and the definition of the main blade and possibly one or more splitter
blades.
NI_BEGIN nirow
NAME impeller
TYPE normal
PERIODICITY 36
UNITS 1
NI_BEGIN NIBlade
NAME main Blade
...
NI_END NIBlade
NI_BEGIN NIBlade
NAME splitter 1
...
NI_END NIBlade
...
NI_END nirow
Row Periodicity
The periodicity defines the number of main blades in the row.
Units
The units keyword is never used by the software. However, it is preserved in export when the
model has been initialized on a target that contains the keyword. Otherwise, it is not exported to
the geomTurbo output!
AutoBlade™ allows a global scaling factor in the Steerings page and is completely unrelated to the
units keyword.
Blade Definition
The blade(s) and possibly the splitter(s) are defined by a name and two surfaces defining the
pressure and the suction side. The surfaces are identified by the keywords pressure and suction:
NI_BEGIN NIBlade
NAME main Blade
NI_BEGIN nibladegeometry
TYPE GEOMTURBO
suction
...
pressure
...
NI_END nibladegeometry
NI_END NIBlade
The pressure side and the suction side are defined by a set of cross sections of the blade at several
spanwise location. Each section is defined by a set of points:
suction
SECTIONAL
13
# section 1
XYZ
100
0.17669 -0.0208609 0.000351471
0.176691 -0.0208788 0.000370063
...
# section 2
XYZ
100
0.17669 -0.0208609 0.000351471
0.176691 -0.0208788 0.000370063
...
The coordinate types of each sections are identified by the following keywords: ZR, XYZ, RTHZ,
ZRTH, THRZ, RZTH,... where X,Y and Z are the 3 Cartesian coordinates and R, TH and Z are the
3 cylindrical coordinates.
A few optional keywords are supported after the suction and pressure keywords. Further details
about the keywords can be found in the AutoGrid™ User Manual.
4.2
SETUP INITIAL MODEL
Before the initialization and fitting processes take place, a starting model must be defined with
topological settings that are well adapted to the target geometry. It is usually advised to load a
template close to the type of machinery to be fitted, especially to satisfy:
l the number of blade types (with or without splitter blade),
l the machinery type (axial or radial)
Then, the designer should review all design steps and check for settings and amounts of defining
parameters. The few next topics can be seen as quick guidelines. Further details about topological
choices and compatibility are available in the section Topological Compatibility Issues.
When an optimization based on the fitted model is planned, the key point is to use as few sections
as possible (from 2 to 5) and the simplest laws to define the curves. Additional sections will
increase the total number of parameters and the fitting process will be much more time
consuming. When ready, a starting model without splitter blade should contain between 50 and
100 parameters.
More parameters can be defined if the goal is simply to 'import' an existing geometry for a
standalone use of AutoBlade™ on the fitted model. More parameters mean possibly slower
convergence of the fitting process, but also finer results.
Endwall Curves
Bezier and B-spline curves defined by up to 10 nodes are generally good choices for most
designs, except in some specific cases:
l when the endwall curve is nearly linear at one or both ends, a composite line-Bezier-line is
preferred. A B-spline curve type is typically the worst choice and should be discarded.
l when no optimization is planned on endwalls, a parameterless curve may be a suitable. The
data points from the target geometry file should be used here.
Stream Surfaces
This critical choice depend on the way sections are defined in the target geometry file.
l Axial turbomachinery are usually defined on cylindrical or conical stream surfaces. In case
of pure axial geometry, a planar section is another common choice.
l Radial turbomachinery should rely on hub to shroud interpolated stream surfaces or planar
radial surfaces.
Stacking Point
Leading or trailing edge stacking is the most efficient choice, but many rotating geometries use the
centre of gravity. This choice is usually dictated by mechanical considerations.
Meridional Location
l Radial compressors and turbines use edge traces
l A stacking law is suitable in most axial cases (stacking on Z coordinate) or pure radial cases
(stacking on R coordinate).
Sections Construction Mode
A single thickness distribution is the most compatible choice and is usually preferred for radial
machinery and thin blades.
Construction curves is a good choice for axial machinery and thick blades, but it is not compatible
with all camber constructions planes.
Effects
Effects are not handled by the initialization process and are not compatible with the fitting
process. Therefore, effects should be disabled in any fitting project. If an effect is active, a
warning is generated within the interface as soon as one of the processes is being launched.
Expressions
The initialization process does not support dependencies and automatically disables any active
expression in the model before trying to guess suitable values for the parameters.
Expressions allow complex dependencies between the defining parameters and are generally not
compatible with the fitting algorithms. Therefore,
it is highly advisable to disable all
expressions before launching the fitting process.
Some dependencies are safe in the fitting process. As soon as all parameters linked by expressions are
included in the same steps, they are almost always compatible with the fitting process. For instance,
linking several parameters from a single curve always produce valid results. On the contrary, linking
several parameters from one section to another will probably produce very bad results since linked
parameters are involved in separate fitting steps!
4.3
INITIALIZATION PROCESS
Once a valid target file has been imported in the Target settings subpad, an initialization of the
model is possible through the button Adapt model (Adapt model). This operation will guess
suitable values for all or some of the following features:
l hub curve,
l shroud curve,
l the meridional stacking law,
l the tangential stacking law,
l main camber curves,
l main side curves,
l splitter camber curves,
l splitter side curves,
l non axisymmetrical hub,
l non axisymmetrical shroud.
This quick operation will also prepare the minimum and maximum bounds of the parameters, so
that a fitting process can be launched with minimum user input.
FIGURE 4.2
Initialization options
Two initialization methods are available: RESET and IMPROVE. These methods allow to either
reset the selected features or improve them. In the IMPROVE case, the initialization only alters
the feature if the new guess improves the comparison.
Clicking the Ok button will start the initialization process. When launching the initialization
process, the model is stored as a persistent step in the undo stack.
It is important to choose the most suitable topological settings before the initialization: improper
settings will result in poor initial and fitted models. If the initialization process provides a very
rough result, it is probable that some topological choices need to be changed or the amount of
parameters is insufficient.
Some parameters are always reset by the initialization process, even when all features are unselected
and the chosen method is improve. This is the case for the parameters controlling the stream surfaces,
the location of the splitters and the meridional reference position.
What it does?
The initialization process is responsible for the following tasks:
l generate suitable parameters for all curves and laws (hub, shroud, sweep and lean laws,
camber curves, side curves or thickness distributions, several lengths and locations). Values
and bounds are guessed.
l find the best traces for planar, cylindrical and conical stream surfaces.
l change the amount of primary sections and their spanwise locations. Each target section is
considered as a primary section in the initialized and fitted models.
l freeze some parameters that are unlikely to improve the model in the fitting process.
What it does not do?
The initialization process is unable
l to correct poor topology choices or suggest more suitable solutions,
l to adapt the reference values of the parameters,
l to guess some parameters like filing lengths and thicknesses
l to capture some edge shapes like a sharp end,
l to provide a precise model, very close to the target geometry.
When a setting is changed, for instance a curve type or its amount of defining parameters, a new
initialization is required for best results. This is however unnecessary when a blunt type or filing
option is changed.
4.4
VISUAL CHECK & PARAMETERS MANUAL
CORRECTION
Once initialized, the parametric model should be a rough approximation of the target geometry. In
some cases, the results are quite close, but it depends on the topological choices, the overall
number of parameters and the shape of the target geometry. This is why a visual comparison
between the target and the initialized model is necessary before a fitting process is launched.
Visual Check
Comparison is achieved by means of the menu Analysis / Fitting graphs.
A progress meter appears as soon as the page is opened and a quick process begins: the sections
of the target geometry are projected to the stream surfaces of the initial model. This operation
takes a few seconds.
It is important to check the meridional view as well as each section in the conformal (RAHMAN
Md Asfiqur, θ) plane.
1. Endwall curves are usually well initialized. The most critical setting is the number of
parameters in use, especially if hub to shroud interpolated surfaces are used. It may be
necessary to increase the amount of points.
2. When a sweep law is used, the endpoints of the traces may drift away if special stacking
points CC or MT are used. The fitting process will improve this without any manual change.
3. Thick blades with bent camber curves may be poorly initialized (a failure message is usually
generated in that case).
4. Leading and trailing edge radii must be precise in all rounded cases. If not, a manual
correction is necessary (ill formed circular arcs in target or sharp edges).
5. The wedge angle parameters could need correction when construction curves are active for
suction and pressure sides.
6. If the model defines a splitter blade with a refined camber curve, the refinement parameters
are never modified in the initialization process and both values and bounds could be too large.
Topological settings of the model usually do not need further checking if the results are good after
correction of the above issues.
The suction side curve must be the suction side curve from an aerodynamic point of view and the
pressure side curve must be the pressure side curve from an aerodynamic point of view. This can be
checked by activating the markers in the legend of the section graph. If the target suction side is not
the aerodynamic suction side, the target geomTurbo file needs a correction! Please refer to sections 4-
2.1 and 4-2.2 for details about the manipulation of the side curves.
Parameter Bounds Check
The starting model has been altered by the initialization process and the parameters should be
carefully checked before a fitting process.
The Parameters list button (on the Icon bar) or the Geometry/Parameter list menu opens a new
window. This window allows to easily check the value and the bounds of the parameters. If the
bounds are not visible, remember to check the View/Show parameter bounds option. Endwalls
and Others groups may be skipped. In all other groups, the value of the parameters should be free
to move with very few exceptions and the ranges must be large enough.
In addition, a parametric report aiming the description of the total number of parameters can be
opened with the Parametric report button (on the Model Editor subpad) or the menu Analysis /
Parameter report.
2D blade sections
l If the camber curve is of Bezier type defined by a custom amount of equally spaced heights,
the ranges need to be large, at least 20 percent of the highest value in both directions, for all
parameters. A narrow range will indeed limit the results of the fitting if one of the bound is
reached!
l When the trailing edge is rounded and circular (independent construction curves or B-spline
thickness), the corresponding radius can be frozen by means of the Reset command (contextual
menu). The estimate of the initialization process is usually precise and cannot be improved by
the fitting process.
l When available, the half wedge angle parameter at leading edge is large when the blade is
thick, so the range needs to be large also. Angles are given in degrees. The range at trailing
edge is usually large enough.
Meridional and tangential locations
The range and value of the angular parameters are usually suitable.
4.5
FITTING PROCESS
Once the parameters of the initialized model have been checked and their bounds corrected, a
fitting process can be launched through the button Fitting model (Fitting Control subpad) to get a
solution closer to the target geometry.
The fitting process uses an optimization algorithm (typically a genetic algorithm) combined to an
estimate of the error between the current model and the target geometry. To achieve a solution
that minimizes this error criterion, the process is split into successive steps which consist in local
optimizations that involve only a subset of the parameters defining the machine.
For each step, a subset of active parameters is extracted and an initial population is generated with
random values of the active parameters inside their allowed range. An iterative process begins in
which a new population is generated from the best representative of the previous population.
4.5.1
Fitting Settings
FIGURE 4.3
Settings controlling the fitting process
Fitting Features
A complete fitting is achieved with default settings. For convenience, AutoBlade™ allows the
user to select the features involved in the fitting process by selecting their order and the number of
times the fitting process has to be applied.
Here are some examples.
l If the endwalls are defined by parameterless curves, they do not need fitting.
l If the endwalls need fitting while hub to shroud interpolated stream surfaces are applied, the
sections cannot be finely fitted in the first fitting run, since the endwalls are usually not
sufficiently improved after the first step. In such a case, it is advised to fit the endwalls only, by
means of two or three fitting processes. Then, in a new computation, the fitting can be applied
on the stacking laws and sections.
Each feature in the list corresponds to one step of the fitting process except for the primary_
sections feature that will lead to several steps function of the number of sections and blades.
When a Non-Axisymmetric Hub/Shroud is defined, additional features non_axisymmetric_hub
and non_axisymmetric_shroud are available for the fitting process. The number of steps equals the
number of cuts, including the start and end cuts.
Optimization Settings
Several algorithms are accessible for the fitting process and it is even possible to combine them or
customize their settings.
However, the genetic algorithm gives the best results and the three default modes Coarse ,
Medium and Fine are sufficient in practise (FIGURE 4.3 ). All those modes use a genetic
algorithm and share the same settings, except
the number of iterations. They correspond
respectively to a number of reproduction cycles of 25, 50 and 100. This really means that a Fine
process is twice slower as a Medium process which is twice slower as a Coarse process.
User- Defined mode is not covered in this manual and should not be enabled. Default settings
Coarse, Medium and Fine are sufficient even for an advanced user.
4.5.2
First Run
Two to three runs are usually sufficient to achieve a good result in single blade cases. The first
run is usually a coarse process because the topological settings could be wrong or bounds of
some parameters reached early. In such a case, a longer process useless.
Clicking the Ok button will start the fitting process. When launching a fitting process, each step is
specified in the status bar. The resulting model at the end of the process is set as persistent. The
convergence history and log file are saved on disk.
An Abort operation button appears on top of the interface to allow abort of the process. If clicked,
the current step is not interrupted, but all next steps are skipped and the message is changed to
"ABORTING – please wait".
Fitting Steps
The first two fitting steps optimize the endwall curves (optional) as well as the meridional and
tangential locations of the edge traces (optional). Then, the parameters defining the sections are
optimized for each single section and each blade. The formula below gives the number of steps
required for a complete fitting run, whatever the amount of reproduction cycles ( Coarse ,
Medium or Fine).
nb(steps) = 2 + nb(primary sections) x nb(blade types)
Processing Speed
The completion time required for a single step is highly dependent on the geometry involved in
the step.
l The first step is very quick because it involves the hub and shroud curves only.
l The second step fits the stacking laws. This is quick if a sweep law is applied, but a full
processing of the sections is required in case of edge traces.
l The next steps involve each section of each blade. For a given blade, the processing time is
equal for all sections. The completion of such a step is usually slightly slower than the two first
steps.
On average, the processing time is therefore proportional to the number of blades, but the use of
edge traces may also significantly slow down the process.
Typically, a coarse fitting on a simple case defined by one blade and 5 sections takes less than a
minute if a sweep law is active.
4.5.3
Fitting Results Check
At the end of the fitting process, the solution can be checked by checking the menu File/Fitting
graphs.
After projection of the target curves on the fitted solution, the comparison graphs show the
remaining differences between the projected target geometry and the fitted model. Overall
improvements should be noticed on all graphs. If not, users should care about the following
potential limitations:
l After a fitting run, some bounds of parameters could have been reached and may prevent good
fitting results as explained in the Visual Check & Parameters Manual Correction.
l If the number of parameters defining a curve is low, the resulting curves will not be able to
give very good results. An increase of the number of parameters will probably improve the
fitted model, but could lead to a significant increase of the complexity (for optimization
purposes).
Additional problems and possible solutions are described in the Fitting Problems section.
4.5.4 Next Fitting Runs
After a first run, the fitted model is shown in the graphical view as the current model. The users
should follow the procedure described below.
1. Open the list of parameters and check the bounds of the free parameters. The range should
be modified when the corresponding parameter appears in yellow color, so that the next fitting
run is able to further improve the value of the parameter. If no bounds are reached in free
parameters, no changes are mandatory, but sometimes, it seems appropriate to reduce some
very wide ranges.
2. If no bounds were enlarged or moved, a finer fitting can be launched: select a coarse or a
medium fitting and click the Ok button. If some bounds were too tight and have been
corrected accordingly, stick with a coarse fitting setting.
The above procedure can be followed several times, until the fitted solution is close enough to the
target geometry. This model can then be used as initial model for database generation or
optimization or simply used as company template in AutoBlade™.
4.6
FITTING PROBLEMS
The fitted solution is globally improved, but some edge radii got
worse
The fitting process is a global optimization, which tries to minimize the error of the shape for
every section. Since the trailing edge is often a small detail when compared to a whole section, the
fitting process may find a set of values for parameters that allow a better error estimate for the
section and for which the quality of the shape is decreased.
Edge radii are usually precisely estimated by the initialization process. Therefore, freezing the
corresponding parameters will ensure a satisfying edge shape (especially the trailing edge).
The initialized model is not very close to the target geometry
l If an error has been generated, this means that some topology settings are probably not suitable
or the amount of defining parameters is insufficient.
l If no error is generated, then the solution monitor should provide some clues about what went
wrong .
The fitting process cannot improve the solution and the value of
parameters do not change any more
If some bounds are reached, moving these bounds should allow further fitting.
If no critical bound is reached, the model may converge to a solution not close enough because
the topology settings are not optimal. Adding some more parameters in the definition of the curves
should help, but could significantly increase the complexity of the model. In such situations,
switching to another camber curve type or construction mode may allow better results .
CHAPTER 5.
EXAMPLE FITTING TARGET GEOMETRY
This section contains two sample target files for the fitting module. As explained in the Preparing
Target Geometry section, support for the geomTurbo format is partial under AutoBlade™.
The axial compressor template in AutoBlade™ is the fitted model of a simplified geometry file
describing the NASA Rotor 37. The two corresponding geomTurbo files below can be used for practise
in a first fitting project of an axial compressor. The first sample is a geomTurbo version 3.7 while the
second is compliant with version 5.3 of the format.
The two target files define exactly the same geometry with hub and shroud in (Z,R) plane as well as
three sections respectively at hub, mid- span and tip. Sections are defined on conical surfaces in
Cartesian coordinates X, Y and Z.
In this section
5.1 GeomTurbo 3.7 Example
5.2 GeomTurbo 5.3 Example
272
293
5.1
GEOMTURBO 3.7 EXAMPLE
The following file complies with geomTurbo 3.7 format and can be used within both AutoGrid™
4 and 5.
GEOMETRY TURBO VERSION 3.7
geometric_tolerance 1E-06
blade_expansion_factor_hub 0.03
blade_expansion_factor_shroud 0.03
blade_merging +0
number_of_blades 36
HUB
ZR
+28
-0.0425 0.17526
-0.0307086 0.17526
-0.0243586 0.175412
-0.0180086 0.175717
-0.0116586 0.176022
-0.0026416 0.177394
0.001016 0.178054
0.007366 0.179578
0.013716 0.181229
0.020066 0.182982
0.0264414 0.184404
0.0327914 0.185674
0.0391414 0.186741
0.045212 0.187681
0.0515366 0.188671
0.0578866 0.189484
0.0642366 0.190297
0.0705866 0.19111
0.0769366 0.19177
0.0832866 0.192354
0.0896366 0.192938
0.0959866 0.193294
0.102337 0.19365
0.108687 0.193904
0.115037 0.194056
0.121387 0.194208
0.126467 0.194335
0.135 0.194335
SHROUD
ZR
+28
-0.0425 0.256692
-0.0312928 0.256565
-0.0249428 0.256388
-0.0185928 0.256083
-0.0122428 0.255626
-0.0058928 0.254864
0.0004572 0.253746
0.0068072 0.252222
0.0131572 0.250495
0.0195072 0.248717
0.0258572 0.246888
0.0322072 0.245161
0.0385572 0.243738
0.0449072 0.242672
0.0512572 0.242062
0.0576072 0.241732
0.0639572 0.241452
0.0703072 0.241097
0.0766572 0.240665
0.0830072 0.240182
0.0893572 0.239827
0.0957072 0.23942
0.102057 0.23876
0.108407 0.238354
0.114757 0.237998
0.121107 0.237642
0.126187 0.23749
0.135 0.237363
SUCTION
SECTIONAL
# section 1
XYZ
+106
0.17669 -0.0208609 0.000351471
0.176689 -0.0208418 0.000335267
0.176689 -0.0208217 0.000321196
0.176689 -0.0208002 0.000308953
0.17669 -0.0207763 0.000298336
0.176691 -0.0207475 0.000289117
0.176697 -0.0206839 0.000281091
0.176706 -0.0206206 0.000289117
0.176711 -0.0205922 0.000298336
0.176716 -0.0205687 0.000308953
0.176721 -0.0205471 0.000321196
0.176726 -0.0205228 0.000335267
0.176733 -0.0204953 0.000351471
0.17674 -0.0204633 0.000370063
0.176748 -0.0204267 0.000391449
0.176758 -0.0203848 0.000415985
0.176769 -0.0203366 0.000444127
0.176781 -0.0202815 0.000476459
0.176796 -0.0202181 0.000513517
0.176812 -0.0201457 0.000555958
0.176831 -0.0200631 0.00060447
0.176853 -0.019969 0.000659739
0.176877 -0.0198621 0.000722525
0.176905 -0.0197415 0.000793617
0.176936 -0.0196056 0.000873903
0.176971 -0.0194527 0.000964298
0.17701 -0.0192817 0.00106579
0.177054 -0.0190908 0.00117948
0.177103 -0.0188783 0.00130655
0.177155 -0.0186552 0.00144058
0.177212 -0.0184092 0.00158921
0.177275 -0.0181384 0.00175377
0.177345 -0.0178413 0.00193573
0.177422 -0.0175159 0.00213666
0.177506 -0.0171605 0.00235832
0.177598 -0.016773 0.00260258
0.177705 -0.0163289 0.00288604
0.177823 -0.0158442 0.00319969
0.177952 -0.0153146 0.00354699
0.178094 -0.0147345 0.00393199
0.178251 -0.0140965 0.00435963
0.178424 -0.0133911 0.00483594
0.178615 -0.0126084 0.00536792
0.178825 -0.0117457 0.00595929
0.179062 -0.0107612 0.00664244
0.179316 -0.00969826 0.00739387
0.179585 -0.0085647 0.00822069
0.179869 -0.00738629 0.00913027
0.18017 -0.00617709 0.0101307
0.180494 -0.00486988 0.0112305
0.180846 -0.00336678 0.0124389
0.181227 -0.00172503 0.0137656
0.181642 -6.61359E-05 0.0152216
0.182088 0.00153746 0.0168217
0.182558 0.00312748 0.0185841
0.183029 0.00477259 0.0205313
0.183445 0.00627275 0.0224897
0.183825 0.00759274 0.0244556
0.184151 0.0087059 0.0262459
0.184444 0.00960719 0.0278742
0.184706 0.010364 0.0293552
0.184939 0.011008 0.0307027
0.185145 0.0115486 0.0319291
0.185325 0.0120016 0.0330455
0.185484 0.0123811 0.0340617
0.185624 0.0126985 0.0349864
0.185748 0.0129647 0.0358278
0.185859 0.0131903 0.0365931
0.185959 0.0133835 0.0372892
0.186044 0.013542 0.0378917
0.186121 0.0136777 0.0384335
0.186189 0.0137936 0.0389184
0.186249 0.0138931 0.0393534
0.186304 0.0139787 0.0397448
0.186353 0.0140526 0.0400976
0.186397 0.0141164 0.0404159
0.186437 0.0141716 0.0407034
0.186472 0.0142172 0.0409509
0.186504 0.0142572 0.0411753
0.186532 0.0142921 0.0413786
0.186558 0.0143228 0.0415626
0.186582 0.0143498 0.0417289
0.186603 0.0143736 0.0418791
0.186622 0.0143946 0.0420144
0.18664 0.0144131 0.0421361
0.186656 0.0144304 0.0422513
0.186671 0.0144455 0.0423542
0.186684 0.0144588 0.0424458
0.186695 0.0144705 0.0425271
0.186706 0.0144808 0.0425992
0.186715 0.0144898 0.0426628
0.186723 0.0144977 0.0427188
0.18673 0.0145044 0.042768
0.186736 0.0145054 0.0428111
0.186743 0.0145001 0.0428487
0.186748 0.0144906 0.0428815
0.186754 0.0144782 0.0429101
0.186759 0.0144635 0.042935
0.186763 0.0144472 0.0429567
0.186768 0.0144296 0.0429756
0.186772 0.0144109 0.0429921
0.186776 0.014391 0.0430064
0.186779 0.0143695 0.0430189
0.186783 0.0143456 0.0430297
0.186786 0.0143166 0.0430392
0.186793 0.0142511 0.0430476
# section 2
XYZ
+102
0.217127 -0.0231681 0.00303258
0.217128 -0.0231547 0.00301933
0.21713 -0.0231404 0.0030078
0.217132 -0.0231247 0.00299778
0.217134 -0.0231074 0.00298909
0.217136 -0.0230861 0.00298156
0.217141 -0.0230388 0.00297498
0.217146 -0.0229917 0.00298156
0.217148 -0.0229704 0.00298909
0.21715 -0.0229528 0.00299778
0.217152 -0.0229354 0.0030078
0.217154 -0.0229154 0.00301933
0.217156 -0.0228924 0.00303258
0.217159 -0.0228659 0.00304783
0.217162 -0.0228354 0.00306532
0.217165 -0.0228007 0.0030854
0.217169 -0.0227605 0.00310845
0.217174 -0.0227146 0.00313489
0.217179 -0.022662 0.00316527
0.217185 -0.0226016 0.00320002
0.217192 -0.0225327 0.00323976
0.217199 -0.0224543 0.00328503
0.217208 -0.0223652 0.00333647
0.217218 -0.0222641 0.00339477
0.217229 -0.0221502 0.00346057
0.217241 -0.022022 0.00353471
0.217255 -0.0218781 0.00361798
0.217271 -0.0217172 0.00371129
0.217289 -0.0215374 0.0038156
0.217307 -0.021348 0.00392571
0.217327 -0.0211382 0.00404787
0.217349 -0.0209063 0.00418319
0.217374 -0.0206503 0.0043329
0.217401 -0.0203681 0.00449835
0.217431 -0.0200576 0.00468094
0.217463 -0.0197164 0.00488234
0.2175 -0.0193216 0.00511623
0.21754 -0.0188862 0.00537524
0.217584 -0.0184058 0.00566229
0.217632 -0.0178749 0.00598079
0.217685 -0.0172871 0.00633486
0.217741 -0.0166341 0.00672957
0.217803 -0.0159073 0.00717072
0.217869 -0.0151029 0.00766143
0.217941 -0.0141796 0.0082285
0.218016 -0.0131724 0.00885233
0.218091 -0.0120731 0.00953855
0.218167 -0.0108711 0.0102934
0.218242 -0.00955873 0.0111238
0.218317 -0.00813882 0.0120372
0.21839 -0.00660734 0.0130419
0.218461 -0.004933 0.0141469
0.218531 -0.00310057 0.0153623
0.218592 -0.00112156 0.0166992
0.218634 0.00100507 0.01817
0.218643 0.00323621 0.0197883
0.218611 0.00530518 0.0214069
0.21855 0.00721804 0.0230256
0.218477 0.00884761 0.0244972
0.218404 0.0102505 0.025835
0.218331 0.0114683 0.0270512
0.218261 0.0125242 0.0281569
0.218193 0.01344 0.029162
0.218127 0.0142372 0.0300757
0.218065 0.0149369 0.0309063
0.218006 0.0155568 0.0316614
0.217951 0.0161082 0.0323478
0.2179 0.0165992 0.0329718
0.217853 0.0170364 0.0335391
0.217813 0.0174069 0.03403
0.217777 0.0177328 0.0344713
0.217744 0.0180183 0.0348661
0.217715 0.0182695 0.0352203
0.21769 0.018492 0.0355389
0.217667 0.0186901 0.0358261
0.217646 0.0188671 0.0360852
0.217628 0.0190257 0.0363191
0.217612 0.0191614 0.0365206
0.217598 0.0192839 0.0367032
0.217585 0.0193943 0.0368687
0.217573 0.019494 0.0370185
0.217563 0.0195838 0.0371539
0.217553 0.0196647 0.0372761
0.217545 0.0197374 0.0373862
0.217537 0.0198026 0.0374853
0.21753 0.0198643 0.0375791
0.217524 0.0199193 0.0376628
0.217518 0.0199682 0.0377374
0.217513 0.0200116 0.0378036
0.217509 0.0200499 0.0378623
0.217505 0.0200838 0.037914
0.217501 0.0201136 0.0379596
0.217499 0.0201321 0.0379997
0.217498 0.0201394 0.0380347
0.217497 0.0201398 0.0380654
0.217497 0.0201358 0.0380921
0.217498 0.0201287 0.0381153
0.217498 0.0201194 0.0381356
0.217499 0.0201085 0.0381533
0.2175 0.0200963 0.0381687
0.217501 0.0200831 0.0381821
0.217502 0.0200688 0.0381938
# section 3
XYZ
+101
0.251068 -0.0250123 0.00642899
0.251071 -0.0250032 0.0064185
0.251075 -0.0249931 0.00640938
0.251078 -0.0249818 0.00640146
0.251081 -0.0249691 0.00639458
0.251084 -0.0249534 0.00638863
0.251089 -0.024918 0.00638343
0.251091 -0.0248824 0.00638863
0.251091 -0.0248664 0.00639458
0.251091 -0.0248518 0.00640146
0.251091 -0.024835 0.00640938
0.25109 -0.0248157 0.0064185
0.25109 -0.0247935 0.00642899
0.251089 -0.024768 0.00644106
0.251088 -0.0247387 0.00645487
0.251087 -0.0247051 0.00647077
0.251086 -0.0246665 0.00648901
0.251085 -0.0246222 0.00650991
0.251084 -0.0245715 0.00653394
0.251082 -0.0245134 0.00656142
0.251081 -0.024447 0.00659284
0.251078 -0.0243714 0.00662865
0.251076 -0.0242856 0.00666932
0.251073 -0.0241885 0.00671539
0.25107 -0.0240789 0.00676743
0.251067 -0.0239556 0.00682603
0.251062 -0.0238174 0.00689184
0.251058 -0.0236627 0.00696557
0.251052 -0.0234903 0.00704804
0.251046 -0.0233086 0.00713503
0.251039 -0.0231077 0.00723155
0.251031 -0.0228858 0.00733848
0.251021 -0.0226413 0.00745676
0.251011 -0.0223724 0.00758744
0.250998 -0.0220769 0.00773168
0.250984 -0.0217526 0.0078907
0.250967 -0.0213778 0.00807538
0.250947 -0.0209644 0.00827987
0.250924 -0.0205076 0.00850645
0.250897 -0.020001 0.0087578
0.250865 -0.019437 0.00903716
0.250829 -0.0188064 0.00934853
0.250786 -0.0180988 0.00969644
0.250736 -0.017309 0.0100834
0.250674 -0.0163931 0.0105304
0.250603 -0.0153838 0.011022
0.250519 -0.0142764 0.0115627
0.250421 -0.0130649 0.0121573
0.250305 -0.0117371 0.0128113
0.25017 -0.0102766 0.0135307
0.250011 -0.00867329 0.0143219
0.249824 -0.00692007 0.0151922
0.249603 -0.00500169 0.0161493
0.249342 -0.00287863 0.0172017
0.249032 -0.000511463 0.0183589
0.248663 0.00199586 0.019631
0.248266 0.00448552 0.0209022
0.247834 0.00725954 0.0221728
0.24743 0.00934753 0.0233276
0.247053 0.0111107 0.0243776
0.246703 0.0126726 0.0253325
0.246382 0.0140067 0.0262008
0.246088 0.0151793 0.0269907
0.245819 0.0162116 0.0277093
0.245576 0.0170985 0.0283629
0.245357 0.017861 0.0289576
0.24516 0.018529 0.0294987
0.244981 0.0191217 0.029991
0.24482 0.0196488 0.0304389
0.244681 0.0200948 0.0308267
0.244557 0.0204871 0.0311756
0.244447 0.0208312 0.0314879
0.244349 0.0211346 0.0317683
0.244262 0.0214037 0.0320206
0.244183 0.0216433 0.0322481
0.244112 0.0218572 0.0324535
0.244049 0.0220488 0.032639
0.243995 0.0222126 0.0327988
0.243946 0.0223602 0.0329438
0.243901 0.0224933 0.0330751
0.243861 0.0226131 0.033194
0.243825 0.0227211 0.0333015
0.243792 0.0228182 0.0333986
0.243763 0.0229055 0.033486
0.243737 0.0229838 0.0335648
0.243712 0.0230577 0.0336393
0.24369 0.0231236 0.0337059
0.24367 0.0231822 0.0337651
0.243653 0.0232341 0.0338177
0.243637 0.02328 0.0338644
0.243624 0.0233206 0.0339055
0.243612 0.0233555 0.0339418
0.243602 0.0233746 0.0339736
0.243595 0.0233824 0.0340015
0.243589 0.0233839 0.0340258
0.243584 0.0233814 0.0340471
0.24358 0.0233762 0.0340656
0.243577 0.0233691 0.0340817
0.243575 0.0233606 0.0340958
0.243573 0.0233511 0.034108
0.243571 0.0233406 0.0341187
PRESSURE
SECTIONAL
# section 1
XYZ
+94
0.17669 -0.0208609 0.000351471
0.176691 -0.0208788 0.000370063
0.176693 -0.0208955 0.000391449
0.176696 -0.0209107 0.000415985
0.1767 -0.0209239 0.000444127
0.176705 -0.0209342 0.000476459
0.176712 -0.0209405 0.000513517
0.17672 -0.0209406 0.000555958
0.17673 -0.0209316 0.00060447
0.176744 -0.0209076 0.000659739
0.176763 -0.0208557 0.000722525
0.176785 -0.0207848 0.000793617
0.17681 -0.0207048 0.000873903
0.176839 -0.0206148 0.000964298
0.176871 -0.0205139 0.00106579
0.176908 -0.0204007 0.00117948
0.176949 -0.0202743 0.00130655
0.176992 -0.0201412 0.00144058
0.17704 -0.0199936 0.00158921
0.177094 -0.0198303 0.00175377
0.177154 -0.01965 0.00193573
0.17722 -0.019451 0.00213666
0.177293 -0.019232 0.00235832
0.177375 -0.0189909 0.00260258
0.17747 -0.0187116 0.00288604
0.177576 -0.018403 0.00319969
0.177694 -0.0180618 0.00354699
0.177825 -0.0176839 0.00393199
0.177972 -0.0172643 0.00435963
0.178136 -0.0167966 0.00483594
0.178319 -0.0162734 0.00536792
0.178522 -0.0156898 0.00595929
0.178756 -0.0150119 0.00664244
0.179011 -0.0142601 0.00739387
0.179287 -0.0134251 0.00822069
0.179586 -0.0124979 0.00913027
0.179911 -0.0114742 0.0101307
0.180262 -0.0103699 0.0112305
0.180643 -0.00920084 0.0124389
0.181063 -0.00789994 0.0137656
0.181529 -0.00639667 0.0152216
0.182033 -0.00472947 0.0168217
0.18256 -0.00298793 0.0185841
0.183087 -0.00118232 0.0205313
0.183552 0.000569893 0.0224897
0.183968 0.00223894 0.0244556
0.184319 0.0036897 0.0262459
0.184627 0.00494096 0.0278742
0.184899 0.00601565 0.0293552
0.185136 0.00695767 0.0307027
0.185341 0.00779946 0.0319291
0.185517 0.00854382 0.0330455
0.185669 0.00919753 0.0340617
0.185801 0.00977275 0.0349864
0.185916 0.0102805 0.0358278
0.186018 0.0107304 0.0365931
0.186108 0.0111305 0.0372892
0.186184 0.0114699 0.0378917
0.186251 0.0117696 0.0384335
0.186311 0.0120332 0.0389184
0.186363 0.0122659 0.0393534
0.186411 0.012472 0.0397448
0.186453 0.0126551 0.0400976
0.186491 0.012818 0.0404159
0.186525 0.0129631 0.0407034
0.186555 0.0130865 0.0409509
0.186582 0.0131972 0.0411753
0.186606 0.0132966 0.0413786
0.186628 0.0133858 0.0415626
0.186648 0.0134658 0.0417289
0.186666 0.0135375 0.0418791
0.186682 0.0136018 0.0420144
0.186696 0.0136594 0.0421361
0.18671 0.0137137 0.0422513
0.186722 0.0137619 0.0423542
0.186733 0.0138048 0.0424458
0.186743 0.0138428 0.0425271
0.186752 0.0138763 0.0425992
0.186759 0.0139059 0.0426628
0.186766 0.0139318 0.0427188
0.186772 0.0139546 0.042768
0.186777 0.0139745 0.0428111
0.186781 0.013992 0.0428487
0.186785 0.0140071 0.0428815
0.186789 0.0140209 0.0429101
0.186791 0.0140361 0.042935
0.186794 0.0140529 0.0429567
0.186795 0.0140709 0.0429756
0.186796 0.0140901 0.0429921
0.186797 0.0141103 0.0430064
0.186797 0.0141321 0.0430189
0.186797 0.0141562 0.0430297
0.186796 0.0141855 0.0430392
0.186793 0.0142511 0.0430476
# section 2
XYZ
+98
0.217127 -0.0231681 0.00303258
0.217125 -0.0231803 0.00304783
0.217124 -0.0231913 0.00306532
0.217123 -0.0232009 0.0030854
0.217122 -0.0232082 0.00310845
0.217121 -0.0232125 0.00313489
0.217121 -0.0232125 0.00316527
0.217121 -0.0232059 0.00320002
0.217123 -0.0231888 0.00323976
0.217126 -0.0231503 0.00328503
0.217133 -0.0230862 0.00333647
0.21714 -0.0230134 0.00339477
0.217148 -0.022931 0.00346057
0.217157 -0.022838 0.00353471
0.217168 -0.0227337 0.00361798
0.217179 -0.0226166 0.00371129
0.217192 -0.0224854 0.0038156
0.217206 -0.0223466 0.00392571
0.217222 -0.0221925 0.00404787
0.217239 -0.0220214 0.00418319
0.217259 -0.0218315 0.0043329
0.21728 -0.0216212 0.00449835
0.217304 -0.0213882 0.00468094
0.21733 -0.0211304 0.00488234
0.21736 -0.02083 0.00511623
0.217394 -0.0204962 0.00537524
0.217432 -0.0201254 0.00566229
0.217473 -0.0197138 0.00598079
0.217519 -0.019257 0.00633486
0.217569 -0.0187499 0.00672957
0.217625 -0.0181856 0.00717072
0.217685 -0.017559 0.00766143
0.217752 -0.0168328 0.0082285
0.217824 -0.0160287 0.00885233
0.2179 -0.0151392 0.00953855
0.217978 -0.0141596 0.0102934
0.21806 -0.0130814 0.0111238
0.218145 -0.0118857 0.0120372
0.218234 -0.0105593 0.0130419
0.218327 -0.0091119 0.0141469
0.218423 -0.00752169 0.0153623
0.218519 -0.00574169 0.0166992
0.218603 -0.00379413 0.01817
0.21866 -0.00166115 0.0197883
0.218675 0.00048992 0.0214069
0.218653 0.00260323 0.0230256
0.218611 0.00445339 0.0244972
0.218559 0.00610324 0.025835
0.2185 0.00758562 0.0270512
0.218438 0.00889941 0.0281569
0.218374 0.0100659 0.029162
0.218309 0.0111166 0.0300757
0.218243 0.0120647 0.0309063
0.218178 0.0129181 0.0316614
0.218117 0.0136848 0.0323478
0.218058 0.0143722 0.0329718
0.218004 0.0149886 0.0335391
0.217956 0.0155155 0.03403
0.217912 0.0159844 0.0344713
0.217872 0.0164004 0.0348661
0.217836 0.0167711 0.0352203
0.217803 0.0171032 0.0355389
0.217774 0.0174016 0.0358261
0.217747 0.0176705 0.0360852
0.217722 0.0179132 0.0363191
0.217701 0.0181223 0.0365206
0.217682 0.0183118 0.0367032
0.217664 0.0184836 0.0368687
0.217648 0.0186392 0.0370185
0.217634 0.0187799 0.0371539
0.217621 0.0189069 0.0372761
0.217609 0.0190214 0.0373862
0.217598 0.0191244 0.0374853
0.217588 0.019222 0.0375791
0.217579 0.0193091 0.0376628
0.217571 0.0193867 0.0377374
0.217564 0.0194556 0.0378036
0.217557 0.0195167 0.0378623
0.217552 0.0195705 0.037914
0.217547 0.019618 0.0379596
0.217542 0.0196597 0.0379997
0.217538 0.0196962 0.0380347
0.217535 0.0197281 0.0380654
0.217532 0.0197559 0.0380921
0.21753 0.0197801 0.0381153
0.217527 0.0198012 0.0381356
0.217525 0.0198196 0.0381533
0.217524 0.0198357 0.0381687
0.217522 0.0198498 0.0381821
0.217521 0.019864 0.0381938
0.217519 0.0198796 0.0382039
0.217518 0.019897 0.0382127
0.217516 0.0199183 0.0382205
0.217511 0.0199664 0.0382273
0.217507 0.0200146 0.0382205
0.217505 0.0200358 0.0382127
0.217503 0.0200533 0.0382039
0.217502 0.0200688 0.0381938
# section 3
XYZ
+99
0.251068 -0.0250123 0.00642899
0.251064 -0.0250204 0.00644106
0.25106 -0.0250273 0.00645487
0.251055 -0.0250325 0.00647077
0.25105 -0.0250354 0.00648901
0.251044 -0.0250351 0.00650991
0.251039 -0.02503 0.00653394
0.251033 -0.0250168 0.00656142
0.251027 -0.0249876 0.00659284
0.251024 -0.0249273 0.00662865
0.25102 -0.0248566 0.00666932
0.251016 -0.0247766 0.00671539
0.251011 -0.0246862 0.00676743
0.251006 -0.0245844 0.00682603
0.251 -0.02447 0.00689184
0.250993 -0.0243419 0.00696557
0.250985 -0.0241987 0.00704804
0.250976 -0.0240475 0.00713503
0.250967 -0.0238797 0.00723155
0.250956 -0.0236939 0.00733848
0.250944 -0.0234884 0.00745676
0.25093 -0.0232613 0.00758744
0.250915 -0.0230106 0.00773168
0.250897 -0.0227341 0.0078907
0.250877 -0.0224127 0.00807538
0.250853 -0.0220564 0.00827987
0.250827 -0.0216606 0.00850645
0.250796 -0.0212198 0.0087578
0.250762 -0.0207276 0.00903716
0.250722 -0.0201762 0.00934853
0.250676 -0.0195583 0.00969644
0.250623 -0.018872 0.0100834
0.250558 -0.0180832 0.0105304
0.250484 -0.0172167 0.011022
0.250399 -0.0162526 0.0115627
0.250302 -0.0151755 0.0121573
0.250189 -0.0139956 0.0128113
0.250058 -0.0127184 0.0135307
0.249907 -0.0112921 0.0143219
0.249732 -0.00968576 0.0151922
0.249527 -0.0079398 0.0161493
0.249286 -0.00599318 0.0172017
0.249003 -0.00381508 0.0183589
0.248667 -0.00141637 0.019631
0.248305 0.000973856 0.0209022
0.247918 0.0033137 0.0221728
0.247544 0.00554123 0.0233276
0.247186 0.00761649 0.0243776
0.24685 0.00937261 0.0253325
0.246542 0.0108178 0.0262008
0.246255 0.0121657 0.0269907
0.245987 0.0134319 0.0277093
0.24574 0.0145632 0.0283629
0.245514 0.0155557 0.0289576
0.24531 0.0164269 0.0294987
0.245124 0.0171942 0.029991
0.244956 0.0178748 0.0304389
0.24481 0.0184539 0.0308267
0.24468 0.0189687 0.0311756
0.244563 0.0194255 0.0314879
0.244458 0.0198325 0.0317683
0.244364 0.0201964 0.0320206
0.24428 0.0205228 0.0322481
0.244203 0.020816 0.0324535
0.244135 0.0210798 0.032639
0.244076 0.0213062 0.0327988
0.244022 0.0215111 0.0329438
0.243973 0.0216963 0.0330751
0.243929 0.0218636 0.033194
0.24389 0.0220145 0.0333015
0.243854 0.0221506 0.0333986
0.243822 0.0222731 0.033486
0.243793 0.0223832 0.0335648
0.243765 0.0224874 0.0336393
0.243741 0.0225803 0.0337059
0.243719 0.0226629 0.0337651
0.2437 0.0227363 0.0338177
0.243682 0.0228012 0.0338644
0.243667 0.0228585 0.0339055
0.243654 0.022909 0.0339418
0.243642 0.0229533 0.0339736
0.243632 0.0229921 0.0340015
0.243623 0.0230259 0.0340258
0.243615 0.0230555 0.0340471
0.243609 0.0230812 0.0340656
0.243603 0.0231036 0.0340817
0.243597 0.0231231 0.0340958
0.243593 0.0231402 0.034108
0.243589 0.023155 0.0341187
0.243586 0.0231679 0.034128
0.243583 0.0231799 0.034136
0.24358 0.0231934 0.0341431
0.243577 0.02321 0.0341492
0.243572 0.023248 0.0341546
0.243569 0.0232861 0.0341492
0.243569 0.0233031 0.0341431
0.243569 0.0233169 0.034136
0.24357 0.0233293 0.034128
0.243571 0.0233406 0.0341187
5.2
GEOMTURBO 5.3 EXAMPLE
The following file complies with geomTurbo 5.3 format and can be used within AutoGrid™ 5.
GEOMETRY TURBO
VERSION 5.3
TOLERANCE 1E-06
NI_BEGIN CHANNEL
NI_BEGIN basic_curve
NAME hub
DISCRETISATION 10
NI_BEGIN zrcurve
ZR
+28
-0.0425 0.17526
-0.0307086 0.17526
-0.0243586 0.175412
-0.0180086 0.175717
-0.0116586 0.176022
-0.0026416 0.177394
0.001016 0.178054
0.007366 0.179578
0.013716 0.181229
0.020066 0.182982
0.0264414 0.184404
0.0327914 0.185674
0.0391414 0.186741
0.045212 0.187681
0.0515366 0.188671
0.0578866 0.189484
0.0642366 0.190297
0.0705866 0.19111
0.0769366 0.19177
0.0832866 0.192354
0.0896366 0.192938
0.0959866 0.193294
0.102337 0.19365
0.108687 0.193904
0.115037 0.194056
0.121387 0.194208
0.126467 0.194335
0.135 0.194335
NI_END zrcurve
NI_END basic_curve
NI_BEGIN basic_curve
NAME shroud
DISCRETISATION 10
NI_BEGIN zrcurve
ZR
+28
-0.0425 0.256692
-0.0312928 0.256565
-0.0249428 0.256388
-0.0185928 0.256083
-0.0122428 0.255626
-0.0058928 0.254864
0.0004572 0.253746
0.0068072 0.252222
0.0131572 0.250495
0.0195072 0.248717
0.0258572 0.246888
0.0322072 0.245161
0.0385572 0.243738
0.0449072 0.242672
0.0512572 0.242062
0.0576072 0.241732
0.0639572 0.241452
0.0703072 0.241097
0.0766572 0.240665
0.0830072 0.240182
0.0893572 0.239827
0.0957072 0.23942
0.102057 0.23876
0.108407 0.238354
0.114757 0.237998
0.121107 0.237642
0.126187 0.23749
0.135 0.237363
NI_END zrcurve
NI_END basic_curve
NI_BEGIN channel_curve hub
NAME hub
VERTEX hub 0
VERTEX hub 1
NI_END channel_curve hub
NI_BEGIN channel_curve shroud
NAME shroud
VERTEX shroud 0
VERTEX shroud 1
NI_END channel_curve shroud
NI_END CHANNEL
NI_BEGIN NIROW
NAME row 1
TYPE normal
PERIODICITY 36
NI_BEGIN NIBLADE
NAME Main Blade
NI_BEGIN NIBLADEGEOMETRY
TYPE GEOMTURBO
GEOMETRY_MODIFIED 0
GEOMETRY TURBO VERSION 5
blade_expansion_factor_hub 0.03
blade_expansion_factor_shroud 0.03
intersection_npts 10
intersection_control 0
number_of_blades 36
suction
SECTIONAL
# section 1
XYZ
+106
0.17669 -0.0208609 0.000351471
0.176689 -0.0208418 0.000335267
0.176689 -0.0208217 0.000321196
0.176689 -0.0208002 0.000308953
0.17669 -0.0207763 0.000298336
0.176691 -0.0207475 0.000289117
0.176697 -0.0206839 0.000281091
0.176706 -0.0206206 0.000289117
0.176711 -0.0205922 0.000298336
0.176716 -0.0205687 0.000308953
0.176721 -0.0205471 0.000321196
0.176726 -0.0205228 0.000335267
0.176733 -0.0204953 0.000351471
0.17674 -0.0204633 0.000370063
0.176748 -0.0204267 0.000391449
0.176758 -0.0203848 0.000415985
0.176769 -0.0203366 0.000444127
0.176781 -0.0202815 0.000476459
0.176796 -0.0202181 0.000513517
0.176812 -0.0201457 0.000555958
0.176831 -0.0200631 0.00060447
0.176853 -0.019969 0.000659739
0.176877 -0.0198621 0.000722525
0.176905 -0.0197415 0.000793617
0.176936 -0.0196056 0.000873903
0.176971 -0.0194527 0.000964298
0.17701 -0.0192817 0.00106579
0.177054 -0.0190908 0.00117948
0.177103 -0.0188783 0.00130655
0.177155 -0.0186552 0.00144058
0.177212 -0.0184092 0.00158921
0.177275 -0.0181384 0.00175377
0.177345 -0.0178413 0.00193573
0.177422 -0.0175159 0.00213666
0.177506 -0.0171605 0.00235832
0.177598 -0.016773 0.00260258
0.177705 -0.0163289 0.00288604
0.177823 -0.0158442 0.00319969
0.177952 -0.0153146 0.00354699
0.178094 -0.0147345 0.00393199
0.178251 -0.0140965 0.00435963
0.178424 -0.0133911 0.00483594
0.178615 -0.0126084 0.00536792
0.178825 -0.0117457 0.00595929
0.179062 -0.0107612 0.00664244
0.179316 -0.00969826 0.00739387
0.179585 -0.0085647 0.00822069
0.179869 -0.00738629 0.00913027
0.18017 -0.00617709 0.0101307
0.180494 -0.00486988 0.0112305
0.180846 -0.00336678 0.0124389
0.181227 -0.00172503 0.0137656
0.181642 -6.61359E-05 0.0152216
0.182088 0.00153746 0.0168217
0.182558 0.00312748 0.0185841
0.183029 0.00477259 0.0205313
0.183445 0.00627275 0.0224897
0.183825 0.00759274 0.0244556
0.184151 0.0087059 0.0262459
0.184444 0.00960719 0.0278742
0.184706 0.010364 0.0293552
0.184939 0.011008 0.0307027
0.185145 0.0115486 0.0319291
0.185325 0.0120016 0.0330455
0.185484 0.0123811 0.0340617
0.185624 0.0126985 0.0349864
0.185748 0.0129647 0.0358278
0.185859 0.0131903 0.0365931
0.185959 0.0133835 0.0372892
0.186044 0.013542 0.0378917
0.186121 0.0136777 0.0384335
0.186189 0.0137936 0.0389184
0.186249 0.0138931 0.0393534
0.186304 0.0139787 0.0397448
0.186353 0.0140526 0.0400976
0.186397 0.0141164 0.0404159
0.186437 0.0141716 0.0407034
0.186472 0.0142172 0.0409509
0.186504 0.0142572 0.0411753
0.186532 0.0142921 0.0413786
0.186558 0.0143228 0.0415626
0.186582 0.0143498 0.0417289
0.186603 0.0143736 0.0418791
0.186622 0.0143946 0.0420144
0.18664 0.0144131 0.0421361
0.186656 0.0144304 0.0422513
0.186671 0.0144455 0.0423542
0.186684 0.0144588 0.0424458
0.186695 0.0144705 0.0425271
0.186706 0.0144808 0.0425992
0.186715 0.0144898 0.0426628
0.186723 0.0144977 0.0427188
0.18673 0.0145044 0.042768
0.186736 0.0145054 0.0428111
0.186743 0.0145001 0.0428487
0.186748 0.0144906 0.0428815
0.186754 0.0144782 0.0429101
0.186759 0.0144635 0.042935
0.186763 0.0144472 0.0429567
0.186768 0.0144296 0.0429756
0.186772 0.0144109 0.0429921
0.186776 0.014391 0.0430064
0.186779 0.0143695 0.0430189
0.186783 0.0143456 0.0430297
0.186786 0.0143166 0.0430392
0.186793 0.0142511 0.0430476
# section 2
XYZ
+102
0.217127 -0.0231681 0.00303258
0.217128 -0.0231547 0.00301933
0.21713 -0.0231404 0.0030078
0.217132 -0.0231247 0.00299778
0.217134 -0.0231074 0.00298909
0.217136 -0.0230861 0.00298156
0.217141 -0.0230388 0.00297498
0.217146 -0.0229917 0.00298156
0.217148 -0.0229704 0.00298909
0.21715 -0.0229528 0.00299778
0.217152 -0.0229354 0.0030078
0.217154 -0.0229154 0.00301933
0.217156 -0.0228924 0.00303258
0.217159 -0.0228659 0.00304783
0.217162 -0.0228354 0.00306532
0.217165 -0.0228007 0.0030854
0.217169 -0.0227605 0.00310845
0.217174 -0.0227146 0.00313489
0.217179 -0.022662 0.00316527
0.217185 -0.0226016 0.00320002
0.217192 -0.0225327 0.00323976
0.217199 -0.0224543 0.00328503
0.217208 -0.0223652 0.00333647
0.217218 -0.0222641 0.00339477
0.217229 -0.0221502 0.00346057
0.217241 -0.022022 0.00353471
0.217255 -0.0218781 0.00361798
0.217271 -0.0217172 0.00371129
0.217289 -0.0215374 0.0038156
0.217307 -0.021348 0.00392571
0.217327 -0.0211382 0.00404787
0.217349 -0.0209063 0.00418319
0.217374 -0.0206503 0.0043329
0.217401 -0.0203681 0.00449835
0.217431 -0.0200576 0.00468094
0.217463 -0.0197164 0.00488234
0.2175 -0.0193216 0.00511623
0.21754 -0.0188862 0.00537524
0.217584 -0.0184058 0.00566229
0.217632 -0.0178749 0.00598079
0.217685 -0.0172871 0.00633486
0.217741 -0.0166341 0.00672957
0.217803 -0.0159073 0.00717072
0.217869 -0.0151029 0.00766143
0.217941 -0.0141796 0.0082285
0.218016 -0.0131724 0.00885233
0.218091 -0.0120731 0.00953855
0.218167 -0.0108711 0.0102934
0.218242 -0.00955873 0.0111238
0.218317 -0.00813882 0.0120372
0.21839 -0.00660734 0.0130419
0.218461 -0.004933 0.0141469
0.218531 -0.00310057 0.0153623
0.218592 -0.00112156 0.0166992
0.218634 0.00100507 0.01817
0.218643 0.00323621 0.0197883
0.218611 0.00530518 0.0214069
0.21855 0.00721804 0.0230256
0.218477 0.00884761 0.0244972
0.218404 0.0102505 0.025835
0.218331 0.0114683 0.0270512
0.218261 0.0125242 0.0281569
0.218193 0.01344 0.029162
0.218127 0.0142372 0.0300757
0.218065 0.0149369 0.0309063
0.218006 0.0155568 0.0316614
0.217951 0.0161082 0.0323478
0.2179 0.0165992 0.0329718
0.217853 0.0170364 0.0335391
0.217813 0.0174069 0.03403
0.217777 0.0177328 0.0344713
0.217744 0.0180183 0.0348661
0.217715 0.0182695 0.0352203
0.21769 0.018492 0.0355389
0.217667 0.0186901 0.0358261
0.217646 0.0188671 0.0360852
0.217628 0.0190257 0.0363191
0.217612 0.0191614 0.0365206
0.217598 0.0192839 0.0367032
0.217585 0.0193943 0.0368687
0.217573 0.019494 0.0370185
0.217563 0.0195838 0.0371539
0.217553 0.0196647 0.0372761
0.217545 0.0197374 0.0373862
0.217537 0.0198026 0.0374853
0.21753 0.0198643 0.0375791
0.217524 0.0199193 0.0376628
0.217518 0.0199682 0.0377374
0.217513 0.0200116 0.0378036
0.217509 0.0200499 0.0378623
0.217505 0.0200838 0.037914
0.217501 0.0201136 0.0379596
0.217499 0.0201321 0.0379997
0.217498 0.0201394 0.0380347
0.217497 0.0201398 0.0380654
0.217497 0.0201358 0.0380921
0.217498 0.0201287 0.0381153
0.217498 0.0201194 0.0381356
0.217499 0.0201085 0.0381533
0.2175 0.0200963 0.0381687
0.217501 0.0200831 0.0381821
0.217502 0.0200688 0.0381938
# section 3
XYZ
+101
0.251068 -0.0250123 0.00642899
0.251071 -0.0250032 0.0064185
0.251075 -0.0249931 0.00640938
0.251078 -0.0249818 0.00640146
0.251081 -0.0249691 0.00639458
0.251084 -0.0249534 0.00638863
0.251089 -0.024918 0.00638343
0.251091 -0.0248824 0.00638863
0.251091 -0.0248664 0.00639458
0.251091 -0.0248518 0.00640146
0.251091 -0.024835 0.00640938
0.25109 -0.0248157 0.0064185
0.25109 -0.0247935 0.00642899
0.251089 -0.024768 0.00644106
0.251088 -0.0247387 0.00645487
0.251087 -0.0247051 0.00647077
0.251086 -0.0246665 0.00648901
0.251085 -0.0246222 0.00650991
0.251084 -0.0245715 0.00653394
0.251082 -0.0245134 0.00656142
0.251081 -0.024447 0.00659284
0.251078 -0.0243714 0.00662865
0.251076 -0.0242856 0.00666932
0.251073 -0.0241885 0.00671539
0.25107 -0.0240789 0.00676743
0.251067 -0.0239556 0.00682603
0.251062 -0.0238174 0.00689184
0.251058 -0.0236627 0.00696557
0.251052 -0.0234903 0.00704804
0.251046 -0.0233086 0.00713503
0.251039 -0.0231077 0.00723155
0.251031 -0.0228858 0.00733848
0.251021 -0.0226413 0.00745676
0.251011 -0.0223724 0.00758744
0.250998 -0.0220769 0.00773168
0.250984 -0.0217526 0.0078907
0.250967 -0.0213778 0.00807538
0.250947 -0.0209644 0.00827987
0.250924 -0.0205076 0.00850645
0.250897 -0.020001 0.0087578
0.250865 -0.019437 0.00903716
0.250829 -0.0188064 0.00934853
0.250786 -0.0180988 0.00969644
0.250736 -0.017309 0.0100834
0.250674 -0.0163931 0.0105304
0.250603 -0.0153838 0.011022
0.250519 -0.0142764 0.0115627
0.250421 -0.0130649 0.0121573
0.250305 -0.0117371 0.0128113
0.25017 -0.0102766 0.0135307
0.250011 -0.00867329 0.0143219
0.249824 -0.00692007 0.0151922
0.249603 -0.00500169 0.0161493
0.249342 -0.00287863 0.0172017
0.249032 -0.000511463 0.0183589
0.248663 0.00199586 0.019631
0.248266 0.00448552 0.0209022
0.247834 0.00725954 0.0221728
0.24743 0.00934753 0.0233276
0.247053 0.0111107 0.0243776
0.246703 0.0126726 0.0253325
0.246382 0.0140067 0.0262008
0.246088 0.0151793 0.0269907
0.245819 0.0162116 0.0277093
0.245576 0.0170985 0.0283629
0.245357 0.017861 0.0289576
0.24516 0.018529 0.0294987
0.244981 0.0191217 0.029991
0.24482 0.0196488 0.0304389
0.244681 0.0200948 0.0308267
0.244557 0.0204871 0.0311756
0.244447 0.0208312 0.0314879
0.244349 0.0211346 0.0317683
0.244262 0.0214037 0.0320206
0.244183 0.0216433 0.0322481
0.244112 0.0218572 0.0324535
0.244049 0.0220488 0.032639
0.243995 0.0222126 0.0327988
0.243946 0.0223602 0.0329438
0.243901 0.0224933 0.0330751
0.243861 0.0226131 0.033194
0.243825 0.0227211 0.0333015
0.243792 0.0228182 0.0333986
0.243763 0.0229055 0.033486
0.243737 0.0229838 0.0335648
0.243712 0.0230577 0.0336393
0.24369 0.0231236 0.0337059
0.24367 0.0231822 0.0337651
0.243653 0.0232341 0.0338177
0.243637 0.02328 0.0338644
0.243624 0.0233206 0.0339055
0.243612 0.0233555 0.0339418
0.243602 0.0233746 0.0339736
0.243595 0.0233824 0.0340015
0.243589 0.0233839 0.0340258
0.243584 0.0233814 0.0340471
0.24358 0.0233762 0.0340656
0.243577 0.0233691 0.0340817
0.243575 0.0233606 0.0340958
0.243573 0.0233511 0.034108
0.243571 0.0233406 0.0341187
pressure
SECTIONAL
# section 1
XYZ
+94
0.17669 -0.0208609 0.000351471
0.176691 -0.0208788 0.000370063
0.176693 -0.0208955 0.000391449
0.176696 -0.0209107 0.000415985
0.1767 -0.0209239 0.000444127
0.176705 -0.0209342 0.000476459
0.176712 -0.0209405 0.000513517
0.17672 -0.0209406 0.000555958
0.17673 -0.0209316 0.00060447
0.176744 -0.0209076 0.000659739
0.176763 -0.0208557 0.000722525
0.176785 -0.0207848 0.000793617
0.17681 -0.0207048 0.000873903
0.176839 -0.0206148 0.000964298
0.176871 -0.0205139 0.00106579
0.176908 -0.0204007 0.00117948
0.176949 -0.0202743 0.00130655
0.176992 -0.0201412 0.00144058
0.17704 -0.0199936 0.00158921
0.177094 -0.0198303 0.00175377
0.177154 -0.01965 0.00193573
0.17722 -0.019451 0.00213666
0.177293 -0.019232 0.00235832
0.177375 -0.0189909 0.00260258
0.17747 -0.0187116 0.00288604
0.177576 -0.018403 0.00319969
0.177694 -0.0180618 0.00354699
0.177825 -0.0176839 0.00393199
0.177972 -0.0172643 0.00435963
0.178136 -0.0167966 0.00483594
0.178319 -0.0162734 0.00536792
0.178522 -0.0156898 0.00595929
0.178756 -0.0150119 0.00664244
0.179011 -0.0142601 0.00739387
0.179287 -0.0134251 0.00822069
0.179586 -0.0124979 0.00913027
0.179911 -0.0114742 0.0101307
0.180262 -0.0103699 0.0112305
0.180643 -0.00920084 0.0124389
0.181063 -0.00789994 0.0137656
0.181529 -0.00639667 0.0152216
0.182033 -0.00472947 0.0168217
0.18256 -0.00298793 0.0185841
0.183087 -0.00118232 0.0205313
0.183552 0.000569893 0.0224897
0.183968 0.00223894 0.0244556
0.184319 0.0036897 0.0262459
0.184627 0.00494096 0.0278742
0.184899 0.00601565 0.0293552
0.185136 0.00695767 0.0307027
0.185341 0.00779946 0.0319291
0.185517 0.00854382 0.0330455
0.185669 0.00919753 0.0340617
0.185801 0.00977275 0.0349864
0.185916 0.0102805 0.0358278
0.186018 0.0107304 0.0365931
0.186108 0.0111305 0.0372892
0.186184 0.0114699 0.0378917
0.186251 0.0117696 0.0384335
0.186311 0.0120332 0.0389184
0.186363 0.0122659 0.0393534
0.186411 0.012472 0.0397448
0.186453 0.0126551 0.0400976
0.186491 0.012818 0.0404159
0.186525 0.0129631 0.0407034
0.186555 0.0130865 0.0409509
0.186582 0.0131972 0.0411753
0.186606 0.0132966 0.0413786
0.186628 0.0133858 0.0415626
0.186648 0.0134658 0.0417289
0.186666 0.0135375 0.0418791
0.186682 0.0136018 0.0420144
0.186696 0.0136594 0.0421361
0.18671 0.0137137 0.0422513
0.186722 0.0137619 0.0423542
0.186733 0.0138048 0.0424458
0.186743 0.0138428 0.0425271
0.186752 0.0138763 0.0425992
0.186759 0.0139059 0.0426628
0.186766 0.0139318 0.0427188
0.186772 0.0139546 0.042768
0.186777 0.0139745 0.0428111
0.186781 0.013992 0.0428487
0.186785 0.0140071 0.0428815
0.186789 0.0140209 0.0429101
0.186791 0.0140361 0.042935
0.186794 0.0140529 0.0429567
0.186795 0.0140709 0.0429756
0.186796 0.0140901 0.0429921
0.186797 0.0141103 0.0430064
0.186797 0.0141321 0.0430189
0.186797 0.0141562 0.0430297
0.186796 0.0141855 0.0430392
0.186793 0.0142511 0.0430476
# section 2
XYZ
+98
0.217127 -0.0231681 0.00303258
0.217125 -0.0231803 0.00304783
0.217124 -0.0231913 0.00306532
0.217123 -0.0232009 0.0030854
0.217122 -0.0232082 0.00310845
0.217121 -0.0232125 0.00313489
0.217121 -0.0232125 0.00316527
0.217121 -0.0232059 0.00320002
0.217123 -0.0231888 0.00323976
0.217126 -0.0231503 0.00328503
0.217133 -0.0230862 0.00333647
0.21714 -0.0230134 0.00339477
0.217148 -0.022931 0.00346057
0.217157 -0.022838 0.00353471
0.217168 -0.0227337 0.00361798
0.217179 -0.0226166 0.00371129
0.217192 -0.0224854 0.0038156
0.217206 -0.0223466 0.00392571
0.217222 -0.0221925 0.00404787
0.217239 -0.0220214 0.00418319
0.217259 -0.0218315 0.0043329
0.21728 -0.0216212 0.00449835
0.217304 -0.0213882 0.00468094
0.21733 -0.0211304 0.00488234
0.21736 -0.02083 0.00511623
0.217394 -0.0204962 0.00537524
0.217432 -0.0201254 0.00566229
0.217473 -0.0197138 0.00598079
0.217519 -0.019257 0.00633486
0.217569 -0.0187499 0.00672957
0.217625 -0.0181856 0.00717072
0.217685 -0.017559 0.00766143
0.217752 -0.0168328 0.0082285
0.217824 -0.0160287 0.00885233
0.2179 -0.0151392 0.00953855
0.217978 -0.0141596 0.0102934
0.21806 -0.0130814 0.0111238
0.218145 -0.0118857 0.0120372
0.218234 -0.0105593 0.0130419
0.218327 -0.0091119 0.0141469
0.218423 -0.00752169 0.0153623
0.218519 -0.00574169 0.0166992
0.218603 -0.00379413 0.01817
0.21866 -0.00166115 0.0197883
0.218675 0.00048992 0.0214069
0.218653 0.00260323 0.0230256
0.218611 0.00445339 0.0244972
0.218559 0.00610324 0.025835
0.2185 0.00758562 0.0270512
0.218438 0.00889941 0.0281569
0.218374 0.0100659 0.029162
0.218309 0.0111166 0.0300757
0.218243 0.0120647 0.0309063
0.218178 0.0129181 0.0316614
0.218117 0.0136848 0.0323478
0.218058 0.0143722 0.0329718
0.218004 0.0149886 0.0335391
0.217956 0.0155155 0.03403
0.217912 0.0159844 0.0344713
0.217872 0.0164004 0.0348661
0.217836 0.0167711 0.0352203
0.217803 0.0171032 0.0355389
0.217774 0.0174016 0.0358261
0.217747 0.0176705 0.0360852
0.217722 0.0179132 0.0363191
0.217701 0.0181223 0.0365206
0.217682 0.0183118 0.0367032
0.217664 0.0184836 0.0368687
0.217648 0.0186392 0.0370185
0.217634 0.0187799 0.0371539
0.217621 0.0189069 0.0372761
0.217609 0.0190214 0.0373862
0.217598 0.0191244 0.0374853
0.217588 0.019222 0.0375791
0.217579 0.0193091 0.0376628
0.217571 0.0193867 0.0377374
0.217564 0.0194556 0.0378036
0.217557 0.0195167 0.0378623
0.217552 0.0195705 0.037914
0.217547 0.019618 0.0379596
0.217542 0.0196597 0.0379997
0.217538 0.0196962 0.0380347
0.217535 0.0197281 0.0380654
0.217532 0.0197559 0.0380921
0.21753 0.0197801 0.0381153
0.217527 0.0198012 0.0381356
0.217525 0.0198196 0.0381533
0.217524 0.0198357 0.0381687
0.217522 0.0198498 0.0381821
0.217521 0.019864 0.0381938
0.217519 0.0198796 0.0382039
0.217518 0.019897 0.0382127
0.217516 0.0199183 0.0382205
0.217511 0.0199664 0.0382273
0.217507 0.0200146 0.0382205
0.217505 0.0200358 0.0382127
0.217503 0.0200533 0.0382039
0.217502 0.0200688 0.0381938
# section 3
XYZ
+99
0.251068 -0.0250123 0.00642899
0.251064 -0.0250204 0.00644106
0.25106 -0.0250273 0.00645487
0.251055 -0.0250325 0.00647077
0.25105 -0.0250354 0.00648901
0.251044 -0.0250351 0.00650991
0.251039 -0.02503 0.00653394
0.251033 -0.0250168 0.00656142
0.251027 -0.0249876 0.00659284
0.251024 -0.0249273 0.00662865
0.25102 -0.0248566 0.00666932
0.251016 -0.0247766 0.00671539
0.251011 -0.0246862 0.00676743
0.251006 -0.0245844 0.00682603
0.251 -0.02447 0.00689184
0.250993 -0.0243419 0.00696557
0.250985 -0.0241987 0.00704804
0.250976 -0.0240475 0.00713503
0.250967 -0.0238797 0.00723155
0.250956 -0.0236939 0.00733848
0.250944 -0.0234884 0.00745676
0.25093 -0.0232613 0.00758744
0.250915 -0.0230106 0.00773168
0.250897 -0.0227341 0.0078907
0.250877 -0.0224127 0.00807538
0.250853 -0.0220564 0.00827987
0.250827 -0.0216606 0.00850645
0.250796 -0.0212198 0.0087578
0.250762 -0.0207276 0.00903716
0.250722 -0.0201762 0.00934853
0.250676 -0.0195583 0.00969644
0.250623 -0.018872 0.0100834
0.250558 -0.0180832 0.0105304
0.250484 -0.0172167 0.011022
0.250399 -0.0162526 0.0115627
0.250302 -0.0151755 0.0121573
0.250189 -0.0139956 0.0128113
0.250058 -0.0127184 0.0135307
0.249907 -0.0112921 0.0143219
0.249732 -0.00968576 0.0151922
0.249527 -0.0079398 0.0161493
0.249286 -0.00599318 0.0172017
0.249003 -0.00381508 0.0183589
0.248667 -0.00141637 0.019631
0.248305 0.000973856 0.0209022
0.247918 0.0033137 0.0221728
0.247544 0.00554123 0.0233276
0.247186 0.00761649 0.0243776
0.24685 0.00937261 0.0253325
0.246542 0.0108178 0.0262008
0.246255 0.0121657 0.0269907
0.245987 0.0134319 0.0277093
0.24574 0.0145632 0.0283629
0.245514 0.0155557 0.0289576
0.24531 0.0164269 0.0294987
0.245124 0.0171942 0.029991
0.244956 0.0178748 0.0304389
0.24481 0.0184539 0.0308267
0.24468 0.0189687 0.0311756
0.244563 0.0194255 0.0314879
0.244458 0.0198325 0.0317683
0.244364 0.0201964 0.0320206
0.24428 0.0205228 0.0322481
0.244203 0.020816 0.0324535
0.244135 0.0210798 0.032639
0.244076 0.0213062 0.0327988
0.244022 0.0215111 0.0329438
0.243973 0.0216963 0.0330751
0.243929 0.0218636 0.033194
0.24389 0.0220145 0.0333015
0.243854 0.0221506 0.0333986
0.243822 0.0222731 0.033486
0.243793 0.0223832 0.0335648
0.243765 0.0224874 0.0336393
0.243741 0.0225803 0.0337059
0.243719 0.0226629 0.0337651
0.2437 0.0227363 0.0338177
0.243682 0.0228012 0.0338644
0.243667 0.0228585 0.0339055
0.243654 0.022909 0.0339418
0.243642 0.0229533 0.0339736
0.243632 0.0229921 0.0340015
0.243623 0.0230259 0.0340258
0.243615 0.0230555 0.0340471
0.243609 0.0230812 0.0340656
0.243603 0.0231036 0.0340817
0.243597 0.0231231 0.0340958
0.243593 0.0231402 0.034108
0.243589 0.023155 0.0341187
0.243586 0.0231679 0.034128
0.243583 0.0231799 0.034136
0.24358 0.0231934 0.0341431
0.243577 0.02321 0.0341492
0.243572 0.023248 0.0341546
0.243569 0.0232861 0.0341492
0.243569 0.0233031 0.0341431
0.243569 0.0233169 0.034136
0.24357 0.0233293 0.034128
0.243571 0.0233406 0.0341187
NI_END NIBLADEGEOMETRY
NI_END NIBLADE
NI_END NIROW
NI_END GEOMTURBO
NI_BEGIN GEOMETRY
NI_END GEOMETRY
CHAPTER 6.
OPTIMIZATION ALGORITHMS FOR
AUTOBLADE™ FITTING
In AutoBlade™ Fitting, four types of optimization algorithms are available: genetic algorithm,
simulated annealing, gradient and random walk.:
FIGURE 6.1
AutoBlade™ Fitting algorithms
317
317
318
In this section
6.1 Random Walk
6.2 Gradient Method
6.3 Simulated Annealing
6.1
RANDOM WALK
From the best sample found in the database, the algorithm steps from the original point to another
point in a random way. If the sample found is better than the original point, the algorithm goes to
this point. Otherwise, another direction is tried. After a number of unsuccessful attempts, the
perturbation amplitude is reduced.
6.2 GRADIENT METHOD
This method is based on the computation of the gradient of the global objective function with
respect to all the design parameters. Then a small step in the direction opposed to the gradient is
performed. This process is repeated a number of times and usually ends when a stable optimum
has been found.
Genetic Algorithm: Default Algorithm
This algorithm mimics natural behavior in terms of biological evolution in order to reach the best
possible solution to a given problem. An initial population is generated and pairs of individuals
are selected from this population based on their performances. Weak individuals tend to die before
reproducing while stronger ones live longer.
FIGURE 6.2
Genetic algorithm parameters
l Population Size: number of individuals generated at each step of the reproduction process.
l Number of Reproduction Cycles: determines how many times the population will reproduce.
l At each generation, the individuals are classified according their performances (from the best
to the worse). That allows to select the x best ones to generate the next population:
l Truncation Rate: number of samples which are selected to reproduce; the default number is
20 that means only the 20 best samples are used to create a new sample in the next generation.
It is advised not to exceed half of the population size.
l Elitism: number of individuals that are directly transmitted to the next generation without any
change; by default, this value is 1, that means the next generation will contain the best
individual of the current population. It is advised not to exceed half of the Truncation rate.
l Extrapolation Range: determines between which values the parameters of the child will be
found. If it is set to 0 (default value), the interval of variation will be delimited by the
parameters of the parents. If not, the interval of variation will be bigger: it is useful only if the
parents are too close to explore a new field of variation.
Then, the user has to define the amplitude of mutation. If set to 0, there is no mutation: the
parameters of the child will be a mixing with the parameters of the parents. If not, the parameters
will be taken in the interval defined with the Extrapolation range and excluding the parameters of
the parents. Higher the amplitude of mutation is, more distant the parameters of the child will be
compared to the ones of the parents. Two parameters define the mutation:
l Search Interval: fixed amplitude of mutation.
l Precision Coefficient: coefficient which determines the fluctuation of the mutation
The amplitude of mutation is proportional to the product Search Interval*2-αPrecision Coefficient
with α generated randomly. So, if Search interval is set to 0, there is no mutation (default case)
and the higher the value of Precision Coefficient is, the lower the mutation amplitude will be. It is
advised to keep the default values of these two parameters.
6.3
SIMULATED ANNEALING
FIGURE 6.3
Simulated Annealing algorithm parameters
This algorithm is based on the analogy of the simulation of the annealing of solids. The algorithm
is similar to the random walk method but has a more sophisticated method to decrease amplitude
of the random perturbation steps.
l Initial temperature: initial temperature of the algorithm
l Final temperature: temperature at the end of the algorithm.
l Temperature Reduction factor: coefficient by which the current temperature is multiplied to
give the temperature of the next step. The number of iterations could be deduced using the
following formula:
(Tini-Tend)/Tred.
l Number of steps: Number of steps performed before the temperature reduction.
l Minimum error: parameter that fixes the convergence level of optimization (10 -Minimum
error). If the algorithm reaches the final temperature or the convergence level specified, the
algorithm will stop.
AutoBlade™ Fitting allows combining these algorithms by selecting the number of optimization
algorithms (FIGURE 6.1 (1)). The processing order of the algorithms is given with the active
optimization algorithm (FIGURE 6.1 (2)). In particular, a genetic algorithm can be applied and
then a gradient method to better refine the final optimum shape.
© NUMECA International, all rights reserved
EN201808281624

CHAPTER 1.
SYSTEM REQUIREMENTS
For proper installation and use of AutoBlade™ please consult the following sections detailing the
system requirements for the applicable operating system.
In this section
1.1 Windows
1.2 Linux
1.1 WINDOWS
1.1.1
Supported platforms and operating systems
NUMECA software is supported in 64 bits on x86_64 processors only (64 bits processors that are
compatible with Intel 8086 set of instructions).
Formally tested on
Windows 7 Professional
Windows 8.1 Professional
Windows 10 Professional
Windows HPC 2012
-
-
-
-
Also known to run ona
-
-
-
VISTA Business
VISTA Ultimate
Windows Server 2008
Windows Server 2012
a. Known from partners and/ or customers. No official support offered on these combinations.
Your platform of preference is not in the list?
Contact NUMECA local sales or support office. NUMECA software does however explicitly not
run on the following configurations:
l Power PC based systems,
l WINDOWS 2000 server workstations,
l WINDOWS 95, 98 or ME workstations.
1.1.2
Hardware requirements
Next to the standard hardware (monitor, keyboard and mouse), some specific recommendations
apply in the use of NUMECA software:
l a mouse with scroll wheel is strongly recommended.
l the monitor should support 24-bit color graphics and have a 1280 x 1024 pixel resolution for
adequate visualization.
l an Ethernet card should be installed and properly configured.
l NUMECA Software does not support CXFS (Clustered XFS) and IBRIX disk file systems.
1.1.3 Memory and disk space requirements
The Random Access Memory (RAM) required to run NUMECA software depends upon several
factors, in particular including the number of grid points inserted in the grid, the physical models
selected (turbulence, adaptation,...), the introduction of non-matching boundary conditions and the
selected calculation mode (mixed or double precision).
Similarly, a minimum disk space is required on the hard disk to allow the storage of the project
files. The size of these files largely depends upon the number of grid points generated.
NTFS file system is recommended for installation and working directories under Windows.
1.1.4
Graphics requirements
NVidia graphics cards are fully supported, installed together with the latest drivers.
NUMECA software makes use of the advantages of the available Graphics Card. Some trouble
may however come up with the default driver OPENGL since it may not be supported by the user
host computer and machine display. In order to set the system compatible with a more portable
driver, typically MSW driver is used under Windows instead. Note however that the proposed
drivers are usually less efficient in terms of graphical speed than the default driver.
To change the used driver
1. Log in as administrator.
2. Launch regedit from the Start/Run menu.
3. Go to the HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International register.
4. Go into the folder of the package for which to modify the driver, e.g.: Fine# where # is the
version number.
5. Modify the DRIVER entry to either OPENGL or MSW.
The selection will take effect at the next session.
1.2
LINUX
1.2.1
Supported platforms and operating systems
NUMECA software is supported in 64 bits on x86_64 processors only (64 bits processors that are
compatible with Intel 8086 set of instructions).
Formally tested on
Also known to run ona
Fedora Core 22.x, 25.x
(K)Ubuntu 14.04b, 16.04b
CentOS 7.0.1406
-
-
-
-
-
-
-
SuSe 10.1, 10.2, 11.0
Enterprise 3.x, 4.x, 5.x
Fedora Core 5.x, 7.x, 8.x, 12.x, 17.x, 18.x, 20.x
(K)Ubuntub 7.x, 8.x, 9.x, 10.x, 11.x, 12.x, 13.x
a. Known from partners and/ or customers. No official support offered on these combinations.
b. Debian based operating systems like Ubuntu, even if LSB compliant, are not recommended as a license
server as it is known to diverge occasionally from the LSB standard.
FlexLM requires LSB (Linux Standard Base) compliance. The list of Linux distributions and
applications
on
http://www.linuxfoundation.org/lsb-cert/productdir.php?by_lsb.
compliance with
available
standard
certified
LSB
the
for
is
When launching NUMECA software, if an error message appears when loading shared libraries,
contact NUMECA local sales or support office.
Your platform of preference is not in the list?
Contact NUMECA local sales or support office. NUMECA Software does however explicitly
not run on the following configurations:
l x86_64 processors running Linux SuSe 10.3,
l IBM PowerPC running Linux.
1.2.2
Hardware requirements
Next to the standard hardware (monitor, keyboard and mouse), some specific recommendations
apply in the use of NUMECA software:
l a mouse with scroll wheel is strongly recommended.
l the monitor should support 24-bit color graphics and have a 1280 x 1024 pixel resolution for
adequate visualization.
l an Ethernet card should be installed and properly configured.
1.2.3 Memory and disk space requirements
The Random Access Memory (RAM) required to run NUMECA software depends upon several
factors, in particular including the number of grid points inserted in the grid, the physical models
selected (turbulence, adaptation,...), the introduction of non-matching boundary conditions and the
selected calculation mode (mixed or double precision).
Similarly, a minimum disk space is required on the hard disk to allow the storage of the project
files. The size of these files largely depends upon the number of grid points generated.
1.2.4
Graphics requirements
NUMECA software makes use of the advantages of the available Graphics Card. By default, the
driver OPENGL is used.
In case a problem appears with the default driver OPENGL, the user should change to the X11 driver
under Linux. Note however that the X11 driver is usually less efficient in terms of graphical speed
than the default driver.
The drivers OPENGL and OPENGL2 may not work when using VNC or remote access by
"ssh". In case of problems, the X11 driver should be used.
To change the used driver
To change the driver permanently for every next launch of the software:
1. Open the file ~\.numeca\.drivers
2. Type: host_name display_name possible_drivers chosen_driver e.g. gauss.numeca.be gauss
OPENGL:X11 X11
The selection will take effect at the next session.
Alternatively, the driver can be manually specified in a shell for that shell session only through the
following commands:
l in csh or tcsh shell:
setenv NI_DRIVER X11
l in bash or korn shell:
NI_DRIVER=X11 export NI_DRIVER
CHAPTER 2.
INSTALLATION
Prior to the installation of AutoBlade™ it is important to consult first the "System requirements"
(p. 3).
This installation note concerns AutoBlade™ as a standalone product.
In this section
2.1 Windows
2.2 Linux
10
23
2.1 WINDOWS
The user is strongly advised to consult the "Windows" (p. 4) system requirements prior to the
installation. Problems may indeed appear during the installation and configuration phases in case
the listed hardware and software requirements would not be fully satisfied.
Please do notice that the documentation package attached to NUMECA software is not installed
during the installation procedure and can be downloaded from the Products page of the Customer
Area of www.numeca.be.
In case of trouble: .
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
At the end of the "Troubleshooting" (p. 21) the information to provide is listed.
2.1.1
Installation
Install AutoBlade™ under Windows
1. Log in as administrator or as a user with administrator privileges on the machine. If the user
the NUMECA software installation will not be
does not have administrator privileges,
performed successfully.
2. Check and make sure that the necessary disk space is available prior to starting the installation
process.
For the disk space requirements, see also: the "Windows" (p. 4) system requirements.
3. Get the installation package from the Products page of the Customer Area (www.numeca.be).
4. Unzip the installation package.
5. Exit all the other active applications and launch the setup.exe executable.
6. During the installation, the user will be asked to accept the terms of the License Agreement.
7. Enter the installation directory (referred to as NUMECA_INSTALLATION_DIRECTORY)
in function of one of the following scenarios:
l If NUMECA software was not installed before on the machine, choose a directory of your
preference. Providing a directory name that does not exist will create it automatically.
l If NUMECA software was already installed before, choose the same NUMECA_
INSTALLATION_DIRECTORY to use the multiple versions and/ or products in one
multi-version environment.
It is important to notice that a common NUMECA_INSTALLATION_DIRECTORY
should be shared by all NUMECA installations (e.g. C:\numeca_software\), otherwise
the multi-version installation will not be set up adequately.
8. At the end of the installation process, instructions to obtain information required for license
generation will be prompted. To this end, the following steps must be performed:
a. Click on Yes.
b. The license information is stored in the file license.info located in NUMECA_
INSTALLATION_DIRECTORY automatically. Once it is saved, send this text file to
NUMECA local sales or support office.
Alternatives to get the license information
The information can also be recovered as the Ethernet Address by clicking on the System
directory NUMECA_
Settings
INSTALLATION_DIRECTORY\<product_name>\flexlm.
lmtools.exe
launching
located
after
the
tab
in
9. After the package is installed, the NUMECA Admin Tool is launched automatically. This is a
tool for license management and provides a graphical user interface for the management of the
license server and client machines. The tool offers a guide through the process of setting up
and configuring a license server.
Alternatives to access the NUMECA Admin Tool
installation,
After
from
Start/Programs/NUMECA software/<product_ name>/Admin Tool menu. Close the
NUMECA Admin Tool dialog box to leave the tool and to finalize the installation.
the NUMECA Admin Tool
started
also
can
be
Tasks that can be performed in the NUMECA Admin Tool
l License Management: to configure the machine as license server and/ or client.
l User Configuration: to set user MPI configuration.
l Diagnostics: to assess and fix problems with license management, graphics, Windows
registry and parallel configuration.
l Network Configuration: to clean and reinitialize PVM, to setup RSH connections to other
machines/ users.
10. When receiving the license file from NUMECA, perform the license installation and user
configuration:
l "License management" (p. 12)
l "User Configuration" (p. 19)
During an installation and license specification, the administrator must launch the software once to
properly initialize flexlm.
In case of installation problems, right-click on setup.exe, select the option Run as... and then either
run as the true Windows Administrator account, or if and only if the user account with Administrator
privileges, run as user, but remove the option to run the program with restricted access. On Windows
7 it may also be necessary to disable the User Account Control feature (UAC) at least during the
installation process and the configuration steps.
2.1.2
License management
Introduction
Before using NUMECA software, a valid floating license is required.
What is a floating license?
With a floating license each software component is managed by an independent maximum
number of concurrent accesses (number of processes). Floating licenses are managed by a license
server which checks if process access is free. If so, when launching a software component, license
access is given to the user process or access is denied otherwise. The license can be accessed on
the same computer but also on other computers (clients) with Linux or Windows, connected
through a network to the license server. The license server can be a Linux or a Windows
machine.
l NUMECA updates the security ID of license files with each major release. License files
with old security ID cannot be used with the latest NUMECA software. Please send your
old license file to NUMECA local sales or support office for an upgrade of the license file.
l Redundant license server can be delivered allowing to manage a floating license by several
servers. For more information, contact NUMECA local sales or support office.
l Machines used as license server must have a fixed first IP address. For example, when
using VPN on Windows, VPN will become the first network interface. In this case, the
license server will not work properly.
l By default it is not possible to use a virtual machine as a license server. To install a license
server on a virtual machine, contact your account manager.
l Running Windows 64-bits, an additional Windows security patch is required to enable
CATIA v5 import with Datakit. For more details, link to the Microsoft official website.
NUMECA software must be installed on the license server. At the end of the installation, the
license information (the HostName and HostID of this computer) must be sent to NUMECA local
sales or support office in order to get a license file.
Before using NUMECA software, the license daemon should be configured on the license server.
See also: "Installation" (p. 10)
To set up the license server it is necessary to prepare the license file and launch the server either
though the NUMECA Administration Tool or in LMTools.
Access to the NUMECA Admin Tool
At the end of the installation of NUMECA software the Administration Tool is launched
automatically.
It can also be started anytime from the Start/Programs/NUMECA software/<product_
name>/Admin Tool menu.
It is required to run the Admin Tool as administrator for its proper functioning.
Prepare the license file
To install the license service:
1. Rename the license file as license.dat
2. Copy the license.dat file in the directory that all users are able to access.
3. Check that the license file has the read-execute access privileges:
l select the license file license.dat using Windows Explorer.
l while keeping the mouse on the selected file right-click and select from the appearing
menu: Properties. This will open a properties window.
l on the General page the Read-only box of the Attributes should not be selected. Unselect
this box if necessary.
l click on Apply and click on Close to close the window.
The "license.dat" file must be readable by every user.
When using a TCP port for the license server, the port number (check the free port with the
command: C:\\netsat -an) has to be added in the license file on the server/ vendor line:
1. SERVER hostname hostid and VENDOR numeca should be replaced by SERVER hostname
hostid portnumber1 and VENDOR numeca portnumber2;
2.
3.
reread the license file,
start NUMECA software and specify the license server writing portnumber@hostname . All
specified ports should be opened and free.
It is no more required to copy the license files on every client workstation if the variables NUMECA_
LICENSE_FILE defined as @license_server or port_number@license_server are added in the registry
database for each client. This allows to update the license file only on the license server.
License set-up in NUMECA Admin Tool
Start floating license service
To start the license service:
1. Select License Management.
2. On the line Activate from license file browse to the license file under the Product
(de)activation tab.
3. Click on the Activate button.
The manual start operations must be repeated each time the server machine is rebooted. Alternatively
it would be possible to define an automatic start of the license service from lmtools or using the
NUMECA Admin Tool.
Automatic start at machine boot
After the manual start of the license service, it is possible to have it automatically start at machine
boot:
1. Select License Management.
2. Under the License server tab, click on the Set Autostart button.
A Windows service called NUMECA License server is used.
Verify license service status
To verify that the license server is correctly running do the following:
1. From the NUMECA Admin Tool home page, click on License Management.
2. Select the License server tab.
3. Select the license server in the first table listing all known servers available on the machine.
4. Information regarding the available features, number of available licenses and number of used
licenses is shown in the second table.
Update of license file
When a license file is expired, contact NUMECA local sales or support office to obtain an
updated license file.
Rename this license file to license.dat and follow the instructions below.
1. Replace the active license file license.dat with the update license provided by NUMECA
(renamed as license.dat).
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
2. From the NUMECA Admin Tool home page, click on License Management .
3. Select the License server tab.
4. Under the Start/Stop/Reread section, make sure the license path is correct and click on the
icon
.
If the version of the Flexlm tool is upgraded or the version of the license file security ID is upgraded,
an update of the license file is not enough. The user must shutdown the running license server and
start a new license server with the latest Flexlm tool and the latest license file.
Alternative: license set-up in lmtools
Start license service
1. In Windows Explorer,
browse
to
the
directory NUMECA_ INSTALLATION_
DIRECTORY/<product_name>/flexlm and double click on lmtools.exe.
2. On the Service/License File page select Configuration using Services.
3. Select the Config Services tab.
4. Enter for Service Name any name indicating that it is related to a NUMECA license (e.g.,
numeca_license).
5. To enter the Path to the lmgrd.exe file click on Browse right next to the text box and browse
select
to NUMECA_ INSTALLATION_ DIRECTORY/<product_ name>/flexlm and
lmgrd.exe.
6. To enter the Path to the license file, click on Browse right next to the text box and browse to
the license file license.dat to select it (files of type from license files (".lic") to license files
(".dat")).
7. Enter HOME_DIRECTORY/.numeca/debug.log to access the path of debug log file. This
file is automatically created when starting the license service.
8. Click on Save Service.
9. Select Use Services and Start Server at Power Up. In this way the license service will be
automatically starting when booting under Windows.
10. To start the server now manually select the tab Start/Stop/Reread.
11. Select
the NUMECA license service under Flexlm license Services installed on this
computer.
12. Click on Start Server.
If the license service was correctly started, numeca.exe and lmgrd.exe should be visible in the list
of processes or services in Windows Task Manager. If these executables are not running verify the
debug.log file.
See also: "Troubleshooting" (p. 21)
13. If NUMECA software is used on the license server, the user should first perform a user
configuration as described in the section "User Configuration" (p. 19).
14. Launch the software a first time.
15. Click on Specify the License Server.
16. Enter the name of the license server or its IP address.
17. Click on Finish.
Verify license service status
To verify that the license server is correctly running do the following:
1. Open the Windows Task Manager.
2. Select the Processes or Services.
3. Check that the processes numeca.exe and lmgrd.exe are running.
or:
1. In Windows Explorer
browse
to
the
directory NUMECA_ INSTALLATION_
DIRECTORY/<product_name>/flexlm and double click on lmtools.exe.
2. Select Configuration using Services.
3. Select the tab Server Status.
4. Click on Perform Status Enquiry and wait to see the server status and the available features.
Update of license file
When a license file is expired, contact NUMECA local sales or support office to obtain an
updated license file.
Rename this license file to license.dat and follow the instructions below.
1. Replace the active license file license.dat with the update license provided by NUMECA
(renamed as license.dat).
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
2. Go to the directory NUMECA_INSTALLATION_DIRECTORY/<product_name>/flexlm.
3. Start the LMTools by double clicking on lmtools.exe
4. Select the tab Start/Stop/Reread.
5. Select the NUMECA license service in the list and click on ReRead License File.
If the version of the Flexlm tool is upgraded or the version of the license file security ID is upgraded,
an update of the license file is not enough. The user must shutdown the running license server and
start a new license server with the latest Flexlm tool and the latest license file.
Floating license on Windows client
When a floating license is installed on a license server, this license may be used by other
computers with a network connection to the license server. In this section, it is assumed that the
license server is running. On each Windows client, the user must:
1. Install NUMECA software.
2. Perform a user configuration on this machine before first use as described in section "User
Configuration" (p. 19).
3. Launch the software a first time.
4. Click on Specify the License Server.
5. Enter the name of the license server or its IP address.
6. Click on Finish.
Student version with activation ID
In general a license certificate (text file) is provided to give access to NUMECA software.
Alternatively the NUMECA Admin Tool allows to use an activation ID to start the license server.
For example, the free student version is based on an activation ID and the instructions how to use
it are provided together with the activation ID. Use of an activation ID requires the use of Trusted
storage and installation of an anchor service. Hence this terminology can be found in the
NUMECA Admin Tool but can be safely ignored in case of a license certificate in text file
format.
Example of an Activation ID: C2a9-561f-7895-435b-acb5-3520-c166-4bcc
2.1.3
User Configuration
A. Optional user configuration
Home directory
On Windows, NUMECA software saves some data (preferences, user fluid database, ...) in the
folder %HOME%\.numeca\, or in the %HOMEDRIVE%%HOMEPATH%\.numeca\ folder in
case %HOME% is not defined. If the user wants to customize the path of the .numeca folder, the
user can redefine the system environment variable HOME.
Note:
l The variable HOME must be defined as a system environment variable.
l Defining HOME to a network disk may significantly slow down the NUMECA software
GUI.
the
runtime, NUMECA software writes
During
directory
%HOME%\.numeca\tmp. This tmp directory can be redefined by defining the environment
variable TMP_DIR.
temporary
data
the
in
B. Software launch
After configuring,
software\<product_name>\ menu.
the product can be
started from the Start\Programs\NUMECA
It is not allowed to start NUMECA software under Windows as administrator in a user domain
environment. This limitation does not apply to user login.
In case the license has not been configured adequately at this stage of the installation process, it is still
possible to launch the product by selecting a license file (server) when prompted after first launch.
The UAC (User Account Control) should be disable for running the solver in parallel otherwise it
prevents mpiexec to record the encrypted login and password in the registry database and the Task
Manager remains open forever without any evolution.
NUMECA software can be launched directly from the user desktop by copying shortcuts from
~\AllUsers\StartMenu\Programs\NUMECA software\<product_name>\ to ~\AllUsers\Desktop.
2.1.4
Uninstallation
Before removing a product, the license service and PVM should be stopped as detailed in the
following section. As a next step the product can be removed.
Uninstall license service
In case the license service is defined based on a version of NUMECA software to uninstall, the
license service should be stopped and removed first. Of course further use of remaining
NUMECA products on the machine will require redefining the license service based on the most
recent product.
In NUMECA Admin Tool
1. Go to the NUMECA Admin Tool home page,
2. click on License Management,
3. under the Product (de)activation tab, click on the Deactivate button and Apply to confirm
and stop the running license server(s) and return all existing fulfillment from this machine.
4. The words "Success" or "Failed" are shown depending on the success or failure of the
uninstalling process, respectively.
5. Click on the Unset Autostart button under the License server tab to complete the uninstalling
process.
Or in LMTools
1. Browse
to
DIRECTORY/<product_name>/flexlm.
in Windows Explorer
the
directory NUMECA_ INSTALLATION_
2. Double click on lmtools.exe.
3. Select Configuration Using Services.
4. Click on the Start/Stop/ReRead tab.
5. Select the NUMECA license service from the list of services.
6. Click on Stop to stop the license service.
7. Click on the tab Configure Services.
8. Select the NUMECA license service through the Service Name pull down menu.
9. Click on Remove Service to remove the service.
Uninstall the product
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in subsection
"Uninstall license service" (p. 20).
3. Open the Windows Control Panel (Start/Control Panel) and double click on the icon
Programs and Features.
4. Select the product from the list and click on Uninstall.
2.1.5
Troubleshooting
Introduction
In most cases, a straightforward and careful execution of the instructions detailed in the
installation note enables to start NUMECA software smoothly. In case it is not working as
expected this section provides information on how to handle most common situations.
Product not starting
In case AutoBlade™ does not start, check the following items:
l Is NUMECA software installed with administrator privileges? If not, perform the installation
again with administrator privileges.
l Check whether 'Hide file extensions for known types' (activated by default for .dat extensions)
is disabled to enter the name of the license file with its extension license.dat.
l Is the license file valid and active to start the product ?
ll Check if the license server is up. If so, the numeca.exe process should run in the Windows
Task Manager. If not, please do the instructions for license installation.
l Some license check problems may occur if the host computer cannot find the server IP-address
corresponding to the hostname information included in the first line of the license key. To
solve this problem, replace the hostname by the IP-address of the license server. This operation
does not invalidate the license key.
l Check if the license key file is well readable by every user.
l Was the user configuration performed? If not, perform the configuration according to the
section "User Configuration" (p. 19); then log out and log in.
l Has the machine been rebooted after a change in the environment variables? If not, reboot it.
l Check if the TCP/IP protocol is installed on the machine. The protocol is mandatory to ensure
the correct function of the floating licenses.
l Are the NUMECA software components visible from the machine? If not, install them.
Graphical problems and system crashes
NUMECA software makes use of the advantages of the available Graphics Card. Some trouble
may however come up with the default driver OPENGL since it may not be supported by the user
host computer and machine display. In order to set the system compatible with a more portable
driver, typically MSW driver is used under Windows instead. Note however that the proposed
drivers are usually less efficient in terms of graphical speed than the default driver.
To change the used driver
1. Log in as administrator.
2. Launch regedit from the Start/Run menu.
3. Go to the HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International register.
4. Go into the folder of the package for which to modify the driver, e.g.: Fine# where # is the
version number.
5. Modify the DRIVER entry to either OPENGL or MSW.
The selection will take effect at the next session.
Screen flashes
In some circumstances, the graphical area can flash during interactive operations, depending upon
the driver selected. Setting the environment variable NI_ DOUBLEBUFFERING to ON in
HKEY_ LOCAL_ MACHINE/SOFTWARE/NUMECA International/<product_ name> register
may solve the problem. To launch the registry editor, access regedit in the Start/Run text box.
Further troubleshooting
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
The following information can be helpful:
l the license key file license.dat.
l the hostname and hostid. This information can be obtained by executing into the subdirectory
NUMECA_ INSTALLATION_ DIRECTORY\<product_ name>\flexlm the lmtools.exe (for
Hostname and HostID for NUMECA as Computer/Hostname and Ethernet Address under
the System Settings tab).
l the product name and version for which installation is causing problems.
l a description of the configuration (in terms of name, Windows version, local or domain user).
l the debug.log file generated when starting the license service.
l the .out files in C:\tmp.
l the pvml.username in C:\tmp (or directory defined by the environment variable PVM_TMP).
2.2
LINUX
The user is strongly advised to consult the "Linux" (p. 6) system requirements prior to start any
installation. Troubles may indeed appear during the installation and configuration phases in case
the listed hardware and software requirements would not be fully satisfied.
Please do notice that the documentation package attached to NUMECA software is not installed
during the installation procedure and can be downloaded from the Products page of the Customer
Area of www.numeca.be.
In case of trouble: .
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
At the end of the "Troubleshooting" (p. 36) section the information to provide is listed.
2.2.1
Installation
Install AutoBlade™ under Linux
1. Log in the workstation corresponding to the selected OS. It is strongly recommended not to
install the software as "root" or using the command "sudo" because the user may have no
permission to execute the software afterward. It is strongly recommended to check the
permission of the disk and directory the user will select for the software installation.
2. Check and make sure that the necessary disk space is available prior to starting the installation
process.
For the disk space requirements, see also: the "Linux" (p. 6) system requirements.
3. Get the installation package from the Products page of the Customer Area (www.numeca.be).
4. Check that the file can be accessed with full permission and extract it by typing the command
line: tar -xvf <package_name>.tar.
Do NOT extract the tar file in the target directory NUMECA_ INSTALLATION_
DIRECTORY in which the product will be installed.
5. Go to the directory containing the files extracted from the tar archive and type the command
./install_numeca <ENTER>.
The trusted storage based licensing requires a LSB compliant platform. After license agreement, a
check is performed to verify whether the host machine is LSB compliant. It is required if the
license server is installed on the host machine.
6. During the installation, the user will be asked to accept the terms of the License Agreement.
7. Enter the installation directory (referred to as NUMECA_INSTALLATION_DIRECTORY)
in function of one of the following scenarios:
l If NUMECA software was not installed before on the machine, choose a directory of your
preference. Providing a directory name that does not exist will create it automatically.
l If NUMECA software was already installed before, choose the same NUMECA_
INSTALLATION_DIRECTORY to use the multiple versions and/ or products in one
multi-version environment.
It is important to notice that a common NUMECA_INSTALLATION_DIRECTORY
should be shared by all NUMECA installations, otherwise the multi-version installation
will not be set up adequately.
the old
If the product has not been installed in the same 'NUMECA_INSTALLATION_DIRECTORY'
as
/NUMECA_ INSTALLATION_
'add_ version.sh'
DIRECTORY/COMMON/ will allow the user to link previous versions by specifying their full
path name (e.g.: /usr/numeca_software/fineautogrid112).
product. The
script
in
8. Finally, the so-called 'HostName' and 'HostID' information required to generate a license file
will be shown. This information should be sent to NUMECA local sales or support office.
Alternative to find the HostName and HostID from a shell
Type the commands:
NUMECA_INSTALLATION_DIRECTORY/<product_
name>/LINUX/install/flex64/lmutil lmhostid -hostname <Enter>
and
NUMECA_INSTALLATION_DIRECTORY/<product_
name>/LINUX/install/flex64/lmutil lmhostid <Enter>.
9. After the package is installed, the NUMECA Admin Tool is launched automatically. This is a
tool for license management and provides a graphical user interface for the management of the
license server and client machines. The tool offers a guide through the process of setting up
and configuring a license server.
Alternative to access the NUMECA Admin Tool
After installation, the NUMECA Admin Tool can also be started through the command
admin#, where # is the software version (e.g. admin131). Close the NUMECA Admin Tool
dialog box to leave the tool and to finalize the installation.
Tasks that can be performed in the NUMECA Admin Tool
l License Management: to configure the machine as license server and/ or client.
l User Configuration: to set the PATH in the .bashrc/.cshrc/.profile files.
l Network Configuration: to clean and reinitialize PVM, to setup SSH connections to other
machines/ users.
l Diagnostics: to assess and fix problems with license management and graphics.
10. When receiving the license file from NUMECA, perform the license management and user
configuration:
l "License management" (p. 26)
l "User Configuration" (p. 33)
Launch the software as described in the user guide of your product while taking into account
the points of attention as listed in the "Software launch" (p. 33) section of the Linux user
configuration.
2.2.2
License management
Introduction
Before using NUMECA software, a valid floating license is required.
What is a floating license?
With a floating license each software component is managed by an independent maximum
number of concurrent accesses (number of processes). Floating licenses are managed by a license
server which checks if process access is free. If so, when launching a software component, license
access is given to the user process or access is denied otherwise. The license can be accessed on
the same computer but also on other computers (clients) with Linux or Windows, connected
through a network to the license server. The license server can be a Linux or a Windows
machine.
Important points of attention for license servers:
l NUMECA updates the security ID of license files with each major release. License files
with old security ID cannot be used with the latest NUMECA software. Please send your
old license file to NUMECA local sales or support office for an upgrade of the license file.
l Redundant license server can be delivered allowing to manage a floating license by several
servers. For more information, contact NUMECA local sales or support office.
l Machines used as license server must have a fixed first IP address. For example, when
using VPN on Windows, VPN will become the first network interface. In this case, the
license server will not work properly.
l By default it is not possible to use a virtual machine as a license server. To install a license
server on a virtual machine, contact your account manager.
l FlexLM requires LSB (Linux Standard Base) compliant OS.
NUMECA software must be installed on the license server. At the end of the installation, the
license information (the HostName and HostID of this computer) must be sent to NUMECA local
sales or support office in order to get a license file.
Before using NUMECA software, the license daemon should be configured on the license server.
To set up the license server it is necessary to prepare the license file and launch the server either
though the NUMECA Administration Tool or in a shell.
Access to the NUMECA Admin Tool
At the end of the installation of NUMECA software the NUMECA Admin Tool is launched
automatically.
It can also be started anytime on Linux using the command: admin#, where # is the software
version.
It is recommended to run the NUMECA Admin Tool as root to fully benefit from all its possibilities.
Example
admin131
Prepare the license file
To install the license service take the following steps:
1. Rename the license file as license.dat.
2. Copy the license.dat file in the directory that all users are able to access.
3. Check that the license file has the read- execute access privileges (execute chmod 755
license.dat).
The "license.dat" file must be readable by each user.
When using a TCP port for the license server, the port number has to be added in the license file on
the server/vendor line:
1. SERVER hostname hostid and VENDOR numeca should be replaced by SERVER
hostname hostid portnumber1 and VENDOR numeca portnumber2;
2.
3.
reread the license file,
start NUMECA software and specify the license server writing portnumber@hostname . All
specified ports should be opened and free.
License set-up in NUMECA Admin Tool
Start floating license service
To start the license service:
1. Select License Management.
2. On the line Activate from license file browse to the license file under the Product
(de)activation tab.
3. Click on the Activate button.
The manual start operations must be repeated each time the server machine is rebooted. Alternatively
it would be possible to define an automatic start of the license service from lmtools or using the
NUMECA Admin Tool.
Automatic start at machine boot
After the manual start of the license service, it is possible to have it automatically start at machine
boot:
1. Select License Management.
2. Under the License server tab, click on the Set Autostart button.
When starting the license service through the NUMECA Admin Tool, it uses the cron daemon of
the user who installs the software to define the automatic start of the license at machine boot. Cron
is a daemon used to schedule various kind of tasks on Linux. This tool uses crontab text files that
specify commands/ tasks to run at certain time intervals. In the case of NUMECA Admin Tool,
the cron daemon automatically starts the license service using the license file(s) or existing server
specified in the previous license server set-up. In absence of a previous set-up, the daemon uses
the dummy address NUMECA_INSTALLATION_DIRECTORY/flexlm/any.lic as the license
server file location for the autostart.
Verify license service status
To verify that the license server is correctly running do the following:
1. From the NUMECA Admin Tool home page, click on License Management.
2. Select the License server tab.
3. Select the license server in the first table listing all known servers available on the machine.
4. Information regarding the available features, number of available licenses and number of used
licenses is shown in the second table.
Floating license on Linux client
When a floating license service is installed on a license server, this license service may be used by
other computers with a network connection to the license server. In this section, it is assumed that
the license server is running.
1. Go to the NUMECA Admin Tool home page,
2. click on License Management,
3. select the Product (de)activation tab,
4. select the Connection to a license server option.
Users willing to launch NUMECA software on a client should perform a user configuration on
this machine before first use as described in the section "User Configuration" (p. 33).
Update of license file
When a license file is expired, contact NUMECA local sales or support office to obtain an
updated license file.
Rename this license file to license.dat and follow the instructions below.
1. Replace the active license file license.dat with the update license provided by NUMECA
(renamed as license.dat).
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
2. From the NUMECA Admin Tool home page, click on License Management .
3. Select the License server tab.
4. Under the Start/Stop/Reread section, make sure the license path is correct and click on the
icon
.
If the version of the Flexlm tool is upgraded or the version of the license file security ID is upgraded,
an update of the license file is not enough. The user must shutdown the running license server and
start a new license server with the latest Flexlm tool and the latest license file.
Alternative license server set-up from a shell
Start of the license service
To start the license daemon manually, do the following operations:
1. Go
to
directory
the
name>/LINUX/install/flex64/
NUMECA_ INSTALLATION_ DIRECTORY/<product_
2. Execute
./lmgrd
DIRECTORY/COMMON/license.dat -l $HOME/.numeca/debug_numeca.log
command:
the
NUMECA_ INSTALLATION_
-
In these lines, 'NUMECA_INSTALLATION_DIRECTORY' should be replaced by the absolute
directory path where you have installed NUMECA software.
The manual start operations must be repeated each time the server machine is rebooted.
Automatic start at machine boot
The license daemon can be automatically started during the workstation boot process. For
example to do so on LINUX Red Hat Enterprise 5.1:
1. Login as "root"
2. Go to the /etc directory
3. Edit the inittab file
4. Add the following line at the end:
lmgr:35:wait:/NUMECA_INSTALLATION_DIRECTORY/<product_
name>/LINUX/install/flex64/lmgrd -c License_path/license.dat
In this line, 'NUMECA_INSTALLATION_DIRECTORY' should be replaced by the absolute
directory path where you have installed NUMECA software, 'License_path' should be replaced
by the absolute directory path where the license file is located.
The license server can also be started from /etc/rc#.d/. For more information contact your system
administrator or NUMECA local sales or support office.
Verify License Service Status
To verify that the license server is correctly running do the following:
1. Go to the directory:
NUMECA_INSTALLATION_DIRECTORY/<product_name>/LINUX/install/flex64/
2. Execute the command: ./lmutil lmstat -c License_path/license.dat
If the license server is up this will be shown in the shell with the words: "license server UP
(MASTER) v11.14". The vendor daemon numeca needs to be up as well as indicated with the
words: "Vendor daemon status (on license_server_machine_name): numeca: UP v11.14
If the license server or vendor daemon is not up, see: "User Configuration" (p. 33)).
3. To display the active users of a given feature, use the following command: ./lmutil lmstat -a -c
License_path/license.dat
Floating license on Linux client
When a floating license is installed on a license server, this license may be used by other
computers with a network connection to the license server. In this section, it is assumed that the
license server is running.
On a Linux client, the path of the NUMECA_ LICENSE_ FILE should be defined in the
~/.flexlmrc file:
l in csh or tcsh shell:
setenv NUMECA_LICENSE_FILE /full-path/license.dat or @servername
l in bash or korn shell:
NUMECA_LICENSE_FILE=/full-path/license.dat or @servername
export NUMECA_LICENSE_FILE
Users willing to launch NUMECA software on a client should perform a user configuration on
this machine before first use as described in section "User Configuration" (p. 33).
Update of license file
When a floating license file is expired, contact NUMECA local sales or support office to obtain
an updated license file and follow the instructions below.
1. Rename the license file to license.dat.
2. Replace the active license file with the updated provided license on license server.
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
3. Go to the directory
NUMECA_INSTALLATION_DIRECTORY/<product_name>/LINUX/install/flex64/
4. Execute the command:
./lmutil lmreread -c LICENSE_FULL_PATH/license.dat
If the version of the Flexlm tool is upgraded or the version of the license file format is upgraded, an
update of the license file is not sufficient. The user must shutdown the running license server and start
a new license server with the latest Flexlm tool and the latest license file.
Student version with activation ID
In general a license certificate (text file) is provided to give access to NUMECA software.
Alternatively the NUMECA Admin Tool allows to use an activation ID to start the license server.
For example, the free student version is based on an activation ID and the instructions how to use
it are provided together with the activation ID. Use of an activation ID requires the use of Trusted
storage and installation of an anchor service. Hence this terminology can be found in the
NUMECA Admin Tool but can be safely ignored in case of a license certificate in text file
format.
Example of an Activation ID: C2a9-561f-7895-435b-acb5-3520-c166-4bcc
2.2.3
User Configuration
Introduction
At the end of the installation, each user willing to use NUMECA software must initially configure
his/ her working environment by running an initialization script.
Configure the user environment
1. Log in as user.
2. Go to the directory NUMECA_INSTALLATION_DIRECTORY/COMMON, and execute
the command ./configure. This operation will add a couple of lines in the user's .cshrc, .tcshrc
or .profile file (located in user's home directory) and add the NUMECA software in user's
default path.
3. Log out and log in again to apply the information in the .cshrc , .tcshrc or .profile file.
On Linux, NUMECA software saves some data (preferences, user fluid database, templates...) in the
folder $HOME\.numeca\. The variable $HOME is imposed by NUMECA software and cannot be
modified.
During the runtime, NUMECA software writes temporary data in the directory $HOME/.numeca/tmp.
This tmp directory can be redefined by defining the environment variable NI_TMP_DIR.
Software launch
To launch the components:
<productname><version#> -print <Enter>
Example
autoblade131-print <Enter>
It is important to outline that no output is displayed by default in the shell where the software is
launched. Instead the output is redirected to log files, located in the directory ~/.numeca/tmp/ and
named as startup_logfile_fine, startup_logfile_hexpress, startup_logfile_cfview.
However, outputs can still be forced for display in the shell. Add the - print command to the
command line. This will give additional information during software launch, especially during the
initial configuration of the software.
2.2.4 Uninstallation
Introduction
This section details the steps required to properly remove an installation of NUMECA software.
This section details the steps required to properly remove an installation of NUMECA software.
Depending upon the configuration, there are several possibilities:
l If the product is the only product and the only version on the computer: uninstall in mono-
version environment.
l If other products and/ or other versions are installed on the same machine, it is possible to: 
l to remove only some of these products/ versions: partly uninstall
in multi- version
environment",
l to remove all products: fully uninstall in multi-version environment".
Furthermore, the license service may be stopped if NUMECA software is not used on any
machine connected to the license server.
Uninstall license service
Points of attention:
l Instructions related to the NUMECA license service must be removed if the machine has
been configured to start automatically the license service at start up. These instructions can
be accessed in the /etc/inittab file.
l It is not possible to stop the license server without an internet connection.
l The license server cannot be started or stopped without a network connection.
In NUMECA Admin Tool
1. Go to the NUMECA Admin Tool home page,
2. click on License Management,
3. under the Product (de)activation tab, click on the Deactivate button and Apply to confirm
and stop the running license server(s) and return all existing fulfillment from this machine.
4. The words "Success" or "Failed" are shown depending on the success or failure of the
uninstalling process, respectively.
5. Click on the Unset Autostart button under the License server tab to complete the uninstalling
process.
In a shell
The license service should be stopped before uninstalling NUMECA software.
To do so, the following operations must be performed:
1. Go
to
directory
the
name>/OSname/install/flex#/
NUMECA_ INSTALLATION_ DIRECTORY/<product_
2. Execute the command: ./lmutil lmdown -c LICENSE_FULL_PATH/license.dat
Uninstall in mono-version environment
Proceed as follows to remove a product in a mono-version environment under Linux:
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in the subsection
"Uninstall license service" (p. 34).
3. Remove the lines from "#begin NUMECA configuration" to "#end NUMECA configuration"
from the user's .cshrc, .tcshrc or .profile file.
4. Remove the directory NUMECA_INSTALLATION_DIRECTORY and its content.
Partly uninstall in multi-version environment
Proceed as follows to remove one product version in a multi-version environment under Linux:
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in the subsection
"Uninstall license service" (p. 34) .
3. Remove the directory NUMECA_INSTALLATION_DIRECTORY/<product_name>/ and
all of its content.
Before removing the directory NUMECA_INSTALLATION_DIRECTORY/<product_name>/, check
and make sure that the license file is not inside the directory.
Fully uninstall in multi-version environment
Proceed as follows to remove all NUMECA products in a multi-version environment under
Linux:
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in the subsection
"Uninstall license service" (p. 34).
3. Remove the lines from "#begin NUMECA configuration" to "#end NUMECA configuration"
from the user's .cshrc, .tcshrc or .profile file.
4. Remove the directory NUMECA_INSTALLATION_DIRECTORY and its content.
2.2.5
Troubleshooting
Introduction
In most cases, a straightforward and careful execution of the instructions detailed in the previous
chapters enables the user to start NUMECA software smoothly. In case of problems, this section
aims at providing guidelines on how to detect and solve possible troubleshooting.
Product not starting
If AutoBlade™ does not start, use the -print argument in the command line to start the product.
For example: autoblade131 -print
This argument will output information in the shell (including the location of the license file) which
may be helpful to understand the problem. With this information at hand, check the following
items:
l Is the license file valid and active to start the product ?
l Check if the license server is up. On the license server, two active daemons should be present.
This can be seen using the commands ps -ealf | grep lmgrd and ps -ealf | grep numeca. If not,
follow the instructions for license installation.
l Some license check problems may occur if the host computer cannot find the server IP-address
corresponding to the hostname information included in the first line of the license key. To
solve this problem, replace the hostname by the IP-address of the license server. This operation
does not invalidate the license key.
l Check if the license key file is well readable by every user.
l Did the user configure the working environment? Before using NUMECA software, each user
must configure the working environment using the command ./configure within the
NUMECA_INSTALLATION_DIRECTORY/COMMON/ directory; then log out and log in.
l Is the graphics driver appropriate for the display?
To change the used driver
To change the driver permanently for every next launch of the software:
1. Open the file ~\.numeca\.drivers
2. Type: host_ name display_ name possible_ drivers chosen_ driver e.g. gauss.numeca.be
gauss OPENGL:X11 X11
The selection will take effect at the next session.
Alternatively, the driver can be manually specified in a shell for that shell session only through
the following commands:
l in csh or tcsh shell:
setenv NI_DRIVER X11
l in bash or korn shell:
NI_DRIVER=X11 export NI_DRIVER
l Check if the TCP/IP protocol is installed on the machine. The protocol is mandatory to ensure
the correct function of the floating licenses.
l Are the NUMECA software components visible from the machine? If not, install them.
l Is the OS adequate? If not, copy the correct tar file and start the installation again.
l Are the Linux permissions sufficient for the user to access NUMECA software installed? Ask
your system administrator.
Graphical problems and system crashes
NUMECA software makes use of the advantages of the available Graphics Card. Some trouble
may however come up with the default driver OPENGL since it may not be supported by the user
host computer and machine display.
In order to set the system compatible with a more portable driver, refer to the following
instructions. Note however that the proposed drivers are usually less efficient in terms of graphical
speed than the default driver.
To change the used driver
To change the driver permanently for every next launch of the software:
1. Open the file ~\.numeca\.drivers
2. Type: host_name display_name possible_drivers chosen_driver e.g. gauss.numeca.be gauss
OPENGL:X11 X11
The selection will take effect at the next session.
Alternatively, the driver can be manually specified in a shell for that shell session only through the
following commands:
l in csh or tcsh shell:
setenv NI_DRIVER X11
l in bash or korn shell:
NI_DRIVER=X11 export NI_DRIVER
GUI flashes
In some circumstances, the graphical area can flash during interactive operations, depending upon
the driver selected. This mostly happens when using the X11 driver. Setting the environment
variable NI_DOUBLEBUFFERING to ON into the user profile (.cshrc, .profile, .tcshrc,...)
may solve the problem under Linux. The variable can be manually specified through the
following commands:
l for csh or tcsh shells: setenv NI_DOUBLEBUFFERING ON
l for
bash
korn
DOUBLEBUFFERING
or
shells:
NI_ DOUBLEBUFFERING=ON
export
NI_
Display drivers not detected
NUMECA products with GUI check the available working drivers and updates automatically in
the .drivers file located in the .numeca directory of the user at first launch on a new machine/
display. This operation is only completed during the first execution, since it may take some time.
As a consequence, the upgrade of drivers on an existing machine/ display cannot be automatically
detected.
Further troubleshooting
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
The following information can be helpful:
l the license key file license.dat.
l the hostname and hostid. This information can be obtained by executing the commands lmutil
lmhostid <Enter> in the NUMECA_
lmhostid - hostname <Enter> and lmutil
INSTALLATION_DIRECTORY/<product_name>/LINUX/install/flex64/ directory.
l the product name and version for which installation is causing problems.
l a description of the configuration (in terms of name, platform and OS for each machine on
which NUMECA software is installed).
l the .log file generated during the installation and located in the /tmp directory on the machine
from where the script ./install_numeca has been launched .
l the "startup_logfile_*" files located in ~\.numeca\tmp.
© NUMECA International, all rights reserved
EN201808281221

11
15
19
CONTENTS
TUTORIALS
TUTORIAL 1. MARINE PROPELLER - BLADE FITTING
1.1
Introduction
Preparation
Introduction
1.1.1
1.1.2
1.2 Blade fitting
1.2.1
1.2.2 Define the target model
1.2.3 Define the initial model
1.2.4
1.2.5
Pre-fitting
Fitting
Create new AutoBlade™ project
1.3 Save the project
TUTORIALS
Where to Find the Files Used in the Tutorials?
The appropriate files (and any other relevant files used in the tutorials) can be downloaded from
the corresponding link: AutoBlade-Tutorials.
Conventions Used in the Tutorials
Several conventions are used in the tutorials to facilitate your learning process.
Inputs required to execute the tutorials are most often restricted to the geometry definition.
The sequence of actions to be executed are described through a step-by-step approach, in the form
of Arabic numbers.
Additional insight about some specific actions and/ or features is frequently added to illustrate the
tutorial further. This information is proposed for the purpose of clarity and completeness, and
should not be executed. It appears as a note with a light blue background.
Contact NUMECA local sales or support office for any question or information you may require. To
allow NUMECA local sales or support office to help you out within the shortest delays, please
provide a detailed description of the observed behavior and performed analysis.
TUTORIAL 1.
MARINE PROPELLER - BLADE FITTING
1.1
INTRODUCTION
1.1.1
Introduction
In order to re-design and optimize existing blades to reach better design goals, NUMECA has
developed a unique integrated environment for the design and parametrization of three
dimensional turbomachinery blades.
This tutorial is particularly adapted to the parametrization of a marine propeller. It makes use of
Autoblade™. This parametric model can be used in the framework of an optimization loop.
In this tutorial:
l fit a target geomTurbo to create a parametric blade model within AutoBlade™.
1.1.2
Preparation
l Copy the provided project "Tutorial_1" located in the archive AutoBlade-Tutorials to your
working directory.
l Start the NUMECA blade modeler for turbomachinery blades AutoBlade™ v13.1:
l For Linux systems, you can access AutoBlade™ with the following command line:
autoblade -niversion 131 -print
l For Windows systems, you can access AutoBlade™ from the Start menu going to
\Programs\NUMECA
software\Fine131\AutoBlade
or
\Programs\NUMECA
software\AutoBlade131\AutoBlade.
The AutoBlade™ graphical user interface includes several sections that enable the simultaneous
visualization of the designed or fitted blade geometry. Access to the main menu and controls is
provided through a menu bar and a quick access pad (QAP), and is complemented with a tool/
icon bar.
1.2
BLADE FITTING
In this tutorial, the target geometry provided by a geomTurbo of the marine propeller will be fitted
and parametrized. The fitting process is an optimization process that consists of minimizing the
distance between the parametric model and the target geometry (predefined geomTurbo). Several
fitting steps may be needed during a blade fitting.
1.2.1
Create new AutoBlade™ project
1. Click on the button Create a new project to create a new AutoBlade™ project.
2. Select the button Start from scratch and click on the button Ok to confirm.
3. Select a directory and enter the project name <DTMB_fitting>, then click on the button Save to
confirm.
1.2.2
Define the target model
4. Click in the QAP on Target Settings to expand it, then click on the button
target geometry file.
to specify a
5. Go to the directory where the target geometry (the .geomTurbo file) is available and select the
geometry file "tutorial_1.geomTurbo". Click on Open. A warning appears informing that the
loaded geometry is not sliced into sections. Click on ok.
6. In order to create the sections, click on the button
.
7. Enter <8> <Enter> for the Number of sections.
8. Enter the following value as Spanwise locations: <0.01 0.2 0.4 0.6 0.8 0.88 0.95 1> <Enter>.
Click on Ok.
1.2.3
Define the initial model
9. Click on the button
in the tool bar to import a predefined template.
10. Click on the button
template, click on the button Ok to confirm.
and select "marine propeller" in the list to import the predefined
Before the initialization and fitting processes take place, a starting model must be defined with
topological settings that are well adapted to the target geometry. It is usually advised to load a
template or an existing parametric model close to the target geometry. Then the user should review all
design steps and modify the settings if necessary.
The marine propeller has been developed from the PPTC marine propeller featuring a rounded tip
topology. More details in the AutoBlade™ User Guide.
11. Review all the design steps in the Model Editor in the QAP.
l Click on Endwalls, under Hub endwall, change the Curve to Composite by using the button
. Click on the Insert button to add an element and change both element types to LINE by
using the button
confirm.
. Keep the settings under Shroud endwall. Click on the button Ok to
l Click on Stream surfaces, unselect the Rounded tip and keep the others settings. Click on
the button Ok to confirm.
l Click on Main blade, under Side curves, select blunt for the TE shape. Keep the others
settings. Click on the button Ok to confirm.
Improper settings will result in poor fitted models. Check all the design steps to be sure:
l use suitable topology,
l use an adequate number of parameters.
A new pre- fitting is required each time the topology and/ or the number of parameters are
modified.
1.2.4
Pre-fitting
12. Click on Fitting Control in the QAP to expand it, then click on the button Adapt model to
start the pre-fitting process.
Once the target and initial models are defined, a pre-fitting process must be performed.
The pre-fitting process will:
l Guess values for the parameters that define prescribed curves and laws (end walls, sweep laws,
camber curves,...).
l Find the best traces for planar, cylindrical and conical stream surfaces.
l Change the amount of primary sections and their spanwise locations.
l Freeze some parameters that are unlikely to improve the model in the fitting process.
l Initialize the lower and upper bounds of the parameters of the geometrical model.
The pre-fitting process will not:
l Make suitable choices for the topology definition.
l Capture special shapes for edges (including sharp ends).
l Check that the pressure and suction sides coincide with the legend of 2D views.
Pre-fitting remains an approximation and a fitting should always be executed afterward.
13. Click on Ok to confirm.
14. Click on Yes in the warning message dialog box to start the pre-fitting process.
15. After the pre-fitting process is finished, activate the button Show projection in Target
Settings in the QAP to check the difference between the target geometry and the parametric
geometry in the MERIDIONAL view and the B2B view.
16. The parametric hub settings are not adapted to fit the target hub. The control points of the line
can be changed to match the relevant hub shape. In the MERIDIONAL view, left-click on the
hub curve, control points will appear.
17. Left-click on the center control point as it turns red. In the keyboard area, enter the following
coordinates <0.067091 0.03082 0> <Enter>.
18. Click on the button
in the tool bar and select "section 8" to compare the difference of the
section 8 in the B2B view. Click on the button
to zoom in/ out the B2B view.
1.2.5
Fitting
19. Click on the button Fit model in Fitting Control in the QAP to start the first fitting process.
20. Select the feature hub_curve from the Selected features and use the button
from the selection.
to remove it
21. Click on the button Ok to confirm, then click on the button Yes to start a coarse fitting
process.
The first fitting process is usually a coarse process because the topological settings could be wrong or
bounds of some parameters are reached early. In such a case, a fine fitting process is useless.
22. After the fitting process is finished, click on the button
access the fitting graph window.
in Fitting Control in the QAP to
23. Choose "M_ RTHETA_ SECTION" for Category and "SECTION_ 3_ SPAN_ 39" for
Selection using the button
geometry of the section 3.
to compare the parametric geometry (fitted result) and the target
24. Click on the button Close to close the fitting graph window.
25. Click on the button
window.
in Fitting Control in the QAP to access the convergence graph
26. Select "10" for Fitting step and "S8_CAMBER_H2" for Graph to view the convergence
history of the parameter S8_CAMBER_H2 in the fitting step 10.
27. Click on the button Close to close the convergence graph window.
28. Select the menu Analysis/Parametric report..., some free parameters are blocked.
The number of blocked free parameters should always be checked before launching the next fitting
process. This number should be 0, so that the next fitting process is able to further improve the value
of the parameters.
29. Click on the Free tab and keep the Show blocked free parameters only option active. The
blocked parameters are listed including "S8_CAMBER_H2".
30. Click on the button Close.
31. Select the menu View/Show parameter status to display the status in the parameter list
window.
32. Select the menu Geometry/Parameter list... to check and modify the bounds and the current
value of the parameters:
l select "all" for Group using the button
,
l write <CAMBER_H> for Filter,
l As it was seen in Show blocked free parameters only list, some camber parameters are
blocked. Increase the bounds to unblock them by clicking on Increase all.
l Click four times on that button, then click Apply and OK.
33. Click on the button Fit model in Fitting Control in the QAP. Keep the default settings and
click on the button Ok to confirm, then click on the button Yes to start a second coarse fitting
process.
34. Select the menu Analysis/Parametric report..., the invalid parameters is 0 and the free
blocked parameters is 1 (the parameter "HUB_R3" under the Free tab is related to the control
point that has been placed previously), click on the button Close.
35. Click on the button Fit model in Fitting Control in the QAP to start the third fitting process.
36. Set the Accuracy to Fine, click on the button Ok to confirm, then click on the button Yes to
start a fine fitting process.
37. After the fitting process is finished, click on the button
access the fitting graph window.
in Fitting Control in the QAP to
38. Choose "M_RTHETA_SECTION" for the Category and "SECTION_1_SPAN_0" for the
Selection using the button
in the blade section, compare the fitted geometry and the target geometry.
, click once in the graph, move the cursor and click again to zoom
The radius at the leading edge or the trailing edge can be difficult to capture. The fitting can be
improved by imposing the value of the radius manually.
The fitting process can be launched several times, until the fitted geometry is sufficiently close to the
target geometry.
39. Click on the button Close to close the fitting graph window.
1.3
SAVE THE PROJECT
40. Select the menu Geometry/Export options....
41. Click on the geomTurbo tab in the Export settings dialog box, click on the button Ok to
confirm.
© NUMECA International, all rights reserved
EN201808281221

CONTENTS
NEW FEATURES IN V13
1.1 Flexlm based security ID updated to v18 (All Products)
1.2
Improve administration wizard
NEW FEATURES IN V13
This document provides a description of the new capabilities and major improvements included in
AutoBlade™ v13, as well as statements outlining main customer benefits and known limitations.
The following is a detailed list of new capabilities and enhancements in AutoBlade™ v13:
All Products:
Flexlm based security ID updated to v18
"Improve administration wizard" (p. 4)
Finally, the following is a detailed list of existing capabilities and enhancements included in
AutoBlade™ but still requiring additional calibration
List of existing BETA capabilities
New parametric template for turbocharger
Improvement in generation of solid sectors
Improved solid sector periodic face generation
1.1
FLEXLM BASED SECURITY ID UPDATED TO
V18 (ALL PRODUCTS)
(New in AutoBlade™ v13.1)
(All Products)
AutoBlade™ requires FlexLM based license keys for execution. In AutoBlade™ v13, the
security ID has been upgraded to v18, thus requiring the delivery of new license keys for
execution.
Customer Benefits
None
Known Limitations
None
1.2
IMPROVE ADMINISTRATION WIZARD
(New in AutoBlade™ v13.1)
(All Products)
The user-friendliness of the license management and diagnostics of the administration wizard is
improved:
l License Management>Product (de)activation: Deactivate button to return all fulfillment and all
servers on the machine.
l License Management>Trusted storage: check-box to return a fulfillment and refresh button to
refresh the fulfillment status if needed.
l License Management>License server: control and display the status of the known servers and
the list of all the features deserves by the selected server.
l Diagnostics: Support request button to generate a file containing the results from the checks
performed.
Customer Benefits
More user-friendly tool to diagnose and manage licensing.
Known Limitations
None
AutoBlade™ 13.1 What's New?
© NUMECA International, all rights reserved
EN201808281624

Best practices 

NUMECA's product strategy is based on the development of automated, integrated and customized software systems for rapid and reliable meshing, simulation, design and optimization. Our software solutions closely follow the industrial requirements for a broad range of applications.
The best practices, sorted by application as listed below, provide guidelines for the entire simulation process. Most of the best practices are designed so as to limit use of expert parameters.

Grid Representation - On a Solid Surface

Best Practice: Capture High Quality Pictures of the Grid
Software: CFView™ v10.1-1.
Application: Power & Propulsion, Aerospace,
 Automotive, Marine, Hydro, Wind Energy, Architecture &
 HVAC, Oil & Gas, Healthcare.

Introduction
The objective of this best practice is to show
 the basics of how to create high quality pictures of a mesh on a surface
      in CFView™.      


FIGURE 1 Mesh from a plane (very thin lines quality)
Visualization
Below are the general guidelines from NUMECA to realize high quality pictures in CFView™:

Put CFView™ in full-screen;
In File -> Print ... menu, select Active View, deactivate the Frame option, set the size to 1920x1080 (Full HD definition) and quality parameter to Thin lines or Very Thin Lines depending on the mesh density to capture (see Output Generation).

Grid on a solid surface
CFView™ enables the user to View Grid Wireframe. Below are the guidelines from NUMECA to realize high quality pictures:

Show the grid wireframe;
Turn Gouraud Shading on;
Modify Rendering Color to a light color to get a good contrast.


  

FIGURE 2 Comparison quality High (default), Thin Lines, Very Thin Lines.
Note that the size of the file is increased with respect to the quality.

Recommendation to capture other physics on a similar case
Scalar Quantity - Cartesian Plot

Scalar Quantity - Contours & Isolines

General Guidelines

Flow separation

Best Practice: Identification of flow separation (draft)
Last update on:24/Jul/2018
Software: CFView™ 12.1.
Application: Aerospace,
 Automotive, Architecture, Healthcare.
Validation data: none
            
Classification of the case:


External Aerodynamics;
3D case;


Introduction
The objective of this best practice is to show the basics  identifying the location of flow-separation based on the shear-stress. This report is based on the DLR-F4 geometry  that is available as a part of the FINE™/Open with OpenLabs™ tutorial  on the DLR-F4 Wing Body. 
The example macro is specific to the DLR-F4 case but can serve as an example to make a similar macro for other cases.


FIGURE 5 Velocity vector lines around the DLR-F4 with a 3 degree angle of attack and M = 0.75.
Flow separation visualization

Flow separation can be identified with multiple techniques such as visualizing vector lines, vectors and friction velocity lines. In this example, flow-separation is identified through the viscous stress on surfaces. The basic underlying principle is that the viscous stress in the streamwise direction exerted by the fluid on the wall at the point of separation is zero.


Select the Viscous stress (wall to fluid) quantity in the Output Parameters in the FINE™/Open GUI (see Data). 


In CFView™ load the viscous stress in the streamwise direction:
Quantity\Field Data\Vector Components\Viscous stress (wall to fluid)_X if X is the streamwise direction. 
If the streamwise direction is not along any of the coordinate axes, create a derived quantity taking into account the components of shear stress in the streamwise direction (see: Create Derived Quantity).


Create a local isoline of the viscous stress in the streamwise direction of value 0: Representation/Isolines/Local Isoline (see: Isolines). The generated Isoline of value 0 divides the regions of separated flow from the unseparated flow.
The CFView™ macro Separation-shear-stress.py can be used to perform the above steps. 


FIGURE 6 The Isoline of 0 viscous stress in the streamwise direction divides the regions of separation from non-separation.

Scalar Quantity - Cartesian Plot

Best Practice: Plot and Compare Scalar Quantities 
Software: CFView™ v10.1-1.
Application: Power & Propulsion, Aerospace,
 Automotive, Marine, Hydro, Wind Energy, Architecture &
 HVAC, Oil & Gas, Healthcare.

Introduction
The objective of this best practice is to show
 the basics of how to create Cartesian plots
      in CFView™. 


FIGURE 1 Plot of the friction coefficient
Visualization
Below are the general guidelines from NUMECA to realize high quality pictures in CFView™:

Put CFView™ in full-screen;
In File -> Print ... menu, select Active View, deactivate the Frame option, set the size to 1920x1080 (Full HD definition) and quality parameter to Thin lines (see Output Generation).

General guidelines on Cartesian plots
In order to get similar Cartesian plot style, please follow those general guidelines:

Indicate units in the axis label;
Do not show more than 4 curves in one plot;
Represent experimental data as symbols only (see Update Curve Type);
Represent results from calculation as symbols and line (see Update Curve Type);
Use different  color tones;
Choose different line style and symbols for each curve such that they can be distinguished also when printed in black & white (Symbols of diamonds, times, plus, boxes or circle should be preferred);
Give intelligible names to the curves (see Manage Legend in Cartesian Plot).

CFView™ Interface
Below are the recommendations from NUMECA to capture correctly the details from a graph in CFView™:

Show H Grid Lines (see Add Grid Lines in Cartesian Plot);
Show V Grid Lines (see Add Grid Lines in Cartesian Plot);
Set axis label and scale font size respectively to 40 and 30;
Set filled marker size to 0.2 and line thickness to 2 to show the results from calculation;
Set marker size to 0.4 and hide line to show experimental data;
Set the legend font size to 30 (see Manage Legend in Cartesian Plot).

Recommendation to capture other physics on a similar case
Grid Representation - On a Solid Surface

Scalar Quantity - Contours & Isolines

Center of pressure

Best Practice: Identification of the center of pressure (Draft)
Last update on: 31/Jul/2018
Software: CFView™ 12.1.
Application: Aerospace,
 Automotive,   Architecture, Healthcare.
Validation data: none
Classification of the case:


External Aerodynamics;
3D case;


Introduction
The objective of this best practice is to show the basics  identifying the center-of-pressure in CFView™. This report is based on the DLR-F4 geometry  that is available as a part of the FINE™/Open with OpenLabs™ tutorial DLR-F4 Wing Body). 
The example macros are specific to the DLR-F4 case but can serve as an example to make a similar macro for other cases.


FIGURE 2 Velocity vector lines around the DLR-F4 with a 3 degree angle of attack and M = 0.75.
Definition center of pressure

The center of pressure (CoP) is a point where the total sum of a pressure field acts, causing a force and no moment to act around that point. Consider the force vector  acting on an aerodynamic body. The objective is to find a point  for which the resulting moment  . 


General set of equations

The moment of the body around the origin  can be calculated in CFView™ or obtained from the .wall file output in the FINE™/Open computation. The moment arm from the origin is referred to as .






A  system of linear equations has a unique nontrivial solution if and only if its determinant is non-zero. IF the determinant of   is zero the system has either no nontrivial solutions or an infinite number of solutions.  


2D and symmetric 3D bodies
Derivation of applicable equation

For two-dimensional and laterally-symmetric three-dimensional bodies (such as a 3D symmetric-airplane with no cross (lateral) flow), the number of points of center of pressure are infinite. For 3D-symmetric bodies that have a lateral symmetry the CoP lies on the symmetry-plane. The force perpendicular to the symmetry-plane and the moments parallel to the symmetry-plane are 0. 
For a 2D body or a symmetric 3D body (symmetry-plane perpendicular to Z-axis), then the following quantities have a value of 0:

 force along the Z-axis ,  
moment along the X-axis, ,
moment along the Y-axis, . 

This leaves for the moment perpendicular to the symmetry-plane :



The above equation has an infinite number of solutions. The same logic can be extended to other directions when the symmetry-plane is aligned along X or Y-axis for symmetric 3D bodies.


Example: DLR-F4

The DLR-F4 geometry is simulated with Mach Number 0.75 and a 3 degree angle of attack. The geometry is symmetric along the Y-axis. As there are no cross-winds, the geometry experiences forces symmetric with respect to the  Y-axis. With the help of the python macro (CoP-2D-and-3D-symmetric.py), the solutions to the above equation are displayed in CFView™ as shown in the figure. The markers () in the image show a few of the possible solutions for the CoP.


FIGURE 3 Various possible centers of pressure are displayed on the symmetry-plane as markers (). 


Non-symmetric 3D bodies
Reduction of applicable equations

For general three-dimensional bodies, the center-of-pressure (CoP) does not exist as the system of equations  does not have a solution. In such cases the user can fix a reference-plane  (eg. ) and find a point where the moments  parallel to the plane (i.e  and ) are 0. The location of such a point is found by solving for two equations from the system of equations and the user-defined reference-plane.


Example: DLR-F4 with crosswinds

In the following example, the DLR-F4 geometry has crosswinds and thus it is no longer symmetric along Y-axis. By constraining the point on the Z-axis with , a point can be obtained where the moment along X   and the moment along Z  are 0. The script CoP-3D-non-symmetric.py identifies and creates a marker in CFView™ where the moments  and  are 0. Note that the moment along  for that point is not 0 and thus it is not the true center of pressure.






FIGURE 4 The 3D body experiences non-symmetric forces. A point () is found where  and  are 0.

Scalar Quantity - Contours & Isolines

Best Practice: Capture and Compare Scalar Quantities on a Surface
Software: CFView™ v10.1-1.
Application: Power & Propulsion, Aerospace,
 Automotive, Marine, Hydro, Wind Energy, Architecture &
 HVAC, Oil & Gas, Healthcare.

Introduction
The objective of this best practice is to show
 the basics of how to create high quality standardized pictures of color contours and isolines on a surface
      in CFView™.      


FIGURE 1 Pressure coefficient color contour and isolines on the symmetry plane of a car.
Visualization
Below are the general guidelines from NUMECA to realize high quality pictures in CFView™:

Put CFView™ in full-screen;
In File -> Print ... menu, select Active View, deactivate the Frame option, set the size to 1920x1080 (Full HD definition) and quality parameter to Thin lines (see Output Generation).

Before realizing any color contour or isoline, the user may define the color map:

In Preferences ->Colormap type ..., in the Text tab set the Legend Type Size to 32 or more and the Numbers Type Size to 30 or more;
In Preferences ->Colormap type ..., in the Colors & Position tab, set the colormap position and the coloring type at convenience.

At the end of CFView™ session, the system will ask whether those changes should be saved or not to the user (see Edit, Save & Restore Defaults). 
For a single modification on a specific window, the user can make local change by right-clicking on the color map or its legend (see Update Colormap Representation).
Comparison from a macro
For comparison, it is important to use a standardized camera position and identical settings for each picture. The easiest way to do so in CFView™ is to use macro scripts (Templates & Macro Scripts).
CFView™ enables the user to record its actions in the GUI. Then, the camera position and all the parameters that make a picture are set by the user once for all in a macro:

Clear Active Macro

Record User Actions

Save Active Macro


Finally, the user can reproduce the picture from the saved macro: Execute Macro Script Data File.
Contours
The user can capture scalar quantities from color contours in CFView™. Below are the recommendations from NUMECA to realize high quality pictures:

Set a consistent colormap range for comparison (see Control Representations Range);



FIGURE 2 Turbulent viscosity over a backward facing step.
Isolines
The user can capture scalar quantities from isolines. Below are the guidelines from NUMECA to realize high quality pictures:

set the Line Type thickness to 3 (see Modifying the Isolines);
Colored Isolines:

show colormap (Colormap & Representations Range);

Uniformed Isolines:

hide colormap (Colormap & Representations Range);
show values on the lines (see Modifying the Isolines);
set the value font size to 30 or more (see Modifying the Isolines).




FIGURE 3 Velocity magnitude over a backward facing step .

CFView™ enables the user to compare results from different views in the same window using Align Views and Superpose Views commands (see FIGURE 4). When making the output picture, in File -> Print ... menu, select Graphics Window instead of Active View to print both views at the same time.


FIGURE 4 Comparison of the velocity magnitude over a backward facing step for k-w SST model (color) and Spalart-Allmaras model (uniform).

Recommendation to capture other physics on a similar case
Scalar Quantity - Cartesian Plot

Grid Representation - On a Solid Surface

Power & Propulsion
The following best practices are available for Power & Propulsion applications:

Rotor/ stator interfaces

Best Practice
Last update on: 16/11/16. 
Software: AutoGrid5™, IGG™, HEXPRESS™, HEXPRESS™/Hybrid,
  FINE™/Turbo, FINE™/Open with OpenLabs™.
Application: Power & Propulsion, Hydro, Wind Energy, Oil & Gas.
Validation data: none
Other: Rotating machinery
Classification of the case:


 Internal Aerodynamics;
With rotating machinery parts
Type of BC's: rotor/ stator interface


Introduction
The objective is to set-up best practices for the location of the rotor/ stator interface and settings.
Meshing guidelines
Rotor/ stator interface location
Using Autogrid5™, the rotor/ stator interfaces are automatically located at mid-distance between consecutive rows. However, it is possible that this choice is not the best one. Furthermore, mixing an Autogrid5™ mesh with external ones (for instance with an unstructured volute mesh) also requires a knowledge on where to place those interfaces.
As a general remark, it is advised not to put rotor/ stator interfaces within a recirculation region. Indeed, rotor/ stator treatment is generally using an approach based on the distinction between upstream and downstream patches (for each span-wise location). Therefore, a clear distinction is more difficult to establish if a recirculation exists. Such a recirculation region can be produced by a blunt trailing edge at the back of a centrifugal impeller or by a back-step between consecutive elements (impeller and volute for instance). A sketch of possible configurations and best locations can be found in the following figure.


FIGURE 1 Rotor/ stator interface positioning

Case set-up guidelines
Rotor/ stator interaction treatment
Choosing the appropriate type of rotor/ stator interface is also of importance. In general, a mixing-plane approach will be selected. In many cases this is the most relevant choice. However, in case of a shock impacting the rotor/ stator interface, this could lead to spurious losses of entropy. The non-reflecting treatment can improve such a behavior (but, to the price of a loss in mass conservation) as illustrated in the following figures. 


FIGURE 2 Absolute Mach number contours on an axial cut upstream of the rotor-stator interface. An optimal range of the field is shown to facilitate clarity.
While the three top images show similar results (the differences are very subtle and essentially in this case they portray the implementation of the same approach), the images corresponding to the 1D and 2D Non Reflecting conditions are different from the other images especially in the wake and near the hub showing less diffusion in these areas.
Similar observations can be made downstream of the interface, although the differences are harder to spot in Figure 3 due to the mixing.


FIGURE 3 Relative Mach number contours on a axial cut downstream of the rotor-stator interface. An optimal range of the field is shown to facilitate clarity.
The difference here is more pronounced in the middle of the domain where the 1D and 2D Non Reflecting conditions show the effect of the upstream wake on the mixing downstream.
In general, it is preferable to start with the Full Non Matching Mixing Plane or the Conservative Coupling by Pitchwise Rows approach . These will most often provide a stable solution with good mass flow conservation. In case a shock is present or the solution is unstable, the 1D or 2D Non Reflecting approach could be used. However, when using this approach, attention should be paid to the mass flow conservation as the Non Reflecting approaches are not conservative by nature.
If an impeller is connected to a volute, a local conservative coupling can be preferred. An even better approach is to use a Non-Linear-Harmonic method (with only one harmonic if we are interested in just capturing the impeller - volute interaction).

As a guide, the following flow chart can be used. These choices are to serve as guide rather than a definitive manual. It essentially showcases what would be the most appropriate method with which to start the analysis.




FIGURE 4 Decision flow chart for the choice of the rotor-stator treatment.

Linear Eddy Viscosity Turbulence Models

Spatial Discretization
The discretization in space is based on a cell centered finite volume approach. Let us write the conservative finite-volume formulation explicitly. 
Considering a discrete volume Ω encompassed by the surface S, the integral conservation laws are written:



where  contains here the inviscid and viscous part of the fluxes:



where  and  are the inviscid and viscous part of the fluxes respectively. These equations should be solved over control volumes ΩJ. Finite-volume discretization gives the following discrete form:



where *  is the numerical flux, sides refers to the external sides of the control cell ΩJ and  is the non-unitary normal vector to the considered side. 
Viscous Fluxes
The viscous fluxes are determined in a purely central way. As they contain gradients, gradients must be evaluated on the cell faces. This is done by applying Gauss' theorem over a volume encompassing the considered face:



Applying a finite volume discretization and considering stationary control volumes, the relation becomes:

, or 
The theorem is applied over a diamond control volume formed by the face vertices and its neighboring cell centers as opposite summits.





FIGURE 5 Diamond control volume approach for gradient computation on faces
The diamond control volume method requires knowledge of the flow quantities at the cell vertices. The choice of an appropriate interpolation method has to be made in order to ensure accurate transfer from cell centers to vertices. This gives the following expression for a quantity Q to be interpolated in a vertex p surrounded by n cells:



A linearity-preserving interpolation, based on the pseudo-Laplacian formula of Holmes and Connell (1989), is used. The value of Q at vertex p is obtained by the above formula, where the weighting functions ωi are defined by:



where Δxi, Δyi and Δzi are the three coordinates differences between cell i and vertex p (Δxi = xi - xp,...). The weighting coefficients λx, λy and λz are computed by assuming that above interpolation should be exact for a linear evolution of Q. Hence we can write:



Rewriting interpolated equation under the following form:



and injecting above equation in this formula, we obtain:



For linear functions, this relation should remain valid for any value of the derivatives. Since there are three unknowns determining ωi, let us choose three particular sets of derivatives, so that we obtain the following three equations from above relation, where ωi is replaced by its definition involving the unknowns λx, λy and λz:



This system of three equation with three unknowns λx, λy and λz can easily be solved since only a symmetric 3x3 matrix must be inverted for each vertex. Moreover, this needs to be done only once during the flow calculation process because, as seen in this expression, the unknown weighting coefficients do not depend on the solution but only on vertex and cell center coordinates.
Inviscid Fluxes
The following form is used to express the inviscid numerical flux across a face k bounded by two cells L and R:



where the first term on the right hand side corresponds to a purely central evaluation of the inviscid numerical flux vector, and the second term dk is called the numerical dissipation term. It may be an artificial dissipation, used in combination with central schemes, or the dissipation associated with upwind schemes.








FIGURE 6 Notations for the inviscid flux formulation
Alternatively, instead of averaging the fluxes, a flux based on the averaged unknowns can be formulated:



In the FINE™/Open solver, the flux averaging formulation is used for internal faces, and the solution-averaging formulation is used on boundaries. Notice that since  denotes the unit normal vector to face k throughout the whole manuscript, we should multiply the above expressions by the face area in order to recover the numerical flux. Hence we have:



where ΔSk is the area of face k.
The central scheme is the default scheme in the FINE™/Open solver. Roe upwind scheme is also available.
Central Scheme
In the central scheme, the scalar artificial dissipation term in equation is formulated by Jameson, Schmidt and Turkel (1981) as a blend of second and fourth-order differences of the conservative variables:



where δUk is the solution first-order differences in face k, δ²UL and δ²UR are the second-order variations in the left and right cell centers. The second and fourth-order scalar coefficients in faces are given by:



and the fourth-order coefficients in cells (, ) relative to one local direction are obtained by arithmetic averaging the fourth-order coefficients on opposite sides, themselves obtained by arithmetic averaging the fourth-order coefficients on their constitutive faces, as shown in FIGURE 7




















FIGURE 7 Calculation of the fourth coefficient in cells
The term  is the spectral radius, i.e. the maximum eigenvalue of the flux Jacobian projected in the direction normal to face k. Using hexahedral control volumes, three local directions, namely ξ, η and ζ can be defined for each cell, see FIGURE 7. The spectral radius  on face k is then obtained by arithmetic averaging the spectral radii in its neighboring cells, evaluated in their local direction corresponding to the face. For the example of FIGURE 7, we have:



where , cL and , cR are the velocity vector and the speed of sound in the left and right cells respectively, and ,  are the unit normal vectors calculated at the center of the left and right cells, in their respective local directions corresponding to face k, see FIGURE 6.
On high aspect ratio meshes, the dissipation in the streamwise direction may become very low. Increasing it may improve the robustness and the convergence rate, although perhaps at the expense of a lower accuracy in such cells. As seen above, before being transferred to faces, three spectral radii are evaluated in cell centers, in the directions corresponding to their local frame of reference. Martinelli (1987) has defined modified spectral radii in each direction by taking into account contributions from the two other directions. For instance, the modified spectral radius in local direction ξ for cell L is given by:



where σ is the Martinelli coefficient, whose default value is 0.5.
The non-dimensional coefficients νL, νR are pressure and temperature variations (depending on the value for the expert parameter spc_TswitchInArtDissip_), which act as sensors to activate the second-order dissipation in regions of strong gradients, e.g. shocks, and to deactivate it elsewhere. 
For instance, we will have for cell L:



where pL-1 is obtained by arithmetic averaging the pressure in all the cells located on the left side of cell L in the considered direction. Similarly, pL+1 is obtained by averaging the pressure in all the cells located on the right side of cell L. Notice that the size and shape of these cells are not taken into account, see FIGURE 8. This is, however, not important since the pressure switches are simply indicators of zones of large gradients. Also note that in our formulation of , only the pressure switches of the neighboring cells of face k are involved whereas in the classic Jameson formulation, four switches are used, namely those of the face neighboring cells as well as of these cells' neighbours. However, this is unsuitable in the context of unstructured adapted meshes since each neighboring cell can itself have one, two, three or four neighbours, whose identification is not straightforward. Finally,  and  are user-defined coefficients, usually equal to 1.0 and 0.1 respectively. They correspond to the non-interfaced expert parameters spc_artDiss2ndCoef_ and spc_artDiss4thCoef_.







FIGURE 8 Pressure switches (cell L)
Central matrix scheme
Starting from the standard scalar scheme of Jameson-Schmidt-Turkel (JST), a matrix dissipation scheme can be easily constructed by substituting the spectral radius with the absolute value of the flux jacobian:



With the second and fourth dissipation coefficients given now by:



The pressure switch has the same definition as for the central scalar scheme.
Now, the dissipative terms for each equations are scaled by the appropriate eigenvalues of the flux Jacobian of the system, rather than the spectral radius.
The central matrix dissipation term is constructed as the upwind scheme dissipation term. The advantage of this formulation is that one reduces the computational cost of the numerical scheme. One has



where L-1  is the matrix of the left eigenvectors of the jacobian matrix of the Euler system in the primitive variables, whereas P is the matrix of the right eigenvectors of the jacobian matrix of the Euler equations expressed in term of conserved variables. The matrix Λ is the diagonal matrix of the eigenvalues of the system. The differences δVk are expressed in terms of the primitive variables (ρ,u,v,w,p). The matrix |Λ| is the diagonal matrix of the absolute value of the eigenvalues (λ)i=1,5 with:



Near stagnation points and sonic points, some of the Jacobian eigenvalues can become very small and would lead to numerical difficulties. This can be avoided by introducing a fix on the eigenvalues of the absolute Jacobian:



Where σ is the spectral radius of the jacobian matrix. The parameters merkle_matdisEntrFx_ and hakimi_matdisEntrFx_ (to be applied when using Merkle and Hakimi preconditionner, respectively) are controlling the entropy fixes. These expert parameters are vectors of two components. The first component corresponds to Vl, and the second to Vn. The default values are (0.1 , 0.1) for merkle_matdisEntrFx_, and (0.3 , 0.3) for hakimi_matdisEntrFx_.
Note that the Hakimi low-Mach version is not compatible with CPU Booster, and that the incompressible Hakimi version is limited to isothermal flows.
Upwind Schemes

Roe type upwind scheme is also available in the FINE™/Open solver.
First Order Roe Scheme
In the FINE™/Open solver, two expressions of the dissipation term dk are available:

the "standard" dissipation.
the "isenthalpic" dissipation that allows the scheme to admit constant total enthalpy while dealing with steady flows. This property is satisfied by expressing the dissipation term dk using enthalpy instead of total energy in the energy equation.

The expert parameter upw_dissipEnthalpy_ controls the use of the standard or isenthalpic dissipation. The default option is the standard dissipation. 
The parameter upw_dissip_ext_ controls the calculation of the dissipation at the inlet and outlet boundaries. If it is 1, the dissipation is calculated at this boundaries, if 0 the dissipation is not computed. Actually by default, the dissipation is calculated at inlet-outlet boundaries. For turbomachinery applications, we advise to not calculate the dissipation at inlet-outlet boundary. Indeed, it was found in this case the mass flow errors are greatly reduced. 
"Standard" Dissipation
In the upwind scheme, the dissipation term dk on a given face k is expressed as follows:



where L-1 is the matrix of the left eigenvectors of the Jacobian matrix of the Euler system in the primitive variables, whereas P is the matrix of the right eigenvectors of the Jacobian matrix of the Euler system in the conservative variables, described in e.g. Hirsch, 1990. |Λ| is the diagonal matrix of the eigenvalues of the system. In order to avoid unphysical solutions such expansion shocks, an entropy fix is used. The absolute values of the eigenvalues are limited as follows:



where  for the linear field (the characteristic variables that propagate with speed ) and  for the non linear field, EntrFx_ are two user-defined parameters that generally vary between 0.001 and 0.3. In subsonic and transonic cases, small values suffice (EntrFx_ = 0.001). For flow simulations in high-speed regime and when shocks are aligned with the mesh (especially for detached shock), it is advised to choose higher values for these parameters (EntrFx_ = 0.3).
The expert parameter EntrFx_ is a vector of two components, the first component is applied to the linear field, and the second component is applied to the non-linear field. By default, the two components are set to 0.01.
δVk is the first-order difference in face k of the primitive variables, namely density, velocity and pressure:



where L and R denote the upwind and downwind cells respectively. The terms in the matrices are evaluated on face k by Roe averaging:

, , 
The upwind scheme is presently only available for compressible flows when not using the preconditioning method for low-Mach flows.
"Isenthalpic" Dissipation
In the case of steady flows, the total enthalpy H is constant. The standard Roe scheme with the dissipation term dk  does not necessary satisfy this property. This may be remedied by calculating the dissipation term dk in the same way as the standard Roe scheme but according to the modified state vector:



Therefore the dissipation term dk reads:



where R is the matrix of the right eigenvectors of the Jacobian matrix of the Euler system in the new set of variables. |Λ| is the diagonal matrix of the absolute values of the eigenvalues of the system. As for the standard discretization, an entropy fix is used in order to avoid unphysical solutions. The same parameter EntrFx_ controls the fix for the linear fields and non-linear fields. The quantity δWk is the first order difference in face k of the variables. The terms in the matrices are evaluated on face k using the Roe averaging.
Second Order Roe Scheme and Limiters
When the "left" and "right" values of the variables used in the previous formulation are the upwind and downwind cell values respectively, the Roe scheme is first-order accurate. A higher order of accuracy can be achieved through the process of solution reconstruction.
Reconstruction is the process of constructing, within each control volume, a continuous, usually polynomial, representation of the solution from the discrete data. Discontinuities are, however, allowed at the control volume interfaces, hence, the representation is piecewise continuous.
When computing the inviscid flux on a given face, the flow quantities in its neighboring cells are no longer used to define the Riemann problem. Instead, reconstruction is used to obtain more accurate estimates of the "left" and "right" states.
Reconstruction methods are classified by their order, which corresponds to the highest degree of the polynomials they can reconstruct exactly.
In order to build a second-order accurate scheme, a linear reconstruction must be used. The reconstructed flow solution on face k, bounded by cells L and R, is represented, on each side of the face, as a - piecewise - linear polynomial of the form:



where  and  represent the solution gradients in cells L and R, respectively. In the case of the "standard" dissipation, the reconstruction step is performed on the set of the primitive variables whereas for the "isenthalpic" formulation the reconstruction is made on density, velocity and total Enthalpy. In both cases, the calculation of the gradient is conducted using the Least Squares method. 
The least squares approximation is used to evaluate the flow quantities gradients in cell centers. The principle is the following: by requiring that the linear polynomial expression  holds at each of the direct - or first-order - neighbours of a given cell c0, the following over-determined linear system of equations is obtained:



where N is the number of first-order neighbours. The system is solved in the least square sense by pre-multiplying through by the matrix transpose to yield the symmetric 3x3 system:



where Δxi is equal to xi - x0, and so on for the other variable differences involved in the system.

When solution discontinuities and steep gradients are present, additional steps must be taken to prevent oscillations developing in the numerical solution. In the FINE™/Open solver, the monotonicity is enforced through the reconstruction step using the Barth and Jespersen (1989) technique
In the linear polynomial expression, the gradients  and  are limited in order to enforce the reconstructed solutions  and  to satisfy monotonicity requirements. The reconstructed flow solutions on face k, bounded by cells L and R, are now given by:



where  and  are the limiters computed in cells L and R, respectively. The limiters are computed such that the reconstructed flow solutions satisfy the following monotonicity criterion:



With



where Uj and Ul are the immediate neighbours cells values of the cells L and R, respectively. Two kinds of methods to calculate ΦL and ΦR, Barth & Jespersen (1989) and Venkatakrishnan (1995), are provided in the FINE™/Open solver.
In several publications it is reported about the deficiencies of the Barth-Jespersen limiting procedure (e.g., Marques & Pereira (2001), Berger et al. (2005), Venkatakrishnan (1995)): One of the mentioned drawbacks of the scheme is that the convergence often stalls after that the residual has dropped a few order in magnitude. A second issue is that the Barth-Jespersen limiter functions are too sensible to small variations in the flow field, which can cause an introduction of excess numerical diffusion in free-stream regions.
To avoid that the convergence stagnates due to limit cycles, Venkatakrishnan (1995) suggests to incorporate the van Albada limiter in the Barth-Jesperesen technique. More details can be found in Venkatakrishnan (1995).
The user can activate the computation of the limiter by setting the expert parameter upw_limit_ to 1. Then the expert parameter upw_limitVenka_ can be used to choose if the Barth-Jespersen limiter is used (upw_limitVenka_=0) or the Venkatakrishnan limiter is used (upw_limitVenka_=1).
In the FINE™/Open solver, the limiters are calculated only at the first stage of the Runge Kutta scheme and only on the finest grid. This approach reduces the computational cost substantially. The recalculation of the limiter at each stage of the Runge-Kutta scheme is governed by the (vector) parameter spc_iCalcLim_ as the parameter spc_iCalcDissip_. Actually, by default, only the first component of spc_iCalcLim_ is equal to 1. If all components are equal to 0, the scheme reduces to first order accurate.

NOx formation
Overview
In combustion processes, the formation of nitrogen oxides (NOx) is one of the major pollution sources. Although nitrogen oxides encompasses the three species NO (nitric oxide), NO2 (nitrogen dioxide) and N2O (nitrous oxide) in high temperature combustion the major pathway to NOx leads through NO. It is thus the nitric oxide which will be considered in the combustion model. The nitric oxide can in principle be formed via three mechanisms: (a) Fuel-bound NO, which is not present for pure hydrocarbon fuels; (b) Prompt NO, which is formed in fuel rich regions of the flame; (c) Thermal NO, which is the prevailing mechanism in high temperature combustion. The relative importance of prompt vs. thermal NO can be low in many applications such as high temperature furnaces with long residence times, but might become large in modern NOx-reduced combustion devices operating under conditions where much of the thermal NO has been already eliminated. We focus here on a description of the thermal formation.
Thermal NO formation in laminar combustion
The kinetics of thermal NO formation are described via the Zel'dovich mechanism:



Of these reactions, the first one is the rate determining due to the large energy needed to break up the triple bonds in the N2 molecules. It becomes relevant only at temperatures above 1700-1800 K, which are often found in near-stoichiometric conditions. Since all of the reactions involved in here are slow compared to the oxidation of the fuel and the concentrations of the species involved are very low, the NO formation can be considered decoupled from the main combustion. Based on a simulated flow field, one can solve an equation for the mass fraction of NO in a postprocessing mode:



The source term for the formation NO now can be expressed using the kinetic data for reactions 1 to 3. In a homogeneous system with a reaction A+B -> C taking place, the concentrations of the species involved evolve like:



where [ ] denotes the molar concentration, ρYi/Mi and r is the reaction rate. This rate is proportional to the concentration of the partners involved:



where the rate coefficient k can be expressed as follows by Arrhenius law:



The coefficients involved in this expression are the pre-exponential factor A, the temperature exponent β and the activation energy Eα. Instead of using the activation energy, an activation temperature  can also be used.
In reversible reactions such as the ones contained in the Zel'dovich mechanism, the respective forward and backward reactions are governed by forward and backwards rates and their corresponding coefficients kf and kr. 
Employing these relations for the production rate of NO gives:



where now



Many different sets of kinetic data are available in the literature. Here the recent data from Bockhorn (1990) is chosen and listed in the following table.
Reaction		A	β	TA
1f:	N2+O -> NO+N	1.80E+11	0	38367
1r:	NO+N -> N2+O	3.98E+10	0	504
2f:	N+O2 -> NO+O	6.40E+06	1	3160
2r:	NO+O -> N+O2	1.36E+06	1	19235
3f:	N+OH -> NO+H	3.00E+10	0	0
3r:	NO+H -> N+OH	8.12E+10	0	24125
All of the rates depend besides a respective coefficients only on the temperature, which in turn is a function of mixture fraction. Since also all the concentrations are functions of mixture fraction, one can also write



Thermal NO Formation in Turbulent Combustion
For turbulent combustion, the NOx modeling has to be incorporated into the concept of presumed PDFs applied for the basic combustion model. Since in the turbulent case mean values are being considered, we also require now the Favre averaged NO formation rate:



Due to turbulence-chemistry interaction, the average NO formation rate cannot be determined by using the mean NO concentration. Rather, the integration over the joint PDF P(f, YNO) yields the proper NO source term.



where we already use the normalized NO concentration. The question is now how the joint PDF of mixture fraction and NO concentration can be modeled. Since the NO chemistry is very low, the fluctuations of NO are not correlated to the mixture fraction fluctuations, i.e., the joint PDF can be expressed as the product of the two marginal PDFs of mixture fraction and NO concentration:



For the mixture fraction it is logical to stick to the β-function formulation. For the NO mass fraction, the simplest approach here is to neglect fluctuations of NO and employ a δ-function PDF



This approach has the advantage that it does not require the solution of an equation for the variance of the NO concentration.
Prompt NO and fuel NO Formations
As mentioned above, the thermal NO is dominant in situations where high temperature and near-stoichiometric conditions prevail. However, in modern combustion devices (e.g., staged combustors), the formation of thermal NO is reduced that much that the prompt NO now becomes important. The prompt pathway involves HCN as an important species for which a concentration equation will have to be solved. For the time being prompt NO is not included in the NO module. This means that for certain cases NO might be under predicted if the prompt mechanism plays a role. Further, fuel NO has not been discussed. This means that the module is not appropriate for the prediction of the NO formation for the fuels containing NO.

Partially-premixed Combustion
Overview
The mixture fraction modeling approach in conjunction with flamelet tables is recognized as a reliable and accurate method for the simulation of diffusion flames. As the flame-structure is calculated in a preprocessing step and thus the chemistry calculations can be kept outside of the flow solver, this method has the advantage of being efficient. Due to the fast chemistry assumption which is only partially relieved by accounting for the effect of strain, this method is however limited to the use for non-premixed flow. A fruitful approach in the development of a reliable combustion model that both can handle non-premixed and premixed situations, seems to be to use a manifold-based modeling technique, like the Flamelet Generated Manifolds (FGM) method. This approach employs tabulated chemistry in conjunction with transport-equations for the mixture fraction and one or several progress variables. Solution to dimensional progress variable is weighted sum of product species. These values are read from tabulated manifold which are typically chemistry based. In the Hybrid BML/Flamelet partially premixed model solution of normalized progress variable can be viewed as a normalized temperature. The source term is modeled as a function of the laminar flame speed, k and epsilon. Laminar flame speed is a function of equivalence ratio which depends on chemistry. An FGM table can be used, but also specific "hybrid BML/flamelet" table consisting of a burning and a non-burning flamelet. In the case that FGM table is used, the source terms are not read from table.
Governing Equations
In the present approaches, the RANS-equations are solved together with a transport equation for the mixture fraction f and its variance g. A transport equation for the progress variable c is solved to parameterize the evolution of the overall reaction. It is assumed that the variance of the progress variable plays a negligible role in the turbulence-chemistry interaction compared to the variance of the mixture fraction. 
The governing equations read as



with the velocity vector , the density r, the effective stress tensor , the source term of the progress variable , the turbulent kinetic energy k and its dissipation rate ϵ. The density ρ, the source term , and the molecular dynamic viscosity μ are determined via look-up tables of the form 



For the case that equilibrium or flamelet tables are used, the governing transport equations are the same, except that no transport equation for the chemical progress is solved. If the latter approach is used, the combustion tables are looked up with the strain rate a instead of the progress variable  as a parameter.
Flamelet Generated Manifolds technique
In this section, the principles behind the construction of the FGM table is explained. The idea of the FGM method is to construct a manifold based on a set of flamelets. The flamelets can either represent a non-burning, a premixed propagating or a stretched non-premixed burning flame. The FGM tables are built either from a library of premixed or from a library of non-premixed flamelets.
Premixed flamelet generated manifolds
Premixed FGM are based on a library of premixed flamelets, with each flamelet corresponding to a different mixture fraction. The main step in the construction of the manifolds consists of mapping the thermochemical states of each flamelet on a grid that spans the complete physical range of the mixture fraction f and the progress variable c. The progress variable is typically defined as a linear combination of the intermediate species and the products. Vreman et al. (2008) suggest using the following definition 



where  and  represent the mass fraction and the molar mass of species i, respectively. It is essential to take a combination of species, so that the progress variable is monotonously increasing along each flamelet. 
It should be noted that since the mixture of fuel and oxidizer in the regular case are not flammable for the complete range of physical values of the mixture fraction, an interpolation has to be carried out for the states with a mixture fraction lying between the pure oxidizer (f = 0) and the lower flammability limit () as well for the states having a mixture fraction between that of the upper flammability limit () and that of the pure fuel (f = 0). 
Non-premixed flamelet generated manifolds
Non-premixed FGMs are created from a library of burning steady-state non-premixed flamelets and one unsteady extinguishing flamelet. A steady flamelet library, which is used as a basis for the construction of a non-premixed FGM, is containing flamelets ranging from a negligible strain until a strain rate, which lies close to that of the quenching limit. To fill the state-space between the steady burning flamelet subject the highest possible strain before extinction and the limit of an unburnt mixture of fuel and oxidizer, the thermochemical states of an unsteady flamelet are used. The necessary unsteady flamelet for the generation of a non-premixed FGM is created using the steady flamelet for the highest strain as initial solution and by prescribing a strain rate that lies slightly above the quenching limit, so that the flame successively dies. After a suitable definition of the progress variable has been found, the flamelet library is remapped onto a two-dimensional grid spanned by the mixture fraction and the progress variable. 
Filling the non-equilibrium part of the reaction domain with the solution of an unsteady flamelet leads to non-smoothness in the manifold. However, the incorporation of an unsteady flamelet may be advantageous, as unsteady flamelets are known to predict intermediate species and slow chemistry well. In addition, it should be noted, that a library of premixed flamelets in general does cover a smaller part of the state space than the set of flamelets used for the construction of a non-premixed FGM.
Turbulence chemistry interaction
To account for the turbulence chemistry interaction, the presumed b-PDF approach is used. In order to be able to pre-integrate the combustion look-up tables, they must first be transformed onto a square domain in the independent variables. This is achieved, by re-mapping the flamelets onto the normalized progress variable:



With this transformation, the thermochemical states are defined on a square domain with mixture fraction and the normalized progress variable as independent parameterizing variables, both going from zero to unity on the whole physical domain. In the present approach statistical independence of the mixture fraction and the normalized progress variable is assumed. It is furthermore assumed that the fluctuations in the normalized progress variables are negligible. After the pre-integration, the tables depend consequently on the mixture fraction f, its variance g and the normalized progress variable c*. Since the transport equations are still solved for the non-normalized progress variable c, a normalization of the latter solution variable is needed, before the combustion tables can be looked up.
Hybrid BML/Flamelet Technique 
The difference between the FGM technique and the hybrid BML/Flamelet model is in the source term closure. In the Hybrid BML/Flamelet model source term in the transport equation for the progress variable and variance of the progress variable are closed using a BML type model. 
The main difference between a premixed and a partially premixed flame is that in a premixed flame, the equivalence ratio is constant. In a partially premixed flame the equivalence ratio of the mixture can vary spatially. This means that the laminar flame speed, the combustion products and the density are now a function of the local equivalence ratio.
The equivalence ratio can be expressed in terms of the mixture fraction f



where  is the stoichiometric mixture fraction. In partially premixed flames, the transport equation for the mixture fraction and turbulence-chemistry interaction is taken care by mixture fraction variance equation.
In Equilibrium chemistry, the thermochemical properties are obtained from an equilibrium table containing the thermochemical properties . In a partially premixed flame these properties are obtained using a linear interpolation between the retrieved states from an equilibrium table and the retrieved states from a mixing table. 



Laminar Flame Speed for Hybrid BML/Flamelet Model
To obtain the laminar flame speed in a partially premixed flame, a possible method is solving the reaction equations for a one-dimensional premixed configuration and determine the laminar flame speed as the solution of the eigenvalue problem. Another approach to obtain the laminar burning velocities is by constructing polynomial fits to experimental data.
The Polynomial is preferred because it is accurate near the flammability limits and does not depend on the presence of the laminar flame speed in the table. Polynomial fits for several fuel types have been reported in the study of Metghalchi and Keck. For different pressure and unburnt temperature, the correlation function of Metghalchi and Keck is being used:



with =298K, =1 atm. and where the exponent are computed by:






The coefficients are fuel-independent and are provided by Metghalchi and Keck (1982):

 = 2.18,   = -0.8,    =-0.16,   = 0.22
The coefficients ,  ,    ,   are controlled by the expert parameter combEquRatioCorrCoefs_. 
This model was tested for methane, ethylene and propane fuels with pressures varying between 0. and 1 MPa. The reference laminar flame speed is given as a function of the equivalence ratio:



with the fuel dependent constants provided by measurement and given in the paper of Metghalchi and Keck for several fuel types. In this expression, A represents the maximum laminar flame speed, which occurs at the equivalence ratio ϕ = C. The constant B is found using a nonlinear least square fit through the experimental data or detailed calculation results. 
Gulder proposed an experimental correlation of the form:



where A, B, C and D are constants and correlation for laminar flame speed are fit for different fuels as function of equivalence ratio based on experimental data. In this case laminar flame speed is maximum at equivalence ratio 1 and roots at the flammability limits.
Parabolic options can be used for Laminar flame speed for unknown fuel-air mixture. The laminar flame speed at stoichiometric fuel-air ratio can be obtained from the chemistry table or from literature. Flammability can also be obtained from literature or experimental data and parabolic curve can fit for laminar flame speed as function of equivalence ratio. 
Flammability limits
When the equivalence ratio ϕ is very high or very low, the flammability limits are reached and the flame can extinguish. (for methane, the flammable region is approximately . Outside of this region, the flame becomes unstable and can extinguish.
The polynomials of Metghalchi and keck gives a flame speed of zero at two equivalence ratio, which will be taken as the flammability limits. Outside of these limits the flame speed is zero and no flame can exist.

Multi-Species Framework
Inert multi-species
With the Multi-species framework, mixing and transport of chemical species can be simulated by solving conservation equations describing convection, diffusion and reaction source terms for each component species. This framework is currently only available for inert flow (without source terms).
Inert multi-species framework solves for convection and diffusion without any chemical reaction source terms. Non-reacting species transport for multi-species framework can be used for simulation such pollutant tracking and chemical mixing flows.
Governing Equations
Governing equation for the multi-species framework is given by:













 is the flux of species j caused by mass diffusion. N is the number of species and E represents the total sensible energy. The energy equation is formulated in dependence of the sensible total energy to keep the energy in the same form for multi-species simulation as for single-species computation. In the inert cases heat release due to destruction and creation of species due to chemical reaction is not considered.
The sensible enthalpy h for ideal gas mixture is given as a mass-weighted sum of the enthalpies of the all individual mixture:



The sensible energy of species j is defined as:



Thus, In the equation that has only one species is present, the equation are the same as that of single specie framework.

 is the mass fraction of species j. In the species equation, first N-1 species equation are solved and the concentration of Nth species is determined via the condition, that the sum of all mass fraction must be equal to 1. Normally the abundant species in mixture is considered as Nth species. 



It is assumed that the gas behaves as an ideal mixture. Thus, the thermal equation of state is given by:



Ensuring Mass Conservation
 To ensure mass conservation (both for a mixture and real gases), the closure conditions:



has to be ensured. The above equation is enforced by setting the N-th species to:



This is done after each solution update and after each time the solution variable are prolongated in the multigrid scheme. To see why the closure condition need to be respected to ensure mass conservation, one may add up the partial densities to yield:



Alternatively, Since the density is determined as: 

,    ,          
It is obvious that the closure condition needs to be respected in order to avoid spurious generation or destruction of mass.
It should further be noted, that the use Fick's law for determining the diffusive fluxes  according to:



does not guarantee the conservation of the species. To avoid a spurious generation of the species a correction velocity has to be introduced. This correction velocity reads as:



which leads to the following flux:



By summing over all fluxes, the mass conservativity of the approach can be demonstrated:



as long as the closure condition is simultaneously enforced.
Species Diffusion
Species Diffusion is given by Fick's law:



Where  represents the effective diffusion coefficient given by:




where, represents the laminar diffusion coefficient and  the turbulent one. Diffusion of species due to the presence of a pressure gradient (pressure diffusion) or temperature gradient (Soret effect) are not considered. In FINE™/Open with OpenLabs™ the user can either specify a constant laminar diffusion coefficient for each species or specify that the diffusion coefficient of each species be calculated from the laminar kinematic viscosity  assuming a constant laminar Schmidt number  for each individual species, which is a user input:



The turbulent diffusivity is determined assuming Schmidt similarity:



where  denotes the turbulent dynamic viscosity of the mixture.
Transport Properties
Determination of the dynamics laminar viscosity of the individual species

In FINE™/Open with OpenLabs™ the user can either specify a constant viscosity:



for each species or specify that the dynamic laminar viscosity of each species be calculated using sutherland's Law.
Determination of the dynamic laminar viscosity of the mixture
The viscosity of the mixture is calculated from the viscosities of the individual species either by taking the mass average:



 or applying the simplified form of Wilke's law:



 The mole fraction  are calculated from the mass fraction  as follows:

 ,    
Determination of the turbulent dynamic viscosity of the mixture
The turbulence model determines the turbulent dynamic viscosity of the mixture. The presence of individual species does influence the modeling of the turbulence.
Determination of laminar conductivity of the individual species

In FINE™/Open with OpenLabs™ the user can either specify a constant laminar conductivity:



for each species or specify that the dynamic laminar viscosity of each species be calculated from the laminar viscosity assuming a constant laminar Prandtl number Pr (Pr is same for all species):



This corresponds to the law used in the single-species framework. Even though the framework principally allows the use of different state laws for the various species, the framework currently requires the user to use one single law for all species. Thus, the user needs either to specify a constant thermal conductivity for each species or use the Prandtl number to determine conductivity of each species.
 Determination of laminar conductivity of the mixture
The conductivity of the mixture is calculated from viscosity of individual species either by taking the mass average:



or applying the simplified form of Wilke's law:



Determination of turbulent conductivity
The turbulent conductivity  is determined assuming Prandtl similarity (as for the single species framework, this is the only option):



where  denotes the turbulent dynamic viscosity (of the mixture),  denotes the turbulent Prandtl number and  denotes the heat capacity of the mixture.

Solid Wall Boundary Conditions
Euler Walls 
For Euler walls the velocity must be tangential to the wall.
To obtain the velocity vector on the wall, the velocity is first extrapolated from the interior with zero order extrapolation:



where subscripts w,1 denote the wall and the first inner cell, respectively.
The tangential component of the extrapolated velocity vector is:



where  is the normal to the wall. 
The wall density and pressure are obtained by zero order extrapolation from the interior:



Navier-Stokes Walls 
Adiabatic Walls
The velocity vector on the wall vanishes. If the cylindrical boundary condition is used, the angular velocity of the wall (in the absolute frame of reference) must be specified. 
The velocity relative to the wall should be zero, leading to:



where subscripts s, w refer to the system and the wall, respectively.
Pressure is extrapolated from the interior, so that the pressure gradient is equal to zero.

.
The temperature on the wall is also extrapolated from the interior:

.
The density is derived from pressure and temperature through the appropriate relation, depending on the type of gas.
Isothermal Walls
The implementation of this boundary condition is very similar to the adiabatic Navier-Stokes wall. The only difference is in the determination of the wall temperature, which is fixed to the specified temperature in the this boundary condition. 
For the cylindrical isothermal walls, the angular velocity of the wall must be specified. 
Pressure is determined as in the adiabatic condition, and the density derived from pressure and temperature through the appropriate relation, depending on the type of gas.
Wall with Imposed Heat Flux
The implementation of this boundary condition is very similar to the previous ones. For this condition the temperature is determined from the imposed heat flux (W/m²).
The pressure is determined as in the adiabatic condition and the density derived from pressure and temperature through the appropriate relation, depending on the type of gas.
Wall with Imposed Heat Transfer Coefficient
The implementation of this boundary condition is very similar to the previous ones. For this condition the temperature is determined from the imposed heat transfer coefficient h (W/m²K):



where d is the distance between the first inner cell and the wall.
The pressure is determined as in the adiabatic condition and the density derived from pressure and temperature through the appropriate relation, depending on the type of gas.
Turbulent Wall Boundary Conditions
For a turbulent calculation with the turbulence model, the turbulent wall boundary conditions need to be treated.   
Spalart-Allmaras model and Simplified SARC
When the Spalart-Allmaras model or simplified SARC model is selected, the turbulent working variable  in the solid wall.
k-ε Models
The values of kw and εw are imposed at the boundary for the Yang-Shih model, while for the High Reynolds number models, they are imposed in the first inner cell.
M-SST k-ω models
When the M-SST k-ω models are selected, the boundary condition on solid wall is the following one:
(0-1) 


(0-2) 


with C = 60.

Troubleshooting
Introduction
In most cases, a straightforward and careful execution of the instructions detailed in the installation note enables to start NUMECA software smoothly. In case it is not working as expected this section provides information on how to handle most common situations.
Product not starting


In case FINE™/Open with OpenLabs™ does not start, check the following items:


Is NUMECA software installed with administrator privileges? If not, perform the installation again with administrator privileges.


Check whether 'Hide file extensions for known types' (activated by default for .dat extensions) is disabled to enter the name of the license file with its extension license.dat.


Is the license file valid and active to start the product ?


Check if the license server is up. If so, the numeca.exe process should run in the Windows Task Manager. If not, please do the instructions for license installation.


Some license check problems may occur if the host computer cannot find the server IP-address corresponding to the hostname information included in the first line of the license key. To solve this problem, replace the hostname by the IP-address of the license server. This operation does not invalidate the license key.


Check if the license key file is well readable by every user.

Did the user configure his/ her working environment? If not, perform the configuration according to the section User Configuration; then log out and log in.

Has the machine been rebooted after a change in the environment variables? If not, reboot it.


Check if the TCP/IP protocol is installed on the machine. The protocol is mandatory to ensure the correct function of the floating licenses.


Are the NUMECA software components visible from the machine? If not, install them.



Clean PMV files:

Close all tasks opened, including the FINE™GUI.
Open the Windows Task Manager and select the thumbnail Processes.
Check that no process pvmd3.exe is running. If so, select the process and click End Process to stop it.
Delete any files called pvm*.username in the directory defined by the environment variable PVM_TMP (usually C:\tmp).






Graphical problems and system crashes

NUMECA software makes use of the advantages of the available Graphics Card. Some trouble may however come up with the default driver OPENGL since it may not be supported by the user host computer and machine display. In order to set the system compatible with a more portable driver, typically MSW driver is used under Windows instead. Note however that the proposed drivers are usually less efficient in terms of graphical speed than the default driver.
To change the used driver


Log in as administrator. 
                                    
Launch regedit from the Start/Run menu. 
                                    
Go to the HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International register. 
                                    
Go into the folder of the package for which to modify the driver, e.g.: Fine#  where # is the version number.
Modify the DRIVER entry to either OPENGL or MSW.


 The selection will take effect at the next session.




Screen flashes

In some circumstances, the graphical area can flash during interactive operations, depending upon the driver selected.  Setting the environment variable NI_DOUBLEBUFFERING to ON in HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International/<product_name> register may solve the problem. To launch the registry editor, access regedit in the Start/Run text box.


Flow solver not starting in parallel mode

The parallel account must be configured at first use (see User Configuration.
To launch parallel computations on Windows, the  solver uses the MPICH2 libraries and the smpd process manager. The smpd service is automatically installed and started during the installation of FINE™. If the user has already the smpd service installation before installing FINE™, there may be a conflict between the smpd services and thus the smpd service in FINE™ may not be started. If the user gets the error message smpd version mismatch during the parallel computation, check if the FINE™ smpd service is started. If not, stop other smpd services and start the one installed by FINE™ (the service name is MPICH2 Process Manager, Argonne National Lab and the linked executable is  Installation_path\fine<version>\bin64\smpd.exe).


Cannot connect to other hosts

At the first execution of task manager

Can the machine be "seen" from the remote hosts (and vice-versa)? Use the ping command to check this item.
Is the machine name included in the computer list within the rhosts.txt file of the  user? Please notice that capital letters must be used; extra-characters like "è, ä, ë, ..." may lead to potential problems and should better be avoided.


Task manager launched once with success


In case the user can no longer connect to other hosts while this operation has at least be successful once, the following should be checked: 




Start the Task Manager (Modules/Task Manager) from the FINE™ GUI and select the Hosts definition  page in the menu on the left.
                                


Click on the button Shutdown. A warning message will appear stating that all hosts will be removed from the Virtual Machine and that FINE™ GUI will be closed. Click on yes to continue.




Close all currently open tasks (including the FINE™ GUI) and remove pvmd.* and pvml.*, located in the directory defined by the environment variable PVM_TMP (by default C:\tmp), if applicable. Additionally kill the PVM daemon pvmd3.exe, if applicable. The status of PVM daemon can be observed by accessing the Windows Task Manager.






Remote copy does not work


The remote copy option can be accessed in Task Manager Tasks Definition area. 
This option does not work if the user configuration file .cshrc (Linux platform) gives output to a shell. To test whether it applies, open a DOS shell on the Windows machine and type the command rsh machine_name echo YES <Enter> (where machine_name refers to the name of the Linux machine). If the value returned is YES, the configuration is correct and the remote copy option is expected to work properly. If additional lines are returned, problems are expected. If so, further troubleshooting is needed as described in the following section.



Further troubleshooting

For more information and troubleshooting:

consult the forum in NUMECA's Customer Area with a section dedicated to installation.
or contact NUMECA local sales or support office (for active maintenance plans only). 

To help to find a solution within the shortest delays, please provide a detailed description of the observed behavior and performed analysis.
The following information can be helpful:

the license key file license.dat.
the hostname and hostid. This information can be obtained by executing into the subdirectory NUMECA_INSTALLATION_DIRECTORY\<product_name>\flexlm the lmtools.exe (for Hostname and HostID for NUMECA as Computer/Hostname and Ethernet Address under the System Settings tab).  
the product name and version for which installation is causing problems.
a description of the configuration (in terms of name, Windows version, local or domain user).
the debug.log file generated when starting the license service.
the .out files in C:\tmp.
the pvml.username in C:\tmp (or directory defined by the environment variable PVM_TMP).

User Configuration
Optional user configuration
Without the optional steps in this section it is still possible to launch a simulation on one processor on the local machine with a default location of the home directory.
Configure account to perform parallel computations

Provided that the parallel capabilities have been adequately installed and valid licenses can be accessed, the user will be able to perform parallel computations. Launching a parallel computation, the system will by default request the user login and password. Before the first launch, the user can register his/ her name and password once and for all, by doing the following steps:


Open a DOS shell, 
Type the command NUMECA_INSTALLATION_SOFTWARE/fineopen72/bin64/mpiexec.exe -register<Enter>.
Enter the user login and password and confirm.


If the user does not register his/ her name and password before launching the parallel computation, the FINE™ GUI will prompt the user to enter credentials (Windows login account) if needed. 
Currently, it is not possible to launch the computation without the registering/ providing the user's credentials. Thus, if no password has been defined during the registration,  it will be necessary to set the password on the machine in any case.
Domain administrators are not allowed to run parallel computations under Windows.
PVM does not support domain accounts.
Parallel computations under Windows (except Windows Server) are limited to one PVM daemon running at a time on the machine. Consequently, access to multiple users on a given machine is not allowed.
MPICH2 library needs Microsoft .net Framework package before installing NUMECA software.
When running parallel computations, the path to the project must be identical on both the local and remote machines. For example, for distributed memory parallel computations, a folder must be mounted on each machine and share the same drive name, in order to store the project directory that will be run in parallel on multiple hosts.



Configure account to allow remote computations

It is possible to launch tasks on remote machines by using the Task Manager capabilities. To be able to perform remote launches, NUMECA software must be installed and explicit permission must be specified on the remote machine. To this end, the following operation must be checked and/ or performed on the remote machine:

Open the Windows Control Panel window (Start/Settings/Control Panel).
Click on the Services icon under System and Security/Administrative tools.
Select from the list of services NUMECA RSH Daemon.
Click on Stop and leave the Services window open.

Edit the file rhosts.txt in the directory C:\WINDOWS on both the host and client machines. 
This can be done through the FINE™/Admin Tool. Launch it from All Programs->NUMECA software-><product_name>->Administration Wizard and select Configure the TaskManager in this machine.
Alternatively edit the rhosts.txt file

Edit the text file and add the following line for each host user you want to give access permission: 
hostname username:
These lines typically give right to the user username, working on the machine hostname, to connect to the machine containing the rhosts.txt file.



Select the NUMECA RSH Daemon from the list of services in the Services window.
Click on Start. Starting this service may take approximately 5 minutes.

Use of the Task Manager under Windows with a Linux host may lead the remote copy to option to fail. See also: Cannot connect to other hosts in the Troubleshooting section for more detail on this problem.
In addition to that, the firewall should also allow remote computations. To do so, follow the steps below:


Add a Port inbound and outbound rule for a TCP protocol with the number 514. The connection should be allowed for all type of profiles.

Allow the following programs to bypass the firewall inbound and outbound rules: smpd, mpiexec, hexstream#x86_64 and hexstream#_impix86_64 (# stands for sp, hp and dp) located in <NUMECA_INSTALLATION_DIRECTORY>\fineopen72\bin64; lib\win32\pvmd3.exe, bin\rsh.exe, bin\rsh_vista.exe and bin\win32\hoster.exe located in <NUMECA_INSTALLATION_DIRECTORY>\pvm.



Home directory

On Windows, NUMECA software saves some data (preferences, user fluid database, ...) in the folder %HOME%\.numeca\, or in the %HOMEDRIVE%%HOMEPATH%\.numeca\ folder in case %HOME% is not defined. If the user wants to customize the path of the .numeca folder, the user can redefine the system environment variable HOME. 
Note: 

The variable HOME must be defined as a system environment variable.
 Defining HOME to a network disk may significantly slow down the NUMECA software GUI.

During the runtime, NUMECA software writes temporary data in the directory %HOME%\.numeca\tmp. This tmp directory can be redefined by defining the environment variable TMP_DIR.


Software launch
After configuring, the product can be started from the Start\Programs\NUMECA software\<product_name>\ menu.
It is not allowed to start NUMECA software under Windows as administrator in a user domain environment. This limitation does not apply to user login.
In case the license has not been configured adequately at this stage of the installation process, it is still possible to launch the product by selecting a license file (server) when prompted after first launch.
The UAC (User Account Control) should be disable for running the solver in parallel otherwise it prevents mpiexec to record the encrypted login and password in the registry database and the Task Manager remains open forever without any evolution.
NUMECA software can be launched directly from the user desktop by copying shortcuts from ~\AllUsers\StartMenu\Programs\NUMECA software\<product_name>\ to ~\AllUsers\Desktop.
It is not suggested for one user to simultaneously open (and therefore launch tasks in) more than one FINE™  environment.

Advanced Parameters for the Numerical Model
Interfaced Advanced Parameters
Pseudo-time integration



An explicit Runge-Kutta scheme accelerated by a multigrid technique is used to march the solution in time towards the steady state solution.
When the multigrid strategy is used (i.e. if more than one grid level has been selected in the Numerical Schemes/ General page), an input box allows the user to select the number of sweeps to be performed on the coarse grid levels. The number of sweeps is the number of times the Runge-Kutta operator is applied. In the default solver configuration, the number of sweeps on each level equals the level number (e.g. 2 sweeps on second level etc.). It has been observed in many cases that the convergence rate may be significantly improved by performing a higher number of sweeps on the coarsest levels. Recommended sets of values are, for instance, (1,2,16) for 3 grid levels or (1,2,8,32) for 4 levels. However, it should be noted that more sweeps imply that more time is required for an iteration.
If the option Coarse Grid Initialization has been activated in the Numerical Schemes/ General  page, the computation starts on the coarsest grid level and includes a finer grid level each time one of the two following criteria is satisfied in the Advanced tab of the Numerical Schemes/ General Parameters page:

The maximum number of cycles to be performed on each grid level is reached. This parameter is specified through the input box in the Coarse grid initialization parameters area as the Maximum number of cycles per grid level.
The residual on the current grid level has dropped by a certain order of magnitude as indicated by the Convergence criteria on each grid level.

Another feature of the pseudo-time integration scheme is the time stepping technique used to march the solution in time. At present, only the local time stepping method can be selected. This self-explanatory approach is used to drive the solution towards the steady state at the fastest rate compatible with the CFL condition.


If the computation is unsteady, the Dual time step inner-iteration control box is unfrozen in the Advanced tab of the Numerical Schemes/ General Parameters page. The user can specify the Convergence criteria and Maximum number of inner iterations for the Dual time stepping method, which is used to compute the right-hand side of the governing equations at each physical time step, see Linear Eddy Viscosity Turbulence Models.




Non-interfaced Advanced Parameters



rot_iVelSy_:	The governing equations for rotating systems, such as turbomachinery problems,  are usually formulated in the relative system and solved for the relative velocity components. However, experience shows that, for propeller, ventilators or wind turbine problems, the formulation based on relative velocities has the disadvantage that the far field relative velocity can reach high values. This induces an excess of artificial dissipation leading to a non-physical rotational flow in the far field region, this dissipation is based on the computed variables. So the governing equations for these cases are often expressed in the relative frame of reference for the absolute velocity components. In FINE™/Open with OpenLabs™, the user has the ability to select the solved velocity for rotating systems through the expert parameter rot_iVelSy_.
0: solve the absolute velocity components in the relative frame of reference for rotating block.
1 (default): solve the relative velocity components in the relative frame of reference for rotating block.
iAsFT_:	Since the numerical methods used in the FINE™/Turbo and FINE™/Open solvers are different, the results obtained with these two solvers are different. The use of  the expert parameter iAsFT_ aims at giving the possibility for a FINE™/Open with OpenLabs™ user to reproduce results obtained with FINE™/Turbo. If this parameter is set to 0, the user employs the original version of the FINE™/Open solver. If this parameter is set to 1, the user is attempting to obtain a version that has the similar behavior with the FINE™/Turbo solver.
There is no guarantee that using the expert parameter iAsFT_ 1 will obtain identical results between FINE™/Turbo and FINE™/Open.
_typeOfBlockID:	Each block has a _typeOfBlockID number in FINE™/Open with OpenLabs™. The user can modify this number. If the _typeOfBlockID numbers of the neighboring blocks that have a FNMB connection, are different, the solver will only consider the heat flux across the FNMB interface.
agglomerationNEW_:	0: old agglomeration method;
1 (default): new agglomeration method. The treatment approach in the boundary layer is improved.
tm_iResSmoothing_: Specifies the implicit residual smoothing method during the computation on the finest grid. The user may always set this parameter to 2 if the residual smoothing module needs to be activated. The solver will check the settings in the .run file and change to 1 automatically if necessary.
0: Deactivate the residual smoothing procedure,
1: The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed for all solved equations (including the turbulence model equations). This value is available for Euler, laminar and turbulent flow with one-equation turbulence models.
2 (default): The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed only for the continuity, momentum and energy equations. This value is available for turbulent flow with two-equation turbulence models.
tm_fmg_iResSmoothing_: Specifies the implicit residual smoothing method applied during the coarse grid initialization. The user may always set this parameter to 2 if the residual smoothing module needs to be activated. The solver will check the settings in the .run file and change to 1 automatically if necessary.
0 (default): Deactivate the residual smoothing procedure,
1: The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed for all solved equations (including the turbulence model equations). This value is available for Euler, laminar and turbulent flow with one-equation turbulence models.
2: The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed only for the continuity, momentum and energy equations. This value is available for turbulent flow with two-equation turbulence models.
tm_iResSmooVersion_: Specifies the numerical method used in the implicit residual smoothing method.
0: the residual smoothing coefficient ϵ is computed on cell faces and the boundary conditions are depending on the boundary type.
1: the residual smoothing coefficient ϵ is computed on cell centers and the boundary conditions are depending on the boundary type.
2: the residual smoothing coefficient ϵ is computed on cell faces and the Neumann boundary conditions are used.
3 (default): the residual smoothing coefficient ϵ is computed on cell centers and the Neumann boundary conditions are used.
tm_mgCycleType_: Applies only for multigrid and selects the type of multigrid cycle
1 (default): V-cycle;
2: W-cycle; 
3: F-cycle;
4: V-cycle in sawtooth;
5: W-cycle in sawtooth;
6: F-cycle in sawtooth.
gradientScheme_: Controls the computation of the gradient at cell centers, which is used mostly for 2 features of the flow solver: the computation of the production term for turbulent models and the reconstruction of the solution at the face from the cell center:
0: use the least square technique. When the 2nd order Roe upwind scheme is used, the expert parameter gradientScheme_ must be set to 0. The technique may fail when dealing with highly stretched meshes, typically in the boundary layers. 
1 (default): use the weighted least square technique. 
2: use the least square technique with the Singular Value Decomposition (SVD).
4: use the weighted least square technique with SVD.
5: use the Green-Gauss gradient technique.
mg_iPrecondFoF_: When using the multigrid method combining preconditioning, the forcing function in the Full Approximation Storage (FAS) approach can be computed before/after applying the preconditioning:
0 (default): compute the forcing function before applying the preconditioning. 
1: compute the forcing function after applying the preconditioning. 
The other expert parameters related to the numerical model are as follows:
Central Discretization

spc_dissip_ext_:	0 (default): the second order dissipation term is applied at inlet, outlet and external boundaries. 
1: both the second and fourth order dissipation terms are applied at these boundaries. 
2: neither the second nor fourth order dissipation are computed at these boundaries. 
spc_dissip_wall_:	0: the second order dissipation term is applied at wall boundary. 
1: the second order dissipation term is applied at wall boundary, and the second-order difference in the first inner cell is set to zero in the direction normal to the wall.
2: neither the second nor fourth order dissipation are applied at wall boundary, and the second-order difference in the first inner cell is set to zero in the direction normal to the wall. 
iFluxAverage_:	In the absence of gravity, two discretizations of the fluxes for the Jameson scheme have been introduced.
0 (default): variable averaging,
1: flux averaging.
iFluxAverageFMG_:	Select the method of discretization of the fluxes during the FMG..
0 (default): variable averaging,
1: flux averaging.
spc_artDiss2ndCoef_:	 Coefficient κ(2) for 2nd order dissipation in the central scheme. Default value is 1.0.
spc_artDiss4thCoef_:	 Coefficient κ(4) for 4th order dissipation in the central scheme. Default value is 0.1.
spc_expMartinelli_:	 Exponent in the multi-dimensional scaling model of Martinelli of the dissipation used in central schemes. Default value is 0.5.
spc_TswitchInArtDissip_:	 Defines whether the second order artificial dissipation switch should be based on both pressure and temperature gradients or on pressure gradients only.
0 (default): only pressure gradients are taken into account. 
1: both pressure and temperature gradients can be taken into account.
spc_XhilnArtDissip_:	 Improve the treatment of artificial dissipation running the second order central scheme for supersonic and hypersonic applications. This parameter varies between 0.0 and 0.99. The value 0.0 corresponds to the original central scheme of Jameson which is not monotonous for cases presenting discontinuities like shocks. The value 0.99 makes the scheme monotonous.


Central matrix discretization

spc_artMatDiss2ndCoeff_: Coefficient k(2) for 2nd order dissipation in the central matrix dissipation scheme. Default value is 1.0.
spc_artMatDiss4thCoeff_:	 Coefficient k(4) for 4th order dissipation in the central matrix dissipation scheme. Default value is 0.15.
spc_artMatDissfmg_:	 In case the central matrix dissipation scheme is selected, another dissipation scheme can be applied during the coarse grid initialization:
0 (default): The central scalar scheme is applied during the FMG
1: The central matrix scheme is applied during the FMG
EntrFx_:	The parameters Vl and Vn used in the limiter of the central matrix dissipation scheme. Default value is 0.1 0.1.
merkle_matdisEntrFx_:	Entropy fixes for the matrix dissipation with Merkle preconditioner. The parameters Vl and Vn used in the limiter of the central matrix dissipation scheme. Default value is 0.3 0.3.
hakimi_matdisEntrFx_:		Entropy fixes for the matrix dissipation with Merkle preconditioner. The parameters Vl and Vn used in the limiter of the central matrix dissipation scheme. Default value is 0.1 0.1.


Upwind Discretization

upw_dissipEnthalpy: Controls the use of the standard or isenthalpic dissipation. The default option is the standard dissipation when value set to 0.
upw_dissip_ext_:	Controls the calculation of the dissipation at inlet-outlet boundaries. If 1 the dissipation is computed (0 not computed).
upw_limit_:	Activate the limiting procedures with the second order upwind scheme for supersonic and hypersonic applications. For cases presenting shocks, this option has to be activated by setting the value to 1 so that a monotonous solution is obtained.
upw_limitVenka_:	Select to use the Barth-Jespersen limiter or the Venkatakrishnan limiter with the second order upwind scheme for supersonic and hypersonic applications.
0 (default): the Barth-Jespersen limiter,
1: the Venkatakrishnan limiter.
EntrFx_:	Values of the entropy fix for the linear fields and the non-linear fields. EntrFx_ is an array of two dimensions set by default at (0.1;0.1). For cases presenting shocks, it is advised to modify the values and set them to (0.3; 0.3).


Time Discretization

tm_nbStage_:	Specifies the desired number of stages in the Runge-Kutta scheme. Default set to 4
tm_drcoeff_:	Runge-Kutta coefficients. One for each stage, the first one for the first stage, the second one for the 2nd stage and so on. If all coefficients are set to zero, default values are taken, depending on the number of stages and the spatial discretization scheme.
spc_iCalcArtifDissip_: One for each Runge-Kutta stage, the first one for the first stage, the second for the second stage and so on. Set to 1 if numerical dissipation is to be recalculated at the associated stage, set to 0 if the numerical dissipation is taken from the previous calculation. For consistency, spc_iCalcArtifDissip_ should be set to 1.
spc_iCalcVFluxes_: One for each Runge-Kutta stage, the first one for the first stage, the second for the second stage and so on. Set to 1 if viscous fluxes are to be recalculated at the associated stage, set to 0 if the numerical dissipation is taken from the previous calculation. For consistency, spc_iCalcVFluxes_ should be set to 1.


Preconditioning

preco_pcEpsVLim_: Coefficient of  when computing  in the Merkle preconditioning(default value is 0.001).
preco_pcEpsVLimC_: Coefficient of the speed of sound when computing  in the Merkle preconditioning(default value is 0.001).

Launching Mode 

The Computation Control/Launching Mode page allows the user to define if the computation will be launched in sequential or in parallel.


The computations using HEXPRESS™/Hybrid in sph format or TGrid mesh must be launched in parallel mode.

After launching a computation, the FINE™/Open solver will automatically allocate memory depending on the computation. Please note, there is a limitation coming from the operating system on the amount of memory that can be used.  In case of large computations, it is suggested to run the computation in parallel mode.


FIGURE 20 Launching Mode page
The Launching Mode page allows the user to select between Serial (sequential mode) or Parallel. By default the computation will be launched in sequential mode.
When activating the Parallel option, the user should define the parameters for the load balancing. With Allow multiple domains per process   activated, it is possible to group and handle more than one block in one single process. This is useful in case there are multiple small blocks in the project. 
When multiple blocks are treated by one process, these blocks must not be partitioned.
After the user specifies the Total number of processes to be used, the load balancing between blocks will be automatically computed. 


FIGURE 21 Parallel Settings
After setting the Total number of processes, the user can still modify the Number of partitions and Weight(%) (if the option Weighted is active) for each block/group. In this case, the Total number of processes will be automatically updated.
The button Default balancing allows to re-set the weight using the default value.
After selecting the number of partitions and their respective weight, FINE™/Open with OpenLabs™ allows the user to visualize the cells composing a selected partition by left-clicking on the "eye" button ().


FIGURE 22 Visualize the cells composing a selected partition
For parallel computations, FINE™/Open provides two partitioners:

Serial partitioner (default): guaranties the same convergence history whatever the number of processors is. It is slow and limited by the maximum memory that can be allocated on a processor.
Parallel partitioner: can be activated by settings the expert parameter PartitionerParallel_=1. It is fully parallelized and thus faster and without memory restriction. 
One disadvantage of the parallel partitioner is that the convergence history of the computation depends on the number of processes, because there is no communication between the processes when performing agglomeration. In order to overcome the disadvantage, a new agglomeration method is introduced, which can be activated by settings the expert parameter newParallelAgglomeration_=1.  This new agglomeration method allows to get the same convergence history whatever the number of processors is. However, this new agglomeration method needs more CPU time because of the communication between the processes.
In case of a structured grid, the expert parameter newParallelAgglomeration_ is automatically set to 0.

For parallel computations with ".hex" mesh (HEXPRESS™ format), by default, the mesh will be partitioned in serial (by only one processor). If the user wants to partition the ".hex" mesh in parallel,  the user must set the expert parameter PartitionerParallel_ to 1 to activate the parallel partitioner.
For parallel computations with ".sph" mesh (HEXPRESS™/Hybrid format) or ".msh" mesh (TGrid format), the mesh will be automatically partitioned in parallel.
When option Allow multiple domains per process checked, the parallel partitioner is automatically activated.

TabGen/Chemistry

TabGen/Chemistry is a tool that generates, retabulates and preintegrates combustion tables according to the user settings. The tool contains the 1D chemistry solver CHEM1D of TU Eindhoven to generate flamelet or equilibrium tables. 
TabGen/Chemistry can be used to:

Generate equilibrium tables (non-premixed combustion),
Generate flamelet tables or flamelet libraries (non-premixed combustion),
Generate tables for the Hybrid BML/flamelet method (partially premixed combustion),
Generate tables for the Flamelet Generated Manifold method (partially premixed combustion),
Extend a given flamelet or equilibrium table so that it accounts for situations with large heat losses.

The limitations using TabGen/Chemistry are:

TabGen/Chemistry is currently only available for Linux platforms,
In a directory several projects can be stored and run. However, if the projects are run simultaneously in the same directory, they might interfere with the log-file of CHEM1D, which is used for monitoring of the convergence status,
The chemical composition of the streams can only be specified using mole fractions in the steering files (mass fractions are not yet supported),
All flamelets are generated assuming constant pressure. The influence of compressibility effects is not accounted for in the table generation process,
FGM tables are based on a counter-flow diffusion flamelets (the table can however also be used for premixed cases) and does not account for differential diffusion effects,
FGM tables with large heat losses assumes a frozen chemistry.

General
Using the General tab, the user can choose which format will be used and which physical variables have to be included in the output generated by the flow solver, see FIGURE 25.


FIGURE 25 Output Parameters - General
In the Flow configuration frame, the configuration choice for the output can be selected: Internal flow, External flow or Turbomachinery. Depending on the choice, the selectable quantities in the Quantities selection frame will be adapted automatically.
In the Output file format frame, the format of the output file can be selected. By default, the CFView™ format is activated. The user has to select at least one format for output. In case that none of them is selected, the CFView™ format will be used.


CFView: This is the native format used by FINE™/Open with OpenLabs™. The format is fully supported by CFView™. By default (out_newCfv_=0), all output generated by the flow solver for CFView™ are written in ".d1.s*" files for scalar quantities and in "d1.v*" files for vector quantities. The flow solver can also write all output into one single ".cfview" file, which can be done by setting the expert parameter out_newCfv_ to 1.
In case of harmonic simulations, the expert parameter out_newCfv_ is set to 1 automatically by the flow solver.
To compare the outputted derived quantities by the flow solver and the derived quantities computed by CFView™, the user must set the expert parameter out_derQntFromNode_ to 1 in order to compute the derived quantities in the flow solver after interpolating the primitive variables to nodes.


Ensight: The flow results can be exported in EnSight format. Thus, the user can post-process the FINE™/Open with OpenLabs™ solution in EnSight. For the use of EnSight, please refer to the EnSight manual.
Validation tests are performed with EnSight v9.1.2.
For unsteady computations, the intermediate solutions can not be saved.


CGNS: The flow results can be exported in CGNS v3.3.1 format. 

When exporting results in CGNS format, the following limitations exist: 

No information on FNMB or R/S interfaces in CGNS file.
No Solid Data in CGNS file.
For sliding mesh cases, the mesh is not rotated.
For PER boundary condition,  one layer of extra cells is added in case of serial computations.



The Quantities selection frame is split up into three parts. On the left side, the different Categories of output are listed. If no variable can be selected, the category will be gray out. On the right side, there are two lists: Available quantities and Selected quantities. The user can click on the button Add to move a selected variable from Available quantities to Selected quantities, or click on the button Remove to move a selected variable from Selected quantities to Available quantities. All the selected variables will then be automatically available when launching CFView™ in order to visualize the results.
The selection of variables is global. If a variable is selected, it will be computed for domains that match the conditions. For the other domains, the value will not be computed (field appears blank in CFView™).
If the user changes the flow configuration, the previous selection is kept. The selected variables, which are not compatible with the new configuration, are hidden. The new selectable variables are added to the list Available quantities.
By default, the following variables are selected, whatever the flow configuration is:

Static temperature
Static pressure
Density
Vxyz
Turbulent viscosity

All the variables that can be selected for output are listed in the following sections.
Thermodynamics

For all the flow configurations, the following variables can be selected for output.

Static/Total temperature
Static/Total pressure
Over static pressure
Static/Total enthalpy
Density
Entropy
When computing the Entropy, the reference pressure, reference temperature and reference density are the averaged values of the static pressure, static temperature and density averaged on all INL patches, respectively. If  there are no INL patches,  all reference values must be defined in the Advanced tab.
Static Energy (only for condensable gas)
Dynamic viscosity
Dryness fraction (only for condensable gas)
Generalized dryness fraction (only for condensable gas): the generalized dryness fraction is defined as: . Where ρ is the local density, ρL and ρv are the liquid density and vapor density computed from the pressure saturation table, respectively.
Void fraction
HeatCapacity (not available for combustion)
Thermal conductivity
Gamma (only for perfect gas and real gas, not available for combustion)

TABLE 2 Thermodynamics quantities generated by the FINE™/Open solver







Quantity


Incompressible


Perfect gas






Static temperature














Total temperature














Static pressure














Total pressure





(The term k only exists when the two or four equation turbulence models are applied)









Density














Entropy














Dynamic viscosity














Thermal conductivity














Heat capacity














Gamma


-









The heat capacities cp and cv are function of the temperature for real gas and condensable gas. When real gas or condensable gas is used, the total pressure and total temperature are computed by the following equations:






In case of condensable gas, some thermodynamic variables are selected by default for output. These variables are used to compute derived quantities in CFView™, for example, the "static energy" and "density" in case of non-preconditioning. If these variables are deselected, a warning will be pop-up for confirmation:
The following five definitions of the pressure coefficient are available for fluid blocks with inlet and outlet boundary conditions:















where  corresponds to the averaged value of the variable X on the inlet. vref is defined as  in case of Turbomachinery activated in the General tab ( Lref the reference length defined in the Advanced tab). In case that Turbomachinery is not activated  in the General tab, vref is defined as Reference velocity in the Advanced tab.
Furthermore the following  definition of the pressure coefficient is available for fluid blocks:



where ,  and  are the reference pressure, reference density and reference velocity defined in the Advanced tab, respectively.
For turbomachine computation (when Turbomachineryactivated in Flow configuration frame), the following additional quantities can be selected for output:

Absolute/Relative total temperature
Absolute/Relative total pressure
Absolute/Relative total enthalpy
Rothalpy: the rothalpy is defined as . Where h is the static enthalpy, w the relative velocity, u the entrainment velocity defined as: .



Vorticity

For all the flow configurations, the following variables can be selected for output:

Vorticity components in the  axes: 
Vorticity magnitude
Vorticity vector



Velocities

For all the flow configurations, the following variables can be selected for output:

Velocity components in the xyz axes: , ,
Velocity magnitude: 
Mach number
Velocity vector: 
Velocity vector with projection of the velocity field in the wall boundary cells onto the surface. This enables visualisation of oil flow traces on solid boundaries with surface streamlines.

For turbomachine computation (when Turbomachinery activated in Flow configuration frame), the following additional quantities can be selected for output:

Absolute Velocity components in the  axes: , ,
Absolute Velocity m-component: 



Relative velocity components in the  axes: , , 
Relative Velocity component in the θ axes: 
Relative velocity magnitude: 
Relative Mach number
Relative velocity vector: 






Residuals


The residuals are computed in FINE™/Open with OpenLabs™ by a flux balance (the sum of the fluxes over all the faces of each cell). The absolute value |RES| resulting from the flux balance is written as output for each cell.
For all the flow configurations, the following residuals can be selected for output:

mass conservation
x-component of the momentum equation
y-component of the momentum equation
z-component of the momentum equation
energy conservation
Spalart viscosity  equation, for the Spalart-Allmaras and SARC models
turbulent kinetic energy k equation, for the k-ε and k-ω models
turbulent energy dissipation rate ε equation, for the k-ε models
Specific dissipation rate ω equation, for the k-ω models

For combustion computations, the following additional residuals may be selected for output:

Residual_Comb_NormalizedProgressVariable
Residual_Comb_MixtFrac
Residual_Comb_VarianceMixtFrac
Residual_Comb_EnthDefect
Residual_Comb_NOxPost
Residual_Comb_ProgressVariable1

For radiation computations using the P1-model, the following additional residuals can be selected for output:

Residual_Rad_GP1Rad



Turbulence

For all the flow configurations, the following variables can be selected for output:

Spalart viscosity , for the Spalart-Allmaras and SARC models
turbulent kinetic energy k, for the k-ε and k-ω models
turbulent energy dissipation rate ε, for the k-ε models
Specific dissipation rate ω, for the k-ω models
Distance to wall
Ratio between turbulent eddy viscosity and molecular viscosity
Dimensionless distance to wall y+
Turbulence production term



Data

For all the flow configurations, the following solid data can be selected for output:

Cf: Skin friction coefficient (only the wall boundary cells are considered. Set to 0 elsewhere).  , where  is the local wall shear stress (magnitude of the vector Viscous stress),  and  are the reference density and reference velocity, respectively (set in the Output page under the tab Advanced).
The quantity Cf =  before FINE™/Open v5.2. Please update your Python script if Cf is used in your existing script.
Viscous stress (wall to fluid): local wall shear stress (vector).
Heat flux (wall to fluid)
Heat transfer coefficient: . Where  is the heat flux (wall to fluid);  is the local wall temperature;  is defined as the averaged absolute total temperature on all inlets in case of the expert parameter out_htcDef_=1 and defined as the reference temperature in the Advanced tab in case  of the expert parameter out_htcDef_=2.



Unsteady

For all the unsteady flow configurations, the following variables can be selected for output:

CFL_phys: the unsteady CFL number, defined by , where v is the local velocity,  is the physical time step and  is the characteristic cell size.
Q_criterion: , where S is the absolute value of the strain rate and Ω the absolute value of Vorticity.
Lambda_2: is defined as the second largest eigenvalue of .



Combustion

For output of non-premixed combustion simulation, see Outputs.
For output of partially-premixed combustion simulation, see Outputs.
For output of premixed combustion simulation, see Outputs.


Radiation

For all the flow configurations, the following variables can be selected for output:

Rad_GP1Rad: Incident radiation
Rad_AbsorptionCoefficient: Absorption coefficient
Rad_SurfRadiationHeatFlux: Surface radiation heat flux
Rad_HeatFlux: Radiation heat flux



Cavitation

For all the flow configurations, the following variables can be selected for output:

Cav_VaporFraction: the vapor mass fraction or the vapor volume fraction, depending on the solved transport equation (cavFCM_iVaporMassFracEqs_). This output is available only when using the cavitation model with the TEM model.



Harmonics

For harmonic output, see output.


Lagrangian

Depending on the settings of Lagrangian computations, the following variables may be selected for output:

Lagr_ParticleVelocity: the velocity of the particles.
Lagr_VolumeFraction: the volume of the particles / m³.
Lagr_TurbulentKineticEnergyK: the turbulent kinetic energy of the particles.
Lagr_NumberConcentration: the number of the particles / m³.
Lagr_MassConcentration: the mass of the particles / m³.
Lagr_ArithmeticMeanDiameter: the arithmetic mean diameter of the particles.
Lagr_ArithmeticDiameterVariance: the variance of the Arithmetic Mean Diameter. 
Lagr_Deposition_Rate: the deposition rate on the solid walls where the option Deposition is selected.
Lagr_InterphaseForces: the components of the interphase force. These are all source terms activated going to the Eulerian equations, thus mass, momentum and energy source terms from the Lagrangian phase to the Eulerian phase. They are also sampled.
Lagr_ReynoldsStress: these are the stresses of Lagrangian particle velocities (again ensemble averaged), ie.: u'u', v'v', w'w', u'v', u'w', ... and so on, where u', v', and w' are the fluctuations of the averaged Lagrangian particles velocities. It is the same as for the fluid, but for the particle velocities.

The output can be computed for each class of particle. The number of classes is defined during the computation settings. All sections concerning Lagrangian quantities are expanded during the saving of the run file, so that it contains as many sections as the number of classes for each quantity.


Deformation

The deformation output is available only when the mechanical coupling method (MpCCI and Modal Approach) is activated:


The  output quantities available are:

Dx, Dy, Dz : scalar quantities of mesh deformation in X, Y and Z respectively.
Magnitude of D : magnitude of deformation
Dxyz : mesh deformation vector



OpenLabs

The available variables depend on the  definition in OpenLabs, see Output by OpenLabs section.

Initial Solution


A FINE™/Open with OpenLabs™ computation is started from an initial solution. The following initial solution types are available:



Constant values,
From file,
For turbomachinery,
Techno effects.

Each of these types is described in the next sections ('Techno effects' is described in the section 'For turbomachinery'). 
It is possible to initialize a multi-domain computation by combining different initial solution types. For example, for an impeller and volute configuration, the impeller can be initialized by using For turbomachinery and the volute by Constant values, or the impeller can be initialized by From file and the volute by Constant values.

File Formats


This appendix describes the files used by FINE™ and the flow solver. It is divided into two parts. The first one gives the file format information needed to use FINE™/Open with OpenLabs™, while the second one describes the format of the files used and produced by the flow solver. As FINE™/Open with OpenLabs™ is intended to handle the file treatment for the user, knowing the exact format of all the files used in a simulation process is not required. This Appendix is therefore written for advanced users.
In the following description, it is assumed that all the files are related to a generic project called 'project'. The chapter is divided in six sections:

Rotor/Stator Interaction
Overview
The Rotor/Stator tab gives access to the definition of the rotor/ stator interfaces as shown in FIGURE 18. This tab is only accessible when the mesh contains rotor/ stator interfaces. Rotor/ stator interfaces are computed in HEXPRESS™. Consult the HEXPRESS™ User Manual for more detailed information on how to set this boundary condition. 
The limitations using rotor/ stator interfaces are as follows:

The Full non-matching frozen rotor method is not compatible with rotor/ stator interfaces containing periodic boundary condition with staircase mesh.
When the rotor/ stator connection is a fluid-solid connection, only the Full non-matching mixing plane approach can be used. The frame of the Flow direction will be hidden since there is no flow through the rotor/ stator interface.
The Non reflecting 1D/2D methods are not compatible with unstructured mesh  containing periodic boundary conditions.
In case the rotor/ stator patches include regions where r=0, the limitations are listed in the following paragraph.



FIGURE 18 Rotor-Stator interface definition in steady mode
Zero radius rotor/stator interface

In case a rotor/ stator interface is present including regions where r=0, the user must change the value of the expert parameter RS_iCorrectionFactor to 1. The expert parameter will apply a correction factor for the cell face area between the image and actual mesh. The change is necessary to have consistent results at zero radius.
Note that the expert parameter change of RS_iCorrectionFactor may lead to small discrepancies in mass flow.
Furthermore, following limitations apply in case of a zero radius rotor/ stator interface:

All zero-radius configurations that are not full-circle, are assumed to have a patch corner at zero radius.
If the zero-radius configurations are full-circle and do not have a patch corner at zero radius, two additional limitations exist:The slope of the rotor-stator meridional profile must not be zero at any point, and it must not change sign. In other words, it must always be possible to start from a point on the shroud, and march toward the axis of rotation by following a path with decreasing radius.All the patches on each side of the interface must be connected at their corners with matching connections along the adjacent edges.



Settings of rotor/ stator interfaces
On the left frame, the list of all rotor/ stator interfaces is displayed. Multiple rotor/ stator interfaces can be treated in one single project. The user can click on sign () to view the left and the right patches of the rotor/ stator interfaces. 
On the right, the treatment method must be specified for each rotor/ stator connection. Also, it should be specified the flow direction for the rotor/ stator connection. Note that the flow direction (upstream/ downstream patches) is set automatically if the mesh comes from AutoGrid5™. If the mesh comes from HEXPRESS™, left patches are set as "upstream" and right patches as "downstream". The default settings can be modified if necessary.
Each time the user is passing from steady to unsteady, and vice-versa, the settings of rotor/ stator interface are kept if possible. If not, the default settings will be used.

Up to now, five rotor/ stator interface treatment methods are provided in FINE™/Open with OpenLabs™:
Steady state

The Full non-matching mixing plane approach is respecting an exact conservation of mass flow, momentum and energy through the interface and has fewer constraints on the interface geometry. 
The Full non-matching frozen rotor approach is considering the rotor/ stator interface as a perfect connection and is neglecting the rotor movement in the connecting algorithm. In this approach, the periodicities between rotor stator must be equal.
The Non Reflecting 1D approach is based upon a characteristic analysis of the linearized Euler equations. The characteristic variables are imposed on each side of the rotor/ stator interface. Such a treatment is recommended when wave reflection is observed at the interface, which can occur when the interface is close to the blade.
The Non Reflecting 2D approach is the extension of the Non Reflecting 1D approach. The Non Reflecting 2D approach is also based upon a characteristic analysis of the linearized Euler equations. The characteristic variables are imposed on each side of the rotor/ stator interface. The Non Reflecting 2D approach will produce a better representation of the shock wave crossing a R/S interface.

Unsteady state

The Domain scaling approach is an unsteady simulation technique for the rotor/ stator interfaces. The effect of displacement due to rotation, is taken into account. In this approach, the periodicities between the rotor and the stator must be equal.

Advanced Parameters for Solid Model
All non-interfaced advanced parameters related to the solid model are accessible on the Control Variables page, in the Advanced sub-menu. 
For all solid solvers
iSolidImpl_:	Select the  method solving the energy equation in solid blocks.
0: use the explicit Runge-Kutta time integration method. This is an explicit method. In general, the suggested CFL number is 1. In case of difficulty of convergence, the CFL number should be reduced (e.g. 0.1).
1: use the classical implicit Gauss-Seidel method. When using this method, the value in all solid blocks should be set to 1. This implicit method is unconditionally stable in theory. While experience shows that the GS method is sensitive to the mesh resolution. If the mesh used in the computation presents some refinements (e.g. viscous layers) or is not uniformly cartesian, then the convergence of the GS method can become extremely poor and in some cases, the computation can even diverge.
3 (default): use the Conjugate Gradient (CG) method (Saad, 2003). This method is less sensitive to the mesh resolution, and is unconditionally stable. When iSolidImpl_=3, the flow solver sets solidImpl_gamma_ to 1 automatically.
solidImpl_gamma_:	Control the level of implicitness of the time-marching scheme. Only apply to iSolidImpl_=0/1.
0: leading to a purely explicit scheme;
1: leading to a purely implicit scheme (first order Euler method);
0.5 (default): leading to a blended scheme (second-order Cranck-Nicholson method).
solidImpl_omSOR_:	Over-relaxation parameter, varies between 0 and 2.
For the CG solver (iSolidImpl_=3)
solidImpl_KSPCFLStart_: a ramp of the CFL is applied at the beginning of the computation to increase the robustness of the computation. At the beginning of the computation, the CFL applied is solidImpl_KSPCFLStart_. The CFL is then increased to the value specified in the GUI during the iterations defined by solidImpl_KSPniterCFL_.
solidImpl_KSPniterCFL_:	number of iterations to apply the ramp of the CFL, see solidImpl_KSPCFLStart_ for more details.
solidImpl_KSPMaxIter_:	maximum number of inner iterations for the CG method.
solidImpl_KSPRelTol_:	relative tolerance applied for the convergence criterion of the CG method.
solidImpl_KSPAbsTol_: absolute tolerance applied for the convergence criterion of the CG method.
solidImpl_KSPDivTol_:	divergence tolerance applied in the inner iterations for the CG method.
solidImpl_KSPPrecondType_:	type of preconditioner applied:
1 (default):	Matrix Diagonal scaling preconditioner (available if solidImpl_KSPSolverType_=1)
solidImpl_KSPSolverType_:	type of the solver applied:
1(default):	Conjugate Gradient.
solidImpl_KSPComputeOnGrid_:	applied from the finest to the coarsest multigrid  in solid blocks. The first number corresponds to the finest grid level. By default, the parameter is set to 1 0 0 0, which means that the heat equation will be solved only on the finest grid level of the finest grid.
0: Do not solve the heat equation on the current multigrid.
1: Solve the heat equation on the finest grid level of the current multigrid.
2: Solve the heat equation on each grid level of the current multigrid.

Mesh deformation methods
Introduction
Mesh deformation plays a crucial role in the analysis of multi-physics problems that involve moving bodies and domain with dynamic boundaries. For example, in Fluid-Structure Interaction (FSI), the fluid mesh has to be deformed at each time step according to the displacements computed by the structural solver at the interface of the fluid domain and solid domain. 
In FINE™/Open with OpenLabs™, two kinds of mesh deformation methods are available: mesh deformation based on quaternions and mesh deformation based on Radial Basis Function (RBF). The user can select the method through the expert parameter mov_iMovingGridMeth_. By default, the mesh deformation based on Radial Basis Function (RBF) is used.
The limitations of the mesh deformation module are:

Only available for mono-block projects.
FNMB is not taken into account during the process.
Not compatible with HEXPRESS™/Hybrid mesh.
Mesh deformation module is not compatible with the coarse grid initialization feature. The coupled simulations are suggested to start from a pre-computation solution (without coupling).

Mesh deformation based on quaternions
In this method, the mesh deformation is based on the use of quaternions. The methodology works well when displacements of the boundaries are small but in case of large displacements, the methodology fails, especially when considering meshes with high aspect ratio and viscous layers. 
The approach to mesh deformation includes the following several stages:
First, the initial deformation specified at every point of the boundaries is converted and divided into two components: translation and rotation. Translation is represented in terms of Cartesian displacement vectors, while rotation is described in terms of quaternions.
Once the initial deformation is converted into translations and rotations of the boundary faces, an interpolation procedure is used to propagate the deformation into the volume mesh. The interpolation procedure is based on weighted Laplacian smoothing approach.
Finally, the interpolated data is converted back into the respective set of Cartesian displacement vectors, which are used for final relocation of the mesh points.
Radial Basis Functions
The mesh deformation based on quaternions works only when the mesh deformation is very small. When performing a mechanical coupling simulation, the structure deformation may be very large. In this case, the mesh deformation method using Radial Basis Function (RBF) can be used. The RBF method gives deformed meshes keeping very good quality even for large deformation. For more information on the RBF method, please refer to the theoretical manual.
The main limitations for the RBF mesh deformation method are as follows:

The mesh deformation method using RBF is not compatible with:

FNMB connections,
SNG boundary condition,
Upwind scheme,
Rigid body motion,
Adaptive wall.


 Please note that memory usage can become higher when the number of boundary nodes increases. 
Expert Parameters
The following non-interfaced advanced parameters related to the mesh deformation module are available:
mov_iMovingGridMeth_:	 Choice of the mesh deformation procedure: 
1: Mesh deformation based on the use of quaternions.
2 (default): Mesh deformation based on the use of Radial Basis Function (RBF).
The parameters related to the mesh deformation with RBF:
mov_iMatSave_:	controls the solving  of the mesh deformation matrix in RBF.
0 (default): the matrix will be recomputed automatically.
1: the flow solver will try to read and use the file "projectName.mat" in the computation folder. If the file format is not correct or if the size of the matrix does not correspond to the mesh, the flow solver will automatically recompute the mesh deformation matrix.
In case of ISVMAT=2, an inverse matrix computed in single precision can not be used in a double precision computation. Otherwise, negative cells may appear after mesh deformation.
mov_rad_:	Radius of the support of the Wendland function (RBF).
mov_rbf_:	Function used for RBF mesh deformation:
1: Wendland function.
2 (default): Thin plate spline.
mov_iFromInitMesh_:	 A way to improve the CPU performance of the methodology is, for a given time, to perform deformation starting from the initial mesh instead of starting from the mesh computed at the previous time step. Indeed, if we choose to perform the deformation from the initial mesh, the matrix of the linear system is constant during all computation and can be inverted one time and stored in a file. The expert parameter mov_iFromInitMesh_ controls if deformation is performed starting from the initial mesh:
0: False
1 (default): True

mov_iLevelCoarse_:	 The RBF mesh deformation methodology can be quite memory and CPU consuming. If one considers a computational domain which contains few thousands of boundary nodes, for example 25 000 boundary nodes, therefore the memory required to store half of the matrix (since it is symmetric) is 4.5 GigaBytes. Moreover, the resolution of the linear system will take several hours, which is not acceptable for an unsteady computation with thousands of physical time-steps. A coarsening of the boundaries has been introduced in the FINE™/Open solver in order to reduce the size of the system and therefore increase the speed of the mesh deformation procedure. The coarsening consists at taking into account the nodes that belong to a given multigrid level. The choice of the multigrid level can be set through the expert parameter mov_iLevelCoarse_. By default, mov_iLevelCoarse_=3. This means that the mesh deformation is performed in the finest grid level (with 4 multigrid levels). When setting mov_iLevelCoarse_=0, the mesh deformation will be performed in the coarsest grid level.

Mixing Plane Approach
In the mixing plane approach the flow solution at the rotor/stator interface is azimuthally averaged and the exchange of information at the interface depends on the local direction of the flow. In this section it is described how to use this approach in FINE™. 
Geometrical and Mesh Constraints

The full non matching mixing plane method (Full Non Matching Mixing plane, Non Reflecting 1D and Non Reflecting 2D) is based on the full non-matching algorithm and has clear advantages:

The only remaining constraint being that the rotor/stator patches belonging to a given interface should lie on the same common axisymmetric surface.
An exact conservation of the mass flow, momentum and energy is guaranteed.

Only one blade passage needs to be meshed for both the rotor and the stator, regardless of their respective periodicities.


FINE™ Settings


The mixing plane approach is a steady simulation technique which requires to set the Time Configuration to Steady on the General properties page.
For each rotating block the rotation speed is defined under the Rotating Domains tab on the Rotating Machinery page.
  Under the Rotor/Stator tab on the Rotating Machinery page, the user has to specify for each of the rotor/stator connections:

the rotor/stator connection treatment method:

Full Non Matching Mixing plane, 
Non Reflecting 1D. 
Non Reflecting 2D.
The Non Reflecting 1D/2D approach can not be used when the flow perpendicular to the rotor/stator interface is supersonic.
The use of the Non Reflecting 1D/2D approach is limited to steady simulations without preconditioning.
The Non Reflecting 1D/2D approach is only compatible with perfect gas or real gas.

the flow direction.




Illustrative Example

To illustrate the mixing plane approach the flow in Aachen turbine is considered as shown in FIGURE 10. Due to the pitchwise averaging process one can see that the wake occurring slightly downstream the trailing edge of the first stator blade is spread when entering in the rotor blade passage. If the rotational speed of the rotor blade is high, this approximation is acceptable since one can consider that the rotor blade "sees" a more statistically averaged flow. If the rotational speed is low, this approximation is essentially invalid and thus another method should be considered.
In some cases, i.e. in low pressure ratio compressors or turbines, the losses at the rotor/stator interfaces are in the order of magnitude of the overall gain in the machine. In such cases, it is recommended to use an unsteady approach


FIGURE 10 Aachen turbine: Mixing Plane approach


Non-interfaced Advanced Parameters



Additional parameters related to the mixing plane method are available in the list located in the Advanced tab of the Control Variables page.
RS_NbH2DNR_:	sets the number of harmonics used for DFT and inverse DFT when using the non-reflecting 2D Rotor/Stator interface. The default value is 3.
RS_LocalCorrection_:	 In some particular cases, a problem of mass flow conservation through a non reflecting 1D or 2D rotor-stator interface can arise. This can be improved by deactivating the local enthalpy correction through the expert parameter RS_LocalCorrection_.
0: local enthalpy correction deactivated
1 (default): local enthalpy correction activated

The Interface for an Unsteady Computation

When selecting Unsteady time configuration in the General Properties page the following additional parameters become accessible in the FINE™/Open GUI:
Rotating Machinery

On the Physical Configuration\Rotating Machinery page, under the Rotor/stator tab, the Domain scaling rotor/stator interface treatment can be activated.


Control Variables

On the  Computation Control/Control Variables page under the tab General, the following parameters appear when selecting an unsteady time configuration:


If Time averaged solution activated, the value  	indicates the number of iteration from which the time-averaging of the solutions will be started.
Time step


Physical time step: in general cases, the user specifies the magnitude of the physical time step in seconds. This time step is constant through the whole calculation. In cases of turbomachinery applications where Rotor/Stator interfaces are detected, the Number Of Angular Positions is requested instead of the Physical time step. A variable physical time is automatically computed by the solver if a variable rotational speed is imposed in  the OpenLabs™ environment using the internally defined rot_Omega_ constant. A variable physical time step can also be directly imposed in  the OpenLabs™ environment using the internally defined PhysTimeStep constant. In both cases, the expert parameter ta_iVariableTimeStepping_ must be set to 1 in the Global parameters list in the Advanced tab in order to activate the use of a variable physical time step.


Number of time steps: to define the number of time steps to perform.



Steady initialization


Number Of Steady Iterations: the number of iterations to initialize the unsteady computation. Such initialisation is performed with the steady state algorithm, using fixed geometry and mesh as well as constant inlet/outlet boundary conditions. In case this initialisation procedure is used the steady state iterations can even be proceeded by a full multigrid process allowing a rapid initialisation of the flow.
Save Steady Solution Every: the number of iterations at which the solution of steady initialisation is saved

Steady initialization is not available when From file is used in the Initial Solution / Initial Solution page.


Output files


Save Solution Every: allows to save the solution after a constant number of time steps. By default the output files will be overwritten, every time the solution is saved. In order to keep the successive unsteady solutions, the option Visualization files must be set to Multiple files.
Time averaged solution after # time steps: When activated, the time averaged solution will be computed and saved in a ".avg" file after the imposed time steps. After the user activates this option, the user must go to the Computation Control / Outputs page under the category Unsteady to select the quantities that will be time averaged. All the quantities surrounded by < > can be selected.

The quantities that can be time averaged appears only when the option  Time averaged solution after # time steps is activated.
 The time averaged solution is computed after the imposed time steps  on fine mesh. All the quantities are averaged as follows:



where  is the time step in time step  i and T is the period.

Visualization files: controls the output files for visualization.

One file: One set of output files for visualization in CFView™ is only saved at the end of the computation.
Multiple files: Multiple sets of output files are saved for visualization in CFView™ during the computation (every x time steps as specified in Save Solution Every).

Intermediate restart files: controls the output files for unsteady restart. In both cases (One file/Multiple files), second order restart is possible.One file: One set of output files for unsteady restart is only saved at the end of the computation.Multiple files: Multiple sets of output files are saved for unsteady restart during the computation (every x time steps as specified in Save Solution Every).





Second Order time-accurate scheme


The FINE™/Open solver performs second order accurate simulations in time. When requesting a restart of an unsteady computation, the FINE™/Open solver will automatically look for a ".btm1" file containing the solution at previous time steps. If this file exists, a second order restart is performed. If this file is not found, a first order scheme is used for the first time step.

Definition of Global Residual

The residuals are computed by the FINE™/Open solver as a flux balance (the sum of the fluxes on all the faces of each cell):

.
The root mean square of the residuals is computed using the following formula:

,
and the maximum of the residuals in the same way:

,
with log the logarithm to the base ten.
On the Convergence History page the global root mean square of the residuals normalized by its value at the first iteration is shown. These values are stored in the file with extension ".steering.binary". Additionally the global residuals are shown in numerical values in the Task Manager window. The RMS ("avRes") value listed in the Task Manager window is the global root mean square normalized by its value at the first iteration. The maximum ("maxRes") value is the maximum residual normalized by the RMS residual at the first iteration.
The equation associated to the displayed residuals is specified through the expert parameter out_toDisplay_ located in the Advanced tab of the Computation control/Control Variables page. By default, the mass equation is used.
If the initial solution is already quite close to the final solution, the obtained residual values are not as low as they would have been when the initial solution is far from the final solution. The obtained residuals values depend on the difference of the used initial solution with the final solution.

Variables, Operators and Control Statements
Comment Lines

The character "#" is used to comment out complete lines or part of the lines. For example:
# This line will be ignored 
@ CONSTANT:  <constant name 1>   # Everything after this symbol will be ignored


Line Break

In some cases, in order to avoid too long lines, it might be useful to break them (for example, in case that a very long formula needs to be introduced). The character "\" is used to break a line. For example:
->EXPRESSION: sigma * StaticTemperature + \
                             + beta * (StaticTemperature–Ref_Temp)
The expression above is equivalent to:
->EXPRESSION: sigma * StaticTemperature + beta * (StaticTemperature–Ref_Temp)
If a line break is used, all the text written in the same line after the symbol "\" will be ignored. For example, the text "This is a source" will be ignored in the following example:
->EXPRESSION: sigma * StaticTemperature  \  This is a source
                             + beta * (StaticTemperature–Ref_Temp)


Implicit Expression


Sometimes, the relation between variables may be implicit. In this case, the variable must be solved iteratively. In OpenLabs, the implicit expression can be solved by using the Newton-Raphson method or by using the user defined iterative expression.
The Newton-Raphson Method

To solve the implicit expression, the relation can be re-written as a zero function f(x)=0 and is solved by:



To formulate the iterative equation, the user has to provide the jacobian  of the function, either analytically (keyword Jacobian) or numerically (keyword Disturbance), and some other informations. The format of giving an implicit expression in the resource file is as follows:
->EXPRESSION: SOLVE(<name of variable, for example x>):{
Zero_Function: <f(x)>
Jacobian: <dfdx>    #(Optional)
or
Disturbance: <dx>    #by default 
InitializeTo: <x0>    # by default 0  (Optional)
LowerLimit: <xmin>
Upper Limit: <xmax>
Iteration_Number: <max number of iterations>     # by default: 30 (Optional) 
Converge_Criterion: <eps>     # by default:  (Optional)
}
If the domain of the implicit expression does not cover all real number, e.g. the domain of log(x) is x>0, it's necessary to either rewrite the expression so that the domain covers all real number, or provide limiters in order to improve the robustness.
For example, to solve x at a given y0, where y=f(x) and f is a monotonically increasing function in the region of [xmin,xmax], the Newton-Raphson method could be used:
->EXPRESSION:SOLVE(x):{
Zero_Function: f(x)-y0
Jacobian: dfdx
InitializeTo:x0

}


User Defined Iterative Expressions

Alternatively, the implicit expression can be solved by an user defined iterative expression:



In this case, the keyword "ITERATIVE" must be used. The iterative function should be given by the user with the keyword "Iterative_Function". The format of giving an implicit expression in the resource file is as follows:
->EXPRESSION:SOLVE(<name of variable, for example x>):ITERATIVE{
Iterative_Function: <x>=<f(x)>
InitializeTo: <x>=<x0>
Iteration_Number: <max number of iterations>     # by default: 30 (Optional) 
}
Besides the variable to be solved, there could be several auxiliary terms being iterative. These auxiliary terms cannot be used in the other expressions and should be defined in SOLVE {} of the current expression. The user-defined iterative expressions can be written as:
->EXPRESSION:SOLVE(<name of variable, for example x>):ITERATIVE{
Iterative_Function: <aux name1> = <aux expression 1>
...
Iterative_Function: <aux nameN> = <aux expression N>
Iterative_Function: <x>=<f(x)>
InitializeTo: <aux name1> = <initial value of aux1>
...
InitializeTo: <aux nameN> = <initial value of auxN>
InitializeTo: <x>=<x0>
Iteration_Number: <max number of iterations>     # by default: 30 (Optional) 
}
For example, to solve x at a given y0, where y=f(x) and f is a monotonically increasing function in the region of [xmin,xmax], the Newton-Raphson method could be used:
->EXPRESSION:SOLVE(x):ITERATIVE{
Iterative_Function:y=f(x)
Iterative_Function: xLower=IF(y<y0) x    ELSE xLower
Iterative_Function: xUpper=IF(y<y0) xUpper    ELSE x
Iterative_Function:x=0.5*(xLower+xUpper)
InitializeTo:xLower=xmin
InitializeTo: xUpper=xmax
InitializeTo:x=x0
}




 Discrete Expression


Discrete expressions are introduced into OpenLabs so that the user can impose a profile data to a variable. According to the dependency, the profiles can be divided into three types:

Profiles dependent on geometric variables, for example, Vx(x). They are usually used in boundary conditions.
Profiles dependent on CFD variables, for example, Cp(T). They are usually used in defining    fluid properties. 
Profiles dependent on physical time, for example, a time dependent source term.

The user has the flexibility to add a profile dependent on arbitrary variable names. The name of the dependent variables must be written explicitly (in the resource or the .dat file).
The profile data can be inputted by file or defined in the resource.
Import Discrete Expression by File

When importing the discrete expression by a file, the user should give the file name after the keyword "->EXPRESSION: PROFILE":
->EXPRESSION: PROFILE<File name>
The inputted file can be in the .p format or .dat format:

The format with the extension .p has the fixed possibilities and recognized by the identity number inside the file. The data must be given in structured format, see File Format for more details about the .p format.
The format with extension .dat is shown below:

<abscissa1> <abscissa2> ...
<number of point of abscissa1> <number of point of abscissa2> ...
<data>
The data in the .dat format should be given in structured format, except for 2-dimensional profile that can be given in both structured/unstructured formats.
In case that the interpolated point exceeds the data range, the value will be clipped by default (LIN_INTERPOLATE_CLIP). However, it is possible to use extrapolation at boundary by using the keyword (LIN_INTERPOLATE_EXTRAPOLATE):
->EXPRESSION: PROFILE: LIN_INTERPOLATE_EXTRAPOLATE<File name>
The linear interpolation of the profile to find the value at a given point in the domain may be time consuming. A preprocessing can be taken for the structured profiles to save time. The profile data are remapped as an equidistant mesh. The borders in each dimension can be obtained via a formula instead of a bisection searching loop. However, please note that this preprocessing is not recommended for the high non­linear profiles since the accuracy would be lost in the remapping process. It is deactivated by default. To activate this preprocessing, the profile expression can be written as:
->EXPRESSION: PROFILE: REGULARIZE_EQUIDISTANT<File name>
In case that the data are loaded from a file, the profile data can be reloaded from this file at every certain iterations:
->EXPRESSION: PROFILE: RELOAD_EVERYITER(number_iteration)<File name>


Define Discrete Expression in the Resource

When defining the discrete expression in the resource, the user can give the complete data after the keyword "->EXPRESSION: PROFILE" with following format:
->EXPRESSION: PROFILE(abscissa1, abscissa2, ..., abscissaN) { 
nbPoint_abscissa1 nbPoint_abscissa2 ... nbPoint_abscissaN
data1_min data2_min … dataN­1_min dataN_min ordinate
data1_min data2_min … dataN­1_min dataN_min+ ordinate
...
data1_min data2_min … dataN­1_min dataN_max ordinate
data1_min data2_min … dataN­1_min+ dataN_min ordinate
...
data1_min data2_min … dataN­1_min+ dataN_max ordinate
…
...
data1_max data2_max … dataN­1_max dataN_min ordinate
...
data1_max data2_max … dataN­1_max dataN_max ordinate
           }
In particular, 2-dimensional profile can be given in points cloud:
->EXPRESSION: PROFILE(abscissa1, abscissa2) { 
N
data1_1   data2_1   ordinate
data1_2   data2_2   ordinate
...
data1_N  data2_N  ordinate
           }
When defining the discrete expression in the resource, the user can also give the expression, instead of giving the data, after the keyword "->EXPRESSION: PROFILE". The expression and the ranges should be provided with following format:
->EXPRESSION: PROFILE(abscissa1, abscissa2, ..., abscissaN){
Function: <expression>
NumberOfPoint: <abscissa1>, <number of point in abscissa1>
Range: <abscissa1>, <minimum value>, <maximum value>
...
NumberOfPoint:  <abscissaN>, <number of point in abscissaN>
Range: <abscissaN>, <minimum value>, <maximum value>
OutToFile: <name of the file>   # (optional, the path is by default the computation folder)
} 
The discrete expression defined by an expression will be computed only once before the flow iteration. The build discrete expression could be outputted into a file by using the optional keyword OutToFile. This function is usually used to reduce the CPU time is case that the expression is quite complex, such as an user defined EOS.
In case that the interpolated point exceeds the data range, the value will be clipped by default (LIN_INTERPOLATE_CLIP). However, it is possible to use extrapolation at boundary by using the keyword (LIN_INTERPOLATE_EXTRAPOLATE):
->EXPRESSION: PROFILE: LIN_INTERPOLATE_EXTRAPOLATE{
...
}
The linear interpolation of the profile to find the value at a given point in the domain may be time consuming. A preprocessing can be taken for the structured profiles to save time. The profile data are remapped as an equidistant mesh. The borders in each dimension can be obtained via a formula instead of a bisection searching loop. However, please note that this preprocessing is not recommended for the high non­linear profiles since the accuracy would be lost in the remapping process. It is deactivated by default. To activate this preprocessing, the profile expression can be written as:
->EXPRESSION: PROFILE: REGULARIZE_EQUIDISTANT{
...
}




Mathematical Operators

The following mathematical operators can be used. An example is included to illustrate the use.







Mathematical Operator


Keyword


Example






sine


sin


sin(angle)




cosine


cos
                                


cos(angle)




tangent


tan


tan(angle)




arc sine


asin


asin(x/r)




arc cosine


acos


acos(y/r)




arc tangent


atan


atan(y/x)




arc tangent of y/x


atan2


atan2(y,x)




hyperbolic sine


sinh


sinh(angle)




hyperbolic cosine


cosh


cosh(angle)




hyperbolic tangent


tanh


tanh(angle)




area hyperbolic sine


asinh


asinh(y/r)




area hyperbolic cosine


acosh


acosh(x/r)




area hyperbolic tangent


atanh


atanh(y/x)




Base-e exponential function


exp


exp(-TA/StaticTemperature)




Base-2 exponential function


exp2


exp2(-TA/StaticTemperature)




Cubic root


cbrt


cbrt(x)




Hypotenuse of a right-angled triangle whose legs are x and y


hypot


hypot(x,y)




Natural logarithm (base-e)


log


log(x)




Binary logarithm (base-2)


log2


log2(x)




Common logarithm (base-10)


log10


log10(x)




Raise to power


pow


pow(StaticTemperature,4.0)




Square root


sqrt


sqrt(TurbK)




Returns the floating-point remainder of numer/denom


fmod


fmod(numer,denom)




Maximum of two reals


MAX


MAX(TurbK,0.0)




Minimum of two reals


MIN


MIN(1.0,yfrac)




Largest integer less than or equal to x


floor


floor(x)




Smallest integer greater than or equal to x


ceil


ceil(x)




Round x to the nearest integer


round


round(x)




Absolute value


fabs


fabs(x)




Gradient of a variable in x direction


GRAD(VariableName,x)


GRAD(Vx,x)




Gradient of a variable in y direction


GRAD(VariableName,y)


GRAD(Vx,y)




Gradient of a variable in z direction


GRAD(VariableName,z)


GRAD(Vx,z)




1D integration


INTEG1D(expression, variable name, min, max)


INTEG1D(cp,T,Tref_,StaticTemperature)




2D integration


INTEG2D(expression, boundary name)


INTEG2D(Density*Vx, ALLINLETS)




3D integration


INTEG3D(expression)


INTEG3D(1)




Variable at the first fluid cell next to a boundary face. This operator should be only used to define boundary conditions.


upcell(VariableName)


upcell(StaticTemperature)



Dot product

DOT(vector1, vector2)

DOT(velocity,velocity)



Note:

When using the operator INTEG1D(), the bounds min and max can be given by a variable name which means it equals to the variable value at the position where the expression is analyzed (in cell, on boundary face...). For example:
INTEG1D(cp_prof, StaticTemperature, TRef_, StaticTemperature) 
When using the operator INTEG2D()

ALLINLETS/ALLSOLIDS/ALLOUTLETS refer to all inlets/solids/outlets in the current block.
In case that the expression inside INTEG2D is a vector, the normal vector should be written in the expression, for example, 

INTEG2D( Density*(Vx*NormalX+Vy*NormalY+Vz*NormalZ) , ALLINLETS)
The following limitations apply for the INTEG1D/INTEG2D/INTEG3D operators:

The indefinite integration is not doable.
The INTEG2D is used only for the integral over boundary patches.
The INTEG3D is used only for the integral over computational domains.
The INTEG1D is used only for the physical variable dependent profiles/expressions. 
Integration over time is not available. 
The INTEG2D/3D cannot be computed over the boundaries/domains that involve both solid and fluid blocks.




Logical Operators

The following logical operators can be used.







Logical Operator


Keyword


Alternative Syntax






Logical AND


AND


&&




Logical OR


OR


||




Logical negation


NOT


!




Equal to


EQ


==




Not equal to


NOTEQ


!=




Greater than


GREATER


>




Less than


LOWER


<




Greater than or equal to


GREATEREQ


>=




Less than or equal to


LOWEREQ


<=






Conditional Statements

The following conditional statements can be used. 





Conditional Operator






IF




ELSEIF




ELSE




The condition of the "IF" and "ELSEIF" must be written inside a parenthesis. See the following example:



The expression in the resource will be written as follows:
->EXPRESSION: A = IF (B>=10)  250   ELSEIF (B>5 AND B<10)  50  ELSE 100
By using the line breaks, the same expression can be written as follows:
->EXPRESSION: A =  IF (B>=10)                            250  \
                                       ELSEIF (B>5 AND B<10)   50    \
                                       ELSE                                     100 
More complex structures can be used. For example:



The expression in the resource will be written as follows:
-> EXPRESSION: A = IF(C>5) IF (B>=5)                              15   \
                                                      ELSEIF (B>3 AND B<5)      19   \
                                                      ELSEIF (B>1 AND B<=3)   17   \
                                                      ELSE                                     18   \
                                       ELSE     IF (B>=10)                            28   \
                                                      ELSE                                      33 
The same expression can be written in a less intuitive form:
-> EXPRESSION: A = IF(C>5) (IF (B>=5) 15 ELSEIF (B>3 AND B<5)  19  \
                                      ELSEIF (B>1 AND B<=3)   17   \
                                      ELSE 18) ELSE   (IF  (B>=10) 28 ELSE 33 )
A conditional statement with several conditions must start with an IF and end by ELSE. The keyword ELSEIF is optional.
A conditional statement can only be used with the keyword EXPRESSION. It can not be used to define constants. For example:
# This is wrong
=>AUXTERMS
@ invYWall = IF (CellVolume>=1e-20)  (2*BFaceSurface)/(CellVolume) \
                        ELSE                                  (2*BFaceSurface)/(CellVolume+1e-20)
# This is right
=>AUXTERMS
@ AUXTERM: invYWall
->EXPRESSION:  IF (CellVolume>=1e-20)  (2*BFaceSurface)/(CellVolume) \
                                ELSE                                 (2*BFaceSurface)/(CellVolume+1e-20)


Geometrical quantities

The following geometrical quantities can be used. 




Geometrical Quantities


Keyword






Cartesian coordinates


xCoord, yCoord, zCoord




Cylindrical coordinates


rCoord, tCoord, aCoord




Volume of the cell


CellVolume




Surface area of a boundary face


BFaceSurface




Components of  surface area vector of a boundary face 


xfaceN, yfaceN, zfaceN




Components of unit surface area vector of a boundary face


NormalX, NormalY, NormalZ




Distance to wall of a cell (used, for example, for turbulence models)


distanceToWall




Normal distance of a boundary cell from the boundary (used to define boundary conditions)


dn






Time variable

The time variables are used to define temporal dependent terms (e.g. time dependent source terms, time dependent boundary conditions,…). These variables are used for unsteady computations only.






Time Variable


Keyword






Physical Time


Time



Time accurate iteration number
TA_IteNum



Maximum time accurate iteration number
TA_IteMax






Vector variable

A vector variable can be defined by its three scalar components enclosed by square brackets, for example [Vx,Vy,Vz]. The vector can directly be used in any expressions.
Alternatively, to simplify the writing, the user can also define the vector in the section auxiliary terms starting with the line "=>AUXTERMS".
=>AUXTERMS
@Velocity=[Vx,Vy,Vz]
Then, the vector name can directly be used in any expressions. The user can also use only one of three components of the vector. For example, Velocity[0] indicates that this is the first component of the vector Velocity.


Control point


In OpenLabs™, the user can use the local value on a control point. The control point can be an internal control point defined in the FINE™/Open graphical interface, or an user defined control point in OpenLabs™.
The variable value on a local control point is expressed by the variable name following with a control point:

In case of an internal control point, the expression should be written as:
VarName[<ID of control point>] #for example Density[CTRL_POINT_b0_1]
In case of an user defined control point, the control point should be expressed by its three Cartesian coordinates enclosed by square brackets. The expression should be written as:
VarName[<coordinates of control point>] #for example Density[0.5, 1, 1]

The coordinates of the control point must be given by values. For example, the expression Density[x,y,z] is wrong.
The control point should be used only for the CFD variables (that are not boundary only variables). It is not suggested to be used for Time and geometrical variables.
The VarName can be the name of an internal quantities or an auxiliary quantities.
The variable value on a local control point can be used in any expressions, except when using a control point value in SOLVE and PROFILE, it has to be defined as an auxiliary term.

List of Advanced Parameters
Under the Advanced tab of the Computation control/Control Variables page is a list of non-interfaced expert parameters. As stated in the interface, these parameters should not be used unless explicitly stated in this manual. This chapter contains a list of all non-interfaced expert parameters that are described in this manual. For each parameter a reference is given to the corresponding section. If more information is desired, please contact our local support office.
List of Advanced Parameters
_typeOfBlockID :	the type ID of the block
agglomerationNEW_	: the agglomeration method
bc_treatThermoOnFace_ : control applying thermodynamic and state laws
bc_wallCondensableFluid_ :  control the type of relation used to compute the density at the wall in case of condensable fluids
cavAmin_ :	user parameter AMIN related to Cavitation
cavFCM_cL_:	Speed of sound of the liquid phase used in the transport equation model.
cavFCM_cL_:	Speed of sound of the vapor phase used in the transport equation model.
cavFCM_Cturb_:	Modeling constant  to account for the turbulence-cavitation interaction.
cavFCM_iFullPreconditioning_:	Control if consider the volume or mass transport equation in the preconditioning matrix when the transport equation cavitation model is activated.
cavFCM_iVaporMassFracEqs_:	Select the vapor equation type used in the transport equation model.
cavFCM_MinDensClip_:	The allowed minimum mixture density used in the transport equation model.
cavFCM_Singhal_Cc_:	Modeling constant in Singhal model.
cavFCM_Singhal_Ce_:	Modeling constant in Singhal model.
cavFCM_SourceRelaxFactor_minus_:	Relaxation factor for the negative source term (condensation) when the transport equation cavitation model is activated.
cavFCM_SourceRelaxFactor_plus_:	Relaxation factor for the positive source term (cavitation) when the transport equation cavitation model is activated.
cavFCM_SourceTerm_:	Select the formulation used in the source term.
cavFCM_SurfTension_:	Surface tension used in Singhal model.
cavFCM_Tani_Cc_:	Modeling constant in Tani model.
cavFCM_Tani_Ce_:	Modeling constant in Tani model.
cavFCM_Zwart_Fc_:	Modeling constant in Zwart model.
cavFCM_Zwart_Fe_:	Modeling constant in Zwart model.
cavMuL_ :	dynamic viscosity of the liquid phase
cavMuV_ :	dynamic viscosity of the vapor phase
cavPreFactorRhoDissip_ :	 control the artificial dissipation of the continuity equation
cavPrV_ :	Prandtl number of the vapor phase
cavPv_	: vapor pressure
cavRhoL_ :	density of the liquid phase
cavRhoV_ :	density of the vapor phase
combEquRatioCorrCoefs_	: constant for equivalence ratio correlation
combInitHybrid_	: Intiallize with fully burned state for partially premixed model
combReInitProgVar_	: reinitialization methods of the progress variable
combSchmidtTurb_	: the turbulent Schmidt number
combSDissConst_	: constant for the mean scalar dissipation rate
combTimeStep_: select the method used to compute the combustion time step
DeltaPress_RestartCav_	: Initial pressure difference when restart for cavitation
dtw_method_ : the algorithm is used for wall distance calculation
EntrFx_	: values of the entropy fix for the linear/non linear fields or the parametersVl and Vn used in the limiter of the central matrix dissipation scheme
GP1Free_	: Initial value for the G-field of the P1 radiation model
gradientScheme_	: compute gradient at cell center
HypInit_ : activate 1st order upwind scheme initialization
HypInitCFL_	: CFL number of 1st order upwind initialization
HypInitItMax_	: the number of iteration of 1st order upwind initialization
HypInitResSmoo_	: activate residual smoothing for 1st order upwind initialization
iAsFT_ :	reproduce the results obtained with FINE™/Turbo
iCavitation_	: parameter to activate cavitation
iCondTableClip_	: the computing method of the thermodynamic tables
iCstInterpol_ :	the method of interpolation to get the nodal values
iFluxAverage_	: the discretization of the fluxes for the Jameson scheme
iFluxAverageFMG_ :	the discretization of the fluxes for the Jameson scheme
iFnmb_treatment	: computes the fluxes at FNMB interface
iGhostCylindExtrapol_	: computes dummy cell coordinates	
iHStablesNotUsed_	: use PHS table or SHP table
iLagr_EvapModel_	: evaporation model for the Lagrangian
iLagr_Evaporation_	: activation of evaporation for the Lagrangian
iLagr_HeatReferenceTemp_ :	model for calculation of the reference temperature
iLag_IntegrationScheme_	: select the Lagrangian integration scheme
iLagr_TimeStepCriteria_ :	 time step criteria for the Lagrangian method
iLagragian_Max_Iterations_ :	 maximum number of iterations for one Lagrangian cycle
iLagrInjectionPoints_: activates the functionality of adding Lagrangian injection points from a file.
iLagrOutputIterations_	: frequency of writing intermediate Lagrangian output
iMpCCIIterCoupling_	: iteration interval for steady MpCCI coupling
iMpCCISteadyMode_	: force to compute a steady solution with MpCCI coupling
iMpCCIzSize_ 	: specify the size of the cell in the third direction in 2D cases
iPartPremNonAdiabEffOnFlameSpeed_: control the non-adiabatic effect when calculating the laminar/turbulent flame speed in partially-premixed combustion.
iRestartCav_PressDiff_	: control restart for cavitation
iSolidImpl_	: select the time-marching method for solid blocks
iSmartRestart_ : activate the option of saving backup files in case of crash and the possibility of a smart restart.
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied to scale the heat fluxes boundary condition(s)
ke_Ceps1_	: Ceps1 constant in the k-eps equations
ke_Ceps2_	: Ceps2 constant in the k-eps equations
Lag_MaxLocalTimeStep_ :	 Maximum particle time step
Lag_MinLocalTimeStep_	 : Minimum particle time step
Lagr_CoeffConductivityVap_ :	 Coefficients for the conductivity of evaporated vapor
Lagr_CoeffcpVap_ :	Coefficients for the heat capacity of evaporated vapor
Lagr_CoeffDynViscVap_	: Coefficients for the dynamic viscosity of evaporated vapor
Lagr_HeatCapacity_liquid_	: heat capacity of the dispersed phase
Lagr_LatentHeatVaporization_ :	 latent heat of vaporization of the Lagrangian liquid
Lagr_NbOfEstimatedStepsPerCell_ :	 Number of step a particle does per cell
Lagr_SumAtomicDiffVol_ :	 diffusion coefficient in droplet evaporation models
LagrHeatReferenceFactor_	 : value for A-rule to calculate reference temperature
LagrInjectionPointsDistanceTol_: tolerance in meters to check if injected parcels are inside or outside the computational domain when iLagrInjectionPoints_=1.
LagrMixFracSchmidtsTurb_	: Turbulent schmidt number for  mixture fraction
LagrRelaxSourceTerms_ :	 relaxation factor for Lagrangian source terms
Lagr_CoeffcpVap_	: Coefficients for the heat capacity of evaporated vapor
MSP_cpConstSpecies_ :	 isobaric heat capacity of each species for a mixture
MSP_cpSpeciesNASACoeff1_	:   NASA polynomials for heat capacity of species
MSP_iConductivityLaw_ :	  parameter to steer the thermal conductivity law of species
MSP_iConductivityMixingLaw_ :	  mixing law for thermal conductivity of species
MSP_iCpSpeciesLaw_ :	law for isobaric heat capacity of each species
MSP_iDiffusionLaw_ :	law for calculating viscosity of each species
MSP_iMultispecies_ :	activation of the multi-species environment
MSP_iSpeciesEOSModel_ :	   law for determining Cp for each species
MSP_iViscosityLaw_	: law for calculating viscosity of each species
MSP_lambdaConstSpecies_	:   thermal conductivity of each species
MSP_massDiffCoeffConstSpecies_ :	  laminar diffusivity of each species
MSP_molarMassSpecies_	:  molar mass of each species
MSP_muConstSpecies_ :	 dynamic viscosity coefficient for each species
MSP_NUM_YSPEC_ :	number of species
MSP_schmidtSpecies_ :	laminar Schmidt number of each species
MSP_Talpha_	: coefficient of limiting thermodynamic variables
MSP_Tinf_	: lower bound of the temperature
MSP_TinfSpecies_ :	 for each species in Sutherland's law
MSP_Tsup_	: upper bound of the temperature
MSP_yspecFree_ :	initial value of each species mass fraction
mg_iPrecondFoF_	: compute forcing function	
mov_iFromInitMesh_	: deformation starting from a initial mesh
mov_iLevelCoarse_	: choose the multigrid level for MpCCI coupling
mov_iMatSave_:	controls the solving  of the mesh deformation matrix in RBF.
mov_iMovingGridMeth_	 : Choice of the mesh deformation procedure
mov_rad_	: radius of the support of RBF
mov_rbf_	: function used for RBF mesh deformation
mpcci_Relax_ : temperature relaxation coefficient for MpCCI coupling
newParallelAgglomeration_: switching this parameter to 1 will ensure that the parallel agglomeration is independent of the number of processors.
NLH_HarmoPressureInit_: Real and imaginary part of the initial harmonic pressure values set for all harmonics.
out_allRes_ta_ :	the interval of the residual outputs
out_copyFiles_: avoid to copy mesh files to computation folder
out_CPUperIteration_	: output of the CPU time of per iteration
out_derQntFromNode_ : control how to compute derived quantities
out_displayForcePatchOfGroup_ : 	output force and torque for each individual patch
out_forceTorqueAreaDefined_	 : output area-defined force and torque
out_gaugeForceTorque_	: get lift and drag independent of the farfield static pressure
out_htcDef_: define reference temperature used to compute heat transfer coefficient
out_mfFileVersion_ : control the structure of .mf output file.
out_periodicForcesAndMoments_ : control the integration limits when computing the forces and moments in the .wall output file.
out_resCluster64_ :	output of the convergence history in parallel computation
out_saveAHEX_ :	save partitioned files
out_snsOnCFV_ :	output of adaptation criteria to CFView™
out_toDisplay_ :	select equation for global residual display
out_wallForcesPerIt_	: output lift, drag and moment per iteration on the fine mesh
out_writeAllCtrlPts_ta_: write the control points at every time-step or sub-iteration
out_writeCtrlPts_ta_: the interval of the  outputs at control points
out_writeForces_ta_: the interval of the force outputs
PartitionerParallel_	: activate the parallel partitioner
preco_NLH_Vunst2Factor_: coefficient controlling the unsteady preconditioning velocity of the Merkle preconditioning in order to be able to run harmonic method for low speed flow applications. Can take the value 0 or 1.
preco_pcEpsVLim_: Coefficient of Vref when computing vlim in the Merkle preconditioning.
preco_pcEpsVLimC_: Coefficient of the speed of sound when computing vlim in the Merkle preconditioning.
phys_PrandtlTurb_	: turbulent Prandtl number (k-ε model)
rot_iVelSy_	: select the solved velocity for rotating systems
Rad_AnisotropicScatteringCoeff :	 Anisotropic scattering coefficient
Rad_ScatteringCoeffValue :  Scattering coefficient value
Rad_ScatteringModel	: Scattering model
RadFVM_AreMirrorsSpecular	 : radiative heat transfer boundary condition at mirror
RadFVM_FixedIterationNumber	: maximum Gauss-Seidel iterations to solve RTE
RadFVM_IterationNumber :	 No. of Gauss-Seidel iterations per global iteration
RadFVM_NbIter :	Number of flow iterations per radiation iteration
RadFVM_NodalInt_AngularErrorTol	  : Tolerance level to solve RTE
RadFVM_Nphi	: angular discretization in Phi direction
RadFVM_Ntheta	: angular discretization in Theta direction
RelaxCombProgVars_	: relaxation factor for the progressive variable equation
RelaxCombvars_	: relaxation factor for combustion variables
RS_iCorrectionFactor_ : Correction factor for zero radius rotor/stator interface
RS_LocalCorrection_ :	local enthalpy correction in non-reflecting R/S
RS_NbH2DNR_ :	number of harmonics used in non-reflecting 2D R/S
RS_OutputMultiple_ :	control saving of the solutions in R-S simulations
S2S_iLevelCoarse_	: choose the multigrid level for S2S
S2S_NbIter_	: iteration interval solving S2S
S2S_nbRayPerFace_	: the number of the rays per face
S2S_BCCycle_: number of cycles of solving the radiosity equation  at each Runge-Kutta stage.
S2S_InnerIter_:  number of the Gauss-Seidel iterations solving the radiosity equation.
S2S_RelaxFactor_: the relaxation factor used in the Gauss-Seidel iteration solving the radiosity equation.
solidImpl_gamma_	: implicitness of the time-marching scheme
solidImpl_omSOR_	: over-relaxation parameter
solidImpl_KSPCFLStart_: starting CFL number used in the CFL ramp.
solidImpl_KSPniterCFL_:	number of iterations to apply the ramp of the CFL.
solidImpl_KSPMaxIter_:	maximum number of iterations for the CG method.
solidImpl_KSPRelTol_:	relative tolerance applied for the convergence criterion of the CG method.
solidImpl_KSPAbsTol_: absolute tolerance applied for the convergence criterion of the CG method.
solidImpl_KSPDivTol_:	divergence tolerance applied for the CG method.
solidImpl_KSPPrecondType_:	type of preconditioner applied.
solidImpl_KSPSolverType_:	type of the solver applied.
solidImpl_KSPComputeOnGrid_:	solve or not the heat equation on the current multigrid level.
spc_artDiss2ndCoef_	: Coefficient k(2) for 2nd order dissipation (central scheme coefficient)
spc_artDiss4thCoef_	: Coefficient k(4) for 4th order dissipation (central scheme coefficient)
spc_artMatDiss2ndCoef_	: Coefficient k(2) for 2nd order dissipation (central matrix scheme coefficient)
spc_artMatDiss4thCoef_	: Coefficient k(4) for 4th order dissipation (central matrix scheme coefficient)
spc_artMatDissfmg_	: applied spatial numerical scheme during coarse grid initialization if the central matrix scheme is selected
spc_dissip_ext_	: space discretization (dissipation on boundaries)
spc_dissip_wall_ :	space discretization (dissipation on boundaries)
spc_expMartinelli_ :	the Martinelli exponent of the dissipation
spc_iCalcArtifDissip_	: strategy for dissipation calculation in Runge-Kutta
spc_iCalcLim_limiters calculation at each stage of the Runge-Kutta
spc_iCalcVFluxes_	: strategy for viscous flux calculation in Runge-Kutta
spc_RhoswitchInArtDissip_ : 	add density switch to compute artificial dissipation
spc_TswitchInArtDissip_ :	 type of computing of the second artificial dissipation
spc_XhilnArtDissip_ :	limiter with the second central scheme
ta_it_restart_ : the iteration at which the computation is restarted
ta_iVariableTimeStepping_ : activation of variable time step
table_cp_Limit_: the Cp limit when using thermodynamic tables
tm_drcoeff_ :	coefficients for the Runge-Kutta scheme
tm_iResSmoothing_	: implicit residual smoothing scheme
tm_fmg_iResSmoothing_	: implicit residual smoothing scheme during coarse grid initialization
tm_mgCycleType_ :	the type of multigrid cycle
tm_nbStage_ :	number of stages in the Runge-Kutta scheme
turb_iRoughModel_ :	select the rough wall model
turb_iYAP_ :	control the Yap correction in the k-ε (Extended Wall Function) and  k-ε (Low Re Yang-Shih, classic) model.
turb_KEpsProd_	: the production term in k-eps equations
turb_mavRem_ :	limiter for turbulent quantities time update
turb_mavRes_ :	limiter for turbulent quantities time update
turb_mutMuLimit_ :	limiter for Mut/Mu
turb_ProdWithDiamondGrad_ :	gradient computing for turbulent production term
TRefBCpAdapt_ :	the reference temperature
upw_dissipEnthalpy_ :	controls the use of the standard or isenthalpic dissipation
upw_dissip_ext_ :	controls dissipation calculation at inlet-outlet boundaries
upw_limit_ :	activate limiter for the second order upwind scheme
upw_limitVenka_ :	select limiter for the second order upwind scheme

Coupling with MpCCI
Introduction

For multi-physics problems, many commercial codes, such as FINE™/Open with OpenLabs™ and Abaqus etc., can be used to solve only one aspect of the physical problem. One way to perform the multi-physics simulations is to use two or more dedicated codes coupled through the exchange of data.
MpCCI (Mesh-based parallel Code Coupling Interface) is a coupling interface developed by the Fraunhofer Institute (SCAI) and used to perform multi-physics simulations. It consists in a server, which handles physical quantities exchanges between two or more heterogeneous solvers (for example a Computational Fluid Dynamics solver and a solid mechanics solver).
FINE™/Open with OpenLabs™ includes a MpCCI code adapter in order to solve the thermal and/or mechanical coupling problems. The adapter takes in charge all communication processes with the MpCCI coupling server. About the settings in MpCCI, please refer to the MpCCI manual. For the coupling quantities with MpCCI, FINE™/Open with OpenLabs™ can send the following quantities:

Global values:

Physical time;
Time step count;
Time step size;
Reference pressure.

Face node values:

Absolute pressure;
Overpressure
Density
Velocity;
Temperature.

Face element values:

Absolute pressure;
Overpressure
Density
Velocity;
Temperature;
Heat flux;
Relative wall force.

FINE™/Open with OpenLabs™ can receive:
Face node values:

Displacements;
Nodal position.
Temperature

Face element values:

Temperature;

The limitations coupling with MpCCI are as follows:
Only surfaces (3D) and lines (2D) coupling are supported by FINE™/Open with OpenLabs™. Volume coupling is not yet supported.

The coupling with MpCCI uses the mesh deformation module. For the limitations related to mesh deformation, see Mesh Deformation Methods section.

The Settings in the FINE™/Open GUI
The Coupling with MpCCI can be accessed in the Optional Models / Coupling page. 


Selecting Coupling with MpCCI in the option Coupling method, then the user will be able to set the parameters for the MpCCI code adapter. The user needs to specify the reference pressure for the exchange of coupling data, which is used to calculate quantities such as overpressure (absolute pressure - reference pressure).
In order to couple with MpCCI, the user needs to activate the option Coupling activation for the coupling solid boundaries. Three kinds of coupling simulations can be performed: 

Thermal coupling: the wall heat load (temperature or heat flux) is sent to structural code, the wall temperature is sent to the FINE™/Open solver;
Thermal coupling is only compatible with MpCCI v4.
Mechanical coupling: the fluid loads (pressure or forces) are sent to structural code, the solid deformation (position or displacement) is sent to the FINE™/Open solver;
Thermo-mechanical coupling: both the fluid loads (pressure or forces) and the wall heat load (temperature or heat flux) are sent to structural code, the solid deformation (position or displacement) and the wall temperature are sent to the FINE™/Open solver.
Thermo-mechanical coupling is only allowed for unsteady computations. 

The coupled boundaries can be moving or fixed:

Moving grid points: The points of the selected boundary are moving. In this case, a mesh deformation module, which is dedicated to the applications related to Fluid-Structure Interaction (FSI), is automatically activated. The mesh deformation method is selected through the expert parameter mov_iMovingGridMeth_, see Advanced Parameters for Coupling with MpCCI for more detail.
Fixed grid points: The points of the selected boundary are fixed.

Advanced Parameters for Coupling with MpCCI
The following non-interfaced advanced parameters related to Coupling with MpCCI are available:
iMpCCISteadyMode_:	 For the FSI simulations, the CFD solver computes a transient solution. However, a special steady coupling mode is implemented in the FINE™/Open solver. It does not use the steady solver but forces the unsteady solver to compute a steady solution. To force such a computation, one has to set the parameter iMpCCISteadyMode_ to 1 instead of 0.
mpcci_Relax_:	In order to avoid convergence problems for steady computations, the received temperature can be relaxed through the following formula:



where  and  are the previous temperature and the received temperature, respectively. The coefficient  is the relaxation parameter. By default, the relaxation parameter is equal to 1.
iMpCCIIterCoupling_: for steady computations, the data exchange is performed at the iteration number N if (N / iMpCCIIterCoupling_)=0
iMpCCIzSize_: 	This parameter is used to specify the size of the cell in the third direction (z) in 2D cases. By default, it is 1.0 [m].

Domain Scaling Method
The Domain Scaling Method is an unsteady simulation technique for rotor/stator interfaces. The effect of displacement due to rotation is taken into account. At each time step, the rotor is set at its correct position and equations are solved for that particular time step for the whole computation domain. The final solution is therefore a succession of instantaneous solutions for each increment of the rotor position.
Mesh Constraints

The blade passages of each blade row to include in the mesh should cover the same pitch distance (have the same periodicity). If the periodicity of the rotor and the stator is not the same this can be solved in three different ways: 

modeling a higher number of blade passages on each side to find a common periodicity,
scaling the geometry (with the scaling being as close to 1 as possible). The common way to scale the geometry is to modify the number of blades during the mesh generation process. The time frequencies are resolved with an error that is proportional to the scaling coefficient.

Apart from this constraint on the periodicity, there is no constraint on the patches and mesh nodes configurations.


FINE™ Settings


The Domain Scaling Method is an unsteady simulation technique. The Time Configuration in the General properties page should thus be set to Unsteady. 
For each rotating block, the rotation speed is defined under the Rotating Domains tab on the Rotating Machinery page.
Under the Rotor/Stator tab on the Rotating Machinery page, the user has to specify for each of the rotor/stator connections:

the rotor/stator connection treatment method: Domain scaling.
the flow direction.

The initialization process can be performed in two ways:

A steady state initialization is performed in a separate computation with Steady as Time Configuration. It is suggested to model all rotor/stator interfaces in this case using frozen rotor approach. The unsteady domain scaling computation is using the result of this steady computation as initial solution. See Initial Solution chapter for more information on how to start a computation from an initial solution file.
The steady initialization is automatically performed before starting the time accurate computation (that means within the same computation). To use steady initialization, specify in the interface an appropriate Number of steady iterations under the Steady Initialization parameters in the Control Variables page.

The Number Of Angular Positions is defined in the Control Variables page. When working with the Domain Scaling method, using a Number Of Angular Positions of 10 points per blade passage is giving a coarse but reasonable result. To have a more accurate (but more CPU consuming) result choose 20 to 30 points per blade passage.


The physical time step will be calculated based on the imposed Number Of Angular Positions and the information will be given below.
The Number Of Time Stepsis defined in the Control Variables page. In general, it is recommended to repeat the period at least 20 times. Usually after 20 periods, the flow becomes periodic.
For example, considering a 1-1/2 turbine with the blade number of 43, 64 and 16. The user can generate a scaled multi-row mesh including 8 stator passages, 12 rotor passages and 3 stator passages with a common periodicity of 5. In this case, the user needs at least 10 time steps for each rotor passage and that is really a coarse result. So the minimum Number of Angular Positions is 120. Usually, 20 periods are needed to reach periodic flow. The user will have to set the Number Of Time Steps to 2400.
For more info on the Steady initialization and Outputs Files available in the Control Variables page, see Control Variables section.



 Illustrative Example

The example case of the flow in Aachen turbine is considered as shown in FIGURE 23. With the domain scaling approach, one can observe a strong interaction between the wake and main flow, leading to a correct physical simulation of the unsteady phenomenon (at the expense of much higher CPU time compared to mixing plane approach).


FIGURE 23 Aachen turbine: Domain Scaling method


Non-interfaced Advanced Parameters



Additional parameters related to the Domain Scaling Method are available in the list located in the Advanced tab of the Control Variables page.
RS_OutputMultiple_:	 In case that Multiple files is selected for visualization and/or restart in the Computation Control / Control variables page under the General tab, the multiple files can be corresponding to the last period or the whole iteration procedure when Domain Scaling Method is used:

0: The FINE™/Open solver will only save the solution corresponding to the last Number of Angular Position physical time steps.
1: The FINE™/Open solver will save the solution from beginning.

Non-premixed Combustion

The modeling techniques applied for the Non-premixed combustion are based on the mixture fraction approach. Besides a basic combustion model for non-premixed combustion, which can account for heat loss due to radiation, a post-processing model for the formation of NOx is available in FINE™/Open with OpenLabs™. 
On the Optional Models / Combustion page, the combustion type Non premixed is available.


FIGURE 24 Non-premixed combustion parameters
Two chemistry models are proposed as a user choice:

Equilibrium: This model is based on the chemical equilibrium assumption, where it is assumed that the time scales related to combustion are infinitely much faster than those of the flow and mixing. With this approach it is assumed that the fuel/air mixture in each point is in chemical equilibrium and the flame is not influenced by strain. 
Flamelet: The flamelet model incorporates non-equilibrium effects. These non-equilibrium effects are mainly important when looking at the concentrations of minor species, especially when pollutant formation (NOx, CO etc.) is of interest. In this approach, a flame (laminar or turbulent) is viewed as an ensemble of flamelets (small flames) embedded in the flow field and that are subjected to strain from the flow. This makes the flamelet model more accurate, although it requires the generation and the use of a library of flamelets. 

A checkbox can be activated to select a specific strain rate. The default value is set to 100/s.
Turbulence-chemistry interaction can be modeled using the Presumed PDF approach. In the Presumed PDF approach, a probability density function (PDF) for the mixture fraction describes the probability that the flow field takes in a certain value for the mixture fraction at a given point. In FINE™/Open with OpenLabs™, it is presumed that the shape of the PDF can be represented by ß-functions, and the distribution is parameterized via its statistical moments. In practice, the calculation of the PDF involves integrals and is thus computationally expensive. A pre-integration of the PDF is done to reduce the overhead, and an additional dimension is stored in the combustion look up tables for the mixture fraction variance.
For the evaluation of NOx, a dedicated post-treatment restricted to the formation of thermal NO can be activated.
A combustion look up table must be specified for the determination of the thermochemical properties of the burnt and unburnt mixture of the fuel and oxidizer.  After specifying the table, the button Preview can be used to view the properties of the table. If needed, the user can click on the button Create/Edit to create a new look up table. For more information on how to create/edit a combustion look up table, see TabGen/Chemistry.
The combustion model is limited to two stream problems. If a combustion problem contains three (or more) streams, then the third stream (or any stream in addition to the first and the second) must represent a linear combination of the two first ones. 
The present approach assumes that the chemistry is much faster than the mixing process. For slow reactions this assumption may not be valid which results in poor accuracy of the predictions. 
The Create/Edit... button is only available on Linux.
The other combustion model parameters in the FINE™/Open GUI can be found in the following menus:
Fluid model



When the combustion model is activated, the fluid is automatically changed to "Reactive fluid". The Fluid Model menu gives restricted access to fluid properties. Both density and temperature field are determined through the interrogation of look-up combustion tables, as function of the mixture fraction and its variance.
However, reference values, heat conduction and diffusivity related parameters can still be edited.


Flow model



When the combustion model is activated, the turbulence model is by default set to the standard k-ε model. The other 2-equation turbulence models available for inert flow can also be selected for combustion simulations. However, the one equation turbulence models cannot be used in conjunction with combustion modeling. 
Laminar regime can be also modeled.


Boundary conditions



Combustion-dedicated boundary conditions have been introduced at inlets, with entries for the mixture fraction and NO mass fraction.

Mixture fraction should range between 0 (oxidizer stream) to 1 (fuel stream).
NO mass fraction relates to the fraction of NO injected through the inlet patch. The recommended value is set to 0.

No dedicated condition is required for the treatment of outlets, since combustion variables are purely convected quantities.


Initial Solution



Minor modifications have been brought to the Initial Solution menu, with the introduction of initial data for the mixture fraction. As a default, pure oxidizer conditions (Mixture fraction f = 0) are recommended in most cases. 


Numerical parameters

When performing non-premixed combustion computations, the following choices are the best recommendation:

In the General Parameters page under the tab General,

set the Number of grid(s) to 3 or 4 (preferred),
activate Coarse grid initialization.

In the General Parameters page under the tab Advanced,

 Increase the Maximum number of cycles per grid level to 400 - 600,
Reduce Convergence criteria on each grid level to -6,
Possibly increase Number of sweeps on successive grid levels to 1 2 16 (3 grid levels), or 1 2 3 32 (4 grid levels)

In the Numerical Schemes page,

The recommended CFL number is 1.5. This is also set as default.


The non-premixed combustion module can be used together with CPU Booster. In order to get the best performance, the following settings are recommended when combining CPU Booster and combustion:

In the Flow Model page,

Set the Turbulence model to  k-epsilon (Extended Wall Function) or k-epsilon (Low Re Yang-Shih, classic),

In the General Parameters page under the tab General,

set the Number of grid(s) to 3 or 4 (preferred),
activate Coarse grid initialization.

In the General Parameters page under the tab Advanced,

 Increase the Maximum number of cycles per grid level to 400 - 600,
Reduce Convergence criteria on each grid level to -6,
Deactivate the CPU Booster during coarse grid initialization,

In the Numerical Schemes page,

The recommended CFL number is 100. This is also set as default.  In case of convergence problem, reduce the CFL number.
Keep the Merkle preconditioning selected.

In the Control Variables page under the tab Advanced,

Increase the density relaxation coefficient to 0.1 (the fifth dimension of the local expert parameter RelaxCombVars_). In case of convergence difficulty, set the density relaxation coefficient to 0.01 (default value).
In case that heat flux solid boundary condition is defined, set the local expert parameter IterScalingFuncHeatFlux_ to 10.
In case that the S2S radiation model is activated, set the local expert parameter RadFVM_IterationNumber to 2.




Outputs

When performing non-premixed combustion computations, the following quantities are available for output in the page Computation Control / Outputs / General under the category Combustion.

Comb_MixtFrac: mixture fraction 
Comb_VarianceMixtFrac: mixture fraction variance 
Comb_EnthDefect: Enthalpy defect
Comb_TempDefect: Temperature defect
Comb_TemperatureClipping: Flag to plot whether temperature was clipped or not. 0: Not. 1: Yes.
Comb_SDissipRate: scalar dissipation rate 

When NOx post-processing is activated, the following variables can be selected for output:

Comb_NOxPost: mass fraction () of NO
Comb_SourceTermNO: source term of the mass fraction () equation

Depending on the lookup table specified for the non-premixed  computation, the following quantities may be available:

LookUpTable_RHO: density of the mixture [kg/m³]
LookUpTable_TEMP: absolute temperature of the mixture [K]
LookUpTable_DYNVISC: dynamic viscosity of the mixture [Pa.s]
LookUpTable_ENTHALPY: specific chemical enthalpy of the mixture [J/Kg]
LookUpTable_CP: isobaric heat capacity of the mixture [J/K/Kg]
LookUpTable_SCNO: first source term of the NO equation
LookUpTable_SPNO: second source term of the NO equation
LookUpTable_MMW: molar weight of the mixture [kg/ kmol]
LookUpTable_QOTM: source term for OTM model, only if applicable
LookUpTable_Temp4: absolute temperature in fourth power
LookUpTable_LAM: laminar heat conductivity coefficient ()
LookUpTable_##: mass fraction of the species ##



Expert parameters

All non-interfaced advanced parameters related to the non-premixed combustion model are accessible on the Control Variables page under the tab Advanced. 
combSDissConst_:	Specify the constant  for the mean scalar dissipation rate. The default value is 2.0.
combSchmidtTurb_:	The turbulent Schmidt number (default value 0.7). 
RelaxCombVars_:	The relaxation coefficient in combustion module. This parameter is an array of seven dimensions, corresponding to the relaxation coefficients for the mixture fraction f, the mixture fraction variance g, the enthalpy defect, the NO variable, the density update, the molecular viscosity and progress variable update respectively (Default value: 1 1 1 1 0.01 1 1). Note: The progress variable relaxation factor is used by the premixed model.
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied to scale the heat fluxes boundary condition(s). During the course grid initialization the heat flux(es) is/are set to zero. The idea of this switch is to ensure that the flow field and/or the combustion process is developed before extracting/adding heat.
combTimeStep_: By default (value=0), the time step solving all the combustion equations is determined by using the acoustic propagation speed (u+c). When setting the expert parameter combTimeStep_ to 1, the time step is determined by using the advective propagation speed (u).

Cavitation with thermodynamic tables
Overview
The derivative of the saturation pressure with the temperature indicates the thermo-sensitivity of the fluid. For example, for water this parameter is around 130Pa/K. Therefore water can be considered as non thermo-sensitive. However, for LH2 (~50000Pa/K) this parameter is quite large and therefore it should be considered as thermo-sensitive. It should also be noted that this parameter can strongly depend on the temperature at which it is evaluated. 
Thermodynamic tables provide a precise description (in equilibrium) of the density in function of pressure and enthalpy. The description of the states provided by the thermodynamic tables will be used both for the pure phases (liquid or gas) and for the biphasic states. Thermo-sensitive effects will automatically be taken into account when thermo-sensitive fluid is used. 
For the cavitating simulation with thermodynamic tables and Hakimi preconditioning, the following tables are essential:

RHP.atab - density in function of enthalpy and pressure
THP.atab - temperature in function of enthalpy and pressure

Moreover, tables for the transport properties are strongly recommended:

MHP.atab - dynamic viscosity in function of enthalpy and pressure
KHP.atab - thermal conductivity in function of enthalpy and pressure

For the cavitation modeling, a table for the quality χ is used to detect the state (liquid, gas or mixture).

AHP.atab - quality in function of enthalpy and pressure. The quality χ can take the following values: 0 for liquid phase, 1 for gas phase and from 0 to 1 for biphasic/mixture. 

When using thermodynamic tables to model cavitating flows, the thermodynamic tables should cover all the thermodynamic states that are present in the converged solution.
The limitations for the cavitation model with thermodynamic tables are:

The cavitation model with thermodynamic tables is ONLY compatible with Hakimi preconditioning.


Settings and Guidelines in FINE™/Open with OpenLabs™
There is no access of the Cavitation Model with thermodynamic tables through the graphical user interface. The user has to activate this model by setting the expert parameter iCavitation_ to 2. 
The other Expert Parameters setting the cavitation model with thermodynamic tables are:
cavPreFactorRhoDissip_: 	Controls the first order density differences term added to the artificial dissipation of the continuity equation in case of cavitation modeling (default value 1.0)
spc_RhoswitchInArtDissip_: 	By default this parameter is set to 0, meaning that the only sensor used to activate second-difference dissipation in regions of strong gradients is a pressure switch. When the cavitation model is used, this parameter should be set to 1 in order to activate a density switch in addition to the pressure switch.
tm_iResSmoothing_	: By default this parameter is set to 2, meaning that the residual smoothing is only applied to the first 5 equations (continuity, momentum and energy). When the cavitation model is used, this parameter should be set to 0.
turb_mutMuLimit_:	 By default this parameter is set to 50000, meaning that the ratio between the turbulent viscosity and the molecular viscosity is limited to 50000. In order to avoid an unphysical behavior of the turbulence model, it is recommended to set this parameter to a higher number, for example 200000.
iCondTableClip_:	By default this parameter is set to 0, meaning that the access to the thermodynamic tables is not clipped. With the cavitation model with thermodynamic tables is activated, it is recommended to set this parameter to 1 in order to activate the clipping when the tables are looked-up.
The other parameters of the cavitation model with thermodynamic tables in the FINE™/Open GUI are:
Fluid model



Thermodynamic tables MUST be used in the Physical Configuration / Fluid Model page in order to use the cavitation model with thermodynamic tables.


Boundary conditions



It has been observed that the following combination of boundary conditions is more robust when a cavitation model is activated:

Static quantities or mass flow imposed at the inlets (velocity, temperature and turbulence variables) 
Static pressure is imposed at the outlet. Imposing the static pressure at the outlet actually means imposing the cavitation number at the outlet (). However, for most of the test cases, the known parameter of the operating conditions is the cavitation number at the inlet (). Then, the idea is to modify the static pressure at the outlet until we obtain the desired cavitation number at the inlet. 



Initial Solution



When the cavitation model with thermodynamic tables is activated, the cavitating flow field can be initialized by Constant values or From file.
When the cavitating flow field is initialized by Constant values, it is recommended to use an initial pressure value significantly larger than the saturation pressure. This enforces the computation to start with a pure liquid flow solution.
In some cases, the cavitation simulation initialized by Constant values may have convergence problem. In this case, it is recommended to start the cavitating flow simulation from a converged solution without cavitation for which the fluid state is pure liquid in the entire computational domain. In order to apply this strategy, a pure liquid solution has to be obtained first for a higher pressure in the domain than the one to be used for the cavitating simulation (avoid zones with pressures below the saturation one). Usually, this can be simply obtained by increasing the pressure at the outlet boundary. Afterwards, the cavitating computation can be started using this pure liquid computation as initial solution. 
In order to accelerate the convergence, the pressure field in the whole domain of this starting solution can be reduced by the difference of the pressure level between the pure liquid computation and the cavitating one. Two expert parameters can be used to control this restarting strategy:
iRestartCav_PressDiff_:	 This expert parameter is by default 0. In case the user sets it to 1, the initial pressure field will be reduced by the expert parameter DeltaPress_RestartCav_.
DeltaPress_RestartCav_:	 value used to reduce the initial pressure field when the parameter iRestartCav_PressDiff_ is activated.


Numerical parameters



When the cavitation model with thermodynamic tables is activated, the CFL number MUST be set to 1.0. In case of convergence problems, it can be even reduced to 0.5 or 0.2.
The Multigrid method is compatible with the cavitation model. Four multigrid levels can in general be used. However, in case of convergence difficulties, the user might consider reducing the number of grid levels to 3 or even 2.

Customized convection speeds
The user can customize convection speeds for external PDEs. The section defining the convection speeds must start with the line "=>CUSTOM_CONVECTION_SPEEDS".
To define convection speeds for external PDEs, each convection speed has to be written by giving a name to the expression. The name should be given after "@CUSTOMCONVSPEED:".
=>CUSTOM_CONVECTION_SPEEDS:

@ CUSTOMCONVSPEED: <expression name of the convection speed>
->EXPRESSION: <mathematical expression of the convection speed>
Note, the mathematical expression of the convection speed must be a vector expression, for example, Density*[Vx,Vy,Vz] or Density*Velocity, where Velocity is a vector.
If the user defines a customized convection speed, the defined customized convection speed must be used at least in one of the external PDEs.

Algebraic Expressions and PDEs
The user can add or modify algebraic formulas or add external transient-convection-diffusion-source equations. The section must start with the line "=> EQUATIONS".
Algebraic Expressions

A variable defined by an algebraic formula can be added or modified (e.g. turbulent viscosity in k-epsilon turbulence models). The section to add algebraic expressions should be added in the section of "=>EQUATIONS" and must start with "@ NONDIFFEXPR:". Then, each algebraic expression must be written by adding a given name to the formula. Finally, the variable name and the expression are written and separated by "=". See the structure below.
=>EQUATIONS
@ NONDIFFEXPR: <Name of the formula 1>
->EXPRESSION:  <Name of the variable 1>= <mathematical expression/formula >
->BOUNDARY_FACE: Extrapolation   (Optional)
->AddToBoundaryOnly: <Patch num/name>, …   (Optional)
->ExportBoundaryProfileToFile: (Abscissas split by ","), <File name>, Patch num  (Optional)
@ NONDIFFEXPR: <Name of the formula 2>
->EXPRESSION:  <Name of the variable 2>= <mathematical expression/formula >
->BOUNDARY_FACE: Extrapolation   (Optional)
->AddToBoundaryOnly: <Patch num/name>, …   (Optional)
->ExportBoundaryProfileToFile: (Abscissas split by ","), <File name>, Patch num   (Optional)
The boundary values of algebraic expressions can be computed in three ways:

compute expression at boundary.
use the extrapolated value from the first inner cell. In order to add this option, the following line must be added "->BOUNDARY_FACE: Extrapolation".
set the expression to 0 on the NS wall. In order to add this option, the following line must be added "->BOUNDARY_FACE: Extrapolation_With_ZERO_On_NSWall".

The attribute line of algebraic expressions with the keyword "->AddToBoundaryOnly:" is optional. When this attribute line exists, the algebraic expression will be computed only along the specified boundaries. To specify the boundaries, the keywords ALLSOLIDS, ALLINLETS and ALLOUTLETS can be used.
The attribute line of algebraic expressions with the keyword "->ExportBoundaryProfileToFile:" is optional. When this attribute line exists, the value of the algebraic expression on the specified boundary will be exported to a file. Where, the Abscissas (split by ",") is used to specify the abscissas. If the user does not specify the absolute path for the file, OpenLabs™ will save the file in the computation folder. For example, the following line exports the value of the algebraic expression with respect to xCoord on the patch 4 to a file /tmp/export.dat. 
->ExportBoundaryProfileToFile: (xCoord), </tmp/export.dat>, 4
The attribute ExportBoundaryProfileToFile is not available in case of parallel computations. 
It is important to note that the name of the formula must be spelled correctly. Otherwise, OpenLabs™ will create a new algebraic expression instead of modifying the internal one.
It is not allowed to modify the value of an internal PDE variable by algebraic expression. 


Convection-diffusion-source transport equations: PDE

The transport equation must have the form of a transient-convection-diffusion-source equation:



where ϕ is the variable to be solved,  is the diffusion coefficient and  is the source term.
The section to add a transport equation (PDE) should be added in the section of "=>EQUATIONS" and must start with "@ PDE:". Each PDE has to be added by giving a name to the equation, and writing the expression of the equation with the following keywords: 

DDT(<VarName>)
CONV(<Name of the convection speed, optional>, <VarName>)
DIFF(<name of the diffusion coefficient >)
SOURCE(<Name of the source term1> + <Name of the source term2> + …)


The keyword CONV() may have two arguments: the name of the convection speed and the name of the variable. The first argument, the name of the convection speed, is optional. If the first argument is not defined, OpenLabs will by default use the expression or , depending on the conservative or non-conservative convection scheme. If the first argument is specified, OpenLabs will use the user customized convection speed, see Customized convection speed for more details.
The transport equation definition in the resource is as follows:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION:DDT(<VarName>)+CONV(<VarName>)= \
DIFF(<name of the diffusion coefficient >)+ \
SOURCE(<Name of the source term1>+…)
In order to solve the transport equation, a number of properties/attributes need to be defined (e.g. convective scheme, initial and boundary conditions, relaxation…). In the following table, a list of possible properties/attributes is shown. If the attribute is not added, the default value is automatically set.






Property


Keyword






Convective scheme:
- Non-conservative form of first order upwind
- Conservative form of first order upwind
- Conservative form of high order upwind


 
->Convective_Scheme: UpwindFirstOrderNonConservative
->Convective_Scheme:UpwindFirstOrderConservative (default)
->Convective_Scheme: UpwindHighOrderConservative




Initial value:
- Constant value for the whole field
- Expression to initialize the field


 
->INITIAL_VALUE: <value>   (default: 0.0)
->InitializeTo: <name of initialization expression>	  




Upper and lower clipping of the field:
- Clip the field to a minimum value
- Clip the field to a maximum value


 
->LowerLimit: <value>   (default: -1e30)
->UpperLimit: <value>   (default:  1e30)




Relaxation type:
- No relaxation
- Constant relaxation factor
- Limit the variation of the variable
- Limit upper and/or lower variation of the variable (same as previous case but being able to limit different upper and lower variations):

Limit the upper variation 
Limit the lower variation



 
Nothing should be added
->ConstantRelaxFactor: <value>    (default:1.0)
->LimitVariation: <value>    (default:0.95, corresponds to 5%)
 
->UpperRelaxationFactor: <value> (1.05, corresponds to 5%)
->LowerRelaxationFactor: <value> (0.95, corresponds to 5%)




Boundary conditions at solids:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …
       or
->UseCustomBC: <name of bc expression>, ALLSOLIDS
      or
->UseCustomWallFunction: <name of wall function>, <Patch num/name>, …




Boundary conditions at inlets:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …
       or
->UseCustomBC: <name of bc expression>, ALLINLETS




Boundary conditions at outlets:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …
       or
->UseCustomBC: <name of bc expression>, ALLOUTLETS




Boundary conditions at externals:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …




In case that the equation added is for the turbulent kinetic energy, the term    needs to be added


->AddTwoThirdsRhoK   (this should not be used unless a 
                                          turbulent kinetic energy equation is 
                                          being added)




The following is the complete structure of a transport equation definition with its attributes:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION: DDT(<VarName>)+CONV(<VarName>)= \
                              DIFF(<name of the diffusion coefficient >)+ \
                              SOURCE(<Name of the source term1>+…)
->Convective_Scheme: <Convection scheme keyword>
->InitializeTo: <Name of expression to initialize the field>
   or
->INITIAL_VALUE: <value>
->LimitVariation: <value between 0 and 1>   (Optional)
   or
->ConstantRelaxFactor: < value between 0 and 1>    (Optional) 
   or
->UpperRelaxationFactor: < value larger than 1>          (Optional)
->LowerRelaxationFactor: < value between 0 and 1>    (Optional)
->LowerLimit: <value>   (Optional)
->UpperLimit: <value>   (Optional)
->UseCustomBC: <name of solid BC expression>, <Patch num>,<Patch num>,…
->UseCustomWallFunction: <name of wall function>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of inlet BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of outlet BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of external BC expression>, <Patch num>,<Patch num>,…
->AddTwoThirdsRhoK    (Optional only in case that a turbulent kinetic energy equation is being added)
Conservative vs. non-conservative convection schemes


A transient-convection-diffusion-source transport equation can be written, in a conservative form. For this kind of equations, two numerical convection schemes can be chosen in OpenLabs:

Conservative first order upwind: UpwindFirstOrderConservative
Conservative high order upwind: UpwindHighOrderConservative

The conservative form of the transport equation is highly recommended, especially when large density gradients are expected.
The UpwindHighOrderConservative is significantly more computationally costly.
In some particular cases, when the transport equations are source term dominated and very stiff (e.g. k and epsilon equations), the non-conservative form can be used to gain in robustness. The equation in the non-conservative form can be written as follows:



In this case, one numerical convection scheme can be chosen in OpenLabs:

Non-conservative first order upwind: UpwindFirstOrderNonConservative

Warning: In case the non-conservative scheme is selected, the source terms and diffusion coefficients formulas must be written accordingly (division by density).


Boundary conditions

To specify the boundaries where a certain boundary condition is applied, two options are possible:

In case all SOLIDS, INLETS or OUTLETS have the same boundary condition (e.g. the epsilon at the wall), the keywords ALLSOLIDS, ALLINLETS or ALLOUTLETS can be used.
In case that each SOLID (INLET, OUTLET or EXTERNAL) has a different boundary condition (e.g. a case with different variable value at different inlet), the corresponding <patch number> or <group name> is required, which can be obtained in the project analysis results. An example is shown below, where BC_periodic and BC_inlet are the group names that defined in the GUI by the user. The numbers in the square brackets are the patch numbers that belong to the group. The physical variables that are imposed to the boundaries in the GUI are listed after "->Imposed_Physical_Variables:".

# This is ana file
…
=>INTERNAL_BOUNDARY_CONDITIONS
@ InternalBC_PERIODIC: BC_periodic[0,1] 
@ InternalBC_INL: BC_inlet [2] 
->Imposed_Physical_Variables: "Vr", "Vt", "Vz", "NormalizedProgressVariable" 
@ InternalBC_OUT: BC_outlet [3] 
->Imposed_Physical_Variables: "StaticPressure"
A group name should never be defined as a number in the GUI, e.g. a group of boundaries cannot be named as "0". Otherwise it will be mistaken as the patch number.
For the boundaries where no customized boundary conditions are applied, the Neumann (null gradient of the variable) boundary condition will be automatically imposed.




 Diffusion transport equation: PDE


The parabolic PDEs, such as diffusion equations,  have the following form.



For parabolic PDEs, the explicit schemes are generally unsuitable because their region of absolute stability is small. Implicit scheme with a generalized Gauss-Seidel method is available for solving diffusion equation. It is set as the default method for the transient-diffusion-source PDEs added in OpenLabs™. The transient-diffusion-source PDE of scalar ϕ is formulated as,



where, R is a function of ϕ and its spatial derivatives. The Crank-Nicolson scheme can be obtained by applying trapezoidal rule to the time integration,



A general implicit scheme can be achieved  by introducing a blending factor γ,



Finally, the solution is updated by,



The general implicit scheme is a combination of the explicit forward Euler scheme (corresponding to γ=0) and the implicit backward Euler scheme (corresponding to γ=1). And only when γ=0.5 (Crank-Nicolson scheme), it is second-order in time accurate. The value of γ is set using the keyword -> IMPLICIT_BLENDING. The over-relaxation factor  is set using the keyword ->IMPLICIT_SOR. The default value for the over-relaxation factor is 1 but a range of values between 0 and 2 can be used for this parameter. A higher relaxation factor (>1) will accelerate the convergence of a slow-converging process,  it helps to reach a super-linear convergence for some problems but may fail for the others (divergence).
Alternatively, the explicit Runge-Kutta method is still available by using the keyword ->ForceExplicitRungeKutta.
The transport equation definition in the resource file is as follows:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION: DDT(<VarName>)=                               DIFF(<name of the diffusion coefficient >)+                               SOURCE(<Name of the source term1>+…)
->InitializeTo: <Name of expression to initialize the field>
 ->IMPLICIT_SOR: <value> 
->IMPLICIT_BLENDING: <value> 
->UseCustomBC: <name of solid BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of inlet BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of outlet BC expression>, <Patch num>,<Patch num>,…
It is not obliged to have DDT term for diffusion PDEs in case of the absence, the attribute "-> VARIABLE_NAME:" has to added with given name. In the absence of transient term in the scalar PDE following structure can be used:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION: 0= DIFF(<name of the diffusion coefficient >)+                               SOURCE(<Name of the source term1>+…)
            ->VARIABLE_NAME: GP1
The properties/attributes need to be defined for diffusion PDEs are listed below.






Property


Keyword






Initial value:
- Constant value for the whole field (Default)
- Expression to initialize the field


 
->INITIAL_VALUE: <value>   (default value: 0.0)
->InitializeTo: <name of initialization expression>	  




Upper and lower clipping of the field:
- Clip the field to a minimum value
- Clip the field to a maximum value


 
->LowerLimit: <value>   (default: -1e30)
->UpperLimit: <value>   (default:  1e30)




Relaxation type when using the explicit Runge-Kutta method:
- No relaxation (Default)
- Constant relaxation factor
- Limit the variation of the variable
- Limit upper and/or lower variation of the variable (same as previous case but being able to limit different upper and lower variations):

Limit the upper variation 
Limit the lower variation



 
Nothing should be added
->ConstantRelaxFactor: <value>    (e.g. 0.5)
->LimitVariation: <value>    (e.g. 0.95, corresponds to 5%)
 
->UpperRelaxationFactor: <value> (e.g. 1.05, corresponds to 5%)
->LowerRelaxationFactor: <value> (e.g. 0.95, corresponds to 5%)




Relaxation type when using the implicit method:
- blending factor γ in the implicit scheme
- the over-relaxation factor used to update the solution


 
-> IMPLICIT_BLENDING (Default: 0.5)
->->IMPLICIT_SOR    (Default: 1)




Boundary conditions at solids:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …
       or
->UseCustomBC: <name of bc expression>, ALLSOLIDS
      or
->UseCustomWallFunction: <name of wall function>, <Patch num/name>, …




Boundary conditions at inlets:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …
       or
->UseCustomBC: <name of bc expression>, ALLINLETS




Boundary conditions at outlets:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …
       or
->UseCustomBC: <name of bc expression>, ALLOUTLETS




Boundary conditions at externals:


->UseCustomBC: <name of bc expression>, <Patch num/name>, …

Outputs by OpenLabs
If new transport properties(Customized transport properties), new algebraic expressions (Algebraic Expressions) or new PDEs (Convection-diffusion-source transport equations: PDE) have been defined in OpenLabs, the new variables will be available for output in the Computation Control / Outputs page under the tab General after building the library. By default, all new variables are selected for output.

Advanced Parameters for Turbulence modeling
Non-interfaced Expert Parameters
All non-interfaced advanced parameters related to the turbulence models are accessible on the Control Variables page, in the Advanced sub-menu. 


All turbulence models

turb_mavRes_:	denoted here ζ, allows the user to control the update of k and ε (k-ε and k-ω models) or of  (Spalart-Allmaras and SARC models) for each Runge-Kutta stage. The default value is set to 0.95. Denoting the new value of k, ϵ or  as , the following restrictions are imposed:
If turb_mavRes_ > 0:






where EPS is equal to 1E-20. EPS is used to avoid possible divisions by zero.
If turb_mavRes_= 0: only the restriction defined  is applied.
turb_mavRem_:	denoted below as ζ, allows the user to control the multigrid corrections for k and ε (k-ε and k-ω models) or of  (Spalart-Allmaras and SARC models). The default value is 0.95.
If turb_mavRem_> 0: 



If turb_mavRem_= 0: restriction to positive values,
If turb_mavRem_< 0: 



turb_mutMuLimit_:	 controls the maximum allowable value for the ratio  in the flow field but not on boundary conditions (default value = 50000).
turb_ProdWithDiamondGrad_:	 controls methodology used to compute the gradients when evaluating the turbulent production term.
0 (default): based on Least Square gradients,
1: based on Diamond gradients.


k-ε models

phys_PrandtlTurb_:	 the turbulent Prandtl number (default = 1.0)
ke_Ceps1_:	Ceps1 constant in the k-ε equations (default = 1.44)
ke_Ceps2_:	Ceps2 constant in the k-ε equations (default = 1.92)
turb_KEpsProd_:	control the production term in the k-ε model.
0 (default): linearized production term;
1: the non-linear production term.
turb_iYAP_:	control the Yap correction in the k-ε (Extended Wall Function) and  k-ε (Low Re Yang-Shih, classic) model.
0: deactivate the Yap correction;
1 (default): activate the Yap correction.


Wall distance

dtw_method_: Controls which algorithm is used for calculation of the distance to the wall.
1 (default): calculates the distance to the wall as the point to the nearest boundary cell center. 


2: calculates the distance to the wall using an orthogonal projection of the point on the solid surface


When changing the method calculating the distance to wall, the .dtw file of the mesh must be removed manually if it exists.

Partially-premixed Combustion
FINE™/Open with OpenLabs™ provides two methods to simulate partially-premixed combustion: Manifold technique (FGM) and Hybrid BML/Flamelet. The difference between the FGM technique and the hybrid BML/Flamelet model is in the source term closure. In the Hybrid BML/Flamelet model, the source term in the transport equation for the progress variable and variance of the progress variable are closed using a BML type model. 
The partially-premixed combustion model can be selected in the Optional Models / Combustion page. The following part explains how to set  up a partially-premixed combustion computation using the Manifold technique (FGM) or the Hybrid BML/Flamelet method.

Flamelet Generated Manifold Model


FIGURE 28 FGM Partially-premixed combustion parameters
Turbulence-chemistry interaction is modeled using the Presumed ß-PDF approach. In the Presumed PDF approach, a probability density function (PDF) for the mixture fraction and the progress variable describes the probability that the flow field takes in a certain value for the mixture fraction and the progress variable at a given point. In practice, the calculation of the PDF involves integrals and is thus computationally expensive. A pre-integration of the PDF is done to reduce the overhead, and an additional dimension is stored in the combustion look up tables for the mixture fraction.
For the evaluation of NOx, a dedicated post-treatment restricted to the formation of thermal NO can be activated.
The NOx information is contained in the combustion look-up table. Please make sure your table including the NOx information.
A combustion look up table must be specified for the determination of the thermochemical properties of the burnt and unburnt mixture of the fuel and oxidizer.  After specifying the table, the button Preview can be used to view the properties of the table. If needed, the user can click on the button Create/Edit to create a new look up table. For more information on how to create/edit a combustion look up table, see TabGen/Chemistry.
The Create/Edit... button is only available on Linux.

Hybrid BML/Flamelet Model 


FIGURE 29 Hybrid/BML Flamelet Partially-premixed combustion parameters 
When the Hybrid/BML Flamelet model is selected, additional parameters are needed for the closure of the source terms of the progress variable and variance of the progress variable. 
The available BML models are the Zimont model and the Dinkelacker model.
In Flamelet definition, the user has to choose one fuel-air mixture used in chemistry model for combustion.
The Laminar flame speed correlation can be defined by Constant, Metghalchi-keck, Gulder or Parabolic. The default option Gulder is recommended. The laminar flame speed at stoichiometric fuel-air ratio can be obtained from the chemistry table or from literature. Flammability limits can also be obtained from literature or experimental data
The other parameters of partially premixed combustion model in the FINE™/Open GUI are:
Fluid model



When the combustion model is activated, the fluid is automatically changed to Reactive fluid. The Fluid Model page gives restricted access to fluid properties. Both density and temperature field are determined through an interrogation of look-up combustion tables, as function of the mixture fraction and its variance.
However, reference values, heat conduction and diffusivity related parameters can still be edited.


Flow model



When the combustion model is activated, the turbulence model is by default set to the standard k-ε model. The other 2-equation turbulence models available can also be selected for combustion simulations. However, one equation turbulence models, such as the Spalart-Allmaras model that are available for inert flow cannot be used in conjunction with combustion modeling. 
Laminar regime can also be modeled.


Boundary conditions



Combustion-dedicated boundary conditions have been introduced at inlets, with entries for the mixture fraction and progress variable.

Mixture fraction should range between 0 (oxidizer stream) to 1 (fuel stream).
 progress variable, the default value is set to 0.

No dedicated condition is required for the treatment of outlets, since combustion variables are purely convected quantities.


Initial Solution



Initial data for the mixture fraction and progress variable has been introduced to the Initial Solution menu. As a default, a value 0 is recommended for the mixture fraction and progress variable. 


FIGURE 30 Initial solution for partially-premixed combustion simulations
If the user activates the option Initialization with fully burned state, the combustion is looked up for a value of the progress variable that corresponds to a fully burned state in the first N iteration. If On finest grid is activated, the progress variable is initialized with fully burned state after Number of iteration specified on the fine grid level.


Numerical parameters

When performing partially-premixed combustion computations, the following choices are the best recommendation:

In the General Parameters page under the tab General,

set the Number of grid(s) to 3 or 4 (preferred),
activate Coarse grid initialization.

In the General Parameters page under the tab Advanced,

 Increase the Maximum number of cycles per grid level to 400 - 600,
Reduce Convergence criteria on each grid level to -6,
Possibly increase Number of sweeps on successive grid levels to 1 2 16 (3 grid levels), or 1 2 3 32 (4 grid levels)

In the Numerical Schemes page,

The recommended CFL number is 1.5. This is also set as default.


The partially-premixed combustion module can be used together with CPU Booster. In order to get the best performance, the following settings are recommended when combining CPU Booster and partially-premixed combustion:

In the Flow Model page,

Set the Turbulence model to  k-epsilon (Extended Wall Function) or k-epsilon (Low Re Yang-Shih, classic),

In the Initial Solution page,

Keep Initialization with fully burned state activated,
Reduce the Number of iterations to 10.

In the General Parameters page under the tab General,

set the Number of grid(s) to 3 or 4 (preferred),
activate Coarse grid initialization.

In the General Parameters page under the tab Advanced,

 Increase the Maximum number of cycles per grid level to 400 - 600,
Reduce Convergence criteria on each grid level to -6,
Deactivate the CPU Booster during coarse grid initialization

In the Numerical Schemes page,

The recommended CFL number is 100. This is also set as default. In case of convergence problem, reduce the CFL number.
Keep the Merkle preconditioning selected.

In the Control Variables page under the tab Advanced,

Increase the density relaxation coefficient to 0.1 (the fifth dimension of the local expert parameter RelaxCombVars_). In case of convergence difficulty, set the density relaxation coefficient to 0.01 (default value).
The relaxation coefficient of the progress variable (the local expert parameter RelaxCombProgVars_) should be kept as 0.1. In case of convergence difficulty, set this relaxation coefficient to 0.01.
						
In case that heat flux solid boundary condition is defined, set the local expert parameter IterScalingFuncHeatFlux_ to 10.
In case that the S2S radiation model is activated, set the local expert parameter RadFVM_IterationNumber to 2.




Outputs

When performing partially-premixed combustion computations, the following quantities are available for output in the page Computation Control / Outputs / General under the category Combustion.

Comb_MixtFrac: mixture fraction 
Comb_VarianceMixtFrac: mixture fraction variance 
Comb_EnthDefect: Enthalpy defect
Comb_TempDefect: Temperature defect
Comb_TemperatureClipping: Flag to plot whether temperature was clipped or not. 0: Not. 1: Yes.
Comb_SDissipRate:  scalar dissipation rate 
Comb_ProgressVariable1: progress variable 
Comb_SourceProgressVariable1: source term of the progress variable equation

When NOx post-processing is activated, the following variables can be selected for output:

Comb_NOxPost: mass fraction () of NO
Comb_SourceTermNO: source term of the mass fraction () equation

Depending on the lookup table specified for the non-premixed  computation, the following quantities may be available:

LookUpTable_RHO: density of the mixture [kg/m³]
LookUpTable_TEMP: absolute temperature of the mixture [K]
LookUpTable_DYNVISC: dynamic viscosity of the mixture [Pa.s]
LookUpTable_ENTHALPY: specific chemical enthalpy of the mixture [J/Kg]
LookUpTable_CP: isobaric heat capacity of the mixture [J/K/Kg]
LookUpTable_SCNO: first source term of the NO equation
LookUpTable_SPNO: second source term of the NO equation
LookUpTable_MMW: molar weight of the mixture [kg/ kmol]
LookUpTable_QOTM: source term for OTM model, only if applicable
LookUpTable_Temp4: absolute temperature in fourth power
LookUpTable_LAM: laminar heat conductivity coefficient ()
LookUpTable_##: mass fraction of the species ##



Expert parameters

All non-interfaced advanced parameters related to the non-premixed combustion model are accessible on the Control Variables page under the tab Advanced. 
combSDissConst_:	Specify the constant  for the mean scalar dissipation rate. The default value is 2.0.
combSchmidtTurb_:	The turbulent Schmidt number (default value 0.7). 
RelaxCombVars_:	The relaxation coefficient in combustion module. This parameter is an array of seven dimensions, corresponding to the relaxation coefficients for the mixture fraction f, the mixture fraction variance g, the enthalpy defect, the NO variable, the density update, the molecular viscosity and progress variable update respectively (Default value: 1 1 1 1 0.01 1 1). Note: The progress variable relaxation factor is used by the premixed model.
RelaxCombProgVars_:	The relaxation coefficient of the progressive variable in the partially-premixed combustion module, the default value is 0.1. 
combInitHybrid_:	It is used when the fully burned state is active for the Hybrid-BML partially premixed model (Default value 1). By setting this expert parameter to 1, in the fully burned state the flammability limits are extended and  is set to .
combReInitProgVar_:	Only used by FGM and Hybrid-BML models in conjunction with the "Initialization with fully burned state" option. Two new reinitialization methods of the progress variable can be selected via this expert parameter.
0: No reinitialization. 
1: Reinitialization of the progress variable based on its initial condition (constant value applied to the entire domain).
2: Reconstruction of the progress variable based on the current temperature field.
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied to scale the heat fluxes boundary condition(s). During the course grid initialization the heat flux(es) is/are set to zero. The idea of this switch is to ensure that the flow field and/or the combustion process is developed before extracting/adding heat.
combEquRatioCorrCoefs_ :  controls the Metghalchi-Keck coefficients [Default:2.18 -0.8 -0.16 0.22]. In the Hybrid-BML/Flamelet model it allows to change ,  ,    ,   coefficients of the linear fit, for alpha and beta exponents respectively, in the equivalent ratio correlation. 
iPartPremNonAdiabEffOnFlameSpeed_ : Activate non-adiabatic effect on the laminar/turbulent flame speed calculation in Hybrid-BML model. By default, the value of this expert parameter is set to 0. If active, the unburned quantities are looked-up in table accounting for heat gains and losses
combTimeStep_: By default (value=0), the time step solving all the combustion equations is determined by using the acoustic propagation speed (u+c). When setting the expert parameter combTimeStep_ to 1, the time step is determined by using the advective propagation speed (u).

Cavitation with the Transport Equation Model
Overview
The Transport Equation Model (TEM) for cavitating flow modeling is based on an Eulerian homogeneous flow model (phases are assumed to be in kinematic and thermodynamic equilibrium). The continuity, momentum and energy equations are solved for the mixture (liquid and vapor) and an additional transport equation is solved for the vapor volume (or mass) fraction. Derived from the Rayleigh-Plesset equations of vapor bubbles growth, condensation and evaporation, source terms are included in this additional transport equation in order to describe the phase change. FINE™/Open provides three formulations of the source terms: Singhal et al. (2002),  Zwart et al. (2004) and Tani et al. (2009). By means of OpenLabs™, the user will be able to modify one of the existing source terms or completely change it by a new one. With the transport equation model, it is possible to model cavitation including or excluding thermal effects. 
The limitations for the cavitating flow modeling with the TEM are:

Can be used only with incompressible fluids.
The cavitation model with the TEM without thermal effects should only be used when the derivative of the saturation pressure with the temperature is small. 
ONLY compatible with the Merkle preconditioning.

               The Singhal model is not compatible with the following flow models
            


                Laminar Navier-Stokes
            

               The turbulence model Spalart-Allmaras
            

                The turbulence model Spalart-Allmaras (Extended Wall Function)
            

                The turbulence model SARC
            
The turbulence model SARC  (Extended Wall Function)
            

              The turbulence model S-BSL-EARSM
The turbulence model S-BSL-EARSM (Extended Wall Function)



Settings and Guidelines in FINE™/Open
There is no access of the Cavitation Model with the TEM through the graphical user interface. The user has to activate this model by setting the expert parameter iCavitation_ to 3. The other expert parameters setting the cavitation model with the TEM excluding thermal effects are as follows.
Define the used transport equation:
cavFCM_iVaporMassFracEqs_:	Select the vapor equation type used in the transport equation model. 
0 (default): Solve for the vapor volume fraction equation.
1: Solve for the vapor mass fraction equation.
cavFCM_iFullPreconditioning_:	Control to consider the volume or mass transport equation in the preconditioning matrix when the transport equation cavitation model is activated.
0: Do not consider the transport equation in the preconditioning.
1 (default): Consider the transport equation in the preconditioning.
Define liquid properties:
cavRhoL_:	Density of the liquid phase [kg/m3] (default value 1000).
cavMuL_:	Dynamic viscosity of the liquid phase [Pa.s] (default value 1.001E-3).
cavFCM_cL_:	Speed of sound of the liquid phase [m/s] (default value 1481.7).
Define vapor properties:
cavMuV_:	Dynamic viscosity of the vapor phase [Pa.s] (default value 9.73E-6).
cavRhoV_:	Density of the vapor phase [kg/m3] (default value 1).
cavPv_:	Vapor pressure [Pa] (default value 2000).
cavPrV_:	Prandtl number of the vapor phase (default value 0.74).
cavFCM_cV_:	Speed of sound of the vapor phase [m/s] (default value 423.08).
cavFCM_MinDensClip_:	The mixture density could vary between the limiting states of pure liquid and pure  gas. However, and especially for industrial cases,  it has been found that allowing the density to reach the pure gas value heavily destabilizes the convergence and even, very often, leads to divergence of the flow solver. It is for this reason that the minimum mixture density allowed is clipped. When the fluid used is water, it has been found that a clipping density value of 60 kg/m3 produces satisfactory convergence rates without significantly damaging the solution. If the value of cavFCM_MinDensClip_ is set to -1, no clip is activated. If the value is set to a positive number, the density is not allowed to be lower than this number. The default value is set to 60.
Define source terms describing the phase change:
cavFCM_SourceTerm_:	Select the formulation used in the source term that describes the phase change.
1 (default): Singhal.
2: Zwart.
3: Tani.
cavFCM_SourceRelaxFactor_minus_:	Relaxation factor for the negative source term (condensation) when the transport equation cavitation model is activated. Default value is 0.2.
cavFCM_SourceRelaxFactor_plus_:	Relaxation factor for the positive source term (evaporation) when the transport equation cavitation model is activated. Default value is 0.02.
cavFCM_Singhal_Cc_:	Modeling constant (default value 0.05) that multiplies the condensation part of the source term. Used when iCavitation_=3 and the Singhal model is used (cavFCM_SourceTerm_=1). 
cavFCM_Singhal_Ce_:	Modeling constant (default value 0.1) that multiplies the evaporation part of the source term. Used when iCavitation_=3 and the Singhal model is used (cavFCM_SourceTerm_=1). 
cavFCM_Zwart_Fc_:	Modeling constant (default value 0.001) that multiplies the condensation part of the source term. Used when iCavitation_=3 and the Zwart model is used (cavFCM_SourceTerm_=2).
cavFCM_Zwart_Fe_:	Modeling constant (default value 5) that multiplies the evaporation part of the source term. Used when iCavitation_=3 and the Zwart model is used (cavFCM_SourceTerm_=2).
cavFCM_Tani_Cc_:	Modeling constant (default value 0.06) that multiplies the condensation part of the source term. Used when iCavitation_=3 and the Tani model is used (cavFCM_SourceTerm_=3).
cavFCM_Tani_Ce_:	Modeling constant (default value 0.12) that multiplies the evaporation part of the source term. Used when iCavitation_=3 and the Tani model is used (cavFCM_SourceTerm_=3).
cavFCM_Cturb_:	Modeling constant (default value 0.39) to account for the turbulence-cavitation interaction. Used when iCavitation_=3 and the turbulence model is k-based (k-epsilon, SST, ...).
cavFCM_SurfTension_:	Surface tension used in Singhal model (default value 0.072759). Used when iCavitation_=3 and the Singhal model is used (cavFCM_SourceTerm_=1).
Settings and Guidelines for the Transport Equation Model with Thermal Effects
In addition to the parameters described above, modeling cavitation with the transport equation model including thermal effects requires setting additional expert parameters.
Define the method used to take into account the thermal effects:
cavFCM_iThermo_:	Select the option of modeling the dependency of the saturation pressure on the temperature that is used in the transport equation model. 
0 (default): No thermal effects taken into account.
1: Model the saturation pressure based on the ideal temperature depression. Solving the energy equation is not required.
2: Model the saturation pressure as a polynomial function of the temperature. Solving the energy equation is required.
Define the model parameters specific to cavFCM_iThermo_=1:
cavFCM_Gsat_:	Derivative of the saturation pressure with respect to the temperature [Pa/K]. The default value is 143.75, which is the value for water at 293 K and a saturation pressure of 0.023 bar. 
Define the model parameters specific to cavFCM_iThermo_=2:
cavFCM_PvPolynomial_:	Coefficients defining the polynomial used to model the dependency of the saturation pressure [Pa] on the temperature [K]. 5 coefficients need to be provided, starting from order 0. The default values are [1.131871e7 -1.483606e5 7.342645e2 -1.628494e0 1.367673e-3], which are the values for water between 280 K and 450 K.
cavFCM_TRange_:	Temperature range used for the calculation of the saturation pressure. 2 bounds need to be provided. If the temperature exceeds the bounds, the saturation pressure will be evaluated at the bound. The default values are [0 5000], which implies that the temperature is not bounded by default.
Define general model parameters:
cavFCM_NSubiterations_:	Number of sub-iterations used per time step to calculate the cavitation source terms (default value 1). At least 20 sub-iterations are required, but it is recommended to use 50 sub-iterations to ensure better convergence of the computation. 
Define additional liquid properties:
cavFCM_Latent_:	Latent heat of vaporization [J/kg]. The default value is 2,453,900, which is the value for water at 293 K and a saturation pressure of 0.023 bar.
Define additional vapor properties:
cavFCM_cpV_:	Heat capacity at constant pressure of the vapor [J/(kg K)]. The default value is 1,905.9, which is the value for steam at 293 K and a saturation pressure of 0.023 bar. The heat capacity at constant pressure of the liquid will be taken from the Fluid Model page.
Define the thermal conductivity. The user can define the thermal conductivity for the liquid and the vapor either by supplying the values directly or by supplying the Prandtl numbers. This is determined by the selection of the Heat conduction law made in the Fluid Model page.
In case the Heat conduction law is defined by Constant K:
cavKappaL_:	Thermal conductivity of the liquid phase [W/(m K)]. The default value is 0.59843, which is the value for water at 293 K and a saturation pressure of 0.023 bar.
cavKappaV_:	Thermal conductivity of the vapor phase [W/(m K)]. The default value is 0.018228, which is the value for steam at 293 K and a saturation pressure of 0.023 bar.
In case the Heat conduction law is defined by Prandtl:
The Prandtl number of the liquid phase is set by the user in the Fluid Model page.
cavPrV_:	The Prandtl number of the vapor phase is described in the section excluding thermal effects.
General guidelines for modeling cavitation using the transport equation model with thermal effects are as follows:

It is recommended to use the Zwart model (cavFCM_SourceTerm_=2) as the condensation/evaporation source term. This model gives the best overall results for TEM with thermal effects. In practice, the Zwart model gives the closest estimate of cavitation pockets. 
It is recommended to set the minimum allowable density cavFCM_MinDensClip_ to 10% of the liquid density (which is given by the expert parameter cavRhoL_). Doing this will considerably help the convergence of the simulation without significantly impacting the results. 
The temperature may vary strongly during the first iterations of the solver. This can cause difficulties with convergence, because the saturation pressure, and thus the phase change source terms, will depend on the temperature. It is recommended to define an interval of temperatures inside which the solution is allowed to evolve, in order to avoid difficulties with convergence. At the end of the simulation, it is necessary to verify that the temperature of the converged results never reaches the bounds defined in the interval cavFCM_TRange_. Otherwise, the results of the simulation may be affected.

               If the temperature is an important output of the simulation, it is recommended to use the second option of modeling the dependency of the saturation pressure on the temperature (cavFCM_iThermo_=2). The first option (cavFCM_iThermo_=1) converges faster and gives a good estimate of the pressure. This option is not recommended for accurate computations in which the temperature is of interest, or if it is expected to have regions of gas only.

               The mass flow error must be carefully verified after a simulation with cavitation.

The other general parameters and guidelines of the cavitation model with the transport equation model in the FINE™/Open GUI are:
Fluid model



Incompressible liquid MUST be used in the Physical Configuration/Fluid Model page in order to use the cavitation model with the transport equation model.
Note, the density and viscosity of the fluid will be overwritten by the expert parameter cavRhoL_ and cavMuL_, respectively.


Initial Solution



When the cavitation model with the transport equation model is activated, the cavitating flow field can be initialized in different ways:


Start from a uniform initial solution of pressure and velocities (Constant values). When  initializing by Constant values, it is recommended to use an initial pressure value significantly larger than the saturation pressure. This enforces the computation to start with a pure liquid flow solution.


For turbomachinery applications, start from the 'initial turbomachinery solution' (For turbomachinery).


Start from a converged solution from a pure incompressible simulation or from another cavitating condition. For high cavitating pockets (low cavitation numbers) it might be difficult to start from a uniform solution. In those cases it is recommended to use the restart option. Further, in order to produce a performance curve for a pump or inducer, the restart option can also reduce the computation (and engineering) time.




Numerical parameters



When the cavitation model with the transport equation model is activated, the CFL number MUST be set to 1.0. In case of convergence problems, it can be even reduced to 0.5 or 0.2.
The multigrid method is compatible with the cavitation model. Four multigrid levels can in general be used. However, in case of convergence difficulties, the user might consider reducing the number of grid levels to 3 or even 2.


Outputs



All the available output variables for cavitating flow are listed in the Computation control/Outputs page. Please refer to the Cavitation section for more details.


Control Variables

In order to improve the robustness of the cavitating flow simulation, the following expert settings are recommended:
spc_RhoswitchInArtDissip_: 	By default this parameter is set to 0, meaning that the only sensor used to activate second-difference dissipation in regions of strong gradients is a pressure switch. When the cavitation model is used, this parameter should be set to 1 in order to activate a density switch in addition to the pressure switch.
tm_iResSmoothing_: By default this parameter is set to 2, meaning that the residual smoothing is only applied to the first 5 equations (continuity, momentum and energy). When the cavitation model is used, this parameter should be set to 0.
spc_dissip_wall_:	The default value of this parameter is 2, meaning that there is no artificial dissipation at the wall boundaries. When a cavitation model is used and is difficult to get convergence, the value can be changed to 1 in order to activate the computation of the artificial dissipation  at the wall boundaries.
turb_mutMuLimit_:	 By default this parameter is set to 50000, meaning that the ratio between the turbulent viscosity and the molecular viscosity is limited to 50000. In order to avoid an unphysical behavior of the turbulence model, it is recommended to set this parameter to a higher number, for example 200000.

Outlet Condition
The outlet boundary condition page is customized according to the configuration of the project (Cartesian or cylindrical). The user has the freedom to access both types of configurations in the boundary conditions page independently of the mesh properties.
For a supersonic outlet all variables are extrapolated. An outlet is considered as supersonic by the velocity normal to the boundary.
Three types of subsonic outlet boundary condition are available, as shown in FIGURE 19. These different boundary conditions are described in the following paragraphs.
An option for treatment of backflow (Backflow Control) can be activated. The purpose of this option is to prevent the flow to re-enter in the domain by applying a slip wall boundary condition locally to the velocity.


FIGURE 19 Outlet boundary conditions page.
Pressure Imposed
There are three different methods to impose the pressure at the outlet:

Static Pressure Imposed: the static pressure is imposed on the boundary, the static temperature and the absolute velocity components are extrapolated. As described for the inlet conditions, the static pressure can be constant or defined as a data profile. To define a profile as a function of space click on the profile button to the right of the input text box. The Profile Manager will appear.
Radial Equilibrium: This boundary condition is applicable only to cylindrical problems. The outlet static pressure is imposed on the given radius and integration of the radial equilibrium law along the spanwise direction allows calculation of the associated profile of the static pressure. A constant static pressure is imposed along the circumferential direction. 
Please note that the given radius should be between hub and shroud. Otherwise, the outlet static pressure will be imposed on the corresponding extreme radius of the outlet instead of the given radius.
Average Static Pressure Imposed: if imposing a uniform static pressure at the outlet is not an appropriate approximation of the physical pressure distribution at the outlet, an averaged static pressure may be used. In this case, only an averaged value for the static pressure is imposed while the pressure profile (around this average) is extrapolated from the interior field.

Mass Flow Imposed
When imposing the mass flow at the outlet the related patches must be grouped. This allows there to be several groups of patches, each of which constitutes an outlet through which the mass flow can be controlled.
The mass flow boundary condition cannot be applied to a group which patches come from different blocks.
When using a mirror periodicity, the mass flow specified in the interface equals the mass flow through only half of the inlet. When using a rotational periodicity, the mass flow specified in the interface equals the mass flow through the whole inlet (360 degrees).
Two different techniques are available to impose the mass flow:

Velocity Scaling: the pressure is extrapolated and the velocity vector is scaled to respect the mass flow. This technique is only valid for subsonic flows and is not recommended in case of significant back flows along the exit boundary.
Pressure Adaptation: this boundary condition is identical to the "Uniform outlet pressure" or "Radial equilibrium" (if the option Radial Equilibrium is activated) boundary conditions, except the fact that the exit pressure is automatically modified during the resolution process so that after convergence, the prescribed mass flow is obtained. When this boundary condition is used, the user has to specified the reference temperature through the expert parameter TRefBCpAdapt_, see more information in the theoretical manual. 

Additionally, the initial pressure which is used to create the initial solution, should be defined by the user. The option Constant Pressure During FMG Initialization uses a uniform static pressure outlet condition during the full-multigrid initialization process. For robustness reasons, it is activated by default.

OpenLabs™

OpenLabs™ is a module of FINE™/Open with OpenLabs™ environment, which allows the user to customize the internal physical models in FINE™/Open and/ or add external physical models. Here, "internal" means that the physical models have already been implemented in FINE™/Open and "external" means that the physical models will be defined by the user through OpenLabs™. 
OpenLabs™ gives the user ability to access the physical model in the FINE™/Open solver. OpenLabs™ transforms the user-defined physical models to a library that will be loaded by the flow solver when launching the computation. To describe a physical model, the user need to write a resource file that lists a set of objects (including constants, transport equations, algebraic relations, source terms and so on) and their math expressions in a metalanguage as described below. OpenLabs™ will transform the resource file to a C++ file and build it to a dynamic library. What user need to do is to set a FINE™/Open project, write the resource and build the library, then launch the computation.

Advanced Parameters
iCstInterpol_:	Select the method of interpolation to get the nodal values.
0 (default): the linear interpolation is used,
1 : the constant interpolation is used. 
out_allRes_ta_:	 Specify the frequency  that the residual is outputted in the .res file when running unsteady computations. When using the dual time stepping method, the frequency is applied to the inner-iteration cycle only. For each inner-iteration cycle, the residuals of the first iteration, every # iteration (# is the frequency) and the last iteration will be outputted. When using the explicit time stepping method, the frequency is applied to the time steps. The residuals of the first time step, every # time step (# is the frequency) and the last time step will be outputted.

out_copyFiles_: by default (value 1), the FINE™/Open solver copies the mesh files to the computation folder. When settings out_copyFiles_ to 0, the FINE™/Open solver will create links instead of copying the mesh files in order to save disk space. 
out_copyFiles_=0 only works on LINUX.
out_CPUperIteration_:	Control the output of the CPU time per iteration.
0 (default): no information on the CPU time of per iteration is outputted.
1: the CPU time of per iteration will be outputted in the .log and .std file. For each iteration, the following information will be outputted:
MainSolver::main-->Iteration performed in 0h 0m 15s
MainSolver::main-->Comm time is 0.5 construction 0.04
The first line gives the CPU time information. The second line gives the time communication between the processors during the calculation (Comm time) and the time to construct links between the processors for the communication (construction).
out_derQntFromNode_:	 When exporting the results to CFView™, the derived quantities can be computed before or after interpolating the primitive variables to nodes:
0 (default): derive quantities before interpolation to nodes;
1: derive quantities after interpolation to nodes.
out_gaugeForceTorque_:	For some applications, for example automotive applications, the outputted lift depends on the far-field value of the static pressure, because the car surface is not a closed one due to the presence of the contact patch between ground and the tyre. Using the expert parameter out_gaugeForceTorque_ will allow the user to get the lift and drag that are independent of the farfield value of the static pressure.
0 (default): the force and torque are computed by integrating the static pressure.
1: the force and torque are computed by integrating the (static pressure - reference pressure). Where the reference pressure is defined in the Advanced tab.
out_globQuantPerIt_: Allow to export the global results in function of the number of time steps on the finest grid level. This function only works in case of unsteady computations. If setting to 1, a ".globalout" file will be saved in the computation folder, which contains the exported data, see The globalout file for more details.
out_mfFileVersion_: Control the content of the MF file.
0 (default): This is the default format used in FINE™/Open.
1: The global performance will be written using the same format as in FINE™/Turbo.
out_periodicForcesAndMoments_ : Control the integration when computing the forces and moments in the .wall output file.
0 : the forces and moments are computed on specified solid patches without taking into account the periodicity.
1 (default): the forces and moments are computed on specified solid patches taking into account the periodicity.
out_resCluster64_:	 Control the save of the .res file in the parallel computation. Sometimes, the .res file generated on 64 bits Cluster can not be read by Monitor. In this case, the user can set out_resCluster64_ to solve the problem.
0 (default): each processor is writing data in .res file.
1: only the first processor is writing data in .res file.
out_saveAHEX_:	If setting this parameter to 0, the partitioning data (".ahex", ".fmf", ".fnmb", ".pmf", ".vmf" and ".dtw") will not be saved to disk. This parameter has an effect in combination with the parallel partitioner (PartitionerParallel_=1) only. Note, the required memory when out_saveAHEX_=0 will be ~10% more than the one when out_saveAHEX_=1.
out_wallForcesPerIt_: Allow to export the lift, drag and moment on per patch or per group of patches in function of the number of iterations on the finest grid level. If setting to 1, a ".fmperit" file will be saved in the computation folder, which contains the exported data, see The fmperit file for more details.
out_writeAllCtrlPts_ta_: Control the output of the solution on the  control points in inner iteration cycles when using the dual time stepping method.
 0 (default): the flow solver will  save the solution  only at the last inner iteration.
 1: the flow solver will  save the solution at each inner iteration.
out_writeCtrlPts_ta_: Control the interval of the time steps at which the solution on the control points is written in unsteady mode. By default, the value is set to 1, which means that the solution will be written at each time step. 
out_writeForces_ta_: Control the  interval of the time steps at which the forces (see out_wallForcesPerIt_) and the global results (see out_globQuantPerIt_) are written in unsteady mode. By default, the value is set to 1, which means that the forces and the global results will be written at each time step.

How to maintain a Multi-species Framework by expert parameters
Introduction

Before FINE™/Open with OpenLabs™ v6.1, the multi-species framework (inert) can only be defined by expert parameters. This section explains all the related settings. It should be noted, this section is just for backward compatibility. The user should always use the interfaced settings.
The limitations of the multi-species framework in FINE™/Open with OpenLabs™ are as follows:

The multi-species environment will not be coupled with reaction source terms
The multi-species environment is not available for the simulation of a mixture of incompressible fluids.
Inlet and external boundary conditions for species mass fractions have to be specified with OpenLabs.

Settings and Guidelines in the FINE™/Open GUI
There is no access of the multi-species transport through the graphical user interface. The user has to activate this model by setting the expert parameter MSP_iMultispecies_ to 1. 
The other expert parameters for multi-species model are:
MSP_NUM_YSPEC_: Number of species (Integer value. Minimum value: 1, default value: 2, maximum value: 20).
MSP_cpConstSpecies_: is an array of 20 dimensions to specify the isobaric heat capacity of each species for a mixture of perfect gases (default value: 1040 J /(kg K) for each dimension).
MSP_cpSpeciesNASACoeff1_, ... , MSP_cpSpeciesNASACoeff20_: an array of 18 dimensions to specify the NASA polynomials for each species. Maximum of 20 species can be simulated with multi-species framework. For example, the array MSP_cpSpeciesNASACoeff1_ defines the coefficients for the first species, MSP_cpSpeciesNASACoeff2_ defines the coefficients of the second species, and so on. 
MSP_iConductivityLaw_: parameter to steer the thermal conductivity law.
0 (default): Constant thermal conductivity.
                                1: Prandtl similarity   
MSP_iConductivityMixingLaw_: Integer valued parameter to steer the mixing law of the thermal conductivity (rule how the thermal conductivity is determined from the thermal conductivity of the individual species).
0 (default): Mass-weighting
1: Simplified form of Wilke's law
MSP_iConductivitySpeciesLaw_: Integer valued array of 20 dimensions to steer the conductivity law of each species. Currently, each parameter has to be the same and equal to the value of MSP_iConductivityLaw_ (default value 0).
0 (default): Constant thermal conductivity coefficient
1: Determination of the thermal conductivity coefficient assuming Prandtl similarity
MSP_iCpSpeciesLaw_: Integer valued parameter for selecting the law applied for determination of the isobaric heat capacity of each species.
0 (default): Read only constant coefficients
1: Read only NASA polynomials
MSP_iDiffusionLaw_: Integer valued parameter to steer the law for determining the way the viscosity is calculated for each species.
0 (default): Constant diffusivity 
1: Schmidt similarity
MSP_iSpeciesEOSModel_: Integer valued array of 20 dimensions to steer the law for determining cp for each species. Currently, each value of the array have to be the same and oriented after the parameter MSP_iCpSpeciesLaw. For MSP_iCpSpeciesLaw_ = 0, each element of the array MSP_iSpeciesEOSModel_ has to be set to 1. For MSP_iCpSpeciesLaw_ = 1, the No. elements of this array have to be set to 2. (In later release, we might open for an own EOS for each species). (default value of each array element: 1). 
MSP_iMultispecies_: Integer valued parameter for activation of the multi-species environment. 
0 (default): Multi-species environment inactive; a standard single species simulation will be carried out.
1: Multi-species environment activated.
MSP_lambdaConstSpecies_: Real valued array of 20 dimensions to define the thermal conductivity of each species (in case of MSP_iConductivityLaw_ =0) (default value of each array element: 0.0283 W/m/K ).
MSP_massDiffCoeffConstSpecies_: Real valued array of 20 dimensions to define the laminar diffusivity of each species (default value of each array element: 2.29e-05 m²/s).
MSP_molarMassSpecies_: Real valued array of 20 dimensions to define the molar mass of each species (default value for each array element: 0.028 kg/mol).
MSP_muConstSpecies_: Real valued array of 20 dimensions to define the dynamic viscosity coefficient for each species (in the case that MSP_iViscosityLaw_ = 0) (default value: 1.8E-5 kg/m/s).
MSP_schmidtSpecies_: Real valued array of 20 dimensions to define the laminar Schmidt number of each species (in case of MSP_iDiffusionLaw_ = 1) (default value of each array element: 0.7).
MSP_yspecFree_: Real valued array of 20 dimensions to define the initial value of each species mass fraction (including the n-th species). The sum of the mass fractions must be equal to 1, otherwise the flow solver will stop (default value of the array: 1, 0, 0, 0, … 0).
Fluid Model



Multi-species simulations can be performed by using either perfect gas or real gas fluid. Computations performed using perfect gas will have constant specific heat capacity () value. For real gas computations,  of each species depends on the temperature and is defined by using NASA polynomial. 


Boundary Conditions



Species Mass fraction of all species has to be specified at all inlet and external boundaries, which must be done by OpenLabs, please refer to OpenLabs chapter to learn how to customize the boundary condition in OpenLabs.

 Inlet boundary: Species mass fraction of all species at inlets by default is set to 0. Mass fraction of each species should be specified and the sum of all species mass fraction should be 1 on any given inlet, otherwise, the flow solver will stop. A sample of OpenLabs ResouceFile is given below. In this sample, there are 4 species on the the inlet Block_1_group_0.
 =>CUSTOM_BOUNDARY_CONDITIONS
@ CUSTOMIZED_BOUNDARY_CONDITION: Y1
->EXPRESSION: 0.
->ExistingVariable: Yspec1, Block_1_group_0
@ CUSTOMIZED_BOUNDARY_CONDITION: Y2
->EXPRESSION: 0.233
->ExistingVariable: Yspec2, Block_1_group_0
@ CUSTOMIZED_BOUNDARY_CONDITION: Y3
->EXPRESSION: 0.
->ExistingVariable: Yspec3, Block_1_group_0
@ CUSTOMIZED_BOUNDARY_CONDITION: Y4
->EXPRESSION: 0.767
->ExistingVariable: Yspec4, Block_1_group_0
External Boundary: In order to perform multi-speices computation with external boundary condition, species mass fraction should be specified at the external boundaries. A sample specifying species mass fraction for external boundary is given below:
@ CUSTOMIZED_BOUNDARY_CONDITION: Y1
->EXPRESSION: 1.0
->ExistingVariable: Yspec1, room_group_1



Numerical Parameters

The CPU Booster can be activated when using the multi-species framework. In case  multi-species simulations do not converge with the CPU Booster,  the following parameters can be modified:

Decrease the CFL number.
Switch off the CPU Booster during the coarse grid initialization.

Cavitation with the barotropic state law
Overview
The first cavitation model is based on the barotropic state law which describes the density change when the pressure falls below the liquid saturation pressure. Barotropic means that the density depends only on the pressure. This model can only be used with incompressible fluids. Both pure phases (liquid and gas) are considered incompressible. The barotropic law is used to describe the density variation in function of pressure from the liquid density to the gas density. Thermo-sensitive effects will NOT be taken into account when using the barotropic law.
The limitations for the cavitation model with the barotropic law are:

The cavitation model with the barotropic law should be used when the derivative of the saturation pressure with the temperature is small.
The cavitation model with the barotropic law is ONLY compatible with Hakimi preconditioning.


Settings and Guidelines in FINE™/Open with OpenLabs™
There is no access of the Cavitation Model with the barotropic law through the graphical user interface. The user has to activate this model by setting the expert parameter iCavitation_ to 1. 
The other expert parameters setting the cavitation model with the barotropic law are:
Define liquid properties:
cavRhoL_:	Density of the liquid phase [kg/m3] (default value 1000)
cavMuL_:	Dynamic viscosity of the liquid phase [Pa.s] (default value 1.001E-3)
Define vapor properties:
cavMuV_:	Dynamic viscosity of the vapor phase [Pa.s] (default value 9.73E-6)
cavRhoV_:	Density of the vapor phase [kg/m3] (default value 1)
cavPv_:	Vapor pressure [Pa] (default value 2000)
cavPrV_:	Prandtl number of the vapor phase (default value 0.74)
Define the barotropic law:
cavAmin_:	User parameter related to the maximum slope of the barotropic law (default value 50). The convergence rate can be quite sensitive to this parameter. Low cavAmin_ value implies large derivative of density with pressure. For values of lower than 20, the solver might have convergence difficulties.
The other parameters of the cavitation model with the barotropic law in the FINE™/Open GUI are:
Fluid model



Incompressible liquid MUST be used in the Physical Configuration / Fluid Model page in order to use the cavitation model with the barotropic law.


Boundary conditions



It has been observed that the following combination of boundary conditions is more robust when the cavitation model with the barotropic law is activated:

Static quantities or mass flow imposed at the inlets (velocity, temperature and turbulence variables) 
Static pressure is imposed at the outlet. Imposing the static pressure at the outlet actually means imposing the cavitation number () at the outlet. However, for most of the test cases, the known parameter of the operating conditions is the cavitation number () at the inlet. Then, the idea is to modify the static pressure at the outlet until we obtain the desired cavitation number at the inlet. 



Initial Solution



When the cavitation model with the barotropic law is activated, the cavitating flow field can be initialized by Constant values or From file.
When the cavitating flow field is initialized by Constant values, it is recommended to use an initial pressure value significantly larger than the saturation pressure. This enforces the computation to start with a pure liquid flow solution.

In some cases, the cavitation simulation initialized by Constant values may have convergence problem. In this case, it is recommended to start the cavitating flow simulation from a converged incompressible simulation without cavitation. The incompressible flow solution will have an extremely low pressure where cavitation is supposed to occur. Experience shows that it is more robust to moderate the intensity of cavitation as an initial solution. In FINE™/Open with OpenLabs™, the strategy used is to start a cavitating flow simulation from an incompressible simulation result but modifying the pressure inside the two-phase region. To use this strategy, the user needs to select From file and deactivate the option Import convergence history in the Initial Solution page.


Numerical parameters



When the cavitation model with the barotropic law is activated, the CFL number MUST be set to 1.0. In case of convergence problems, it can be even reduced to 0.5 or 0.2.
The Multigrid method is compatible with the cavitation model. Four multigrid levels can in general be used. However, in case of convergence difficulties, the user might consider reducing the number of grid levels to 3 or even 2.


Control Variables

In order to improve the robustness of the cavitating flow simulation, the following expert settings are recommended:
cavPreFactorRhoDissip_: 	Controls the first order density differences term added to the artificial dissipation of the continuity equation in case of cavitation modeling (default value 1.0)
spc_RhoswitchInArtDissip_: 	By default this parameter is set to 0, meaning that the only sensor used to activate second-difference dissipation in regions of strong gradients is a pressure switch. When the cavitation model is used, this parameter should be set to 1 in order to activate a density switch in addition to the pressure switch.
tm_iResSmoothing_	: By default this parameter is set to 2, meaning that the residual smoothing is only applied to the first 5 equations (continuity, momentum and energy). When the cavitation model is used, this parameter should be set to 0.
spc_dissip_wall_:	The default value of this parameter is 2, meaning that there is no artificial dissipation at the wall boundaries. When a cavitation model is used and is difficult to get convergence, the value can be changed to 1 in order to activate the computation of the artificial dissipation  at the wall boundaries.
turb_mutMuLimit_:	 By default this parameter is set to 50000, meaning that the ratio between the turbulent viscosity and the molecular viscosity is limited to 50000. In order to avoid an unphysical behavior of the turbulence model, it is recommended to set this parameter to a higher number, for example 200000.

Files Produced by the FINE™/Open Solver
This section describes the files produced and used by the FINE™/Open solver. The flow solver uses most of the files described above and produces the following files:
The bout file: project_computationName.bout

This binary file contains the flow solution. It is used to restart the flow solver.


The mf file: project_computationName.mf

This ASCII file contains global performance data.


The .wall file: project_computationName.wall

This self-explained ASCII file gives information about forces and torques on the patches/groups for which the Compute force and torque option is activated on the Boundary Conditions page in the Solid  tab. In the first part of the .wall file, the force and torque on all patches/groups for which the Compute force and torque option is activated is given. Then, the force and torque on each individual patch/group for which the Compute force and torque option is activated is given. 


The res file: project_computationName.res

This file contains the residual values for each iteration of a computation. It is continuously updated during the computation. It is used by the monitor to visualize the convergence history.
The header format for this file is the following:

line 1:	Version line.

line 2:	Number of blocks (1 in FINE™/Open with OpenLabs™ projects)
line 3:	2D or 3D.
line 4:	NO-K-E, SPL-ALM or K-EPS (5-equation, 6-equation or 7-equation problem)
line 5:	Number of chemistry species (not used, for backward compatibility only).
line 6:	STEADY or UNSTEADY.
line 7:	AERO or TURBO (external or internal flow configuration).
The core file format is the following:
For iteration i=1 to itmax
4 numbers (5 numbers for unsteady) corresponding to:

For steady computations, the total iteration number, the number of adaptations performed, the number of iterations on current grid and 0.
For unsteady computations, the number of physical time steps, the total number of subiterations, the number of subiterations at the current time step, 0 and the physical time step

7 numbers corresponding to:

For internal configurations, 0, Force[Y], Force[X], irrelevant number, pressure ratio between inlet and outlet, Mass flow at inlet, Mass flow at outlet.
For external flow configurations, Lift, Drag, Moment, 0, 0, 0, 0

Finally, first the maximum and then the RMS residual for the mass equation, the 3 momentum components, the energy equation, the turbulent variables  or k and ε.



The log & std files: project_computationName.log (.std)


These ASCII files contain all the information related to the current computation. It contains a summary of the computation variables as well as any warnings and/or error messages. If the flow solver encounters a problem, this is described in the log file. This file is used for support purposes only. When a problem appears please send this file together with a detailed problem description to our local support office. The log file is written directly by the FINE™/Open solver, whereas the std file is written through the Task Manager when launching the flow solver from the FINE™/Open GUI. Both files have the same content.
For parallel calculations a ".log" file is written for each process with the filename _p<process_number>.log. The 0th process contains all output information as given in the serial case. The log files for the other process only contains a limited subset of the information specific to that process. If problems are encountered during a parallel computation all ".log" files should be sent to our local support office.


The cfv file: project_computationName.cfv

This ASCII file contains information for flow field visualization under CFView™. A complete description of the contents of this file is given in the CFView™ manual.


The ctl_out file: project_computationName.ctl_out

This file is only written if the user has specified output control points on the Computation control/Outputs(see Advanced section) page. The file has slightly different formats depending on if the calculation is steady or unsteady.
Steady Computations

A header is outputted at the beginning of the file. The header contains the coordinates of the control point and the explanation of the variables which are exported to the ".ctl_out" file. In case that preconditioning is activated, the reference quantities used by preconditioning are also outputted.
Below the header section, each iteration on fine mesh exports a separate line that contains the five primitive flow variables at the specified location. In the case of turbulent computations, the relevant turbulent quantities (, k and ϵ/ω) are also stored. The five primitive flow variables are depending on the fluid and settings in the computation:

Incompressible fluid: Pressure, velocity components and temperature. Note, as preconditioning is used by default for incompressible fluid, the pressure is replaced by the difference between the pressure and the gauge reference pressure.
Compressible fluid without preconditioning: Density, velocity components and pressure.
Compressible fluid with preconditioning: Pressure, velocity components and temperature. Note, as preconditioning is used, the pressure is replaced by the difference between the pressure and the gauge reference pressure.
Condensable fluid without preconditioning: Density, velocity components and total energy.
Condensable fluid with preconditioning: Pressure, velocity components and total enthalpy.

Note that for parallel calculations only one ctl_out file is written which contains the data for all control points on all partitions.


Unsteady Computations

In case of unsteady computations, more information is outputted in each iteration. Below the header section, each physical time step exports a separate line. In unsteady cases, each line contains the global time step, the physical time, the number of iterations and the five primitive flow variables at the specified location. In the case of turbulent computations, the relevant turbulent quantities (, k and ϵ/ω) are also stored. The order of these variables is the same as described in the section steady computations above. Data for each point is written on a separate line.
Note that for parallel calculations only one ctl_out file is written which contains the data for all control points on all partitions.




The fmperit file: project_computationName.fmperit

This file is written only if the user sets the expert parameter out_wallForcesPerIt_ to 1. The file has slightly different formats depending on if the computation is steady or unsteady.
Steady Computations

A header is outputted at the beginning of the file. The header contains the explanation of the variables which are exported to the ".fmperit" file. Below the header section, each iteration on fine mesh exports a separate line that contains the iteration number, the force along x/y/z direction and the moment along x/y/z direction.


Unsteady Computations

A header is outputted at the beginning of the file. The header contains the explanation of the variables which are exported to the ".fmperit" file. Below the header section, each physical time step exports a separate line that contains the physical time, the time step, the force along x/y/z direction and the moment along x/y/z direction.




The globalout file: project_computationName.globalout

This file is written only if the computation is unsteady and the user sets the expert parameter out_globQuantPerIt_ to 1. The file has slightly different formats depending on the flow configuration of the computation.
Internal flow or Turbomachinery

A header is outputted at the beginning of the file. The header contains the explanation of the variables which are exported to the ".globalout" file. Below the header section, each physical time step exports a separate line that contains the time step, the physical time, 0, the axial thrust, the torque, theefficiency the pressure ratio, the inlet/outlet mass flow rate.


External flow

A header is outputted at the beginning of the file. The header contains the explanation of the variables which are exported to the ".globalout" file. Below the header section, each physical time step exports a separate line that contains the time step, the physical time, the lift, the drag, the moment, 0, 0, 0, 0.

Expert Parameters
iSmartRestart_: Activate the option of saving backup files at each intermediate save and the possibility of a smart restart.
0 (default): no  backup files will be saved. When restarting a computation that had ended unexpectedly, the flow solver will read the files from the  computation folder. The convergence history cannot be kept.
1: the flow solver will save backup files at each intermediate save. When restarting a computation that had ended unexpectedly, the flow solver will read the proper files from the  computation folder or the "backup" folder, depending on the moment that the computation had ended, thus allowing the user to restart while keeping the convergence history
ta_it_restart_: the time step at which the unsteady computation will be restarted.
-1 (default): inactive
#: allow to restart from the same directory an unsteady computation from the solution saved at the time step #.
 adapt_id_restart_: the adaption step at which the mesh adaptation computation will be started.
-1 (default): inactive
		
#: allow to restart a mesh adaptation computation from the saved intermediate solution on adapted mesh #, see Save solution on intermediate adapted meshes.
The following expert parameters are dedicated to initialization procedure for the simulation of supersonic and hypersonic flows (no preconditioning):
HypInit_:	If HypInit_=1, a first order upwind discretization scheme is applied during the coarse grid initialization process and HypInitItMax_ iteration on the finest grid before switching automatically to second order scheme. 
If HypInit_=0, the solver will apply the selected scheme in Numerical Scheme menu from the beginning to the end of the simulation.
HypInitItMax_:	Gives the number of iteration that the first order upwind scheme will be applied on the finest grid before the solver switches automatically to the second order scheme. Taken into account only if HypInit_=1.
HypInitCfl_:	The CFL number used during the hypersonic initialization. Taken into account only if HypInit_=1.
HypInitResSmoo_:	Allow to activate the residual smoothing during the first order upwind initialization. Taken into account only if HypInit_=1.

Multi-species Framework
Introduction

The Multi-species framework in FINE™/Open with OpenLabs™ allows the user to simulate mixing of chemical species by solving conservation equations describing convection, diffusion and reaction of the species.  Please refer to Multi-Species Framework for more information of the theoretical part.
The limitation of the multi-species framework in FINE™/Open with OpenLabs™ is as follows:

The multi-species environment is not available for the simulation of a mixture of incompressible fluids.


Settings and Guidelines in the FINE™/Open GUI
To set up a multi-species simulation, the user should follow the steps below:

Enable multi-species framework, define a multi-species fluid.
Define multi-species parameters.
Define boundary condition of each species.

The details of each step are explained in the following sections.
Before FINE™/Open with OpenLabs™ v6.1, the multi-species framework could be defined only by expert parameters. When opening an existing project created before v6.1, the interface will keep the multi-species settings (Everything is defined by expert parameters). Please see How to maintain a Multi-species Framework by expert parameters for more details.
Define a multi-species fluid
To simulate a multi-species flow, the first step is to define a multi-species fluid. Go to the Physical Configuration / Fluid Model page, click the button Edit to open the edit panel of the fluid properties. Enter a fluid name and select the fluid type Multi-Species, the entries defining a multi-species fluid appears.



First, the user should specify the reference pressure and temperature at which the properties are defined. Then, a mixture file should be specified. The mixture file defines all the species and their properties. After specifying the mixture file, the user may be able to select the definition of each property, depending on the contents of the mixture file.
Multi-species simulations can be performed by using either perfect gas or real gas model. The user can select the model in the option Mixture type.
 
The mixture file is an external file that provides the information of the species and their properties. 
Example of a mixture file


# Version number
Version 1.0
 
# Atomic elements description: symbol + atomic mass (kg/mol)
NI_BEGIN ELEMENTS

H	0.0010079
O	0.0159996
N	0.01401
C	0.01201
NI_END ELEMENTS

 
# define the species. The molar mass is computed automatically
NI_BEGIN SPECIES

O2
N2
C3H8
NI_END SPECIES

 
# Mixture type: Real gas mixture (Cp defined by the NASA polynomials)
NI_BEGIN THERMO

C3H8	300   1000   0.93355381  2.6424579E-2  6.1059727E-6   -2.1977499E-8   9.5149253E-12  -13958.520     19.201691    1000   5000   7.5341368  1.8872239E-2  -6.2718491E-6  9.1475649E-10  -4.7838069E-14   -16467.516   -17.892349
N2	300   1000   3.298677    1.4082404E-3 -3.963222E-6     5.641515E-9   -2.444854E-12   -1020.8999     3.950372     1000   5000   2.926640   1.4879768E-3  -5.684760E-7   1.0097038E-10  -6.753351E-15    -922.7977     5.980528
O2	200   1000   3.78245636 -2.99673416E-3 9.84730201E-6  -9.68129509E-9  3.24372837E-12 -1.06394356E+3 3.65767573   1000   3500   3.28253784 1.48308754E-3 -7.57966669E-7 2.09470555E-10 -2.16717794E-14  -1088.45772   5.45323129
NI_END THERMO

 
# Mixture type: Perfect gas mixture (Cp defined by a constant)
NI_BEGIN THERMO_CP_CONST

C3H8	1670
N2	1039
O2	909
NI_END THERMO_CP_CONST

 
# Heat conduction law: Constant K
NI_BEGIN THERMAL_CONDUCTIVITY_CONST

C3H8	0.015198
N2	0.02583
O2	0.0238
NI_END THERMAL_CONDUCTIVITY_CONST

 
# Heat conduction law: Prandtl
NI_BEGIN THERMAL_CONDUCTIVITY_PRANDTL

C3H8	0.72
N2	0.72
O2	0.72
NI_END THERMAL_CONDUCTIVITY_PRANDTL

 
# Viscosity law: Constant Viscosity
NI_BEGIN DYNAMIC_VISCOSITY_CONST

C3H8	1.1e-05
N2	1.657e-05
O2	1.909e-05
NI_END DYNAMIC_VISCOSITY_CONST

 
# Mass diffusion law: Constant diffusion
NI_BEGIN DIFFUSIVITY_CONST

C3H8	1.119e-05
N2	2.23e-05
O2	1.98e-05
NI_END DIFFUSIVITY_CONST

 
# Mass diffusion law: Schmidt
NI_BEGIN DIFFUSIVITY_SCHMIDT

C3H8	1
N2	1
O2 1
NI_END DIFFUSIVITY_SCHMIDT




Syntax of the mixture file

The mixture file is subjected to the following conventions:

The mixture file starts with keyword Version following the version number 1.0.
Each property is defined inside a section, which starts with NI_BEGIN following a keyword and ends with NI_END following the same keyword.
Each line in a section defines one species or one property.
Blank spaces (Blank lines) are ignored.
All lines starting with the symbol # are comment lines.
The element symbol is case-sensitive.



Define species and properties

In the mixture file, the user needs to specify the species and their properties. A description of these parameters is presented below.
Elements

The section starts and ends with the keyword ELEMENTS. This section defines the basic atoms used in the species and its atomic mass (kg/mol). Each line defines one atom following its atomic mass.


Species

The section starts and ends with the keyword SPECIES. This section defines the species. Each line defines one species. The molecular mass is computed automatically based on the atoms in the species and its number.


Specific heat

The specific heat at constant pressure can be defined by a constant or by the 7-coefficient NASA polynomials. In the mixture file, the user can provide both definitions and then select one in the GUI under the option Mixture type.

When the specific heat is defined by a constant, the section starts and ends with the keywords THERMO_CP_CONST. In each line, one species should be given following the value of its specific heat. When the specific heat is defined as constant, the species are considered as perfect gas. In the GUI under the option Mixture type, the option Perfect gas mixture will be available for selection.
When the specific heat is defined by  the 7-coefficient NASA polynomials, the section starts and ends with the keywords THERMO. In each line, one species should be given following 18 numbers. The first 9 numbers define the low-temperature range following its 7 coefficients and the second 9 numbers define the high-temperature range following its 7 coefficients. When the specific heat is defined by  the 7-coefficient NASA polynomials, the species are considered as real gas. In the GUI under the option Mixture type, the option Real gas mixture will be available for selection.



Thermal conductivity

The thermal conductivity can be defined by a constant or by the Prandtl number. In the mixture file, the user can provide both definition and then select one in the GUI under the option Heat conduction law.

When the thermal conductivity is defined by a constant, the section starts and ends with the keywords THERMAL_CONDUCTIVITY_CONST. In each line, one species should be given following the value of its thermal conductivity. When the thermal conductivity is defined as constant,  the option Constant K will be available in the GUI under the option Heat conduction law for selection.
When the thermal conductivity is defined by the Prandtl number, the section starts and ends with the keywords THERMAL_CONDUCTIVITY_PRANDTL. In each line, one species should be given following the value of its Prandtl number. When the thermal conductivity is defined by  the Prandtl number,  the option Prandtl will be available in the GUI under the option Heat conduction law for selection.



Viscosity

The viscosity can be defined only by a constant. The section starts and ends with the keywords DYNAMIC_VISCOSITY_CONST. In each line, one species should be given following the value of its dynamic viscosity. In the GUI under the option Viscosity law, the option Constant Viscosity will be available and selected by default.
                        


Mass diffusivity

The mass diffusivity can be defined by a constant or by the Schmidt number. In the mixture file, the user can provide both definitions and then select one in the GUI under the option Mass diffusion law.

When the mass diffusivity is defined by a constant, the section starts and ends with the keywords DIFFUSIVITY_CONST. In each line, one species should be given following the value of its mass diffusivity. When the mass diffusivity is defined as constant,  the option Constant Diffusion will be available in the GUI under the option Mass diffusion law for selection.
When the mass diffusivity is defined by the Schmidt number, the section starts and ends with the keywords DIFFUSIVITY_SCHMIDT. In each line, one species should be given following the value of its Schmidt number. When the mass diffusivity is defined by the Schmidt number,  the option Schmidt will be available in the GUI under the option Mass diffusion law for selection.





Define multi-species parameters
In the page Optional Models / Multi-Species, the user can define the parameters used for multi-species simulations.


In the section General properties, the user should select the reaction type. Currently, only Inert is available. The inert multi-species simulation does not take any reactions between the species into account.
In the section Mixing laws, the user should select the mixing law (how to compute the heat conductivity and viscosity of the mixture based on the definition of each species). Two methods are available:

Averaged: the property of the mixture is computed by a mass weighted average.
Wilke: the property of the mixture is computed by using the Simplified form of the Wilke's law, see Multi-Species Framework for more details.

Boundary Conditions

            In the Boundary Conditions / Boundary Conditions page, the mass fraction of each species has to be specified at all inlet and external boundaries.


The mass fraction of each species should be specified and the sum of all species mass fraction should be 1 on any given boundary.
The other settings related multi-species are explained below:
Numerical Parameters

The CPU Booster can be activated when using the multi-species framework. In case that the multi-species simulation does not converge with the CPU Booster,  the following parameters can be modified:

Switch off the CPU Booster during the coarse grid initialization,
Decrease the CFL number.

CPU Booster is compatible only with the Merkle preconditioning.

Advanced Parameters for the Boundary Condition
Non-Interfaced Advanced Parameters
iFnmb_treatment:	 The purpose of this treatment is to avoid the appearance of spurious pressure spots along curved FNMB connections where the mesh densities on both sides of the interface are different.
0 (default): the default treatment of the FNMB connections;
1: the improved treatment of the FNMB connections. The fluxes on each faces are computed using the different normal vectors on both sides instead of using the identical common normal vector.
iGhostCylindExtrapol_:	 Control the approach of computing dummy cell coordinates:
0 (default): the old treatment;
1: the coordinates of dummy cells are computed using cylindrical extrapolation.
bc_treatThermoOnFace_:	 Control where the thermodynamic and state laws are applied when applying the boundary conditions:
0: apply thermodynamic and state laws in boundary dummy cells;
1 (default): apply thermodynamic and state laws at boundary.
bc_wallCondensableFluid_:	 Control the type of relation used to compute the density at the wall in case of condensable fluids.
0 (default): Relation used in versions older than FINE™/Open v5.2;
1: Relation used  for iCavitation_ = 2 and iCavTablesNEWALGO_ = 1.
out_forceTorqueAreaDefined_: If the solid patches are defined by using Area Defined Rotation Speed, the force and torque can be computed only on the central part of the patches with Area Defined Rotation Speed:
0 (default): the force and torque are computed on the full patch(es).
1: the force and torque are computed only on the central part of the patch(es) with Area Defined Rotation Speed.
The rotation speed of the central part of the patches with Area Defined Rotation Speed  must be not equal to 0.
out_displayForcePatchOfGroup_: The information of the force and torque is available in the ".wall" file. The expert parameter out_displayForcePatchOfGroup_ is used to control the output in ".wall" file.
0 (default): the force and torque are given only for the solid boundary groups/  patches. 
1: the force and torque are given not only for the solid boundary groups/  patches, but also for each patch in the solid boundary groups.

Advanced Parameters for Radiation Model
Non-interfaced Expert Parameters
All non-interfaced advanced parameters related to the radiation model are accessible on the Control Variables page, in the Advanced tab.
P1-model 
GP1Free_:	Initial value for the G-field of the P1 radiation model.
S2S model
S2S_nbRayPerFace_:	 The number of the rays per face used in view factor calculation. The drawback of the stochastic ray tracing method is that the accuracy is dependent on the number of the rays. In some special cases, the user can increase the value of the expert parameter S2S_nbRayPerFace_ to improve the accuracy. Note, the computational cost solving the view factors is proportional to the number of the rays.

S2S_iLevelCoarse_:	 The S2S radiation model can be quite memory and CPU consuming.  A coarsening of the boundaries, based on the agglomerated mesh, has been introduced in the FINE™/Open solver in order to reduce the computational cost. The choice of the multigrid level can be set through the expert parameter S2S_iLevelCoarse_. Note, the value of 0 means that the view factor is computed in the coarsest grid level and 1 means the second coarsest level.
S2S_NbIter_:	The radiosity equations will be solved at every S2S_NbIter_ iterations. 
S2S_BCCycle_: Number of cycles of solving the radiosity equation  at each Runge-Kutta stage. In each cycle, the flow solver solve the radiosity equation based on the boundary temperature, and then updates the boundary temperature. Iterating more cycles means deeper convergence of the coupling but needs more CPU time.
S2S_InnerIter_: The radiosity equation is solved by a Gauss-Seidel iteration. The expert parameter S2S_InnerIter_ is used to define the number of the Gauss-Seidel iterations.
S2S_RelaxFactor_: The relaxation factor used in the Gauss-Seidel iteration solving the radiosity equation.
FVM model
RadFVM_AreMirrorsSpecular:	FVM for radiative heat transfer at mirror boundaries as Specular or Diffuse.
0: Diffuse
1 (default): Specular.
RadFVM_FixedIterationNumber:	 Use the criterion of maximum number of Gauss-Seidel iterations to solve the radiative transfer equation. (default value 1)
RadFVM_IterationNumber:	Number of Gauss-Seidel iterations to solve the radiative transfer equation at each global iteration (default value 1).
RadFVM_NbIter:	Iteration frequency to compute radiation heat transfer with FVM. Number of flow iterations per radiation iteration (default value 1: means that they are synchronized )
RadFVM_NodalInt_AngularErrorTol:	Tolarance to solve the radiative transfer equation at each iteration (default value 0.1)
RadFVM_Nphi:	Angular discretization in Phi direction (default value 4).
RadFVM_Ntheta:	Angular discretization in Theta direction (default value 4).
Rad_AnisotropicScatteringCoeff:	Anisotropic scattering coefficient (default value 0.0).
If Rad_ScatteringModel = 2; this parameter is the linear anisotropically scattering coefficient
If Rad_ScatteringModel = 4; this parameter is the asymmetry scattering coefficient of the Henyey-Greenstein phase function
Rad_RelaxHeatFluxBC:	Relaxation factor for the radiation heat flux calculation at the boundaries (default value 0.2)
Rad_ScatteringCoeffValue:	Scattering coefficient value (default value 0.0)
Rad_ScatteringModel:	Scattering model.
0 (default): No scattering model
1: Linear Isotropic scattering
2: Linear Anisotropic scattering 
3: Rayleigh scattering
4: Henyey-Greenstein scattering
5: F1 Forward scattering phase function
6: F2 Forward scattering phase function
7: B1 Backward scattering phase function
8: B2 Backward scattering phase function

Mathematical Model

Advanced Parameters for Fluid-Particle Interaction
For all Lagrangian models
Lag_MaxLocalTimeStep_: Upper global bound for particle time step (default value 1.0e-4).
Lag_MinLocalTimeStep_: Lower global bound for particle time step (default value 1.0e-6).
iLag_IntegrationScheme_: Integration schemes for particles.
0 (default): First-order Euler scheme
1: Exponential Integration Scheme
iLagr_CellResidenceTime_: Controls the number of Lagrangian time steps a particle may stay in a cell before it is deleted (default value is 1000).
iLagr_TimeStepCriteria_: Controls the time step criteria for the Lagrangian method, if iLagr_Method_ is set to 1. 0 means deactivated and 1 means activated. (default value 1 1).
First: Using the particle response time as time step criterion.
Second: Using a time step criterion if droplet evaporation is activated, which limits evaporation to 10% of the mass to evaporate during one time step.
LagrMixFracSchmidtsTurb_: Turbulent schmidt number used in the modeling of the turbulent contribution to the diffusion coefficient for the lagrangian mixture fraction. The laminar contribution of the diffusion coefficient is calculated (default Value 0.7).
LagrRelaxSourceTerms_: Relaxation factor for Lagrangian source terms. The number of the Lagrangian cycles must be chosen such that the product of the number of cycles and relaxation factor is larger or equal to one, in order to account for the full source term at the end of the two-phase simulation (default value 1).
iLagr_Evaporation_: Selects evaporation for the Lagrangian.
0 (default): not selected
1: selected
iLagr_EvapModel_: Selects the evaporation model to be used.
0 (default): Rapid Mixing model
1: Abramzon-Sirignano model
2: Non-Equilibrium model of Miller, Harstand and Bellan
iLagr_HeatReferenceTemp_: Selects the model for calculation of the reference temperature.
0 (default): 1/3-rule
1: Wet-bulb -temperature
2: A-rule
iLagragian_Max_Iterations_: Defines the maximum number of iterations during one Lagrangian cycle (default value is 1000000).
Lagr_NbOfEstimatedStepsPerCell_: Controls the number of steps a particle does approximately per cell. The higher the value, the better the resolution of the statistics sampled, but computational cost will increase. The minimum value is 3.0. Any lower value is corrected by the solver to 3.0 (default value is 3.0).
LagrHeatReferenceFactor_: Provides the value of the A-rule selected with iLageHeatReferenceTemp (default value is 0.5).
Lagr_HeatCapacity_liquid_: Heat capacity of the dispersed phase for the particle/droplet evaporation models (default value 4180 J/kg/K).
Lagr_SumAtomicDiffVol_: Diffusion coefficient in droplet evaporation models. The values are sum of atomic diffusion values. The first value corresponds to the carrier phase and the second value to the vapour phase of the dispersed droplet (default values 19.7 13.1).
Lagr_CoeffConductivityVap_: Polynomial Coefficients for the conductivity of evaporated vapour for the droplet evaporation models (default values 0.007341 -1.013e-05 1.801e-07 -9.10001e-11).
Lagr_CoeffcpVap_: Polynomial Coefficients for the heat capacity of evaporated vapour for the droplet evaporation models (default values 33.76336 -5.945958e-03 2.235754e-05 -9.962009e-09 1.097487e-012).
Lagr_CoeffDynViscVap_: Polynomial Coefficients for the dynamic viscosity of evaporated vapour for the droplet evaporation models. It has three coefficients (default values -0.003189 4.145e-05 -8.272e-1).
Lagr_LatentHeatVaporization_: For droplet evaporation models this is latent heat of vaporization of the Lagrangian liquid (default value 2257000 J/kg).
iLagrOutputIterations_: Intermediate output is written during the particle tracking every iLagrOutputIterations_ iteration. The mean fields cannot be directly visualized in CFView, but the end of the simulation must be waited for in One-Way coupling mode and an output in the Eulerian cycle in Two-Way coupling mode. This expert parameter is mostly of interest if iLagr_Method == 0 is used. (default value 5000).
For injection points from file
iLagrInjectionPoints_: activates the functionality of adding Lagrangian injection points from a file.
0: No injection points file
1: Use injection points file (.lagrInjPoints)
LagrInjectionPointsDistanceTol_: tolerance in meters to check if injected parcels are inside or outside the computational domain when iLagrInjectionPoints_=1. If the distance of the injection point to the closest boundary face coordinates is smaller than the value of the parameter, then the injection point coordinates are changed to the closest boundary face coordinates. Otherwise, the flow solver will stop with an error message in the .std file.
For primary atomization and secondary breakup models

iLagr_PrimaryAtomization_: (default: 0) Activates primary atomization capabilities in FINE™/Open in combination with Fluid-Particle Interaction.
0: Deactivated
1: Activated
iLagr_PrimaryAtomizationModel_: (default: 0) For primary atomization models. Controls the primary atomization model used.
0: Blob model (for liquid core atomization)
1: LISA model (for liquid sheet atomization)
iLagr_SecondaryBreakup_: (default: 0) Activates secondary break-up capabilities in FINE™/Open in combination with Fluid-Particle Interaction.
0: Deactivated
1: Activated
iLagr_SecondaryBreakupModel_: (default: 4) For secondary break-up models. Controls the secondary break-up model used.
0: Reitz and Diwakar model
1: Pilch and Erdman model
2: Hsiang and Faeth
3: Schmehl
4: Taylor Analogy Break-up (TAB)
5: Enhanced Taylor Analogy Break-up (ETAB)
6: Cascade Atomization and Break-up (CAB)
iLagr_AtomizationAndBreakupParameters_: (default: 10000 0 1 0) Used for spray atomization and secondary break-up modeling.
First: Number of Lagrangian parcels to initialize from injector.
Second: Number of child parcel creations per parcel allowed.
Third: Number of new child parcels to initialize at each breakup.
Fourth: Activates delay of first breakup for Taylor analogy based models if set to 1.
Lagr_AtomizationInjectionCoordAndDirection_:  (default: 0.0 0.0 0.0 0.0 0.0 1.0) Used for spray atomization modeling. Coordinates of injection nozzle exit [m] and vector indicating the direction of injection [-].
First three: Coordinates of injection nozzle (x,y,z).
Second three: Direction of injection (u,v,w).
Lagr_AtomizationNozzleDiameter_: (default: 0.001) Used for spray atomization modeling with Blob model or LISA model. Diameter of the nozzle exit [m].
Lagr_AtomizationMassFlow: (default: 0.0) Used for spray atomization. Mass flow through the nozzle in kilograms per second [kg/s].
Lagr_AtomizationPressureDifference_: (default: 1000000) Used for spray atomization modeling. Pressure difference between the nozzle exit and domain [Pa].
Lagr_Atomization_InjectionTemperature_: (default: 293.15) Used for spray atomization modeling. Injection static temperature of parcels [K]. (Inside the parcels, the temperature distribution is uniform)
Lagr_AtomizationModel_LISA: (default: 12.0 3.5) Used for spray atomization in the LISA model.
First: Logarithm of the amplitude ratio of disturbances.
Second: Exponent used in the Rosin Rammler method.
Lagr_Atomization_HalfConeAngle_: (default: 0.5) Used for spray atomization modeling in LISA model. Half cone angle of the spray [rad].
Lagr_SecondaryBreakUpModel_CAB_: (default: 80 350.0 0.05) 	Specific parameters for CAB model.
						First: Critical Weber number for stripping breakup.
		Second: Critical Weber number for catastrophic breakup.
		Third: Energy ratio factor k1 (default: 0.05)
Lagr_SecondaryBreakUpModel_ETAB_: (default: 80 0.222222 0.222222) 		Specific parameters for ETAB model.
				First: Critical Weber number for stripping breakup.
		Second: Bag breakup coefficient for the energy ratio factor.
		Third: Stripping breakup coefficient for the energy ratio factor.
Lagr_SecondaryBreakUpModel_PilchErdman_: (default: 0.375 0.2274) 		Specific parameters for Pilch and Erdman model.
			First: Coefficient for T.
		Second: Coefficient for T*T.
Lagr_SecondaryBreakUpModel_ReitzDiwakar_: (default: 12 3.14158 1.0 10.0) 		Specific parameters for Reitz and Diwakar model.
		First: Critical Weber number for bag breakup regime.
		Second: Modeling constant for the characteristic time of bag breakup.
		Third: Criterion for the second regime.
		Fourth: Modeling constant for the characteristic time of stripping breakup.
Lagr_SecondaryBreakUpModel_Schmehl_: (default: 1.0 0.238 1.2) 		Specific parameters for Schmehl model.
		First: Expected value for the root-normal distribution.
		Second: Variance for the root-normal distribution.
Third: Simmons mass median mean-Sauter mean ratio.
Lagr_SecondaryBreakUpModel_TAB_: (default: 3.5 3.333333 1.0) 		Specific parameters for TAB model.
		First: Exponent used in the Rosin-Rammler distribution k.
		Second: Energy ratio factor K.
		Third: Velocity factor Cv.

Customized Fluid Property
The fluid properties (equation of state (EOS) and transport properties) can be customized. The section must start with the line "=>CUSTOM_FLUID_PROPERTIES''.
Customized EOS

All the state variables of the fluid can be customized. The section to customize the EOS must be added in the section "=>CUSTOM_FLUID_PROPERTIES" and must start with "@EQUATION_OF_STATE:". A name of the EOS has to be provided by the user. The keyword       "->UseDatabase" is used in case that the existing EOS needs to be customized. This keyword can be omitted when creating a new EOS. To change the state relation, the user is required to provide the name of the relation using the keyword "->EOS_RELATION" followed by the keyword "->EXPRESSION" to define the relation. The name of the relation must be the same as that given in the project analysis results. See the structure below.
@ EQUATION_OF_STATE: <name of the EOS>
->UseDatabase: <name of the internal EOS>                           #optional
->EOS_RELATION: <relation name1>
->EXPRESSION: <math expression>
->EOS_RELATION: <relation name2>
->EXPRESSION: <math expression>
...
The following basic EOS types have been defined and can be used:


Ideal gas: The EOS of an ideal gas follows the perfect gas law with a constant specific heat capacity. This EOS will also be adapted corresponding to the "Perfect gas" settings in the FINE™/Open GUI. The following EOS are implemented based on the ideal gas EOS:

 For premixed combustion: Combustion BML. In this EOS, the density depends on the normalized progress variable. The fluid type will be automatically adapted to "Reactive Fluid" settings in the FINE™/Open GUI when the premixed combustion model is activated.
 For non-premixed/partial-premixed combustion: Combustion Tables. In this EOS, the thermal quantities are coming from a table. The fluid type will be automatically set to "Reactive Fluid" settings in the FINE™/Open GUI when non-premixed or partially-premixed combustion model is activated.

Real gas: The EOS of a real gas follows the perfect gas law with the specific heat capacity as a function of temperature. This EOS will be adapted when "Real gas" in the FINE™/Open GUI is selected.
Incompressible fluid: The EOS of an incompressible fluid assumes a constant density and a constant . This EOS will be adapted corresponding to the settings in the FINE™/Open GUI:

 Barotropic law: dedicated to cavitation model type 1
 Full Cavitation: dedicated to cavitation model type 2
 VOF: dedicated to VOF model

Condensable gas: In this EOS, the thermodynamic quantities depend on thermodynamic table.The fluid type is set to "Condensable gas" in the FINE™/Open GUI.

The fluid type defined in OpenLabs should be the same or the upper level as the one defined in the FINE™/Open GUI. For example, when Combustion BML is used in the computation, the user can use "->UseDatabase: Ideal gas", but cannot use "->UseDatabase: Incompressible fluid" in OpenLabs™
If the user wants to define a new EOS which is not available in the FINE™/Open, the user has to define all the necessary state relations required to define the EOS.
The following limitations apply to the customized EOS:

The customized EOS is not compatible with turbo initial solution.
The customized SoundSpeed is not compatible with Mach number imposed External boundary condition (Riemann BC). 
The customized EOS is not compatible with FSI (fluid structure interaction).
The customized gas constant RGas is not compatible with Lagrangian.
The customized RGas/SoundSpeed/Temperature based on "Real gas" framework is not compatible with CPUBooster.
The customized EOS is not compatible with R/S connections.
The visualization of customized Pt, Tt is not compatible with the expert parameter out_derQntFromNode_ = 0.



Guidelines on how to customize the EOS

The equation of state (EOS) is used to close the system of Navier-Stokes equations. Five independent variables, including 2 thermodynamic variables & 3 velocity components, are solved through RANS. The other thermodynamic variables are computed from the EOS. There are various ways to compute the thermodynamic variables, either by thermodynamic EOS or by caloric EOS, for example,  or . In more general situation, it could be dependent on additional scalars, such as the mixture fraction. To customize the EOS in the solver, the user is strongly recommended to follow the following guidelines:
(1) Always select the closest fluid model as database. For example, a mixture behaves as ideal gas, the ideal gas framework is recommended as the database. Then, the user could refer to the detailed ana file, to decide which relations need to be modified.
(2) Decide to use expressions or tabulation. When the EOS is quite complex, the computational cost may not be acceptable because the EOS is calculated at each flow iteration. In this case, the user can firstly tabulate the EOS into several profiles. Then the EOS can be calculated by the interpolation of those profiles at each flow iteration. The tabulation of the EOS works with the same behavior as the fluid type condensable gas. For the tabulation of the EOS, please refer to Discrete Expression section on how to define a discrete expression by an expression.
(3) The EOS relations should be given by using the independent variables, which can be found in the ana file. For example, the following is the EOS of a premixed combustion model:



and ,
where Tu is the temperature of the unburned mixture, Tad is the adiabatic temperature of the burnt mixture. The "ProgVariable" c is resolved from a PDE and the "CombTemp" T is dependent on the variable c. In this case, the user should define the density as a function of the independent variable (variable resolved from a PDE) c rather than using the function "CombTemp" T itself. Use of dependent variables (derived from independent variables) may lead to a wrong solution or divergence. 
The resource file below demonstrates how to use the independent variables when defining the density relation for a premixed combustion model.
             The correct approach, where ProgVariable is an independent variable: 
=>CUSTOM_FLUID_PROPERTIES
@EQUATION_OF_STATE: MyEOS
->EOS_RELATION: Density
->EXPRESSION: StaticPressure/ phy_RGaz/   \
                            (1-ProgVariable)*unburnedTemp+ProgVariable*premixedFlameTemp
             The incorrect approach, where CombTemp is a dependent variable: 
=>CUSTOM_FLUID_PROPERTIES
@EQUATION_OF_STATE: MyEOS
->EOS_RELATION: Density
->EXPRESSION: StaticPressure/ phy_RGaz/CombTemp                        
(4) Since the independent variables are different according to whether the project uses preconditioning or not, the EOS are usually formulated in different way for the case with/without preconditioning.
- Without preconditioning, (ρ, p) are the independent variables. The pressure relation should be given in terms of (ρ, E) (which are resolved from the continuity & energy equations) and/or additional independent variables. The other thermodynamic variables, T, H, E, cp, ..., should be given in terms of the independent variables, i.e. ρ, p and the additional independent variables.
- With preconditioning, (p, T) are the independent variables. The temperature relation should be given in terms of (p, H) (which are resolved from the continuity & energy equations) and/or additional independent variables. The other thermodynamic variables, ρ, E, H, cp, ..., should be given in terms of the independent variables, i.e. p, T, and the additional independent variables.
TABLE 1 List of the dependent and independent thermodynamic variables







 

Without Preconditioning   


With Preconditioning       
Compressible



   Incompressible






Independent variables


 Density (ρ) and
 Pressure (p)


 Pressure (p) and 
Temperature (T)


 Pressure (p) and 
Temperature (T)




Dependent Variables


Temperature (T)
Energy (E)
Enthalpy (H)
Heat Capacity (cp) and Specific heat ratio (γ)
Speed of Sound (c)


Density (ρ)
Energy (E)
Enthalpy (H)
Heat Capacity (cp), Gamma (γ)
Speed of Sound (c)


Density (ρ)
Energy (E)
Enthalpy (H)
Heat Capacity (cp and cv)
Speed of Sound (c)




Independent          Variable relation


Pressure p=f(E) and Density =f(p,T) 
                            ρ


Temperature T=f(H)


Temperature T=f(E)




(5) Since the EOS is also used for initialization, applying boundary conditions, visualization and some numerical procedures, the relation of independent variables are also needed. To formulate the independent variables, the user certainly may use some dependent variables.

(6) For the thermodynamic quantities like static energy, enthalpy and other quantities, the values computed in CFView™ are not consistent with the values from the FINE™/Open solver. It is advised to redefine these quantities in OpenLabs and use them in CFView™.
(7) The consistency of the EOS should be maintained by the user. For example, given the energy function E=f(p,ρ), the pressure function has to be the inverse function p=f-1(E,ρ). The non-consistent relations will result in a wrong solution and divergence. Therefore, in case that the user modifies one relation from the database, the user should check all other relations for consistency (check in the ana file).


Customized transport properties

All the transport properties of the fluid (e.g., Viscosity and Conductivity) can be customized. The section to customize the transport properties must be added in the section of "=>CUSTOM_FLUID_PROPERTIES".

To add a new transport property: it must start with "@TRANSP_PROPERTY:". Then, the name of the transport property has to be given by the user and the expression of the transport property has to be defined. See the structure below.
@TRANSP_PROPERTY: <transport property name1>
->EXPRESSION: <math expression>
...
The new transport property can be outputted for post-processing, see Outputs by OpenLabs.
To modify an internal transport property: it must start with "@TRANSP_PROPERTY:". The name of the transport property has to be given by the user and the expression of the transport property has to be defined. Then, the keywords "->ExistingCalculator:" has to be used and the name of the internal property calculator must be given. The name of the internal property calculator must be the same as that in the detailed project analysis results. See the structure below.
@TRANSP_PROPERTY: <transport property name1>
->EXPRESSION: <math expression>
->ExistingCalculator: <name of the internal transport property>
...

Solid Wall Boundary Condition
The solid wall boundary condition page is customized according to the type of calculation (inviscid or viscous).
For Euler cases (i.e. inviscid), no parameter is requested for the wall boundary conditions. For Navier-Stokes cases, the upper box enables the user to choose the required thermal conditions and the lower box the associated velocity conditions.
On the SOLID page, FINE™ will group automatically the patches of a same FNMB connections in order to reduce the list of solid patches displayed. The group name will be the FNMB connection name. In particular cases, the user can still ungroup them when different settings must be applied to these patches.
If the project includes AutoGrid5™ meshes converted into HEXPRESS™ format (from v211-1), FINE™ will group automatically the patches related to turbomachinery elements (Hub, Shroud and Blade). The grouping is based on the patch names generated by AutoGrid5™. The connection types PER/PERNM/NMB existing in AutoGrid5™ will be converted into FNMB in HEXPRESS™. All FNMB connections will also be grouped automatically for each row.
Cartesian Boundary Conditions
The user can define a translation or a rotation velocity vector. In the latter case, the coordinates of the rotation centre are required. Four options are available for the thermal condition: adiabatic, constant heat flux (in W/m²), isothermal or constant heat transfer coefficient (in W/m²K). The imposed heat flux or temperature can be constant on the patch or defined as a profile. Use the pull down menu to change Constant Value to Fct(space). Click on the profile button to launch the Profile Manager


FIGURE 26 Solid boundary conditions page in case of a Cartesian boundary condition
Cylindrical Boundary Condition
The wall rotation velocity can be constant or area defined (see FIGURE 27). The area defined option allows the user to attribute a specific rotation velocity to a rectangular zone in the meridional plane independently of the grid structure. When the area defined option is selected, a small picture defining the parameters is displayed (the z axis is the rotation axis, the r axis is the radial axis). The rotation velocity is set to  outside the domain and to  inside the domain.


FIGURE 27 Solid boundary conditions page in case of a cylindrical boundary condition
The specified range must be a valid range for the geometry. For example, for an axial machine the limits for rotation of the hub can be defined by setting the lower and higher axial limit to appropriate values. In such a case it is important to set the radial limits such that they include the full solid (hub) patch.
The thermal conditions are similar to those for Cartesian flows (more details in previous section).
Euler or Navier-Stokes Wall for Viscous Flow
If the flow type is selected as laminar or turbulent Navier-Stokes, it is possible to choose between an Euler wall (zero normal velocity) and a Navier-Stokes wall (no-slip condition). Further details on the numerical treatment of walls are provided in the theoretical manual: Solid Wall Boundary Conditions. Note that the default  is a Navier-Stokes wall.  



Force and Torque
At the bottom of the right page, a "Compute force and torque" button is provided that allows the user to include the selected patches in the calculation of the global solid boundary characteristics. 
In the case of external flows (see Computation Control / Outputs page) the force and torque are computed as:

the lift,
the drag,
the moment.

The direction of the forces, as well as the reference axis and the location of the point for the moment are determined in the Computation Control / Outputs page.
In the case of internal flows, the axial thrust and torque at (0,0,0) are computed.
Properties of Solid for Turbulence
In addition, when turbulence models with extended wall function are used, the user has to specify the type of wall ("Smooth" or "Rough") and the following constants: the Von Karman constant κ and the Bo constant. If the wall type is rough, the equivalent roughness height k0 and the height of the zero displacement plane d0 are also required. A description of these constants is provided in the theoretical manual. 
Two methods considering the wall function for roughness is implemented. With the old method (default, turb_iRoughModel_=0), the constant Bo has to be computed according to the value of y+. And the value of Bo will also correct y+. The user has to iterate this procedure and converge to the desired value of Bo. This is not straightforward and a new approach has been introduced in the flow solver in order to simplify the computations with roughness. To use the new method, the user has to set the expert parameter turb_iRoughModel_ to 1.

For rough walls, the following limitations are applied:

 the distance from the wall to the cell-centre of the first inner cell should be bigger than k0 + d0. 
 the first inner cell should be located within the fully turbulent layer.




The application field of the "law of the wall" imposes restrictions on the grid. The user is strongly advised to check the conformity of this grid with these conditions (Mathematical Model section).

Premixed Combustion
Premixed combustion occurs whenever fuel and air are mixed at the molecular level prior to ignition. Reaction takes place in a combustion zone that separates unburnt reactants and burnt combustion products. This combustion mode is found in classical spark ignition engines, in many household appliances and in Bunsen burners.

Premixed Combustion in FINE™/Open GUI
On the Optional Models / Combustion page, the combustion type premixed is available. Only the BML type model can be selected as Premixed combustion model. These model assume that chemical reactions are localized in thin surface which may be represented as a sheet separating unburnt mixture from burnt gas. The formulation is based on introducing and solving progress variable equation. The progress variable equation has source terms which can be modeled using chemistry mode. Chemistry modes are the Zimont model, the Zimont model with the modification of Dinkelacker and the Lindstedt-Vaos Model. The Laminar flame speed, the adiabatic flame temperature of burnt mixture and density, the temperature, the kinematic viscosity of the unburnt mixture are inputs to the model.


FIGURE 11 Premixed Combustion parameters
Fluid model



When the combustion model is activated, the fluid is automatically changed to "Reactive fluid". The Fluid Model menu gives restricted access to fluid properties. 


Flow model



When the combustion model is activated, the turbulence model is by default set to the standard k-ε model. The other 2-equation turbulence models available can also be selected for combustion simulations. However, one equation turbulence models, such as the Spalart-Allmaras model, that are available for inert flow can not be used in conjunction with combustion modeling. 
Laminar regime can also be modeled. In the absence of turbulence, the laminar speed is taken as the effective flame speed.
In the absence of turbulent fluctuations (), the modified TFC model gives  while the TFC model gives . Hence, the modified TFC model is recommended in laminar simulations. 


Boundary conditions



Combustion-dedicated boundary conditions have been introduced at inlets, with entries for the Normalized progress variable.

The Normalized progress variable should range between 0 (unburnt state) to 1 (burnt state), the default value is set to 0.

No dedicated condition is required for the treatment of outlets, since combustion variables are purely convected quantities.


Initial Solution



Initial data for progress variable has been introduced to the Initial Solution menu. As a default, a value of unity is recommended for the Normalized progress variable. This value corresponds to a fully burnt state type initialization.


Numerical parameters

When performing premixed combustion computations, the following choices are the best recommendation:

In the General Parameters page under the tab General,

set the Number of grid(s) to 3 or 4 (preferred),
activate Coarse grid initialization.

In the General Parameters page under the tab Advanced,

 Increase the Maximum number of cycles per grid level to 400 - 600,
Reduce Convergence criteria on each grid level to -6,
Possibly increase Number of sweeps on successive grid levels to 1 2 16 (3 grid levels), or 1 2 3 32 (4 grid levels)

In the Numerical Schemes page,

The recommended CFL number is 1.5. This is also set as default.


The premixed combustion module can be used together with CPU Booster. In order to get best performance, the following settings are recommended when combining CPU Booster and premixed combustion:

In the Flow Model page,

Set the Turbulence model to  k-epsilon (Extended Wall Function) or k-epsilon (Low Re Yang-Shih, classic),

In the General Parameters page under the tab General,

set the Number of grid(s) to 3 or 4 (preferred),
activate Coarse grid initialization.

In the General Parameters page under the tab Advanced,

 Increase the Maximum number of cycles per grid level to 400 - 600,
Reduce Convergence criteria on each grid level to -6,
Deactivate the CPU Booster during coarse grid initialization

In the Numerical Schemes page,

The recommended CFL number is 100. This is also set as default.  In case of convergence problem, reduce the CFL number.
Keep the Merkle preconditioning selected.

In the Control Variables page under the tab Advanced,

Increase the density relaxation coefficient to 0.1 (the fifth dimension of the local expert parameter RelaxCombVars_). In case of convergence difficulty, set the density relaxation coefficient to 0.01 (default value).
In case that heat flux solid boundary condition is defined, set the local expert parameter IterScalingFuncHeatFlux_ to 10.
The relaxation coefficient of the progress variable (the seventh dimension of the local expert parameter RelaxCombVars_) should be kept as 1. In case of convergence difficulty, set this relaxation coefficient to 0.1.
                
In case that the S2S radiation model is activated, set the local expert parameter RadFVM_IterationNumber to 2.  




Outputs

When performing partially-premixed combustion computations, the following quantities are available for output in the page Computation Control / Outputs / General under the category Combustion.

Comb_NormalizedProgressVariable: normalized progress variable 
Comb_SourceProgressVariable1: source term of the normalized progress variable equation
Comb_Temperature: temperature of the mixture
TurbulentFlamespeed: turbulent flame speed



Expert parameters

All non-interfaced advanced parameters related to the non-premixed combustion model are accessible on the Control Variables page under the tab Advanced. 
combSDissConst_:	Specify the constant  for the mean scalar dissipation rate. The default value is 2.0.
combSchmidtTurb_:	The turbulent Schmidt number (default value 0.7). 
RelaxCombVars_:	The relaxation coefficient in combustion module. This parameter is an array of seven dimensions, corresponding to the relaxation coefficients for the mixture fraction f, the mixture fraction variance g, the enthalpy defect, the NO variable, the density update, the molecular viscosity and progress variable update respectively (Default value: 1 1 1 1 0.01 1 1).
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied to scale the heat fluxes boundary condition(s). During the course grid initialization the heat flux(es) is/are set to zero. The idea of this switch is to ensure that the flow field and/or the combustion process is developed before extracting/adding heat.
combTimeStep_: By default (value=0), the time step solving all the combustion equations is determined by using the acoustic propagation speed (u+c). When setting the expert parameter combTimeStep_ to 1, the time step is determined by using the advective propagation speed (u).

Advanced
The tab Advanced contains advanced output parameters and the control points definition.


FIGURE 9 Output Parameters - Advanced
When mesh adaptation is performed with FINE™/Open with OpenLabs™, the user can save the meshes and solution files on each intermediate, adapted mesh, by activating the Save solution on intermediate adapted meshesoption. In this case, the FINE™/Open solver outputs at the end of each computation a "*_a#.cfv"  file for the intermediate project, a "*_a#.hex" file containing mesh information related to the current grid, and associated solution files for CFView™. The number following "*_a" corresponds to the number of adaptations performed before archiving the solution. It is therefore possible in CFView™ to visualize intermediate adapted meshes and solutions. This is accomplished by opening the ".cfv" file corresponding to an intermediate project and is possible even when the flow computation is terminated on a different ("adapted") final mesh.
In the frame Reference parameters, all required reference parameters in the computation, depending on the settings, are listed. The user should specify correct value for the available parameters. When the parameters is not used by the computation, it is disabled. 
In the Control points definition frame, the user can define "control points". These are specific locations where the user can follow the evolution of the solution or to extract the final solution. The Add Point button is used to add a new control point definition in the control points area. After adding a new control point,  the control point coordinates can be modified. It is possible to remove control points by selecting the control point to be removed and then clicking on the Remove point button. The Import and Export buttons are used to import or export control points definition to file, which has the extension ".ctl" and the format as follows:
Two header lines, e.g.:

#List of control points (X Y Z)

#Created on 07/21/2003 15:08:43


This is followed by a line containing the number of control points required, e.g.:
2

There then follows a list of x,y,z coordinates of each control point, each on a separate line, e.g.:

0.5     0.5     1

0.55    0.55    1.1


 Note that all coordinates should be defined in meters irrespective of the mesh units. 
The evolution of the solution at the defined control points can be followed at each iteration (steady computations) or at each physical time update (unsteady computations) in the Convergence History page or in the Steering (). The evolution is also outputted in a ".ctl_out" file.
Note that it is impossible to change the control points definition during a computation.

Harmonic Method
Introduction
FINE™/Open with OpenLabs™ allows to compute unsteady flows at minimum costs thanks to the
			so-called nonlinear harmonic method (NLH). This approach, introduced by He and Ning (1998), can
			be considered as a hybrid method that conjugates the advantages of classical steady state and full
			unsteady calculations.
        

			
			
			
			
			The method is based on solving steady flow transport equations for the time-mean flow and the time
			harmonics. In particular, in a turbomachinery configuration, due to the relative motion, the blade
			passing frequencies (BPF) of the blade rows are the fundamentals in time of the periodic disturbances
			entering the adjacent blade rows. Solving the periodic perturbation in a row is performed in the
			frequency domain by a time-marching to the pseudo-steady state of the solution of the transport
			equations associated with the BPFs and their harmonics, the number of these being a user input. One
			important advantage of the method is that the effect of the periodic unsteadiness onto the time-averaged
			flow, the deterministic stresses, is calculated directly from the in-phase and out-of-phase
			components of the solved harmonics. Thanks to the transposition to the frequency domain, only one
			blade channel is required like a steady flow simulation. More details about the harmonic method can
			be found in the theoretical manual.
			
			
The harmonic method in FINE™/Open with OpenLabs™ is a generalized multi-rank method, which considers the unsteady effects provoked by the relative rotation of the direct adjacent blade row(s) on a reference row, as well as the interactions between the harmonics on that reference row. The maximum rank is currently limited to 2:

In case of 1-rank, the harmonic method deals with rotor/ stator interaction of only adjacent rows.
In case of 2-rank, the harmonic method considers not only the perturbation from the direct adjacent row(s) of the reference row, but also the interaction of harmonics between the direct adjacent rows. In this case, the harmonic can simulate the effects between consecutive rotors or stators (including clocking effect), or the effects between two adjacent rows that have the same rotation speed (such as configuration stator-stator-rotor). For example, for a contra-rotating open rotors (CROR) case, if the pylon of the CROR mounted on the fuselage is taken into account, then the reproduction of its unsteady effects on the flow in the rotor that is not adjacent to the pylon can be performed by the rank-2 harmonic method.

Limitations
The harmonic method can be used only in case of:

perfect gas1Compatibility with a fluid defined by thermodynamic tables is available but requires additional calibration.;
no preconditioning or Merkle preconditioning;
no inlet distortion;
no CPU Booster;
the Spalart-Allmaras2Compatibility with two equations turbulent models is available but requires additional calibration. model in case of turbulent simulations;
Adiabatic wall;
The effects are limited to 2-rank;
The maximum number of harmonics in each row is limited to 40;
The nonlinear harmonic method can only be used for turbomachinery applications. This method cannot be used for cascade configurations with translational periodic boundaries;
The flow perpendicular to the inlet (INL), outlet (OUT), external boundary (EXT) and rotor/ stator interface (ROT) has to be subsonic;
The number of frequencies per perturbation in a row is the same all over the multistage machine. 

Interface and best practices
The harmonic method can be switched on through the radio button Harmonic in the Physical Configurations / General Properties page. 


FIGURE 12 General properties
Then, the user can access the Physical Configuration / Harmonic Model page to set all parameters for the harmonic computation.
Mesh constraints

The rotor/ stator interface treatment in the harmonic method is based on the full non-matching algorithm, which requires the rotor/ stator patches belonging to a given interface to have the same spanwise extension.
Although the harmonic method does not impose a specific azimuthal position for the blade, it is recommended for post-processing purposes to align the adjacent rows in the circumferential direction. Visualization of the flow across the interface is much clearer. 
Mesh resolution in the tangential direction
The harmonic method is based on the spatial Fourier decomposition of the time-averaged flow and the harmonics in the tangential direction.
It is suggested to guarantee at least 30 grid nodes in the azimuthal direction to represent in space the first harmonic (or fundamental) of a periodic disturbance at the inlet/ outlet of a row. Then, the number of nodes in the tangential direction of the row channel should be at least 30 times the number of blades of the adjacent blade row generating this harmonic divided by the number of the blades of the row. The narrower the adjacent blade row channels, the more refined the channel should be.
It is assumed that the amplitude of the subharmonics decreases very quickly. The constraint can thus be relaxed for the other harmonics. In general, at least 30 grid notes for the first harmonic and 15 for the other harmonics are suggested.
Example

For a stator/ rotor/ stator configuration in case of 1-rank, where the number of blades in the rotor and stators are Nbrotor, Nbstator 1 and Nbstator 2 and NH is the number of harmonics:
Number of Points in Azimuthal Direction in stator 1:
30 x    if(NH=1)
15 x  x NH   if(NH>1)
Number of Points in Azimuthal Direction in rotor:
max(30 x , 30 x )   if(NH=1)
max(15 x  x NH, 15 x  x NH)   if(NH>1)
Number of Points in Azimuthal Direction in stator 2:
30 x    if(NH=1)
15 x  x NH   if(NH>1)




Harmonic Model



FIGURE 13 Harmonic settings
In the frame Harmonic Settings, the number of Maximum rank should be specified. The maximum rank of the perturbations is limited to 2. After setting the number of Maximum rank, the user needs to set the Number ofharmonics per perturbation (Default value: 3). Note, the Number ofharmonics per perturbation is common to all perturbations. 
When the Maximum rank is set to 2, the option Clocking position becomes accessible to control if the clocking position is Fixed or Variable:

Variable: From this simulation, all the harmonics from different perturbations in the same row will be resolved, whether the harmonics have the same properties or not. The user can reconstruct the flow in time or in space.  For both time and space reconstructions, the initial relative position of the rows can be defined by the user. In case of clocking effect, it allows to display the solutions for different azimuthal offset of one stator relatively to the other.
Fixed: From this simulation, all the harmonics from different perturbations in the same row will be merged if the harmonics have the same properties (phase angle and angular velocity). In this case, the user can only reconstruct the flow solution in time. Unlike the option "Variable", the relative initial position of the rows can only be changed by a multiple of the pitch. The rank-2 effects are also limited to the initial position of the rows in the input mesh.

In addition to the perturbations coming from the rows adjacent to the reference row, the multi-rank harmonic method can also consider the interaction between the harmonics.. By default, the multi-rank harmonic method does not consider the interaction of harmonics between the upstream row and the downstream row of the reference row (No interaction). But in some applications, this interaction may have important influence on the flow in the reference row. In this case, the user can activate the interaction of harmonics by checking the option  Interaction in the frame Harmonics Range. The Max order in interaction is set by default to 1. This number can be increased but cannot be larger than the number of harmonics per perturbation. For example, a max order in interaction of 3 will introduce the interaction of the first three harmonics from the upstream row and the downstream row into the reference row.
In the harmonic method, the perturbations are linearly combined. All harmonics and their conjugate harmonic are taken into account. Only harmonics having a non-negative frequency will be kept for the computation.
In the frame Harmonics Results, the harmonics defined in each group can be inspected and their status updated.


FIGURE 14 Check harmonics in each row
Each group listed in the left-tree menu can be expanded with the symbol "+"/"-".  Selecting an harmonic in the expanded menu displays its characteristics (name, angular velocity, phase angle, aliases properties and base – these parameters are detailed later on in this section) on the right side of the window.
For each group, the list of disturbers and associated harmonics can be displayed by expanding the menus  Disturbers and Harmonics, respectively. 
The expandable menu Disturbers indicates the number of harmonics considered for the modeling of the perturbation originated from the adjacent row(s). 
The expandable menu Harmonics allows to modify the harmonics to be solved. Thanks to the flexibility of the NLH method, each harmonic displayed in a group can be disabled, i.e. not solved by the solver, by unchecking the checkbox on the left of its name. 
When deactivating an harmonic (for example "1G2" in row 1), all other conjugate harmonics defined as a linear combination of the one unselected (e.g. "(-3G3;1G2)") will be ignored by the solver even if they  appear checked in the interface. 

Note that changing the settings in the menus Disturbers or Harmonics will display a warning message: 
Some global harmonics settings have changed. Harmonics need to be recomputed.
If the change is global, the harmonics results are all hidden. If the modification is local (for example, a modification in the number of harmonics for a disturber), a warning sign icon is displayed in front of the affected group in the left-tree menu.
			In both cases, the set of harmonics to be considered for the simulation must be updated by clicking the button Update.


The maximum number of harmonics in each group is limited to 40. If this limits is exceeded, a specific warning message is displayed in the interface, asking to decrease the number of harmonics in the group(s) exceeding this limit:
Warning ! The number of harmonics exceeds the limit of 40 for some groups. 
Please modify the settings to decrease the number of harmonics, or deactivate some harmonics.

FIGURE 15 illustrates the information displayed when selecting an harmonic from a given group. The following information is displayed:

The Name of the harmonic indicates where it is originated. For example, the name "(-3G3;1G2)" means that the harmonic is a linear combination of the third harmonic from G3 (row 3) and the first harmonic from G2 (row 2), where the symbol ";" should be considered as the operator "+". The frequency of this harmonic will be given by the algebraic sum of the individual frequencies. For example, if 3G3 has 10000 Hz and 1G2 has 15000 Hz, then frequency of  "(-3G3;1G2)" will be -10000+15000 = 5000 Hz.
The Angular Velocity shows the angular velocity of the harmonics.
The Phase Angle depends on the differences between the circumferential angles due to the differences in blade count.
It may happen that harmonics of different origins have the same properties. In this case, the harmonics having the same properties can be merged by using the fixed clocking position. Then, the Number of aliases of a harmonic can be larger than one (alias could be understood as 'name' of the harmonic). For example, a Stator-Rotor-Stator configuration with 36/41/36 blades will have number of aliases greater than 1 if the simulation has only one set of azimuthal positions of the stators (fixed clocking). Indeed, in this case, for one harmonic per perturbation, the harmonic in the central rotor from the second stator has the same frequency and phase angle as the harmonic from the first stator, because the two stators have identical numbers of blades. Therefore, the harmonic from the first stator is an alias of the harmonic from the second stator and only one harmonic will be resolved in the rotor instead of two.
Alias name gives the name of all the harmonics that have the same properties and are merged.
The Base can be:

-999: if the harmonic is a LONE TIME HARMONIC (no clocking impact at the frequency of this harmonic).
(-1)*Harmonic number: if the harmonic is a BASE TIME HARMONIC with associated clocking harmonics.
associated base time harmonic number: if the harmonic is a CLOCKING HARMONIC (note that a particular case is zero, which means that the harmonic is associated with the time-averaged flow).




FIGURE 15 Check properties of each harmonic


The other parameters for the harmonic method in the FINE™/Open GUI can be found in the following menus:
Flow Model



When Harmonic is checked in the Physical Configurations / General Properties page, the turbulence model is set by default to Spalart-Allmaras. The Euler flow and the Laminar flow can also be selected.


Rotating Machinery



In the Physical Configurations / Rotating Machinery page under the tab Rotor/stator, the rotor/ stator connection treatment parameters will be set automatically by the flow solver when the harmonic method is activated. 


Boundary Conditions



The boundary conditions of the NLH computation are non-reflective at the far inlet and far outlet. They are based on 1D non-reflective treatment that computes the flow variables on the boundary as a resulting combination of incoming and outgoing characteristics. The flow at the far inlet and far outlet is assumed to be the time-averaged without the deterministic stress terms.


Initial Solution



It is recommended to use a previous steady flow simulation as the initial solution. This can be done by using the option from file in the Initial Solution page.


Outputs



The Harmonics category in the Computation Control / output page allows to select the harmonic variables for output.
The user can select to output the Real & Imaginary parts of the harmonic variables (such as Harmonic Pressure) and/ or the Amplitude of the harmonic variables (such as Harmonic Pressure Amplitude). 
Note, the reconstruction in time/ space is based on the Real & Imaginary parts of the outputted harmonic variables. If no harmonic variables are outputted, it is not possible to reconstruct the flow in time/ space.
Reconstruction in time/ space
The harmonic simulations can be reconstructed in time or in space in CFView™. For more information, see the CFView user manual.


Control Variables



NLH computations need more CPU time and memory, in comparison with a steady mixing-plane method, due to the additional transport equations associated with each harmonic. If N harmonics of a perturbation are to be modeled, then there are 10N additional transport equations to be solved (5 for the real part and 5 for the imaginary part of the complex amplitude of each harmonic). Then, the ratio R of the required CPU time or memory between the harmonic method and the steady method is:



where  is the number of the grid nodes in the blade row bi (i in range of [1,B]),  is the number of harmonics per perturbation,  is the number of the equations in the steady computation (5 for Euler, Laminar and turbulent flow with the 0-equation turbulence models; 6 for the turbulent flow with the 1-equation turbulence models).
As an approximation, the number of the grid nodes can be assumed to be the same for all the blade rows. The ratio R can be simplified as:



For example, for a 3-harmonic () simulation of a one-stage turbine (B=2) and using the Spalart-Allmaras model (=6), the CPU time is therefore 6 times that of a steady simulation.


Troubleshooting in rotor/ stator interface
Convergence


	
		In case of convergence issues when using the NLH with perfect gas and Merkle preconditioning, the following parameters may be modified:


set preco_NLH_Vunst2Factor_ to 1	
set NLH_HarmoPressureInit_ to (10,10) or (1,1)				



Conservation of flow variables

In some cases, the conservation of the flow variables such as entropy may not be accurately respected through the rotor-stator interface, even with more than 3 harmonics per perturbation. This situation is often due to a strong wake or shock wave on one side of the rotor-stator interface.
Within the NLH method, the conservative variable is decomposed into a time-averaged value and a sum of periodic perturbations, which in turn are decomposed into N harmonics. In some special cases, the perturbation can not be accurately reconstructed by using the decomposed harmonics. The error is depending on the number of the used harmonics.
FIGURE 16 shows how a square wave signal is captured by using a Fourier series (harmonics) and the influence of the number of harmonics on the reconstructed signal.  One can see that the accuracy of the reconstruction increases with the number of harmonics. However, it is impossible to reproduce the vertical line in the signal. This can only be reached if the number of harmonics is infinite.


FIGURE 16 The first four Fourier series approximations for a square wave
As an example, FIGURE 17 shows the iso-radius contours of entropy in a contra rotating propeller using the 1-rank harmonic method. In this case, there is a strong peak in entropy upstream the rotor-stator interface due to the wake of the front blade. To capture such a sharp signal with Fourier series (that is what non-linear harmonics computations do) is indeed very difficult. As shown in the image, the signal is better captured when increasing the number of harmonics. This is in agreement with the theory: increasing the number of harmonics will improve the accuracy, but with higher computation costs.


FIGURE 17 The contours of the entropy at a constant r surface for a contra-rotating propeller

Expert Parameters
All expert parameters are available in the Advanced tab of the Computation Control/Control Variables page. For these parameters the default values are generally the appropriate ones and only have to be changed if the user has specific wishes concerning the fluid modeling.
phys_PrandtlTurb_: allows to define the turbulent Prandtl number. Default value is set to 1.0.
iCondTableClip_:	The thermodynamic tables are generated in a given range of thermodynamic variables. When the thermodynamic variable is not in the given range, the expert parameter iCondTableClip_ can be used to control the computing method of the dependent thermodynamic variable.
0: the dependent thermodynamic variable is extrapolated from the interior field.
1 (default): a clipping value will be used for the dependent thermodynamic variable.
iHStablesNotUsed_:	 When a coarse PHS table is used, the computation may produce a very large error when calculating the total pressure and total temperature from the static pressure and static temperature, and vice versa. Instead, a SHP table will be more accuracy when the pressure from enthalpy and entropy is needed. But it needs a bit more CPU time because an iterative procedure is needed. The expert parameter iHStablesNotUsed_ is used to control which table will be used.
0: the PHS table will be used.
1 (default): the SHP table will be used.
table_cp_Limit_: When the heat capacity is computed by using thermodynamic table, the heat capacity shows a singularity at the critical point, where the value becomes infinite. In order to avoid numerical problems, the parameter table_cp_Limit_ is introduced to clip the heat capacity. By default, the value is set to 100000. If the heat capacity is clipped, a message is given in the .std file, indicating the number of cells for which the clipped value is used.

Demo Cases FINE™/Open with OpenLabs™

FINE™/Open with OpenLabs™
 is packed with a set of 4 demo cases. These are "ready-to-run" public 
 cases which include all the necessary elements to start a 
 calculation and analyze the corresponding solution with a limited number
 of clicks. They must be understood as a complement to tutorials and 
 necessitate basic knowledge in the management of the graphical user 
 interface and execution of templates in CFView™. 
Each
 demo case is completed with a set of illustrative pictures. The macro 
 files (*.py) required to create these pictures are also provided. 
 However, the solution files are not included in the package but can be 
 quickly reproduced through the execution of the related computations, as
 follows: 

open FINE™/Open graphical user interface;
load the desired *.iec file;
import grid file if links to the /_mesh directory are broken. If so, then accept the merging process;
start the calculation process.

The main characteristics of the demo cases are listed here below. Files for demo case 1 and 2 can be downloaded.  Files for all other demo cases are available from the Products page of the Customer Area (www.numeca.be).


Demo Case 1 : Flow through an Automotive Manifold 

Demo Case 2 : Transonic Flow & Temperature Prediction over a High Pressure Turbine Nozzle (2D)

Demo Case 3 : Subsonic Transport Aircraft (DLR-F4)

Demo Case 4 : Flow in a Centrifugal Compressor


Demo Case 1 : Flow through an Automotive Manifold 
  
Introduction
The 3D automotive manifold is a sample case designed for demonstration purposes. It includes three inlet sections with a reference length close to 40 mm and an exit section located at 90 degrees from the inflow sections.
Objective
The objective is to demonstrate the ability of FINE™/Open with OpenLabs™ to simulate the flow in an internal automotive manifold, using high Reynolds number turbulence models. Models tested include Spalart-Allmaras (SA), standard k-epsilon and shear stress transport (SST).
Grid & Numerical Parameters
The grid is generated using HEXPRESS™ with a total of 237,204 cells including the viscous layers. Air modeled as a perfect gas is used for the working fluid. Velocity conditions are selected at the inlets of the manifold and the static pressure is imposed at the exit. A coarse grid initialization strategy with 4 grid levels is used, with a maximum of 500 iterations performed on each grid level. Residuals on the finest grid level reached 5 orders of magnitude reduction within 650 to 725 iterations depending on the turbulence model. Mass flow rate is converging after 650 iterations. Fully convergence of residuals is obtained after 1300 iterations with a computational time of 43 CPU minutes on an Intel E3-1230v6 processor (3.50GHz) running Ubuntu 16.04. Average memory (RAM) required by the flow solver during the calculation is about 420 MB.
A demonstration of the breakthrough convergence algorithm CPU Booster is demonstrated on the case using the Spalart-Allmaras turbulence model. Residuals are reduced by 5 orders of magnitude after 355 iterations. Full convergence of residuals and mass flow rate is reached after 425 iterations. 22 CPU minutes (half the computation time of the original runs) on an Intel E3-1230v6 processor (3.50GHz) processor running Ubuntu 16.04 are required to reach full convergence.
Computations
The project includes four computations named as follows:

SA_ExtWF: calculation using Spalart-Allmaras (SA) turbulence model with extended wall functions;
ke_ExtWF: calculation using k-epsilon turbulence model with extended wall functions;
SST_ExtWF: calculation using shear stress transport (SST) model with extended wall functions;
SA_ExtWF_booster: calculation using SA turbulence model with extended wall functions, and boosted by convergence breakthrough. 

Files
The files for this project are organized as follows:

DemoCase_1.iec: project file, including parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport);
_macros: directory including a few sample macro files (.py) to be run with CFView™.

References
None
Demo Case 2 : Transonic Flow & Temperature Prediction over a High Pressure Turbine Nozzle (2D)
 
Introduction
The MARK II case is a high pressure turbine nozzle guide vane cooled by ten cooling channels.
Objective
The objective is to demonstrate the ability of FINE™/Open with OpenLabs™ to simulate conjugate heat transfer phenomena in a high pressure turbine nozzle guide vane.
Grid & Numerical Parameters
The grid is generated using HEXPRESS™ with a total of 20,213 cells. Two separate domains are created for the fluid and solid (blade) domains. The clustering at the wall for the fluid domain is adapted to have a Y+ value lower than 1. Air modeled as a perfect gas is used for the working fluid. Turbulence is modeled with the Spalart-Allmaras model. The inlet is imposed with an inlet total pressure of 334,000 Pa and a total temperature of 788 K. The outlet pressure is set to 167,000 Pa in order to obtain an isentropic Mach number of 1.04. For each cooling hole, the wall temperature is imposed to a fixed value. The blade is made of ASTM type 310 stainless steel with a thermal conductivity of 18.7 W/m.K. A coarse grid initialization strategy with 4 grid levels is used, with a maximum of 200 iterations performed on each grid level. Convergence on the finest grid level with 5 orders of magnitude reduction in residuals is reached in approximately 980 iterations. This required 5 CPU minutes on an Intel E3-1230v6 processor (3.50GHz) running Ubuntu 16.04. Complete stabilization of the mass flow can be observed after 200 iterations. Average memory (RAM) required by the flow solver during the calculation is about 106 MB.
Computations
The project includes one computation named as follows: 

Spalart-Allmaras: calculation with conjugate heat transfer capabilities included and Spalart-Allmaras turbulence model.

Files
The files  for this project are organized as follows:

DemoCase_2.iec: project file, including parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport);
_data: directory including experimental data for static pressure distribution along the blade; 
_macros: directory including a few sample macro files (.py) to be run with CFView™ .

References
L. Hylton, M. Mihelc, E. Turner, D. Nealy and R. York, "Analytical and Experimental Evaluation of the Heat Transfer Distribution Over Surfaces of Turbine Vanes", NASA CR 168015, Final Report (1983).
Demo Case 3 : Subsonic Transport Aircraft (DLR-F4)
  
Introduction
The DLR-F4 is a simplified subsonic transport type aircraft including only the wing and the fuselage.
Objective
The objective is to demonstrate the ability of FINE™/Open with OpenLabs™ to predict aerodynamic effects in a local flow in M-range 0.75-0.8 with regions of  supersonic flow on the upper wing terminated by weak shock waves, as well as a small separation region close to the trailing edge.
Grid & Numerical Parameters
The grid is entirely generated using HEXPRESS™ with a total of 1,792,132 cells. The clustering at the wall is adapted to have a Y+ value lower than 50. Air modeled as a perfect gas is used for the working fluid. The Spalart-Allmaras turbulence model with extended wall functions is used. On the external boundaries, the Mach number is set to 0.75 and the angle of attack to 0.68 degrees. A static pressure of 100,909.2 Pa, a static temperature of 293 K, and a turbulent viscosity of 1.21e-5 m²/s is also imposed on the external boundaries. A coarse grid initialization strategy with 4 grid levels is used, with a maximum of 200 iterations performed on each grid level. The computation is launched in parallel on 4 processors. Full convergence on the finest grid level with at least 6 orders of magnitude reduction in residuals is reached in about 1600 iterations and 2 CPU hours on an Intel E3-1230v6 processor (3.50GHz) running Ubuntu 16.04. Complete stabilization of the axial thrust is observed after 750 iterations. An average memory (RAM) of 3.5 GB is required by the flow solver during the calculation.
Computations
The project includes one computation named as follows: 

SA_ExtWF: calculation using Spalart-Allmaras (SA) turbulence model with extended wall functions.

Files
The files for this project are organized as follows:

DemoCase_3.iec: project file, including parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport);
_data: directory including experimental data for Cp distribution along the wing (at a specific location Eta=0.331 or y=-0.19447[m]); 
_macros: directory including a few sample macro files (.py) to be run with CFView™.

References
None
Demo Case 4 : Flow in a Centrifugal Compressor
 
Introduction
The case is a centrifugal compressor composed of a multisplitter impeller and a volute.
Objective
The objective is to demonstrate the ability of FINE™/Open with OpenLabs™ to predict
 complex flow in a centrifugal compressor (volute/impeller) configuration, where there exist lots of vortices, such as a passage vortex and a tip leakage vortex.
Grid & Numerical Parameters
The mesh in the volute is generated in HEXPRESS™ while the mesh in the impeller is converted in HEXPRESS™ from an AutoGrid5™ mesh. Only one rotor blade channel is considered. The total number of cells is 1,468,454 and the averaged Y+ on the wall is approximately 1.7. The rotor-stator interface is treated by using the full non-matching mixing plane method. Air modeled as a perfect gas is used. A mass flow rate of 0.2 kg/s and a static temperature of 293 K is imposed at the inlet. A constant static pressure of 200,000 Pa is imposed at the outlet. The impeller rotation speed is 115,000 RPM. The turbulence model selected is the Spalart-Allmaras model. CPU Booster is activated to speed up convergence. A coarse grid initialization strategy with 4 grid levels is used, with a convergence criterion of 6 orders of magnitude on each coarse grid level. The computation is launched in serial mode. Convergence on the fine mesh is reached in a total of about 250 iterations and 80 CPU minutes on an Intel E3-1230v6 processor (3.50GHz) processor running Ubuntu 16.04. Complete stabilization of the mass flow rate and efficiency can be observed after about 210 iterations. An average memory (RAM) of 3 GB is required by the flow solver during the calculation.
Computations
The project includes one computation named as follows: 

SA_CPUbooster: calculation using Spalart-Allmaras (SA) turbulence model and CPU Booster.

Files
The files for this project are organized as follows:

DemoCase_4.iec: project file, including parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport); Autogrid5 files are included in the sub-directory                         _autogrid5 (geomTurbo.xmt_txt, .geomTurbo and .trb);
_macros: directory including a few sample macro files (.py) to be run with CFView™.

References
None

Demo Cases

FINE™/Open with OpenLabs™
 is packed with the following demo cases:
Mesh generation in HEXPRESS™

The full CFD chain from pre-processing to post-processing
Customization using OpenLabs™

Mesh generation in HEXPRESS™/Hybrid

In case FINE™/Open with OpenLabs™ is used in combination with a  HEXPRESS™/Hybrid mesh, the Demo Cases dedicated to HEXPRESS™/Hybrid can be useful as well.
 These are "ready-to-run" public 
 cases which include all the necessary elements to start a 
 calculation and analyze the corresponding solution with a limited number
 of clicks. They can be of help as a complement to tutorials and 
 necessitate basic knowledge in the management of the graphical user 
 interface and execution of templates in CFView™ .
Each
 demo case is completed with a set of illustrative pictures. The macro 
 files (*.py) required to create these pictures are also proposed. 
 The solution files are not included in the package but can be 
 quickly reproduced through the execution of the related computations, as
 follows: 

open FINE™/Open graphical user interface;
load the desired *.iec file;
import grid file if links to /mesh directory are broken. If so, then accept the merging process;
start the calculation process.

All input files for the demo cases can be found in the archive as available from the Products page of the Customer Area (www.numeca.be). For some of the demo cases a direct link  is also available through this documentation platform.

Demo Cases Customization using OpenLabs™

FINE™/Open with OpenLabs™ is packed with a set of 5 OpenLabs™ demo cases. These are "ready-to-run" public cases which include all the necessary elements to start a calculation and analyze the corresponding solution with a limited number of clicks. They must be understood as a complement to tutorials and necessitate basic knowledge in the management of the graphical user interface and execution of OpenLabs™. 
Each demo case is completed with a set of illustrative pictures. The solution files are not included in the package but can be quickly reproduced through the execution of the related computations, as follows: 

open FINE™/Open graphical user interface;
load the desired *.iec file;
import grid file if links to /mesh directory are broken. If so, then accept the merging process;
build library for each block;
start the computation process.

The main characteristics of the demo cases are listed here below. All the demo case files can be downloaded or found in the demo cases archive as available for download from the Products page of the Customer Area (www.numeca.be).


Demo Case 1: Diffusion of a Pollutant in a Room

Demo Case 2: Unsteady Turbine Blade simulation due to Wake Passing

Demo Case 3: Combustion Zimont Model

Demo Case 4: Electric Field of Plasma

Demo Case 5: Porous Media


Demo Case 1: Diffusion of a Pollutant in a Room
 
Introduction
The case simulates the diffusion of a pollutant in a room. The case includes two inlets: one with cold air simulating air-conditioning and one with warm air simulating door. One outlet simulates window. The pollutant enters the room from air-conditioning.
Objective
The objective is to demonstrate the ability of OpenLabs™ to define a convection-diffusion equation (PDE), to add source term in the momentum equation and to integrate a quantity over a boundary.
Grid & Numerical Parameters
The mesh is generated in HEXPRESS™  with viscous layer. The total cell number is 68,330 and the averaged Y+ of the first inner cell is about 20.
Air modeled as incompressible fluid is considered. The fluid properties have been modified, so that the solutal Rayleigh number is equivalent to the thermal Rayleigh number. The inlet temperature of air-conditioning is set to 300K and the inlet temperature of door is set to 320K. The static pressure is imposed at outlet with a value of 101,142.6Pa.
CPU Booster is activated. A coarse grid initialization strategy (4 grid levels on the finest mesh) is used. The computation is launched in serial mode. Convergence on the fine mesh is reached in about 300 iterations. The CPU time is about 14 minutes  on Intel(R) Core(TM) i7-6700HQ @2.60GHz running Windows 10.  An average memory (RAM) of 125 Mb is required by the flow solver during the calculation.
OpenLabs™
Here, OpenLabs™ will solve a natural convection problem, which is driven by both temperature difference (already in FINE™/Open) and concentration difference.
The distribution of the pollutant can be solved by the following transport equation based on the mass fraction Y of the pollutant:



For the inlet boundary condition, Y=1 at the cold air inlet and Y=0 at the warm air inlet.
The solutal buoyancy source term will be added to the momentum equation. The solutal buoyancy source term can be expressed as:



Where the constants:
the Lewis number Le=(κcp)/(ρD)=1;
the solutal expansion coefficient βS=0.14372;
the Reference mass fraction Yref=0;
the turbulent Prandtl number δY=1.


Computations
The project includes one computation named as follows:

Ra12: calculation with OpenLabs™.

Files
Files are organized as follows:

DemoCase_1.iec: project file, including OpenLabs™ resource, parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg and .fnmb);
_macros: directory including few sample macro files (.py) to be run with CFView™.

References
A.A. Mohamad, R. Bennacer. Double diffusion, natural convection in an enclosure filled with saturated porous medium subjected to cross gradients; stably stratified fluid. International Journal of Heat and Mass Transfer 45 (2002) 3725""3740, 2002.
Demo Case 2: Unsteady Turbine Blade simulation due to Wake Passing
 
Introduction
The case simulates the effect of upstream weak of the vane on the blade. The blade of the first stage of GE-E³ engine is used here.
Objective
The objective is to demonstrate the ability of OpenLabs™ to modify a boundary condition either using an expression or a profile. 
Grid & Numerical Parameters
The 2D mesh is generated using AutoGrid5™  with a total number of cells of 10,176.
The computation is set as unsteady, non-rotational, and the relative values are imposed at the inlet. Air (perfect gas) is selected. The Spalart-Allmaras turbulence model is used. The total quantities and velocity direction are imposed at the inlet, with the value of total pressure 223,331 Pa, total temperature 606.3 K, and velocity direction [Vr/|V| Vθ/|V| Vz/|V|] =[0 0.53 0.848].
CPU Booster is activated. A coarse grid initialization strategy (4 grid levels on the finest mesh) is used. A steady initialization is performed with 50 iterations.
The physical time step is 1e-5 s, The convergence criteria of the inner-iteration is set to 20/-6. 200 physical time-steps are computed. The computation is launched in serial mode, which need about 18 minutes CPU time on Intel(R) Core(TM) i7-6700HQ @2.60GHz running Windows 10. An average memory (RAM) of 75 MB is required by the flow solver during the computation.
OpenLabs™
The time-dependent relative total pressure is imposed at the blade inlet, by using the following expression,



where, n is the number of blades, t is the physical time, θ is the tangential coordinate, Pt-bgis the background relative total pressure, and τ is the time period of one wake passage being computed by:



The computation parameters are:

n set to 76,
Pt-bgset to 223,331 Pa,
Pout (static pressure at outlet) set to 142,675 Pa,
ω (rotation speed) set to 8,283 RPM.

Two simulations are performed to define the unsteady inlet boundary: one with an expression and the second one with a profile.
 
Computations
The project includes two computations named as follows:

UDF_Modif_Inlet_unsteadyPt: calculation using unsteady inlet boundary defined as an expression;
UDFProfile_Modif_Inlet_unsteadyPt: calculation using unsteady inlet boundary defined as a profile.

Files
Files are organized as follows:

DemoCase2.iec: project file, including parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport).

References
Ali A. Ameri, David L. Rigby, Erlendur Steinthorsson, et al. Unsteady turbine blade and tip heat transfer due to wake passing, NASA/TM-2007-214942, 2007.
Demo Case 3: Combustion Zimont Model
 
Introduction
The case implements the premixed combustion model, turbulent flame speed closure (TFC) model based on a laminar flow. A simple jet is computed.
Objective
The objective is to demonstrate the ability of OpenLabs™ to modify the equation of state and transport property, and to add a convection-diffusion-source equation (PDE).
Grid & Numerical Parameters
A 2D mesh is generated in IGG™  without viscous layer, the angle of the sector is 5 degrees. The total  number of cells is 17,920.
Air(Perfect) is selected for the equation of state database, which will be modified by OpenLabs™. The static temperature at the inlet is 293 K, which will be overwritten by the inlet boundary condition of progress variable. The static pressure is imposed at the outlet with a value of 101,300 Pa. The following inlet velocity is imposed.


CPU Booster is activated. A coarse grid initialization strategy (4 grid levels on the finest mesh) is used. The computation is launched in serial mode. Convergence on the fine mesh is reached in about 420 iterations and 9 minutes CPU time on Intel(R) Core(TM) i7-6700HQ @2.60GHz running Windows 10.  An average memory (RAM) of 188 MB is required by the flow solver during the calculation.
OpenLabs™
The TFC approach models premixed flames by tracking the position of the flame-front by means of a normalized progress variable c, which is evaluated using the following convection-diffusion-source equation (for laminar flow),



in which, ρ is the density,  is the velocity vector, D is the diffusion coefficient computed as D=ν/sc, where ν is the kinematic viscosity and sc is the Schmidt number. The combustion source term is modeled by the Zimont model,



where, ρu is the unburnt density, SL is the laminar flame speed. A Dirichlet boundary condition is imposed for the progress variable at the inlet, where the jet flame is assumed as progressed (c=1.0). The state of the mixture (burnt or unburnt) is expressed in terms of the normalized progress variable, 



where Tu is the unburnt premixed gas temperature and Tad  is the adiabatic flame temperature. 
The computation parameters are:

sc set to 0.7,
SL set to 0.1,
ρu set to 1.2 kg/m³,
Tu set to 293 K,
Tad set to 1665 K,
υ set to 1.57e-5 m²/s,
Pr set to 0.72.

The equation of state is changed based on the perfect gas framework, and the combustion temperature is computed by using the progress variable. The Sutherland viscosity law is used, in which the temperature is also modified by using this combustion temperature.



Computations

The project includes one computation named as follows:

Zimont: calculation using combustion Zimont model.

Files
Files are organized as follows:

DemoCase3.iec: project file, including parameters of the computations and link to the mesh;
_mesh        : directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport).

References
FINE™/Open User Manual

Demo Case 4: Electric Field of Plasma



Introduction
The plasma actuator can be used in flow control. It is made up of two electrodes separated by a dielectric material. A voltage is applied to the electrodes which causes the air to ionize in the vicinity of the electrodes. This air results in a body force acting on the flow. This force will modify the velocity components and can delay the separation of the flow around the airfoil. This case computes the electric field of a plasma actuator in a square. The electric field is not coupled with the flow.
Objective
The objective is to demonstrate the ability of OpenLabs™ to define a Poisson's equation.
Grid & Numerical Parameters
The mesh is generated in HEXPRESS™  without viscous layer. The total cell number is 223,095. Both blocks are set as fluid blocks. Air (perfect gas) is selected and a laminar flow is computed (the flow solution will not be used in this example). The inlet temperature is set as 293 K and the inlet velocity is 100 m/s. The static pressure is imposed at the outlet with a value of 101,325 Pa.
A coarse grid initialization strategy (4 grid levels on the finest mesh) is used. The computation is launched in serial mode. Convergence on the fine mesh is reached in about 1000 iterations and 1h 30m CPU on  Intel(R) Core(TM) i7-6700HQ @2.60GHz running Windows 10.  An average memory (RAM) of 1155 MB is required by the flow solver during the calculation.
OpenLabs
The following Poisson's equations of the electric potential are solved by using OpenLabs™,



with the boundary conditions, φ=1.0 on the exposed electrode, φ=0.0 on the covered electrode , and =0.0 at the outer boundaries. In which, ε is the electrical permittivity, with the value of 1.0 and 2.7 in two blocks respectively.
 
Computations
The project includes one computation named as follows: 

potential: calculation of the electric field of a plasma actuator in a square.

Files
Files are organized as follows:

DemoCase_4.iec: project file, including parameters of the computations and link to the mesh;
_mesh: directory including mesh files (.bcs, .dom, .hex, .igg, .fnmb, .dtw, .rep and .qualityReport).

References
Y. B. Suzen , P. G. Huang , et.al. Numerical Simulations of Plasma Based Flow Control Applications. AIAA 2005-4633. 35th Fluid Dynamics Conference and Exhibit. June 6-9, 2005, Toronto, Ontario
Demo Case 5: Porous Media
Introduction
The case implements the Darcy homogenous porous media model using OpenLabs™.  The pressure drop along the porous media is known from physical characteristics of the media:
 
Objective
The objective is to use OpenLabs™ to define a porous media model using source terms.
Grid & Numerical Parameters
The configuration is 0.25 [m] long and 0.1 [m] high and the porosity is fixed to 10 [kg/(m³.s)]. The velocity at the inlet is fixed to 2 [m/s]. Therefore a pressure drop of 5 [Pa] is expected. The mesh is generated in IGG™  without viscous layer. The total cell number is 1000.
The block is set as fluid block. Air (perfect gas) is selected and a laminar flow with preconditioning is computed in full-double-precision mode. The inlet temperature is set as 293 [K] and the inlet velocity is 2 [m/s]. The static pressure is imposed at the outlet with a value of 100,000 [Pa].
OpenLabs™
In OpenLabs™ there are two possibilities to use the Darcy porous media model with homogeneous permeability as shown in the two computations of this demo case.
Creation of the Porous Media model from scratch
In the first computation named "Darcy_Homogeneous", the porous media model is defined from scratch. The porous media model in the FINE GUI is deactivated and the model is entirely defined in OpenLabs™. This is important as having both the model activated in the GUI while also adding new source terms in the Lab, would result in the undesired result of adding two times the same source term to the Navier-Stokes equations. 
The Lab is shown here: 
 
The keyword AddToViscous set to NO is optional and ensures that the source term is updated at each Runge-Kutta stage.
The results of the calculation are shown below with a pressure graph along the media. One can check that the pressure is linear. The pressure is fixed at the outlet so this quantity should change up to the inlet during the convergence process. One also can check that the pressure drop is 5 [Pa] which is the expected value. 




Easy modification of an existing porous media model
Instead of writing a Lab with a porous media model from scratch, it is also possible to take benefit of the models already available through the FINE™/Open GUI. This method is illustrated in the computation "Darcy_Homogeneous_Analysis".

In the FINE™/Open GUI select in the Physical Configuration/General Properties page the Porous media option. Select in the Optional Models/Porous Media page the Darcy law with the User defined (homogeneous) option. Keep the default value for the K' coefficient for now, it will be defined in OpenLabs™. No flow direction is specified.
 The flow direction as it can be defined in the GUI, is not accessible for modification in OpenLabs™. Nonetheless, if a flow direction is defined through the GUI, it will be taken into account even when making modifications to the constant(s) or source terms of the porous media model in OpenLabs™.

In the OpenLabs/Resource Manager, Tools/Analyze in detail menu can be used to get access to the definition of the porous media model as just selected through the GUI.
For example, under the CONSTANTS one can find:
@darcy_Kprim_ = 0 
The value of the constant corresponds to the default of the Porous media model in the GUI. It is redefined in OpenLabs™ by copying the definition of this constant to the resource area and putting the desired value:
=>CONSTANTS
 @darcy_Kprim_ = 10.0
In this example the value of "Kprim" is still a fixed number. But using OpenLabs™ it is now possible to define the permeability in function e.g. of other constants. The value defined in OpenLabs™ will overwrite the default value if the same name "darcy_Kprim_" is kept. 
In this example the permeability is still defined by a constant and could be redefined by a function of other constants. In case we want to define the permeability as a function of e.g. the temperature, it is no longer a constant and therefore should be defined elsewhere. In that case the name "darcy_Kprim_" can not be used as it is already reserved for the constant in the solver. A new name needs to be given in such case to the variable and the same new name should then be used in the source terms.
Under the =>SOURCETERMS in the detailed analysis the source terms added to the momentum and energy equations can be found:
@ SOURCE: PorousMedia
->EXPRESSION(MomentumXEquation): - Vx * darcy_Kprim_
->EXPRESSION(MomentumYEquation): - Vy * darcy_Kprim_
->EXPRESSION(MomentumZEquation): - Vz * darcy_Kprim_
->EXPRESSION(EnergyEquation): - darcy_Kprim_ * (Vx*Vx + Vy*Vy + Vz*Vz)
It is not necessary to copy this definition of the source terms in the Lab if it is not changed and e.g. only the constant defining the permeability needs to be modified. On the other hand, if the user desires to modify the source terms, a simple copy-paste can be made to the resource area to allow modification of any part of it. As long as the same name of the source terms ("PorousMedia") is kept, the new definition will then overwrite the one activated through the FINE™/Open GUI. 
If the entire definition of the porous media model (the constant and the source terms) is copied into the Lab, it is no longer necessary to keep the porous media model activated through the GUI Only when the Lab contains e.g. just the modification of the constant, it is important to keep the porous media model selected through the GUI. This allows to keep the Lab very compact but it may be good to inform other users of your Lab through the header of the Lab about this need to have the porous media model set to e.g. Darcy with homogeneous permeability in the GUI. It is also possible to redefine in a Lab all constants used in the various porous media models. In that case the Lab will work for any of the available models in the GUI as the constants of the selected model will be used from the Lab and the other constants in the Lab will not have any effect.
The result of using this Lab is as expected the same as the one of the first computation ("Darcy_Homogeneous") as long as the same permeability is used and the source terms are copied from the detailed analysis and kept unaltered.

Tutorials


The tutorials for FINE™/Open with OpenLabs™ provide detailed step-by-step instructions for the entire simulation process. Additional tutorials of HEXPRESS™ and the tutorials of HEXPRESS™/Hybrid allow a further detailed insight into the mesh generation process. Most of the tutorials are designed so as to limit use of computational resources but some of them may require a significant amount of computational time assuming they are executed on the finest mesh level. 

Where to Find the Files Used in the Tutorials?
Most of the tutorials starts from mesh generation and uses an existing geometry. The appropriate files (and any other relevant files used in the tutorial) can be downloaded from the corresponding links: 

download Beginner level files
download Advanced level files
 the Expert level files can be found in a separate tutorials archive as available from the Products page of the Customer Area (www.numeca.be).
download Customization with OpenLabs™ level files

Some of the project files (mesh and project, excluding solution files) can also be found in the demo cases package dedicated to ready-to-run demonstration cases and presented in the Demo Cases section. This allows to quickly start a calculation and observe the behavior of FINE™/Open with OpenLabs™, without necessarily going through all the steps of the tutorials.
Conventions Used in the Tutorials
Several conventions are used in the tutorials to facilitate your learning process.
Following a short introduction, most of the tutorials are divided into 3 sections, respectively related to mesh generation, settings and calculation, and post-treatment.
Inputs required to execute the tutorials are most often restricted to the geometry, either in a ".dom" or CAD related format, and profiles of boundary conditions.
The sequence of actions to be executed are described through a numbered step-by-step approach.
Additional insight about some specific actions and/ or features is frequently added to further illustrate the tutorial. This information is for the purpose of clarity and completeness, and should not be executed. It appears as a note with a light blue background.
The calculations executed to illustrate the behavior of the flow solver include a reasonable number of grid points, so as to limit the computational resources required to complete the tutorials. As a consequence, most of the underlying flow solutions must be considered as qualitative. Additional mesh refinement may be required in some circumstances so as to obtain a more quantitative picture.
For more information and troubleshooting:

consult the forum in NUMECA's Customer Area.
or contact NUMECA local sales or support office (for active maintenance plans only). 

To help to find a solution within the shortest delays, please provide a detailed description of the observed behavior and performed analysis.

Flow Settings
A step by step approach is proposed in the following lines. It aims at driving you through the various steps that need to be executed to set up and start the computation.



Set solver precision

Manage Computations

Set Physical Configuration

Boundary Conditions

Initial Solution

Numerical Parameters

Output Parameters

Control Variables

Launching Mode

Save Project & Computation

Start & Stop Computation

Monitoring


Set solver precision
59. In Project/Preferences... select Full-double-precision mode and click on Ok.


Manage Computations
60. In the Computations menu, right-click on the computation name and select Rename.
61. Rename "computation_1" as <SA_EXT_angle-0.68> <Enter> (as a reference to the turbulence model: "Spalart-Allmaras Extended Wall Function" and the angle of attack used in this tutorial).
 
In the Computations menu, the list of computations are shown. It is possible to Rename, creates a new one by duplicating the highlighted one (New button) or just delete the computation by clicking on Delete.
Set Physical Configuration
62. In the Physical Configuration menu, double left-click on General Properties menu.
63. Keep Steady mode and Fluid block active for the domain "3".
64. Click on Ok to validate.


65. In the Physical Configuration menu, double left-click on Fluid Model.
66. In the Edit/Select fluid section, click on Select....
67. Click on New fluid... to create a new fluid.


68. Set Fluid name as <Air> - Select Perfect gas - Click on Next>>.


69. Impose fluid properties as defined in figure below.


70. Click on Finish to select and add new fluid in database.
71. Click on Ok to confirm.
72. Click on Close.
73. In the Physical Configuration menu, double left-click on Flow Model.
74. Select Spalart-Allmaras (Extended Wall Function) as Turbulence model.
75. Change the reference parameters:

Set Reference length as <0.1412> <Enter> [m];
Set Reference velocity as <257.25> <Enter> [m/s].



76. Click on Ok to confirm.
Boundary Conditions
77. In the Boundary Conditions menu, double left-click on Boundary Conditions.
78. Select all solid patches (left-click on first one and left-click + <Shift> on last one) under the SOLID tab.
79. Keep Adiabatic for all solid patches and activate Compute force and torque.


80. Under EXTERNAL tab, select all patches (left-click on first one and left-click + <Shift> on last one). Select Mach Number and Velocity Angle as external boundary conditions for all the patches.
81. Impose same boundary condition on all patches:

Set Static Pressure to <100909.2> <Enter> [Pa],
Set Static Temperature to <293> <Enter> [K],
Set Mach number to <0.75> <Enter> (corresponds to a free stream velocity around 257.25 [m/s]),
Set arctg(Vy/Vx) to <0> <Enter> [rad] and arctg(Vz/Vx) to <-0.0118682> <Enter> [rad] (corresponds to an angle of attack of -0.68 [degrees]),
Set Turbulent Viscosity to <1.21e-5> <Enter> [m²/s].

 
82. Click Ok to close the window.
Initial Solution
83. In the Initial Solution menu, double left-click on Initial Solution.
84. Keep Constant values and Coordinate system as Cartesian.
85. Set the values accordingly:

Pressure = <100909.2> <Enter> [Pa],
Temperature = <293> <Enter> [K],
Vx = <257.23> <Enter> [m/s],
Vy = <0.0> <Enter> [m/s],
Vz = <-3.05> <Enter> [m/s],
Nut/Nu = <50> <Enter> .



86. Click on Ok to close the window.
Numerical Parameters
87. In the Numerical Parameters menu, double left-click on General Parameters.
88. Check if the Number of grid(s) is set to 4.
The flow solver is based on an explicit time integration technique, which is accelerated by means of dedicated multi-grid methods. To this end, several levels of intermediate grids must be generated starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
89. Keep Coarse grid initialization active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be significantly reduced by activating the coarse grid initialization process. In that case, the simulation starts on the coarsest grid level available, leading to fast convergence. Once it is done, the flow solver automatically interpolates the current flow solution on the intermediate levels before the iterative process is restarted. A similar process repeats until the expected finest grid level is achieved. The iterative process stop when the convergence criteria is reached or the maximum number of iterations is exceeded.
90. Keep the defaults and click on Ok.


91. In the Numerical Parameters menu, double left-click on Numerical Schemes.
92. Keep the default values for the domain "3".


The CFL number drives the pseudo-time step selected to reach a steady state solution using the time-marching method integrated in the flow solver. In combination with the 4-steps Runge-Kutta integration scheme included in the flow solver, it has a theoretical stability limit close to 2.8. However, the additional implicit smoothing scheme can increase this value slightly, which justifies the default value of 3. The default value for CFL number is adequate in most cases, but can be decreased in some circumstances, in particular at off-design conditions or for CHT computations, for the solid block.
93. Click on Ok.
Output Parameters
94. In the Computation Control menu, double left-click on Outputs menu.
95. Select External flow outputs in Flow configuration area.


By default depending of the Flow configuration selected, a list of quantities is defined to be computed in the flow solver. The list can be manually adapted by selecting a quantity in a category and clicking on the Add --> and <-- Remove buttons.
96. Select Turbulence under Categories. Select Y+ and Wall Distance and click on Add --> button.
97. Go to External flow tab and adapt Lift direction to <0.01186 0 0.99993> and Drag direction to <0.99993 0 -0.01186>.


98. Click on Ok.
Control Variables
99. In the Computation Control menu, double left-click on Control Variables menu.
100. Set the Number of iterations to <850> <Enter>.
101. Set the Convergence criteria to <-7> <Enter>.
102. Save the solution at every <200> <Enter> iterations.


103. Click on Ok to confirm.
Launching Mode
104. In the Computation Control menu, double left-click on Launching Mode menu.
105. Select Parallel in Launching mode area.
106. Increase the Number of partitions to <4> <Enter>.


107. Click on Ok to confirm.
On Windows the account needs to be configured to be able to run parallel computations (see: Windows User Configuration).
Save Project & Computation
108. Click on Save Project button to save the project.
109. Click on Save Selected 'Run' files button to save the computation.


Start & Stop Computation
110. Click on Start Solver button to launch the computation dialog box to set-up parallel settings is appearing.


111. Click on Parallel settings... button to adapt if needed the host of each partition.




112. Click on Ok twice to confirm and start the process in parallel. 
To save and stop a computation while running, the button Suspend Solver should be pressed. However, to stop the computation without saving, the Kill Solver button should be used.


The pop up Task manager window allows following the convergence history of the computation.


Monitoring
Evolution of averaged residuals on the entire domain can be observed during the convergence process (Steering icon). Similarly, the evolution of the mass flow balance (in/out for internal flow) and/or global quantities (lift, drag and momentum on solid walls selected in the boundary conditions page) can be performed in the steering. Local and global quantities may also be added for follow up during the convergence process. However, their representation in the graphical area will be effective only once they will be added, and the history will not be available.




To check the convergence of the computation, NUMECA recommends observing the evolution of multiple criteria which includes:

an adequate decrease in residuals (minimum 3 orders of magnitude);
complete stabilization of global performances;
stabilization of mass flow in/out (for internal flow), with satisfactory correspondence (usually less than 0.5% difference between in/out). To do so, select the inlet and outlet mass flow at once. An information about the difference is automatically computed.

The examination of residuals per block for a given primitive variable or the comparison of convergence histories from different computations, can be achieved by accessing the Monitor tool. The tool is included in the package and can be accessed via the icon bar.




The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated within the environment and includes numerous tools.
113. To access CFView™ from the FINE™ graphical user interface, press the CFView™ icon ().
You are now entering to the CFView™ interface and ready to proceed with the Post Processing of the results!

TUTORIAL 4. DLR-F4 Wing Body

The resolution of computational fluid dynamics (CFD) problems involves three main steps:

Spatial discretization of the flow equations,
Flow computation,
Visualization of the results.

For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in internal and external configurations can be simulated. The unstructured CFD package consists of the following tools:

HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to automatically generate meshes for the discretization of complex 2D and 3D geometries,
HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
CFView™ is a highly interactive flow visualization and post-processing software,
FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish all steps, from grid generation to flow visualization.

This tutorial is particularly adapted to a 3D internal application. It makes use of FINE™/Open with OpenLabs™ including HEXPRESS™ and CFView™.
The following steps will be discussed:

Use HEXPRESS™ user interface,
Import an existing domain,
Visualize a mesh,
Progress in the mesh wizard to generate the mesh,
Control the quality of the mesh,
Set up a computation in FINE™/Open interface,
Start/stop the computation,
Visualize the results with CFView™.



Introduction

Prerequisites

Problem Description

Preparation


Introduction
Prerequisites
This tutorial does not require any particular prerequisite but it is strongly recommended for beginners to perform the Beginner level tutorials.
Problem Description
In order to study the flow around a subsonic transport type aircraft, the 3D geometry of the DLR-F4 test case is here considered. The objective is to demonstrate the ability of FINE™/Open to predict aerodynamic effects in a local flow in M-range 0.75-0.8 with supersonic flows regions on upper wing terminated by weak shock waves as well as a small separation close to the trailing edge.
The geometric configuration is shown in the following figure.


(picture from A selection of Experimental Test Cases for the Validation of CFD Codes - AGARD ADISORY REPORT NO 303, Volume II)
Air, modeled as a perfect gas with a constant kinematic viscosity of 1.21e-5 m²/s, is considered at 293K and at density of 1.2kg/m3. Static-to-static pressure conditions are imposed as external conditions (100909.2Pa), with a speed of 257.25m/s. The Mach number is then approximately 0.75 and the Reynolds number, determined using the velocity and the chord-length, is about 3e6.
Preparation

Start FINE™/Open v7.2:


For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the following command line:
fine -niversion open72 -print 
For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.






Click on the icon Creating a mesh under Create a new project to create a new project and a new mesh. Click on Ok.
Select your directory of choice to store the project.
Enter the project name in the dialog box as <dlr-f4.iec> and click on Save or Ok.

FINE™/Open will automatically create a project folder called "dlr-f4" which will contain the project file (".iec") and a folder "_mesh" where the mesh will be stored. Later, computation folders will appear inside the project folder. It is strongly advised to keep this file structure all along the project.

Click on Yes to start HEXPRESS™ unstructured mesh generator.



You are now ready to start the Mesh Generation process and mesh the DLR-F4 aircraft!

Post Processing

                                                A step by step approach is proposed in the following lines. It aims at driving you through the various steps that need to be executed from reading the solution to the extraction of the main results. CFView™ automatically opens the file ".run" file associated with the active computation.



Select Surfaces/Quantities

Representation on Solid Patches

Representation on Cutting Plane (Vector Lines)

Representation on a Cartesian Plot (Validation Data)


Select Surfaces/Quantities
114. In the Surfaces section, all solid surfaces are selected by default.
115. Go to Quantities section in the Quick Access Pad.
116. Double left-click on the Wall Distance.


All quantities selected in FINE™ graphical user interface are transferred to CFView™. However, additional derived output can also be accessed directly from the visualization and post-treatment tool, including vector components, gradients, divergence and curl of selected quantities. New quantities, defined from existing quantities combined by regular operations (arithmetic functions, trigonometric functions, logarithmic functions,...) can be created with the Quantity/Field Data/Define New Quantity... menu.
117. Check full range of the Wall Distance quantity in Information Area.



118. To limit the range to the selected surfaces (all "solid" surfaces), click on the Colormap Optimum Range icon () and check that the range is going from 0 to 0 on solid walls.



When selecting all "solid" surfaces (when not involved in FNMB connections) the Wall Distance should be equal to 0. If not that means that the wall distance computation in flow solver is incorrect and should be corrected (more details in User Manual).
119. Go to Quantities section in the Quick Access Pad.
120. Double left-click on the Y+.
121. Check range (limited to "solid" surfaces with  icon) of the Y+ quantity in Information Area to check that the imposed first cell size is in agreement with the turbulence model used. In this tutorial, the averaged value of Y+ is about 29 and in agreement with the "Spalart-Allmaras Extended Wall Function" turbulence  model used. 



122. Go to Quantities section in the Quick Access Pad.
123. Double left-click on the Static Pressure.
Once the candidate quantity for visualization is selected, a representation mode should also be selected. Representation is typically executed in the form of color contours (smoothed or stripped) and/or isolines. CFView™ also includes the possibility to interrogate the flow field locally ("local value") and create 1D Cartesian plots. Advanced capabilities involving curve and/or surface integration can also be accessed.
Representation on Solid Patches
124. Click on Representations/Contours & Iso Values section and then on Strip Contour icon to display the selected quantity.


125. Click on the icon Isolines.
126. Increase the number to <21> <Enter> isolines.
127. Select Uniform.
128. Click on Apply and then on Close.
129. Select Geometry/Repetition on/off menu to plot the whole plane.




Representation on Cutting Plane (Vector Lines)
130. Click on Update/Delete/All to delete all previous manipulations in the Graphics area.
131. Select Geometry/Repetition on/off menu to hide the repetition.
132. Under Representations/Grid section, click on Render Gouraud icon to activate the shading on solid surfaces.
133. Click on Geometry/Create Cutting plane... menu.
134. Enter the X, Y, Z values for Point and Normal as shown on the following figure.
135. Select Geometry and click on Apply to pre-visualize the cutting plane.
136. Click on Save to add this cutting plane to the Surfaces section in Quick Access Pad, that will be activated by default.


137. Click on Close.
138. In Surfaces section, select "CUT1" by left-click, right-click and Select.
139. Double left-click on the quantity Vxyz (Velocity).
140. Click on Representations/Vector Lines section.
141. Click on Vector Lines Parameters icon.


142. Under the tab General, change the Direction to both, Representation to line, Mode to surface and the Color to Uniform.
143. Click on Apply button to validate and then on Close.
144. Click on the icon Vector Lines from Section.
145. Keep "5" in the keyboard input area to draw 5 vector lines per section.
146. With the mouse, draw a line (left-click and drag) on the cutting plane close to the plane body and wing to plot the vortex behind the tip of the wing.
147. Select Geometry/Repetition on/off menu to plot the whole plane.


Representation on a Cartesian Plot (Validation Data)
The objective is to compare computational results to experimental data (pressure coefficient (Cp) along the wing at a specific location Eta = 0.331 or y = -0.19447 m).


148. Click on Quantity/Field Data/Define New Quantity... to open the dialog box allowing to create a new quantity based on existing ones.
149. Keep Scalar and Field active under Quantity Type.
150. Set Name as <Cp>.
151. Set Definition as <(100909.2-Static Pressure)/(0.5*1.2*257.25*257.25)>.



The pressure coefficient Cp is defined as:



where p is the static pressure,  is the freestream pressure (100909.2 Pa),  is the freestream fluid density (1.2 kg/m³) and  is the freestream velocity of the fluid or the velocity of the body through the fluid (257.25 m/s).

152. Click on Apply to add the new quantity.
153. Click on Close.
154. In Surfaces section (Quick Access Pad), select all solid patches:

left-click on first solid patch;
left-click+<Shift> on last solid patch;
right-click and Select.

155. Click on Z-projection icon in the viewing buttons.
156. Click on Representations/Plots & Values section.
157. Click on Section button.
158. Set X1 Y1 Z1 X2 Y2 Z2 to <0 -0.19447 0 0.5 -0.19447 0> in the keyboard input area.
159. Left-click on Cartesian plot (highlighted with red border).
160. Left-click on X-axis.
161. Right-click and select Function of X.
162. Right-click and select Fit Range.
163. Left-click on one of the curves.
164. Right-click and select Curve Type to whole section.
165. Under Marker tab, deactivate Visible, Apply and Close.
166. Click on File/Load Validation Data... menu and open "dlrf4_onera_ExpData.dat" (contains experimental data of Cp at Eta = 0.331) available in the "FINE-Open_Advanced/Tutorial_1" folder of the tutorial package (download Advanced tutorial archive).
167. Click on Quantity/Validation Data/dlrf4_onera_ExpData menu.
168. Accept the comparison (yes): markers for experimental data and curve for computational results. 


169. Select File/Print... menu.
170. Click on Ok after defining the picture settings (more details in User Manual).
171. Click on Ok after selecting the location to save and the name of the picture.
172. Select File/Quit CFView to leave CFView™  session.

Mesh Generation


HEXPRESS™ graphical user interface allows to visualize the geometry and mesh of the internal or external test case in a graphics area. The access to main menu and controls is proposed through a menu bar and a quick access pad, and is completed with a tool/icon bar and a control area (including the keyboard input area).

Open Existing Domain File

Set Boundary Conditions

Mesh Wizard : Initial Mesh

Mesh Wizard : Adaptation Step

Mesh Wizard : Snapping Step

Mesh Wizard : Optimization Step

Mesh Wizard: Viscous Layers Insertion Step

Save Mesh


Open Existing Domain File
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be progressively defined. That is why the tutorial starts from the domain file ".dom". It should be noticed that the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL), import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS dialog box.


2. Locate and select "dlrf4.dom" in the dialog box (download Advanced tutorial archive)  and click on Open or Ok.
Set Boundary Conditions

                                                            3. Go to the Grid/Boundary Conditions... menu or click on Boundary Conditions icon () in the Tool bar and set the boundary conditions using the Set face type button :

set "exterior_#" for 1 to 5 as external ("EXT");
set "mirror" as mirror ("MIR");
keep "facet", "extrados", "tail", "body" and "intrados" as solid ("SOL").



4. Close the dialog box.

Mesh Wizard : Initial Mesh
5. Left-click the check box for Initial mesh in Mesh Wizard to activate the step. The corresponding step is accessible for users at once. The same behavior is applied for the following steps in the Mesh Wizard.
6. Click on Initial mesh and the Initial mesh parameters dialog box appears.
7. In Set the number of divisions along cartesian axis section, impose Nb of cells to <100,000>.
8. Click on Auto button.



By using the Auto button, HEXPRESS™ computes the required number of cells in each direction to get an isotropic mesh. The total number of cells may then vary (in this case the number of cells is adapted from 100,000 to 97,556).
9. Click on OK and on Step button from the Mesh Wizard to create the initial mesh with 97,556 cells.


Number of cells in the initial mesh can be increased in order to impose a smaller size to the biggest cell that will be included in the computational domain.
Mesh Wizard : Adaptation Step

This mesh generation step is probably the most important in terms of user interaction in HEXPRESS™. Indeed, the parameters selection in this action directly dictates the computed mesh obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement and the trimming.
During the first one, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry dependent criteria. With the second step, it removes cells intersecting the geometry or located outside the computational domain.

10. Left-click the check box for Adapt to geometry in Mesh Wizard to activate the step.
11. Click on Adapt to geometry and the Refinement and trimming parameters dialog box appears.
12. Under Global tab, set the Maximum number of refinements to <10>.



In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.


In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.


The adaptation process successively bisects the cells flagged for refinement in one or several different directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive refinements. This may result in an exponential growth of the total number of cells in the mesh, even though the refinement may be confined to some areas of the computational domain. To bound the number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification may therefore alter the success of the meshing process. More details are available in the User Manual.

13. Left-click on Curve refinement tab.

The refinement process is defined by three classes of criteria: curve, surface and volume criteria. Surface criterion is considering cells which are intersecting surfaces as candidates for refinement. Three criteria are implemented and are respectively based on:

a proximity between surfaces (Distance),
a surface curvature measurement (Curvature),
a specification of cell target sizes on the surfaces (Target cell sizes).


14. Use left-click and <Ctrl> to select in the curve (edge) list "Curve 17", "Curve 19", "Curve 48".
15. Click on Active to access the refinement parameters.
16. Set the Max nb of refinements to <8>.
17. Select the Target cell sizes criterion and keep the default values.



The Maximum number of refinements per surface ultimately controls the refinement of cells intersecting that surface (if it is presenting a value lower than the Global maximum number of refinements from the Global parameters tab). This parameter supersedes any other selected adaptation criteria. Fine tuning of this parameter is useful when it may be difficult to determine the appropriate Target cell size, or if the Distance and Curvature criteria yield a prohibitive number of cells. The default value (10000) is an arbitrary large number such that the criteria are controlled by the Global maximum number of refinements.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user-defined target cell sizes for each geometrical surface. The size of a cell intersecting a geometrical surface are compared to the prescribed user target and the cell is refined until its actual size is lower than the target.

18. Repeat step 14 to step 17 for "Curve 218" except setting the Maximum number of refinements to <10>.
19. Go to Surface refinement tab.

Surface criterion considers cells intersecting surfaces as candidates for refinement. Three criteria have been implemented and are respectively based on:

a proximity between surfaces (Distance),
a surface curvature measurement (Curvature),
a specification of cell target sizes on the surfaces (Target cell sizes).

Volume criterion (found in Box refinement tab) considers cells intersecting or located inside a three-dimensional volume as candidates for refinement if their cell size is larger than some user prescribed target size.

20. Select "facet" from the surface list (tip of the wing).
21. Click on Active.
22. Set the Max nb of refinements to <8>.
23. Select the Target cell sizes criterion and keep the default values.
24. Repeat step 20 to step 23:

For "extrados" and "intrados" (wing) except setting the Max nb of refinements to <7> and adding Curvature criterion,
For "tail" except setting the Max nb of refinements to <10>,
For "body" except setting the Max nb of refinements to <6> and adding Curvature criterion.



25. Left-click on Trimming tab.
26. Keep default Not used for trimming for all EXT and MIR faces to keep cells on the selected faces at the end of the adaptation step. 
27. Click on Go to launch the adaptation step.


Mesh Wizard : Snapping Step
28. Left-click the check box for Snap to geometry in Mesh Wizard.
29. Click on Snap to geometry and the Snapping parameters dialog box appears.
30. Left-click on Advanced >>> button. It gives access to three extra tabs (Global parameters, Curve snapping and Buffer insertion).
31. Activate Insert buffer on faces not used for trimming under Global parameters tab.



The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh adaptation on the surface to obtain a good quality body conforming mesh. In addition to a simple projection on the geometry, this action involves sophisticated algorithms to recover lower dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner of the geometry and that a path of mesh edges is attached to the curve.
Layers of additional cells (buffer insertion) are introduced into the mesh also on faces not used for trimming as the symmetry plane (when option Insert buffer on faces not used for trimming is active) to create a body conforming mesh. 
Finally, a mesh smoothing is performed which moves points on the surface and in the volume.

32. Left-click on Ok to proceed.
Mesh Wizard : Optimization Step
33. Left-click the check box for Optimize in Mesh Wizard.
34. Left-click on Optimize and the Optimization parameters dialog box appears. 
35. Keep all default settings and click Ok to proceed.
36. Click on Start in Mesh Wizard to snap and optimize the mesh. 
The mesh obtained after the snapping step may involve poor quality cells usually located close to corners and curves. Some of these cells are concave or may even present a negative volume. HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly displacing their vertices.






37. Left-click on Mesh quality icon () in the Tool bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e. cells with a negative volume. Negative cells are not allowed in the final mesh to be used for the computation. Concave or twisted cells are less likely to present robustness or stability issues for solvers, however they should be prohibited.
When negative, concave or twisted cells are detected, they should be usually removed by changing mesh adaptation settings or advanced settings of snapping/optimization.
38. Check the mesh quality by using the Criterion drop-down list for the following criteria :

Negative cells,
Concave cells,
Twisted cells.

Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are presented through histograms. Each bar represents the number of cells whose criterion value is included in the bar interval. By left-clicking on one of the bars, the corresponding cells are displayed in the graphics area. Cells are displayed in a color varying depending on the value of the quality criterion. The Show markerscheck button activates the display of circle markers for each vertex of the displayed cells, which facilitates the localization of the selected cells.


39. After checking the mesh quality, click on Close to exit.
Mesh Wizard: Viscous Layers Insertion Step
40. Left-click the check box for Viscous layers in Mesh Wizard.
41. Left-click on Viscous layers and the Viscous layers insertion parameters dialog box appears.
42. Under Global tab, keep Fixed first layer thickness Method --> Inflate viscous layers --> Floating number of layers active. Do not change the range, it will be adapted automatically.
43. Go to the Surface tab.
44. Select all surfaces of the aircraft geometry of the list: left-click on first surface ("facet") and left-click + <Shift> on last surface ("intrados").
45. Click on Active to access the parameters for viscous layers insertion.
46. Left-click on the Compute button. This button opens a pop up window to compute the necessary first layer thickness.

The width of the first cell close to the wall must be selected with care since the quality of the flow solution will often depend upon the capture of the flow phenomena inside the boundary layers which develop along the solid walls. Depending upon the turbulence model selected, NUMECA recommends to locate the nearest grid point along the wall, at a distance that corresponds to parietal coordinate y+ ranging from 1-5 (low Reynolds number models) or 30-50 (high Reynolds number models). Assuming thermal effects must be modeled accurately, y+ can reach values as low as 0.1.
The relation between the parietal coordinate y+ and width of the first cell close to the wall y is driven by the Blasius equation, expressed as follows for turbulent flows :





where :

Ywall is the distance of the nearest grid point to the wall (in meter),
Vref is a reference velocity of the flow, for instance the inlet velocity (in m/s),
ν is the kinematic viscosity of the fluid (in m²/s), i.e. the dynamic viscosity divided by the density,
Lref is a reference length of the test case (in meter),
Y1+ is a non-dimensional value.


In the present case, Vref = 257.25 m/s ; Lref = 0.1412 m ; ν = 1.21e-05 m²/s. To get Y1+ = 50 at the wall, it comes Ywall = 8.3483e-5 m.
47. Set the inputs accordingly as shown below and click on Apply to validate the first layer thickness.


48. Select "facet" in the list with a left-click. Keep 1.2 for the stretching ratio and click on Apply button to use the advised value of viscous layers (8). HEXPRESS™ gives an indication about the appropriate number of viscous layers to insert. This number is computed based on the current mesh after optimization (this indication is not available if the optimization step is not performed yet). This value will be the minimum to activate the inflation method.
49. Repeat the above step for "extrados", "tail", "body" and "intrados" to use advised value of viscous layers (from 4 to 15 depending of the selected surface).
50. Click on Go to start the viscous layer insertion step.





In the viewing buttons, the cutting plane icon () will perform a cut inside the mesh to visualize the quality and viscous layers insertion along the wing as presented below. Cutting plane was performed at constant Y (press <y>) and translated (middle-click) on the wing



51. Repeat step 37 to step 39 to check the mesh quality after viscous layers insertion.
Save Mesh
52. Impose mirror type of periodicity so that users are allowed to plot full plane within CFView™:

Go to Grid/Periodicity... menu.
Click on New, and then Edit to define a new periodicity.
Set the periodicity name to <Mirror>.
Select MIRROR for the Periodicity type and set the Periodicity parameters (Origin and Axis) respectively to <0 0 0> and <0 1 0>.
Click on Ok to confirm and then close the Periodicity dialog box.



53. Go to Project/Save as... or click on the Save icon () in icon bar.
54. Under the "_mesh" folder (if FINE™/Open project), enter the name of the mesh project as <dlr-f4.igg> and press Ok or Save to save mesh files.


The mesh folder contain the mesh topology, geometry, grid points and the boundary condition types among other. The files list is written below :

.bcs : boundary conditions files,
.dom : geometry files,
.igg : topology file,
.hex : grid points files,
.hxp : extra information for the mesh generation,
.rep : report file,
.log : mesh generation information,
.dist : distance file (prefix is domain name),
.fnmb : FNMB connections,
.nmb : Non matching connections,
.qualityReport : quality report file.

In addition a subdirectory named "cache" contains resulting mesh files after each step of the mesh generation (for example "_snap.hex" as resulting mesh after snapping process). It allows to delete some steps and come back to a previous one without generating the necessary steps again.
55. Click on the Close button.


56. You can save the project (if not done already) and accept to link the new mesh to the project (if requested).
57. Acknowledge the warning that solver precision should be changed and click on Ok.


58. The Mesh properties dialog box appears. Check that the information is correct (keep Grid units to Meters) and click on Ok.


You are now back to the FINE™/Open interface and ready to proceed with the Flow Settings!

TUTORIALS
simulation
The tutorials for FINE™/Open with OpenLabs™ provide detailed step- by- step instructions for the
entire
of
HEXPRESS™/Hybrid allow a further detailed insight into the mesh generation process. Most of the
tutorials are designed so as to limit use of computational resources but some of them may require a
significant amount of computational time assuming they are executed on the finest mesh level.
of HEXPRESS™ and
process. Additional
tutorials
tutorials
the
Where to Find the Files Used in the Tutorials?
Most of the tutorials starts from mesh generation and uses an existing geometry. The appropriate
files (and any other relevant files used in the tutorial) can be downloaded from the corresponding
links:
l download Beginner level files
l download Advanced level files
l the Expert level files can be found in a separate tutorials archive as available from the
Products page of the Customer Area (www.numeca.be).
l download Customization with OpenLabs™ level files
Some of the project files (mesh and project, excluding solution files) can also be found in the
demo cases package dedicated to ready-to-run demonstration cases and presented in the Demo
Cases section. This allows to quickly start a calculation and observe the behavior of
FINE™/Open with OpenLabs™, without necessarily going through all the steps of the tutorials.
Conventions Used in the Tutorials
Several conventions are used in the tutorials to facilitate your learning process.
Following a short introduction, most of the tutorials are divided into 3 sections, respectively
related to mesh generation, settings and calculation, and post-treatment.
Inputs required to execute the tutorials are most often restricted to the geometry, either in a ".dom"
or CAD related format, and profiles of boundary conditions.
The sequence of actions to be executed are described through a numbered step-by-step approach.
Additional insight about some specific actions and/ or features is frequently added to further
illustrate the tutorial. This information is for the purpose of clarity and completeness, and should
not be executed. It appears as a note with a light blue background.
The calculations executed to illustrate the behavior of the flow solver include a reasonable number
of grid points, so as to limit the computational resources required to complete the tutorials. As a
consequence, most of the underlying flow solutions must be considered as qualitative. Additional
mesh refinement may be required in some circumstances so as to obtain a more quantitative
picture.
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
BEGINNER
The following Beginner level tutorials for FINE™/Open with OpenLabs™ allow to familiarize with
the Graphical User Interface and and basis of the mesh generation technique, project set up and
solution procedures.
TUTORIAL 1.
AUTOMOTIVE MANIFOLD
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l Spatial discretization of the flow equations,
l Flow computation,
l Visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated.
The unstructured CFD package consists of the following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
This tutorial is particularly adapted to a 3D internal application. It makes use of FINE™/Open with
OpenLabs™ including HEXPRESS™ and CFView™.
In this tutorial the user will learn how to:
l Use HEXPRESS™ user interface,
l Import an existing domain,
l Visualize a mesh,
l Progress in the mesh wizard to generate the mesh,
l Control the quality of the mesh,
l Set up a computation in FINE™/Open interface,
l Start/stop the computation,
l Visualize the results with CFView™.
1.1
INTRODUCTION
1.1.1
Prerequisites
This tutorial does not require any particular prerequisite to learn the basics of the interface usage.
1.1.2
Problem Description
In automotive engineering, an intake manifold or inlet manifold is the part of an engine that
supplies the fuel/air mixture to the cylinders. An exhaust manifold or header collects the exhaust
gases from multiple cylinders into one pipe. The word manifold refers to the folding together of
multiple inputs and outputs (source Wikipedia). The geometric configuration is shown in the
following figure.
Air, modeled as a perfect gas with constant kinematic viscosity of 1.716e-5 m²/s and density of
1.1751 kg/m3, is considered. Extrapolated static pressure to static pressure conditions are imposed
respectively at inlet and outlet. The outlet pressure corresponds to atmospheric conditions 101,300
Pa. The inlet velocity components are Vy = 35.35 m/s and Vz = -35.35 m/s.
1.1.3
Preparation
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <manifold.iec> and click on Save or Ok.
FINE™/Open will automatically create a project folder called "manifold" which will contain the
project file (" .iec") and a folder " _mesh" where the mesh will be stored. Later, computation
folders will appear inside the project folder. It is strongly advised to keep this file structure all
along the project.
l Click on Yes to start HEXPRESS™ unstructured mesh generator.
You're now ready to start the Mesh Generation process and mesh the Automotive
Manifold!
MESH GENERATION
HEXPRESS™ graphical user interface allows to visualize the geometry and mesh of the internal
or external test case in a graphics area. The access to main menu and controls is proposed through
a menu bar and a quick access pad, and is completed with a tool/icon bar and a control area
(including the keyboard input area).
1.2
OPEN EXISTING DOMAIN FILE
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined and therefore it starts from the domain file ".dom". It should be noticed that
the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL), import
HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS dialog box.
2. Locate and select "automotive_manifold.dom" in the dialog box (download Beginner tutorial
archive) and click on Open or Ok.
1.3
VISUALIZATION
Use the viewing buttons at the bottom of the interface to display the geometry as preferred. In
View subpanel from the Quick Access Pad, it is possible to:
l Left-click on Mesh icon (
) to hide/show mesh (toggle),
l Left-click on Solid icon (
) to hide/show faces (toggle),
l Right-click on Face icon (
) or left-click on icon
to open Face Viewer window.
The face selection can be done interactively in the graphics area or thanks to the Face Viewer
window.
1.4
SET BOUNDARY CONDITIONS
3. Go to the Grid/Boundary Conditions... menu or click on Boundary Conditions icon (
in the icon bar and set the boundary conditions using the Set face type button:
)
l set "manifold_group_#" for 0, 3 and 4 as inlet ("INL");
l set "manifold_group_2" as outlet ("OUT");
l set "manifold_group_1" as solid ("SOL").
l <11> <Enter> for X axis,
l <6> <Enter> for Y axis,
l <4> <Enter> for Z axis.
These numbers allow to create an initial mesh which aspect ratio is close to 1. The settings also
allow to have at least approx. 2 to 3 cells everywhere in the domain in each direction. For more
details, see Initial Mesh.
8. Click on Go to create the Initial Mesh with 264 cells.
9. By default the mesh is not loaded. To visualize the mesh, hit Mesh button in the View
subpanel.
1.6
MESH WIZARD : ADAPTATION STEP
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selection in this action directly dictates the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming. See Adapt To Geometry for more information.
in terms of user
important
During the first one, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry
dependent criteria. With the second step, it removes cells intersecting the geometry or located outside
the computational domain.
10. Left-click on check box for Adapt to geometry in Mesh Wizard to activate the step.
11. Left-click on Adapt to geometry to open the Refinement and trimming parameters dialog
box.
12. Under the Global tab, set the Maximum number of refinements to <3> <Enter>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement. The sizes of the initial
mesh cells are therefore divided by a factor 2N after N successive refinements. This may result in an
exponential growth of the total number of cells in the mesh. To bound the number of cells, the user
should set the maximum number of refinements to a reasonable limit. The maximum number of
refinements should be large enough so that the geometry is well captured, but a too large number will
result in a big total number of cells.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may therefore alter the success of the meshing process. More details are available in the User Manual.
13. Left-click on Surface refinement tab.
The adaptation process is defined by three classes of criteria: curve, surface and volume criteria.
Surface criterion is considering cells which are intersecting surfaces as candidates for refinement.
Three criteria are implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
Volume criterion (found in Box Adaptation tab) is considering cells which are intersecting or
located inside a three-dimensional volume as candidates for refinement if their cell size is larger than
some user prescribed target size.
14. Left-click on "manifold_group_1" in the list of patches.
15. Click on Active.
16. Set the Maximum number of refinements to <3> <Enter>.
17. Select the Curvature and Target cell sizes criteria and keep the default values (<0.0>).
The Maximum number of refinements per surface ultimately controls the refinement of cells
intersecting that surface (if it is presenting a value lower than the Global maximum number of
refinements from the Global parameters tab). This parameter supersedes any other selected
adaptation criteria. Fine tuning of this parameter is useful when it may be difficult to determine the
appropriate Target cell size, or if the Distance and Curvature criteria yield a prohibitive number
of cells. The default value (10000) is an arbitrary large number such that the criteria are controlled by
the Global maximum number of refinements.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell sizes for each
intersecting a geometrical surface are compared to the
geometrical surface. The size of a cell
prescribed user target and the cell is refined until its actual size is lower than the target.
18. Click on Ok and then on Step to launch the adaptation (refinement/trimming) step.
1.7
MESH WIZARD: SNAPPING/OPTIMIZATION
STEPS
19. Left-click on check box for Snap to geometry in Mesh Wizard. An activation sign will
appear inside the box dedicated to the step.
20. Left-click on Snap to geometry to edit.
21. Keep the default and close the dialog box (OK button)
The aim of this fully automated mesh step ( Snap to geometry) is to project the staircase mesh
obtained after the mesh adaptation on the surface to obtain a good quality body conforming mesh. In
addition to a simple projection on the geometry, this action involves sophisticated algorithms to
recover lower dimensional geometric features such as corners and curves in the mesh. These
algorithms guarantee that, when the mesh is projected onto the surface geometry, a mesh vertex is
attached to each corner of the geometry and that a path of mesh edges is attached to the curve.
Layers of additional cells (buffer insertion) are introduced into the mesh to create a body conforming
mesh. Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
The mesh obtained after the snapping step may contains poor quality cells which usually located close
to corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
22. Left-click on check box for Optimize in Mesh Wizard to activate the step.
23. Left-click on Optimize.
24. Keep default settings.
25. Left-click on OK.
26. Click on Start in Mesh Wizard to snap and optimize the mesh.
27. Left-click on icon
in icon bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e. cells with a
negative volume. Negative cells are not allowed in the final mesh to be used for the computation.
Concave or twisted cells are less likely to present robustness or stability issues for solvers,
however they should be avoided as much as possible.
When negative, concave or twisted cells are detected, they should be usually removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
28. Check the mesh quality using the Criterion pull-down menu for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are
presented through histograms. Each bar represents the number of cells whose criterion value is
included in the bar interval. By left-clicking on one of the bars, the corresponding cells are
displayed in the graphics area. Cells are displayed in a color varying depending on the value of
the quality criterion. The Show markers check button activates the display of circle markers for
each vertex of the displayed cells, which facilitates the localization of the selected cells.
29. After checking the mesh quality, click on Close.
1.8
MESH WIZARD: VISCOUS LAYERS
INSERTION STEP
HEXPRESS™ proposes a very specific approach for the insertion of layers of large aspect ratio cells
to accurately resolve boundary layers. The technique is based on successive subdivisions of the cells
connected to the walls. See Viscous Layers for more information.
30. Left-click on check box for Viscous layers in Mesh Wizard to activate the step.
31. Left-click on Viscous layers to edit.
32. Under Global tab, keep Fixed first layer thickness Method -> Inflate viscous layers ->
Floating number of layers active. Do not change the range, it will be adapted automatically.
33. Click on Surface tab.
34. Left-click on manifold_group_1 and click on Active.
35. Click on the Compute button. This button opens a pop up window to compute the necessary
first layer thickness.
The width of the first cell close to the wall must be selected with care since the quality of the flow
solution will often depend upon the capture of the flow phenomena inside the boundary layers which
develop along the solid walls. Depending upon the turbulence model selected, NUMECA recommends
to locate the nearest grid point along the wall, at a distance that corresponds to parietal coordinate y+
ranging from 1- 5 (low Reynolds number models) or 30- 50 (high Reynolds number models).
Assuming thermal effects must be modeled accurately, y+ can reach values as low as 0.1.
The relation between the parietal coordinate y+ and width of the first cell close to the wall y is driven
by the Blasius equation, expressed as follows for turbulent flows:
where:
l Ywall is the distance of the nearest grid point to the wall (in meter),
l Vref is a reference velocity of the flow, for instance the inlet velocity (in m/s),
l ν is the kinematic viscosity of the fluid (in m²/s), i.e. the dynamic viscosity divided by the density,
l Lref is a reference length of the test case (in meter),
l Y1
+ is a non-dimensional value.
In the present case, Vref = 50 m/s ; Lref = 0.04 m ; ν = 1.716e-05 m²/s. To get Y1
it comes Ywall = 8.11678e-6 m.
36. Set the inputs accordingly as shown below and click on Apply to validate the first layer
thickness.
+ = 1 at the wall,
37. Keep <1.2> for the stretching ratio.
38. Click on Apply button to use the advised value of viscous layers (set to 24). HEXPRESS™
gives an indication about the appropriate number of viscous layers to insert. This number is
computed based on the current mesh after optimization (this indication is not available if the
optimization step is not performed yet). This value will be the minimum to activate the inflation
method.
39. Click on Ok to confirm the values.
41. Repeat step 27 to step 29 to check mesh quality after viscous layers insertion.
1.9
SAVE MESH
42. Go to Project/Save as... or click on the Save icon (
) in icon bar. Under the "_mesh"
folder (if FINE™/Open project), enter the name of the mesh project as < automotive_
manifold.igg> and press Ok or Save to save mesh files.
The mesh folder contain the mesh topology, geometry, grid points and the boundary condition
types among other. The files list is written below:
l .bcs: boundary conditions files,
l .dom: geometry files,
l .igg: topology file,
l .hex: grid points files,
l .rep: report file,
l .dist: distance file (prefix is domain name),
l .fnmb: FNMB connections,
l .qualityReport: quality report file.
43. Click on the Close button (
to link the new mesh to the project (if requested).
). You can save the project (if not done already) and accept
44. Acknowledge the warning that solver precision should be changed and click on Ok.
FINE™/Open with OpenLabs™ will check the mesh quality when linking a mesh to the project. If the
value of the quality items is not reached the criteria, a warning will be given. See Mesh Properties
for more information. Bad mesh quality will reduce the solution accuracy, and even leads to the crash
of the solver.
45. The Mesh properties dialog box appears. Check that the information is correct (keep Grid
units to Meters) and click on Ok.
You are now back to the FINE™/Open interface and ready to define the "Flow Settings"
(p. 39).
FLOW SETTINGS
A step by step approach is proposed in the following lines. It aims at driving you through the
various steps that need to be executed to set up and start the computation.
1.10 SET SOLVER PRECISION
46. In Project/Preferences... select Full-double-precision mode and click on Ok.
1.11 MANAGE COMPUTATIONS
47. In the Computations menu, right-click on the computation name and select Rename.
48. Rename "computation_1" as <KeExtWF> <Enter> (as a reference to the turbulence model:
"K-Epsilon extended wall function", used in this tutorial).
In the Computations menu, the list of computations are shown. It is possible to Rename, create a
new one by duplicating the highlighted one (New button) or just delete the computation by clicking
on Delete.
1.12
SET PHYSICAL CONFIGURATION
49. In the Physical Configuration menu, double left-click on General Properties menu.
50. Keep Steady mode and Fluid block active for the "fluid" domain.
51. Click on Ok to validate.
52. In the Physical Configuration menu, double left-click on Fluid Model.
53. In the Edit/Select fluid section, click on Select... and pick AIR(Perfect) up from the list.
54. Click on Ok to confirm.
55. Click on Close.
42
FINE™/Open with OpenLabs™ 7.2 Tutorials
56. In the Physical Configuration menu, double left-click on Flow Model. Select k-epsilon
(Extended Wall Function) as Turbulence model.
The wall functions are used to mimic the presence of the walls by reflecting the effect of the steep,
non- linear variations of the flow properties through the turbulent boundary layer. They define the
shear stress and the heat flux on the cell faces lying on solid boundaries as well as the values of the
turbulent variables in the vicinity of the wall. FINE™/Open provides both standard wall function
(only for k-ε model) and extended wall function. For more details, see Modeling the flow near the
wall.
57. Select the option Low Speed Flow (M<0.3)
58. Change the reference parameters:
l Set Reference length as <0.04> <Enter> [m],
l Set Reference velocity as <50> <Enter> [m/s].
59. Click on Ok to confirm.
1.13
BOUNDARY CONDITIONS
FINE™/Open with OpenLabs™ provides various boundary conditions for use, see Boundary
Conditions for more information.
60. In the Boundary Conditions menu, double left-click on Boundary Conditions.
61. Under the INLET tab, create a group of the three inlet patches:
l left-click on first patch,
l left-click + <Shift> on last patch,
l click on Group button,
l in Enter the new group name, type <INLET> <Enter> to create group.
62. Keep default settings (Static Quantities Imposed -> Static Pressure Extrapolated) and
impose the values below (inlet patches are not aligned with the Cartesian axis but in the Y-Z
plane: two components of the velocity need to be defined):
l Set Vx to <0> <Enter> [m/s],
l Set Vy to <35.35> <Enter> [m/s],
l Set Vz to <-35.35> <Enter> [m/s],
l Set Static Temperature to <293> <Enter> [K],
l Set k to <9.375> <Enter> [m2/s2],
l Set Epsilon to <10833.6> <Enter> [m2/s3].
The values of the turbulent kinetic energy k is derived from the turbulence intensity Tu (more details
in Best Practice for Turbulence modeling).
They are:
where:
l u" is the streamwise fluctuating velocity,
l Uref is the streamwise velocity,
l Tu is about 5% for internal flows.
As for the turbulent dissipation Epsilon , the estimation is made by specifying the ratio of the
turbulent viscosity to the laminar viscosity (more details in Best Practice for Turbulence modeling).
where: Cμ = 0.09 and μt/μ = 50. *The reference values of the density and dynamic viscosity depend
on the fluid model used.
The value of k can also be derived from the wall shear stress while the estimation of Epsilon can be
obtained from the asymptotic turbulent kinetic energy equation.
Please refer to Best Practice for Turbulence modeling for more information.
63. Set Static Pressure to <101300> <Enter> [Pa] for the outlet under the OUTLET tab and
keep the solid boundary conditions under the SOLID tab.
64. Click Ok to close the window.
1.14
INITIAL SOLUTION
65. In the Initial Solution menu, double left- click on Initial Solution and set the values
accordingly:
l Pressure = <101300> <Enter> [Pa],
l Temperature = <293> <Enter> [K],
l Vx = <0> <Enter> [m/s],
l Vy = <35.35> <Enter> [m/s],
l Vz = <-35.35> <Enter> [m/s],
l k = <9.375> <Enter> [m2/s2],
l epsilon = <1083.36> <Enter> [m2/s3]
It is recommended to impose 10% of the Epsilon value at the inlet to initialize the field. By doing
this, the possibility to have oscillations for the skin friction due to non- physical relaminarization
during convergence can be reduced.
66. Click on Ok to close the window.
1.15 NUMERICAL PARAMETERS
67. In the Numerical Parameters menu, double left-click on General Parameters.
68. Check if the number of grid(s) is set to 4.
The flow solver is based on an explicit time integration technique, which is accelerated by means of a
dedicated multigrid method. To this end, several levels of intermediate grids must be generated
starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
69. Check the Coarse Grid Initialization to make sure it is active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be
significantly reduced by activating the Coarse Grid Initialization process. In that case, the simulation
starts on the coarsest grid level available, leading to fast convergence. Once it is done, the flow solver
automatically interpolates the current flow solution on the intermediate levels before the iterative
process is restarted. A similar process repeats until the expected finest grid level is achieved. The
iterative process stop when the convergence criteria is reached or the maximum number of iterations
is exceeded.
70. Keep the defaults and click on Ok.
71. In the Numerical Parameters menu, double left-click on Numerical Schemes.
72. Set the preconditioning to Merkle, set the Characteristic velocity to <50> m/s.
In the low subsonic Mach number regime, time marching algorithms designed for compressible flows
show a pronounced lack of efficiency. The low speed preconditioner provides fast convergence
characteristics and accurate solutions as the Mach number approaches zero. See Preconditioning for
more details.
73. Click on Ok.
The CFL number drives the pseudo- time step selected to reach a steady state solution using the
time-marching method integrated in the flow solver. In combination with the 4-steps Runge-Kutta
integration scheme included in the flow solver, it has a theoretical stability limit close to 2.8.
However, the additional implicit smoothing scheme can increase this value slightly, which justifies the
default value of 3. The default value for CFL number is adequate in most cases, but can be
decreased in some circumstances, in particular at off-design conditions.
1.16 OUTPUT PARAMETERS
74. In the Computation Control menu, double left-click on Outputs menu.
75. Select Internal flow outputs (default) in Flow configuration area.
By default and in function of the Flow configuration selected, a list of quantities is defined to be
computed in the flow solver. The list can be manually adapted by selecting a quantity in a category
and clicking on the Add --> and <-- Remove buttons.
76. Click on Ok.
1.17 CONTROL VARIABLES
77. In the Computation Control menu, double left-click on Control Variables menu.
78. Set the Number of iterations to <400> <Enter>.
79. Set the Convergence criteria to <-6> <Enter>.
80. Save the solution at every <100> <Enter> iterations.
81. Click on Ok to confirm.
1.18 SAVE PROJECT & COMPUTATION
82. Click on Save Project button to save the project.
83. Click on Save Selected 'Run' files button to save the computation.
1.19
START & STOP COMPUTATION
84. Click on Start Solver button to launch the computation and click on Ok to run in serial mode.
To save and stop a computation while running, the button Suspend Solver should be pressed.
However, to stop the computation without saving, the Kill Solver button should be used.
When a computation is finished or suspended, it can be restarted, see Initial Solution from File for
more details.
The pop up Task manager window allows following the convergence history of the
computation.
1.20 MONITORING
Evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out) and/or global
quantities (efficiency, pressure ratio, torque and axial thrust on solid walls selected in the
boundary conditions page) can be performed in the steering. Local and global quantities may also
be added for follow up during the convergence process. However, their representation in the
graphical area will be effective only once they will be added, and past history will not be
available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out, with satisfactory correspondence (usually less than 0.5%
difference between in/out).
To do so, select the inlet and outlet mass flow at once. An information about the difference is
automatically computed.
The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations, can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via the icon bar.
The iterative process is now over. The convergence curve shows a peak each time a new grid
level in the multigrid initialization is started. However the number of iterations imposed in the
control variable page corresponds to the computation on the finest grid level, explaining why the
total number of iterations of the simulation (including the multigrid initialization phase) is larger
than expected.
As part of the FINE™ environment, NUMECA proposes the visualization and post-treatment
tool CFView™ for that purpose. CFView™ is entirely integrated within the environment and
includes numerous tools.
85. To access CFView™ from the FINE™ graphical user interface, press the CFView™ icon (
).
You are now entering to the CFView™ interface and ready to proceed with the "Post
Processing" (p. 57) of the results!
POST PROCESSING
A step by step approach is proposed in the following lines. It aims at driving you through the
various steps that need to be executed from reading the solution to the extraction of the main
results. CFView™ automatically opens the file ".run" file associated with the active computation.
1.21
SELECT QUANTITIES
86. In the Surfaces section, all solid surfaces are selected by default.
87. Go to Quantities section in the Quick Access Pad.
88. Double left-click on the Static Pressure.
All quantities selected in FINE™ graphical user interface are transferred to CFView™. However,
additional derived output can also be accessed directly from the visualization and post-treatment tool,
including vector components, gradients, divergence and curl of selected quantities. New quantities,
defined from existing quantities combined by regular operations (arithmetic functions, trigonometric
functions, logarithmic functions,...) can be created with the Quantity/Field Data/Define New
Quantity... menu.
Once the candidate quantity for visualization is selected, a representation mode should also be
selected. Representation is typically executed in the form of color contours (smoothed or stripped)
and/or isolines. CFView™ also includes the possibility to interrogate the flow field locally ("local
value") and create 1D Cartesian plots. Advanced capabilities involving curve and/or surface
integration can also be accessed.
1.22 REPRESENTATION ON SOLID PATCHES
89. Click on Representations/Contours & Iso Values section and then on Strip Contour icon
to display the selected quantity.
90. Click on the icon Isolines.
91. Increase the number to <21> <Enter> isolines and select Uniform.
92. Click on Apply and then on Close.
1.23 REPRESENTATION ON CUTTING PLANE
(VECTORS)
93. Click on Update/Delete/All to delete all previous manipulations in the Graphics area.
94. Click on Geometry/Create Cutting plane... menu.
95. Enter the X, Y, Z values for Point and Normal as shown on the following figure.
96. Click on Apply and Geometry to pre-visualize the cutting plane.
97. Click on Save to add this cutting plane to the Surfaces section in Quick Access Pad, that will
be activated by default.
98. Click on Close.
99. In Surfaces section, select "CUT1" by left-click, right-click and Select.
100. Double left-click on the quantity Vxyz (Velocity) in Quantities section (Quick Access
Pad).
101. Click on Representations/Vectors section and on the icon Vectors on Grid Nodes.
1.24 REPRESENTATION ON CUTTING PLANE
(VECTOR LINES)
102. Click on Update/Delete/All to delete all previous manipulations in the Graphics area.
103. In Surfaces section, left-click on "CUT1", then right-click and Delete to remove the cutting
plane. Now, select all inlets by double left-clicking on the corresponding group ("INLET").
104. Keep Vxyz (Velocity) quantity selected.
105. Click on Representations/Vector Lines section.
106. Click on Vector Lines Parameters icon.
107. Change the Representation to tube and the Color to Velocity.
108. Click on Apply button to validate and then on Close.
109. Click on the icon Vector Lines from Section.
110. Enter <5> in the keyboard input area to draw 5 vector lines.
111. With the mouse, draw a line on one of the inlet surfaces by left-clicking and drag on it and
repeat the action on all inlet patches.
112. In Surfaces section, select "manifold_group_1 Solid" by left-clicking, right-click and Select.
113. Then under Representations/Grid section, click on Render Gouraud icon to activate the
shading.
114. Click on Opacity section, and decrease it to 0.50.
115. Select File/Print... menu.
116. Click on Ok after defining the picture settings.
117. Click on Ok after selecting the location to save and the name of the picture.
118. Select File/Quit CFView to leave CFView™ session.
TUTORIAL 2.
TURBINE MARK II
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l Spatial discretization of the flow equations,
l Flow computation,
l Visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated.
The unstructured CFD package consists of the following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
This tutorial is particularly adapted to a 2D internal application. It makes use of FINE™/Open with
OpenLabs™ including HEXPRESS™ and CFView™.
In this tutorial it is possible to learn how to:
l Use HEXPRESS™ user interface,
l Import an existing domain,
l Visualize a mesh,
l Progress in the mesh wizard to generate the mesh,
l Control the quality of the mesh,
l Set up a computation in FINE™/Open interface,
l Start/stop the computation,
l Visualize the results with CFView™.
2.1
INTRODUCTION
2.1.1
Prerequisites
This tutorial does not require any particular prerequisite to learn the basics of the interface usage.
2.1.2
Problem Description
In order to increase the efficiency and the specific power of gas turbine engines, the turbine inlet
temperature study is increasingly important. Nevertheless, material progress is not sufficiently
important to guarantee an economically acceptable lifespan of the components, in contact with the
hot gases. Accordingly, the flow through turbine nozzle guide vane known as Mark II is here
considered. The objective is to demonstrate the ability of FINE™/Open to predict aerodynamic
effects and conjugate heat transfer phenomena occurring in a 2D high-pressure turbine blade.
The geometric configuration is shown in the following figure. The 2D vane is cooled by 10
cooling channels, where the air is supplied. The vane is made of ASTM type 310 stainless steel.
This material is not normally used for turbine vanes but was initially selected by the researchers
due to its low thermal conductivity (18.7 W/m.K). The temperature at the walls inside the cooling
channels is ranging from 455 K to 621 K while the total temperature at the inlet of the fluid
domain is fixed to 788 K. Air, modeled as a perfect gas with a constant kinematic viscosity of
7.77e-5 m²/s, is considered. Total-to-static pressure conditions are imposed respectively at inlet
and exit, resulting in a driving mass flow close to 1.44 kg/s. The prescribed pressure ratio
corresponds to an isentropic exit Mach number of 1.01. The Reynolds number, determined using
the exit velocity and the chord-length, is about 1.8e5. No boundary conditions, especially for the
coupling of the fluid region and the vane material, are required as an input of the simulation.
2.1.3
Preparation
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <turbine_markII.iec> and click on Save or Ok.
FINE™/Open will automatically create a project folder called " turbine_ markII" which will
contain the project file (" .iec") and a folder " _mesh" where the mesh will be stored. Later,
computation folders will appear inside the project folder. It is strongly advised to keep this file
structure all along the project.
l Click on Yes to start HEXPRESS™ unstructured mesh generator.
You are now ready to start the "Mesh Generation" (p. 70) process and mesh the turbine
Mark II!
MESH GENERATION
HEXPRESS™ graphical user interface allows you to visualize the geometry and mesh of the
internal or external test case in a graphics area. The access to the main menu and controls is
provided by a menu bar and a quick access pad, and is completed with a tool/icon bar and a
control area (including the keyboard input area).
2.2 OPEN EXISTING DOMAIN FILE
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined. That is why the tutorial starts from a domain file ".dom". It should be
noticed that the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL),
import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as execute Python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS dialog box.
2. Locate and select "turbine_ MarkII.dom" in the dialog box ( download Beginner tutorial
archive) and click on Open or Ok.
2.3
VISUALIZATION
Use the viewing buttons at the bottom of the interface to display the geometry as preferred. In the
View subpanel from the Quick Access Pad, it is possible to:
l Left-click on the Mesh icon (
) to hide/show mesh (toggle),
l Left-click on the Solid icon (
) to hide/show faces (toggle),
l Right-click on the Face icon (
) or left-click on the Face viewer icon (
) to open the
Face Viewer window.
Face selection can be done interactively in the graphics area or thanks to the Face Viewer
window.
2.4
SET BOUNDARY CONDITIONS
3. Left-click on the 2D button to change the grid generation mode in the Tool bar and hit Yes in
the pop-up window to confirm.
The three-dimensional mesh generation mode is the default configuration. A two-dimensional domain
is still three-dimensional, however it is then bounded in the Z-direction by two planes, parallel to the
2D mesh generation plane separated by an arbitrary distance. HEXPRESS™ will only generate one
cell in the Z-direction. A valid two-dimensional mesh project is obtained if the following conditions
are met:
l The axes of the two-dimensional domain are assumed to be X and Y.
l The Z-axis is assumed orthogonal to the 2D plane of interest.
l The two planes orthogonal to the Z-axis are flagged as mirror surfaces (MIR).
The two- dimensional grid generation mode in the Icon bar must be selected before executing any
action on the mesh wizard. All specific mesh action parameters related to the Z-axis are disabled in
this mode. Therefore, changing the mesh generation mode during the mesh generation may lead to
unpredictable behavior of the mesh generator.
4. Go to the Grid/Boundary Conditions... menu or click on the Boundary Conditions icon (
) in the Tool bar and set the boundary conditions using the Set face type button:
l "fluid_group_1" as outlet ("OUT");
l "fluid_group_3" as inlet ("INL");
l "fluid_group_4" and "fluid_group_5" as mirror ("MIR");
l "blade_group_0" and "blade_group_1" as mirror ("MIR").
5. Close the dialog box.
2.5 MESH WIZARD FLUID BLOCK: INITIAL MESH
6. The current domain file contains two different domains: the "fluid" and the "blade" (solid) part.
The selection of one of the two can be done directly by left-clicking on it in the graphics area or
via the Active domain drop-down list in the Tool bar. Select "fluid" as the Active domain from
the drop-down list or through the graphics area.
7. Left- click the checkbox for Initial mesh in Mesh Wizard to activate the step. The
corresponding step becomes accessible for the user. The same behavior is applied for the
following steps in the Mesh Wizard.
8. Left-click on Initial mesh and the Initial mesh parameters dialog box appears.
9. Set Nb of cells to <500> and click on the Auto button.
By using the Auto button, HEXPRESS™ computes the required number of cells in each direction to
get an isotropic mesh. The total number of cells may then vary (here the number of cells is adapted
from 500 to 493).
10. Click on Ok in the dialog box and then the Step button from the Mesh Wizard or hit the Go
button directly to create the initial mesh with 493 cells. By default, the mesh is not loaded. To
visualize the mesh, hit the Mesh button in the View subpanel.
2.6 MESH WIZARD FLUID BLOCK: ADAPTATION
STEP
2.6.1
Refinement
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selected in this action directly dictate the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming.
regarding the user
important
During the first step, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry-
dependent criteria. With the second step, it removes the cells intersecting the geometry or located
outside the computational domain.
11. Left-click the checkbox for Adapt to geometry in Mesh Wizard.
12. Click on Adapt to geometry and the Refinement and trimming parameters dialog box
appears.
13. Under the Global tab, set the Maximum number of refinements to <6>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement in one or several different
directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive
refinements. This may result in an exponential growth of the total number of cells in the mesh, even
though the refinement may be confined to some areas of the computational domain. To bound the
number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may alter the success of the meshing process. More details are available in the User Guide.
14. Left-click on the Surface refinement tab.
The adaptation process is defined by three classes of criteria: curve, surface and volume criteria. The
surface criterion considers cells which are intersecting surfaces as candidates for refinement. Three
criteria are implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
The volume criterion (found in the Box refinement tab) considers cells which are intersecting or
located inside a three-dimensional volume as candidates for refinement if their cell size is larger than
some user prescribed target size.
15. Select "fluid_group_6". The selected solid faces are highlighted in the graphics area. Left-
clicking on faces in the graphics area allows selecting them as well.
16. Click on Active to access the refinement parameters.
17. Set the Max nb of refinements to <6>.
18. Select the Target cell sizes criterion and keep the default values.
The Max nb of refinements per surface ultimately controls the refinement of cells intersecting that
surface (if it is presenting a value lower than the Maximum number of refinements from the
Global tab). This parameter supersedes any other selected adaptation criteria. Fine tuning of this
parameter is useful when it may be difficult to determine the appropriate Target cell size, or if the
Distance and Curvature criteria yield a prohibitive number of cells. The default value (10000) is
an arbitrarily large number such that the criteria are controlled by the Maximum number of
refinements from the Global tab.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell size for each
intersecting a geometrical surface are compared to the
geometrical surface. The size of a cell
prescribed user target and the cell is refined until its actual size is lower than the target.
19. Repeat the above steps for "fluid_group_7" except setting the Max nb of refinements to
<5>.
2.6.2
Trimming
20. Left-click on the Trimming tab.
21. Select "fluid_group_1" and "fluid_group_3" patches in the list by using left-click + <Ctrl>.
22. Select Not used for trimming from the Set patch trimming status drop-down list.
23. Click on Ok to validate the choice.
The trimming step removes all the cells intersecting or located outside of the geometry.
The trimming parameters allow modifying the default selected surfaces for the trimming operation.
Only planar surfaces parallel to Cartesian axes are present. Surfaces which are set as Not used for
trimming will keep a Cartesian mesh close to them.
24. Hit the Step button in the Mesh Wizard to start the mesh refinement and trimming.
2.7 MESH WIZARD FLUID BLOCK: SNAPPING
STEP
25. Left-click the checkbox for Snap to geometry in Mesh Wizard.
26. Click on Snap to geometry and the Snapping parameters dialog box appears.
27. The Advanced >>> button gives access to three extra tabs (Global parameters, Curve
snapping and Buffer insertion). It is not necessary to change the default settings in this tutorial.
28. Left-click on Ok to proceed.
The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh
adaptation onto the surface to obtain a good quality, body-conforming mesh. In addition to a simple
projection onto the geometry,
lower-
dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee
that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner
of the geometry and that a path of mesh edges is attached to the curve.
this action involves sophisticated algorithms to recover
Layers of additional cells (buffer insertion) are introduced into the mesh to create a body-conforming
mesh. Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
2.8 MESH WIZARD FLUID BLOCK:
OPTIMIZATION STEP
The mesh obtained after the snapping step may contain poor quality cells which are usually located
close to corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
29. Left-click the checkbox for Optimize in Mesh Wizard.
30. Left-click on Optimize and the Optimization parameters dialog box appears.
31. Keep all the default settings.
32. Left-click on Ok to proceed.
33. Hit the Start button in Mesh Wizard to snap and optimize the mesh.
34. Left-click on the Mesh quality icon (
) in the Tool bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e. cells with a
negative volume. Negative cells are not allowed in the final mesh to be used for the computation.
Concave or twisted cells are less likely to present robustness or stability issues for solvers,
however they should be prohibited.
When negative, concave or twisted cells are detected, they should usually be removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
35. Check the mesh quality by using the Criterion drop-down list for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are
presented through histograms. Each bar represents the number of cells whose criterion value is
included in the bar interval. By left-clicking on one of the bars, the corresponding cells are
displayed in the graphics area. Cells are displayed in a color varying depending on the value of
the quality criterion. The Show markers check button activates the display of circle markers for
each vertex of the displayed cells, which facilitates the localization of the selected cells.
36. After checking the mesh quality, click on Close to exit.
2.9 MESH WIZARD FLUID BLOCK: VISCOUS
LAYERS INSERTION STEP
37. Left-click the checkbox for Viscous layers in Mesh Wizard.
38. Left-click on Viscous layers and the Viscous layers insertion parameters dialog box
appears.
39. Go to the Surface tab.
40. Left-click and drag to select "fluid_group_6" and "fluid_group_7" surfaces.
41. Click on Active to access the parameters for viscous layers insertion.
Clicking on Group as Adapt button will automatically group the surfaces like in the Surface
refinement tab of the Refinement menu. Manual grouping can also be done thanks to the Group
button. Since no group was defined in this tutorial, clicking on the button will have no impact.
42. Go to the Global tab.
43. Click on the Compute button. This button opens a pop-up window which is used to compute
the necessary first layer thickness.
The width of the first cell close to the wall must be selected with care since the quality of the flow
solution will often depend upon the capture of the flow phenomena inside the boundary layers which
develop along the solid walls. Depending upon the turbulence model selected, NUMECA recommends
to locate the nearest grid point along the wall, at a distance that corresponds to parietal coordinate y+
ranging from 1- 5 (low Reynolds number models) or 30- 50 (high Reynolds number models).
Assuming thermal effects must be modeled accurately, y+ can reach values as low as 0.1.
The relation between the parietal coordinate y+ and width of the first cell close to the wall y is driven
by the Blasius equation, expressed as follows for turbulent flows:
where:
l Ywall is the distance of the nearest grid point to the wall (in meter),
l Vref is a reference velocity of the flow, for instance the inlet velocity (in m/s),
l ν is the kinematic viscosity of the fluid (in m²/s), i.e. the dynamic viscosity divided by the density,
l Lref is a reference length of the test case (in meter),
l Y1
+ is a non-dimensional value.
In the present case, Vref = 106 m/s; Lref = 0.13 m; ν = 7.7e-05 m²/s. To get Y1
comes Ywall = 1.8126e-5 m.
44. Set the inputs accordingly as shown below and click on Apply to validate the computed first
layer thickness.
+ = 1 at the wall, it
45. Keep 1.2 for the stretching ratio.
46. Click on the Apply to Active Surfaces button to use the computed first layer thickness on the
surfaces activated in step 40 and step 41.
47. Hit Yes in the pop-up menu to apply the computed first layer thickness on the activated
surfaces.
HEXPRESS™ gives an indication about the appropriate number of viscous layers to insert. This
number is computed based on the current mesh after optimization (this indication is not available if
the optimization step is not performed yet). This value will be the minimum to activate the inflation
method.
48. Go back to the Surface tab.
49. Activate "fluid_group_6" and "fluid_group_7" to check the settings imposed. The number of
viscous layers proposed is 8 (fluid_group_6) and 11 (fluid_group_7) respectively for the two
activated surfaces.
50. Click on Go to start the viscous layer insertion step.
51. Repeat step 34 to step 36 to check the mesh quality after the viscous layers insertion.
We are about to repeat the same actions to set the parameters for the solid block. Please refer to
the previous sections "Mesh Wizard Fluid Block" to find out more about the different steps.
2.10 MESH WIZARD SOLID BLOCK: INITIAL MESH
52. Select the solid block ("blade") from the Active domain drop-down list or by clicking directly
from the graphics area.
53. Left- click the checkbox for Initial mesh in Mesh Wizard. The corresponding step becomes
accessible for the user. The same behavior is applied for the following steps in the Mesh Wizard.
54. Click on Initial mesh and the Initial mesh parameters dialog box appears.
55. Keep the default parameters and click on Ok.
56. Left-click on the Step button in the Mesh Wizard to create the initial mesh with default
parameters.
2.11 MESH WIZARD SOLID BLOCK: ADAPTATION
STEP
57. Left-click the checkbox for Adapt to geometry. Click on Adapt to geometry.
58. Under the Global tab, set the Maximum number of refinements to <4>.
59. Go to the Surface refinement tab.
60. Left-click and drag to select the faces "blade_group_#" from 6 to 13 (or select by using left-
click + <Shift>).
61. Click on the Group button and name this group as <group_1> and press <Enter>.
62. Click on Active to access the refinement parameters.
63. Set the Max nb of refinements to <3>.
64. Activate the Target cell sizes criterion and keep the default values.
65. Select the faces "blade_group_#" from 2 to 5.
66. Group them as "group_2", then click on Active.
67. Set the Max nb of refinements to <4>.
68. Activate the Target cell sizes criterion and keep the default values.
69. Hit the Go button to start the mesh adaptation step.
2.12 MESH WIZARD SOLID BLOCK: SNAPPING &
OPTIMIZATION STEPS
70. Left-click the checkboxes to activate the Snap to Geometry and Optimize steps in the Mesh
Wizard.
71. Keep the default settings for both and launch the mesh generation of these steps by clicking
on the Start button of the Mesh Wizard.
Solid blocks do not need viscous layers for Conjugate Heat Transfer (CHT) computations.
However, grid quality should be checked visually to prevent problems from arising through
the full non-matching boundaries. On the figures below, one can observe that one cell in the
solid part is facing two cells in the fluid part, which is sufficient here.
91
FINE™/Open with OpenLabs™ 7.2 Tutorials
2.13 FULL NON MATCHING BOUNDARIES
(FNMB)
A multi- domain computation needs to transfer data between the different blocks. This transfer is
ensured by one or several FNMB connections, computed by HEXPRESS™.
In this present case, a simultaneous calculation of the flow and temperature within the solid bodies is
performed with a solid- fluid coupling at the thermal connections, represented here by the FNMB.
Besides that, this geometry contains a periodicity by translation. The data transfer is also computed
thanks to an FNMB connection.
72. Go to the Grid/Periodicity... menu.
73. Select the "fluid" and "blade" domains together by dragging the mouse over the 2 domains or
holding <Ctrl> key and select with left-click.
74. Click on New and then on Edit to define a new periodicity.
75. Keep the default periodicity name to <Periodicity_1>.
76. Select TRANSLATION for the Periodicity type and set the Axis to <0 0.12974 0>.
77. Click on Ok to confirm and then click on Close to exit the Periodicity window.
78. Go to Grid/Non Matching Connections... to access the Blocks connections dialog box.
79. Click on the Search Connections button (HEXPRESS™ searches automatically for new
connections). Three connections are found: 1 for the periodicity ("periodic_1") and 2 for the
domains connection ("connection_#").
80. Left-click and drag to select all connections.
81. Click on the Compute button to perform all the FNMB computations.
A visual check can be performed to ensure that the FNMB connections are well computed. Indeed
colors are shown in the graphics area. A yellow color means that the patches have been successfully
connected.
It is also possible to manually edit the FNMB connections by clicking on the Add button and then on
the Edit button. The automatic search, however, is sufficient in this tutorial. It should be also noticed
that the patches involved in the FNMB connections have turned into "SOL*" in the Boundary
conditions settings dialog box (
).
82. Click on Close when the computation is over (all statuses are marked as "Successful").
2.14 SAVE MESH
83. Go to Project/Save as... or click on the Save icon (
) in the Icon bar.
84. Under the "_mesh" folder (if FINE™/Open project), enter the name of the mesh project as
<turbine_MarkII.igg> and hit the Ok or Save button to save the mesh files.
The mesh folder contains the mesh topology, geometry, grid points and the boundary condition
types among others. The files are listed below:
l .bcs: boundary conditions files,
l .dom: geometry files,
l .igg: topology file,
l .hex: grid points files,
l .hxp: extra information for the mesh generation,
l .rep: report file,
l .log: mesh generation information,
l .dist: distance file (prefix is domain name),
l .fnmb: FNMB connections,
l .nmb: Non matching connections,
l .qualityReport: quality report file.
In addition a subdirectory named "cache" contains the resulting mesh files after each step of the
mesh generation (for example "_snap.hex" as resulting mesh after snapping process). It allows for
deleting some steps and coming back to a previous one without generating the necessary steps
again.
85. Click on the Close button.
86. You can save the project (if not done already) and accept to link the new mesh to the project
(if requested).
87. Acknowledge the mesh quality warning and click on Ok.
88. The Mesh properties dialog box appears. Check that the information is correct (keep Grid
units as Meters) and click on Ok.
You are now back to the FINE™/Open interface and you are ready to proceed with the
definition of the "Flow Settings" (p. 98)!
FLOW SETTINGS
A step by step approach is proposed in the following lines. It aims at guiding you through the
various steps that need to be executed to set up and start the computation.
2.15 MANAGE COMPUTATIONS
89. In the Project/Preferences ... menu, change the Calculation accuracy to Full-double-
precision mode. Click on Ok to confirm.
90. In the Computations menu, right- click on the computation name and select Rename .
Rename "computation_ 1" as < Spalart-Allmaras> < Enter> (as a reference to the turbulence
model: "Spalart-Allmaras").
In the Computations menu, the list of computations is shown. It is possible to Rename, to create a
new one by duplicating the highlighted one (New button), to clean the files into the computation
subfolder (Clean button) or just to delete the computation by clicking on Delete.
2.16 SET PHYSICAL CONFIGURATION
91. In the Physical Configuration menu, double left-click on the General Properties menu.
92. Keep Steady mode. Select Fluid block for the "fluid" domain and Solid block for the
"blade" domain.
93. Click on Ok to validate.
94. In the Physical Configuration menu, double left-click on Fluid Model.
95. In the Edit/Select fluid section, click on Select....
The fluid database includes some pre- defined fluids, covering various approximations in fluid
definition such as perfect gas, ideal (real) gas, incompressible fluids and fluids defined as a set of
thermodynamic tables (optional, subjected to a separate license key).
96. Click on the New fluid... button to create a new fluid.
97. Set Fluid name as <Air> - Select Perfect Gas - Click on Next>>.
98. Impose the fluid properties as defined below:
l Reference pressure = <100000> <Enter> [Pa]
l Reference temperature = <773> <Enter> [K]
l Cp = <1009> <Enter> [J/(kg.K)]
l Gamma = <1.36> <Enter>
l Heat conduction law = Prandtl
l Prandtl number = <0.72> <Enter>
l Viscosity law = Sutherland law
l Kinematic Viscosity = <7.7e-5> <Enter>[m2/s]
l Temperature inf = <293.111> <Enter> [K]
l Density inf = <1.0> <Enter> [kg/m3]
l Sutherland temperature = <110.555> <Enter> [K]
99. Click on Finish to select and add the new fluid to the database.
100. Click on Ok to confirm.
101. Click on Close.
102. In the Physical Configuration menu, double left-click on Flow Model.
103. Keep Spalart-Allmaras as the Turbulence model.
104. Change the reference parameters:
l Set Reference length to <0.13> <Enter> [m];
l Set Reference velocity to <106> <Enter> [m/s].
105. Click on Ok to confirm.
Reference variables (length, velocity) are required to estimate the Reynolds number. This number is
used at a few locations inside the flow solver, in particular inside the damping functions related to the
modeling of turbulence down to the walls. The impact of the characteristic variables on the flow
solution is very limited, but it is advised to select values in accordance with reference values of the
geometrical domain and flow conditions. As an example, the reference length may be defined by a
reference diameter or length at inlet and/or outlet of the computational domain, and/or the chord of
the blade (if any). The reference velocity may be set to the averaged inlet velocity
106. In the Physical Configuration menu, double left-click on Solid Model.
107. Set Conductivity to <18.7> <Enter> [W/m.K].
108. Click on Ok.
2.17 BOUNDARY CONDITIONS
109. In the Boundary Conditions menu, double left-click on Boundary Conditions.
110. Under the INLET tab, select Total Quantities Imposed/Mach Number extrapolated as
the inlet boundary condition for patch "fluid_group 3".
111. Impose the following boundary conditions:
l Set Vx/|V| to <1> <Enter> (if necessary),
l Set Vy/|V| and Vz/|V| to <0> <Enter> (if necessary),
l Set Absolute Total Pressure to <334000> <Enter> [Pa],
l Set Absolute Total Temperature to <788> <Enter> [K],
l Set Turbulence Viscosity to <0.0001> <Enter> [m2/s] (if necessary).
112. Click on the OUTLET tab.
113. Keep the outlet boundary condition as Pressure Imposed/Static Pressure Imposed and set
Static Pressure to <167000> <Enter> [Pa].
114. Click on the SOLID tab.
115. Keep the default settings for the FNMB connections ("periodic_1", "connection_1" and
"connection_2").
116. Set Temperature Imposed for the remaining patches and set the following values for Static
Temperature:
l for "blade_group_3": <588> <Enter> [K],
l for "blade_group_4": <621> <Enter> [K],
l for "blade_group_5": <555> <Enter> [K],
l for "blade_group_6": <521> <Enter> [K],
l for "blade_group_7", "blade_group_8", "blade_group_9": <488> <Enter>[K],
l for "blade_group_10", "blade_group_11", "blade_group_12": <455> <Enter> [K].
117. Click Ok to close the window.
2.18 INITIAL SOLUTION
118. In the Initial Solution menu, double left-click on Initial Solution and set the following
values for the fluid part ("fluid"):
l Pressure = <330000> <Enter> [Pa],
l Temperature = <787> <Enter> [K],
l Vx = <110> <Enter> [m/s],
l Vy = <0> <Enter> [m/s],
l Vz = <0> <Enter> [m/s],
l ~Nu/Nu = <50> <Enter>.
119. Click on "blade" and change the Temperature of the blade to <787> <Enter> [K].
120. Click on Ok to close the window.
2.19 NUMERICAL PARAMETERS
121. In the Numerical Parameters menu, double left-click on General Parameters.
122. Check that the Number of grid(s) is set to 4.
The flow solver is based on an explicit
time integration technique, which is accelerated using
dedicated multi- grid methods. To this end, several levels of intermediate grids must be generated
starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
123. Keep Coarse grid initialization active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be
significantly reduced by activating the coarse grid initialization process. In that case, the simulation
starts on the coarsest grid level available, leading to fast convergence. Once it is done, the flow solver
automatically interpolates the current flow solution on the intermediate levels before the iterative
process is restarted. A similar process repeats until the expected finest grid level is achieved. The
iterative process stops when the convergence criterion is reached or the maximum number of
iterations is exceeded.
124. Under the Advanced tab, keep the default settings and click on Ok.
125. In the Numerical Parameters menu, double left-click on Numerical Schemes.
126. Keep the default values for the fluid domain ("fluid").
127. Select "blade" and set the CFL number of the "Numerical scheme" to <1> <Enter>.
The CFL number drives the pseudo- time step selected to reach a steady state solution using the
time-marching method integrated in the flow solver. In combination with the 4-steps Runge-Kutta
integration scheme included in the flow solver, it has a theoretical stability limit close to 2.8.
However, the additional implicit smoothing scheme can increase this value slightly, which justifies the
default value of 3. The default value for CFL number is adequate in most cases but can be
decreased in some circumstances, in particular at off-design conditions or for CHT (Conjugate Heat
Transfer) computations, for the solid block. By default, the CFL number during the coarse grid
initialization is set to 1.
128. Click on Ok.
2.20 OUTPUT PARAMETERS
129. In the Computation Control menu, double left-click on Outputs.
130. Select Internal flow outputs (default) in the Flow configuration area.
By default, depending on the Flow configuration selected, a list of quantities is defined to be
computed in the flow solver. The list can be manually adapted by selecting a quantity in a category
and clicking on the Add --> and <-- Remove buttons.
131. Click on Ok to confirm.
2.21 CONTROL VARIABLES
132. In the Computation Control menu, double left-click on Control Variables.
133. Set the Number of iterations to <1500> <Enter>.
134. Set the Convergence criteria to <-12> <Enter>.
135. Keep the Save solution every to <100> <Enter> iterations.
136. Click on Ok to confirm.
Depending upon the quality of the initial solution, the density of the mesh (number of nodes) and the
complexity of the underlying flow field, from a few hundred to a few thousand iterations are
typically required to reach convergence. The iterative process is stopped once the convergence
criterion is reached over the entire domain or the maximum number of iterations is executed on the
finest grid level.
The Advanced tab contains the list of expert parameters. Please refer to the User Guide to find out
more about the expert parameters.
2.22 SAVE PROJECT & COMPUTATION
137. Click on the Save Project icon to save the project.
138. Click on the Save Selected 'Run' files icon to save the computation.
2.23 START & STOP COMPUTATION
139. Click on the Start Solver icon to launch the computation and click on Ok to run in serial
mode.
The pop- up Task manager window allows following the convergence history of
computation.
the
To save and stop a computation while running, the icon Save Solution And Stop Flow Solver
should be pressed. However, to stop the computation without saving, the Kill Flow Solver icon
should be used.
2.24 MONITORING
The evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out) and/or global
quantities (efficiency, pressure ratio, torque and axial thrust on solid walls selected in the
boundary conditions page) can be performed in the steering. Local and global quantities may also
be added for follow up during the convergence process. However, their representation in the
graphical area will be effective only once they are added, and the history will not be available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out, with satisfactory correspondence (usually less than 0.5%
difference between in/out). To do so, select the inlet and outlet mass flow at once. Information
about the difference is automatically computed.
The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via the icon bar.
The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the
visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated
within the environment and includes numerous tools.
140. To access CFView™ from the FINE™ graphical user interface, press the Start CFView™
icon (
).
You are now entering the CFView™ interface and you are ready to proceed with the "Post
Processing" (p. 118) of the results!
POST PROCESSING
A step by step approach is proposed in the following lines. It aims at guiding you through the
various steps that need to be executed from reading the solution to the extraction of the main
results. CFView™ automatically opens the ".run" file associated with the active computation.
2.25 SELECT SURFACES/QUANTITIES
141. In the Surfaces area, all solid surfaces are selected by default (including FNMB
 in front of the "Mirror" group to see all mirror patches
connections). Left-click on the symbol
included in the group.
142. Left-click + <Ctrl> key on "fluid_group_4" and on "blade_group_1" to highlight them.
143. Right-click to open the pop-up menu and choose Select to activate these surfaces only.
144. Left-click twice on the Z Projection button and then left-click on the Fit the View button
(in the Viewing buttons area).
145. Then go to the Quantities area in the Quick Access Pad.
146. Double left-click on the Static Temperature.
All quantities selected in FINE™ graphical user interface are transferred to CFView™. However,
additional derived output can be accessed directly from the visualization and post- treatment tool,
including vector components, gradients, divergence and curl of selected quantities. New quantities,
defined as an arithmetic combination of existing quantities possibly combined with regular operations
(trigonometric functions, logarithmic functions, ...) can further be created with the Quantity/Field
Data/Define New Quantity... menu.
Once the candidate quantity for visualization is selected, a representation mode should be selected.
Representation is typically executed in the form of color contours (smoothed or stripped) and/or
isolines. CFView™ also includes the possibility to interrogate the flow field locally ("local value")
and create 1D Cartesian plots. Advanced capabilities involving curve and/or surface integration can
also be accessed.
2.26 REPRESENTATION ON MIRROR PATCHES
147. In the Representations area, click on the Contours & Iso-Values section.
148. Click on the Strip Contour button.
149. Then click on the Isolines button to open the Static Temperature Isolines menu.
150. Increase the number of isolines to <21> <Enter> and set the color to Uniform.
151. Click on Apply and then on Close.
152. In the Viewing buttons area, select the Zoom Area button and then left-click and drag the
mouse to draw a square around the leading edge of the blade.
CFView™ gives the possibility to superpose representation modes. In the present case, isolines with
uniform color (black) are superposed to the static temperature field to outline more clearly the
diffusion of the temperature around the blade and the cooling holes. The number and/or increment of
the isolines can be controlled, and the range of application can be modified.
2.27 VALIDATION DATA
Usually, validation data comes from experiments or other computations. They can be used for
comparison with the currently loaded computation. The representation of the validation data
allows to plot experimental data and to compare them with the computational results.
153. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
154. Click on the Default Orientation button (in the Viewing buttons area).
155. As the project is 2D, it is no more possible to use the cutting plane function. In the Surfaces
area, left-click on the symbol
 in front of the "connection_1" and "connection_2" groups to see
all connection patches included in these groups.
156. Left-click + <Ctrl> key on "fluid_group_6 Solid" of connection_1 group and on "fluid_
group_7 Solid" of connection_2 group to highlight them.
157. Right-click to open the pop-up menu and choose Select to activate these surfaces only.
158. In the Quantities area, select the Static Pressure by double-clicking.
159. Go to the Representations area below and click on the Boundary button in the Plots &
Values area. CFView™ plots in a Cartesian plot the selected quantity all around the boundaries
of the selected surfaces.
160. Left-click in the Cartesian plot area to select the view.
161. Left-click on the plot representing the quantity along the external boundary.
162. Right-click and select Curve Type... to modify the plot representation.
163. In the Line area, increase the Thickness to <3>.
164. In the Marker area, left-click on the Visible button to switch off the marker, click on Apply
and then on Close.
165. Double left-click on the abscissa axis to select it.
166. Right-click on the abscissa axis and select Function of X.
167. Right-click on the abscissa axis and select Fit Range.
168. Select the File/Load Validation Data... menu and open "turbine_MarkII_ExpData.dat"
available in "FINE- Open_ Beginner/Tutorial_ 2" folder of the tutorial package ( download
Beginner tutorial archive).
169. Select the Quantity/Validation Data/Static Pressure menu and select the loaded file.
170. Accept the comparison ( Yes ): markers for the experimental data appear alongside the
existing curve for the computational results.
171. Select the File/Print... menu.
172. Click on Ok after defining the picture settings (more details in the User Guide).
173. Click on Ok after selecting the location to save and the name of the picture.
174. Select the File/Quit CFView menu and Yes to leave the CFView™ session.
TUTORIAL 3.
TURBOWIZARD FOR TURBOCHARGERS
is particularly adapted to the use of
This tutorial
the TurboWizard applied to a turbocharger
(volute/impeller). The TurboWizard is designed to effortlessly set up a ready- to- run project of a
turbocharger or centrifugal compressor. In just five main steps, the TurboWizard is able to:
l Import a structured mesh of the impeller generated within AutoGrid5™,
l Read a volute domain file,
l Perform an automatic, unstructured meshing of the volute,
l Merge the meshes of the volute and the impeller, including the creation of the rotor/stator interface
between the impeller and the volute,
l Automatically create a ready- to- run computation in FINE™/Open with OpenLabs™ respecting
user-imposed flow settings.
In this tutorial, the user will learn how to:
l Use the user interface of the TurboWizard,
l Create a project using the TurboWizard,
l Import an existing AutoGrid5™ structured mesh,
l Import an existing domain,
l Clean the geometry of the volute domain,
l Control the refinement level of the mesh of the volute,
l Impose flow settings using the TurboWizard,
l Run a computation created using the TurboWizard,
l Perform automatic post processing of the results using the TurboWizard within CFView™.
The TurboWizard is provided as a beta version. This means that the TurboWizard may still require
additional calibration to be compatible with more applications. The TurboWizard imposes settings
based on the expertise of the developers and users of NUMECA software. However, depending on the
application, users could have different preferred settings that better suit their needs. Sometimes, the
user will be required to change some settings for the mesh generation in HEXPRESS™ or to change
some computational settings in FINE™/Open with OpenLabs™ in order to improve the functionality.
3.1
INTRODUCTION
3.1.1
Prerequisites
This tutorial does not require any particular prerequisite.
3.1.2
Problem Description
The flow in a turbocharger (volute/impeller) is considered here. The turbocharger consists of a
volute and a multisplitter (main blade + splitter) impeller. A steady solution for this configuration
using only one rotor blade channel is considered. Since the periodic angles for the volute and
impeller are different, the full non-matching mixing plane method is used at the rotor/ stator
interface.
The geometric configuration is shown in the following figure.
Air (perfect gas), defined in the fluid database, is used. The conditions imposed at the inlet are a
total pressure of 93,000 Pa and a total temperature of 308 K. The mass flow rate is 0.2 kg/s. The
impeller rotation speed is 115,000 RPM.
3.1.3
Preparation
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Using the TURBO-Wizard under Create a new project to start creating a
new project using the TurboWizard. Click on Ok.
You are now ready to start using the TurboWizard!
Each of the five steps of the TurboWizard is treated separately. The progress through the steps of the
wizard is indicated by the ribbon at
the
TurboWizard in general, or one of its steps, see also the TurboWizard module User Guide.
the top of the window. For more information about
In addition to the TurboWizard, a dialog box with a Resume button will appear to allow to resume
the ongoing TurboWizard after closing it or after a switch to HEXPRESS™ (step 17).
3.2
STEP 1: PROJECT MANAGEMENT
1. Click on Create Project to create a project file and a folder to store the project data.
2. Select your directory of choice to store the project.
3. Enter the project name in the dialog box as compressor.iec and click on Save or Ok.
FINE™/Open with OpenLabs™ will automatically create a project folder called compressor"
which will contain the project file (.iec) and a folder _mesh where the mesh will be stored.
Later, computation folders will appear inside the project folder. It is strongly advised to keep this
file structure all along the project.
4. Change the Geometry Units to mm.
5. Click on Next >> to go to the next step of the TurboWizard.
3.3
STEP 2: COMPUTATION SETTINGS
6. For the Inlet Conditions, impose the following settings:
l Set Total Pressure to <93000> <Enter> [Pa],
l Set Total Temperature to <308> <Enter> [K],
l Set Turbulence Intensity to <10> <Enter> [%],
l Set Turbulence Length Scale to <1e-5> <Enter> [m].
7. For the Turbomachinery Configuration, impose the following settings:
l Set Mass Flow Rate to <0.2> <Enter> [kg/s],
l Set Rotational Speed to <-115000> <Enter> [rpm],
l Keep Rotating Wheel Maximum Radius as <1000> <Enter> [m],
l Set Estimated Pressure Ratio to <2.55> <Enter> [-].
8. For Fluid & Flow Modeling, keep the default settings.
9. Click on Next >> to go to the next step of the TurboWizard.
3.4
STEP 3: BLADE ROWS MESH IMPORT
10. In the section AutoGrid5 Mesh , use the file browser to locate and select impeller.igg
available in the folder FINE- Open_ Beginner/Tutorial_ 3/impeller of the tutorial package
(download Beginner tutorial archive) and click on Open or Ok.
After importing the mesh of the impeller, information about the mesh is displayed.
11. Click on Next >> to go to the next step of the TurboWizard.
3.5
STEP 4: VOLUTE DEFINITION
12. For the Import Option, select Import HEXPRESS Domain . The section Volute Domain
appears.
13. Click on Read Volute Domain File. Locate and select volute.dom available in the folder
FINE-Open_Beginner/Tutorial_3/volute of the tutorial package (download Beginner tutorial
archive) and click on Open or Ok.
14. Click on Clean Volute Domain.
15. Click on Next >> to go to the next step of the TurboWizard.
3.6
STEP 5: VOLUTE MESH GENERATION
16. For the Volute Mesh Refinement Level, select Coarse.
Depending on the selected refinement level, the Volute Mesh Settings will show different values.
These values are used for the mesh generation within HEXPRESS™.
17. Click on Generate HEXPRESS Mesh in order to start the mesh generation for the volute.
Generating the mesh of the volute may require some time depending on the selected refinement level.
When the mesh of the volute has been generated, information about the mesh is displayed. Here, the
user has the option to switch to HEXPRESS™ in order to inspect or make changes to the mesh.
18. Click on Merge Meshes in order to merge the meshes of the impeller and the volute.
Merging the meshes of the impeller and the volute may require some time.
When the meshes have been merged, information about the quality of the global mesh is displayed.
19. Click on Finish to set up the project and switch to FINE™/Open with OpenLabs™. Click on
OK in order to accept the warning about the mesh quality.
20. In the Mesh properties window, change the Grid units to Millimeters. Click on Ok.
You have completed the TurboWizard and you are in the user interface of FINE™/Open with
OpenLabs™. The TurboWizard has created and set up the computation "design_point_1".
21. Before launching the computation, go to the Numerical Parameters menu, double left-click
on General Parametersand select the Advanced tab. Activate the CPU booster in the coarse
grid initialization parameters area and press OK.
22. In the Boundary Conditions menu, double left-click on Boundary Conditions and go to the
OUTLET tab. Deactivate the Constant Pressure During FMG Initialisation button. Click on
OK.
The latest version of FINE™/Open, v7.2, contains a number of changes to ensure a higher level of
robustness. The Turbowizard is not yet adapted to deal with these changes, which may lead to early
crashes in the computation process. In anticipation of the necessary adaptations in the Turbowizard in
the coming version, the user may have to do some changes in the simulation setup to make the
simulation converge. Some examples are: increase the number of iterations per grid level during
coarse grid initialization, decrease the CFL number or (de)activate the CPU booster.
3.7
STARTING THE COMPUTATION
23. Click on the Save Project icon to save the project.
24. Click on the Save Selected 'Run' files icon to save the computation.
25. Click on the Start Flow Solver icon to launch the computation.
26. Click on the Ok button to start the computation in serial mode.
The pop- up Task manager window allows following the convergence history of
computation.
the
To save and stop a computation while running, the icon Save Solution And Stop Flow Solver
should be pressed. However, to stop the computation without saving, the Kill Flow Solver icon
should be used.
Evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/ out for internal
flow) and/ or global quantities (lift, drag and momentum on solid walls selected in the boundary
conditions page) can be performed in the steering. Local and global quantities may also be added
for follow up during the convergence process. However, their representation in the graphical area
will be effective only once they are added, and the past convergence history will not be available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria including:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/ out (for internal flow), with satisfactory correspondence (usually
less than 0.5% difference between in- and outgoing flow). To do so, select the inlet and outlet
mass flow at once. Information about the difference is automatically computed.
The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via the icon bar.
The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the
visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated
within the environment and includes numerous tools.
27. To access CFView™ from the FINE™ graphical user interface, click on the Start
CFView™ icon (
) and then on OK.
3.8
POST PROCESSING USING THE
TURBOWIZARD
The TurboWizard in CFView™ enables automatic post processing of a turbomachinery project. It
consists of four steps, in which the user can select the desired outputs.
Before launching the TurboWizard in CFView™, the user should define one or more cutting planes
on which the results will be computed and displayed. In this tutorial, cutting planes are created at
constant cross stream (M) and radius (R).
28. In the menu bar, click on File/TurboMachinery in order to switch to the TurboMachinery
mode that will open STM views allowing the creation of constant cross stream cutting planes.
29. In the Start Turbo Mode dialog box, click on Load hub and shroud.
impeller_ hub_ shroud.dat available in the folder FINE- Open_
30. Locate and select
Beginner/Tutorial_3/impeller folder of the tutorial package (download Beginner tutorial archive)
and click on Open or Ok. You will return to the Start Turbo Mode dialog box.
31. Click on Ok to start the TurboMachinery mode.
The TurboMachinery mode facilitates the creation of standard views used in turbomachinery
analysis, such as the meridional view and blade-to-blade view.
32. In the menu bar, click on Geometry/Blade to Blade Surface ... to open the Blade to blade
Surface window.
33. For the Surface type, select Cross stream and set the value for M to <0.6>. Next, click on
Apply and then on Save to create and save the cutting plane at M = 0.6. Close the dialog box.
34. Locate the surface CUT1 in the Surfaces section of the Quick Access Pad, right click and
select Rename. Enter the name <Cut at M=0.6> and press <Enter> to confirm.
35. In the tool bar, click on the icon New RTZ View to open a cylindrical view that will allow
the creation of constant radius cutting planes. Then, click anywhere in the graphics window to
define the first corner of the view. Hold down the mouse and drag the mouse to the opposite
corner of the view. Release the mouse in order to create the new view.
36. Maximize the newly created view either by clicking on the Maximize View icon in the
toolbar or by rightclicking anywhere in the view and selecting Maximize View.
37. In the menu bar, click on Geometry/Create Cutting Plane ... to open the Create Cutting
Plane window.
38. Set the values for Point to <0.0355>, <0>, and <0>; and set the values for Normal to <1>,
<0>, and <0>. Then, click on Apply and then on Save in order to create and save the cutting
plane at R = 0.0355. Close the dialog box.
39. Locate the surface CUT2.D1 in the Surfaces section of the Quick Access Pad, right click and
select Rename. Enter the name <Cut at R=0.0355> and press <Enter> to confirm.
40. Close the RTZ view either by clicking on Window/Close in the menu bar or by right-clicking
anywhere in the view and selecting Close View.
41. Activate the 3D view by clicking anywhere in the view. Then, maximize the view either by
clicking on the Maximize View icon in the tool bar or by right-clicking anywhere in the view and
selecting Maximize View.
In some cases, it may be necessary to delete cuts on the volute, such that only the cuts on the impeller
remains. In this case, expand the group "Cut at M=0.6" in the Surfaces section of the Quick Access
Pad, right click on the surface "Cut at M=0.6.D2" and select Delete.
You have now created the impeller cutting planes on which the results of the simulation will be
displayed using the TurboWizard.
42. In the menu bar, click on Macros/TurboWizard in order to open the TurboWizard in
CFView™.
43. The first step is to create a configuration file in which the user-inputs of the TurboWizard are
saved. Click on Create new configuration file.
44. Select your directory of choice and provide a name for the configuration file, for example
< compressor.in >. Click on Save or Ok to create the configuration file and to return to the
TurboWizard.
45. Click on Next >> to go to the second step of the TurboWizard.
46. Click on Choose stations on which to perform averages.
47. In the Select stations dialog box, activate the surfacic average for "Cut at M=0.6" and "Cut at
R=0.0355". Furthermore, activate the azimuthal average for "Cut at R=0.0355". Click on OK to
confirm your selection.
48. Click on Choose quantities to average.
49. In the Select quantities to average dialog box, activate the Area average for Static
Temperature, Static Pressure, and Absolute Total Pressure. Furthermore, activate the Mass
average for Absolute Total Temperature and Absolute Total Pressure . Click on OK to
confirm your selection.
50. Click on Next >> to go to the third step of the TurboWizard.
51. In the section Hub & Shroud File Selection , use the file browser to locate and select
impeller_hub_shroud.dat available in the folder FINE-Open_Beginner/Tutorial_3/impeller of
the tutorial package (download Beginner tutorial archive) and click on Open or Ok.
52. In the section Span heights (%), define spanwise locations at 10 %, 50 %, and 90 %. Use the
plus button to add more sections.
53. Click on Choose blades on which to sample local profiles.
54. In the Select blades dialog box, select all blades by clicking on select all. Click on OK to
confirm your selection.
55. Click on Choose quantities to sample on blades.
56. In the Select quantities dialog box, select Static Pressure. Click on OK to confirm your
selection.
57. Click on Start to start generating the outputs.
The TurboWizard in CFView™ automatically generates plots based on the selected outputs by the
user. The plots and the data files of these plots are stored in the same location as where the
TurboWizard configuration file is saved in step 43.
58. In the final step of the TurboWizard in CFView™, the generated outputs can be selected and
displayed.
59. In the section Station averages outputs, select all for the station and select Absolute Total
Temperature for the quantity. In the section Blade profiles outputs, select all for the heights,
select row_1_flux_1_Main_Blade for the blade and select Static Pressure for the quantity.
60. Click on Show buttons to display the selected plots.
61. Click on Close to close the TurboWizard.
ADVANCED
The following are Advanced level tutorials for FINE™/Open with OpenLabs™.
TUTORIAL 1.
DLR-F4 WING BODY
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l Spatial discretization of the flow equations,
l Flow computation,
l Visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated. The unstructured CFD package consists of the
following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
This tutorial is particularly adapted to a 3D internal application. It makes use of FINE™/Open with
OpenLabs™ including HEXPRESS™ and CFView™.
The following steps will be discussed:
l Use HEXPRESS™ user interface,
l Import an existing domain,
l Visualize a mesh,
l Progress in the mesh wizard to generate the mesh,
l Control the quality of the mesh,
l Set up a computation in FINE™/Open interface,
l Start/stop the computation,
l Visualize the results with CFView™.
1.1
INTRODUCTION
1.1.1
Prerequisites
This tutorial does not require any particular prerequisite but it is strongly recommended for
beginners to perform the Beginner level tutorials.
1.1.2
Problem Description
In order to study the flow around a subsonic transport type aircraft, the 3D geometry of the DLR-
F4 test case is here considered. The objective is to demonstrate the ability of FINE™/Open to
predict aerodynamic effects in a local flow in M-range 0.75-0.8 with supersonic flows regions on
upper wing terminated by weak shock waves as well as a small separation close to the trailing
edge.
The geometric configuration is shown in the following figure.
(picture from A selection of Experimental Test Cases for the Validation of CFD Codes - AGARD
ADISORY REPORT NO 303, Volume II)
Air, modeled as a perfect gas with a constant kinematic viscosity of 1.21e-5 m²/s, is considered at
293K and at density of 1.2kg/m3 . Static-to-static pressure conditions are imposed as external
conditions (100909.2Pa), with a speed of 257.25m/s. The Mach number is then approximately
0.75 and the Reynolds number, determined using the velocity and the chord-length, is about 3e6.
1.1.3
Preparation
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <dlr-f4.iec> and click on Save or Ok.
FINE™/Open will automatically create a project folder called " dlr-f4" which will contain the
project file (" .iec") and a folder " _mesh" where the mesh will be stored. Later, computation
folders will appear inside the project folder. It is strongly advised to keep this file structure all
along the project.
l Click on Yes to start HEXPRESS™ unstructured mesh generator.
You are now ready to start the "Mesh Generation" (p. 161) process and mesh the DLR-F4
aircraft!
MESH GENERATION
HEXPRESS™ graphical user interface allows to visualize the geometry and mesh of the internal
or external test case in a graphics area. The access to main menu and controls is proposed through
a menu bar and a quick access pad, and is completed with a tool/icon bar and a control area
(including the keyboard input area).
1.2
OPEN EXISTING DOMAIN FILE
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined. That is why the tutorial starts from the domain file ".dom". It should be
noticed that the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL),
import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS dialog box.
2. Locate and select "dlrf4.dom" in the dialog box (download Advanced tutorial archive) and
click on Open or Ok.
1.3
SET BOUNDARY CONDITIONS
3. Go to the Grid/Boundary Conditions... menu or click on Boundary Conditions icon (
in the Tool bar and set the boundary conditions using the Set face type button :
)
l set "exterior_#" for 1 to 5 as external ("EXT");
l set "mirror" as mirror ("MIR");
l keep "facet", "extrados", "tail", "body" and "intrados" as solid ("SOL").
4. Close the dialog box.
1.4
MESH WIZARD : INITIAL MESH
5. Left- click the check box for Initial mesh in Mesh Wizard to activate the step. The
corresponding step is accessible for users at once. The same behavior is applied for the following
steps in the Mesh Wizard.
6. Click on Initial mesh and the Initial mesh parameters dialog box appears.
7. In Set the number of divisions along cartesian axis section,
<100,000>.
impose Nb of cells to
8. Click on Auto button.
By using the Auto button, HEXPRESS™ computes the required number of cells in each direction to
get an isotropic mesh. The total number of cells may then vary (in this case the number of cells is
adapted from 100,000 to 97,556).
9. Click on OK and on Step button from the Mesh Wizard to create the initial mesh with 97,556
cells.
Number of cells in the initial mesh can be increased in order to impose a smaller size to the biggest
cell that will be included in the computational domain.
1.5
MESH WIZARD : ADAPTATION STEP
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selection in this action directly dictates the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming.
in terms of user
important
During the first one, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry
dependent criteria. With the second step, it removes cells intersecting the geometry or located outside
the computational domain.
10. Left-click the check box for Adapt to geometry in Mesh Wizard to activate the step.
11. Click on Adapt to geometry and the Refinement and trimming parameters dialog box
appears.
12. Under Global tab, set the Maximum number of refinements to <10>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement in one or several different
directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive
refinements. This may result in an exponential growth of the total number of cells in the mesh, even
though the refinement may be confined to some areas of the computational domain. To bound the
number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may therefore alter the success of the meshing process. More details are available in the User Manual.
13. Left-click on Curve refinement tab.
The refinement process is defined by three classes of criteria: curve, surface and volume criteria.
Surface criterion is considering cells which are intersecting surfaces as candidates for refinement.
Three criteria are implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
14. Use left-click and <Ctrl> to select in the curve (edge) list "Curve 17", "Curve 19", "Curve
48".
15. Click on Active to access the refinement parameters.
16. Set the Max nb of refinements to <8>.
17. Select the Target cell sizes criterion and keep the default values.
The Maximum number of refinements per surface ultimately controls the refinement of cells
intersecting that surface (if it is presenting a value lower than the Global maximum number of
refinements from the Global parameters tab). This parameter supersedes any other selected
adaptation criteria. Fine tuning of this parameter is useful when it may be difficult to determine the
appropriate Target cell size, or if the Distance and Curvature criteria yield a prohibitive number
of cells. The default value (10000) is an arbitrary large number such that the criteria are controlled by
the Global maximum number of refinements.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell sizes for each
intersecting a geometrical surface are compared to the
geometrical surface. The size of a cell
prescribed user target and the cell is refined until its actual size is lower than the target.
18. Repeat step 14 to step 17 for "Curve 218" except setting the Maximum number of
refinements to <10>.
19. Go to Surface refinement tab.
Surface criterion considers cells intersecting surfaces as candidates for refinement. Three criteria have
been implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
Volume criterion (found in Box refinement tab) considers cells intersecting or located inside a
three- dimensional volume as candidates for refinement if their cell size is larger than some user
prescribed target size.
20. Select "facet" from the surface list (tip of the wing).
21. Click on Active.
22. Set the Max nb of refinements to <8>.
23. Select the Target cell sizes criterion and keep the default values.
24. Repeat step 20 to step 23:
l For "extrados" and "intrados" (wing) except setting the Max nb of refinements to <7> and
adding Curvature criterion,
l For "tail" except setting the Max nb of refinements to <10>,
l For "body" except setting the Max nb of refinements to < 6 > and adding Curvature
criterion.
25. Left-click on Trimming tab.
26. Keep default Not used for trimming for all EXT and MIR faces to keep cells on the
selected faces at the end of the adaptation step.
27. Click on Go to launch the adaptation step.
1.6
MESH WIZARD : SNAPPING STEP
28. Left-click the check box for Snap to geometry in Mesh Wizard.
29. Click on Snap to geometry and the Snapping parameters dialog box appears.
30. Left-click on Advanced >>> button. It gives access to three extra tabs (Global parameters,
Curve snapping and Buffer insertion).
31. Activate Insert buffer on faces not used for trimming under Global parameters tab.
The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh
adaptation on the surface to obtain a good quality body conforming mesh. In addition to a simple
lower
projection on the geometry,
dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee
that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner
of the geometry and that a path of mesh edges is attached to the curve.
this action involves sophisticated algorithms to recover
Layers of additional cells (buffer insertion) are introduced into the mesh also on faces not used for
trimming as the symmetry plane (when option Insert buffer on faces not used for trimming is
active) to create a body conforming mesh.
Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
32. Left-click on Ok to proceed.
1.7
MESH WIZARD : OPTIMIZATION STEP
33. Left-click the check box for Optimize in Mesh Wizard.
34. Left-click on Optimize and the Optimization parameters dialog box appears.
35. Keep all default settings and click Ok to proceed.
36. Click on Start in Mesh Wizard to snap and optimize the mesh.
The mesh obtained after the snapping step may involve poor quality cells usually located close to
corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
37. Left-click on Mesh quality icon (
) in the Tool bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e. cells with a
negative volume. Negative cells are not allowed in the final mesh to be used for the computation.
Concave or twisted cells are less likely to present robustness or stability issues for solvers,
however they should be prohibited.
When negative, concave or twisted cells are detected, they should be usually removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
38. Check the mesh quality by using the Criterion drop-down list for the following criteria :
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are
presented through histograms. Each bar represents the number of cells whose criterion value is
included in the bar interval. By left-clicking on one of the bars, the corresponding cells are
displayed in the graphics area. Cells are displayed in a color varying depending on the value of
the quality criterion. The Show markerscheck button activates the display of circle markers for
each vertex of the displayed cells, which facilitates the localization of the selected cells.
39. After checking the mesh quality, click on Close to exit.
1.8
MESH WIZARD: VISCOUS LAYERS
INSERTION STEP
40. Left-click the check box for Viscous layers in Mesh Wizard.
41. Left-click on Viscous layers and the Viscous layers insertion parameters dialog box
appears.
42. Under Global tab, keep Fixed first layer thickness Method --> Inflate viscous layers -->
Floating number of layers active. Do not change the range, it will be adapted automatically.
43. Go to the Surface tab.
44. Select all surfaces of the aircraft geometry of the list: left-click on first surface ("facet") and
left-click + <Shift> on last surface ("intrados").
45. Click on Active to access the parameters for viscous layers insertion.
46. Left-click on the Compute button. This button opens a pop up window to compute the
necessary first layer thickness.
The width of the first cell close to the wall must be selected with care since the quality of the flow
solution will often depend upon the capture of the flow phenomena inside the boundary layers which
develop along the solid walls. Depending upon the turbulence model selected, NUMECA recommends
to locate the nearest grid point along the wall, at a distance that corresponds to parietal coordinate y+
ranging from 1- 5 (low Reynolds number models) or 30- 50 (high Reynolds number models).
Assuming thermal effects must be modeled accurately, y+ can reach values as low as 0.1.
The relation between the parietal coordinate y+ and width of the first cell close to the wall y is driven
by the Blasius equation, expressed as follows for turbulent flows :
where :
l Ywall is the distance of the nearest grid point to the wall (in meter),
l Vref is a reference velocity of the flow, for instance the inlet velocity (in m/s),
l ν is the kinematic viscosity of the fluid (in m²/s), i.e. the dynamic viscosity divided by the density,
l Lref is a reference length of the test case (in meter),
l Y1
+ is a non-dimensional value.
In the present case, Vref = 257.25 m/s ; Lref = 0.1412 m ; ν = 1.21e-05 m²/s. To get Y1
the wall, it comes Ywall = 8.3483e-5 m.
47. Set the inputs accordingly as shown below and click on Apply to validate the first layer
thickness.
+ = 50 at
48. Select "facet" in the list with a left-click. Keep 1.2 for the stretching ratio and click on
Apply button to use the advised value of viscous layers (8). HEXPRESS™ gives an indication
about the appropriate number of viscous layers to insert. This number is computed based on the
current mesh after optimization (this indication is not available if the optimization step is not
performed yet). This value will be the minimum to activate the inflation method.
49. Repeat the above step for "extrados", "tail", "body" and "intrados" to use advised value of
viscous layers (from 4 to 15 depending of the selected surface).
50. Click on Go to start the viscous layer insertion step.
In the viewing buttons, the cutting plane icon (
) will perform a cut inside the mesh to visualize
the quality and viscous layers insertion along the wing as presented below. Cutting plane was
performed at constant Y (press <y>) and translated (middle-click) on the wing
51. Repeat step 37 to step 39 to check the mesh quality after viscous layers insertion.
1.9
SAVE MESH
52. Impose mirror type of periodicity so that users are allowed to plot full plane within
CFView™:
l Go to Grid/Periodicity... menu.
l Click on New, and then Edit to define a new periodicity.
l Set the periodicity name to <Mirror>.
l Select MIRROR for the Periodicity type and set the Periodicity parameters (Origin and
Axis) respectively to <0 0 0> and <0 1 0>.
l Click on Ok to confirm and then close the Periodicity dialog box.
53. Go to Project/Save as... or click on the Save icon (
) in icon bar.
54. Under the "_mesh" folder (if FINE™/Open project), enter the name of the mesh project as
<dlr-f4.igg> and press Ok or Save to save mesh files.
The mesh folder contain the mesh topology, geometry, grid points and the boundary condition
types among other. The files list is written below :
l .bcs : boundary conditions files,
l .dom : geometry files,
l .igg : topology file,
l .hex : grid points files,
l .hxp : extra information for the mesh generation,
l .rep : report file,
l .log : mesh generation information,
l .dist : distance file (prefix is domain name),
l .fnmb : FNMB connections,
l .nmb : Non matching connections,
l .qualityReport : quality report file.
In addition a subdirectory named "cache" contains resulting mesh files after each step of the mesh
generation (for example "_snap.hex" as resulting mesh after snapping process). It allows to delete
some steps and come back to a previous one without generating the necessary steps again.
55. Click on the Close button.
56. You can save the project (if not done already) and accept to link the new mesh to the project
(if requested).
57. Acknowledge the warning that solver precision should be changed and click on Ok.
58. The Mesh properties dialog box appears. Check that the information is correct (keep Grid
units to Meters) and click on Ok.
You are now back to the FINE™/Open interface and ready to proceed with the "Flow
Settings" (p. 181)!
FLOW SETTINGS
A step by step approach is proposed in the following lines. It aims at driving you through the
various steps that need to be executed to set up and start the computation.
1.10 SET SOLVER PRECISION
59. In Project/Preferences... select Full-double-precision mode and click on Ok.
1.11 MANAGE COMPUTATIONS
60. In the Computations menu, right-click on the computation name and select Rename.
61. Rename "computation_ 1" as < SA_ EXT_ angle- 0.68 > < Enter > (as a reference to the
turbulence model: "Spalart-Allmaras Extended Wall Function" and the angle of attack used in this
tutorial).
In the Computations menu, the list of computations are shown. It is possible to Rename, creates a
new one by duplicating the highlighted one (New button) or just delete the computation by clicking
on Delete.
1.12
SET PHYSICAL CONFIGURATION
62. In the Physical Configuration menu, double left-click on General Properties menu.
63. Keep Steady mode and Fluid block active for the domain "3".
64. Click on Ok to validate.
65. In the Physical Configuration menu, double left-click on Fluid Model.
66. In the Edit/Select fluid section, click on Select....
67. Click on New fluid... to create a new fluid.
68. Set Fluid name as <Air> - Select Perfect gas - Click on Next>>.
69. Impose fluid properties as defined in figure below.
70. Click on Finish to select and add new fluid in database.
71. Click on Ok to confirm.
72. Click on Close.
73. In the Physical Configuration menu, double left-click on Flow Model.
74. Select Spalart-Allmaras (Extended Wall Function) as Turbulence model.
75. Change the reference parameters:
l Set Reference length as <0.1412> <Enter> [m];
l Set Reference velocity as <257.25> <Enter> [m/s].
76. Click on Ok to confirm.
1.13
BOUNDARY CONDITIONS
77. In the Boundary Conditions menu, double left-click on Boundary Conditions.
78. Select all solid patches (left-click on first one and left-click + <Shift> on last one) under the
SOLID tab.
79. Keep Adiabatic for all solid patches and activate Compute force and torque.
80. Under EXTERNAL tab, select all patches (left-click on first one and left-click + <Shift> on
last one). Select Mach Number and Velocity Angle as external boundary conditions for all the
patches.
81. Impose same boundary condition on all patches:
l Set Static Pressure to <100909.2> <Enter> [Pa],
l Set Static Temperature to <293> <Enter> [K],
l Set Mach number to <0.75> <Enter> (corresponds to a free stream velocity around 257.25
[m/s]),
l Set arctg(Vy/Vx) to <0> <Enter> [rad] and arctg(Vz/Vx) to <-0.0118682> <Enter> [rad]
(corresponds to an angle of attack of -0.68 [degrees]),
l Set Turbulent Viscosity to <1.21e-5> <Enter> [m²/s].
82. Click Ok to close the window.
1.14
INITIAL SOLUTION
83. In the Initial Solution menu, double left-click on Initial Solution.
84. Keep Constant values and Coordinate system as Cartesian.
85. Set the values accordingly:
l Pressure = <100909.2> <Enter> [Pa],
l Temperature = <293> <Enter> [K],
l Vx = <257.23> <Enter> [m/s],
l Vy = <0.0> <Enter> [m/s],
l Vz = <-3.05> <Enter> [m/s],
l Nut/Nu = <50> <Enter> .
86. Click on Ok to close the window.
1.15 NUMERICAL PARAMETERS
87. In the Numerical Parameters menu, double left-click on General Parameters.
88. Check if the Number of grid(s) is set to 4.
The flow solver is based on an explicit time integration technique, which is accelerated by means of
dedicated multi- grid methods. To this end, several levels of intermediate grids must be generated
starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
89. Keep Coarse grid initialization active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be
significantly reduced by activating the coarse grid initialization process. In that case, the simulation
starts on the coarsest grid level available, leading to fast convergence. Once it is done, the flow solver
automatically interpolates the current flow solution on the intermediate levels before the iterative
process is restarted. A similar process repeats until the expected finest grid level is achieved. The
iterative process stop when the convergence criteria is reached or the maximum number of iterations
is exceeded.
90. Keep the defaults and click on Ok.
91. In the Numerical Parameters menu, double left-click on Numerical Schemes.
92. Keep the default values for the domain "3".
The CFL number drives the pseudo- time step selected to reach a steady state solution using the
time-marching method integrated in the flow solver. In combination with the 4-steps Runge-Kutta
integration scheme included in the flow solver, it has a theoretical stability limit close to 2.8.
However, the additional implicit smoothing scheme can increase this value slightly, which justifies the
default value of 3. The default value for CFL number is adequate in most cases, but can be
decreased in some circumstances, in particular at off-design conditions or for CHT computations, for
the solid block.
93. Click on Ok.
1.16 OUTPUT PARAMETERS
94. In the Computation Control menu, double left-click on Outputs menu.
95. Select External flow outputs in Flow configuration area.
By default depending of the Flow configuration selected, a list of quantities is defined to be
computed in the flow solver. The list can be manually adapted by selecting a quantity in a category
and clicking on the Add --> and <-- Remove buttons.
96. Select Turbulence under Categories. Select Y+ and Wall Distance and click on Add -->
button.
97. Go to External flow tab and adapt Lift direction to < 0.01186 0 0.99993 > and Drag
direction to <0.99993 0 -0.01186>.
98. Click on Ok.
1.17 CONTROL VARIABLES
99. In the Computation Control menu, double left-click on Control Variables menu.
100. Set the Number of iterations to <850> <Enter>.
101. Set the Convergence criteria to <-7> <Enter>.
102. Save the solution at every <200> <Enter> iterations.
103. Click on Ok to confirm.
1.18
LAUNCHING MODE
104. In the Computation Control menu, double left-click on Launching Mode menu.
105. Select Parallel in Launching mode area.
106. Increase the Number of partitions to <4> <Enter>.
107. Click on Ok to confirm.
On Windows the account needs to be configured to be able to run parallel computations
(see: Windows User Configuration).
1.19
SAVE PROJECT & COMPUTATION
108. Click on Save Project button to save the project.
109. Click on Save Selected 'Run' files button to save the computation.
1.20 START & STOP COMPUTATION
110. Click on Start Solver button to launch the computation dialog box to set-up parallel settings
is appearing.
111. Click on Parallel settings... button to adapt if needed the host of each partition.
112. Click on Ok twice to confirm and start the process in parallel.
To save and stop a computation while running, the button Suspend Solver should be pressed.
However, to stop the computation without saving, the Kill Solver button should be used.
The pop up Task manager window allows following the convergence history of the
computation.
1.21 MONITORING
Evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out for internal
flow) and/or global quantities (lift, drag and momentum on solid walls selected in the boundary
conditions page) can be performed in the steering. Local and global quantities may also be added
for follow up during the convergence process. However, their representation in the graphical area
will be effective only once they will be added, and the history will not be available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude);
l complete stabilization of global performances;
l stabilization of mass flow in/out (for internal flow), with satisfactory correspondence (usually
less than 0.5% difference between in/out). To do so, select the inlet and outlet mass flow at
once. An information about the difference is automatically computed.
The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations, can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via the icon bar.
The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the
visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated
within the environment and includes numerous tools.
113. To access CFView™ from the FINE™ graphical user interface, press the CFView™ icon (
).
You are now entering to the CFView™ interface and ready to proceed with the "Post
Processing" (p. 200) of the results!
POST PROCESSING
A step by step approach is proposed in the following lines. It aims at driving you through the
various steps that need to be executed from reading the solution to the extraction of the main
results. CFView™ automatically opens the file ".run" file associated with the active computation.
1.22 SELECT SURFACES/QUANTITIES
114. In the Surfaces section, all solid surfaces are selected by default.
115. Go to Quantities section in the Quick Access Pad.
116. Double left-click on the Wall Distance.
All quantities selected in FINE™ graphical user interface are transferred to CFView™. However,
additional derived output can also be accessed directly from the visualization and post-treatment tool,
including vector components, gradients, divergence and curl of selected quantities. New quantities,
defined from existing quantities combined by regular operations (arithmetic functions, trigonometric
functions, logarithmic functions,...) can be created with the Quantity/Field Data/Define New
Quantity... menu.
117. Check full range of the Wall Distance quantity in Information Area.
118. To limit the range to the selected surfaces (all "solid" surfaces), click on the Colormap
Optimum Range icon (
) and check that the range is going from 0 to 0 on solid walls.
When selecting all "solid" surfaces (when not involved in FNMB connections) the Wall Distance
should be equal to 0. If not that means that the wall distance computation in flow solver is incorrect
and should be corrected (more details in User Manual).
119. Go to Quantities section in the Quick Access Pad.
120. Double left-click on the Y+.
icon) of the Y+ quantity in
121. Check range (limited to "solid" surfaces with
Information Area to check that the imposed first cell size is in agreement with the turbulence
model used. In this tutorial, the averaged value of Y+ is about 29 and in agreement with the
"Spalart-Allmaras Extended Wall Function" turbulence model used.
122. Go to Quantities section in the Quick Access Pad.
123. Double left-click on the Static Pressure.
Once the candidate quantity for visualization is selected, a representation mode should also be
selected. Representation is typically executed in the form of color contours (smoothed or stripped)
and/or isolines. CFView™ also includes the possibility to interrogate the flow field locally ("local
value") and create 1D Cartesian plots. Advanced capabilities involving curve and/or surface
integration can also be accessed.
1.23 REPRESENTATION ON SOLID PATCHES
124. Click on Representations/Contours & Iso Values section and then on Strip Contour icon
to display the selected quantity.
125. Click on the icon Isolines.
126. Increase the number to <21> <Enter> isolines.
127. Select Uniform.
128. Click on Apply and then on Close.
129. Select Geometry/Repetition on/off menu to plot the whole plane.
1.24 REPRESENTATION ON CUTTING PLANE
(VECTOR LINES)
130. Click on Update/Delete/All to delete all previous manipulations in the Graphics area.
131. Select Geometry/Repetition on/off menu to hide the repetition.
132. Under Representations/Grid section, click on Render Gouraud icon to activate the
shading on solid surfaces.
133. Click on Geometry/Create Cutting plane... menu.
134. Enter the X, Y, Z values for Point and Normal as shown on the following figure.
135. Select Geometry and click on Apply to pre-visualize the cutting plane.
136. Click on Save to add this cutting plane to the Surfaces section in Quick Access Pad, that
will be activated by default.
137. Click on Close.
138. In Surfaces section, select "CUT1" by left-click, right-click and Select.
139. Double left-click on the quantity Vxyz (Velocity).
140. Click on Representations/Vector Lines section.
141. Click on Vector Lines Parameters icon.
142. Under the tab General, change the Direction to both, Representation to line, Mode to
surface and the Color to Uniform.
143. Click on Apply button to validate and then on Close.
144. Click on the icon Vector Lines from Section.
145. Keep "5" in the keyboard input area to draw 5 vector lines per section.
146. With the mouse, draw a line (left-click and drag) on the cutting plane close to the plane body
and wing to plot the vortex behind the tip of the wing.
147. Select Geometry/Repetition on/off menu to plot the whole plane.
1.25 REPRESENTATION ON A CARTESIAN PLOT
(VALIDATION DATA)
The objective is to compare computational results to experimental data (pressure coefficient (Cp)
along the wing at a specific location Eta = 0.331 or y = -0.19447 m).
148. Click on Quantity/Field Data/Define New Quantity... to open the dialog box allowing to
create a new quantity based on existing ones.
149. Keep Scalar and Field active under Quantity Type.
150. Set Name as <Cp>.
151. Set Definition as <(100909.2-Static Pressure)/(0.5*1.2*257.25*257.25)>.
The pressure coefficient Cp is defined as:
where p is the static pressure,
density (1.2 kg/m³) and
is the freestream pressure (100909.2 Pa),
is the freestream fluid
is the freestream velocity of the fluid or the velocity of the body through
the fluid (257.25 m/s).
152. Click on Apply to add the new quantity.
153. Click on Close.
154. In Surfaces section (Quick Access Pad), select all solid patches:
l left-click on first solid patch;
l left-click+<Shift> on last solid patch;
l right-click and Select.
155. Click on Z-projection icon in the viewing buttons.
156. Click on Representations/Plots & Values section.
157. Click on Section button.
158. Set X1 Y1 Z1 X2 Y2 Z2 to <0 -0.19447 0 0.5 -0.19447 0> in the keyboard input area.
159. Left-click on Cartesian plot (highlighted with red border).
160. Left-click on X-axis.
161. Right-click and select Function of X.
162. Right-click and select Fit Range.
163. Left-click on one of the curves.
164. Right-click and select Curve Type to whole section.
165. Under Marker tab, deactivate Visible, Apply and Close.
166. Click on File/Load Validation Data... menu and open "dlrf4_ onera_ ExpData.dat"
(contains experimental data of Cp at Eta = 0.331) available in the "FINE- Open_
Advanced/Tutorial_1" folder of the tutorial package (download Advanced tutorial archive).
167. Click on Quantity/Validation Data/dlrf4_onera_ExpData menu.
168. Accept the comparison (yes): markers for experimental data and curve for computational
results.
169. Select File/Print... menu.
170. Click on Ok after defining the picture settings (more details in User Manual).
171. Click on Ok after selecting the location to save and the name of the picture.
172. Select File/Quit CFView to leave CFView™ session.
TUTORIAL 2.
CENTRIFUGAL COMPRESSOR (VOLUTE-
IMPELLER)
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l Spatial discretization of the flow equations,
l Flow computation,
l Visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated. The unstructured CFD package consists of the
following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
This tutorial is particularly adapted to a 3D centrifugal compressor application (volute/impeller). It
makes use of FINE™/Open with OpenLabs™ including HEXPRESS™ and CFView™.
The following steps will be discussed:
l Use HEXPRESS™ user interface,
l Import an existing domain,
l Progress in the mesh wizard to generate the mesh,
l Control the quality of the mesh,
l Import an existing AutoGrid5™ structured mesh,
l Add a rotor-stator interface,
l Set up a computation in FINE™/Open interface,
l Use CPU Booster,
l Start/stop the computation,
l Visualize the results with CFView™.
2.1
INTRODUCTION
2.1.1
Prerequisites
This tutorial does not require any particular prerequisite but it is strongly recommended for
beginners to perform the Beginner level tutorials.
2.1.2
Problem Description
The flow in a 3D centrifugal compressor (volute/impeller) is considered here. The compressor
consists of a volute and a multisplitter (main blade + splitter) impeller. A steady solution for this
configuration using only one rotor blade channel is considered. Since the periodic angles for the
volute and impeller are different, the full non-matching mixing plane method is used at the
rotor/stator interface.
The geometric configuration is shown in the following figure.
Air (perfect gas), defined in the fluid database, is used. A mass flow condition is imposed at the
inlet with the mass flow rate of 0.2 kg/s and the static temperature of 293 K. The static pressure is
imposed at the outlet with the value of 200,000 Pa and the impeller rotation speed is 115,000
RPM.
The objective is to demonstrate how to mesh a volute/ impeller configuration and the ability of
FINE™/Open to predict the flow in a volute/ impeller configuration.
2.1.3
Preparation
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <compressor.iec> and click on Save or Ok.
FINE™/Open will automatically create a project folder called "compressor" which will contain
the project file (".iec") and a folder "_mesh" where the mesh will be stored. Later, computation
folders will appear inside the project folder. It is strongly advised to keep this file structure all
along the project.
l Click on Yes to start HEXPRESS™ unstructured mesh generator.
You are now ready to start the "Mesh Generation" (p. 214) process for the volute and the
impeller!
MESH GENERATION
HEXPRESS™ graphical user interface allows you to visualize the geometry and mesh of the
internal or external test case in a graphics area. The access to the main menu and controls is
provided by a menu bar and a quick access pad, and is completed with a tool/icon bar and a
control area (including the keyboard input area).
HEXPRESS™ allows meshing of multiblock configurations. The user can generate the mesh for
each block. Alternatively, the user can import several existing projects to make a multiblock mesh.
Both HEXPRESS™ and IGG™ (including AutoGrid5™) projects can be imported. In this
tutorial, the mesh in the volute will be generated in HEXPRESS™ while the mesh in the impeller
will be converted in HEXPRESS™ from an existing AutoGrid5™ project.
2.2 OPEN THE EXISTING VOLUTE DOMAIN FILE
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined. That is why the tutorial starts from a domain file ".dom". It should be
noticed that the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL),
import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as execute Python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS dialog box.
2. Locate and select "volute.dom" in the dialog box (download Advanced tutorial archive) and
click on Open or Ok.
2.3
VISUALIZATION
Use the viewing buttons at the bottom of the interface to display the geometry as preferred. In the
View subpanel from the Quick Access Pad, it is possible to:
l Left-click on the Mesh icon (
) to hide/show mesh (toggle),
l Left-click on the Solid icon (
) to hide/show faces (toggle),
l Right-click on the Face icon (
) or left-click on the Face viewer icon (
) to open the
Face Viewer window.
Face selection can be done interactively in the graphics area or thanks to the Face Viewer
window.
2.4
SET VOLUTE BOUNDARY CONDITIONS
3. Go to the Grid/Boundary Conditions... menu or click on the icon
set the boundary conditions, using the Set face type button:
in the icon bar and
l set "volute_group_0" as outlet ("OUT");
l set "volute_group_#" for 1 to 3 as solid ("SOL");
l set "volute_group_#" for 4 to 5 as inlet ("INL").
4. Close the dialog box.
2.5 MESH WIZARD VOLUTE BLOCK : INITIAL
MESH
5. Left- click the checkbox for Initial mesh in Mesh wizard to activate this step. The
corresponding step becomes accessible for the user.
6. Left-click on Initial mesh and the Initial mesh parameters dialog box appears.
7. In the Set the number of cells along cartesian axis section, impose X axis to <28>, Y axis to
<30>, Z axis to <8>, which corresponds to 6720 cells.
8. Click on Ok and on the Step button in the Mesh Wizard to create the initial mesh.
The number of cells along the X/Y/Z axis in the initial mesh can be increased in order to impose a
smaller size to the biggest cell that will be included in the computational domain.
2.6 MESH WIZARD VOLUTE BLOCK :
ADAPTATION STEP
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selected in this action directly dictate the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming.
regarding the user
important
During the first step, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry-
dependent criteria. With the second step, it removes the cells intersecting the geometry or located
outside the computational domain.
9. Left-click the checkbox for Adapt to geometry. The corresponding step becomes accessible
for the user.
10. Left-click on Adapt to geometry to open the Refinement and trimming parameters dialog
box.
11. Under the Global tab, set the Maximum number of refinements to <3> <Enter>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement in one or several different
directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive
refinements. This may result in an exponential growth of the total number of cells in the mesh, even
though the refinement may be confined to some areas of the computational domain. To bound the
number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may alter the success of the meshing process. More details are available in the User Guide.
12. Left-click on the Curve refinement tab.
The adaptation process is defined by three classes of criteria: curve, surface and volume criteria. The
curve criterion considers cells which are intersecting edges as candidates for refinement. Three criteria
are implemented and are respectively based on:
l a proximity between edges (Distance),
l an edge curvature measurement (Curvature),
l a specification of cell target sizes on the edge (Target cell sizes).
13. Select in the curve (edge) list "Curve 7".
14. Select Active.
15. Set the Max nb of refinements to <3> <Enter>.
16. Select the Target cell sizes criterion and keep the default values.
The Max nb of refinements per curve ultimately controls the refinement of cells intersecting that
particular curve (if the prescribed value is lower than the Maximum number of refinements set in
the Global tab). This parameter supersedes any other selected adaptation criteria. Fine tuning of this
parameter is useful when the appropriate Target cell size is hard to determine, or when the
Distance and Curvature criteria yield a prohibitive number of cells. The default value (10000) is
an arbitrarily large number such that the criteria are controlled by the Maximum number of
refinements set in the Global tab.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved edges. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell size for each
geometrical curve. The size of a cell intersecting a geometrical curve are compared to the prescribed
user target and the cell is refined until its actual size is lower than the target.
17. Click on the Surface refinement tab.
The surface criterion considers cells intersecting surfaces as candidates for refinement. Three criteria
have been implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
The volume criterion (found in the Box refinement tab) considers cells which are intersecting or
located inside a three-dimensional volume as candidates for refinement if their cell size is larger than
some user prescribed target size.
18. Select in the surface list "volute_group_1".
19. Select Active.
20. Set the Max nb of refinements to <2> <Enter>.
21. Select the Target cell sizes criterion and keep the default values.
22. Repeat step 18 to step 21:
l for "volute_group_2" except for the Max nb of refinements set to <3> <Enter>,
l for "volute_group_3" except for the Max nb of refinements set to <1> <Enter>.
223
FINE™/Open with OpenLabs™ 7.2 Tutorials
The Max nb of refinements per surface ultimately controls the refinement of cells intersecting that
surface (if it is presenting a value lower than the Maximum number of refinements set in the
Global tab). This parameter supersedes any other selected adaptation criteria. Fine tuning of this
parameter is useful when it may be difficult to determine the appropriate Target cell size, or if the
Distance and Curvature criteria yield a prohibitive number of cells. The default value (10000) is
an arbitrarily large number such that the criteria are controlled by the Maximum number of
refinements set in the Global tab.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell size for each
geometrical surface. The size of a cell
intersecting a geometrical surface are compared to the
prescribed user target and the cell is refined until its actual size is lower than the target.
23. Go to the Trimming tab.
24. Set patch trimming status to Used for trimming for the patches "volute_ group_ 0",
"volute_group_2", and "volute_group_3" if necessary.
25. Click on Ok.
26. Click on the Step button in the Mesh Wizard to launch the adaptation step.
2.7 MESH WIZARD VOLUTE BLOCK : SNAPPING
STEP
27. Left-click the checkbox for Snap to geometry. The corresponding step becomes accessible
for the user.
28. Left-click on Snap to geometry and the Snapping parameters dialog box appears.
29. The Advanced >>> button allows to activate 3 extra tabs (Global parameters, Curve
Snapping and Buffer Insertion).
30. Keep the Enable snapping option active and keep the default advanced parameters.
31. Left-click on Ok.
The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh
adaptation onto the surface to obtain a good quality, body-conforming mesh. In addition to a simple
projection onto the geometry,
lower-
dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee
that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner
of the geometry and that a path of mesh edges is attached to the curve.
this action involves sophisticated algorithms to recover
Layers of additional cells (buffer insertion) are introduced into the mesh to create a body-conforming
mesh.
Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
2.8 MESH WIZARD VOLUTE BLOCK :
OPTIMIZATION STEP
The mesh obtained after the snapping step may contain poor quality cells which are usually located
close to corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
32. Left-click the checkbox for Optimize to activate the step. The corresponding step becomes
accessible for the user.
33. Left-click on Optimize and the Optimization parameters dialog box appears.
34. Keep the default settings.
35. Left-click on Ok.
36. Click on the Start button in the Mesh Wizard to snap and optimize the mesh.
37. Left-click on the Mesh quality icon (
) in the Tool bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e. cells with a
negative volume. Negative cells are not allowed in the final mesh to be used for the computation.
Concave or twisted cells are less likely to present robustness or stability issues for solvers,
however they should be prohibited.
When negative, concave or twisted cells are detected, they should usually be removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
38. Check the mesh quality by using the Criterion drop-down list for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are
presented through histograms. Each bar represents the number of cells whose criterion value is
included in the bar interval. By left-clicking on one of the bars, the corresponding cells are
displayed in the graphics area. Cells are displayed in a color varying depending on the value of
the quality criterion. The Show markers check button activates the display of circle markers for
each vertex of the displayed cells, which facilitates the localization of the selected cells.
39. After checking the mesh quality, click on Close to exit.
2.9 MESH WIZARD VOLUTE BLOCK : VISCOUS
LAYERS INSERTION STEP
40. Left-click the checkbox for Viscous layers. The corresponding step becomes accessible for
the user.
41. Left- click on Viscous layers and the Viscous layer insertion parameters dialog box
appears.
42. Under
<0.005><Enter>. Keep the default values for all other settings.
the Global
set First
tab,
layer thickness under Global parameters
to
43. Go to the Surface tab.
44. Select the surface "volute_group_1".
Clicking on the Group as Adapt button will automatically group the surfaces like in the Surface
Adaptation tab of the Refinement menu. Manual grouping can also be done thanks to the Group
button. Since no group was defined in this tutorial, clicking on the button will have no impact.
45. Left-click on Active.
46. Set First layer thickness to < 0.005 >< Enter>, Stretching ratio to < 1.5 >< Enter> and
Number of layers to <13><Enter>.
The width of the first cell close to the wall must be selected with care since the quality of the flow
solution will often depend upon the capture of the flow phenomena inside the boundary layers which
develop along the solid walls. Depending upon the turbulence model selected, NUMECA recommends
to locate the nearest grid point along the wall, at a distance that corresponds to parietal coordinate y+
ranging from 1- 5 (low Reynolds number models) or 30- 50 (high Reynolds number models).
Assuming thermal effects must be modeled accurately, y+ can reach values as low as 0.1.
The relation between the parietal coordinate y+ and width of the first cell close to the wall y is driven
by the Blasius equation, expressed as follows for turbulent flows :
where :
l Ywall is the distance of the nearest grid point to the wall (in meter),
l Vref is a reference velocity of the flow, for instance, the inlet velocity (in m/s),
l ν is the kinematic viscosity of the fluid (in m²/s), i.e. the dynamic viscosity divided by the density,
l Lref is a reference length of the test case (in meter),
l Y1
+ is a non-dimensional value.
The Compute button allows the user to estimate the width of the first cell close to the wall.
In the present case, the first layer thickness of 0.005 [mm] corresponds to a Y+ of about 1.
47. Repeat step 44 to step 46:
l for "volute_group_2" except for the Number of layers set to <11> <Enter>,
l for "volute_group_3" except for the Number of layers set to <11> <Enter>.
231
FINE™/Open with OpenLabs™ 7.2 Tutorials
232
FINE™/Open with OpenLabs™ 7.2 Tutorials
48. Click on Go to start the viscous layer insertion step.
49. Repeat step 37 to step 39 to check the mesh quality after viscous layers insertion.
2.10
IMPORT EXISTING AUTOGRID5™ MESH
(IMPELLER)
AutoGrid5™ is an automatic structured meshing system for turbomachinery configurations. Please
refer to the AutoGrid5™ User Guide and Tutorials on how to generate the 3D mesh.
50. Go to the Project/Import.../Project menu.
the
51. Select
"FINE- Open_
Advanced/Tutorial_ 2/impeller/" folder of the tutorial package ( download Advanced tutorial
archive) and confirm by pressing Open or Ok.
existing AutoGrid5™ mesh
"impeller.igg"
the
in
52. Keep active the option keep all the NMB, PER and PERNM connections so that periodic
boundaries are computed with the new periodic treatment. Else, these boundaries will be treated
as FNMB. Click on the button Ok to convert and import the structured mesh.
53. Under the "_mesh" folder (if FINE™/Open project), enter the name of the mesh project as
<volute_impeller.igg> and press Ok or Save to save the mesh files.
54. For the coarsening strategy, keep the default value <0> and press Continue.
HEXPRESS™ allows the user to import the structured mesh based on the selected multigrid level. In
this tutorial, the grid level 0/2 means that three grid levels are available and the finest grid level (0)
will be imported.
Then, the structured AutoGrid5™ mesh will be converted into HEXPRESS™ format and saved
on the disk.
2.11
ADD ROTOR-STATOR INTERFACE
55. Go to the Grid/Boundary Conditions... menu and set the following boundaries to UND,
using the Set face type button :
l "volute_group_4";
l "volute_group_5";
l "row_1_flux_1_Main_Blade_outlet_outlet";
l "row_1_flux_1_Main_Blade_down_outlet";
l "row_1_flux_1_Splitter_1_outlet_outlet";
l "row_1_flux_1_Splitter_1_down_outlet".
Close the dialog box.
It is to be noticed that rotor/stator connections are always defined on top of existing patches and the
existing patches must have a valid basic type (SOL or UND). In case that a patch has an undefined
type (UND) and is used in the definition of the rotor/stator, HEXPRESS™ automatically sets its type
to ROT.
56. Go to the Grid/Non Matching Connections ... menu and press Search Connections and
Yes. One connection is found, named <connection_1>.
57. Click on the Edit button and check in the Non Matching Connections - Edition panel that
the connection between the patches from step 55 is found. The boundary condition type for these
patches is set to ROT.
58. Left-click on the "connection_1" and click on the button Compute to compute the rotor/stator
connection. Close the dialog box.
2.12 SAVE MESH
59. Go to Project/Save as... or click on the Save icon
in the Icon bar.
The mesh folder "_mesh" contains the mesh topology, geometry, grid points and the boundary
condition types among others. The files are listed below :
l .bcs : boundary conditions files,
l .dom : geometry files,
l .igg : topology file,
l .hex : grid points files,
l .rep : report file,
l .dist : distance file (prefix is domain name),
l .fnmb : FNMB connections,
l .nmb: NMB connections,
l .qualityReport : quality report file.
In addition, a subdirectory named "cache" contains the resulting mesh files after each step of the
mesh generation (for example "_snap.hex" as resulting mesh after snapping process). It allows for
deleting some steps and coming back to a previous one without generating the necessary steps
again.
60. Click on the Close button.
61. You can save the project (if not done already) and accept to link the new mesh to the project
(if requested).
62. Mesh quality information is then displayed. Acknowledge the warning and click on Ok.
63. The Mesh properties dialog box appears. Check that the information is correct (change Grid
units to Millimeters) and click on Ok.
64. In Project/Preferences... select Full-double-precision mode and click on Ok.
You are now back to the FINE™/Open interface and you are ready to proceed with the
definition of the "Flow Settings" (p. 242)!
FLOW SETTINGS
A step by step approach is proposed in the following lines. It aims at guiding you through the
various steps that need to be executed to set up and start the computation.
2.13 MANAGE COMPUTATIONS
65. In the Computations menu, right-click on the computation name and select Rename.
66. Rename "computation_1" as <SA_CPUBooster> <Enter>.
In the Computations menu, the list of computations is shown. It is possible to Rename, to create a
new one by duplicating the highlighted one (New button), to clean the files into the computation
subfolder (Clean button) or just to delete the computation by clicking on Delete.
2.14 SET PHYSICAL CONFIGURATION
67. In the Physical Configuration menu, double left-click on the General Properties menu.
68. Keep Steady mode and Fluid block active for the domains "volute" and "row_1".
69. Click on Ok to confirm.
70. In the Physical Configuration menu, double left-click on Fluid Model.
71. Select the domain "volute".
72. In the Edit/Select fluid section, click on Select....
73. Keep AIR(Perfect) selected in the fluid list and press Ok to confirm.
74. Repeat step 71 to step 73 to set the same fluid for the domain "row_1".
75. Click on Close.
76. In the Physical Configuration menu, double left-click on Flow Model.
77. Left-click on the domains "volute" and "row_1" by holding the <Ctrl> key to select them.
78. Keep Spalart-Allmaras as the Turbulence model.
79. Change the reference parameters:
l Set Reference length to <0.01> <Enter> [m],
l Set Reference velocity to <300> <Enter> [m/s].
80. Click on Ok to confirm.
81. In the Physical Configuration menu, double left-click on Rotating Machinery.
82. In the Rotating domains tab, left-click on the domain "row_1".
83. Select the option Rotating and set the Rotation speed to <-115000> <Enter> [RPM].
The Rotation speed of the block has to be given in Revolutions Per Minute (RPM). A positive value
for the rotation speed indicates a rotation in positive θ-direction with θ positive according to a right-
handed coordinate system.
84. Left-click on the tab Rotor/stator to set the rotor-stator interface parameters.
85. Select the interface "connection_1".
86. Keep the Full non- matching mixing plane method for the Rotor/Stator connection
treatment.
87. Set the Flow direction from Left (upstream) -----> Right (downstream).
88. Left-click on Ok to confirm.
The flow direction (upstream/downstream) should be well defined. Otherwise, the initial solution for
turbomachinery may not be available.
2.15 BOUNDARY CONDITIONS
89. In the Boundary Conditions menu, double left-click on Boundary Conditions.
90. Under the INLET tab, select all the patches (left-click on the first one and left-click + <Shift>
on the last one).
91. Left-click on the button Group and set the name to <Inlet> <Enter>.
92. Select Mass flow imposed and Velocity Direction, set the following boundary conditions for
the inlet:
l Set Mass Flow to <0.2> <Enter> [kg/s],
l Set Vr/V to <0> <Enter>,
l Set Vt/V to <0> <Enter>,
l Set Vz/V to <1> <Enter>,
l Set Static Temperature to <293> <Enter>[K],
l Keep Turbulence Viscosity to <0.0001> <Enter> [m²/s].
93. Left-click on the OUTLET tab, select the patch "volute_group_0".
94. Keep the outlet boundary condition type Static Pressure Imposed and set the Static
Pressure to Constant Value <200000> <Enter> [Pa].
95. Under the SOLID tab, select the patches "volute_group_1" to "volute_group_3" (left-click on
the first one and left-click + <Shift> on the last one).
96. Left-click on the button Group and set the name to <volute> <Enter>.
97. Keep the default parameters for these solid patches.
98. Left-click on the groups "row_1_hub_(r.p.m. 500)" and "row_1_blade_(r.p.m. 500)" by
holding the <Ctrl> key.
99. Keep the option Constant Rotation Speed, set the Rotation speed to <-115000> <Enter>
[RPM], and keep the option Compute force and torque active.
100. Keep the default parameters for the group "row_1_shroud".
101. Click Ok to close the window.
2.16
INITIAL SOLUTION
102. In the Initial Solution menu, double left-click on Initial Solution.
103. Select the domain "volute", keep Constant values and select Coordinate system as
Cylindrical.
104. Set the following values:
l Pressure = <200000> <Enter> [Pa],
l Temperature = <293> <Enter> [K],
l Velocity type = Absolute,
l Vr = <50> <Enter> [m/s],
l Vtheta = <-100> <Enter> [m/s],
l Vz = <0.0> <Enter> [m/s],
l Nut/Nu = <50> <Enter>.
105. Select the domain "row_1", select For turbomachinery.
106. Select Main Entrance under the Channel Parameters area, keep Constant distribution
as Pressure type and set Static pressure to <101325> <Enter> [Pa] at Inlet.
107. Select Main Exit under the Channel Parameters area, keep Constant distribution as
Pressure type and set Static pressure to <200000> <Enter> [Pa] at connection_1.
108. Click on Ok to close the window.
2.17 NUMERICAL PARAMETERS
109. In the Numerical Parameters menu, double left-click on General Parameters.
110. Activate the option CPU Booster.
FINE™/Open includes an innovative breakthrough in convergence acceleration. Based on enhanced
implicitness, it leads to a drastic reduction in computational time with respect to the current advanced
technologies in FINE™/Open.
111. Check that the Number of grid(s) is set to 4.
The flow solver is based on an explicit
time integration technique, which is accelerated using
dedicated multi- grid methods. To this end, several levels of intermediate grids must be generated
starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
112. Keep Coarse grid initialization active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be
significantly reduced by activating the coarse grid initialization process. In that case, the simulation
starts on the coarsest grid level available, leading to fast convergence. Once it is done, the flow solver
automatically interpolates the current flow solution on the intermediate levels before the iterative
process is restarted. A similar process repeats until the expected finest grid level is achieved. The
iterative process stops when the convergence criterion is reached or the maximum number of
iterations is exceeded.
113. Under the Advanced tab, in the Coarse grid initialization parameters area, activate the
option CPU booster. Click on Ok.
114. In the Numerical Parameters menu, double left-click on Numerical Schemes.
115. Check that the CFL number is set to 100 for both domains "volute" and "row_1". Click on
Ok.
The CFL number drives the pseudo- time step selected to reach a steady state solution using the
time- marching method integrated in the flow solver. In case the CPU Booster is activated, the
default CFL number in the Numerical Parameters/Numerical Schemes page is set to 100.
2.18 OUTPUT PARAMETERS
116. In the Computation Control menu, double left-click on Outputs.
117. Select Turbomachinery outputs in the Flow configuration area.
By default, depending on the Flow configuration selected, a list of quantities is defined to be
computed in the flow solver. The list can be manually adapted by selecting a quantity in a category
and clicking on the Add --> and <-- Remove buttons
118. Select Thermodynamics under Categories. Select Relative Total Temperature and click
on the Add --> button. Then also add Relative Total Pressure.
119. Select Velocities under Categories. Select Wxyz and click on the Add --> button.
120. Select Turbulence under Categories. Select Y+ and click on the Add --> button. Then also
add Wall Distance.
121. Click on Ok.
2.19 CONTROL VARIABLES
122. In the Computation Control menu, double left-click on Control Variables.
123. Set the Number of iterations to <100> <Enter>.
Using CPU Booster, the computation usually converges within 50 iterations on the finest grid level.
In this tutorial, the computation converges after 100 iterations (after 50 iterations on the finest grid
level).
124. Set the Convergence criteria to <-12> <Enter>.
125. Keep the Save solution every to <100> <Enter> iterations.
126. Click on Ok to confirm.
2.20 LAUNCHING MODE
127. In the Computation Control menu, double left-click on Launching Mode.
128. Keep Serial in the Launching mode area.
129. Click on Ok to confirm.
2.21 SAVE PROJECT & COMPUTATION
130. Click on the Save Project icon to save the project.
131. Click on the Save Selected 'Run' files icon to save the computation.
2.22 START & STOP COMPUTATION
132. Click on the Start Flow Solver icon to launch the computation.
133. Click on the Ok button to start the computation in serial mode.
To save and stop a computation while running, the icon Save Solution And Stop Flow Solver
should be pressed. However, to stop the computation without saving, the Kill Flow Solver icon
should be used.
The pop- up Task manager window allows following the convergence history of
computation.
the
2.23 MONITORING
Evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out for internal
flow) and/or global quantities (lift, drag and momentum on solid walls selected in the boundary
conditions page) can be performed in the steering. Local and global quantities may also be added
for follow up during the convergence process. However, their representation in the graphical area
will be effective only once they are added, and the past convergence history will not be available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes :
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out (for internal flow), with satisfactory correspondence (usually
less than 0.5% difference between in/out). To do so, select the inlet and outlet mass flow at
once. Information about the difference is automatically computed.
The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via the icon bar.
The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the
visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated
within the environment and includes numerous tools.
134. To access CFView™ from the FINE™ graphical user interface, press the Start CFView™
icon (
).
You are now entering the CFView™ interface and you are ready to proceed with the "Post
Processing" (p. 262) of the results!
POST PROCESSING
A step by step approach is proposed in the following lines. It aims at guiding you through the
various steps that need to be executed from reading the solution to the extraction of the main
results. CFView™ automatically opens the ".run" file associated with the active computation.
2.24 CHECK Y+
135. In the Surfaces section, all solid surfaces are selected by default.
136. Go to the Quantities section in the Quick Access Pad, double left-click on the Y+.
All quantities selected in the FINE™ graphical user interface are transferred to CFView™. However,
additional derived output can also be accessed directly from the visualization and post-treatment tool,
including vector components, gradients, divergence and curl of selected quantities. New quantities,
defined from existing quantities
functions,
...) can be created with the Quantity/Field
trigonometric functions,
Data/Define New Quantity... menu.
combined with regular operations
logarithmic functions,
(arithmetic
137. Check the full range of the Y+ quantity in the Information Area, to ensure that the imposed
first cell size is in agreement with the turbulence model used. In this tutorial, the maximum value
of Y+ is close to 30.
138. Click on the Representations/Contours & Iso Values section and then on the Strip
Contour icon to display the selected quantity Y+.
139. Click on the Representations/Lighting & shadows section and then on the Toggle Light
Contour icon to toggle light on for the contour of Y+.
140. Click on the icon
in the Icon Bar to set the colormap range.
141. Input <0 5><Enter> in the keyboard input area.
142. Click on the Representations/Integrals section and then on the Scalar Average icon to
compute the averaged value of Y+. The averaged value shown in the Message Area is around
1.7 (in agreement with the selected turbulence model).
2.25 CREATE PRESSURE CONTOUR ON
CUTTING PLANE IN VOLUTE
143. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
144. Go to the Quantities section in the Quick Access Pad.
145. Double left-click on the Static Pressure.
146. Select the Geometry/Create Cutting Plane... menu.
147. Enter the X, Y, Z values for Point, Normal and Rotation Axis as shown in the following
figure.
148. Select Geometry and click on Apply to pre-visualize the cutting plane.
149. Click on Save to add this cutting plane to the Surfaces section in the Quick Access Pad.
The cutting plane will be activated by default.
150. Click on Close.
151. In the Surfaces section, left- click on the symbol
"CUT1.D1" only by left-clicking, right-clicking and pressing Select.
in front of "CUT1", then select
152. Click on the Representations/Contours & Iso Values section and then on the Smooth
Contour icon to display the static pressure.
153. Click on the icon
in the Icon Bar to use the colormap optimum range.
154. Go to the menu Representation/Isolines/Isolines....
155. Change the number of isolines to <21> in the Mode frame, keep the default values in the
Range frame, then select Uniform.
156. Click on Apply and then on Close.
2.26 CREATE 3D STREAMLINES IN VOLUTE
157. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
158. Go to the Quantities section in the Quick Access Pad.
159. Double left-click on the Vxyz (Velocity).
160. Click on the Representations/Vector Lines section.
161. Click on the Vector Lines Parameters icon.
162. Under the tab General, change Direction to both, Representation to tube and Color to
Velocity.
163. Click on the Apply button to confirm and then click on Close.
164. In the Surfaces section in the Quick Access Pad, select "volute_group_0 Outlet" by left-
clicking, right-clicking and pressing Select.
165. Click on the icon Local Vector Line.
166. With the mouse, left-click somewhere on the patch "volute_group_0 Outlet" in the Graphics
area to create a streamline. Create multiple streamlines by clicking on different locations on the
patch "volute_group_0 Outlet".
167. In the Filter (type) section in the Quick Access Pad/Surfaces, choose the option Type,
then select SOL under Select. All solid surfaces will be selected in the Surfaces section.
168. Click on the Representations/Grid section in the Quick Access Pad.
169. Click on the Render Gouraud icon.
170. Click on the Representations/Opacity section in the Quick Access Pad.
171. Set the Opacity to 0.3.
2.27 TIP LEAKAGE VORTEX IN IMPELLER
172. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
before "Connections", then select "row_
173. In the Surfaces section, left-click on the symbol
1.S24 row_1_group_24" and "row_1.S52 row_1_group_52" by left-clicking (holding the key
<Ctrl>), right-clicking and pressing Select.
174. Click on the menu Geometry/Boundary to show the boundary of the selected surfaces
(shortcut <b>).
175. Go to the Quantities section in the Quick Access Pad, double left-click on the Wxyz
(Relative Velocity).
176. Click on the Representations/Vector Lines section.
177. Click on the Vector Lines Parameters icon.
178. Under the tab General, change Direction to both, Representation to tube and the Color to
Velocity.
179. Under the tab Ribbon & Tube Type, set r0 to <0.2><Enter>.
275
FINE™/Open with OpenLabs™ 7.2 Tutorials
180. Click on the Apply button to confirm and then click on Close.
181. With the mouse, use the viewing buttons to zoom in the area of the blade tips.
182. Click on the icon Vector Lines from Section.
183. Keep "5" in the keyboard input area to draw 5 vector lines per section.
184. With the mouse, draw lines (left-click and drag) on the selected surfaces (in the blade tips) to
plot the streamlines through the impeller (main blade and splitter) tip gaps.
185. In the Surfaces section in the Quick Access Pad, select "row 1_hub_(r.p.m.500)" and "row
1_blade_(r.p.m.500)" by left-clicking (holding the key <Ctrl>), right-clicking and pressing Select.
186. Click on the Representations/Grid section in the Quick Access Pad and then on the
Render Gouraud icon.
2.28 PLOT VELOCITY CONTOUR ON IMPELLER
B2B SURFACE
187. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
188. Go to the menu File/TurboMachinery.
to load the hub and shroud curves definition. Select the
189. Left-click on the button
provided AutoGrid5™ mesh "impeller.cgns" in the "Tutorials/FINE- Open/FINE- Open_
Advanced/Tutorial_2/impeller" folder of the tutorial package and left-click on the button Ok to
confirm.
190. Left-click on the button Ok to initialize the turbomachinery mode.
191. Left-click on the TM view (blade-to-blade bottom left view) in the Graphics area.
192. In the Surfaces section in the Quick Access Pad, select "Cut at S=0.5.D2" by left-clicking,
right-clicking and pressing Select. By default, a blade-to-blade surface at S = 0.5 is created and
shown in the TM view.
193. Select the Quantity/Field Data/Vector Components/Wxyz/Magnitude of W menu to
create the new quantity Magnitude of W from the vector Wxyz.
194. Click on the Representations/Contours & Iso Values section and then on the Smooth
Contour icon to display the magnitude of W.
195. Click on the icon
in the Icon Bar to use the colormap optimum range.
2.29 DEFINE NEW QUANTITY
196. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
197. Go to the menu Geometry/Boundary to deactivate the boundary of the surface "Cut at
S=0.5.D2".
198. Go to the menu Geometry/Blade to Blade Surface....
199. Set S to <0.1> <Enter>, press Save to save the B2B surface. Here a blade-to-blade surface
"CUT2.D2" close to the hub (S=0.1) will be created.
200. Left-click on Close to close the dialog window.
201. Go to the Surfaces section in the Quick Access Pad.
202. Select "CUT2.D2" by left-clicking, right-clicking and pressing Select.
203. Go to the Quantities section in the Quick Access Pad.
204. Left-click on the button New to define a new quantity Relative Mach number.
In the FINE™/Open interface, the quantity Relative Mach Number was not selected as output.
Here, a new quantity Relative Mach number will be defined. For perfect gas, the Relative Mach
Number is defined as :
where γ is the specific heat ratio, p is the static pressure and ρ is the density.
205. Input the quantity name <Relative Mach number> and definition as shown in the following
picture <Magnitude of W/sqrt(1.4*Static Pressure/Density)>.
206. Left-click on the button Apply to define the new quantity and press Close. The quantity
Relative Mach number will appear in the Quantities section in the Quick Access Pad and will
be selected by default.
207. Click on the Representations/Contours & Iso Values section and then on the Smooth
Contour icon to display the relative Mach number.
208. Click on the icon
in the Icon Bar to use the colormap optimum range.
2.30 PLOT BLADE LOADING ON IMPELLER
(CARTESIAN PLOT)
209. Left-click on the SM view (bottom right view) in the Graphics area.
210. In the Surfaces section, select "row 1_hub_(r.p.m.500)", "row 1_shroud" and "row 1_
blade_(r.p.m.500)" by left-clicking (holding the key <Ctrl>), right-clicking and pressing Select.
211. Go to the Quantities section in the Quick Access Pad, and double left-click on the Static
Pressure.
212. Click on the Representations/Plots & Values section and then on the Blade Section
button.
213. Input <0.5> <Enter> in the keyboard input area to draw a Cartesian plot of the blade loading
on the impeller main and splitter blade at mid-span.
214. Select the File/Quit CFView menu and Yes to leave the CFView™ session.
TUTORIAL 3.
GAMM HYDRAULIC TURBINE
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l Spatial discretization of the flow equations,
l Flow computation,
l Visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated.
The unstructured CFD package consists of the following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
This tutorial is particularly adapted to a 3D Francis Hydraulic Turbine application (stay vanes/guide
vanes/runner/draft tube). It makes use of FINE™/Open including HEXPRESS™ and CFView™.
The following steps will be discussed :
l Use HEXPRESS™ user interface,
l Progress in the mesh wizard to generate the mesh,
l Control the quality of the mesh,
l Import an existing AutoGrid5™ structured mesh,
l Add a rotor-stator interface,
l Set up a computation in FINE™/Open interface,
l Start/Suspend the computation,
l Visualize the results with CFView™.
3.1
INTRODUCTION
3.1.1
Prerequisites
This tutorial does not require any particular prerequisite but it is strongly recommended for
beginners to perform the Beginner level tutorials.
3.1.2
Problem Description
The problem is related to a Francis hydraulic turbine with medium/high specific speed. It has been
designed at IMHEF for experimental research in the hydraulic laboratory. The model has been
used as a test case in the 1989 GAMM workshop.
The spiral casing of the GAMM turbine has been designed to ensure a constant meridional
velocity distribution, and fillets have been added on both sides of the distributor inlet in order to
achieve well-defined inlet conditions. The distributor consists of 24 stay vanes and 24 guide
vanes. The runner includes 13 blades, with an external diameter of 0.4 m.
A draft tube connects the Francis hydraulic turbine to a "tail race". The velocity of the water at the
the runner outlet is very high. The increasing of the draft tube section area allows to decrease this
velocity and thus, a part of the kinetic energy is recovered as a gain of water pressure.
3.1.3
Preparation
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <GAMM_turbine.iec> and click on Save or Ok.
FINE™/Open will automatically create a project folder called "GAMM_ turbine" which will
contain the project file (" .iec") and a folder " _mesh" where the mesh will be stored. Later,
computation folders will appear inside the project folder. It is strongly advised to keep this file
structure all along the project.
l Click on Yes to start HEXPRESS™ unstructured mesh generator.
You are now ready to start the "Mesh Generation" (p. 290) process for the GAMM Turbine
configuration!
MESH GENERATION
HEXPRESS™ graphical user interface allows you to visualize the geometry and mesh of the
internal or external test case in a graphics area. The access to the main menu and controls is
provided by a menu bar and a quick access pad, and is completed with a tool/icon bar and a
control area (including the keyboard input area).
HEXPRESS™ allows meshing of multiblock configurations. The user can generate the mesh for
each block. Alternatively, the user can import several existing projects to make a multiblock mesh.
Both HEXPRESS™ and IGG™ (including AutoGrid5™) projects can be imported. In this
tutorial, the mesh in the draft tube will be generated in HEXPRESS™ while the mesh in the stay
vanes, guide vanes and the runner will be converted in HEXPRESS™ from an existing
AutoGrid5™ project.
3.2
IMPORT DRAFT TUBE DOMAIN
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined. That is why the tutorial starts from a domain file ".dom". It should be
noticed that the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL),
import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as execute Python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS dialog box.
2. In the dialog box, locate and select "DT.dom" (download Advanced tutorial archive), then
click on OK to confirm.
3. Use the viewing buttons at the bottom of the interface to display the geometry as preferred. In
the View subpanel from the Quick Access Pad, it is possible to:
l Left-click on the Mesh icon (
) to hide/show mesh (toggle),
l Left-click on the Solid icon (
) to hide/show faces (toggle),
l Right-click on the Face icon (
) or left-click on the Face viewer icon (
) to open the
Face Viewer window.
Face selection can be done interactively in the graphics area or thanks to the Face Viewer
window.
3.3
SET BOUNDARY CONDITIONS FOR DRAFT
TUBE
4. Go to the Grid/Boundary Conditions... menu or click on the icon
set the boundary conditions, using the Set face type button:
in the icon bar and
l Set "DT_group_9" as outlet ("OUT"),
l Set "DT_group_12" as inlet ("INL"),
l Set "DT_group_13" as inlet ("INL"),
l Keep all other faces as solid ("SOL").
5. Close the dialog box.
3.4 MESH WIZARD DRAFT TUBE BLOCK :
INITIAL MESH
6. Left- click the checkbox for Initial mesh in Mesh wizard to activate this step. The
corresponding step becomes accessible for the user. The same behavior is applied for the
following steps in the Mesh Wizard.
7. Left-click on Initial mesh and the Initial mesh parameters dialog box appears. In the Set the
number of cells along cartesian axis frame, impose X axis to <46>, Y axis to <121>, Z axis to
<86>.
8. Click on the button Go to create the initial mesh with 478,676 cells.
The number of cells along the X/Y/Z axis in the initial mesh can be increased in order to impose a
smaller size to the biggest cell that will be included in the computational domain.
3.5 MESH WIZARD DRAFT TUBE BLOCK :
ADAPTATION STEP
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selected in this action directly dictate the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming.
in terms of user
important
During the first step, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry-
dependent criteria. With the second step, it removes the cells intersecting the geometry or located
outside the computational domain.
9. Left-click the check box for Adapt to geometry in Mesh Wizard.
10. Left-click on Adapt to geometry to open the Refinement and trimming parameters dialog
box.
11. Under the Global tab, set the Maximum number of refinements to <5> <Enter>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement in one or several different
directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive
refinements. This may result in an exponential growth of the total number of cells in the mesh, even
though the refinement may be confined to some areas of the computational domain. To bound the
number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may alter the success of the meshing process. More details are available in the User Guide.
12. Left-click on the Curve refinement tab.
The adaptation process is defined by three classes of criteria: curve, surface and volume criteria. The
curve criterion considers cells which are intersecting edges as candidates for refinement. Three criteria
are implemented and are respectively based on:
l a proximity between edges (Distance),
l an edge curvature measurement (Curvature),
l a specification of cell target sizes on the edge (Target cell sizes).
13. Select in the curve (edge) list "Curve 13", select Active and set the parameters as follows:
l Set the Max nb of refinements to <4> <Enter>,
l Select the Target cell sizes criterion and keep the default values,
l Select the Curvature criterion.
The Max nb of refinements per curve ultimately controls the refinement of cells intersecting that
particular curve (if the prescribed value is lower than the Maximum number of refinements set in
the Global tab). This parameter supersedes any other selected adaptation criteria. Fine tuning of this
parameter is useful when the appropriate Target cell size is hard to determine, or when the
Distance and Curvature criteria yield a prohibitive number of cells. The default value (10000) is
the criteria are controlled by the Maximum number of
an arbitrary large number such that
refinements set in the Global tab.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved edges. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell size for each
geometrical curve. The size of a cell intersecting a geometrical curve are compared to the prescribed
user target and the cell is refined until its actual size is lower than the target.
14. Repeat step 13:
l for "Curve 14" with the same settings,
l for "Curve 15" except for the Max nb of refinements set to <1> <Enter>,
l for "Curve 16" except for the Max nb of refinements set to <1> <Enter>.
15. Click on the Surface refinement tab.
The surface criterion considers cells intersecting surfaces as candidates for refinement. Three criteria
have been implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
The volume criterion (found in the Box refinement tab) considers cells which are intersecting or
located inside a three-dimensional volume as candidates for refinement if their cell size is larger than
some user prescribed target size.
16. Select in the surface list "DT_group_0", select Active and set the parameters as follows :
l Set the Max nb of refinements to <3> <Enter>.
l Select the Target cell sizes criterion and keep the default values.
The Max nb of refinements per surface ultimately controls the refinement of cells intersecting that
surface (if it is presenting a value lower than the Maximum number of refinements from the
Global tab). This parameter supersedes any other selected adaptation criteria. Fine tuning of this
parameter is useful when it may be difficult to determine the appropriate Target cell size, or if the
Distance and Curvature criteria yield a prohibitive number of cells. The default value (10000) is
an arbitrarily large number such that the criteria are controlled by the Maximum number of
refinements from the Global tab.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell size for each
geometrical surface. The size of a cell
intersecting a geometrical surface are compared to the
prescribed user target and the cell is refined until its actual size is lower than the target.
17. Repeat step 16:
l for "DT_group_12" except for the Max nb of refinements set to <1> <Enter>,
l for "DT_group_13" except for the Max nb of refinements set to <1> <Enter>.
18. Click on the Trimming tab. Keep all the default settings.
19. Click on the button Go to launch the adaptation step.
3.6 MESH WIZARD DRAFT TUBE BLOCK :
SNAPPING STEP
20. Left-click the checkbox for Snap to geometry in Mesh Wizard.
21. Left-click on Snap to geometry and the Snapping parameters dialog box appears. Then
click on the button Advanced >>> and select the tab Buffer insertion. Set the Buffer layer
insertion type to Type II for "Curve 13", "Curve 14", "Curve 15" and "Curve 16". Click Ok to
confirm.
The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh
adaptation onto the surface to obtain a good quality, body-conforming mesh. In addition to a simple
projection onto the geometry,
lower-
dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee
that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner
of the geometry and that a path of mesh edges is attached to the curve.
this action involves sophisticated algorithms to recover
Layers of additional cells (buffer insertion) are introduced into the mesh to create a body-conforming
mesh. Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
3.7 MESH WIZARD DRAFT TUBE BLOCK :
OPTIMIZATION STEP
The mesh obtained after the snapping step may contain poor quality cells which are usually located
close to corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
22. Left-click the checkbox for Optimize in Mesh Wizard.
23. Left-click on Optimize and the Optimization parameters dialog box appears. Keep all the
default settings and click on the button Ok to confirm.
24. Click on the Start button in the Mesh Wizard to snap and optimize the mesh.
25. Left-click on the Mesh quality icon (
) in the Tool bar to check the mesh quality.
An important step of the mesh quality check is to detect the presence of negative cells, i.e. cells
with a negative volume. Negative cells are not allowed in the final mesh to be used for the
computation. Concave or twisted cells are less likely to present robustness or stability issues for
solvers, however they should be prohibited.
When negative, concave or twisted cells are detected, they should usually be removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
26. Check the mesh quality by using the Criterion drop-down list for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are
presented through histograms. Each bar represents the number of cells whose criterion value is
included in the bar interval. By left-clicking on one of the bars, the corresponding cells are
displayed in the graphics area. Cells are displayed in a color varying depending on the value of
the quality criterion. The Show markers check button activates the display of circle markers for
each vertex of the displayed cells, which facilitates the localization of the selected cells.
27. After checking the mesh quality, click on Close to exit.
3.8 MESH WIZARD DRAFT TUBE BLOCK :
VISCOUS LAYERS INSERTION STEP
28. Left-click the checkbox for Viscous layers in Mesh Wizard.
29. Left- click on Viscous layers and the Viscous layer insertion parameters dialog box
appears.
30. Under the Global
tab, set First layer thickness under Global parameters to < 5e-
05 >< Enter> and Stretching ratio to < 1.4 > < Enter>. Keep the default values for all other
parameters.
31. Under the Surface tab, select the surface "DT_group_0", then hold <Shift> and left-click on
"DT_group_8" to select all the surfaces, click the button Active and set the parameters as follows
:
Clicking on the Group as Adapt button will automatically group the surfaces like in the Surface
Adaptation tab of the Refinement menu. Manual grouping can also be done thanks to the Group
button. Since no group was defined in this tutorial, clicking on the button will have no impact.
l Set First layer thickness to <5e-05> <Enter>,
l Set Stretching ratio to <1.4> <Enter>
l Set Number of layers to <10> <Enter>.
The width of the first cell close to the wall must be selected with care since the quality of the flow
solution will often depend upon the capture of the flow phenomena inside the boundary layers which
develop along the solid walls. Depending upon the turbulence model selected, NUMECA recommends
to locate the nearest grid point along the wall, at a distance that corresponds to parietal coordinate y+
ranging from 1- 5 (low Reynolds number models) or 20- 50 (high Reynolds number models).
Assuming thermal effects must be modeled accurately, y+ can reach values as low as 0.1.
The relation between the parietal coordinate y+ and width of the first cell close to the wall y is driven
by the Blasius equation, expressed as follows for turbulent flows :
where :
l Ywall is the distance of the nearest grid point to the wall (in meter),
l Vref is a reference velocity of the flow, for instance, the inlet velocity (in m/s),
l ν is the kinematic viscosity of the fluid (in m²/s), i.e. the dynamic viscosity divided by the density,
l Lref is a reference length of the test case (in meter),
l Y1
+ is a non-dimensional value.
The Compute button allows the user to estimate the width of the first cell close to the wall.
In the present case, the first layer thickness of 0.00005 [mm] corresponds to a Y+ of about 1.
32. Click on the button Go to start the viscous layer insertion step.
33. Repeat step 25 to step 27 to check the mesh quality after viscous layers insertion.
34. Go to Project/Save as... or click on the Save icon (
) in the Icon bar..
35. Under the "_mesh" folder, enter the name of the mesh project as <DT.igg> and press Ok to
save the mesh files of the draft tube.
3.9
IMPORT EXISTING AUTOGRID5™ MESH
(SVS, GVS AND RUNNER)
AutoGrid5™ is an automatic structured meshing system for turbomachinery configurations. Please
refer to the AutoGrid5™ User Guide and Tutorials on how to generate the 3D mesh.
36. Go to the Project/Import.../Project menu.
37. Locate and select the existing AutoGrid5™ mesh "SV_GV_Runner.igg" provided in the
"FINE-Open_Advanced/Tutorial_3/AG5/" folder of the tutorial package (download Advanced
tutorial archive) and confirm by pressing Open or Ok.
38. Click on the Ok button on the pop-up window, allowing to keep all the NMB, PER and
PERNM connections when converting the structured mesh.
39. Under the "_mesh" folder, enter the name of the mesh project as <GAMM.igg> and press Ok
or Save to save the mesh files, which consist of the draft tube and converted stay vanes, guide
vanes and runner.
40. For the coarsening strategy, keep the value at <0> and press Continue.
HEXPRESS™ allows the user to import the structured mesh based on the selected multigrid level. In
this tutorial, the grid level 0/2 means that three grid levels are available and the finest grid level (0)
will be imported.
Then, the structured AutoGrid5™ mesh will be converted into HEXPRESS™ format and saved
on the disk.
3.10 ADD ROTOR-STATOR INTERFACE
41. Go to the Grid/NonMatching Connections... menu. Click on the Search Connections
button.
42. In the pop-up window, click Yes to search Full Non Matching connections or Rotor/Stator
interfaces.
43. Select the newly found connection "connection_1", click on the button Compute to compute
the rotor-stator connection and then click on the button Close to close the window.
3.11 CHECK AND SAVE MESH
44. Go to the Grid/Boundary Conditions... menu. Check that the boundary condition type for
the patches "DT_group_12", "DT_group_13" and "Runner_flux_1_Main_Blade_downStream_
outlet" is set to ROT. Click the button Close.
45. Go to Project/Save as... or click on the Save icon (
) in the Icon bar..
The mesh folder "_mesh" contains the mesh topology, geometry, grid points and the boundary
condition types among others. The files are listed below :
l .bcs : boundary conditions files,
l .dom : geometry files,
l .igg : topology file,
l .hex : grid points files,
l .rep : report file,
l .dist : distance file (prefix is domain name),
l .fnmb : FNMB connections,
l .nmb : NMB connections,
l .qualityReport : quality report file.
In addition, a sub directory named "cache" contains the resulting mesh files after each step of the
mesh generation (for example "_snap.hex" as resulting mesh after snapping process). It allows for
deleting some steps and coming back to a previous one without generating the necessary steps
again.
46. Click on the Close button in the Icon bar to close HEXPRESS™ and switch back to the
FINE™/Open interface.
47. You can save the project (if not done already) and accept to link the new mesh to the project
(if requested).
48. Acknowledge the warning that the mesh quality could be improved and click on Ok.
49. The Mesh properties dialog box appears. Check that the information is correct and click on
Ok.
50. Go to the menu Project/Preferences....
51. Select Full-double-precision mode and click on Ok.
You are now back to the FINE™/Open interface and you are ready to proceed with the
definition of the "Flow Settings" (p. 315)!
FLOW SETTINGS
A step by step approach is proposed in the following lines. It aims at guiding you through the
various steps that need to be executed to set up and start the computation.
3.12 MANAGE COMPUTATIONS
52. In the Computations menu, right-click on the computation name and select Rename.
53. Rename "computation_1" as <SA_Ext> <Enter>.
In the Computations menu, the list of computations is shown. It is possible to Rename, to create a
new one by duplicating the highlighted one (New button), to clean the files into the computation
subfolder (Clean button) or just to delete the computation by clicking on Delete.
3.13 SET PHYSICAL CONFIGURATION
54. In the Physical Configuration menu, double left-click on the General Properties menu.
55. Keep all the default settings and click on Ok to confirm.
56. In the Physical Configuration menu, double left-click on Fluid Model.
57. Left-click on the domain "DT" and then left-click on the domain "Runner_ flux" while
holding <Shift> to select all the domains, then click on the button Select...,
58. Select WATER (Incompressible) in the fluid list and click on the button Ok to confirm.
59. Click on the button Close in the Fluid Model window.
60. In the Physical Configuration menu, double left-click on Flow Model.
61. Left-click on the domain "DT" and then left-click on the domain "Runner_ flux" while
holding <Shift> to select all the domains, then set the parameters as follows :
l Change the Turbulence model to Spalart-Allmaras (Extended Wall Function),
l Set Reference length as <0.4> <Enter> [m],
l Set Reference velocity as <8.6> <Enter> [m/s].
62. Click on Ok to confirm.
63. In the Physical Configuration menu, double left-click on Rotating Machinery.
64. In the Rotating domains tab, left-click on the domain "Runner_flux", check that the option
Rotating is active and that the Rotation speed is set to <408.93> <Enter> [RPM].
The Rotation speed of the block has to be given in Revolutions Per Minute (RPM). A positive
value for the rotation speed indicates a rotation in positive θ-direction with θ positive according to a
right-handed coordinate system.
65. Left-click on the tab Rotor/stator to set the rotor/stator interface parameters.
66. Select the interface "connection_1", set the Flow direction to "Left (upstream) --> Right
(downstream)".
67. Keep all other settings and click on Ok to confirm.
The flow direction (upstream/downstream) should be well defined. Otherwise, the initial solution for
turbomachinery may not be available.
3.14 SET BOUNDARY CONDITIONS
68. In the Boundary Conditions menu, double left-click on Boundary Conditions.
69. Under the INLET tab, select the only patch available named "SV_flux_1_Main_Blade_
upStream_inlet", select Mass flow imposed and Velocity Direction. Set the following boundary
conditions for the inlet:
l Set Mass Flow to <293> <Enter> [kg/s],
l Set Vr/V to <-0.485> <Enter>,
l Set Vt/V to <0.875> <Enter>,
l Keep Vz/V to <0> <Enter>,
l Keep Static Temperature to <293> <Enter>[K],
l Set Turbulence Viscosity to <5e-06> <Enter> [m²/s].
70. Left-click on the OUTLET tab.
71. Select the patch "DT_group_9", keep the outlet boundary condition type Static Pressure
Imposed and set the Static Pressure to Constant Value <101300> <Enter> [Pa].
72. Set Backflow Control active.
73. Left-click on the SOLID tab.
74. Left-click on the patch "DT_group_2" and then left-click on the patch "DT_group_8" while
holding the <Shift> key, click on the button Group to group the selected patches, enter the name
<DT_walls> <Enter>.
75. Left-click on the patch "DT_group_0", set the Rotation Speed to <408.93> <Enter>[RPM],
activate the option Compute force and torque.
76. Left- click on the patch "runner_ hub_ (r.p.m. 408.93)", select the option Area Defined
Rotation Speed and set the following values:
l Set Rotation Speed 1 to <0> <Enter> [RPM],
l Set Rotation Speed 2 to <408.93> <Enter> [RPM],
l Set Lower Radius Limit to <0> <Enter> [m],
l Set Higher Radius Limit to <0.158> <Enter> [m],
l Set Lower Axial Limit to <-1> <Enter> [m],
l Set Higher Axial Limit to <0.0565> <Enter> [m],
l Keep the option Compute force and torque active.
77. Left-click on the patch "runner_shroud_(r.p.m. 408.93)", select the option Area Defined
Rotation Speed and set the following values:
l Set Rotation Speed 1 to <0> <Enter> [RPM],
l Set Rotation Speed 2 to <408.93> <Enter> [RPM],
l Set Lower Radius Limit to <0> <Enter> [m],
l Set Higher Radius Limit to <0.203> <Enter> [m],
l Set Lower Axial Limit to <-0.165> <Enter> [m],
l Set Higher Axial Limit to <-0.0703> <Enter> [m],
l Keep the option Compute force and torque active.
78. Keep the default parameters for all the other patches. Click Ok to close the window.
3.15 SET INITIAL SOLUTION
79. In the Initial Solution menu, double left-click on Initial Solution.
80. Left-click on the domain "DT", keep Constant values and set the the parameters as follows :
l Set Coordinate system to Cylindrical,
l Set Pressure to <100000> <Enter> [Pa],
l Set Temperature to <293> <Enter> [K],
l Set Velocity type to Absolute,
l Set Vr to <2> <Enter> [m/s],
l Set Vtheta to <0> <Enter> [m/s],
l Set Vz to < -1> <Enter> [m/s],
l Keep ~Nut/Nu to <50>.
81. Left-click on the domain "ROWS" and then select For turbomachinery under General
settings.
It is possible to initialize a multi-domain computation by combining different initial solution types.
For example, for an impeller and volute configuration, the impeller can be initialized by using For
turbomachinery and the volute by Constant values, or the impeller can be initialized by From
file and the volute by Constant values.
82. Left- click on the channel zone Main Entrance and set Static pressure to < 140000 >
<Enter>.
83. Left-click on the channel zone Internal R/S Connections, select "connection_RS_1" and set
Static pressure to <135000> <Enter>, then select "connection_RS_2" and set Static pressure to
<125000> <Enter>.
84. Left-click on the channel zone Main Exit and set Static pressure to <90000> <Enter>.
85. Click Ok to confirm.
3.16 SET NUMERICAL PARAMETERS
86. In the Numerical Parameters menu, double left-click on General Parameters.
87. Check that the Number of grid(s) is set to 4.
The flow solver is based on an explicit
time integration technique, which is accelerated using
dedicated multi- grid methods. To this end, several levels of intermediate grids must be generated
starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
88. Keep Coarse grid initialization active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be
significantly reduced by activating the coarse grid initialization process. In that case, the simulation
starts on the coarsest grid level available, leading to fast convergence. Once it is done, the flow solver
automatically interpolates the current flow solution on the intermediate levels before the iterative
process is restarted. A similar process repeats until the expected finest grid level is achieved. The
iterative process stops when the convergence criterion is reached or the maximum number of
iterations is exceeded.
89. Click on Ok to confirm.
90. In the Numerical Parameters menu, double left-click on Numerical Schemes.
91. Click on the domain "DT" and then click on the domain "Runner_flux" while holding the
<Shift> key to select all the domains. Select Hakimi preconditioning and set the Characteristic
Velocity to <8.6> <Enter> [m/s].
92. Keep Local velocity scaling active.
Preconditioning is applied at low-speed flows and/or modeling incompressible fluids. At low Mach
numbers, the convergence rate of the iterative process can be largely slowed down due to the
numerical formulation selected in the flow solver. The equations are then preconditioned to recover a
satisfactory rate for convergence. Preconditioning is controlled in the Hakimi method through a user-
controlled parameter β.
This parameter β is imposed by the user through a coefficient β* and the characteristic velocity Uref
such as :
β² = β*.Uref²
β² = β* . max(Uref²,Uloc²) when local velocity scaling is active (Uloc is the local velocity)
Uref is the representative value of the maximum velocity in the flow field. For the user's convenience,
the constant Uref is however always set equal to the reference velocity specified in the Flow Model
page and used in the calculation of the Reynolds Number. In that case, Uref must be carefully selected
since it influences the convergence.
93. Keep all other parameters and click on Ok.
3.17 SET OUTPUT PARAMETERS
94. In the Computation Control menu, double left-click on Outputs.
95. Select Turbomachinery outputs in Flow configuration area. Select
the category
Turbulence and then select the quantity Y+, click the button Add -> to add the quantity Y+ to
the selected quantities list.
By default, depending on the Flow configuration selected, a list of quantities is defined to be
computed in the flow solver. The list can be manually adapted by selecting a quantity in a category
and clicking on the Add --> and <-- Remove buttons.
96. Keep all other settings and selections, click on Ok.
3.18 SET CONTROL VARIABLES
97. In the Computation Control menu, double left-click on Control Variables .
98. Keep all default settings under the tab General.
99. Click on the tab Advanced, select Select category as Local parameters (by domains).
Click on the domain "DT" and then click on the domain "Runner_flux" by holding the <Shift>
key to select all the domains, set the expert parameter turb_ mutMuLimit_ to < 500000 >
<Enter>.
100. Click on Ok to confirm.
3.19 SET LAUNCHING MODE
101. In the Computation Control menu, double left-click on Launching Mode.
102. Select the option Parallel under Launching mode, set Total number of processes to <5>
<Enter>.
103. Click on Ok to confirm.
3.20 SAVE PROJECT & COMPUTATION
104. Click on the Save Project icon to save the project.
105. Click on the Save Selected 'Run' files icon to save the computation.
3.21 START & STOP COMPUTATION
106. Click on the Start Flow Solver icon to launch the computation.
107. Click on the Ok button to start the computation in parallel mode.
To save and stop a computation while running, the icon Save Solution And Stop Flow Solver
should be pressed. However, to stop the computation without saving, the Kill Flow Solver icon
should be used.
The pop- up Task manager window allows following the convergence history of
computation.
the
3.22 MONITORING
Evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out for internal
flow) and /or global quantities (lift, drag and momentum on solid walls selected in the boundary
conditions page) can be performed in the steering. Local and global quantities may also be added
for follow up during the convergence process. However, their representation in the graphical area
will be effective only once they are added, and the past convergence history will not be available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out (for internal flow), with satisfactory correspondence (usually
less than 0.5% difference between in/out). To do so, select the inlet and outlet mass flow at
once. Information about the difference is automatically computed.
The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via the icon bar.
The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the
visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated
within the environment and includes numerous tools.
108. To access CFView™ from the FINE™ graphical user interface, press the Start CFView™
icon (
).
You are now entering the CFView™ interface and you are ready to proceed with the "Post
Processing" (p. 342) of the results!
POST PROCESSING
A step by step approach is proposed in the following lines. It aims at guiding you through the
various steps that need to be executed from reading the solution to the extraction of the main
results. CFView™ automatically opens the ".run" file associated with the active computation.
3.23 CHECK Y+
109. In the Surfaces section in the Quick Access Pad, all solid surfaces are selected by default.
110. Go to the Quantities section in the Quick Access Pad, double left-click on the Y+.
All quantities selected in FINE™ graphical user interface are transferred to CFView™. However,
additional derived output can also be accessed directly from the visualization and post-treatment tool,
including vector components, gradients, divergence and curl of selected quantities. New quantities,
defined from existing quantities combined by regular operations (arithmetic functions, trigonometric
functions, logarithmic functions, ...) can be created with the Quantity/Field Data/Define New
Quantity... menu.
111. Check the full range of the Y+ quantity in the Information Area, to ensure that the imposed
first cell size is in agreement with the turbulence model used.
112. Click on the Representations/Contours & Iso Values section and then on the Strip
Contour icon to display the selected quantity Y+.
113. Click on the Representations/Lighting & shadows section and then on the Toggle Light
Contour icon to toggle light on for the contour of Y+.
114. Check the contour of Y+.
115. Click on the Representations/Integrals section and then on the Scalar Average icon to
compute the averaged value of Y+. The averaged value shown in the Message Area is about 2.1
(in agreement with the selected turbulence model).
3.24 CREATE PRESSURE CONTOUR ON
CUTTING PLANE IN DRAFT TUBE
116. Select the Update/Delete/All menu to delete all previous manipulations in the Graphics
area.
117. Select the Geometry/Create Cutting plane... menu. Enter the X, Y, Z values for Point and
Normal as shown in the following figure.
118. Select Geometry and click on Apply to pre-visualize the cutting plane.
119. Click on Save to add this cutting plane to the Surfaces section in the Quick Access Pad.
The cutting plane will be activated by default.
120. Click on Close.
121. Go to the Surfaces section in the Quick Access Pad, left-click on "CUT1.D1", then right-
click and Select.
122. Go to the Quantities section in the Quick Access Pad and  double left-click on the Static
Pressure.
123. Click on the Representations/Contours & Iso Values section and then on the Smooth
Contour icon to display the Static Pressure.
124. Click on the icon
in the Icon Bar to use the colormap optimum range.
125. Go to the menu Representation/Isolines/Isolines....
126. Keep the default value in the Mode and Range frames, then select Uniform.
127. Click on Apply and then on Close.
3.25 CREATE 3D STREAMLINES IN DRAFT TUBE
128. Go to the menu Geometry/Boundary to hide the cutting plane and then go to the menu
Update/Delete/All to delete all previous manipulations in the Graphics area.
129. Go to the Quantities section in the Quick Access Pad.
130. Double left-click on the Vxyz (Velocity).
131. Click on the Representations/Vector Lines section.
132. Click on the Vector Lines Parameters icon.
133. Under the tab General, change Representation to tube and Color to Velocity.
134. Click on the Apply button to confirm and then click on Close.
135. In the Surfaces section in the Quick Access Pad, left-click on the symbol
before "Rotor -
Stator", then select "DT_group_12 RotorStator" and "DT_group_13 RotorStator" by left-clicking
(holding the key <Ctrl>), right-clicking and pressing Select.
136. Click on the icon Local Vector Line.
137. With the mouse, click-left multiple times on the patches "DT_group_12 RotorStator" and
"DT_group_13 RotorStator" (inlet of the draft tube) to create streamlines.
138. In the Filter (type) section in the Quick Access Pad/Surfaces, choose the option Type,
then select SOL under Select. All solid surfaces will be selected in the Surfaces section.
139. Click on the Representations/Grid section in the Quick Access Pad.
140. Click on the Render Gouraud icon.
141. Click on the Representations/Opacity section in the Quick Access Pad.
142. Set the Opacity to 0.3.
3.26 SHOW VELOCITY CONTOUR ON SV, GV
AND RUNNER B2B SURFACE
143. Go to the menu Geometry/Boundary  to hide all geometries and then go to the menu
Update/Delete/All to delete all previous manipulations in the Graphics area.
144. Go to the menu File/TurboMachinery.
The Turbomachinery mode is a unifying mode for turbomachinery analysis. It combines the display
of a SM view and a TM view in order to facilitate the creation of standard views used in
turbomachinery analysis.
To activate the Turbomachinery mode, the hub and shroud curves must be imported in CFView™.
The file used to define the hub and shroud curves can be either a CGNS file generated by
AutoGrid5™ or an ASCII data file (".dat").
145. Click on the button
to load the hub and shroud curves definition. Locate and select the
provided AutoGrid5™ mesh "SV_ GV_ Runner.cgns" in the ".../Tutorials/FINE- Open/FINE-
Open_Advanced/Tutorial_3/AG5/" folder of the tutorial package and left-click on the button Ok
to confirm.
146. Click on the button Ok to initialize the Turbomachinery mode.
147. Click on the TM view (left-bottom view) in the Graphics area. In the Surfaces section in
the Quick Access Pad, the surface "Cut at S=0.5" is selected by default.
148. Go to the menu Quantity/Field Data/Computed Thermodynamics/Wxyz to create the
new quantity Wxyz from the vector Vxyz.
149. Go to the menu Quantity/Field Data/Vector Components/Wxyz/Magnitude of W to
create the new quantity Magnitude of W from the vector Wxyz.
150. Click on the Representations/Contours & Iso Values section and then on the Smooth
Contour icon to display the Magnitude of W.
151. Click on the icon
in the Icon Bar to use the colormap optimum range.
152. Go to the menu Geometry/Repetition on/off to switch on repetition.
3.27 CREATE PRESSURE CONTOUR ON THE
HUBS AND BLADES
153. Click on the 3D view (right-upper view) to activate the 3D view.
154. Go to the menu Geometry/Boundary to hide all geometries and then go to the menu
Update/Delete/All to delete all previous manipulations in the Graphics area.
155. In the Surfaces section, left-click on the surfaces "SV_hub_(r.p.m.0)", "SV_blade", "GV_
hub_ (r.p.m.0)", "GV_ blade", "Runner_ hub_ (r.p.m. 408.93)" and "Runner_ blade_ (r.p.m.
408.93)" while holding the key <Ctrl>, then right-click and click on Select to select all the hubs
and blades of the SV, GV and Runner.
156. Click on the 3D view (right-upper view) to activate the 3D view.
157. Click on the menu Geometry/Boundary to show the boundary of the selected surfaces.
158. Go to the Quantities section in the Quick Access Pad. Double left-click on the Static
Pressure to select the quantity Static Pressure.
159. Click on the Representations/Contours & Iso Values section and then on the Strip
Contour icon to display the Static Pressure.
160. Click on the Colormap Full Range icon (
range.
) in the Icon Bar to use the colormap full
161. Click on the Fit the View icon (
) to fit the blades within the window.
162. Make use of the Viewing buttons to modify the representation mode and find a suitable
viewpoint.
3.28 PLOT BLADE LOADING ON MID-SPAN
(CARTESIAN PLOT)
163. Click on the SM view (right-bottom view) in the Graphics area to activate it. In the
Surfaces section in the Quick Access Pad, the surface "Blades" is selected by default.
164. Go to the Quantities section in the Quick Access Pad. Double left-click on the Static
Pressure to select the quantity Static Pressure.
165. Click on the Representations/Plots & Values section and then on the Blade Section
button.
166. Input <0.5> <Enter> in the keyboard input area to draw a Cartesian plot of the blade loading
at mid-span.
167. Select the File/Quit CFView menu and Yes to leave the CFView™ session.
EXPERT
The following are Expert level tutorials for FINE™/Open with OpenLabs™.
TUTORIAL 1.
USING NON-PREMIXED COMBUSTION
MODEL
This tutorial describes how to use the multiphysics modeling capabilities in FINE™/Open with
OpenLabs™ to simulate the non- premixed combustion processes and the radiative heat transfer in a
generic gas turbine combustor:
l A modeling approach for adiabatic non--premixed combustion,
l A modeling approach for non--adiabatic combustion where radiative heat losses are accounted for.
The tutorial will in special demonstrates how to:
l Generate a mesh and control the mesh quality of it,
l Define the global configuration,
l Generate combustion look-up table,
l Link the project with combustion look--up table,
l Set parameter for the combustion and radiation models,
l Set boundary and initial conditions,
l Define the numerical parameters,
l Select adequate output variables,
l Launch the calculation process,
l Monitor the convergence,
l Visualize and analyze the results,
1.1
INTRODUCTION
1.1.1
Prerequisites
The tutorial assumes that the user is familiar with the menu structure in FINE™/Open with
OpenLabs™. Some steps in the setup and solution procedure will thus not be shown explicitly.
The user is referred to the Beginner level tutorials for details on the menu structure. A more
detailed description of the combustion capabilities offered in FINE™/Open with OpenLabs™ can
be found in the User Manual in the Combustion modeling section.
1.1.2
Problem Description
A schematic picture of the generic gas turbine combustor is shown below. The main air flow is
entering the combustion chamber via a swirler nozzle. The fuel is entering the combustion
chamber separately from the air via a pipe in the center of the swirler nozzle. The swirl of the air
is causing a recirculation zone, which stabilizes the flame. After the primary combustion zone a
secondary air is injected to rapidly dilute the fuel and oxidizer mixture and to lower the
temperature in the combustor.
1.1.3
Preparation
l Download the tutorial archive as available from the Products page of the Customer Area
(www.numeca.be). Then extract the tutorial input files Tutorial_1.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <GGT-Non-premixed.iec> and click on Save or
Ok.
FINE™/Open will automatically create a project folder called "GGT-Non-premixed" which will
contain the project file (" .iec") and a folder " _mesh" where the mesh will be stored. Later,
computation folders will appear inside the project folder. It is strongly advised to keep this file
structure all along the project.
You're now ready to start the "Mesh Generation" (p. 361) process and mesh the GGT
Combustor!
MESH GENERATION
A step by step approach is proposed in the following. It aims at driving you through the various
steps that need to be executed from the creation of the mesh project to the validation of the quality
of the final mesh.
1.2
OPEN EXISTING DOMAIN
The Welcome to HEXPRESS dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined. That is why the tutorial starts from the domain file ".dom". It should be
noticed that the dialog box also enables to load geometrical files (Parasolid, CATIA v5, STL),
import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as python script.
1. Click on Import computational domain <.dom> to import the domain.
2. Select
the file GGTCombustor.dom (from your local copy of the tutorial archive as
downloaded from the Products page of the Customer Area (www.numeca.be)) and click on OK.
1.3
CREATE INITIAL MESH
3. Left-click on check box for Initial mesh in Mesh Wizard to activate the step. An activation
sign will appear inside the box dedicated to the state of the corresponding step.
4. Left-click on the Initial mesh.
5. Set the number of divisions along Cartesian axis:
l <54> <Enter> for X axis,
l <56> <Enter> for Y axis,
l <166> <Enter> for Z axis.
6. Press Go to create the Initial Mesh.
7. Use the icon
display.
in View to toggle mesh display and the icon
in View to toggle solid
1.4
MESH ADAPTATION
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selection in this action directly dictates the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming.
in terms of user
important
During the first one, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry
dependent criteria. With the second step, it removes cells intersecting the geometry or located outside
the computational domain.
8. Left-click to tick the check box for Adapt to geometry in the Mesh Wizard.
9. Left-click on Adapt to geometry.
10. Click on Global tab.
11. Set the Maximum number of refinements to <3> <Enter>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement in one or several different
directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive
refinements. This may result in an exponential growth of the total number of cells in the mesh, even
though the refinement may be confined to some areas of the computational domain. To bound the
number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may therefore alter the success of the meshing process. More details are available in the User Manual.
12. Click on Surface refinement tab.
The adaptation process is defined by three classes of criteria: curve, surface and volume criteria.
Surface criterion is considering cells which are intersecting surfaces as candidates for refinement.
Three criteria are implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
13. Define a group of entities "Level1":
l Left-click + <Ctrl> on "ggt0_group_#" for 213, 223, 235 and 264,
l Click on Group,
l Enter group name as <Level1>.
14. Left-click on "Level1".
15. Click on Active.
16. Set the maximum number of refinements to <1> <Enter>.
17. Select Target cell sizes and keep default values.
367
FINE™/Open with OpenLabs™ 7.2 Tutorials
The Maximum number of refinements per surface ultimately controls the refinement of cells
intersecting that surface (if it is presenting a value lower than the Global maximum number of
refinements from the Global parameters tab). This parameter supersedes any other selected
adaptation criteria. Fine tuning of this parameter is useful when it may be difficult to determine the
appropriate Target cell size, or if the Distance and Curvature criteria yield a prohibitive number
of cells. The default value (10000) is an arbitrary large number such that the criteria are controlled by
the Global maximum number of refinements.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell sizes for each
geometrical surface. The size of a cell
intersecting a geometrical surface are compared to the
prescribed user target and the cell is refined until its actual size is lower than the target.
18. Define a group of entities "Level2":
l Left-click + <Ctrl> on "ggt0_group_#" for 69, 70, 74, 75, 79, 80, 84, 85, 89,90, 94, 95, 99,
100, 104, 105, 109, 110, 114, 115, 119, 120, 124, 125, 198, 205, 249 and 261,
l Click on Group,
l Enter group name as <Level2>.
19. Left-click on "Level2".
20. Click on Active.
21. Set the maximum number of refinements to <2> <Enter>.
22. Select Target cell sizes and keep default values.
370
FINE™/Open with OpenLabs™ 7.2 Tutorials
23. Left-click on Box refinement tab.
Volume criterion (found in Box refinement tab) consider cells intersection or located inside a three-
dimensional volume as candidates for refinement if their cell size is larger than some user prescribed
target size.
24. Create two boxes as shown in the figures below:
l Click on New box button,
l Press <c> to define boxes by two opposite corners instead of center and corner,
l In the input bar, type <--11 -11 26> <Enter> to place the first box corner,
l In the input bar, type <11 11 42> <Enter> to place the second box corner,
l Left-click to accept "Box #0",
l Repeat above steps to create a second box "Box #1" with corners set respectively to <-3.8 -3.8
38.8> and <3.8 3.8 34.4>,
25. Impose settings for "Box #0":
l Left-click on "Box #0" in the list,
l Target cell sizes set to <0.5> <Enter> for all directions,
l Select Volumic option.
The Volumic check button allows a further control of the refinement of the cells tagged for
refinement, i.e. the cells which are within or intersection the box. When this button is unchecked, the
refinement will only occur for cells with intersection solid surfaces (SOL). If the button is checked,
the refinement applies to all cells criterion (found in Box refinement tab) consider cells intersection
or located inside a three-dimensional volume as candidates for refinement if their cell size is larger
than some user prescribed target size.
26. Impose settings for "Box #1":
l Left-click on "Box #1" in the list,
l Target cell sizes set to <0.0> <Enter> for all directions,
l Select Volumic option.
374
FINE™/Open with OpenLabs™ 7.2 Tutorials
27. Click on Go to perform the refinement and trimming.
1.5
SNAPPING & OPTIMIZATION
28. Left-click on check box for Snap to geometry in Mesh Wizard.
29. Left-click on Snap to geometry.
The Advanced >>> button gives access to three extra tabs (Global parameters, Curve snapping
and Buffer insertion). It is not necessary to change the default in this tutorial.
30. Left-click on Ok.
The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh
adaptation on the surface to obtain a good quality body conforming mesh. In addition to a simple
projection on the geometry,
lower
dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee
that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner
of the geometry and that a path of mesh edges is attached to the curve.
this action involves sophisticated algorithms to recover
Layers of additional cells (buffer insertion) are introduced into the mesh to create a body conforming
mesh. Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
31. Left-click on check box for Optimize in Mesh Wizard to activate the step.
The mesh obtained after the snapping step may involve poor quality cells usually located close to
corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
32. Left-click on Optimize.
33. Keep default settings.
34. Left-click on Ok.
35. Click on Start in Mesh Wizard to snap and optimize the mesh.
36. The mesh can be examined by using a cutting plane:
l Click on
of the viewing buttons,
l Press <x> (located among the viewing buttons) to create a cutting plane at X constant,
l Middle--click and move mouse in the view to translate the cutting plane,
l Click on the viewing buttons to perform a suitable view,
l Right-click to quit viewing options and the cutting plane menu.
379
FINE™/Open with OpenLabs™ 7.2 Tutorials
1.6
MESH QUALITY
37. Left-click on icon in Icon bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e., cells with a
negative volume. Negative cells are not allowed in the final mesh, that will be used for a flow
simulation. Concave or twisted cells are less likely to cause robustness or stability issues for the
flow solver, however their presence should be avoided.
When negative, concave or twisted cells are detected, they should be usually removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
Check mesh quality using the Criterion pull-down menu for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled. There are
presented through histograms. Each bar represents the number of cells whose criterion value is
included in the bar interval. By left-clicking on one of the bars, the corresponding cells are
displayed in the graphics area. Cells are displayed in a color varying depending on the value of
the quality criterion. The Show markers check button activates the display of circle markers for
each vertex of the displayed cells, which facilitates the localization of the selected cells.
1.7
DEFINE BOUNDARY CONDITIONS
38. Select Grid/Boundary Conditions... menu and set the boundary conditions, using the Set
face type button:
l "ggt0_group_#" for 71, 76, 81, 86, 91, 96, 101, 106, 111, 116, 121, 126, 194 and 202 as inlet
("INL"),
l "ggt0_group_177" as outlet ("OUT"),
l "ggt0_group_#" for 69, 70, 74, 75, 79, 80, 84, 85, 89, 90, 94, 95, 99, 100, 104, 105, 109, 110,
114, 115, 119, 120, 124, 125, 180, 183, 188, 193, 195, 198, 205, 213, 220, 223, 235, 249,
261, 264 and 269 as solid ("SOL").
39. Close the dialog box.
1.8
SAVE MESH
40. Go to Project/Save or click on the Save button in Icon bar.
41. Under the "_mesh" folder, enter the name of the mesh project as <GGTCombustor.igg> and
press Ok to save mesh files.
The mesh folder contain the mesh topology, geometry, grid points and the boundary condition
types among other. The files list is written below:
l .bcs: boundary conditions files,
l .dom: geometry files,
l .igg: topology file,
l .hex: grid points files,
l .rep: report file,
l .dist: distance file (prefix is domain name),
l .fnmb: FNMB connections,
l .qualityReport: quality report file.
In addition a subdirectory named "cache" contains resulting mesh files after each step of the mesh
generation (for example "_snap.hex" as resulting mesh after snapping process). It allows to delete
some steps and come back to a previous one without generating the necessary steps again.
42. Click on Close in Icon bar to quit HEXPRESS™ and return to FINE™/Open.
43. You can save the project (if not done already) and accept (yes) to link the new mesh to the
project.
44. The Mesh properties dialog box appears. Check that the information are correct (set Grid
units to Millimeters) and click on Ok.
You are now ready to start the flow settings and the post-processing of "Non-Premixed
Combustion" (p. 385)!
NON-PREMIXED COMBUSTION
1.9
FLOW SETTINGS
In this part of the tutorial, the non premixed combustion modeling capabilities are presented. The
combustion process is assumed to be adiabatic, i.e., the heat transfer due to conduction and
radiation will not be modeled.
This tutorial offers a step by step approach aiming to guide you through the various steps that
need to be executed from mesh linking to the execution of the calculation.
1.9.1
Computation Management
45. Right-click on "computation_1" in Computations area and select Rename.
46. Rename it to <NonPremixed> <Enter>.
1.9.2
Global Properties
47. In Project Parameters area, double left-click on Physical Configuration to access sub-
pages (if necessary).
48. Double left-click on General Properties to access the global parameters dialog box:
l Keep Steady mode,
l Keep Fluid block to indicate that the medium is considered as a fluid,
l Select Combustion to activate the use of the combustion modeling module.
49. Press on OK to accept and close the dialog box.
A warning issues that indicates the combustion model is not compatible with the current flow model.
The flow model will be reset to "Turbulent k-epsilon (Standard)".
50. Acknowledge the warning message and click Yes to continue.
1.9.3
Fluid Model
51. Double left-click on Fluid Model to access the fluid parameters.
52. Click on Edit ... to adapt default parameters.
53. Set the Reference pressure = <200000> <Enter> and set the Reference temperature =
<599> <Enter>.
The reference pressure is set to the outlet pressure to avoid round-off errors at low Mach number (the
reference temperature is only of importance for inert flows).
The thermal conductivity and the diffusivity coefficient are calculated via the viscosity coefficient
using the Prandtl and Schmidt numbers.
The turbulent Prandtl and Schmidt numbers can be changed via the expert parameters phys_
PrandtTurb_ and combSchmidtTurb_ in Computation Control/Control Variables menu.
54. Click on OK and Close to accept and close the dialog box.
1.9.4
Flow Model
55. Double left-click on Flow Model to access the Flow Model Parameters dialog box.
56. Keep Turbulent Navier--Stokes as Flow model.
57. Keep k-epsilon (Standard) as Turbulence model.
The gravity is kept inactive because not relevant for this test case.
58. Set Reference length to <0.004> <Enter>.
59. Set Reference velocity to <120.0> <Enter>.
Reference length and velocity inputs are required for the definition of dimensionless coefficients that
may be requested by the user during the post-treatment. However, both settings are also part of the
damping functions embedded in low Reynolds number turbulence models. The impact of both
reference parameters on the flow solution is however negligible for most practical applications.
In this tutorial, the reference length is set as the diameter of the fuel injector. The reference velocity is
fixed as the average velocity of the fuel that exits the nozzle.
60. Press on OK to accept and close the dialog box.
1.9.5
Combustion Model
61. Double left-click on the Optional Models menu.
62. Double left-click on Combustion page to access dialog box.
63. Select Non-premixed as Combustion type to model the combustion process as being of non--
premixed type.
64. Select the Flamelet as Chemistry model to use a library of flamelets.
65. Keep Mixture fraction variance eq. active to account for the turbulence chemistry
interaction.
66. Choose Thermal NO as NOx post-processing to determine the NOx formation via the post-
processing module.
The flamelet modeling assumption assumes fast chemistry. The NOx formation is however a slow
process wherefore the use of the flamelet approach does not yield accurate results.
To improve the prediction of the NOx formation, a post-processing module has been implemented in
FINE™/Open. In the NOx post-processing module, the NOx concentrations are determined directly
by solving an own transport equation for the NO concentration.
67. In the combustion table variables, a table should be linked to the computation (select under
Combustion look--up table the flamelet library "GGT_NonPremixed_Flamelet_pre.tab" from the
tutorial package under "../_tables/_NonPremixed/").
Alternatively, the user can create a new table with TabGen/Chemistry Editor:
l Click on Create/Edit...,
l Select the bb_flamelet template, the selected template is loaded in the TABGen/Chemistry Editor,
l Set Pressure value to <2e05> [Pa],
l For the fuel stream:
l Set <Species>CH4 to <1>,
l Remove <Species>H2=0.5</Species>,
l Set Temperature value to <368> [K].
l For the oxidizer stream, set Temperature value to <623> [K],
l Click on File/Rename to rename the table as <GGT_NonPremixed_Flamelet>,
l Click on Build/Generate Table to launch TABGen/Chemistry tool.
The steering file contains the inputs to generate a preintegrated flamelet table for a pressure of
200,000 Pa, preheated air at 623 K and preheated methane at 368 K for methane-air combustion. The
chemical mechanism GRI-3.0 is used, which is read from the file "gri30.chm".
At the end, the table is successfully generated and automatically linked to the computation.
l Click on File/Close,
l Click on Preview... to visualize the table.
TABGen/Chemistry is a tool that generates, retabulates and preintegrates combustion tables according
to user. The tool is currently only available for Linux platforms (please refer to user manual for more
information).
The generated tables contain the density, the temperature, viscosity, thermal conductivity, species
concentrations as well as source terms for the NOx post- processing module. These tables are
generated for a given pressure in dependence of the temperature and the composition of the fuel and
oxidizer streams and thus specific for each configurations.
All the thermodynamic, chemical, and transport properties are determined from combustion look-up
tables. In these tables the thermo-chemical properties of a given reactive fuel-oxidizer mixture are
stored in dependence of one or several combustion transport variables (mixture fraction, its variance,
progress variable, enthalpy defect and/or strain).
All
the
independent solution variables are available for post- processing by default. However,
dependent, thermo-chemical quantities will only be available for post-processing after the user has
specifically selected them for output.
68. Press on OK to accept and close the dialog box.
1.9.6
Boundary Conditions
69. Double left-click on the Boundary Conditions menu.
70. Double left-click on the Boundary Conditions page to access dialog box.
71. Go to the INLET tab.
72. Create a group "Primary Air" of the 12 entrances of the primary air stream:
l Left-click + <Ctrl> on "ggt0_group_71", "ggt0_group_76", "ggt0_group_81", "ggt0_group_
86", "ggt0_ group_ 91", "ggt0_ group_ 96", "ggt0_ group_ 101", "ggt0_ group_ 106", "ggt0_
group_111", "ggt0_group_116", "ggt0_group_121" and "ggt0_group_126",
l Click on Group,
l Enter group name as <PrimaryAir> <Enter>.
73. Impose primary air stream conditions:
l Click on group "PrimaryAir",
l Select Subsonic and Cylindrical,
l Select Mass flow imposed/Velocity Direction,
l Set Vr/V to <1> <Enter>,
l Set Vt/V and Vz/V to <0> <Enter>,
l Set Mass-Flow to <0.03> <Enter>,
l Set k to <13.5> <Enter>,
l Set Epsilon to <8150> <Enter>,
l Set Mixture fraction to <0> <Enter>,
l Set NO mass fraction to <0> <Enter>.
394
FINE™/Open with OpenLabs™ 7.2 Tutorials
395
FINE™/Open with OpenLabs™ 7.2 Tutorials
The mixture fraction variable can be considered as a normalized fuel mass fraction or more precisely
the mass fraction of the flow that originates from the fuel inlet. Its value should consequently equal to
unity for the fuel stream and vanish for the oxidizer stream.
The inlet concentration of NO should be set to zero (except in situation where NO has been generated
upstream of the inlet plane).
74. Impose secondary air stream conditions:
l Select the "ggt0_group_194",
l Select Subsonic and Cylindrical,
l Select Mass flow imposed/Velocity Direction,
l Set Vr/V and Vt/V to <0> <Enter>,
l Set Vz/V to <1> <Enter>,
l Set Mass-Flow to <0.045> <Enter>,
l Set k to <13.5> <Enter>,
l Set Epsilon to <8150> <Enter>,
l Set Mixture fraction to <0> <Enter>,
l Set NO mass fraction to <0> <Enter>.
397
FINE™/Open with OpenLabs™ 7.2 Tutorials
Since the secondary air stream has the same temperature (and composition) as the primary one, the
present configuration still represents a two-stream problem.
75. Impose fuel stream conditions:
l Select the "ggt0_group_202",
l Select Subsonic and Cylindrical,
l Select Mass flow imposed/Velocity Direction,
l Set Vz/V to <1> <Enter>,
l Set Vr/V and Vt/V to <0> <Enter>,
l Set Mass--Flow to <0.0014> <Enter>,
l Set k to <132> <Enter>,
l Set Epsilon to <620000> <Enter>,
l Set Mixture fraction to <1> <Enter>,
l Set NO mass fraction to <0> <Enter>.
76. Go to the OUTLET tab.
77. Select the outlet patch.
78. Select Subsonic and Cartesian.
79. Select Pressure Imposed/Static Pressure Imposed.
80. Set Static Pressure to <200000> <Enter>.
Since the combustion transport variables represent convected quantities, no extra condition needs to
be specified for these variables at an outlet.
81. Go to the SOLID tab.
82. Create a group "solid" of all solid patches:
l Left-click on first patch,
l Left-click + <Shift> on last patch,
l Click on Group,
l Enter group name as <Solid> <Enter>.
83. Impose solid conditions:
l Click on group "Solid",
l Keep Adiabatic to set all solid walls as adiabatic.
Even if no radiation modeling is chosen, the selection of a non-adiabatic wall treatments activates the
solution of a transport equation for the enthalpy.
84. Press on OK to accept and close the dialog box.
1.9.7
Initial Solution
85. Double left-click on the Initial Solution menu.
86. Double left-click on the Initial Solution page to access dialog box.
87. Activate Constant values.
88. Select Cartesian.
89. Set Pressure = <200000> <Enter>.
90. Set Vx and Vy to <0.0> <Enter>.
91. Set Vz to <1.0> <Enter>.
92. Set k to <13.5> <Enter>.
93. Set epsilon to <8150.0> <Enter>.
94. Set Mixture fraction to <0.0> <Enter>.
95. Left-click on OK to accept and close the dialog box.
Set the mixture fraction to zero (it makes sense to start the simulation of the combustor from a
condition where it is filled with pure air).
Initialize the flow velocities by defining a small initial axial velocity component (Vz = 1 m/s). Set the
initial field of the turbulent quantities to the boundary conditions of the air streams.
1.9.8 Numerical Parameters
96. Double left-click on the Numerical Parameters menu.
97. Double left-click on the General Parameters page.
98. Keep Number of grid(s) to <4> <Enter>.
99. Keep Correction damping and Coarse grid initialization active.
100. Go to the Advanced tab.
101. Set Maximum number of cycles per grid level to <600> <Enter>.
102. Set Convergence criteria on each grid level to <-6.0> <Enter>.
103. Left-click on OK to accept and close the dialog box.
104. Double left-click on the Numerical Schemes page.
105. Keep 2nd order central scheme for the RANS equations (the combustion transport equations
and the turbulent flow equations are solved using an upwind discretization).
106. Keep CFL number set to <1.5> <Enter>.
When simulating combustion, the CFL number is by default set to 1.5 instead of 3.
Time derivative preconditiong is always activated when combustion modeling is used.
107. Set Characteristic velocity to < 20.0 > < Enter >. This velocity is representative in its
magnitude for the velocities in the combustor.
108. Keep default parameters for preconditioning and local velocity scaling active.
109. Left-click on OK to accept and close the dialog box.
1.9.9
Computation Control
110. Double left-click on the Computation Control menu.
111. Double left-click on the Outputs page.
112. Under General thumbnail, select Combustion in Categories.
113. Select the quantities "LookUpTable_ RHO", "LookUpTable_ TEMP", "LookUpTable_
CO2",
and
"LookUpTable_ CO" to post-process ("Comb_ NOxPOst" (NO concentration) and "Comb_
SourceTermNO" are selected by default):
"LookUpTable_ H2O",
"LookUpTable_ CH4"
"LookUpTable_ OH",
l Left-click on quantity or species in the list,
l Click on Add -->.
114. Left-click on OK to accept and close the dialog box.
115. Double left-click on the Control Variables page.
116. Set Number of iterations to <4000> <Enter>.
An increase (from default values) in the number of iterations conducted on the finest grid level is
often needed running combustion projects. This is mainly related to coexistence of different physical
scales, which makes the convergence slower.
117. Set Convergence criteria to <-6> <Enter>.
The flow filed is very dependent on the mixture fraction field. Thus, for an accurate result, it is
important to ensure that the mixture fraction field is properly converged.
118. Set Save solution every to <100> <Enter>.
119. Double left-click on the Launching Mode page.
120. Select Parallel. Change the Total number of processors to 3. When clicking on icon in
front of "Partition #", the partition can be visualized in the GUI.
121. Left-click on OK to accept and close the dialog box.
1.9.10 Save Project & Computation
122. In Project/Preferences menu, select Full-double-precision mode to run the flow solver in
double precision mode.
123. In Project menu, select Save to save the project (".iec").
124. In Project menu, select Save Selected 'Run' Files to save the ".run" file of the selected
computation.
FINE™/Open will automatically create a computation folder inside the project folder. It is strongly
advised to stick with this file structure.
1.9.11 Monitoring Convergence
125. Click on icon to start the calculation in parallel.
126. Click on Parallel settings... to adapt the default assignment of the partitions in the Parallel
settings dialog box.
127. Double left-click on OK to accept and start the computation in parallel.
FINE™/Open includes the ability to manage computation through a task manager (
batch mode. More details can be found in FINE™/Open User Manual.
) and /or in
128. Click on the icon
to track the evolution of residuals with the iterations.
The evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out) and/or global
quantities (efficiency, pressure ratio, torque and axial thrust on solid walls selected in the
boundary conditions page) can be performed in the steering. Local and global quantities may also
be added for follow up during the convergence process. However, their representation in the
graphical area will be effective only once they will be added, and past history will not be
available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out, with satisfactory correspondence (usually less than 0.5%
difference between in/out). To do so, select the inlet and outlet mass flow at once. An
information about the difference is automatically computed.
A more detailed description of the convergence history per equation and per domain is available
in the Monitor
.
Once the calculation is converged or reaches the maximum number of iterations allowed on the
finest grid level, the flow solver stops. The final solution is then stored for post--processing and the
task manager window is closed.
1.10 POST-PROCESSING: NON-PREMIXED
COMBUSTION
129. Click on the icon
to access CFView™ from the FINE™/Open GUI.
For post processing and visualization of computational results, NUMECA has CFView™, which
is integrated in the FINE™/Open environment and includes numerous tools.
A step by step approach is taken in the following. It aims at guiding you through the various steps
that need to be executed from reading the solution to the extraction of the main results. Quantities
will be plotted on cutting planes.
1.10.1
Create Cutting Plane
130. Click on Cut in the Surfaces area to create a cutting plane or click on Geometry/Create
Cutting plane... menu.
131. Select Geometry.
132. Set the Point coordinates to X = <0> <Enter> and Y = <0> <Enter>.
133. Click on X button to define a plane at X constant.
134. Click on Apply and Save.
135. Click on Y button to define a plane at Y constant.
136. Click on Apply and Save.
137. Close the dialog box.
1.10.2 Select Area of Interest
138. Visualize solid surfaces with rendering:
l In the Surfaces area, left-click on "Solid" group in the Surfaces area.
l Right-click and Select to only activate "Solid" group (all solid surfaces).
l Click on
in Representations/Grid in Quick Access Pad.
l Set Opacity to 0.3 in Representations area.
139. Left-click + <Ctrl> on "CUT1" and "CUT2" in the Surfaces area.
140. Right-click and Select to only activate cutting planes.
1.10.3 Select & Visualize Quantities
141. In Quantities area, double left-click on "LookUpTable_TEMP". This is done to visualize
the static temperature, which is determined in the simulation via a look-up in the combustion
tables.
142. Left-click on Contours & Iso Values in Representations area.
143. Click on the icon
cutting planes.
Smooth Contour to plot color contour of the temperature on the
144. Click on the icon Isolines
to plot isolines of the temperature on the cutting planes:
l Set number of isolines to <21> <Enter>,
l Set Color to Uniform,
l Click on Apply,
l Close the dialog box.
145. Select Update/Delete/All to refresh the graphics area.
146. Repeat above steps to plot on cutting planes the "Comb_NOxPost" (NO concentration),
"LookUpTable_CO2" and "LookUpTable_CH4".
416
FINE™/Open with OpenLabs™ 7.2 Tutorials
417
FINE™/Open with OpenLabs™ 7.2 Tutorials
147. Remove boundaries of cutting planes in graphics area:
l Left-click + <Ctrl> on "CUT1" and "CUT2" in the Surfaces area,
l Right-click and Select to only activate cutting planes,
l Type on <b> to remove boundaries.
148. Visualize solid surfaces with rendering:
l In the Surfaces area, left-click on "Solid" group in the Surfaces area,
l Right-click and Select to only activate "Solid" group (all solid surfaces),
l Click on
in Representations/Grid in Quick Access Pad,
l Set Opacity to 0.5 in Representations area
149. Select all inlets:
l Select Type as Filter (type) in the Surfaces area,
l Select "All" in Unselect entry box,
l Select "INL" in Select entry box.
150. In Quantities area, double left-click on "Vxyz".
151. Left-click on Vector Lines in Representations area.
152. Click on the icon Vector Lines Parameters
to set streamlines settings.
153. Change Representation to ribbon.
154. Set Color to Velocity.
155. Keep Direction to forward and Mode to volume.
156. Apply and Close.
157. Click on the icon Vector Lines from Section
inlets.
to create streamlines from sections on
158. Move the mouse close to one of the inlets of the main air stream.
159. Left-click and drag in graphics area on inlet to select first and second point of the section as
presented in below figures.
160. Repeat above steps on all inlets of the main air stream.
Next part shows the flow settings and the post-processing of "Non-Premixed Combustion
with radiative heat losses" (p. 423)!
NON-PREMIXED COMBUSTION WITH
RADIATIVE HEAT LOSSES
1.11
FLOW SETTINGS
This part of the tutorial will show how to use the radiation modeling capabilities:
l activation of the radiation modeling;
l setting of parameters of the radiation model;
l definition of boundary conditions for the radiation model.
161. Create a new computation as a duplicate of the computation "NonPremixed":
l Left-click on "NonPremixed" in Computations area,
l Right-click and Select New,
l Right-click on "new_NonPremixed" and select Rename,
l Rename it to <NonPremixed_Radiation> <Enter>.
When selecting a computation and then creating a new computation, the new computation is a copy of
the selected computation. All the settings in the selected computation will be kept in the new one.
In Project Parameters area, double left- click on Physical Configuration to access
162.
subpages (if necessary).
163. Double left-click on General Properties to access the global parameters dialog box:
l Keep Steady mode,
l Keep Fluid block to indicate that the block is considered as fluid,
l Keep Combustion to activate the use of the combustion module,
l Select Radiation to activate the use of the radiation module,
l Click on OK to accept and close the dialog box.
1.11.1
Radiation Model
164. Double left-click on the Optional Models menu (if necessary).
165. Double left-click on Combustion page to access dialog box.
166. In the combustion table variables, a table taking non-adiabatic effect into account should be
used (select under Combustion look-- up table the flamelet library "GGT_ NonPremixed_
Flamelet_ NonAdiabatic_ pre.tab" from the tutorial package under ../_ tables/_ NonPremixed_
Radiation/)
Alternatively, the table considering non- adiabatic effect can be created with TABGen/Chemistry
Editor:
l Click on Create/Edit...
l Add the command <nonadiabatic/>,
l Click on File/Rename to rename the table as <GGT_NonPRemixed_Flamelet_NonAdiabatic>,
l Click on Build/Generate Table to launch TABGen/Chemistry tool.
The steering file contains the inputs to generate a non adiabatic preintegrated flamelet table for a
pressure of 200,000 Pa, preheated air at 623 K and preheated methane at 368 K for methane- air
combustion. The chemical mechanism GRI-3.0 is used, which is read from the file "gri30.chm".
At the end, the table is successfully generated and automatically linked to the computation.
167. Keep all other settings and click on the button OK.
168. Double left-click on Radiation page to access dialog box.
169. Select the 1st order spherical harmonics (P1) as Radiation model, the Weighted-Sum-
Gray- Gases (WSGG) for the determination of the optical properties and set the level of
Turbulence--radiation interaction to None.
170. Left-click on OK to accept and close the dialog box.
If both combustion and radiation modelling are selected, a transport equation for the enthalpy is
solved. The thermochemical properties in this case are to be tabulated in dependence of the enthalpy
defect.
1.11.2
Boundary Conditions
171. Double left-click on the Boundary Conditions menu (if necessary).
172. Double left-click on the Boundary Conditions page to access dialog box.
173. Go to the SOLID tab.
174. Keep Emission coefficient set to <1.0> <Enter> for the "solid" group.
175. Press on OK to accept and close the dialog box.
1.11.3
Save Project & Computation, Monitoring Convergence
176. launch the computation and monitor the convergence.
428
FINE™/Open with OpenLabs™ 7.2 Tutorials
1.12
POST-PROCESSING: NON-PREMIXED
COMBUSTION WITH RADIATIVE HEAT
LOSSES
177. Click on the icon
to access CFView™ from the FINE™/Open GUI.
178. Select the menu Update / Insert Text , click in the view and enter the text <With
Radiation>.
179. Right-click and select the contextual menu Text Type ....
180. Set the font Size to <32> and click the button Apply. Click Close.
181. Left-click on the text, keep left button pressed and move the mouse to move the location of
the text.
182. Open the combustion result without radiation ).
l Select the menu File / Open Project ....
l Locate the computation directory (GGT-Non-premixed\GGT-Non-premixed_NonPremixed\)
and open the computation file 'GGT-Non-premixed_NonPremixed.run'.
183. Select the menu Update / Insert Text, enter the text <Without Radiation> and set its size to
<32>.
184. Select the menu Window / Tile view.
185. Create contour in the left view (refer to "Non-Premixed Combustion" (p. 385)).
l Click on the left view,
l Create two cutting planes,
l Create contour of "LookUpTable_TEMP", use Strip Contour instead of Smooth Contour.
186. Create contour in the right view following the step above.
187. Click on the left view, select the menu View / Align Views, then click on the right view to
align view in the left view and right view.
188. Click on the left view, select the menu View / Match Ranges, then click on the right view
to match the legend in the left view and right view.
In the last picture, the temperature field of the non- adiabatic simulation is shown (left). A
comparison with the temperature field of the adiabatic simulation would show that the radiative
heat transfer has the effect of slightly decreasing the temperature.
TUTORIAL 2.
SIMULATE NON-PREMIXED COMBUSTION
WITH CHT
This tutorial describes how to use the multiphysics modeling capabilities in FINE™/Open with
OpenLabs™ to simulate the non- premixed combustion processes considering the conjugate heat
transfer in the chamber wall in a generic gas turbine combustor. The tutorial will start from a well
set non-premixed combustion computation and explain how to consider the solid domain in detail.
The tutorial will in special demonstrates how to:
l Generate a solid mesh and control the mesh quality,
l How to connect the fluid block and solid block,
l Generate combustion look-up table when considering CHT,
l Set parameter for CHT simulation,
l Visualize and analyze the results,
2.1
INTRODUCTION
2.1.1
Prerequisites
The tutorial assumes that the user is familiar with the non-premixed combustion simulation. Some
steps in the setup and solution procedure will thus not be shown explicitly. The user should refer
to the tutorial "USING NON-Premixed combustion model" (p. 357) for details. A more detailed
description of the combustion capabilities offered in FINE™/Open with OpenLabs™ can be
found in the User Manual in the Combustion modeling section.
2.1.2
Problem Description
A schematic picture of the generic gas turbine combustor is shown below. The main air flow is
entering the combustion chamber via a swirler nozzle. The fuel is entering the combustion
chamber separately from the air via a pipe in the center of the swirler nozzle. The swirl of the air
is causing a recirculation zone, which stabilizes the flame. After the primary combustion zone a
secondary air is injected to rapidly dilute the fuel and oxidizer mixture and to lower the
temperature in the combustor.
In this tutorial, the heat transfer in the combustion chamber wall will be considered.
2.1.3
Preparation
l Download the tutorial archive as available from the Products page of the Customer Area
(www.numeca.be). Then extract the tutorial input files 'Tutorial_2'.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
2.2 OPEN EXISTING PROJECT
1. After launching the FINE™/Open GUI, click on the icon Open an existing project and click
on the button Ok to confirm.
2. Locate and select the project name "GGT-CHT/GGT-CHT.iec" in the dialog box and click on
the button Ok to confirm.
3. Select the computation "NonPremixed" under Computations. Check all the settings in the
FINE™/Open GUI. In this tutorial, a Non-premixed combustion computation has been created
and provided. The main settings are:
l Fluid model: Reactive fluid
l Flow model: Turbulence Navier-Stokes with k-epsilon (Standard) model
l Combustion model
l Combustion type: Non-Premixed
l Chemistry model: Flamelet
l Mixture fraction variance eq. is activated
l Combustion look-up table: not defined
l Inlet boundary condition - PrimaryAir: Mass flow imposed - Velocity Direction
l Vr/V = 1
l Vz/V = Vt/V = 0
l Mass-Flow = 0.03 kg/s
l k = 13.5 m2/s2
l Epsilon = 8150 m2/s3
l Mixture fraction = 0
l NO mass fraction = 0
l Inlet boundary condition - SecondaryAir: Mass flow imposed - Velocity Direction
l Vr/V = Vt/V = 0
l Vz/V = 1
l Mass-Flow = 0.045 kg/s
l k = 13.5 m2/s2
l Epsilon = 8150 m2/s3
l Mixture fraction = 0
l NO mass fraction = 0
l Inlet boundary condition - fuel: Mass flow imposed - Velocity Direction
l Vr/V = Vt/V = 0
l Vz/V = 1
l Mass-Flow = 0.0014 kg/s
l k = 132 m2/s2
l Epsilon = 620000 m2/s3
l Mixture fraction = 1
l NO mass fraction = 0
l Outlet boundary condition: Pressure Imposed
l Static Pressure = 200000 Pa
l Initial solution: Constant values
l Pressure = 200000 Pa
l Vx = 0 m/s
l Vy = 0 m/s
l Vz = 1 m/s
l k = 13.5 m2/s2
l epsilon = 8150 m2/s3
l Mixture fraction = 0
l Coarse grid initialization is activated in the Numerical Parameters / General Parameters
page with 4 grid levels. The convergence criteria is set to 600/-6.
l CFL = 1.5
l Hakimi preconditioning is used with the characteristic velocity of 20 m/s.
2.3 MESH GENERATION
This part of the tutorial shows how to add a solid block surrounding the chamber and generate the
mesh.
4. Click on HEXPRESS™ button in the Icon Bar to open HEXPRESS™.
Keep the mesh of the combustion chamber. A solid block will be added to generate a new mesh.
5. Import the solid domain:
l Left-click on Project in Menu Bar,
l Left-click on Import.../Domain,
l Select the "solid_1.dom" file from the tutorial folder and click on OK.
The block is automatically added.
2.3.1
Create Initial Mesh
6. Select "solid_1" in Active domain in the Icon Bar.
7. Left-click to tick the check box for Initial mesh in Mesh Wizard for activation.
8. Left-click on the Initial mesh.
9. Set the number of divisions along Cartesian axis:
l <300> <Enter> for X axis,
l <300> <Enter> for Y axis,
l <100> <Enter> for Z axis.
10. Press Go to create the Initial Mesh.
2.3.2 Mesh Adaptation
11. Left-click to check Adapt to geometry in the Mesh Wizard.
12. Click on Step in Mesh Wizard to perform the step without refinement.
2.3.3
Snapping & Optimization
13. Left-click on check box for Snap to geometry in Mesh Wizard.
14. Left-click on Snap to geometry.
15. Keep default settings.
16. Left-click on Ok.
17. Left-click on check box for Optimize in Mesh Wizard to activate the step.
18. Left-click on Optimize.
19. Keep default settings.
20. Left-click on Ok.
21. Click on Start in Mesh Wizard to snap and optimize the mesh.
2.3.4
FNMB Connection
22. Go to Grid/Non matching Connections....
23. Left-click on Search Connections.
24. Select "connection_1" and left-click on Compute.
25. Click on Close when the computation is over (status is marked as "Successful").
2.3.5 Mesh Quality
26. Left-click on icon in Icon Bar to check the mesh quality.
An important check of the mesh quality is to detect the presence of negative cells, i.e., cells with a
negative volume. Negative cells are not allowed in the final mesh, that will be used for a flow
simulation. Concave or twisted cells are less likely to cause robustness or stability issues for the
flow solver, however their presence should be avoided.
Check mesh quality using the Criterion pulldown menu for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
Furthermore, the cell orthogonality, aspect ratio and expansion ratio can be controlled.
2.3.6
Save Mesh
27. Go to Project/Save as....
28. Under the "_mesh" folder, enter the name of the mesh project as <GGTCombustor_wall>.
29. Click OK to save mesh files.
30. Click on Close in Icon Bar to quit HEXPRESS™ and return to FINE™/Open.
31. You can save the project (if not done already) and accept (yes) to link the new mesh to the
project.
32. Left-click on Merge and Close.
33. The Mesh properties dialog box appears. Check that the information are correct (set Grid
units to Millimeters) and click on Ok.
2.4
FLOW SETTINGS
2.4.1
Global Properties
34. In Project Parameters area, double left-click on Physical Configuration to access sub-
pages (if necessary).
35. Double left-click on General Properties to access the global parameters dialog box:
l Select "solid_1" under Domain Configuration,
l Activate Solid block to indicate that block is considered as a solid,
l Left-click on Ok.
36. Double left-click on Solid Model to access the global parameters dialog box:
l Select "solid_1",
l Set the Constant value to <10> <Enter>.
l Left-click on Ok.
2.4.2
Combustion Model
37. Double left-click on Combustion page to access dialog box.
38. In the combustion table variables, a table should be linked to the computation (select under
Combustion look--up table the flamelet library "GGT_NonPremixed_Flamelet_HighHeatLoss_
pre.tab" from the tutorial package under .../_tables/_NonPremixed_CHT/).
If the user generates the look up table by TabGen/Chemistry, the keyword <nonadiabatic/> is not
sufficient due to the high heat loss (> 2E5 J/kg). So the keyword <nonadiabatic_extrapolation/>
should be used to generate a table with a high heat loss (default value is 2.4E6 J/kg).
2.4.3
Boundary Conditions
39. Double left-click on the Boundary Conditions menu.
40. Double left-click on the Boundary Conditions page to access dialog box.
41. Go to the SOLID tab.
42. Select the patch "group_0":
l Select Temperature Imposed.
l Set Static Temperature to <1200> <Enter>.
l Keep Adiabatic to set "group_1connection_1*", "group_2" and "group_3" as adiabatic.
l Left-click on Ok.
2.4.4
Initial Solution
43. Double left-click on the Initial Solution menu. Double left-click on the Initial Solution page.
44. Select "solid_1" and set Temperature to <1500> <Enter>. Left-click on Ok.
2.4.5 Numerical Parameters
45. Double left-click on the Numerical Parameters menu.
46. Double left-click on the General Parameters page.
47. Keep Number of grid(s) to 4.
48. Keep Correction damping and Coarse grid initialization active.
49. Left-click on Ok to accept and close the dialog box.
50. Double left-click on the Numerical Schemes page.
51. Select "solid_1" and set CFL number to <1.5> <Enter>.
52. Left-click on Ok to accept and close the dialog box.
2.4.6
Computational Control
53. Double left-click on the Computation Control menu.
"LookUpTable_ RHO",
54. On the Outputs page under the General tab, select Combustion in Categories, Then select
the quantities
"LookUpTable_ CO2",
"LookUpTable_H2O", "LookUpTable_OH", "LookUpTable_CH4" and "LookUpTable_CO"
to post-process ("Comb_ NOxPOst" (NO concentration) and "Comb_ SourceTermNO" are
selected by default):
"LookUpTable_ TEMP",
55. Double left-click on the Control Variables page.
56. Go to the Advanced tab and Select category as Local Parameters (by domain).
57. Select the fluid block:
l Set RelaxCombVars_ expert parameter to <0.5 0.5 0.5 1.0 0.01 0.5 1.0> <Enter>,
l Keep turb_KEpsProd_ expert parameter to <1> <Enter>,
l Set IterScalingFuncheatFlux_ expert parameter to <500> <Enter>.
58. Left-click on Ok to accept and close the dialog box.
59. Double left-click on the Launching Mode page.
60. Select Parallel, set Total number of processors to <6> <Enter>.
61. Left-click on OK to accept and close the dialog box.
2.4.7
Save Project & Computation
62. In Project/Preferences menu, select Full-double-precision mode to run the flow solver in
double precision mode.
63. In Project menu, select Save to save the project (".iec").
64. In Project menu, select Save Selected 'Run' Files to save the ".run" file of the selected
computation.
2.4.8 Monitoring Convergence
65. Click on Start Flow Solver icon to start the calculation in parallel.
66. Double left-click on Ok to accept and start the computation in parallel.
67. Click on
or
icons to track the evolution of residuals with the iterations.
Once the calculation is converged or reaches the maximum number of iterations allowed on the
finest grid level, the flow solver stops. The final solution is then stored for post--processing and the
task manager window is closed.
2.5
POST-PROCESSING
68. Click on the icon
to access CFView™ from the FINE™/Open GUI.
69. Click on Cut in the Surfaces area to create a cutting plane or click on Geometry/Create
Cutting plane... menu.
70. Select Geometry.
71. Set the Point coordinates to X = <0> <Enter> and Y = <0> <Enter>.
72. Click on X button to define a plane at X constant.
73. Click on Apply and Save.
74. Click on Y button to define a plane at Y constant.
75. Click on Apply and Save.
76. Close the dialog box.
77. Visualize solid surfaces with rendering:
l In the Surfaces area, <Ctrl> + left-click on the groups "Solid", "group_0_Solid", "group_1_
Solid", "group_2_Solid" and "group_3_Solid".
l Right-click and click on Select to activate "Solid" groups (all solid surfaces).
l Click on
in Representations/Grid in Quick Access Pad.
l Set Opacity to 0.3 in Representations area.
78. Left-click + <Ctrl> on "CUT1" and "CUT2" in the Surfaces area.
79. Right-click and Select to only activate cutting planes.
80. In Quantities area, double left-click on "LookUpTable_TEMP". This is done to visualize the
static temperature, which is determined in the simulation via a look-up in the combustion tables.
81. Left-click on Contours & Iso Values in Representations area.
82. Click on the icon
cutting planes.
Smooth Contour to plot color contour of the temperature on the
83. Click on the icon Isolines
to plot isolines of the temperature on the cutting planes:
l Set number of isolines to <21> <Enter>,
l Set Color to Uniform,
l Click on Apply,
l Close the dialog box.
454
FINE™/Open with OpenLabs™ 7.2 Tutorials
TUTORIAL 3.
SIMULATE PARTIALLY-PREMIXED
COMBUSTION
This tutorial describes how to use the multiphysics modeling capabilities in FINE™/Open with
OpenLabs™ to simulate the partially-premixed combustion in a generic gas turbine combustor. The
tutorial will start from a generated mesh and explain how to setup a partially-premixed combustion
simulation. The use of the partially premixed module has the advantage that finite rate effects can be
captured and that the lifting of the flame can be predicted.
The tutorial will in special demonstrates how to:
l Set up a partially-premixed combustion simulation with the FGM model,
l Set up a partially-premixed combustion simulation with the BML/Flamelet model,
3.1
INTRODUCTION
3.1.1
Prerequisites
The tutorial assumes that the user is familiar with the menu structure in FINE™/Open with
OpenLabs™. Some steps in the setup and solution procedure will thus not be shown explicitly.
The user is referred to the Beginner level tutorials for details on the menu structure. A more
detailed description of the combustion capabilities offered in FINE™/Open with OpenLabs™ can
be found in the User Manual in the Combustion modeling section.
3.1.2
Problem Description
A schematic picture of the generic gas turbine combustor is shown below. The main air flow is
entering the combustion chamber via a swirler nozzle. The fuel is entering the combustion
chamber separately from the air via a pipe in the center of the swirler nozzle. The swirl of the air
is causing a recirculation zone, which stabilizes the flame. After the primary combustion zone a
secondary air is injected to rapidly dilute the fuel and oxidizer mixture and to lower the
temperature in the combustor.
3.1.3
Preparation
l Download the tutorial archive as available from the Products page of the Customer Area
(www.numeca.be). Then extract the tutorial input files 'Tutorial_3'.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
3.2
IMPORT AN EXISTING MESH
1. After launching the FINE™/Open GUI, click on the icon Importing a mesh and click on the
button Ok to confirm.
2. Select a directory and enter a project name "GGT-Partially-Premixed" in the dialog box and
click on the button Ok to confirm.
3. Select the provided mesh "GGTCombustor.igg" located "../_mesh/"
4. The mesh properties dialog box appears. Check that the information are correct (set Grid units
to Millimeters) and click on Ok to close the mesh properties dialog box.
3.3
FLOW SETTINGS AND POST-PROCESSING:
FGM MODEL
3.3.1
Computation Management
5. Right-click on "computation_1" in Computations area and select Rename.
6. Rename it to "FGM" <Enter>.
3.3.2
Global Properties
7. In Project Parameters area, double left-click on Physical Configuration to access sub-pages
(if necessary).
8. Double left-click on General Properties to access the global parameters dialog box:
l Keep Steady mode,
l Keep Fluid block to indicate that the medium is considered as a fluid,
l Select Combustion to activate the use of the combustion modeling module.
9. Press on OK to accept and close the dialog box.
A warning issues that indicates the combustion model is not compatible with the current flow model.
The flow model will be reset to "Turbulent k-epsilon (Standard)".
10. Acknowledge the warning message and click Yes to continue.
3.3.3
Fluid Model
11. Double left-click on Fluid Model to access the fluid parameters.
12. Click on Edit ... to adapt default parameters.
13. Set the Reference pressure = <200000> <Enter> and set the Reference temperature =
<599> <Enter>.
The reference pressure is set to the outlet pressure to avoid round-off errors at low Mach number (the
reference temperature is only of importance for inert flows).
The thermal conductivity and the diffusivity coefficient are calculated via the viscosity coefficient
using the Prandtl and Schmidt numbers.
The turbulent Prandtl and Schmidt numbers can be changed via the expert parameters phys_
PrandtTurb_ and combSchmidtTurb_ in Computation Control/Control Variables menu.
14. Click on OK and Close to accept and close the dialog box.
3.3.4
Flow Model
15. Double left-click on Flow Model to access the Flow Model Parameters dialog box.
16. Keep Turbulent Navier--Stokes as Flow model.
17. Keep k-epsilon (Standard) as Turbulence model.
The gravity is kept inactive because not relevant for this test case.
18. Set Reference length to <0.004> <Enter>.
19. Set Reference velocity to <120.0> <Enter>.
Reference length and velocity inputs are required for the definition of dimensionless coefficients that
may be requested by the user during the post-treatment. However, both settings are also part of the
damping functions embedded in low Reynolds number turbulence models. The impact of both
reference parameters on the flow solution is however negligible for most practical applications.
In this tutorial, the reference length is set as the diameter of the fuel injector. The reference velocity is
fixed as the average velocity of the fuel that exits the nozzle.
20. Press on OK to accept and close the dialog box.
3.3.5
Combustion Model
21. Double left-click on the Optional Models menu.
22. Double left-click on Combustion page to access dialog box.
23. Select the Partially premixed as Combustion type to model the combustion process as
being of partially premixed type.
24. Select the Manifold technique (FGM) as Chemistry model.
25. Keep active Mixture fraction variance eq.
interaction.
to account for the turbulence chemistry
26. Select under Combustion look--up table a look-up table "GGT_PartialPremixed_FGM.tab"
from the tutorial package under ./_tables/_PartiallyPremixed_FGM/.
27. Choose Thermal NO as NOx post-processing to determine the NOx formation via the post-
processing module.
28. Press on OK to accept and close the dialog box.
3.3.6
Boundary Conditions
29. Double left-click on the Boundary Conditions menu.
30. Double left-click on the Boundary Conditions page to access dialog box.
31. Go to the INLET tab.
32. Create a group "Primary Air" of the 12 entrances of the primary air stream:
l Left-click + <Ctrl> on "ggt0_group_71", "ggt0_group_76", "ggt0_group_81", "ggt0_group_
86", "ggt0_ group_ 91", "ggt0_ group_ 96", "ggt0_ group_ 101", "ggt0_ group_ 106", "ggt0_
group_111", "ggt0_group_116", "ggt0_group_121" and "ggt0_group_126",
l Click on Group,
l Enter group name as <PrimaryAir> <Enter>.
33. Impose primary air stream conditions:
l Click on group "PrimaryAir",
l Select Subsonic and Cylindrical,
l Select Mass flow imposed/Velocity Direction,
l Set Vr/V to <1> <Enter>,
l Set Vt/V and Vz/V to <0> <Enter>,
l Set Mass-Flow to <0.03> <Enter>,
l Set k to <13.5> <Enter>,
l Set Epsilon to <8150> <Enter>,
l Set Mixture fraction to <0> <Enter>,
l Set NO mass fraction to <0> <Enter>.
l Set ProgressVariable1 set to <0.0> <Enter>.
The mixture fraction variable can be considered as a normalized fuel mass fraction or more precisely
the mass fraction of the flow that originates from the fuel inlet. Its value should consequently equal to
unity for the fuel stream and vanish for the oxidizer stream.
The inlet concentration of NO should be set to zero (except in situation where NO has been generated
upstream of the inlet plane).
34. Impose secondary air stream conditions:
l Select the "ggt0_group_194",
l Select Subsonic and Cylindrical,
l Select Mass flow imposed/Velocity Direction,
l Set Vr/V and Vt/V to <0> <Enter>,
l Set Vz/V to <1> <Enter>,
l Set Mass-Flow to <0.045> <Enter>,
l Set k to <13.5> <Enter>,
l Set Epsilon to <8150> <Enter>,
l Set Mixture fraction to <0> <Enter>,
l Set NO mass fraction to <0> <Enter>.
l Keep ProgressVariable1 set to <0.0> <Enter>.
Since the secondary air stream has the same temperature (and composition) as the primary one, the
present configuration still represents a two-stream problem.
35. Impose fuel stream conditions:
l Select the "ggt0_group_202",
l Select Subsonic and Cylindrical,
l Select Mass flow imposed/Velocity Direction,
l Set Vz/V to <1> <Enter>,
l Set Vr/V and Vt/V to <0> <Enter>,
l Set Mass--Flow to <0.0014> <Enter>,
l Set k to <132> <Enter>,
l Set Epsilon to <620000> <Enter>,
l Set Mixture fraction to <1> <Enter>,
l Set NO mass fraction to <0> <Enter>.
l Keep ProgressVariable1 set to <0.0> <Enter>.
36. Go to the OUTLET tab.
37. Select the outlet patch.
38. Select Subsonic and Cartesian.
39. Select Pressure Imposed/Static Pressure Imposed.
40. Set Static Pressure to <200000> <Enter>.
Since the combustion transport variables represent convected quantities, no extra condition needs to
be specified for these variables at an outlet.
41. Go to the SOLID tab.
42. Create a group "solid" of all solid patches:
l Left-click on first patch,
l Left-click + <Shift> on last patch,
l Click on Group,
l Enter group name as <Solid> <Enter>.
43. Impose solid conditions:
l Click on group "Solid",
l Keep Adiabatic to set all solid walls as adiabatic.
44. Press on OK to accept and close the dialog box.
3.3.7
Initial Solution
45. Double left-click on the Initial Solution menu.
46. Double left-click on the Initial Solution page to access dialog box.
47. Activate Constant values.
48. Select Cartesian.
49. Set Pressure = <200000> <Enter>.
50. Set Vx and Vy to <0.0> <Enter>.
51. Set Vz to <1.0> <Enter>.
52. Set k to <13.5> <Enter>.
53. Set epsilon to <8150.0> <Enter>.
54. Set Mixture fraction to <0.0> <Enter>.
55. Initialize Progress Variable 1 to <10.0> <Enter> [mol/kg].
56. Keep activate Initialization with fully burned state.
57. Deactivate On finest grid.
58. Set Number of iterations to <700> <Enter>.
59. Left-click on OK to accept and close the dialog box.
To achieve a burning solution, care must be taken with regards to the initialization of the flow field.
Only if initialized properly, the source terms of the progress variable will be triggered so that the
progress variable field will yield a non-trivial, burning solution.
To ignite the combustion process, the progress variable field should be initialized with a burned stated
by setting the progress variable to a value that is equal or higher than the value reached in chemical
equilibrium. (A value of 10 mol/kg should for most cases be sufficient to activate the progress
variable field.).
In any case, since the progress variable is not realistic in the beginning of a simulation, it makes a
certain number of global iterations (here 700) sense to determine the thermochemical properties for a
fully burned state instead of looking them up for the local value of the progress variable.
By activating the box on On finest grid, the thermochemical properties are determine by looking up
the combustion table for a completely burned state until a specific number of iterations have been
reached in the finest grid.
3.3.8 Numerical Parameters
60. Double left-click on the Numerical Parameters menu.
61. Double left-click on the General Parameters page.
62. Keep Number of grid(s) to <4> <Enter>.
63. Keep Correction damping and Coarse grid initialization active.
64. Go to the Advanced tab.
65. Set Maximum number of cycles per grid level to <600> <Enter>.
66. Set Convergence criteria on each grid level to <-6.0> <Enter>.
67. Left-click on OK to accept and close the dialog box.
68. Double left-click on the Numerical Schemes page.
69. Keep 2nd order central scheme for the RANS equations (the combustion transport equations
and the turbulent flow equations are solved using an upwind discretization).
70. Keep CFL number set to <1.5> <Enter>.
When simulating combustion, the CFL number is by default set to 1.5 instead of 3.
Time derivative preconditiong is always activated when combustion modelling is used.
71. Set Characteristic velocity to < 20.0 > < Enter >. This velocity is representative in its
magnitude for the velocities in the combustor.
72. Keep default parameters for preconditioning and local velocity scaling active.
73. Left-click on OK to accept and close the dialog box.
3.3.9
Computation Control
74. Double left-click on the Computation Control menu.
75. Double left-click on the Outputs page.
76. Under General thumbnail, select Combustion in Categories.
"LookUpTable_ H2O",
77. Select
CO2",
ProgressVariable1" and "LookUpTable_ CO"
concentration) and "Comb_SourceTermNO" are selected by default):
the quantities "LookUpTable_ RHO", "LookUpTable_ TEMP", "LookUpTable_
"Comb_
(NO
"LookUpTable_ CH4",
"LookUpTable_ OH",
("Comb_ NOxPOst"
to post-process
l Left-click on quantity or species in the list,
l Click on Add -->.
78. Left-click on OK to accept and close the dialog box.
79. Double left-click on the Control Variables page.
80. Set Number of iterations to <5000> <Enter>.
An increase (from default values) in the number of iterations conducted on the finest grid level is
often needed running combustion projects. This is mainly related to coexistence of different physical
scales, which makes the convergence slower.
81. Set Convergence criteria to <-6> <Enter>.
The flow filed is very dependent on the mixture fraction field. Thus, for an accurate result, it is
important to ensure that the mixture fraction field is properly converged.
82. Set Save solution every to <100> <Enter>.
83. Double left-click on the Launching Mode page.
84. Select Paralleland set the total number of processes to <6>.
85. Left-click on OK to accept and close the dialog box.
3.3.10 Save Project & Computation
86. In Project/Preferences menu, select Full-double-precision mode to run the flow solver in
double precision mode.
87. In Project menu, select Save to save the project (".iec").
88. In Project menu, select Save Selected 'Run' Files to save the ".run" file of the selected
computation.
FINE™/Open will automatically create a computation folder inside the project folder. It is strongly
advised to stick with this file structure.
3.3.11 Monitoring Convergence
89. Click on icon to start the calculation in parallel.
90. Left-click on OK to accept and start the computation in parallel.
FINE™/Open includes the ability to manage computation through a task manager (
batch mode. More details can be found in FINE™/Open User Manual.
) and /or in
91. Click on the icon
to track the evolution of residuals with the iterations.
The evolution of averaged residuals on the entire domain can be observed during the convergence
process (Steering icon). Similarly, the evolution of the mass flow balance (in/out) and/or global
quantities (efficiency, pressure ratio, torque and axial thrust on solid walls selected in the
boundary conditions page) can be performed in the steering. Local and global quantities may also
be added for follow up during the convergence process. However, their representation in the
graphical area will be effective only once they will be added, and past history will not be
available.
To check the convergence of the computation, NUMECA recommends observing the evolution
of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out, with satisfactory correspondence (usually less than 0.5%
difference between in/out). To do so, select the inlet and outlet mass flow at once. An
information about the difference is automatically computed.
A more detailed description of the convergence history per equation and per domain is available
in the Monitor
.
474
FINE™/Open with OpenLabs™ 7.2 Tutorials
Once the calculation is converged or reaches the maximum number of iterations allowed on the
finest grid level, the flow solver stops. The final solution is then stored for post--processing and the
task manager window is closed.
3.3.12 Post-Processing
92. Click on the icon
to access CFView™ from the FINE™/Open GUI.
93. Click on Cut in the Surfaces area to create a cutting plane or click on Geometry/Create
Cutting plane... menu.
94. Select Geometry.
95. Set the Point coordinates to X = <0> <Enter> and Y = <0> <Enter>.
96. Click on X button to define a plane at X constant.
97. Click on Apply and Save.
98. Click on Y button to define a plane at Y constant.
99. Click on Apply and Save.
100. Close the dialog box.
101. Visualize solid surfaces with rendering:
l In the Surfaces area, left-click on "Solid" group in the Surfaces area.
l Right-click and Select to only activate "Solid" group (all solid surfaces).
l Click on
in Representations/Grid in Quick Access Pad.
l Set Opacity to 0.3 in Representations area.
102. Left-click + <Ctrl> on "CUT1" and "CUT2" in the Surfaces area.
103. Right-click and Select to only activate cutting planes.
104. In Quantities area, double left-click on "LookUpTable_TEMP". This is done to visualize
the static temperature, which is determined in the simulation via a look-up in the combustion
tables.
105. Left-click on Contours & Iso Values in Representations area.
106. Click on the icon
cutting planes.
Smooth Contour to plot color contour of the temperature on the
107. Click on the icon Isolines
to plot isolines of the temperature on the cutting planes:
l Set number of isolines to <15> <Enter>,
l Set Color to Uniform,
l Click on Apply,
l Close the dialog box.
108. Repeat the steps 104-107 to post-process other quantities.
479
FINE™/Open with OpenLabs™ 7.2 Tutorials
3.4
FLOW SETTINGS AND POST-PROCESSING:
HYBRID BML/FLAMELET MODEL
In this part of the tutorial, the computation using the hybrid BML/Flamelet model is created by
duplicating the existing computation using the FGM model. All the settings in the FGM
computation are kept. the following part shows only the different settings between the two
models.
3.4.1
Computation Management & Global Properties
109. Create a new computation as a duplicate of computation "FGM":
l Left-click on "FGM" in Computations area,
l Click on New,
l Right-click on "new_FGM", and select Rename,
l Rename it to <Hybrid_BML_flamelet> <Enter>.
3.4.2
Combustion Model
110. Double left-click on the Optional Models menu to access sub-pages (if necessary).
111. Double left-click on Combustion page to access dialog box.
112. Select the Hybrid BML/Flamelet as Chemistry model.
113. In the combustion table variables, a table should be linked to the computation (select under
Combustion look- up table a Hybrid BML/Flamelet look- up table "GGT_PartiallyPremixed_
Hybrid_BML_pre.tab" from the tutorial package under ./_tables/_PartialyPremixed_HybridBML)
Alternatively, a new table can be generated with TABGen/Chemistry Editor:
l Click on Create/Edit...
l Click on File/New/Fom template...
l Select the bb_hybrid and click on Ok, the selected template is loaded in the TABGen/Chemistry
Editor,
l Set Pressure value to <2e05> [Pa],
l For the fuel stream:
l Set <Species>CH4 to <1>,
l Remove <Species>H2=0.5</Species>,
l Set Temperature value to <368> [K],
l For the oxidizer stream, set Temperature value to <623> [K],
l Click on File/Rename to rename the table as <GGT_PartiallyPremixed_Hybrid_BML>,
l Click on Build/Generate table to launch TABGen/Chemistry tool.
The steering file generates a preintegrated hybrid BML/flamelet table for a pressure of 200,000 Pa,
preheated air at 623 K and preheated methane at 368 K for methane-air combustion. The chemical
mechanism GRI-3.0 is used, which is read from the file "gri30.chm".
At the end, the table is successfully generated and automatically linked to the computation.
l Click on File/Close,
l Click on Preview... to visualize the table.
114. Keep the default Zimont model for the BML model.
115. Select User-defined in the Flamelet definition.
116. Set the Laminar flame speed correlation as Constant type.
117. In Constant laminar speed set SL = <1.1> <Enter>.
118. Under the Flammability limits, specify the Min equivalence ratio = <0.4> <Enter> and
Max equivalence ratio = <1.6> <Enter>.
119. Press on Ok to accept and close the dialog box.
Laminar flame speed at equivalence ratio close to 1 is used and assumed to be constant across the
flammability limits. Flammability limits are obtained for methane from literature at given pressure
and temperature.
3.4.3
Initial Solution
120. Double left-click on the Initial Solution menu to access sub-pages (if necessary).
121. Double left-click on the Initial Solution page to access dialog box.
122. Initialize Progress Variable 1 to <1.0> <Enter>.
123. Keep all other settings.
124. Press on Ok to accept and close the dialog box.
3.4.4
Computation Control
125. Double left-click on the Computation Control menu to access sub-pages (if necessary).
126. Double left-click on the Control Variables page.
127. Under the tab General, set Number of iterations to <5000> <Enter>.
128. Go to the Advanced tab. Pick Local parameters (by domain) in Select category.
129. Set iPartPremVariableRefCond_ expert parameter to <1> <Enter>.
130. Left-click on Ok to accept and close the dialog box.
3.4.5
Save Project & Computation, Monitoring Convergence
131. launch the computation and monitor the convergence.
486
FINE™/Open with OpenLabs™ 7.2 Tutorials
3.4.6
Post-Processing
132. Repeat the steps 92-107 to post-process the quantities.
488
FINE™/Open with OpenLabs™ 7.2 Tutorials
Progress variable is defined as non-dimensional temperature in Hybrid BML/flamelet model, hence
you see range from 0 to 1 for progress variable.
TUTORIAL 4.
USING PREMIXED COMBUSTION MODEL
This tutorial describes how to use the multiphysics modeling capabilities in FINE™/Open to simulate
the premixed combustion in a 2D Axi-symmetric geometry:
l Generate a 2D axi-symmetric mesh using HEXPRESS™,
l Set up a premixed combustion computation in FINE™/Open interface,
l Start/stop the computation,
l Visualize the results with CFView™.
4.1
INTRODUCTION
4.1.1
Prerequisites
This tutorial does not require any particular prerequisite but it is strongly recommended for
beginners to complete the Beginner level tutorials.
4.1.2
Problem Description
The TECFLAM combustion chamber is fired with natural gas and can be operated under
diffusion as well as under premixed conditions. The TECFLAM configuration has been
extensively studied experimentally and numerically at TU Darmstadt. The analysis of this swirl
flame is of great interest as it mimics the main features that are observed in industrial burners.
4.1.3
Preparation
l Download the tutorial archive as available from the Products page of the Customer Area
(www.numeca.be). Then extract the tutorial input files 'Tutorial_4'.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
l Click on the icon Creating a mesh under Create a new project to create a new project and a
new mesh. Click on Ok.
l Select your directory of choice to store the project.
l Enter the project name in the dialog box as <Tecflam.iec> and click on Save or Ok.
FINE™/Open will automatically create a project folder called "Tecflam" which will contain the
project file (" .iec") and a folder " _mesh" where the mesh will be stored. Later, computation
folders will appear inside the project folder. It is strongly advised to keep this file structure all
along the project.
You are now ready to start the "Mesh Generation" (p. 494) process with HEXPRESS™!
MESH GENERATION
HEXPRESS™ graphical user interface allows to visualize the geometry and the mesh of an
internal or an external test case in a graphics area. The access to the main menu and controls is
enabled through a menu bar and a quick access pad, and is completed with a tool/icon bar and
a control area (including the keyboard input area).
4.2
LOAD EXISTING DOMAIN
The Welcome to HEXPRESS™ dialog box enables the user to open an ".igg" project file
including the mesh and the data required to regenerate a mesh. In this tutorial, these data will be
progressively defined. That is why the tutorial starts from the domain file ".dom". It should be
noticed that the dialog box also enables the loading of geometry (Parasolid™ , CATIA v5, STL),
import HEXPRESS™/Hybrid, ANSYS or CGNS meshes, as well as python script.
1. Select Import computational domain <.dom> in the Welcome to HEXPRESS™ dialog
box.
2. In the dialog box, locate and select "tecflam.dom" provided in the tutorial archive. This file can
be found in your local copy of the tutorial archive as downloaded from the Products page of the
Customer Area (www.numeca.be).
3. In the Grid generation mode click on icon (
on Yes to confirm the 2D mode.
) to mesh a 2D axis symmetric domain. Click
Periodic boundary conditions are automatically recognized according to the new 2D boundary
conditions recognition. Mirror conditions (MIR) are applied in the periodic directions.
Later on in this tutorial the 2D domain is going to be used to create an axisymmetric mesh. When
creating 2D geometry that is later going to be used for an axisymmetric mesh it is recommended to
cut off the geometry at a small radius (i.e. the geometry should stop at some small distance away
from the axis that is to become the symmetry axis) to avoid singular cells
4.3
VISUALIZATION
Use the viewing buttons at the bottom of the interface to display the geometry as preferred. In
View subpanel from the Quick Access Pad, it is possible to:
l Left-click on Mesh icon (
) to hide/show mesh (toggle),
l Left-click on Solid icon (
) to hide/show faces (toggle),
l Right-click on Face icon (
) or left-click on icon
to open Face Viewer window.
The face selection can be done interactively in the graphics area or thanks to the Face Viewer
window.
4.4
SET BOUNDARY CONDITIONS
4. Go to Grid/Boundary conditions... menu or click on icon
boundary conditions using the Set face type button:
in the Icon Bar and set the
l set "outlet" as outlet ("OUT"),
l set "mixture_inlet" , "bluff_body2" and "air_inlet" as inlet ("INL").
5. Close the dialog box.
The bluff body between the coflow and the inflow is modeled as a coflow and not as a solid wall This
is to prevent a false prediction of a flame attachment to the bluff body.
4.5 MESH WIZARD : INITIAL MESH
6. Left-click on check box for Initial mesh in Mesh Wizard to activate the step. An activation
sign will appear inside the box dedicated to the state of the corresponding step.
7. Left-click on Initial mesh.
8. In Set the number of divisions along Cartesian axis section, impose X axis to < 20 >
<Enter>, Y axis to <50> <Enter>.
9. Click on Ok and on Step button from the Mesh Wizard to create the initial mesh.
The number of cells along X/Y axis in the initial mesh can be increased in order to impose a smaller
size to the biggest cell that will be included in the computational domain
4.6 MESH WIZARD : ADAPTATION STEP
This mesh generation step is probably the most
interaction in
HEXPRESS™. Indeed, the parameters selection in this action directly dictates the computed mesh
obtained with HEXPRESS™. This adaptation step consists of two successive actions: the refinement
and the trimming.
in terms of user
important
During the first one, HEXPRESS™ adapts the initial mesh such that the cell sizes satisfy geometry
dependent criteria. With the second step, it removes cells intersecting the geometry or located outside
the computational domain.
10. Left-click on check box for Adapt to geometry in Mesh Wizard to activate the step.
11. Left-click on Adapt to geometry.
12. Under the Global tab, set the Maximum number of refinements to <5> <Enter>.
In this action, cells are successively subdivided such that specific geometrical criteria are satisfied.
In order to limit the number of cells created during refinement, HEXPRESS™ subdivides cells
anisotropically as often as possible. A cell can thus be subdivided in 2, 4 or 8 cells.
The adaptation process successively bisects the cells flagged for refinement in one or several different
directions. The sizes of the initial mesh cells are therefore divided by a factor 2N after N successive
refinements. This may result in an exponential growth of the total number of cells in the mesh, even
though the refinement may be confined to some areas of the computational domain. To bound the
number of cells, the user should set the maximum number of refinements to a reasonable limit.
Several global expert parameters are available when clicking on Advanced >>> button to finely tune
the mesh adaptation process. Since HEXPRESS™ is optimized for these defaults, any modification
may therefore alter the success of the meshing process. More details are available in the User Manual.
13. Left-click on Surface refinement tab.
The adaptation process is defined by three classes of criteria: curve, surface and volume criteria.
Surface criterion is considering cells which are intersecting surfaces as candidates for refinement.
Three criteria are implemented and are respectively based on:
l a proximity between surfaces (Distance),
l a surface curvature measurement (Curvature),
l a specification of cell target sizes on the surfaces (Target cell sizes).
Volume criterion (found in Box refinement tab) is considering cells which are intersecting or
located inside a three-dimensional volume as candidates for refinement if their cell size is larger than
some user prescribed target size.
14. Select "side_ a". The selected face is highlighted in the graphics area. Furthermore, left-
clicking in the graphics area on a face allows to select it as well.
15. Click on Active.
16. Set the Maximum number of refinements to <2> <Enter>.
17. Set Target cell sizes criterion to <0.001> for X axis and <0.015> for Y axis.
The Maximum number of refinements per surface ultimately controls the refinement of cells
intersecting that surface (if it is presenting a value lower than the Global maximum number of
refinements from the Global parameters tab). This parameter supersedes any other selected
adaptation criteria. Fine tuning of this parameter is useful when it may be difficult to determine the
appropriate Target cell size, or if the Distance and Curvature criteria yield a prohibitive number
of cells. The default value (10000) is an arbitrary large number such that the criteria are controlled by
the Global maximum number of refinements.
The aim of the Distance criterion is to allow enough refinements of the cells in order to fill any gaps
between very close surfaces with a sufficient amount of cells.
The aim of the Curvature criterion is to automatically compute a target cell size suitable for
resolving curved surfaces. Smaller cells are expected where the geometry has high curvature.
The aim of the Target cell sizes criterion is to enforce a user- defined target cell sizes for each
geometrical surface. The size of a cell
intersecting a geometrical surface are compared to the
prescribed user target and the cell is refined until its actual size is lower than the target.
18. Repeat the steps above for "side_b".
19. Left-click on Box refinement tab.
Volume criterion (found in Box refinement tab) considers cells intersecting or located inside a
three- dimensional volume as candidates for refinement if their cell size is larger than some user
prescribed target size.
20. Create a box for volume refinement:
l Click on New box button,
l Press <c> to define box by two opposite corners instead of center and corner,
l In the input bar, type <0.1 0 -0.01> <Enter> to place the first box corner,
l In the input bar, type <0.2 0.14 -0.01> <Enter> to place the second box corner,
l Left-click to accept "Box #0".
21. Repeat above steps to create three more boxes.
l "Box #1" with corners set respectively to <0 0.14 -0.01> and <0.2 0.24 -0.01>,
l "Box #2" with corners set respectively to <0 -0.07 -0.01> and <0.1 0.14 -0.01>,
l "Box #3" with corners set respectively to <0.013 -0.07 -0.01> and <0.032 0 -0.01>.
Box #0, #1 and #2 are right next to each other. Setting Refinement diffusion to 0 
will ensure that
the neighboring box will not be modified. Concerning the Box #3, a higher
Refinement diffusion can be used so that smaller cells are generated at the jet exit.
22. Impose settings for "Box #0"
l Make sure the box is Active,
l Set the Maximum nb of refinements to <3> <Enter>,
l Set Target cell sizes criterion to <0.004> <Enter> for the X axis and <0.004> <Enter> for the
Y axis,
l Select Volumic option,
l Set the advanced option Refinement diffusion to <0> <Enter>.
23. Impose settings for "Box #1":
l Make sure the box is Active,
l Set the Maximum nb of refinements to <3> <Enter>,
l Set Target cell sizes criterion to <0.004> <Enter> for the X axis and <0.004> <Enter> for the
Y axis,
l Select Volumic option,
l Set Refinement diffusion to <0> <Enter>.
24. Impose settings for "Box #2":
l Make sure the box is Active,
l Set the Maximum nb of refinements to <3> <Enter>,
l Set Target cell sizes criterion to <0.0005> <Enter> for the X axis and <0.013> <Enter> for
the Y axis,
l Select Volumic option,
l Set Refinement diffusion to <0> <Enter>.
25. Impose settings for "Box #3":
l Make sure the box is Active,
l Set the Maximum nb of refinements to <4> <Enter>,
l Set Target cell sizes criterion to <0.0> <Enter> for the X axis and <0.0> <Enter> for the Y
axis,
l Select Volumic option,
l Set Refinement diffusion to <5> <Enter>.
26. Go to the Trimming tab.
27. Note that the patches with boundary type "Mirror" ("side_a" and "side_b") are automatically
flagged to not be used for trimming. Leave these patches flagged to Not used for trimming.
In the present case, it is advised to not use some of the boundary for trimming as the projection
operation can deteriorate the quality of the mesh in 2D.
28. Set patch trimming status to Not Used for trimming for the patches "bottom", "outlet",
"top".
29. Click on Ok.
30. Click on Step in Mesh Wizard to launch the adaptation step.
4.7 MESH WIZARD : SNAPPING STEP
31. Left-click on check box for Snap to geometry in Mesh Wizard. An activation sign will
appear inside the box dedicated to the step.
32. Left-click on Snap to geometry.
33. The Advanced>>> button allows to activate 3 extra tabs (Global parameters , Curve
snapping and Buffer insertion) and advanced flags for the snapping step. It is not necessary to
change the default in this tutorial.
34. Keep default parameters for advanced options.
35. Left-click on Ok.
The aim of this fully automated mesh step is to project the staircase mesh obtained after the mesh
adaptation on the surface to obtain a good quality body conforming mesh. In addition to a simple
projection on the geometry,
lower
dimensional geometric features such as corners and curves in the mesh. These algorithms guarantee
that, when the mesh is projected onto the surface geometry, a mesh vertex is attached to each corner
of the geometry and that a path of mesh edges is attached to the curve.
this action involves sophisticated algorithms to recover
Layers of additional cells (buffer insertion) are introduced into the mesh to create a body conforming
mesh. Finally, a mesh smoothing is performed which moves points on the surface and in the volume.
4.8 MESH WIZARD : OPTIMIZATION STEP
The mesh obtained after the snapping step may involve poor quality cells usually located close to
corners and curves. Some of these cells are concave or may even present a negative volume.
HEXPRESS™ provides specific algorithms to convert concave cells to convex ones by slightly
displacing their vertices.
36. Left-click on check box for Optimize in Mesh Wizard to activate the step.
37. Left-click on Optimize.
38. Keep default settings.
39. Left-click on Ok.
40. Click on Start in Mesh Wizard to snap and optimize the mesh.
41. For this tutorial no viscous layers are required so this step will not be performed.
In combustion case, the zone of interest are located in the domain off the walls.
4.9 MAKING MESH AXI-SYMMETRIC
42. To make the mesh axisymmetric go to Grid/Mesh transformation... and select
Axisymmetric tab.
the
43. Apply the following settings to set the axisymmetric axis, which is coincident with the y-axis:
l Enter <0 0> as the Origin of the axisymmetric axis,
l Enter <0 1> as the 2D axis (indicating the y-direction),
l Set Angle [degree] to <5.0>,
l Set Nb of layers in theta <1>,
l Click Apply to transform the mesh.
Note that after the transformation the axisymmetric axis is aligned with the z-axis.
By default angle is 1 degree but it is too small and close to the axis, cells are too elongated which has
a negative impact on convergence. 5 degrees was found to be a reasonable value.
44. The final axisymmetric mesh is shown below.
513
FINE™/Open with OpenLabs™ 7.2 Tutorials
4.10 PERIODIC FNMB CONNECTION
We need FNMB connection since we are dealing with the swirling flow.
45. Go to the Grid/Boundary Conditions... menu or click on icon
the boundary conditions using the Set face type button:
in the Icon Bar and set
l Set "bottom" and "top" as Mirror ("MIR").
Note that the patches "side_a" and "side_b" are automatically recognized as 'SOL*' by making
the mesh axisymmetric.
46. Close the dialog box.
47. Go to Grid/Periodicity... . Verify that a periodicity definition of type 'ROTATION'
('Periodicity_1') was automatically created by making the model axisymmetric.
48. Select 'Periodicity 1' and click on Edit.
49. Compare the settings with the settings shown below.
Periodicity should correspond to the number of times the axis-symmetric should be repeated to get a
360 degrees (360/5=72).
50. Click Cancel and Closeto continue.
51. Go to Grid/Non Matching Connections... menu.
52. A non-matching connection was automatically created when making the mesh axisymmetric:
"connection_2". Check the settings of the connection by selecting "connection_2" and clicking
on the Edit button.
53. Select the "connection_2" and left-click on Compute.
54. Click on Close when the computation is over (status is marked as "Successful").
4.11 CHECK MESH QUALITY IN HEXPRESS™
55. Left-click the Mesh Quality
button in Icon Bar to check the mesh quality.
The check of mesh quality allows you to detect the presence of negative cells, i.e. cells with a negative
volume. Negative cells are not allowed in the final mesh to be used for the computation. Concave or
twisted cells are less likely to present robustness or stability issues for solvers, however they should be
prohibited.
When negative, concave or twisted cells are detected, they could be usually removed by changing
mesh adaptation settings or advanced settings of snapping/optimization.
56. Check the mesh quality using the Criterion drop-down menu for the following criteria:
l Negative cells,
l Concave cells,
l Twisted cells.
4.12 SAVE MESH
57. Go to Project/Save as... or click on the Save icon
in Icon Bar.
58. Under the "./Tecflam/_ mesh/" folder, enter the name of the mesh project as < tecflame_
axis.igg>.
59. Click Ok to save mesh files.
The mesh folder contain the mesh topology, geometry, grid points and the boundary condition
types among other. The files list is written below:
l .bcs: boundary conditions files,
l .dom: geometry files,
l .igg: topology file,
l .hex: grid points files,
l .rep: report file,
l .dist: distance file (prefix is domain name),
l .fnmb: FNMB connections,
l .qualityReport: quality report file.
In addition a subdirectory named "cache" contains resulting mesh files after each step of the mesh
generation (for example "_snap.hex" as resulting mesh after snapping process). It allows to delete
some steps and come back to a previous one without generating the necessary steps again.
60. Click on Close in Icon Bar to quit HEXPRESS™ and return to FINE™/Open. You can
save the project (if not done already) and accept (yes) to link the new mesh to the project.
61. The Mesh properties dialog box appears.
62. Check that the information are correct (set Grid units to Meters).
63. Click on Ok.
You are now ready to start the flow settings and the post-processing!
Start the "BML-Premixed Combustion" (p. 519) case.
BML-PREMIXED COMBUSTION
A step by step approach is proposed in the following lines. It aims at driving you through the
various steps that need to be executed to set up, start the computation and post-process the results.
4.13 FLOW SETTINGS
4.13.1 Manage Computations
64. You can rename the computation in the Computations menu on the left:
l Right-click on "computation_1" and select Rename,
l Enter new name as <Tecflame_Premixed> as we are going to simulate using BML premixed
combustion model,
l Press <Enter> key to save the new name.
In the Computations menu, the list of computations are shown. It is possible to Rename, creates a
new one by duplicating the highlighted one (New button) or just delete the computation by clicking
on Delete.
4.13.2 Set Physical Configuration
65. In the Physical Configuration menu, double left-click on General Properties to open the
dialog box:
l Keep Steady and Fluid Block for the domain "tecflam",
l Select Combustion in Optional properties to activate the use of the combustion modeling
module.
l Press on Ok to accept and close the dialog box.
l Acknowledge the warning message and click Yes to continue.
66. In the Physical Configuration menu, double left-click on Fluid Model to open the dialog
box:
l keep all the settings,
l Press on Ok to accept and close the dialog box.
The reference pressure is set to the outlet pressure to avoid round-off errors at low Mach numbers
(the reference temperature is only of importance for inert flows). The thermal conductivity and the
diffusivity coefficients are calculated via the viscosity coefficient using the Prandtl and Schmidt
numbers. The turbulent Prandtl and Schmidt numbers can be changed via the expert parameter phys_
PrandtTurb_ and combSchmidtTurb_ in Computation Control/Control Variables page.
67. In the Physical Configuration menu, double left-click on Flow Model to open the dialog
box:
l Keep Turbulent Navier-Stokes as Flow model,
l Keep k-epsilon (Standard) as Turbulence model,
l Enter <0.2> as Reference length,
l Enter <6.0> as Reference velocity,
l Press on Ok to accept and close the dialog box.
4.13.3 Combustion Model
68. Double left-click on the Optional Models menu and double left-click on Combustion page
to access dialog box.
l Select Premixed as Combustion type to model the combustion process as being of premixed
type,
l Set Chemistry model as TFC model (Zimont),
l Enter <0.2> [m/s] as Laminar flame speed,
l Enter <2000> [K] as Adiabatic flame temperature,
l Enter <1.18> [kg/m³] as Unburnt density,
l Enter <300> [K] as Unburnt temperature,
l Keep <1.568e-05> [m²/s] as Unburnt kinematic viscosity.
l Press on Ok to accept and close the dialog box.
4.13.4 Boundary Conditions
69. In the Boundary Conditions menu, double left-click on Boundary Conditions to open the
dialog box.
70. Go to INLET tab, select "mixture_inlet" patch. Keep Subsonic and change to Cylindrical
coordinate system.
71. Select Mass flow imposed and Meridional Flow Angle and Tangential Velocity:
l Set Vr/Vm to <0> <Enter>,
l Set Vt to <5.6> <Enter> [m/s],
l Set Vz/Vm to <1> <Enter>,
l Set Mass-Flow to <0.012> <Enter> [kg/s],
l Set k <0.135> <Enter> [m²/s²],
l Set Epsilon to <7.5> <Enter> [m²/s³],
l Keep NormalizedProgressVariable as <0> <Enter>.
72. In INLET tab, select both "bluff_body2" and "air_inlet" patches. Keep Subsonic and change
to Cylindrical coordinate system.
Imposed and Velocity Components
(Static Pressure
73. Select Static Quantities
extrapolated):
l Set Vr to <0> <Enter> [m/s],
l Set Vt to <0> <Enter> [m/s],
l Set Vz to <0.5> <Enter> [m/s],
l Set k <0.001> <Enter> [m²/s²],
l Set Epsilon to <0.06> <Enter> [m²/s³],
l Keep NormalizedProgressVariable as <0> <Enter>.
Note that the bluff body between the coflow and the inflow is modeled as a coflow and not as a solid
wall. This is to prevent a false prediction of a flame attachment to the bluff-body.
74. Go to OUTLET tab, select "outlet" patch.
l Keep Pressure Imposed and Static Pressure Imposed,
l Keep Static Pressure value as <101325.0> <Enter> [Pa].
l Press on Ok to accept and close the dialog box.
4.13.5 Initial Solution
75. In the Initial Solution menu, double left-click on Initial Solution.
76. Select the domain "tecflam", keep General Setting as Constant values.
77. Set the following values in Parameters:
l Set the Coordinate system to Cylindrical,
l Set Pressure to <101325.0> <Enter> [Pa],
l Set Velocity type to Absolute,
l Set Vr to <0> <Enter> [m/s],
l Set Vthetato <0> <Enter> [m/s],
l Set Vz to <6> <Enter> [m/s],
l Set k <1> <Enter> [m²/s²],
l Set epsilon to <100> <Enter> [m²/s³],
l Keep NormalizedProgressVariable as <1> <Enter>.
78. Click on Ok to accept and close and the window.
4.13.6 Numerical Parameters
79. In the Numerical Parameters menu, double left-click on General Parameters.
80. Set the Number of grid(s) is set to <3> <Enter>.
The flow solver is based on an explicit time integration technique, which is accelerated by means of
dedicated multi- grid methods. To this end, several levels of intermediate grids must be generated
starting from the finest one. It is strongly advised to enable the definition of at least 3 grid levels.
81. Keep Correction damping and Coarse grid initialization active.
In addition to the multi-grid acceleration technique, the number of iterations to convergence can be
significantly reduced by activating the coarse grid initialization process. In that case, the simulation
starts on the coarsest grid level available. Once converged, the flow solver automatically interpolates
the current flow solution on the next finer level. This process repeated until the finest grid level is
reached. The iterative process stops when the convergence criteria are reached or the maximum
number of iterations is exceeded.
82. Left-click on Advanced tab.
l In Multigrid parameters the change number of sweeps on successive grid levels to <1> <
4> <8> for first three values,
l In Coarse grid initialization parameters set Maximum number of cycles per grid level to
<1000> <Enter> and Convergence criterion on each grid level set to <-5> <Enter>.
83. Click left on Ok to accept the changes.
84. In the Numerical Parameters menu, double left-click on Numerical Schemes.
85. Keep CFL number <1.5> <Enter>, change the Characteristic velocity to <6> <Enter> and
left-click on Ok to accept the changes.
For combustion, the default CFL number is lowered to 1.5. The characteristic velocity is set to 6 m/s,
which is approximately the maximum velocity of the swirling flow.
4.13.7 Computation Control
86. In the Computation Control menu, double left-click on Outputs menu.
87. Under Quantities selection, select Combustion in Categories. Select the quantities "Comb_
NormalizedProgressVariable" and "Comb_Temperature":
l Left-click on quantity,
l Click on Add --> to add,
l Left-click on Ok to accept and close the dialog box.
88. In the Computation Control menu, double left-click on Control Variables menu:
l Set the Number of iterations to <3000> <Enter>,
l Set the Convergence criteria to <-6> <Enter>,
l Save the solution at every <200> iterations <Enter>.
89. In Advanced tab, select category Local parameters (by domain):
l To improve convergence rates for case with periodic FNMBs, set iNew_FnmbPER_ROT_
to <1> <Enter>,
l Click on Ok to accept and close the window.
4.13.8 Save Project & Computation
90. Click on Save Project button to save the project.
91. Click on Save Selected 'Run' files button to save the computation.
4.13.9 Start & Stop Computation
92. Click on Start Flow Solver button to launch the computation and click on Ok to run in serial
mode.
93. To save and stop a computation while running, the button Save Solution And Stop Flow
Solver should be pressed. However, to stop the computation without saving, the Kill Flow
Solver button should be used.
94. The pop up Task manager window allows following the convergence history of the
computation.
4.13.10 Monitoring
The evolution of averaged residuals on the entire domain can be monitored during the
convergence process. Similarly, the evolution of the mass flow balance (in/out) and/or global
quantities. Local and global quantities may also be added for follow up during the convergence
process. However, their representation in the graphical area will be effective only once they have
been added, and past history will not be available.
95. To check the convergence of the computation, NUMECA recommends observing the
evolution of multiple criteria which includes:
l an adequate decrease in residuals (minimum 3 orders of magnitude),
l complete stabilization of global performances,
l stabilization of mass flow in/out, with satisfactory correspondence (usually less than 0.5%
difference between in/out). To do so, select the inlet and outlet mass flow at once. An
information about the difference is automatically computed.
96. The examination of residuals per block for a given primitive variable or the comparison of
convergence histories from different computations, can be achieved by accessing the Monitor
tool. The tool is included in the package and can be accessed via Icon Bar.
The iterative process is now over. As part of the FINE™ environment, NUMECA proposes the
visualization and post-treatment tool CFView™ for that purpose. CFView™ is entirely integrated
within the environment and includes numerous tools.
4.14 POST-PROCESSING
97. To access CFView™ from the FINE™ graphical user interface, press the CFView™ icon (
).
A step by step approach is proposed in the following lines. It aims at driving you through the
various steps that need to be executed from reading the solution to the extraction of the main
results. CFView™ automatically opens the run file associated with the active computation.
98. Go to Surfaces area panel.
99. Left-click + <Ctrl> key on all the surface to highlight them. Right-click to open the pop-up
menu and choose Select to activate all the surfaces selected.
100. Press <b> (or go to Geometry/Boundary) to hide the boundaries and press <b> again to
make all geometry selected visible.
101. Double left-click on the Y-axis button and on the Fit the View button (Viewing buttons).
102. Then go to Quantities area in the Quick Access Pad.
103. Double left-click on the "Comb_Temperature".
All quantities selected in FINE™ graphical user interface are transferred to CFView™. However,
additional derived output can be accessed directly from the visualization and post- treatment tool,
including vector components, gradients, divergence and curl of selected quantities. New quantities,
defined as an arithmetic combination of existing quantities possibly combined with regular operations
(trigonometric functions, logarithmic functions,...) can further be created with the Quantity/Field
Data/Define New Quantity... menu.
Once the candidate quantity for visualization is selected, a representation mode should be selected.
Representation is typically executed in the form of color contours (smoothed or stripped) and/or
isolines. CFView™ also includes the possibility to interrogate the flow field locally ("local value")
and create 1D Cartesian plots. Advanced capabilities involving curve and/or surface integration can
also be accessed.
104. In the Representations area, click on the Smooth Contour icon.
105. Left-click on X Projection.
106. Left-click on Y Projection.
107. Left-click on Fit the View.
108. Double left-click on the "Comb_NormalizedProgressVariable" to view normalized progress
variable contours.
109. Select File/Print... menu.
110. Click on Ok after defining the picture settings (more details in the User Manual).
111. Click on Ok after selecting the location to save and the name of the picture.
112. Select File/Quit CFView to leave CFView™ session.
TUTORIAL 5.
SIMULATE FLUID-PARTICLE INTERACTION
This tutorial describes how to use the Lagrangian particle tracking method in FINE™/Open with
OpenLabs™ to simulate inertial dispersed two-phase flows. The tutorial will start from a well set flow
computation and explain how to setup a Lagrangian computation in detail.
The tutorial will in special demonstrates how to:
l How to setup a Lagrangian computation,
l How to post-processing the Lagrangian computation results.
5.1
INTRODUCTION
5.1.1
Prerequisites
This tutorial assumes that you are familiar with the whole FINE™/Open with OpenLabs™ chain
and that you have completed all the Beginner tutorials, so that you can set up a FINE™/Open
project correctly. This tutorial will start from an existing FINE™/Open project. Some steps in the
setup of a FINE™/Open project and post-processing procedure will not be shown explicitly.
5.1.2
Problem Description
This tutorial is based on a spray test case provided by Sommerfeld. It is a hollow cone atomizer,
with a wide range of droplet diameters. The evaporation of the spray is neglected for this tutorial
and only the spray dynamics for three different sized classes are simulated.
In this case, the volume fraction of the dispersed phase is small (smaller than 0.0001). A one-way
coupling simulation will be considered. Only the influence of the carrier phase (gas in this case) to
the particles is taken into account. For cases with higher volume fractions, the influence of the
dispersed phase on the carrier phase cannot be neglected anymore and two-way coupling should
be used. See Fluid-Particle Interaction for more details.
5.1.3
Preparation
l Download the tutorial archive as available from the Products page of the Customer Area
(www.numeca.be). Then extract the tutorial input files 'Tutorial_5'.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
5.2
OPEN EXISTING PROJECT
1. After launching the FINE™/Open GUI, click on the icon Open an existing project and click
on the button Ok to confirm.
2. Locate and select the project file "Tutorial_5/Lagrangian.iec" in the dialog box and click on the
button Ok to confirm.
3. Select the computation GAS under Computations. Check all the settings in the FINE™/Open
GUI. In this tutorial, a pure flow computation has been created and provided. The main settings
are:
l Solver precision: Double
l Fluid model: Air (perfect gas)
l Flow model: Turbulence Navier-Stokes with k-epsilon (Extended wall function) model
l Inlet boundary condition: Subsonic - Cylindrical - Static Quantities Imposed - Velocity
Components
l Vr = profile
l Vt = 0 m/s
l Vz = profile
l Static Temperature = 373 K
l k = profile
l Epsilon = profile
l Outlet boundary condition: Subsonic - Cylindrical - Static Pressure Imposed
l Static Pressure = 101325 Pa
l Backflow Control is activated
l Solid wall boundary condition (DOMAIN1_group_4): Subsonic - Cylindrical - Temperature
Imposed
l Static Temperature = profile
l Coarse grid initialization is activated in the Numerical Parameters / General Parameters
page with 4 grid levels. The convergence criteria is set to 500/-5.
l CFL = 3
l Hakimi preconditioning is used with the characteristic velocity of 18 m/s.
4. Click on the button Start Flow Solver to launch the computation GAS.
5.3
SETUP LAGRANGIAN SIMULATION
The Lagrangian simulations are based on a standard fluid simulation and are executed after the
Eulerian simulation. It is therefore recommended to do a fluid simulation first and restart the
particle simulation based on this fluid simulation.
5.3.1
Create a restart computation
5. In the QAP Computations, select the computation GAS and create a new computation
Lagrangian_simulation.
6. Select the computation Lagrangian_simulation.
7. In the Initial Solution page, change the General Settings to From file, select the finished fluid
computation file Lagrangian_GAS.run.
8. In the Computation Control / Control Variables page, set the Number of iterations to 0.
The computation Lagrangian_simulation will restart from the finished fluid computation GAS and
perform 0 iteration. Then, the Lagrangian calculation will be started.
5.3.2
Set Lagrangian parameters
9. Double clicking on Fluid-Particle Interaction in the Optional Models. Select Fluid-particle
calculation to activate the Lagrangian model.
10. In the tab Parameters, keep 1-way coupling selected.
In the 1-way coupling approach the flow calculation (ignoring the influence of the particles on the
flow field) is followed by a calculation of the trajectories of particles. In this case, there is no
influence of the particles on the flow.
11. Keep Number of particles injected per cell as 30. This number defines the number of
computational particles per class and per cell.
12. Keep the particle force Drag selected, which by default uses the correlation of Schiller-
Naumann for the drag coefficient.
13. Select Dispersion, which will activate the turbulence modeling for the particles.
In FINE™/Open with OpenLabs™, the following particle forces can be activated:
l Pressure: the pressure force is a force on the particle that results from a pressure gradient in the
fluid around the particle.
l Drag: due to the velocity difference of the particle and the fluid. Two different correlations can
be used for the drag coefficient: the Stokes drag for low particle Reynolds number particles and
the drag correction from Schiller-Naumann for higher particle Reynolds numbers.
l Virtual mass: due to the acceleration of the surrounding fluid by the particle.
l Gravity: the force acting on the particle due to gravity.
l Buoyancy: the buoyancy force acts against the direction of gravity and thus in opposite direction
of the gravity force on a particle. The buoyancy force is accessible only when the gravity forces
are selected in the Physical Configuration / Flow Model page.
l Dispersion: while moving through a turbulent flow, each particle faces a sequence of random
turbulent eddies that result in a lack of accuracy in particle velocity and position. A model for the
instantaneous fluid velocity is constructed that takes into account the turbulent dispersion of the
particles. The treatment is only available for the k-based turbulence models.
14. Clicking on the tab Boundary Conditions to define the boundary conditions for each particle
class.
15. Under the sub-tab Inlet, set the boundary condition for Class #1 as follows:
l Change the type of Velocity Vx to fct(space) and import the profile Tutorial_5/Profiles_
Particles/Class_1_Vx.p.
l Change the type of Velocity Vz to fct(space) and import the profile Tutorial_5/Profiles_
Particles/Class_1_Vz.p.
l Change the type of Volume fraction to fct(space) and import the profile Tutorial_5/Profiles_
Particles/Class_1_VolumeFraction.p.
l Set the Density to 785 kg/m3.
l Set the Diameter to 2.5e-6 m.
l Change the type of k to fct(space) and import the profile Tutorial_5/Profiles_Particles/Class_
1_k.p.
l Keep all other parameters as default.
The inlet boundary parameters that need to be set are the velocity components, the volume fraction,
density, diameter and turbulent kinetic energy of the particles. Except for the density a constant value
or a profile can be chosen.
16. Under the sub-tab Inlet, click on the button Add class to add the Class #2 and set the
boundary condition as follows:
The added class is a copy of the selected class.
l Set Velocity Vx to the profile Tutorial_5/Profiles_Particles/Class_2_Vx.p.
l Set Velocity Vz to the profile Tutorial_5/Profiles_Particles/Class_2_Vz.p.
l Set Volume fraction to the profile Tutorial_5/Profiles_Particles/Class_2_VolumeFraction.p.
l Set the Density to 785 kg/m3.
l Set the Diameter to 4.75e-5 m.
l Set k to the profile Tutorial_5/Profiles_Particles/Class_2_k.p.
l Keep all other parameters as default.
17. Under the sub-tab Inlet, click on the button Add class to add the Class #3 and set the
boundary condition as follows:
l Set Velocity Vx to the profile Tutorial_5/Profiles_Particles/Class_3_Vx.p.
l Set Velocity Vz to the profile Tutorial_5/Profiles_Particles/Class_3_Vz.p.
l Set Volume fraction to the profile Tutorial_5/Profiles_Particles/Class_3_VolumeFraction.p.
l Set the Density to 785 kg/m3.
l Set the Diameter to 9.75e-5 m.
l Set k to the profile Tutorial_5/Profiles_Particles/Class_3_k.p.
l Keep all other parameters as default.
18. Click on the sub-tab Solid, keep all parameters as default.
When the particles reach the walls, the particles are by default reflected from the wall (Rebound). In
this case, a reflection coefficient (default value 1) is required. The Reflection ratio is only used to
consider the loss of normal velocity of the particles. If the ratio is zero, the normal velocity of all the
particles will be zero after collision with the walls. Whereas if it is 1.0, all particles are reflected,
without any loss of energy.
19. In the tab Outputs, keep all parameters as default.
The averaging type can be mass or number averaged.
The output of the statistics of the particle classes can be selected. It can be chosen between, first, the
averages over all classes individually. Second, the mean over all classes, which is the ensemble
averaged over all classes together. Third, a combination of the first two.
20. Click on the button Ok to close the dialog box.
5.3.3
Select output quantities.
21. Go to the Computation Control / Outputs page. Under the category Lagrangian, select the
following quantities for output.
l Lagr_ParticleVelocity: the velocity of the particles
l Lagr_Velocity_xyz: the velocity vector of the particles
l Lagr_VolumeFraction: the volume of the particles / m³.
l Lagr_TurbulentKineticEnergyK: the turbulent kinetic energy of the particles.
5.3.4
Save Project & Computation
22. In Project menu, select Save to save the project (".iec").
23. In Project menu, select Save Selected 'Run' Files to save the ".run" file of the selected
computation.
5.3.5
Launch computation
24. Click on Start Flow Solver icon to start the calculation.
25. Click on Ok to accept and start the computation in serial.
Once the calculation is finished, the flow solver stops. The final solution is then stored for post--
processing and the task manager window is closed.
5.4
POST-PROCESSING
26. Click on the icon
to access CFView™ from the FINE™/Open GUI.
27. In the QAP Surfaces, expand the group periodic_1, select the patch DOMAIN1_group_2.
28. Select the quantity Lagr_ParticleVelocity_W (MEAN) to view the mean particle velocity
component
.
29. Select the quantity Lagr_TurbelentKineticEnergyK (class #3) to view the turbulent kinetic
energy of the class #3.
The contour of the quantity Lagr_ParticleVelocity_W (MEAN) is not smooth enough. This is because
the default value of the number of particles injected per cell is not enough in this case. Increasing this
number will improve the distribution.
5.5
REFERENCE:
Sommerfeld M., Qiu H.-H., 1998, Experimental studies of spray evaporation in turbulent flow,
Int. J. of Heat and Fluid Flow, 19, pp. 10-22
CUSTOMIZATION IN OPENLABS™
The following tutorials allow to familiarize with the possibilities of OpenLabs™ to customize physical
models.
In this section
558
FINE™/Open with OpenLabs™ 7.2 Tutorials
TUTORIAL 1.
CUSTOMIZED INITIAL SOLUTION FOR
BEND PIPE
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l spatial discretization of the flow equations,
l flow computation,
l visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated. The unstructured CFD package consists of the
following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
l OpenLabs™ is a tool allowing the user to customize the internal physical models in FINE™/Open
with OpenLabs™ and/or add external physical models.
OpenLabs™ gives the user ability to customize physical models in the FINE™/Open solver. In
OpenLabs™, the physical problem to solve is described in easy and clear meta-language using the user
interface and saved in ResourceFile. Then, OpenLabs™ will transform the ResourceFile to a C++ file
and build it
to a dynamic library, which will be loaded automatically by the flow solver when
launching the computation. To start the process, you need to do the following steps:
l Create a FINE™/Open project;
l Analyze the project to get potential input parameters;
l Define a physical model and build the library;
l Run the computation and post-process the results.
This tutorial is particularly adapted to an OpenLabs™ application. It makes use of FINE™/Open
including OpenLabs™ and CFView™.
In this tutorial, you will learn how to:
l open an existing project in the FINE™/Open GUI;
l activate OpenLabs™;
l analyze your project to get potential input parameters;
l define a new initial flow field;
l build the library;
l start the computation;
l visualize the results with CFView™.
1.1
INTRODUCTION
1.1.1
Prerequisites
This tutorial assumes that you are familiar with the whole FINE™/Open with OpenLabs™ chain
and that you have completed all the Beginner tutorials, so that you can set up a FINE™/Open
project correctly. This tutorial will start from an existing FINE™/Open project. Some steps in the
setup of a FINE™/Open project and post-processing procedure will not be shown explicitly.
1.1.2
Problem Description
The problem to be considered is a 3D bend pipe as shown in the following figure. The case
consists of one inlet, one outlet, one mirror (inside surface) and three solid boundaries (top,
bottom and outside surfaces). The working fluid is AIR (perfect gas) defined in the FINE™/Open
fluid database. The fluid enters the pipe at a velocity of 0.1 m/s. The Reynolds number based on
the inlet velocity and the inlet width is 68,479, which means the flow is laminar.
If the flow field is initialized by using the constant values, the flow direction will be uniform. For
example, the following figure shows the initialized flow field on the mirror boundary when a
constant initial velocity is given: Vx=0.1 m/s; Vy=0.1 m/s; Vz=0 m/s.
This figure is generated in CFView™ by using the provided project, where the option Coarse grid
initialization is deactivated and the Number of iterations is set to 0. The boundary conditions have
been applied, so that the velocity is normal to inlet at the inlet boundary and the magnitude of the
velocity is 0 at the solid boundary.
Now, suppose that you want to give a better initial velocity and let the initialized flow direction
following the pipe, which can be described by:
where (0.001, 0.028) is the center of the circle (bend of the pipe) in the XY plane.
To apply this initial velocity, you can do it in OpenLabs™ within FINE™ /Open.
1.1.3
Preparation
l Copy the provided project "Tutorial_ OL_ BendPipe" ( download Customization with
OpenLabs™ tutorial archive) to your working directory.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
1.2
CREATE FINE™/OPEN WITH OPENLABS™
PROJECT
In this tutorial, an existing project will be opened as starting point.
1.2.1
Open Existing Project
1. After launching the FINE™/Open GUI, click on the icon Open an existing project and click
on the button Ok to confirm.
2. In the dialog box, locate and select the project name "Tutorial_OL_BendPipe.iec" available in
"FINE-Open_ OpenLabs/Tutorial_ 1" folder of the tutorial package (download Customization
with OpenLabs™ tutorial archive).
3. Select the computation "OL_ initial" under Computations . Check all the settings in the
FINE™/Open GUI. In this tutorial, a project has been created and provided. The main settings
are:
l Fluid model: AIR(Perfect)
l Flow model: Laminar Navier-Stokes
l Low speed flow is activated in the Physical Configuration / Flow Model page
l Inlet boundary condition: Static Quantities Imposed
l Static Temperature = 293 K
l Vx = 0.1 m/s
l Vy = 0 m/s
l Vz = 0 m/s
l Outlet boundary condition: Pressure Imposed
l Static Pressure = 101325 Pa
l Initial solution: Constant values
l Pressure = 101325 Pa
l Temperature = 293 K
l Vx = 0.1 m/s
l Vy = 0.1 m/s
l Vz = 0 m/s
l Coarse grid initialization is deactivated in the Numerical Parameters / General
Parameters page
l Number of iterations is set to 0 in the Computation Control / Control Variables page
In this project, the option Coarse grid initialization is deactivated and the Number of iterations
is set to 0, so that the user can check the initialized flow field in CFView™.
It is recommended to set- up the FINE™/Open project as similar as possible to the final modeling
approach. For example, if the user wants to modify an internal k-ε turbulence model, a project with
the internal k-ε turbulence model should be set-up. A complete customized turbulence model can be
added in a Laminar Navier-Stokes simulation. However, it might be easier to start from an internal
turbulent framework and modify it according to the specific needs.
1.3
ANALYZE THE PROJECT
A step by step approach is proposed in the following lines. It aims at driving you through various
steps that need to be executed to analyze the project in order to get the potential input parameters.
4. In the OpenLabs menu, double left-click on Resource Manager to open the OpenLabs
Resource Editor.
The OpenLabs Resource Editor is a basic editor
the
ResourceFile and build the dynamic library, see the user manual on how to use the OpenLabs
Resource Editor.
that allows the user
to create/edit
5. Click on the block name "Block_1" and click on the sign
OpenLabs™ for the selected block.
before the block name to activate
OpenLabs™ is block-dependent. The user can activate OpenLabs™ for part of the blocks or all the
blocks in the project.
6. Click on the menu Tools / Analyze to analyze the current computation and display the results
of the project analysis.
When writing the resource to define a physical model, the user should refer to the results of the
internal constants, variables, algebraic
project analysis. The project analysis gives the list of
expressions, transport equations with their corresponding source terms and diffusion coefficients,
equation of state, as well as the internal boundary conditions. All these items can be used in the
resource or customized by the user in the resource.
7. Click on the menu View / Analysis to hide the Analysis frame.
1.4
DEFINE A PHYSICAL MODEL & BUILD THE
LIBRARY
A step by step approach is proposed in the following lines. It aims at driving you through various
steps that need to be executed to define a physical model and build the library.
1.4.1
Define a physical model
8. In the frame Resource, type the following code under the section starting with =>INITIAL_
PROFILES.
#Customize the initial solution for Vx
@ INITIAL_FIELD: Initial_VelocityX
->EXPRESSION: IF(xCoord<0.001) 0.1 ELSEIF(yCoord>0.028) 0.0 ELSE 0.1*cos(atan
((xCoord-0.001)/(0.028-yCoord)))
->ExistingField: Vx
#Customize the initial solution for Vy
@ INITIAL_FIELD: Initial_VelocityY
->EXPRESSION: IF(xCoord<0.001) 0.0 ELSEIF(yCoord>0.028) 0.1 ELSE 0.1*sin(atan
((xCoord-0.001)/(0.028-yCoord)))
->ExistingField: Vy
The character "#" is used to comment out complete lines or part of the lines. All the text written in
the same line after the symbol "#" will be considered as comments.
The character "\" is used to break too long lines. All the text written in the same line after the symbol
"\"  will be ignored.
OpenLabs™ language is a kind of meta-language. The user should refer to OpenLabs™ to learn how
to write a resource in Openlabs™ language. To write a resource, the user can start from the empty
resource (File/New/Empty Resource), from the template (File/New/From Template...) or from
an imported resource (File/Import...).
In this tutorial, the initialization of two internal variables "Vx" and "Vy" is customized. In order to
modify the initialization of an internal variable, the keyword ->ExistingField:  must be used and the
name of the internal variable must be given. The name of the internal variables can be found in the
project analysis results (step 6). All the other variables will be initialized by the values imposed in the
Initial Solution / Initial Solution page.
1.4.2
Build the Library
9. Select the block "Block_1", click on the menu Build / Build current to build the dynamic
library of the current block.
After the resource is written, the user needs to Build Library for each block. The information of
building a library will be outputted in the Output frame. If building a library fails, error messages
will be given in the Output frame.
If building a library is successful, the check mark before the block name will be green. If building a
library has failed, the check mark will be red.
10. Click on the menu File / Close to exit the OpenLabs Resource Editor.
1.5
RUN COMPUTATION & POST-PROCESS
RESULTS
The following procedure aims at driving you through various steps that need to be executed to
launch the computation and post-process the results.
1.5.1
Save Project & Computation
11. Click on Save Project button to save the project.
12. Click on Save Selected 'Run' files button to save the computation.
1.5.2
Start Computation
13. Click on Start Flow Solver button to launch the computation and click on Ok to run in serial
mode.
In this computation, the option Coarse grid initialization is deactivated and the Number of
iterations is set to 0, so that the flow solver will stop after applying the initial solution and boundary
conditions.
1.5.3
Post-process Results
14. After the computation finished, launch CFView™ from the FINE™ graphical user interface
by clicking on the CFView™ icon (
customized initial solution is implemented correctly.
). Check the velocity vector on the mirror boundary. The
The boundary conditions have been applied, so that the magnitude of the velocity is 0 at the solid
boundary.
TUTORIAL 2.
CUSTOMIZED UNSTEADY INLET
BOUNDARY CONDITION
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l spatial discretization of the flow equations,
l flow computation,
l visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated. The unstructured CFD package consists of the
following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
l OpenLabs™ is a tool allowing the user to customize the internal physical models in FINE™/Open
and/or add external physical models.
OpenLabs™ gives the user ability to customize physical models in the FINE™/Open solver. In
OpenLabs™, the physical problem to solve is described in easy and clear meta-language using the user
interface and saved in ResourceFile. Then, OpenLabs™ will transform the ResourceFile to a C++ file
and build it
to a dynamic library, which will be loaded automatically by the flow solver when
launching the computation. To start the process, you need to do the following steps:
l Create a FINE™/Open project;
l Analyze the project to get potential input parameters;
l Define a physical model and build the library;
l Run the computation and post-process the results.
This tutorial is particularly adapted to an OpenLabs™ application. It makes use of FINE™/Open
including OpenLabs™ and CFView™.
In this tutorial, you will learn how to:
l open an existing project in the FINE™/Open GUI;
l activate OpenLabs™;
l analyze your project to get potential input parameters;
l define a new inlet boundary condition;
l build the library;
l start/stop the computation;
l visualize the results with CFView™ .
2.1
INTRODUCTION
2.1.1
Prerequisites
This tutorial assumes that you are familiar with the whole FINE™/Open with OpenLabs™ chain
and that you have completed all the Beginner tutorials, so that you can set up a FINE™/Open
project correctly. This tutorial will start from an existing FINE™/Open project. Some steps in the
setup of a FINE™/Open project and post-processing procedure will not be shown explicitly.
2.1.2
Problem Description
The problem to be considered is the second guide vane in the GE-E³ high pressure turbine, as
shown in the following figure. In this tutorial, 2D configuration is used. One cell is generated in
the radial direction and both hub and shroud are set to MIRROR boundary condition. The
working fluid is AIR (perfect gas) defined in the FINE™/Open fluid database. The inlet/outlet
pressure ratio is about 0.61 so that the outlet Mach number is close to 1.
In this tutorial, an unsteady inlet temperature will be defined to simulate the effect of the hot
streak, which comes from the upstream rotor blade. It is assumed that the total pressure and
velocity direction at inlet are constant. The total temperature at inlet is specified by the following
profile, which is rotating at a speed of 8283 RPM. The frequency of the inlet total temperature
corresponds to a rotor/stator blade number ratio of 1:1.
The total temperature profile at inlet can be described by:
where Tt0 is the total temperature of the free stream; n is the number of the upstream rotor blade, τ
is the period of the upstream rotor blade passing.
To apply this unsteady inlet boundary condition, you can do it
OpenLabs™.
in FINE™/Open with
2.1.3
Preparation
l Copy the provided project "Tutorial_ OL_ UnsteadyBC" ( download Customization with
OpenLabs™ tutorial archive) to your working directory.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
2.2
CREATE FINE™/OPEN WITH OPENLABS™
PROJECT
In this tutorial, an existing project will be opened as starting point.
2.2.1
Open Existing Project
1. After launching the FINE™/Open GUI, click on the icon Open an existing project and click
on the button Ok to confirm.
2. In the dialog box, locate and select the project name "Tutorial_OL_UnsteadyBC.iec" available
in "FINE-Open_OpenLabs/Tutorial_2" folder of the tutorial package (download Customization
with OpenLabs™ tutorial archive).
3. Check all the settings in the FINE™/Open GUI. In this tutorial, a project has been created and
provided. The main settings are:
l Time Configuration: Unsteady
l Fluid model: AIR(Perfect gas)
l Turbulence model: Spalart-Allmaras
l Inlet boundary condition: Total Quantities Imposed / Velocity direction (V extrapolated)
l Vr/|V| = 0
l Vt/|V| = -0.1922
l Vz/|V| = 0.9574
l Absolute Total Pressure = 153138 Pa
l Absolute Total Temperature 544.5 K
l Turbulence Viscosity = 0.0001 m²/s
l Outlet boundary condition: Pressure Imposed / Static Pressure Imposed
l Static Pressure = 93966 Pa
l Initial solution: For turbomachinery
l Inlet Static pressure = 140000 Pa
l CPU Booster is activated
l Dual time step inner-iteration control
l Convergence criteria = -6.0
l Maximum number of inner iterations = 20
l Computation Control / Control Variables:
l Physical time step = 7.5456e-6 s
l Number of time steps = 200
l Number of steady iterations = 50
In this project, 20 time steps are used for each upstream rotor blade period and 10 periods are
simulated.
It is recommended to set- up the FINE™/Open project as similar as possible to the final modeling
approach. For example, if the user wants to modify an internal k-ε turbulence model, a project with
the internal k-ε turbulence model should be set-up. A complete customized turbulence model can be
added in a Laminar Navier-Stokes simulation. However, it might be easier to start from an internal
turbulent framework and modify it according to the specific needs.
2.3
ANALYZE PROJECT
A step by step approach is proposed in the following lines. It aims at driving you through various
steps that need to be executed to analyze the project in order to get the potential input parameters.
2.3.1
Get Analysis File
4. In the OpenLabs menu, double left-click on Resource Manager to open the OpenLabs
Resource Editor.
The OpenLabs Resource Editor is a basic editor
the
ResourceFile and build the dynamic library, see the user manual on how to use the OpenLabs
Resource Editor.
that allows the user
to create/edit
5. Click on the block name "stator_flux" and click on the sign
activate OpenLabs™ for the selected block.
before the block name to
OpenLabs™ is block-dependent. The user can activate OpenLabs™ for part of the blocks or all the
blocks in the project.
6. Click on the menu Tools / Analyze to analyze the current computation and display the results
of the project analysis
When writing the resource to define a physical model, the user should refer to the results of the
project analysis. The project analysis gives the list of
internal constants, variables, algebraic
expressions, transport equations with their corresponding source terms and diffusion coefficients,
equation of state, as well as the internal boundary conditions. All these items can be used in the
resource or customized by the user in the resource.
7. Click on the menu View / Analysis to hide the Analysis file.
2.4
DEFINE PHYSICAL MODEL & BUILD
LIBRARY
A step by step approach is proposed in the following lines. It aims at driving you through various
steps that need to be executed to define a physical model and build the library.
2.4.1
Define Physical Model
8. In the frame Resource, type the following code under the corresponding sections starting with
=>CONSTANTS and =>CUSTOM_BOUNDARY_CONDITIONS.
=>CONSTANTS
@ Tt0=544.5
@ PI=3.14159265
@ timePeriod= 1.509115E-4
=>CUSTOM_BOUNDARY_CONDITIONS
@ CUSTOMIZED_BOUNDARY_CONDITION: unsteadyTtInlet
->EXPRESSION: MIN( Tt0*(1.0+0.4*pow((sin(48*tCoord/2-PI*Time/timePeriod)),10)),
1.2*Tt0)
->ExistingBC: "Absolute Total Temperature" , Inlet
The user can add new external constants or modify internal constants. When modifying an internal
constant, the constant name must be the same as the one in the results of the project analysis (step 6).
It is important to pay attention to the spelling of the internal constants. In case of a misspelling,
OpenLabs™ will create a new constant instead of modifying the internal one!
OpenLabs™ language is a kind of meta-language. The user should refer to the user manual to learn
how to write a resource in Openlabs™ language. To write a resource, the user can start from the
empty resource (File/New/Empty Resource), from the template (File/New/From Template) or
from an imported resource (File/Import).
In this tutorial, the boundary condition Absolute Total Temperature at inlet is customized. In
order to modify the boundary condition of an internal PDE, the keyword ->ExistingBC:  must be
used and the name of the internal boundary must be given. The name of the internal boundary can be
found in the project analysis results (step 6). All the other boundary conditions at inlet will be
imposed by the values imposed in the Boundary Conditions / Boundary Conditions page under
the tab INLET.
2.4.2
Build Library
9. Select the block "stator_flux", click on the menu Build / Build current to build the dynamic
library for the current block.
After the resource is written, the user needs to Build Library for each block. The information of
building a library will be outputted in the Output frame. If building a library fails, error messages
will be given in the Output frame.
If building a library is successful, the check mark before the block name will be green. If building a
library has failed, the check mark will be red.
10. Click on the menu File / Close to exit the OpenLabs Resource Editor.
2.5
RUN COMPUTATION & POST-PROCESS
RESULTS
The following procedure aims at driving you through various steps that need to be executed to
launch the computation and post-process the results.
2.5.1
Save Project & Computation
11. Click on Save Project button to save the project.
12. Click on Save Selected 'Run' files button to save the computation.
2.5.2
Start & Stop Computation
13. Click on Start Flow Solver button to launch the computation and click on Ok to run in serial
mode.
To save and stop a computation while running, the button Save Solution And Stop Flow Solver
should be pressed. However, to stop the computation without saving, the Kill Flow Solver button
should be used.
2.5.3 Monitoring
14. Click on Steering button to monitor the convergence history of the global variables.
In this case, the periodic fluctuating of the global variables is reached at about the sixth period.
2.5.4
Post-process Results
15. After the computation finished, launch CFView™ from the FINE™ graphical user interface
by clicking on the CFView™ icon (
). The following figure shows the contour of the total
temperature on the Blade-to-Blade surface at the last time step. The customized inlet boundary
condition is implemented correctly.
585
FINE™/Open with OpenLabs™ 7.2 Tutorials
TUTORIAL 3.
INTRODUCE COMBUSTION MODEL
The resolution of computational fluid dynamics (CFD) problems involves three main steps:
l spatial discretization of the flow equations,
l flow computation,
l visualization of the results.
For this purpose, NUMECA has developed a Flow INtegrated Environment with which the flow in
internal and external configurations can be simulated. The unstructured CFD package consists of the
following tools:
l HEXPRESS™ is an automatic unstructured Hexahedral mesh generator software designed to
automatically generate meshes for the discretization of complex 2D and 3D geometries,
l HEXPRESS™/Hybrid is an isotropic hybrid mesh generator designed for complex geometries
which comprises mainly hexahedral cells with tetrahedral, pyramids and prism cells,
l FINE™/Open flow solver is a state-of-the-art multi-domain unstructured code for the solution of
the Euler and Navier-Stokes equations to compute laminar, transitional and turbulent flow,
l CFView™ is a highly interactive flow visualization and post-processing software,
l FINE™ Graphical User Interface is a user-friendly environment that allows the user to accomplish
all steps, from grid generation to flow visualization.
l OpenLabs™ is a tool allowing the user to customize the internal physical models in FINE™/Open
and/or add external physical models.
OpenLabs™ gives the user ability to customize physical models in the FINE™/Open solver. In
OpenLabs™, the physical problem to solve is described in easy and clear meta-language using the user
interface and saved in ResourceFile. Then, OpenLabs™ will transform the ResourceFile to a C++ file
and build it
to a dynamic library, which will be loaded automatically by the flow solver when
launching the computation. To start the process, you need to do the following steps:
l Create a FINE™/Open project;
l Analyze the project to get potential input parameters;
l Define a physical model and build the library;
l Run the computation and post-process the results.
This tutorial is particularly adapted to an OpenLabs™ application. It makes use of FINE™/Open
including OpenLabs™ and CFView™.
In this tutorial, you will learn how to:
l open an existing project in the FINE™/Open GUI;
l activate OpenLabs™;
l analyze your project to get potential input parameters;
l define a new premixed combustion model: customize fluid properties and define a new PDE;
l build the library;
l manage outputs by OpenLabs™;
l start/stop the computation;
l monitor the convergence history of the new PDE variable;
l visualize the results with CFView™.
3.1
INTRODUCTION
3.1.1
Prerequisites
This tutorial assumes that you are familiar with the whole FINE™/Open with OpenLabs™ chain
and that you have completed all the Beginner tutorials, so that you can set up a FINE™/Open
project correctly. This tutorial will start from an existing FINE™/Open project. Some steps in the
setup of a FINE™/Open project and post-processing procedure will not be shown explicitly.
3.1.2
Problem Description
The problem to be considered is a Bunsen burner, as shown in the following figure. In this
tutorial, 2D axisymmetric configuration is used. One cell is generated in the tangential direction.
The boundaries with the lowest and highest radius are set to MIRROR type. The flow model is
set to Laminar Navier-Stokes in the starting project.
In this tutorial, a premixed combustion model will be added by OpenLabs™. The added
premixed combustion model, TFC model, is a progress variable based model. Assuming the flow
is laminar, the flame front propagation can be modeled by solving a transport equation for the
progress variable, denoted by c:
The progress variable is defined as:
and the source term:
Ignoring the pressure fluctuations, the density of the fluid can be calculated by using the relation:
The temperature can be calculated from the definition of the progress variable:
where the constants:
l the Schmidt number Sc=0.7;
l the laminar flame speed U=0.1 m/s;
l the temperature of the unburned mixture Tu=293 K;
l the density of the unburned mixture ρu=1.2 kg/m³;
l the adiabatic temperature of the burnt mixture Tad=1665 K.
For the progress variable, the inlet boundary condition needs to be defined. Here, the progress
variable is set to 0 if r < 0.0125m and 1 if r >= 0.0125m.
To apply this premixed combustion model, you can do it in FINE™/Open with OpenLabs™.
3.1.3
Preparation
l Copy the provided project "Tutorial_ OL_ Combustion" ( download Customization with
OpenLabs™ tutorial archive) to your working directory.
l Start FINE™/Open v7.2:
l For Linux systems, you can access FINE™/Open v7.2 graphical user interface with the
following command line:
fine -niversion open72 -print
l For Windows systems, you can access FINE™/Open v7.2 graphical user interface from the
start menu by going to /Programs/NUMECA software/FineOpen72/FINEOpen.
3.2
CREATE FINE™ /OPEN PROJECT
In this tutorial, an existing project will be opened as starting point.
3.2.1
Open Existing Project
1. After launching the FINE™/Open GUI, click on the icon Open an existing project and click
on the button Ok to confirm.
2. In the dialog box, locate and select the project name "Tutorial_OL_Combustion.iec" available
in "FINE-Open_OpenLabs/Tutorial_3" folder of the tutorial package (download Customization
with OpenLabs™ tutorial archive)
3. Check all the settings in the FINE™/Open GUI. In this tutorial, a project has been created and
provided. The main settings are:
l Time Configuration: Steady
l Fluid model: AIR(Perfect)
l Flow model: Laminar Navier-Stokes
l Low speed flow is activated. The Merkle preconditioning is used.
l Inlet boundary condition: Static Quantities Imposed / Velocity Components
l Vr = 0 m/s
l Vt = 0 m/s
l Vz = profile
l Static Temperature 293 K
l Outlet boundary condition: Pressure Imposed / Static Pressure Imposed
l Static Pressure = 101300 Pa
l Initial solution: Constant values
l Pressure = 101300 Pa
l Temperature = 293 K
l Velocity type = Relative
l Vr = 0 m/s
l Vt = 0 m/s
l Vz = 1 m/s
l CPU Booster is activated with CFL number = 100
l Computation Control / Control Variables:
l Number if iterations = 1000
l Convergence criteria = -6
It is recommended to set- up the FINE™/Open project as similar as possible to the final modeling
approach. For example, if the user wants to modify an internal k-ε turbulence model, a project with
the internal k-ε turbulence model should be set-up. A complete customized turbulence model can be
added in a Laminar Navier-Stokes simulation. However, it might be easier to start from an internal
turbulent framework and modify it according to the specific needs.
3.3
ANALYZE PROJECT
A step by step approach is proposed in the following lines. It aims at driving you through various
steps that need to be executed to analyze the project in order to get the potential input parameters.
3.3.1
Get Analysis File
4. In the OpenLabs menu, double left-click on Resource Manager to open the OpenLabs
Resource Editor.
The OpenLabs Resource Editor is a basic editor
the
ResourceFile and build the dynamic library, see the user manual on how to use the OpenLabs
Resource Editor.
that allows the user
to create/edit
5. Click on the block name "DOMAIN1" and click on the sign
activate OpenLabs™ for the selected block.
before the block name to
OpenLabs™ is block-dependent. The user can activate OpenLabs™ for part of the blocks or all the
blocks in the project.
6. Click on the menu Tools / Analyze in detail to analyze the current computation and display
the results of the project analysis.
When writing the resource to define a physical model, the user should refer to the results of the
internal constants, variables, algebraic
project analysis. The project analysis gives the list of
expressions, transport equations with their corresponding source terms and diffusion coefficients,
equation of state, as well as the internal boundary conditions. All these items can be used in the
resource or customized by the user in the resource.
When analyzing the computation in detail, the analysis will give not only the name of the objects, but
also the math expression defining the objects. In addition, the user is able to use the expression in the
project analysis results to describe the user defined model.
7. Click on the menu View / Analysis to hide the Analysis frame.
3.4
DEFINE PHYSICAL MODEL & BUILD
LIBRARY
A step by step approach is proposed in the following lines. It aims at driving you through various
steps that need to be executed to define a physical model and build the library.
3.4.1
Define Physical Model
8. In the frame Resource, type the following code under the corresponding sections.
=>CONSTANTS
@ combSchmidtLam =0.7 #define laminar Schmidt number
@ laminarFlameSpeed=0.1 #define laminar flame speed
@ premixedFlameTemp = 1665 #define adiabatic flame temperature
@ unburntDens=1.2 #define unburned density
@ unburntTemp=293 #define unburned temperature
@ phys_Prandtl_=0.72 #define Prandtl number of the fluid
=>CUSTOM_FLUID_PROPERTIES
#customize the density of the fluid
@ EQUATION_OF_STATE: MyEOS
->EOS_RELATION: Density
->EXPRESSION: unburntDens*unburntTemp / ((1-
ProgVariable)*unburntTemp+ProgVariable*premixedFlameTemp)
#customize the conductivity of the fluid
@TRANSP_PROPERTY: MyConductivity
->EXPRESSION: phys_cp_ / phys_Prandtl_ * Viscosity
->ExistingCalculator: Thermal Conductivity calculator
#customize the viscosity of the fluid (Sutherland law). The viscosity is clipped if the temperature
is less than 120K for robustness
@TRANSP_PROPERTY: MyViscosity
->EXPRESSION: IF(CombTemp<=120) nuRef_*rhoInf_ * sqrt(120.0/Tinf_) * (120.0/Tinf_)
* (Tinf_+Tsuther_) / (120.0+Tsuther_) ELSE nuRef_*rhoInf_ * sqrt(CombTemp/Tinf_) *
(CombTemp/Tinf_) * (Tinf_+Tsuther_) / (CombTemp+Tsuther_)
->ExistingCalculator: Viscosity calculator
#define the diffusion coefficient for the new PDE
@TRANSP_PROPERTY: CombDiffCoeff
->EXPRESSION: Viscosity/combSchmidtLam
The viscosity must be customized corresponding to the combustion temperature.
=>EQUATIONS
#define combustion temperature
@ NONDIFFEXPR: CombustionTemperature
->EXPRESSION: CombTemp= (1-
ProgVariable)*unburntTemp+ProgVariable*premixedFlameTemp
->BOUNDARY_FACE: Extrapolation
->INITIAL_VALUE: 1665.0
->IS_PART_OF_VISCOUS: NO
#add new PDE for progress variable
@ PDE: ProgressVariableEquation
->EXPRESSION: DDT(ProgVariable) + CONV(ProgVariable) = DIFF(ProgressVariable_
diff_coeff) + SOURCE(sourceProgressVariable)
->Convective_Scheme: UpwindHighOrderConservative
->UseCustomBC: ProgressVariableInlet, 2
->InitializeTo: ProgressVariableInit
->ConstantRelaxFactor: 0.5
->LowerLimit: 1e-20
->UpperLimit: 1.0
When a new PDE is added, its boundary condition, diffusion coefficient, initial solution and source
term must be defined in the corresponding sections, as defined below.
#define boundary condition for new PDE
=>CUSTOM_BOUNDARY_CONDITIONS
@ CUSTOMIZED_BOUNDARY_CONDITION: ProgressVariableInlet
->EXPRESSION: IF(rCoord>=0.0125) 1 ELSE 0.0
#define diffusion coefficient for new PDE
=>ALGEBRAIC_DIFFUSION_COEFFICIENTS
@ ALGDIFFCOEFF: ProgressVariable_diff_coeff
->EXPRESSION: CombDiffCoeff
#define initial solution for new PDE
=>INITIAL_PROFILES
@ INITIAL_FIELD: ProgressVariableInit
->EXPRESSION: 1.0
#define source term for new PDE
=>SOURCETERMS
@ SOURCE: sourceProgressVariable
->EXPRESSION: unburntDens*laminarFlameSpeed*progressVariableGradient
->AddToViscous: YES
=>AUXTERMS
@ progressVariableGradient = sqrt(GRAD(ProgVariable,x)*GRAD(ProgVariable,x)+GRAD
(ProgVariable,y)*GRAD(ProgVariable,y)+GRAD(ProgVariable,z)*GRAD(ProgVariable,z)
)
The character "#" is used to comment out complete lines or part of the lines. All the text written in
the same line after the symbol "#" will be considered as comments.
The character "\" is used to break too long lines. All the text written in the same line after the symbol
"\"  will be ignored.
OpenLabs™ language is a kind of meta-language. The user should refer to the user manual to learn
how to write a resource in Openlabs™ language. To write a resource, the user can start from the
empty resource (File/New/Empty Resource), from the template (File/New/From Template) or
from an imported resource (File/Import).
3.4.2
Build Library
9. Select the block "DOMAIN1", click on the menu Build / Build current to build the dynamic
library of the current block.
After the resource is written, the user needs to Build Library for each block. The information of
building a library will be outputted in the Output frame. If building a library fails, error messages
will be given in the Output frame.
If building a library is successful, the check mark before the block name will be green. If building a
library has failed, the check mark will be red.
10. Click on the menu File / Close to exit the OpenLabs Resource Editor.
3.5
RUN COMPUTATION & POST-PROCESS
RESULTS
The following procedure aims at driving you through various steps that need to be executed to
launch the computation and post-process the results.
3.5.1
Select New Variables Outputs
11. Select OpenLabs from the Categories list in the Computation Control / Outputs page
under the tab General. Make sure the new variables are selected to be outputted. Click on the OK
button to confirm.
All the new transport properties defined in the section =>CUSTOM_FLUID_PROPERTIES and
new algebraic expression/PDE variables defined in the section =>EQUATIONS are available for
output. By default, all variables are selected.
The category OpenLabs will appear only after building the library.
3.5.2
Save Project & Computation
12. Click on Save Project button to save the project.
13. Click on Save Selected 'Run' files button to save the computation.
3.5.3
Start & Stop Computation
14. Click on Start Flow Solver button to launch the computation and click on Ok to run in serial
mode.
To save and stop a computation while running, the button Save Solution And Stop Flow Solver
should be pressed. However, to stop the computation without saving, the Kill Flow Solver button
should be used.
3.5.4 Monitor New PDE Variable
15. Click on Start Monitor button to launch Monitor.
16. Select Other variables in the frame Quantities to display and then select ProgVariable to
monitor the convergence history of the new PDE variable.
The residual of the new PDE variable can only be monitored in Monitor. In case of multiblock
computations, the global residual of the new PDE variable can not be monitored.
3.5.5
Post-process Results
17. After the computation finished, launch CFView™ from the FINE™ graphical user interface
by clicking on the CFView™ icon (
variable. The position of the frame front is predicted correctly.
). The following figure shows the contour of the progress
602
FINE™/Open with OpenLabs™ 7.2 Tutorials
© NUMECA International, all rights reserved
EN201805172159

CONTENTS
NOMENCLATURE
CHAPTER 1. GOVERNING EQUATIONS
CHAPTER 2. FLUID MODELS
2.1 Calorically Perfect Gas
2.1.1
2.1.2
Equation of State
Transport Properties
A. The Laminar Viscosity
B. The Heat Conductivity
Equation of State
Transport Properties
2.2 Real Gas
2.2.1
2.2.2
Incompressible Fluid
2.3.1
2.3.2
2.3
Equation of State
Transport Properties
2.4 Condensable Fluid
2.4.1
2.4.2
2.4.3
2.4.4
Introduction
Thermodynamic Tables
Integration of Thermodynamic Tables in the Solver
Selection of the Viscosity, Conductivity, and Specific Heat
CHAPTER 3. TURBULENCE MODELS
3.1 Linear Eddy Viscosity Turbulence Models
3.1.1
3.1.2
3.1.3
3.1.4
Spalart-Allmaras
SARC
k-ε Turbulence Models
A. Yang-Shih model
B. Extended wall functions model
k-ω (M-SST) Turbulence Model
3.2 Nonlinear Eddy Viscosity Turbulence Models
S-BSL-EARSM Model
3.2.1
3.3 Modeling the flow near the wall
3.3.1 Velocity
3.3.2
3.3.3
A. Smooth walls
B. Rough walls
Temperature
Turbulence
A. Standard Wall Function for k-ε model
B. Extended Wall Function for k-ε model
C. Extended Wall Function for Spalart-Allmaras and SARC models
D. Extended Wall Function for k-ω (M-SST) model
3.4 Large Eddy Simulation & Detached Eddy Simulation
FINE™/Open with OpenLabs™ 7.2 Theory Guide
21
21
22
22
22
23
23
24
24
24
24
25
25
25
26
27
29
29
31
32
32
34
34
36
36
39
39
39
40
42
43
43
43
43
3.4.1
Large Eddy Simulation and Sub-Grid-Scale models
A. Governing equations for LES of a compressible fluid
B. Smagorinsky model
C. WALE model
3.4.2 Detached Eddy Simulation models
A. DES97 (natural DES)
B. Delayed DES
C.
Improved Delayed DES
CHAPTER 4. CONJUGATE HEAT TRANSFER
4.1 Simulation of Conduction
4.1.1
4.1.2
Time discretization
Space discretization
4.2 Thermal Coupling Between the Solid and Fluid Blocks
4.3 Full Non-Matching Thermal Connections
CHAPTER 5. BOUNDARY CONDITIONS
5.1
Inlet Boundary Conditions
5.1.1
Imposing the Complete Flow Conditions (Supersonic)
Cartesian Inlet Boundary Conditions
A. Static Quantities Imposed (Subsonic)
B. Total Quantities Imposed (Subsonic)
C. Mass flow, Direction of Absolute Velocity Vector and Static Temperature Imposed (Subsonic)
D.
Cylindrical Inlet Boundary Conditions
A. Static Quantities Imposed (Subsonic)
B. Total Quantities Imposed (Subsonic)
C. Mass Flow Imposed (Subsonic)
D. Total Enthalpy & Dryness Fraction Imposed (Subsonic - Condensable Gas)
E.
Imposing the Complete Flow Conditions (Compressible, Supersonic)
Turbulent Inlet Boundary Conditions
5.1.2
5.1.3
5.2 Outlet Boundary Conditions
5.2.1 Outlet Boundary Conditions for Subsonic Flow
A. Pressure Imposed
B. Mass Flow Imposed
5.2.2 Outlet Boundary Conditions for Supersonic Flow
5.2.3
Treatment of Backflow at Outlet
5.3 Solid Wall Boundary Conditions
Euler Walls
5.3.1
5.3.2 Navier-Stokes Walls
A. Adiabatic Walls
Isothermal Walls
B.
C. Wall with Imposed Heat Flux
D. Wall with Imposed Heat Transfer Coefficient
E. Turbulent Wall Boundary Conditions
5.4 Far-field Boundary Condition
FINE™/Open with OpenLabs™ 7.2 Theory Guide
44
44
46
48
49
49
50
51
55
55
56
56
57
59
59
59
59
61
61
61
61
62
64
65
65
66
66
66
66
67
68
68
68
68
69
69
70
70
70
CHAPTER 6. NUMERICAL SCHEME
6.1 Discretisation and solution theory
6.1.1
Spatial Discretization
A. Viscous Fluxes
Inviscid Fluxes
B.
Time Discretization: Multistage Runge-Kutta
6.1.2
6.1.3 Multigrid Strategy
A. Full Approximation Storage approach
B. Grid transfer operators
Full Multigrid Strategy
Implicit residual smoothing
6.1.4
6.1.5
6.2 Preconditioning
6.2.1 Hakimi preconditioning
A. General Form of the Preconditioning Matrix
B. Eigenvalues of the System
C. Choice of the Parameters α, β and the Reference Velocity
6.2.2 Merkle preconditioning
6.3 Time Configuration
6.3.1
Standard Time Accurate Solver (Non-preconditioned Formulation)
A. First Order Backward Method
B. Second Order Backward Method
C. The Time Stepping
D.
Initial Solution at Each Physical Time Step
6.3.2 Density Based Time Accurate Solver and Preconditioning
A. The Time Stepping
B.
Initial Solution at Each Physical Time Step
CHAPTER 7. MESH ADAPTATION
7.1 H-type adaptation
7.1.1 Anisotropic refinement
7.1.2 Mesh coarsening
7.2 Flow feature detection
7.2.1
7.2.2
7.2.3
Introduction
Sensor and threshold formulations
Flow quantities used for feature detection
7.3 Boundary layer insertion/regularization
Introduction
Boundary layer insertion and regularization
7.3.1
7.3.2
7.3.3 Viscous mesh adaptation
CHAPTER 8. OPTIONAL MODELS
8.1 Combustion Modeling
8.1.1 Non-premixed Combustion
A. Overview
B. Mixture Fraction
C. Chemistry Models
FINE™/Open with OpenLabs™ 7.2 Theory Guide
74
74
74
76
86
90
90
92
94
95
97
97
98
99
100
101
104
105
105
105
106
107
107
108
109
111
111
112
114
114
115
116
117
117
118
120
122
122
122
8.1.2
8.1.3
D. Turbulent Combustion
Premixed Combustion
A. Overview
B. The Bray-Moss-Libby Model
C. Modeling the Source Term
D. Calculation of the gas density and the gas temperature
Partially-premixed Combustion
A. Overview
B. Governing Equations
C. Flamelet Generated Manifolds technique
D. Hybrid BML/Flamelet Technique
8.1.4 NOx formation
8.2 Radiation Modeling
8.2.1 Overview
8.2.2
Radiation with participating media
A. Radiative transfer equation
B. P1-Model
C. Optically Thin Model (OTM)
D. Finite Volume method (FVM)
E. Radiative Properties of Molecular Gases
F. Coupling Radiation with Combustion
G. Turbulence-Radiation Interaction (TRI)
The S2S model
A. Overview
B. Radiosity irradiosity method
C. Boundary Conditions
8.2.3
8.3 Porous Media Model
8.3.1
8.3.2
8.3.3
8.3.4
The Darcy law
The Ergun law
The Integral Law
Thermal Heat Flux Model
8.4 Fluid Structure Interaction
8.4.1 Modal Coupling
8.4.2 Mesh deformation
A. Mesh Deformation with Quaternions
B. Mesh Deformation with RBF
8.5.1
8.5 Fluid-Particle Interaction
Particle tracking
A. Particle tracking procedure
B. Trajectories Calculation - Integration Method
C. Turbulent Dispersion
D. Momentum Two-way Coupling
E. Time Step Calculation
8.5.2 Heat and mass exchange
A. Heating/Cooling
B. Droplet Evaporation
C. Determination of droplet diameter
D. Liquid properties
FINE™/Open with OpenLabs™ 7.2 Theory Guide
126
129
129
130
130
132
133
133
133
134
136
138
141
142
144
144
144
146
148
152
154
154
156
156
157
159
159
160
160
161
162
162
162
164
164
165
166
166
166
167
169
169
170
170
170
171
8.5.3
E. Vapour and gas phase properties
F. Evaporation with 2-Way Coupling
Primary atomization and secondary breakup
A. Primary Atomization
B. Secondary break-up
8.6 Cavitation
8.6.1
8.6.2
The Cavitation Model with the Barotropic Law
The cavitation model with the transport equation model
A. Thermal and transport properties for the liquid-vapor mixture
B. Formulation of the Transport Equation Model (TEM)
C. The effect of turbulence
D. The Transport Equation Model with Thermal Effects
The Cavitation Model with Thermodynamic Tables
8.6.3
8.7.1
8.7 Multi-Species Framework
Inert multi-species
A. Governing Equations
B. Ensuring Mass Conservation
C. Species Diffusion
D. Transport Properties
CHAPTER 9. ROTATING MACHINE
9.1 Rotor/Stator Interaction
9.1.1
9.1.2
Introduction
Full Non-matching Mixing Planes
A. Full Non-matching Technique
B.
Implementation of Mixing Plane Approach with Full Non Matching Technique
9.1.3 Non Reflecting Boundary Conditions
A. Concept
B. Characteristic Variables
C. Non Reflecting 1D
D. Non Reflecting 2D
E. Correction for Enthalpy
Frozen Rotor
9.1.4
9.2 Unsteady Turbomachinery Calculations
9.2.1 Domain Scaling Method
A. Geometry Constraints
B. Full Non-matching Approach
C. Rotor/stator interaction treatment
D. Solution Strategy
Choice of the Physical Time Step
9.2.2
9.3 Harmonic Method
9.3.1 Viscous Stresses & Turbulence Model
9.3.2
9.3.3
Closure of the Model
Rotor/Stator Connection Treatment
CHAPTER 10. COMPUTED VARIABLES
10.1 Global Performance Output
FINE™/Open with OpenLabs™ 7.2 Theory Guide
176
178
178
178
181
191
191
193
193
194
196
196
199
200
200
200
201
203
203
207
207
208
208
209
211
211
211
212
212
215
215
216
216
216
217
217
217
218
219
221
222
CHAPTER 11. REFERENCES
NOMENCLATURE
c*
cp
cv
Eb
FINE™/Open with OpenLabs™ 7.2 Theory Guide
acceleration
vector
speed of
sound;
progress
variable
Normalized
progress
variable
specific heat
at constant
pressure
specific heat
at constant
volume
diffusivity
of the
species
internal
energy per
unit mass
total energy
per unit
volume;
emissive
power
blackbosy
emissive
power
mixture
fraction
view factor
vector
(column
matrix) of
inviscid flux
incident
radiation
vector
(column
matrix) of
viscous flux
gravity
acceleration;
mixture
fraction
variance
enthalpy per
unit mass;
heat transfer
coefficient
total
enthalpy;
irradiation
on a surface
intensity of
radiation
blackbody
intensity
blackbody
intensity at
control
volume
centre P
Ib
Ib,p
Imn
P(f)
Pr
Prt
10
FINE™/Open with OpenLabs™ 7.2 Theory Guide
radiation
intensity at
face j
associated
with
direction by
polar angle
and
azimuthal
angle θm
and
azimuthal
angle φn
radiosity
turbulent
kinetic
energy, rate
coefficient
mass flow
rate
molecular
weight;
Mach
number
pressure
probability
density
function
Prandtl
number
turbulent
Prandtl
number
heat flux
flux of
Qjm
r, θ, z
Re
ST
sT
sL
T+
Tu
11
FINE™/Open with OpenLabs™ 7.2 Theory Guide
Heat flux
through the
face j and
with a solid
angle Δ Qmn
gas constant
per unit
mass
cylindrical
coordinates
universal
gas constant
Reynolds
number
entropy per
unit mass
surface
mean strain
tensor
vector
(column
matrix) of
source term
Turbulent
flame speed
Laminar
flame speed
surface
vector
time
temperature
dimensionle
ss
temperature
(u,v,w)
Wf
x,y,z
y+
12
FINE™/Open with OpenLabs™ 7.2 Theory Guide
vector
(column
matrix) of
conservative
variables
velocity
vector with
component
u, v, w
specific
volume;
vector
(column
matrix) of
primitive
variables
relative
velocity
vector
work
performed
by the
external
forces
x, y, z
cartesian
coordinates
dimensionle
ss normal
distance
from the
wall
mass
fraction of
the species
absorptivity
extinction
coefficient
μt
σs
13
FINE™/Open with OpenLabs™ 7.2 Theory Guide
turbulent
dissipation
rate;
emissivity
polar angle
coefficient
of thermal
conductivit
y;
absorption
coefficient
coefficient
of dynamic
viscosity
coefficient
of turbulent
viscosity
density;
reflectivity
Schmidt
number;
Stefan-
Bolzmann
constant
scattering
coefficient
pseudo time;
optical
thickness;
transmissivi
ty
stress tensor
kinematic
viscosity
turbulent
kinematic
viscosity
scalar
scattering
phase
function
average
scattering
phase
function
from the
control solid
angle to the
control solid
angle
azimuthal
angle
equivalence
ratio
angular
velocity;
specific
dissipation
rate;
weighting
function,
chemical
source term,
scattering
albedo
volume
CHAPTER 1.
GOVERNING EQUATIONS
The flow solver integrated into the FINE™/Open user environment is a multipurpose unstructured code
for 2D and 3D flows in complex geometries, using the latest numerical developments in CFD.
Complex geometries can be easily handled through a nearly fully automatic all-hexahedra unstructured
meshing procedure available in the HEXPRESS™ software.
This chapter describes the basic governing equations solved in the FINE™/Open solver. For more
detailed information on the different aspects such as turbulence, fluid models, multigrid strategy etc.,
see the relevant chapters in this manual.
General Navier-Stokes Equations
The general Navier-Stokes equations written in a Cartesian frame can be expressed as:
where Ω is the control volume and S is the control surface, U is the set of conservative variables:
and
are the advective and diffusive part of the fluxes respectively, also denoted by inviscid
and viscous fluxes in the present manuscript.
where H is the total enthalpy per mass unit:
Only Newtonian fluids are currently considered, which is the case for most gases and common
liquids. For such fluids, the stress tensor is a linear function of the shear rate.
where μ is the dynamic molecular viscosity
The heat flux vector is defined by Fourier's law:
where T is the static temperature and
is the molecular thermal conductivity.
contains the source terms:
with
the
expressing
the
effects
of
external
forces
vector
and
the work
performed by those external forces:
. Other source terms are possible, such as
gravity, depending on the chosen functionality.
More information about the constitutive laws and properties of the fluids can be referred to Fluid
Models chapter.
Time Averaging of Quantities
In principle, the Navier-Stokes equations describe both laminar and turbulent flows. However,
turbulence is a nonlinear process with a wide range of spatial and temporal scales. The direct
simulation of complex turbulent flows in most engineering applications is not possible and will
not be for the foreseeable future.
In the context of scale modeling, the most direct approach is offered by the partitioning of the
flow field into a mean and fluctuating part. This process will produce the Reynolds Averaged
Navier-Stokes (RANS) equations.
The Reynolds averaged equations are derived by averaging the viscous conservation laws over a
time interval T, large enough with respect to the time scales of the turbulent fluctuations, but small
enough with respect to all other time- dependent effects. Time averaging is appropriate for
stationary turbulence and is performed as follows. For any given quantity A, we have:
where
mean turbulent averaged value and
is the fluctuating component. Furthermore, we have:
is
the
The corresponding density-weighted averaging is defined by:
with
and
Density and pressure are time averaged, whereas energy, velocity components and temperature
are density-weighted time averaged.
Treatment of Turbulence in the Equations
The Reynolds-averaged Navier-Stokes equations lead to the introduction of the Reynolds stress
tensor and turbulent heat diffusion term. Since these quantities are unknown, the application of the
Navier-Stokes equations to the computation of turbulent flows requires the introduction of some
modelizations of these unknown relations, based on theoretical considerations coupled to
unavoidable empirical information.
For all the turbulence models, a first-order closure model based on Boussinesq's assumption is
used. This assumption, introducing the concept of eddy-viscosity, consists of considering a linear
connection between the Reynolds-stress tensor and the mean flow strain:
where
is the Reynolds stress tensor, which contains all the effects of turbulence on the
averaged momentum conservation. This term appears after Reynolds averaging the momentum
and energy equations.
is the turbulent eddy-viscosity.
is the mean strain tensor, and
Finally, k is the turbulent kinetic energy.
The turbulent heat flux vector must also be modeled. This is done by introducing a turbulent
through a turbulent Prandtl number
thermal conductivity
, connected to the eddy-viscosity
:
where
After Reynolds averaging and making the Boussinesq assumption, the resulting system of
governing equations is formally equivalent to the original Navier-Stokes system, except that the
dynamic viscosity μ is replaced by
and the thermal conductivity
is replaced by
. The static pressure is also modified by adding the last term in the
mean flow strain correlation, and the averaged total energy also contains - from the Reynolds
averaging process - a term involving the turbulent kinetic energy k.
Notice that in the turbulence models not directly involving the turbulent kinetic energy k, e.g. the
Spalart-Allmaras model, the contribution of this is neglected and static pressure and energy are not
modified.
CHAPTER 2.
FLUID MODELS
In this chapter, details are provided about the different fluid types available in FINE™/Open with
OpenLabs™.
In this section
2.1 Calorically Perfect Gas
2.2 Real Gas
2.3 Incompressible Fluid
2.4 Condensable Fluid
21
23
24
25
2.1
CALORICALLY PERFECT GAS
2.1.1
Equation of State
The perfect gas law is used as constitutive equation:
with r the gas constant for the perfect gas under consideration:
,
with R the universal gas constant and M the molecular weight of the perfect gas.
is the specific heat ratio,
the specific heat at constant pressure, and
the specific heat at
constant volume with:
.
When the gas temperature is so low that the vibrational and electronic modes are frozen, the
internal energy of the gas will be proportional to the temperature, and the specific heats as well as
γ are constant. The gas is "calorically perfect". This is the usual assumption of moderate speed
aerodynamics.
The relation between r and
is given by
.
The values of γ and
variables through the following relation:
are user input. The static pressure is obtained from the conservative
.
2.1.2
Transport Properties
A. The Laminar Viscosity
The laminar kinematic viscosity can be:
l constant,
l given by a profile for a certain temperature range,
l varying according to Sutherland's law.
The dynamic viscosity is then computed within the code by multiplying the kinematic viscosity by
the reference density.
The Sutherland law is given by:
For
For
The
viscosity
,
the
reference
density
page.
B. The Heat Conductivity
The laminar heat conductivity can be:
l constant,
l given by a profile for a certain temperature range,
l specified through the Prandtl number.
,
the
temperature
, and the Sutherland temperature
reference
are specified in the Fluid Model
In case the Prandtl number Pr is specified, the laminar thermal conductivity is obtained as:
The turbulent viscosity is calculated iteratively using one of the turbulence models discussed in
Turbulence Models chapter. The turbulent conductivity is obtained from the turbulent viscosity
and a turbulent Prandtl number
whose value can be controlled through the expert
parameter phys_PrandtlTurb_:
By default, the expert parameter phys_PrandtlTurb_ is set to 1.
2.2
REAL GAS
2.2.1
Equation of State
For real gases or more precisely thermally perfect gases, and depend on the temperature T. The
corresponding values can be entered either through a polynomial approximation or through a
profile.
The thermally perfect gas model is based on two equations:
l the perfect gas relation, still valid:
l the enthalpy equation:
where T0 is a reference temperature. In practice T0 is set equal to the minimum temperature of
the temperature range specified in the Fluid Model page.
These two equations lead to:
In the case of a real gas with varying specific heats one can notice that it is not possible to respect
the 2 above equations with a constant value of r, unless the difference (cp-cv) does not vary with
temperature.
A Constant r model is proposed in the FINE™/Open solver in order to model real gases. The user
specifies the gas constant r(R). Then cp(T) is provided and respectively γ is calculated as:
2.2.2
Transport Properties
The theory of the real gas transport properties is the same as that of the perfect gas. The details
can be found in Transport Properties section.
2.3
INCOMPRESSIBLE FLUID
2.3.1
Equation of State
The density is an user input:
.
This implies a decoupling of the mass and momentum conservation equations from the energy
conservation equation, since no term in the mass and momentum equations depends on the
temperature.
2.3.2
Transport Properties
The theory of the real gas transport properties is the same as that of the perfect gas. The details
can be found in Transport Properties section.
2.4
CONDENSABLE FLUID
2.4.1
Introduction
The aim of the condensable fluid module is to model the real thermodynamic properties of the
fluid by means of interpolation of the variables from dedicated tables.
The module can be used for a single-phase fluid whose properties are too complex to be treated
with a perfect or real gas model. It can also be used in order to treat thermodynamic conditions
that are close to the saturation line. Note that the model can be used on the liquid or on the vapour
side of the saturation curve. In case the thermodynamic state lies inside the two-phase region, a
homogeneous equilibrium two-phase mixture of vapour and liquid is considered. The hypothesis
of an equilibrium mixture is however not valid if the dryness fraction exceeds 20%. The module
can not be used above these fractions, as it completely ignores evaporation- condensation
phenomena.
For a real fluid, the equation of state may be a complicated and usually implicit expression,
generating unacceptable computational overhead if the corresponding equations are explicitly
introduced in the solver. Similarly when an equilibrium mixture of vapour and droplets (wet steam
for instance) is considered as a single fluid, the calculation from the saturation properties of
thermodynamic variables must be done iteratively.
The approach that has been adopted in the FINE™/Open solver consists of using a series of
thermodynamic tables, one table being required each time a thermodynamic variable must be
deduced from two other ones. This implies the creation of many tables as input, but presents the
advantage that no iterative inversion of the tables is done in the solver, with as a consequence a
very small additional CPU time. This additional time corresponds to the one that is needed by the
bilinear (or bicubic) interpolation procedures through the tables. In order to optimize the efficiency
of these interpolations, the input tables are built on the basis of a Cartesian mesh in the plane of
the input variables (V1,V2) (N1 and N2 values for the variables V1 and V2 respectively).
2.4.2
Thermodynamic Tables
Tables are generated using NUMECA internal tools, which are based on various sets of well-
known equations as described below:
l Vander Waals equation,
l Benedict Webb Rubin equation,
l Starling modified Benedict Webb Rubin equation (usually used for hydrocarbons),
l 32 terms modified Benedict-Webb-Rubin equation,
l Equation of state derived from the Helmoltz free energy equation (as for water tables that are
based on the release 1997 IAPWS).
Single tables are generally used, which means that the tables cover both single-phase and two-
phase regions. A bilinear interpolation approach is well adapted to these tables, providing an
adequate smoothing of the saturation region. Bicubic interpolation techniques have also been
implemented and tested. They provide a higher accuracy for a given number of data points but
tend to create spurious oscillations in the saturation region. These oscillations can be weakened by
using more points.
Five categories of tables are used by the solver:
1. Basic tables: p(e,ρ) and T(e,ρ) or ρ(h,p) and T(h,p)
For non-preconditioned equations, the numerical scheme is based on a formulation of the
equations on basis of the energy and the density. The basic tables are used in order to update
the pressure and the temperature after each update of the formulation variables. For
preconditioned equations, the basic variables are enthalpy and pressure, they are used in order
to update the density and temperature.
2. Entropy tables: p(h,s), ρ(h,s), s(h,p), h(s,p)
The entropy tables are used at the inlet/outlet boundary conditions, and are required in order to
calculate the total (static) thermodynamic conditions from the static (total) ones.
3. The (p,T) tables: e(p,T) and ρ(p,T)
These tables are required in order to allow the use of the inlet boundary conditions based on
total pressure and temperature. They are also required by the turbomachinery initial solution
procedure.
4. The viscosity and conductivity tables: μ(e,ρ) and κ(e,ρ)
The viscosity and conductivity can also be interpolated from tables. If these tables are not
present, the other laws available within the user interface can be used.
5. The saturation table
This table contains the liquid and vapour values of all thermodynamic variables along the
saturation line. It is only required if the user activates the dryness fraction output and/or if the
inlet boundary condition based on total enthalpy and dryness fraction is selected.
2.4.3
Integration of Thermodynamic Tables in the Solver
Provided that all the input tables are present, the full functionality of the basic solver is accessible.
All boundary conditions are available, as well as the initial solution procedures. The numerical
schemes are not different, making use of the same acceleration techniques (multigrid, local time
stepping, residual smoothing) providing robust and fast convergence to steady state.
The evaluation of the advective, viscous and artificial dissipation fluxes involves the pressure in
the momentum and energy equations and the temperature in the energy equation. For a perfect gas
both are easily deduced from the equation of state, the conversion being so rapid that only the
pressure and the density are stored and the other variables recalculated from these whenever they
are needed. In the condensable fluid module the density, the pressure, the temperature and the
energy are stored in order to limit the number of interpolations. Only one interpolation is made in
order to deduce the new values of pressure and temperature after the update of the density and the
energy.
The speed of sound is also required. It enters the numerical solution process through the spectral
radius in the time step and in the residual smoothing and artificial dissipation coefficients. It can
either be interpolated from a table or computed from the partial derivatives of the p(e,ρ) table:
The turbulent conductivity calculation is based on the usual relation:
The specific heat at constant pressure can either be constant (the value being provided in the user
interface) or deduced from the specific table.
2.4.4
Selection of the Viscosity, Conductivity, and Specific
Heat
As mentioned above the viscosity and conductivity can be specified in two-dimensional tables. If
it is not the case, the other laws can be used (constant, polynomial expression or user profiles).
Since the complete integration of the condensable fluid module in the user interface is not yet
finished, the selection of these laws is no longer available as soon as a condensable fluid is
chosen.
The way to select these laws is the following:
1. create a perfect gas,
2. enter the desired properties for the viscosity and conductivity,
3. save the corresponding computation,
4. change the fluid type by selecting the condensable fluid.
The same procedure applies to the specific heat at constant pressure, that is used in order to derive
the turbulent conductivity from the turbulent viscosity.
CHAPTER 3.
TURBULENCE MODELS
This chapter provides details of the different turbulence models and the wall functions available in
FINE™/Open with OpenLabs™:
l Linear eddy viscosity turbulence models:
l 1-equation model:
Spalart-Allmaras
Spalart-Allmaras (Extended wall function)
SARC
SARC (Extended wall function)
l 2-equation models:
k-ε (Extended wall function)
k-ε (low Re Yang-Shih, classical)
k-ω (M-SST)
k-ω (M-SST, Extended wall function)
l Nonlinear eddy viscosity turbulence models:
l 2-equation models:
S-BSL-EARSM
S-BSL-EARSM (Extended wall function)
l Modeling flow near the wall
In this section
3.1 Linear Eddy Viscosity Turbulence Models
3.2 Nonlinear Eddy Viscosity Turbulence Models
3.3 Modeling the flow near the wall
3.4 Large Eddy Simulation & Detached Eddy Simulation
29
36
39
44
3.1
LINEAR EDDY VISCOSITY TURBULENCE
MODELS
3.1.1
Spalart-Allmaras
The Spalart-Allmaras turbulence model is a complete one equation turbulence model, which has
become quite popular in the last years because of its robustness and its ability to treat complex
flows. The main advantage of the Spalart-Allmaras model when compared to algebraic models,
like for example the Baldwin-Lomax model, is that the turbulent eddy viscosity field is always
continuous. Its advantage over the k-ε model is mainly its robustness and the lower CPU and
Memory usage.
The principle of this turbulence model is based on the resolution of an additional transport
equation for the eddy viscosity. The equation contains an advective, a diffusive and a source term
and is implemented in a non conservative manner. The implementation is based on the papers of
Spalart and Allmaras (1992) with the improvements described in Ashford and Powell (1996).
The Spalart-Allmaras equation can be written in the following non-conservative form:
where the advection terms are located on the left-hand side, and the diffusion, anti-diffusion,
production, destruction and trip terms are located on the right- hand side. The trip term is
introduced only when the boundary layer transition locations are defined explicitly by the user.
The production term is defined by the following functions:
where d is the distance to nearest wall. In order to prevent divisions by zero in the function fv3, χ
differs from the original one presented
is replaced by max(χ, 0.001). Note that the definition of
in Spalart and Allmaras (1992) in that the function fv2 has been changed and that a new function
fv3 has been introduced so that
does not become negative, see Ashford and Powell (1996).
The destruction term is constructed using the following functions:
In order to prevent overflow in the above equation, r is replaced by min(r, 2). This does not affect
the function fw since it is nearly constant when g is large.
An additional function, ft2, is introduced into both the production and destruction terms in order to
make
a stable solution of the linearized problem.
The trip term is defined using the following function:
where dt is the distance to the nearest trip point, St is the vorticity at the wall at the trip point, and
ΔU is the norm of the difference of velocity between the trip point and the field point where the
trip term is calculated. The term gt is defined by:
where Δx is the spacing along the wall at the trip point.
Finally, the eddy-viscosity itself is obtained from by:
The values of the constants used in the definition of all these functions are the following:
where κ = 0.41 is the Von Karmann constant, and σ = 2/3.
,
3.1.2
SARC
The SARC model results from modifications brought to the Spalart-Allmaras (S-A) model, which
have been introduced by Spalart and Shur (2000), in order to take into account rotation and
curvature effects.
The SARC model differs from the original Spalart-Allmaras model in the production term of the
Spalart-Allmaras eddy viscosity transport equation, which is multiplied by the following function:
Assuming that all variables and their derivatives are defined with respect to the reference frame of
the calculation, which is rotating at a rate Ω, the non-dimensional quantities r* and
are defined
as:
where the strain rate and the vorticity tensors are defined as:
and the remaining variables derived from those two tensors:
and
and D² = 0.5 (S² + ω²)
The model constants are defined as: cr1 = 1.0, cr2 = 12, and cr3 = 1.0.
3.1.3
k-ε Turbulence Models
The k-ε models implemented in the FINE™/Open solver are linear. Two models are available:
l Yang-Shih, low Reynolds number k-ε model (Yang & Shih, 1993).
l Extended wall functions (Hakimi, 1997), which is derived from the Yang-Shih model.
A. Yang-Shih model
Two additional equations, written in their conservative form, are solved for the turbulent kinetic
energy k and the turbulent dissipation ϵ.
where P is the turbulence production, T is the turbulent time scale, E is a term specific to the
and
Yang-
is the
model
Shih
Yap correction. Denoting the trace of a matrix product by Tr, the production term is defined by:
where
turbulent
Reynolds
stress
tensor
is the
and
is the
mean flow strain tensor. In the FINE™/Open solver, the incompressible formulation of the
production is considered, even when compressible flows are simulated. This assumption
since
term
guarantees
production
negative,
becomes
never
that
the
The turbulent time scale T and the term E are defined according to Yang and Shih (1993):
.
The Yap correction is defined as:
The turbulent constants are those given by Launder and Spalding (1974):
,
,
,
and
The turbulent eddy viscosity μt is defined by a Kolmogorov-Prandtl type formula:
The damping function fμ is defined by Yang and Shih (1992) as a function of the Reynolds
number based upon the distance to the wall y:
with
where the constants are given by:
,
,
B. Extended wall functions model
In this model, the turbulent equations for the turbulent kinetic energy, k and the turbulent
dissipation, ϵ are not solved in the first layer of cells next to the wall. The k and ϵ variables are
defined by using wall functions derived from Direct Numerical Simulation (DNS).
This wall function k-ε model differs from the standard one (Launder and Spalding, 1974) since
different wall functions are used for k and ϵ. Moreover, the turbulent time scale and the turbulent
viscosity are defined in the same way as in the Yang-Shih model. This model, which allows the
use of coarser meshes in wall regions, permits a reasonable representation of the flow features.
3.1.4
k-ω (M-SST) Turbulence Model
The Wilcox k-ω turbulence model is another prominent two-equation model as it is more accurate
and more robust near the solid wall. One shortcoming of this model is that it is not able to
accurately predict the asymptotic behavior of the turbulence eddy viscosity. Another shortcoming
is that this model is not able to accurately reproduce the DNS profiles of k and e in the boundary
layer. The worst shortcoming of this model is that its results are extremely sensitive to the small
free stream value of ω in free-shear layer and adverse-pressure-gradient boundary layer flows. In
order to solve these problem, a blended model has been proposed by Menter (1994) that allows to
use the Wilcox k-ω model near solid walls and the standard k-ε model, in a k-ω formulation, in the
free-stream.
In order to blend the k-ω and the k-ε model, the latter is transformed into a k-ω formulation. The
differences between this formulation and the original k-ω model are that an additional cross-
diffusion term appears in the ω-equation and that the modeling constants are different. The
original k-ω model is then multiplied by a function F 1 and the transformed k-ε model by the
function 1-F1 and the corresponding equations of each model are added together. The function F1
is designed to be a value of one in the half inner part of the boundary layer (where the model
behaves like the original model) and decreases to vanish far from the wall.
In this model, the turbulent kinematic viscosity is defined as a function of the turbulent kinetic
energy, k, and the specific dissipation rate of the turbulent frequency, ω, as follows:
The two transport model equations for the k and ω scalar turbulence scales are defined below.
where
with
Notice that this is actually a modification recently brought to the model by Menter et al. (2003),
who replaced vorticity by the strain rate in the eddy-viscosity expression. The limiter on the eddy
viscosity was added, for robustness issues but can be removed.
with
and
with
The standard coefficients for the k and ω by Menter (1994):
,
,
,
,
,
,
, β* = 0.09
,
3.2
NONLINEAR EDDY VISCOSITY
TURBULENCE MODELS
3.2.1
S-BSL-EARSM Model
Explicit Algebraic Reynolds Stress Model (EARSM) can be considered as a subset of nonlinear
constitutive relations in which a part of the higher-order description of physical processes on the
RSM-level is transferred into the two-equation modeling level. As a result, an EARSM is much
less demanding than RSM from the computational standpoint and, at the same time, is capable of
reproducing some important features of turbulence (e.g. its anisotropy in the normal stresses),
which are beyond the capabilities of linear eddy viscosity turbulence models.
The EARSM model implemented in FINE™/Open with OpenLabs™ is the simplified baseline
explicit algebraic Reynolds stress model (S-BSL-EARSM) proposed by Menter et al. (2009),
which is based on the BSL k-ω model of Menter (1994) and allows the inclusion of anisotropic
effects into the turbulence model.
In the S-BSL-EARSM model, the Reynolds-stress tensor is expressed using an effective eddy-
viscosity formulation including a corrective extra-anisotropy tensor
:
(0-1)
where the effective turbulence eddy viscosity is defined as:
(0-2)
and the extra anisotropy tensor terms are defined as:
(0-3)
All the terms and coefficients of the effective turbulence eddy viscosity and the extra anisotropy
tensor are defined as follows:
37
FINE™/Open with OpenLabs™ 7.2 Theory Guide
The turbulence time scale, τ, is
(0-4)
The k and ω equations write:
(0-5)
(0-6)
where the production term is
(0-7)
and the turbulent kinematic viscosity in the k and ω equations is defined as:
(0-8)
The constants β, σk, σω and γ, denoted with the generic symbol ϕ, are defined as:
(0-9)
with the coefficients:
l Inner model constants
l Outer model constants
,
,
,
,
where κ=0.41
The auxiliary blending function F1, designed to blend the model coefficients of the original k-ω
model in boundary layer zones with the transformed k-ϵ model in free-shear layer and free-stream
zones, is defined as:
(0-10)
3.3 MODELING THE FLOW NEAR THE WALL
The wall functions are used to mimic the presence of the walls by reflecting the effect of the steep,
non-linear variations of the flow properties through the turbulent boundary layer. They define the
shear stress and the heat flux on the cell faces lying on solid boundaries as well as the values of
the turbulent variables in the vicinity of the wall.
For the models that do not use wall functions, the profile of the boundary layer is directly inferred
from the input values at the wall. Consequently, particular attention must be paid to the grid
refinement in this region in order to capture the viscous sublayer. A typical value is given by
at the first cell from the wall.
3.3.1
Velocity
A. Smooth walls
For smooth walls, the wall function in the viscous sublayer is given by:
with
, the dimensionless normal distance from the walls and
, the
wall friction velocity directly related to the wall shear stress.
While in the turbulent layer, the wall function becomes:
where κ is the von Karman constant (default value 0.41) and Bo another constant (default value
5.36).
B. Rough walls
Old Method (turb_iRoughModel_=0)
The wall function is given by (no viscous sublayer considered):
where κ is the Von Karman constant (default value 0.41). For rough walls, the constant Bo is
). Otherwise the value of Bo is evolving as
usually zero (when k s
+ > 70 with
presented in below graph.
k0 and d0 are constants asked for each rough wall. The constant k0 is the equivalent roughness
height inputted in the GUI.
where ks is the sand-grain roughness height.
The constant d0 is known as the height of the zero displacement plane, defined by:
if Bo = 0
For small roughness elements, d0 = 0. For high roughness elements, the flow behaves as if the
wall was located at a distance d0 from the real wall position.
New Method (turb_iRoughModel_=1)
Using the old method, seen above, the user has to give the constant Bo as input parameters.
However, the value of the constant Bo is depending on the value of the wall friction velocity uτ.
And the value of Bo will also correct the wall friction velocity uτ. The user has to iterate this
procedure and converge to the desired value of Bo . This is not straightforward and a new
approach has been introduced in the flow solver in order to simplify the computations with
roughness.
For the new method, the wall function is given by (no viscous sublayer considered):
where κ is the Von Karman constant (default value 0.41) and Bo another constant (default value
5.36). Both κ and Bo can be modified by the user in the Boundary Condition page.
McKeon et al. (2004) have shown the ΔU is a function of
with
, as shown in
FIGURE 3.1. The function has a special behavior in the range
. Below
=
3, the flow is considered as smooth and there is no modification of the classical log-law (
=
> 70, the flow is considered as fully rough and ΔU+ shows logarithmic increase with
0). For
increasing
.
FIGURE 3.1
Roughness function
A function is used to interpolate ΔU+ in the flow solver:
where a1=-0.7649, a2=1.9 and
is a constant.
The new method has the advantage that no more iteration has to be done on the constant Bo.
3.3.2
Temperature
Similarly, for isothermal walls, the following laws are considered in the code:
in the viscous sublayer, where Pr is the laminar Prandtl number and:
in the turbulent layer, where
.
The heat flux at the wall is defined as:
A complete description of the available thermal boundary conditions at walls is provided in Solid
Wall Boundary Conditions section.
The "law of the wall" distributions of velocity, temperature and other variables are assumed to prevail
across the boundary layer. They are imposed at the node of a single grid cell for which the user is
advised to check that 20 < y+ < 100. As a result, if the first cell node from the wall is placed too
close, calculation is conducted in the viscous sublayer and the law is no longer valid. Similarly, if the
first node is placed too far away, then a discrepancy may exist between the profiles and their assumed
shape.
3.3.3
Turbulence
A. Standard Wall Function for k-ε model
The values of k and ε in the first inner cell are imposed based on the value of the wall friction
velocity uτ:
where Cμ = 0.09 and κ is the Von Karman constant (default value 0.41).
B. Extended Wall Function for k-ε model
For the extended wall functions model, the wall functions for k and ε are fitted with polynomials
to the DNS data.
C. Extended Wall Function for Spalart-Allmaras and SARC
models
The turbulent working variable
in the first inner cell is imposed based on the
value of the wall friction velocity uτ:
with
,
and κ is the Von Karman constant (default value 0.41).
This relation can be rewritten as:
and holds true in the viscous layer and in the log layer.
D. Extended Wall Function for k-ω (M-SST) model
The value of k in the first inner cell is obtained from the tabulated values already used for the k-ε
model. ω in the first inner cell can be imposed based on the value of the wall friction velocity uτ,
in the sublayer
in the log layer
where β1 = 0.075, Cμ = 0.09 and κ is the Von Karman constant (default value 0.41).
In the intermediate region, ω+ is approximated with the form of interpolation between the viscous
and log layer value:
with
3.4
LARGE EDDY SIMULATION & DETACHED
EDDY SIMULATION
3.4.1
Large Eddy Simulation and Sub-Grid-Scale models
A. Governing equations for LES of a compressible fluid
Written in conservative form for the conservative variables i.e. the density ρ, the momentum ρui
and the total energy E, the governing equations for a compressible flow is written as:
The density ρ, the pressure p and the temperature T are linked by the perfect gas state law:
The total energy E is obtained by
The viscous stress tensor
The heat flux qj is given by
The governing equations for LES are obtained by applying a spatial filter to the Navier-Stokes
equations which separates any flow variable ϕ into a part representing the large scales (low
frequencies -
) and one representing the small scales (high frequency - ϕ′):
where
with GΔ being the kernel filter function and Δ the associated cut-off length-scale.
The filtering operator is assumed to commute with the space and time derivatives. Additionally, it
is convenient to introduce the Favre density-based filtering which, for an arbitrary variable ϕ, is
defined as:
As a consequence, any flow variable is now decomposed as:
where the double prime represents a mass-weighted Sub-Grid-Scale (SGS) fluctuation.
By applying these to the continuity and momentum equations, one gets the filtered equations:
in which
is the viscous stress tensor, which is defined as
where
denotes the kinematic viscosity, and δij denotes the Kronecker delta function. For the
energy equation several variants are possible.
The filtered energy equation thus writes as
B. Smagorinsky model
The Smagorinsky model (Smagorinsky, 1963) is probably the most widely used SGS model and
historically the first to have appeared. It reads:
where Cs is a constant and
is the filter width and is a length scale representing the
sub-grid eddies. From a practical point of view, one often takes the cubic root of the cell volume.
The value of Cs has to be determined and the proposal of Lilly (1967) assuming that the cut-off
lies in the inertial range of the turbulent spectrum. This leads to the constant being written as:
with Ck taken equal to 1.4. This leads to a Cs value to 0.18.
For wall-bounded flows, a somewhat smaller value of 0.1 is usually taken (Deardorff, 1970) as
the model tends to be dissipative and, thus, unduly suppresses the turbulence.
The assumption behind the Smagorinsky model is that the small scales are in equilibrium and that
the energy received from the resolved scales is instantaneously dissipated. Hence, the model,
although very simple and widely used for its simplicity, is purely dissipative and will not account
for back-scatter (the phenomenon of energy being transmitted for the smaller scales to the larger
ones). Another problem is the fact that the model does not vanish when the flow is laminar.
Finally, the model does not provide the correct asymptotic near-wall decay proportional to y+3.
This latter defect can be corrected by introducing a damping function as a multiplier of the
Smagorinsky constant.
The Smagorinsky model including a damping function reads:
where ld is the damping function chosen as
in which d is the distance to the wall and Δx, Δy and Δz represent the edges of the cell in all three
directions.
This choice is motivated by the fact that it does not require to compute a wall shear velocity,
which is required when van Driest damping functions are used, and is thus straightforward to
implement in an unstructured solver.
C. WALE model
The WALE model was proposed by Nicoud and Ducros (1999) and is another eddy-viscosity
model. WALE stands for Wall-Adapted Local Eddy-Viscosity. The model is constructed on an
operator based on the square of the gradient velocity tensor
:
with
.
Two reasons motivate this choice:
l The wish to take into the effects of the strain and rotation rates of the smallest resolved scales;
l The need for an operator able to vanish in the near-wall regions.
Scaling considerations lead Nicoud and Ducros (1999) to propose the following model:
where S ij
is the strain- rate tensor and Δ is the filter width defined as
.
Additionally, the model only uses local information and is invariant to any chance of co-ordinate.
The model should also be able to handle transition.
Nicoud and Ducros (1999) recommend, based on theoretical considerations, a value of C w
between 0.55 and 0.6. Experiments with decaying isotropic turbulence showed the best results for
Cw = 0.5. They also highlighted a dependence of this parameter on the grid size. In practice, a
value of 0.1 is chosen for
.
3.4.2 Detached Eddy Simulation models
DES stands for Detached Eddy Simulation and was originally proposed by Spalart et al. (1997).
In the present work, the DES idea is implemented using the Spalart-Allmaras RANS model
(Spalart et Allmaras, 1992) and the SST model (Menter, 1994) as underlying models. The
concept of DES can readily be extended to any type of RANS models with the methods having
been proved to be insensitive to this choice. A preference for one particular model will therefore
essentially depends on the practionner wishes and tastes. A recommendation coming out of the
ATAAC project (EC FP7) is to prefer a two-equation models such as the SST model as the
turbulence quantities such the turbulent energy and the turbulent dissipation are readily available
and this is thus much easier to work in case of block-coupling between steady RANS and
unsteady regions with synthetic turbulence being used to provide fluctuating content.
A. DES97 (natural DES)
DES97 was originally proposed by Spalart et al. (1997). The underlying idea is to compute the
attached boundary layer with RANS models where those are performing best while the detached
content is simulated using LES. This is achieved by defining a new turbulent length scale defined
as:
where d w represents the distance to the wall, C DES is a constant taken equal to 0.65 and Δ
represents a filter width which is defined as:
where Δx, Δy and Δz represent the edges of the cell.
If the Spalart-Allmaras RANS model is used, the implementation is simply achieved by replacing
the wall distance dw by the DES length scale lDES wherever dw appears.
The implementation of lRES as described here above in the Spalart-Allmaras model leads to the
problem that, in certain circumstances, certain wall- damping terms may become active and
DES97 may misinterpret this as proximity of a wall and thus reduce excessively the turbulent
eddy viscosity. This situation however only occurs at relatively low Reynolds and/or with very
fine grid.
The extension to other underlying models has been proposed by Travin et al (2000) and reads:
For the particular case of the SST model, lRANS and lRES are respectively given by:
where CDES is defined as:
in which F1 is a blending function used in the SST model,
and
are constant whose values have been obtained through calibration by
reference to the case of isotropic turbulence.
A second shortcoming of DES97 is related to grid ambiguities and has been first identified by
Menter and Kuntz (2004) who proposed a solution for the DES-SST model. A more general
proposal was then made by Spalart et al (2006) and is described in the next section.
B. Delayed DES
In the previous section, an abnormal behavior of DES97 related to grid ambiguities was
mentioned. The present section explains this in more details and report the remedy proposed by
Spalart et al (2006). This is due to the fact that the grid spacing parallel to the wall becomes much
smaller than the boundary layer thickness, through grid refinement or boundary layer thickening.
The DES length scale follows then the LES branch of DES. Unfortunately, the resolved content
may not have replaced the modeled content due to the grid/time step not fine enough to support
LES-type instabilities and/or delay its generation. The resulting depleted stresses thus reduce the
skin friction, potentially leading to a premature separation (Grid Induced Separation).
Spalart et al (2006) propose to redefine, for the Spalart-Allmaras model, the DES length scale as:
fd = 0 yields RANS mode while fd = 1 returns DES97. fd is defined as:
where the parameter rd is given by:
The subscript d stands for "delayed". νt is the turbulent eddy-viscosity and ν is the molecular
viscosity, Uij is the velocity gradient. The function fd is designed so that it is equal to 1 in LES
regions where rd << 1, and 0 elsewhere. This approach is termed Delayed DES (DDES).
The constant C d 1 and C d 2 involved in the f d function depend on the background RANS
turbulence model used for the DDES computations. For the SA RANS turbulence model, one has
, Spalart et al (2006). For the SST RANS turbulence
and
model, these constants are
and
, Griskevitch et al (2013).
The extension to other RANS models, such as the SST model, is straightforward as it consists in
multiplying by fd the term constituting the difference between RANS and DES, as shown here
above for the Spalart-Allmaras model. A more general formulation is thus:
C.
Improved Delayed DES
Following DDES, another variation was developed by Shur et al (2008) with the aim of
combining both the capabilities of DDES  and Wall- Modeled LES
(WMLES), in an attempt to resolve the issue of mismatch between the modeled and resolved log
layer which was first identified by Nikitin et al (2000).
The method was developed in the course of DESider (Haase et al, 2009) and was named as
Improved DDES (IDDES) . In their original paper, Shur et al (2008) claim that IDDES
significantly broadens the application area of (D)DES by permitting the activation of RANS and
LES in different flow regions.
the implementation of IDDES is
Provided that DDES is already available in a solver,
straightforward, as it only requires embedding a new length scale in place of lDDES. This new
length-scale is defined as:
This guarantees that, for simulations with inflow turbulent content, rdt << 1, and fdt is close to 1
and fd is equal to fB so that lIDDES reduces to an alternative form of lDDES defined as:
Otherwise, fe becomes zero and lIDDES reduces to:
Coming back to the description of lIDDES, the definition of lLES is as follows:
where Shur et al (2008) propose a new definition of which should be more physically justified.
is an empirical constant set to 0.15 by Shur et al (2008) based on a wall-resolved LES of a
channel flow,
is the wall distance,
and
is the grid step
in the wall normal direction.
The function
is defined as
with
and
The constants C dt 1 and C dt 2 involved in the fdt function depend on the background RANS
turbulence model used for the IDDES computations. For the SA RANS turbulence model,
(Spalart et al (2006)). For the SST RANS turbulence model, these
and
constants are
and
according to Griskevitch et al (2013).
The other function, fe , aims at preventing an excessive reduction of the RANS Reynolds stresses
as caused by the interaction of RANS and LES regions in the vicinity of their interface and is
instrumental in combating the log-layer mismatch. It is defined in the following way:
with
where
and
The function fe2 equals to
with
and
.
cl and ct are additional constants whose values depend on the background RANS model.
.
For SA-IDDES,
and
CHAPTER 4.
CONJUGATE HEAT TRANSFER
This chapter describes the Conjugate Heat Transfer model implemented within FINE™/Open with
OpenLabs™:
In this section
4.1 Simulation of Conduction
4.2 Thermal Coupling Between the Solid and Fluid Blocks
4.3 Full Non-Matching Thermal Connections
55
56
57
4.1
SIMULATION OF CONDUCTION
For steady state computations, the time marching (pseudo time stepping) method is applied in the
FINE™/Open flow solver. The governing energy equation in solid blocks is:
where:
is the pseudo time (s),
is the density of the solid block (
),
is the specific heat capacity of the solid block (
is the thermal conductivity of the solid block (
),
),
T is the temperature (K).
Considering the density and the specific heat capacity of the solid as constant, the equation above
can be written as:
with
.
4.1.1
Time discretization
The general time discretization scheme of the energy equation in solid blocks can be written as:
is an expert parameter (solidImpl_gamma_ ) defining the time discretization scheme.
l When =0, the time explicit scheme is obtained. For 1 dimensional problem, a linear von
Neumann stability analysis shows that the explicit scheme is stable under the condition:
l When =0.5, the time semi-implicit scheme of Crank and Nicolson (1947) is obtained. This
scheme is unconditionally stable (no restriction condition on the pseudo time step applied) and
is second order in time.
l When
=1, the unconditionally stable time implicit scheme (first order Euler method) is
obtained.
4.1.2
Space discretization
After space discretization, the time discretization yields to a system of equations to obtain the
temperature at the cell centers at the pseudo time n+1:
A is the matrix of the system of equations. The dimension of the system is the number of cells of
the solid block. b is the source term.
4.2
THERMAL COUPLING BETWEEN THE SOLID
AND FLUID BLOCKS
The fluid-solid interfaces constitute a new type of boundary condition, referred to as "thermal
connections", along which the heatflux and temperature are imposed to be equal.
The calculation is performed simultaneously on the fluid and solid blocks. The thermal coupling is
applied each time the boundary conditions are applied. Note that no particular procedure is
required in order to initiate the calculation. The full multigrid strategy allows to rapidly establish
an overall temperature distribution in the domain.
On both solid and fluid sides, the thermal boundary condition imposes a temperature profile. This
profile is iteratively recalculated in order to ensure equality of the heatfluxes calculated on both
sides:
hf(Tw-Tf)=-hs(Tw-Ts)
where hf and hs are the heat transfer coefficients and Tf and Ts are the inner temperatures. The
heat transfer coefficients are calculated in a simple way, assuming a sufficient orthogonality of the
mesh:
where κ is the local conductivity and Δy is the distance between the inner cell centre (where the
temperature of Tf and Ts is taken) and the wall.
4.3
FULL NON-MATCHING THERMAL
CONNECTIONS
The Full Non-matching algorithm is available in the Conjugate Heat Transfer (CHT) module. It is
used to calculate the interface temperature and heat flux of the full non-matching boundaries. In
case that the patches are not fully connected (as shown below), the remaining part of the patch
will use the boundary condition defined through the FINE™/Open GUI.
CHAPTER 5.
BOUNDARY CONDITIONS
This chapter describes all the theories related to the boundary conditions available in the FINE™/Open
solver.
In this section
5.1 Inlet Boundary Conditions
5.2 Outlet Boundary Conditions
5.3 Solid Wall Boundary Conditions
5.4 Far-field Boundary Condition
59
66
68
71
5.1
INLET BOUNDARY CONDITIONS
5.1.1
Cartesian Inlet Boundary Conditions
A. Static Quantities Imposed (Subsonic)
The complete absolute velocity vector followed by the static temperature on the boundary are
specified. Several possibilities exist:
l the cartesian velocity components are specified;
l the Mach number and the flow angles α and γ are specified:
l the magnitude of the velocity is specified. The velocity direction is normal to the inlet.
The static pressure is extrapolated from the interior. Using subscript 0 for the boundary, and
subscript 1 for the first internal cell one has:
which allows calculation of all the primitive variables on the boundary.
For incompressible flows, the user can only specify the cartesian velocity components, since the
Mach number is meaningless.
B. Total Quantities Imposed (Subsonic)
Magnitude of Absolute Velocity extrapolated
The user first specifies a direction (in the form of a vector) that corresponds to the direction of the
absolute velocity vector. Note that this vector does not have to be a unit vector. The x,y,z
components of the direction vector are given. For example, entering the direction (0,1,1) imposes
that the y- and z-component of the absolute velocity vector at inlet should be equal. In other
words, the flow enters at an angle of 45 degrees between z- and y-direction, whereas the angle
between z- and x-direction is 0 degrees.
The absolute total pressure and the absolute total temperature on the inlet boundary are also
specified. The magnitude of the absolute velocity is extrapolated from the interior field.
where
represents the absolute velocity.
Mach Number extrapolated
The user first specifies a direction (in the form of a vector) that corresponds to the direction of the
absolute velocity vector. Note that this vector does not have to be a unit vector. The x,y,z
components of the direction vector are given. For example, entering the direction (0,1,1) imposes
that the y- and z-component of the absolute velocity vector at inlet should be equal. In other
words, the flow enters at an angle of 45 degrees between z- and y-direction, whereas the angle
between z- and x-direction is 0 degrees.
The absolute total pressure and the absolute total temperature on the inlet boundary are also
specified. The absolute Mach number is extrapolated from the interior field (only available for
compressible fluid):
,
Velocity Normal to Inlet (V extrapolated)
The absolute total pressure and the absolute total temperature on the inlet boundary are specified.
The orientation of the velocity will be set to be normal to the inlet surface. The magnitude of the
absolute velocity is extrapolated from the interior field.
where
represents the absolute velocity at the inlet,
is the velocity norm inside the domain
and
is the normal unit vector pointing outside of the domain.
C. Mass flow, Direction of Absolute Velocity Vector and
Static Temperature Imposed (Subsonic)
This boundary condition imposes a supplied value of the mass flow through a specified control
surface. The control surface is defined by grouping several patches into the same group. In
addition to the mass flow, the direction of the velocity vector and the static temperature are also
imposed.
l the direction of the absolute velocity vector is imposed in the Cartesian coordinate system
.
D.
Imposing the Complete Flow Conditions (Supersonic)
The flow at inlet is completely specified by giving the static pressure and static temperature. This
boundary condition is only available for a compressible fluid. Several possibilities exist:
l the cartesianal velocity components are specified;
l the Mach number and the flow angles α and γ are specified:
5.1.2
Cylindrical Inlet Boundary Conditions
A. Static Quantities Imposed (Subsonic)
The complete absolute velocity vector and the static temperature on the boundary are specified.
Several possibilities exist:
l the magnitude of the velocity and the flow angles α and γ are specified:
l the magnitude of the velocity and other flow angles δ and ε are specified:
with v m the meridional velocity
. This option has been designed to
allow radial inlet with zero axial velocities,
l the cylindrical velocity components are specified.
The static pressure is extrapolated from the interior, which allows calculation of all the primitive
variables on the boundary.
These conditions can also be used for incompressible flows.
B. Total Quantities Imposed (Subsonic)
Several variants are available based on the specification of flow angles or velocity components.
Absolute flow angles from axial direction
The user specifies two flow angles (of the absolute flow) at the boundary, α and γ, which are
defined by the magnitude of the velocity and given in radians.
The absolute total pressure and the absolute total temperature on the inlet boundary are also
specified and imposed.
Two variants are available depending on the value that is extrapolated.
l the modulus of the absolute velocity vector is obtained, by extrapolation, from the interior
field.
l the axial velocity component is extrapolated:
Note that it is assumed that the angular velocity vector is in the z-direction,
and the z-axis is therefore the axial direction. Also note that, as a result of this equation the
absolute and relative axial velocity component are equal.
Velocity direction
The user first specifies a direction (in the form of a vector) that corresponds to the direction of the
absolute velocity vector. Note that this vector does not have to be a unit vector. The r,θ,z
components of the direction vector are given. For example, if the user enters the direction (0,1,1)
the user imposes that the θ- and z-components of the absolute velocity vector at inlet are equal and
that the radial velocity is zero.
The absolute total pressure and the absolute total temperature on the inlet boundary are also
specified. These values will be imposed.
The modulus of the absolute velocity vector is extrapolated, from the interior field.
Tangential velocity and meridional angle
Imposing the tangential velocity at the inlet is useful for turbomachinery configurations with high
absolute tangential velocities.
The user specifies the direction of the radial and axial velocity, together with the magnitude of the
tangential velocity in [m/s]. The absolute total pressure and the absolute total temperature on the
inlet boundary are also specified. The application of the boundary condition can be described as
follows:
l The meridional velocity is extrapolated from the interior of the computational domain
l The velocity magnitude is deduced from the input of the tangential velocity
l The static pressure and temperature are computed from the imposed total values
l The radial and axial velocities are imposed in the appropriate direction
l The velocity components in the Cartesian frame of reference are deduced
Relative flow angles from axial direction
This procedure is only available in case total conditions and flow angles are imposed. Note also
that both flow angles and total conditions are then treated in the relative mode.
The user specifies two relative flow angles (in radians) at the boundary, β and ϒ:
The relative total pressure and the relative total temperature on the inlet boundary need also to be
specified.
In addition to that the extrapolation of vz will be used
Relative velocity direction
The user first specifies a direction (in the form of a vector) that corresponds to the direction of the
relative velocity vector. Note that this vector does not have to be a unit vector. The r,θ,z
components of the direction vector are given. For example, if the user enters the direction (0,1,1)
the user imposes that the θ- and z-components of the relative velocity vector at inlet are equal and
that the radial velocity is zero.
The relative total pressure and the relative total temperature on the inlet boundary are also
specified. These values will be imposed.
The modulus of the relative velocity vector is extrapolated from the interior field in the same way
as the magnitude of the absolute velocity
where
represents the relative velocity.
Velocity normal to inlet
The absolute total pressure and the absolute total temperature on the inlet boundary are specified.
The orientation of the velocity will be set to be normal to the inlet surface. The magnitude of the
absolute velocity is extrapolated from the interior field.
where
represents the absolute velocity at the inlet,
is the velocity norm inside the domain
and
is the normal unit vector pointing outside of the domain.
C. Mass Flow Imposed (Subsonic)
This boundary condition specifies the value of the mass flow through a given control surface. The
control surface is defined by grouping several patches into the same group. In addition to the mass
flow the direction of the velocity vector and the static temperature are imposed.
Two variants are available:
l the swirl can be imposed, as well as the direction of the velocity vector in the meridional plane
(
,
,
).
l the direction of the absolute velocity vector can be imposed (
,
,
).
D. Total Enthalpy & Dryness Fraction Imposed (Subsonic -
Condensable Gas)
In cases where the inlet thermodynamic state is located on the saturation curve or inside the
biphasic zone, traditional boundary conditions based on total temperature and total pressure are
not sufficient, as pressure and temperature become interdependent. An additional information is
required, which is the dryness fraction.
The boundary condition proposed under the FINE™/Open GUI is based on the absolute total
enthalpy and the dryness fraction. The velocity direction is also specified, either by means of two
flow angles (from axial direction) or of velocity direction vectors.
The implementation of the boundary condition is based on extrapolation of the static pressure,
which permits to evaluate the saturated liquid and gas values of the density and enthalpy. The
dryness fraction permits to deduce the values of the local static enthalpy and density. The other
boundary conditions are then used to calculate the velocity vector.
E.
Imposing the Complete Flow Conditions (Compressible,
Supersonic)
Static quantities
The flow at inlet is completely specified, by giving the static pressure, static temperature and the
three absolute cylindrical velocity components.
Total quantities
Instead of specifying static pressure, static temperature and the three absolute velocity
components, one can also specify absolute total pressure, absolute total temperature, absolute
Mach number and two flow angles α, β defined as:
,
with the angles given in radians.
5.1.3
Turbulent Inlet Boundary Conditions
For a turbulent calculation with the turbulence model, the turbulent inlet boundary conditions
must be specified. It is important to note that the level of turbulence quantities (i.e. turbulence
intensity, μ t, k, ε) specified at the inlet boundary can have a strong effect on the flow-field
prediction for quantities like the total pressure, velocity profiles, flow angles, total temperature etc.
5.2
OUTLET BOUNDARY CONDITIONS
5.2.1
Outlet Boundary Conditions for Subsonic Flow
A. Pressure Imposed
Static Pressure Imposed
The static pressure at the outlet boundary is specified. The remaining dependent variables on the
outlet boundary are obtained from the interior field through extrapolation.
The default extrapolation is a zero order extrapolation of the static temperature and the absolute
velocity.
The backflow treatment can be activated or not. The purpose of the backflow treatment is to avoid
flow re-entry into the domain at the outlet. In case where the flow partially re-enters the domain
through the exit boundary, a slip wall boundary condition is locally applied to velocity, while
pressure is extrapolated.
Radial Equilibrium
The static pressure in the outlet section is assumed to be uniform in the tangential direction and to
vary in radial direction according to:
.
The user specifies the static pressure at a specific radius, followed by that radius and the radial
direction.
The pressure distribution on the outlet section is then found by integrating this equation with
pitchwise averaged values of vθ and r.
The other variables are extrapolated as above.
Average Static Pressure Imposed
In some cases, an uniform pressure can not be imposed on the outlet. The average static pressure
imposed boundary condition allows imposing an averaged static pressure.
The pressure profile is obtained by extrapolation from the interior field and it is translated to
ensure that the computed averaged pressure on the outlet area is the target averaged pressure
specified by the user. This translated profile is then the imposed pressure profile.
The other variables are extrapolated as in Pressure imposed section.
B. Mass Flow Imposed
Pressure adaptation
This boundary condition is an adaptation of the "uniform static pressure imposed" and "static
pressure imposed with radial equilibrium" boundary conditions.
The only difference is that an automatic procedure is included that introduces a variation of the
imposed exit pressure at each iteration of the calculation. The pressure is iteratively updated in
order to reach the imposed mass flow at convergence. The successive pressure modifications are
calculated according to:
,
where Lref is the characteristic length defined in the Flow Model page Tref is the fluid reference
temperature controled by the expert parameter TRefBCpAdapt_. rgas is the universal gas constant,
which is deduced from fluid properties. The term RELAXP introduces an under-relaxation of the
successive modifications of the exit pressure. The initial value of the exit pressure is provided by
the user. When radial equilibrium is used, the initial value of the exit pressure is imposed at
midspan.
Velocity scaling
This boundary condition fixes the mass flow at a given control surface by scaling the velocity
vectors on this surface. The other variables are extrapolated following the system of options
exposed above.
Given that the pressure is also extrapolated with this condition, it is imperative that the inlet
boundary condition fixes the pressure through the total pressure.
Fixing the mass flow is not as robust as to impose the pressure and this is particularly sensitive
with full-multigrid. A initial pressure is thus requested as input and is imposed during the full-
multigrid process. The user can choose if the constant pressure is used or not during the FMG
initialisation. If the constant pressure is used, the mass flow computed at outlet is not exactly the
target mass flow during the computation on the coarse grids.
This option is not recommended in case significant backflow is detected along the exit. The
previous option (exit pressure adaptation) is then recommended.
5.2.2 Outlet Boundary Conditions for Supersonic Flow
This condition is to be used in case of supersonic outflow and is only valid for compressible
fluids.
The dependent variables at the outlet are extrapolated from the interior through first- order
extrapolation.
5.2.3
Treatment of Backflow at Outlet
The option for the treatment of backflow can be activated by pressing the corresponding button in
the FINE™/Open GUI.
The treatment is local, i.e. it is applied only to boundary faces for which the flow re-enters the
domain. It consists in the following parts:
l extrapolation of pressure
l imposition of velocity in the same way as a slip (Euler) wall condition, see Euler Walls section.
This treatment better represents the physics of the flow.
5.3
SOLID WALL BOUNDARY CONDITIONS
5.3.1
Euler Walls
For Euler walls the velocity must be tangential to the wall.
To obtain the velocity vector on the wall, the velocity is first extrapolated from the interior with
zero order extrapolation:
where subscripts w,1 denote the wall and the first inner cell, respectively.
The tangential component of the extrapolated velocity vector is:
where
is the normal to the wall.
The wall density and pressure are obtained by zero order extrapolation from the interior:
5.3.2 Navier-Stokes Walls
A. Adiabatic Walls
The velocity vector on the wall vanishes. If the cylindrical boundary condition is used, the angular
velocity of the wall (in the absolute frame of reference) must be specified.
The velocity relative to the wall should be zero, leading to:
where subscripts s, w refer to the system and the wall, respectively.
Pressure is extrapolated from the interior, so that the pressure gradient is equal to zero.
The temperature on the wall is also extrapolated from the interior:
.
.
The density is derived from pressure and temperature through the appropriate relation, depending
on the type of gas.
B.
Isothermal Walls
The implementation of this boundary condition is very similar to the adiabatic Navier-Stokes wall.
The only difference is in the determination of the wall temperature, which is fixed to the specified
temperature in the this boundary condition.
For the cylindrical isothermal walls, the angular velocity of the wall must be specified.
Pressure is determined as in the adiabatic condition, and the density derived from pressure and
temperature through the appropriate relation, depending on the type of gas.
C. Wall with Imposed Heat Flux
The implementation of this boundary condition is very similar to the previous ones. For this
condition the temperature is determined from the imposed heat flux (W/m²).
The pressure is determined as in the adiabatic condition and the density derived from pressure and
temperature through the appropriate relation, depending on the type of gas.
D. Wall with Imposed Heat Transfer Coefficient
The implementation of this boundary condition is very similar to the previous ones. For this
condition the temperature is determined from the imposed heat transfer coefficient h (W/m²K):
where d is the distance between the first inner cell and the wall.
The pressure is determined as in the adiabatic condition and the density derived from pressure and
temperature through the appropriate relation, depending on the type of gas.
E. Turbulent Wall Boundary Conditions
For a turbulent calculation with the turbulence model, the turbulent wall boundary conditions
need to be treated.
Spalart-Allmaras model and Simplified SARC
When the Spalart-Allmaras model or simplified SARC model is selected, the turbulent working
variable in the solid wall.
k-ε Models
The values of kw and εw are imposed at the boundary for the Yang-Shih model, while for the
High Reynolds number models, they are imposed in the first inner cell.
M-SST k-ω models
When the M-SST k-ω models are selected, the boundary condition on solid wall is the following
one:
(0-1)
(0-2)
with C = 60.
5.4
FAR-FIELD BOUNDARY CONDITION
For compressible flows, far-field boundary condition uses Riemann invariants that are defined as:
where
are the Riemann variables associated with the direction
and c is the local speed of
sound.
For subsonic inflow,
corresponds to a positive, incoming characteristic.
is then obtained
from the free stream values:
where
is the free stream velocity and
the free stream speed of sound.
, on the other hand, corresponds to an outgoing characteristic and must be estimated from
inside the computational domain:
where subscript 1 refers to values from the first inner cell.
The normal velocity and the local speed of sound can now be obtained on the boundary by
adding and subtracting both Riemann variables
and
:
The entropy on the boundary is set to the free stream entropy. All the flow variables can then be
obtained.
Corresponding formulas hold for a subsonic outflow with the difference that
and the
boundary entropy are obtained from interior values.
For supersonic flows, both Riemann variables and the entropy are obtained from free stream
values for inflow and interior values for outflow.
For preconditioning computation, the same principle is used with modified invariants defined as:
where
The free stream variables of static pressure, static temperature and the three velocity components
are specified by the user in the boundary condition file.
For a turbulent calculation with a two-equation model, the k and ε values on the boundary are set
to their free stream values (inflow) or extrapolated from the interior (outflow).
CHAPTER 6.
NUMERICAL SCHEME
This chapter describes the basic solution theory in the FINE™/Open solver.
In this section
6.1 Discretisation and solution theory
6.2 Preconditioning
6.3 Time Configuration
74
97
104
6.1
DISCRETISATION AND SOLUTION THEORY
6.1.1
Spatial Discretization
The discretization in space is based on a cell centered finite volume approach. Let us write the
conservative finite-volume formulation explicitly.
Considering a discrete volume Ω encompassed by the surface S, the integral conservation laws are
written:
where
contains here the inviscid and viscous part of the fluxes:
where
and
are the inviscid and viscous part of the fluxes respectively. These equations
should be solved over control volumes Ω J . Finite-volume discretization gives the following
discrete form:
where
* is the numerical flux, sides refers to the external sides of the control cell ΩJ and
is
the non-unitary normal vector to the considered side.
A. Viscous Fluxes
The viscous fluxes are determined in a purely central way. As they contain gradients, gradients
must be evaluated on the cell faces. This is done by applying Gauss' theorem over a volume
encompassing the considered face:
Applying a finite volume discretization and considering stationary control volumes, the relation
becomes:
, or
The theorem is applied over a diamond control volume formed by the face vertices and its
neighboring cell centers as opposite summits.
FIGURE 6.1
Diamond control volume approach for gradient computation on faces
The diamond control volume method requires knowledge of the flow quantities at the cell
vertices. The choice of an appropriate interpolation method has to be made in order to ensure
accurate transfer from cell centers to vertices. This gives the following expression for a quantity Q
to be interpolated in a vertex p surrounded by n cells:
A linearity- preserving interpolation, based on the pseudo- Laplacian formula of Holmes and
Connell (1989), is used. The value of Q at vertex p is obtained by the above formula, where the
weighting functions ωi are defined by:
where Δxi, Δyi and Δzi are the three coordinates differences between cell i and vertex p (Δxi = xi -
x p ,...). The weighting coefficients λ x , λ y and λ z are computed by assuming that above
interpolation should be exact for a linear evolution of Q. Hence we can write:
Rewriting interpolated equation under the following form:
and injecting above equation in this formula, we obtain:
For linear functions, this relation should remain valid for any value of the derivatives. Since there
are three unknowns determining ωi, let us choose three particular sets of derivatives, so that we
obtain the following three equations from above relation, where ωi is replaced by its definition
involving the unknowns λx, λy and λz:
This system of three equation with three unknowns λx, λy and λz can easily be solved since only a
symmetric 3x3 matrix must be inverted for each vertex. Moreover, this needs to be done only
once during the flow calculation process because, as seen in this expression , the unknown
weighting coefficients do not depend on the solution but only on vertex and cell center
coordinates.
B.
Inviscid Fluxes
The following form is used to express the inviscid numerical flux across a face k bounded by two
cells L and R:
where the first term on the right hand side corresponds to a purely central evaluation of the
inviscid numerical flux vector, and the second term dk is called the numerical dissipation term. It
may be an artificial dissipation, used in combination with central schemes, or the dissipation
associated with upwind schemes.
FIGURE 6.2
Notations for the inviscid flux formulation
Alternatively, instead of averaging the fluxes, a flux based on the averaged unknowns can be
formulated:
In the FINE™/Open solver, the flux averaging formulation is used for internal faces, and the
denotes the unit normal
solution-averaging formulation is used on boundaries. Notice that since
vector to face k throughout the whole manuscript, we should multiply the above expressions by
the face area in order to recover the numerical flux. Hence we have:
where ΔSk is the area of face k.
The central scheme is the default scheme in the FINE™/Open solver. Roe upwind scheme is also
available.
Central Scheme
In the central scheme, the scalar artificial dissipation term in equation is formulated by Jameson,
Schmidt and Turkel (1981) as a blend of second and fourth-order differences of the conservative
variables:
where δUk is the solution first-order differences in face k, δ²UL and δ²UR are the second-order
variations in the left and right cell centers. The second and fourth-order scalar coefficients in faces
are given by:
and the fourth-order coefficients in cells (
,
) relative to one local direction are obtained
by arithmetic averaging the fourth-order coefficients on opposite sides, themselves obtained by
arithmetic averaging the fourth-order coefficients on their constitutive faces, as shown in FIGURE
6.3
FIGURE 6.3
Calculation of the fourth coefficient in cells
The term
is the spectral radius, i.e. the maximum eigenvalue of the flux Jacobian projected in
the direction normal to face k. Using hexahedral control volumes, three local directions, namely ξ,
on face k is then
η and ζ can be defined for each cell, see FIGURE 6.3. The spectral radius
obtained by arithmetic averaging the spectral radii in its neighboring cells, evaluated in their local
direction corresponding to the face. For the example of FIGURE 6.3, we have:
where
, cL and
, cR are the velocity vector and the speed of sound in the left and right cells
respectively, and
,
are the unit normal vectors calculated at the center of the left and right
cells, in their respective local directions corresponding to face k, see FIGURE 6.2.
On high aspect ratio meshes, the dissipation in the streamwise direction may become very low.
Increasing it may improve the robustness and the convergence rate, although perhaps at the
expense of a lower accuracy in such cells. As seen above, before being transferred to faces, three
spectral radii are evaluated in cell centers, in the directions corresponding to their local frame of
reference. Martinelli (1987) has defined modified spectral radii in each direction by taking into
account contributions from the two other directions. For instance, the modified spectral radius in
local direction ξ for cell L is given by:
where σ is the Martinelli coefficient, whose default value is 0.5.
The non-dimensional coefficients νL, νR are pressure and temperature variations (depending on
the value for the expert parameter spc_TswitchInArtDissip_), which act as sensors to activate the
second-order dissipation in regions of strong gradients, e.g. shocks, and to deactivate it elsewhere.
For instance, we will have for cell L:
where pL-1 is obtained by arithmetic averaging the pressure in all the cells located on the left side
of cell L in the considered direction. Similarly, pL+1 is obtained by averaging the pressure in all
the cells located on the right side of cell L. Notice that the size and shape of these cells are not
taken into account, see FIGURE 6.4. This is, however, not important since the pressure switches
, only
are simply indicators of zones of large gradients. Also note that in our formulation of
the pressure switches of the neighboring cells of face k are involved whereas in the classic
Jameson formulation, four switches are used, namely those of the face neighboring cells as well as
of these cells' neighbours. However, this is unsuitable in the context of unstructured adapted
meshes since each neighboring cell can itself have one, two, three or four neighbours, whose
are user-defined coefficients, usually
identification is not straightforward. Finally,
and
equal to 1.0 and 0.1 respectively. They correspond to the non-interfaced expert parameters spc_
artDiss2ndCoef_ and spc_artDiss4thCoef_.
FIGURE 6.4
Pressure switches (cell L)
Central matrix scheme
Starting from the standard scalar scheme of Jameson-Schmidt-Turkel (JST), a matrix dissipation
scheme can be easily constructed by substituting the spectral radius with the absolute value of the
flux jacobian:
With the second and fourth dissipation coefficients given now by:
The pressure switch has the same definition as for the central scalar scheme.
Now, the dissipative terms for each equations are scaled by the appropriate eigenvalues of the flux
Jacobian of the system, rather than the spectral radius.
The central matrix dissipation term is constructed as the upwind scheme dissipation term. The
advantage of this formulation is that one reduces the computational cost of the numerical scheme.
One has
where L-1 is the matrix of the left eigenvectors of the jacobian matrix of the Euler system in the
primitive variables, whereas P is the matrix of the right eigenvectors of the jacobian matrix of the
Euler equations expressed in term of conserved variables. The matrix Λ is the diagonal matrix of
the eigenvalues of the system. The differences δ V k are expressed in terms of the primitive
variables (ρ, u , v , w , p ). The matrix |Λ| is the diagonal matrix of the absolute value of the
eigenvalues (λ)i=1,5 with:
Near stagnation points and sonic points, some of the Jacobian eigenvalues can become very small
and would lead to numerical difficulties. This can be avoided by introducing a fix on the
eigenvalues of the absolute Jacobian:
Where σ is the spectral radius of the jacobian matrix. The parameters merkle_matdisEntrFx_
and hakimi_matdisEntrFx_ (to be applied when using Merkle and Hakimi preconditionner,
respectively) are controlling the entropy fixes. These expert parameters are vectors of two
components. The first component corresponds to Vl, and the second to Vn. The default values are
(0.1 , 0.1) for merkle_matdisEntrFx_, and (0.3 , 0.3) for hakimi_matdisEntrFx_.
Note that
incompressible Hakimi version is limited to isothermal flows.
the Hakimi
low- Mach version is not compatible with CPU Booster, and that
the
Upwind Schemes
Roe type upwind scheme is also available in the FINE™/Open solver.
First Order Roe Scheme
In the FINE™/Open solver, two expressions of the dissipation term dk are available:
l the "standard" dissipation.
l the "isenthalpic" dissipation that allows the scheme to admit constant total enthalpy while
dealing with steady flows. This property is satisfied by expressing the dissipation term dk using
enthalpy instead of total energy in the energy equation.
The expert parameter upw_ dissipEnthalpy_ controls the use of the standard or isenthalpic
dissipation. The default option is the standard dissipation.
The parameter upw_dissip_ext_ controls the calculation of the dissipation at the inlet and outlet
boundaries. If it is 1, the dissipation is calculated at this boundaries, if 0 the dissipation is not
the dissipation is calculated at inlet- outlet boundaries. For
computed. Actually by default,
turbomachinery applications, we advise to not calculate the dissipation at inlet-outlet boundary.
Indeed, it was found in this case the mass flow errors are greatly reduced.
"Standard" Dissipation
In the upwind scheme, the dissipation term dk on a given face k is expressed as follows:
where L-1 is the matrix of the left eigenvectors of the Jacobian matrix of the Euler system in the
primitive variables, whereas P is the matrix of the right eigenvectors of the Jacobian matrix of the
Euler system in the conservative variables, described in e.g. Hirsch, 1990. |Λ| is the diagonal
matrix of the eigenvalues of the system. In order to avoid unphysical solutions such expansion
shocks, an entropy fix is used. The absolute values of the eigenvalues are limited as follows:
where
for
the linear
field (the
characteristic variables that propagate with speed
) and
for the non linear field, EntrFx_ are two user-defined parameters that generally vary between
0.001 and 0.3. In subsonic and transonic cases, small values suffice (EntrFx_ = 0.001). For flow
simulations in high-speed regime and when shocks are aligned with the mesh (especially for
detached shock), it is advised to choose higher values for these parameters (EntrFx_ = 0.3).
The expert parameter EntrFx_ is a vector of two components, the first component is applied to the
linear field, and the second component is applied to the non-linear field. By default, the two
components are set to 0.01.
δVk is the first-order difference in face k of the primitive variables, namely density, velocity and
pressure:
where L and R denote the upwind and downwind cells respectively. The terms in the matrices are
evaluated on face k by Roe averaging:
,
,
The upwind scheme is presently only available for compressible flows when not using the
preconditioning method for low-Mach flows.
"Isenthalpic" Dissipation
In the case of steady flows, the total enthalpy H is constant. The standard Roe scheme with the
dissipation term dk does not necessary satisfy this property. This may be remedied by calculating
the dissipation term dk in the same way as the standard Roe scheme but according to the modified
state vector:
Therefore the dissipation term dk reads:
where R is the matrix of the right eigenvectors of the Jacobian matrix of the Euler system in the
new set of variables. |Λ| is the diagonal matrix of the absolute values of the eigenvalues of the
system. As for the standard discretization, an entropy fix is used in order to avoid unphysical
solutions. The same parameter EntrFx_ controls the fix for the linear fields and non-linear fields.
The quantity δWk is the first order difference in face k of the variables. The terms in the matrices
are evaluated on face k using the Roe averaging.
Second Order Roe Scheme and Limiters
When the "left" and "right" values of the variables used in the previous formulation are the
upwind and downwind cell values respectively, the Roe scheme is first-order accurate. A higher
order of accuracy can be achieved through the process of solution reconstruction.
Reconstruction is the process of constructing, within each control volume, a continuous, usually
polynomial, representation of the solution from the discrete data. Discontinuities are, however,
allowed at the control volume interfaces, hence, the representation is piecewise continuous.
When computing the inviscid flux on a given face, the flow quantities in its neighboring cells are
no longer used to define the Riemann problem. Instead, reconstruction is used to obtain more
accurate estimates of the "left" and "right" states.
Reconstruction methods are classified by their order, which corresponds to the highest degree of
the polynomials they can reconstruct exactly.
In order to build a second-order accurate scheme, a linear reconstruction must be used. The
reconstructed flow solution on face k, bounded by cells L and R, is represented, on each side of
the face, as a - piecewise - linear polynomial of the form:
where
and
represent the solution gradients in cells L and R, respectively. In
the case of the "standard" dissipation, the reconstruction step is performed on the set of the
primitive variables whereas for the "isenthalpic" formulation the reconstruction is made on
density, velocity and total Enthalpy. In both cases, the calculation of the gradient is conducted
using the Least Squares method.
The least squares approximation is used to evaluate the flow quantities gradients in cell centers.
The principle is the following: by requiring that the linear polynomial expression holds at each of
the direct - or first-order - neighbours of a given cell c0, the following over-determined linear
system of equations is obtained:
where N is the number of first-order neighbours. The system is solved in the least square sense by
pre-multiplying through by the matrix transpose to yield the symmetric 3x3 system:
where Δxi is equal to xi - x0, and so on for the other variable differences involved in the system.
When solution discontinuities and steep gradients are present, additional steps must be taken to
prevent oscillations developing in the numerical solution. In the FINE™/Open solver,
the
monotonicity is enforced through the reconstruction step using the Barth and Jespersen (1989)
technique
In the linear polynomial expression, the gradients
and
are limited in order to
enforce the reconstructed solutions
and
to satisfy monotonicity
requirements. The reconstructed flow solutions on face k, bounded by cells L and R, are now
given by:
where
and
are the limiters computed in cells L and R, respectively.
The limiters are computed such that the reconstructed flow solutions satisfy the following
monotonicity criterion:
With
where U j and U l are the immediate neighbours cells values of the cells L and R, respectively.
Two kinds of methods to calculate ΦL and ΦR, Barth & Jespersen (1989) and Venkatakrishnan
(1995), are provided in the FINE™/Open solver.
In several publications it is reported about the deficiencies of the Barth- Jespersen limiting
procedure (e.g., Marques & Pereira (2001), Berger et al. (2005), Venkatakrishnan (1995)): One of
the mentioned drawbacks of the scheme is that the convergence often stalls after that the residual
has dropped a few order in magnitude. A second issue is that the Barth-Jespersen limiter functions
are too sensible to small variations in the flow field, which can cause an introduction of excess
numerical diffusion in free-stream regions.
To avoid that the convergence stagnates due to limit cycles, Venkatakrishnan (1995) suggests to
incorporate the van Albada limiter in the Barth-Jesperesen technique. More details can be found
in Venkatakrishnan (1995).
The user can activate the computation of the limiter by setting the expert parameter upw_limit_ to
1. Then the expert parameter upw_limitVenka_ can be used to choose if the Barth-Jespersen
limiter is used (upw_limitVenka_=0) or the Venkatakrishnan limiter is used (upw_limitVenka_=1).
In the FINE™/Open solver, the limiters are calculated only at the first stage of the Runge Kutta
scheme and only on the finest grid. This approach reduces the computational cost substantially.
The recalculation of the limiter at each stage of the Runge-Kutta scheme is governed by the
(vector) parameter spc_iCalcLim_ as the parameter spc_iCalcDissip_. Actually, by default, only
the first component of spc_iCalcLim_ is equal to 1. If all components are equal to 0, the scheme
reduces to first order accurate.
6.1.2
Time Discretization: Multistage Runge-Kutta
Pseudo-time integration is performed in the FINE™/Open solver by using a Runge-Kutta scheme
accelerated by a multigrid technique. An explicit q-stage Runge-Kutta scheme for the equation
can be written:
Where Un is the value of U at the time step t and Un+1 at the time step t + Δt. 1, 2 , ... and q is the
step of the Runge-Kutta method. The coefficients αi determine the stability area and the order of
accuracy of the Runge-Kutta scheme. They can be chosen in such a way that they suit the
problem to be solved.
For inviscid calculations the local (i.e. for each cell) inviscid time step is calculated as:
where Ω is the cell volume,
and c the velocity vector and speed of sound in the cell
respectively, and CFL is the Courant-Friedrichs-Lewy number.
Finally,
are the non unit normal vectors calculated in the control volume center in the
three local directions of the cell. They are evaluated by averaging the non unit vectors normal to
opposite sides of the cell, hence they are evaluated in the same way as when calculating the
spectral radii in the artificial dissipation of the central scheme, see Inviscid Fluxes section.
In the case of viscous computations, a local viscous time step is also calculated:
where μ eff is the effective viscosity, equal to the molecular viscosity when laminar flows are
simulated, and to the sum of the molecular viscosity and the turbulent eddy-viscosity in the case of
turbulent flows. ρ is the density in the cell where the time step is evaluated.
The resultant local time step, used when viscous flows are simulated, is then a harmonic-like
mean of the inviscid and viscous local time steps:
If local time stepping is used, as it is the case in the FINE™/Open solver, each cell in the
computation domain has its own time step for inviscid calculations and for viscous calculations.
In practice, 4 or 5 stage Runge-Kutta schemes are mostly used. In the FINE™/Open solver the
following coefficients are default (expert parameter tm_drcoeff_ in the Computation Control /
Control Variables page):
These are in principle only valid for 4-stage Runge-Kutta schemes.
By setting the coefficients in tm_drcoeff_ to zero, other sets of coefficients are used by the code,
depending on the number of schemes and the space discretization method:
For central schemes:
For first-order upwind schemes:
For second-order upwind schemes:
The user can specify the number of stages of the Runge- Kutta scheme through the expert
parameter tm_nbStage_ in the Computation Control / Control Variables page.
In Jameson (1985) the dissipative terms are calculated only once or a few times in a q-stage
Runge-Kutta scheme. This approach reduces the computational cost substantially.
The disadvantage is that the dissipative terms need to be stored separately. For the laminar Navier-
Stokes equations with 5 equations, 5 extra arrays are required to store the dissipative residuals
from the artificial dissipation. The same principle holds for viscous residuals.
The residual R ( U ) is therefore split into a purely convective, a dissipative part (numerical
dissipation) and a viscous part:
where Rc(U) is the convective part of the residual, Rd(U) is the dissipative part, and Rv(U) the
viscous residual.
The expression for F in the explicit q-stage Runge-Kutta scheme at any stage m is then
where m is the current stage, n is the latest stage at which the dissipative residuals have been
evaluated, and p is the latest stage at which the viscous residuals have been evaluated.
located in the Advanced tab of the Computation Control
The recalculation of the dissipative residuals is governed by the (vector) parameter spc_
/ Control
iCalcArtifDissip_,
Variables page. For a m-stage Runge-Kutta scheme the m first elements of this vector are used,
the first element corresponding to the 1st stage, the 2nd element to the 2nd stage and so on. If the
element of spc_ iCalcArtifDissip_ is 0 it means that the dissipative residual should not be
calculated at the corresponding stage, and the latest available dissipative residuals will be used; if
it is 1, Rd will be calculated.
Note that for consistency reasons, the first value of spc_iCalcArtifDissip_ should always be one.
For upwind schemes, in order to run at high CFL numbers, it is advised to recalculate the upwind
dissipation at every stage. Hence, all elements of spc_iCalcArtifDissip_ should be set to 1.
Central schemes are usually less sensitive to the recalculation of the artificial dissipation, so that,
depending on the Runge-Kutta scheme, calculation of the dissipation can be skipped at several
(default value) for a 4-stage
stages. Advised values for spc_iCalcArtifDissip_ are
scheme, and
for a 5-stage scheme.
For the viscous residuals, a similar parameter, called spc_iCalcVFluxes_ exists. Note that for
consistency reasons, the first value of spc_iCalcVFluxes_ should always be one. Actually, by
default, only the first component of the spc_iCalcVFluxes_ vector is equal to 1, i.e., viscous
residuals are evaluated only once per iteration, at the first Runge-Kutta stage.
Within multigrid, the Runge-Kutta operator can be applied more than once on each grid level, to
ensure a better smoothing. The parameter "Number of sweeps on successive grid levels", located
in the Advanced tab of the Numerical Schemes page gives the number of times the Runge-Kutta
operator will be applied to each grid level during the fine-to-coarse or coarse-to-fine - part of the
multigrid cycle. They can take different values on each grid level.
Within the explicit Runge-Kutta approach, the source terms of the turbulence models are treated
in a point implicit way.
6.1.3 Multigrid Strategy
The FINE™/Open solver uses multigrid for efficiency and fast convergence. The power of this
method lies in the fact that it damps most of the low frequency errors that cannot be damped by
explicit schemes. The algorithm is organized in the following way:
1. Apply one or more sweeps of a smoother of the high frequency errors, so that the error
behavior is sufficiently smooth to be adequately represented on a coarser mesh. This last point
is crucial for the strategy to be effective.
2. Transfer the problem to coarser grids, where an approximation to the solution correction ΔU is
obtained at reduced computational costs since there are fewer mesh points. On the coarser
grids, the low-frequency errors are more easily damped as they manifest themselves as higher-
frequency errors.
3. Transfer the corrections back to the fine grid in order to generate a new approximation of the
solution.
This sequence can be repeated recursively on coarser and coarser grids, where each grid level is
responsible for eliminating a particular frequency bandwidth of errors. The input variable given
by the user (Numerical Schemes page: Number of grids) precisely denotes the number of grid
levels to be used in the multigrid strategy. The coarser grids are created within the FINE™/Open
solver by using agglomeration only.
In the FINE™/Open solver, an explicit multigrid scheme is developed, that is, an explicit Runge-
Kutta scheme is used as smoother to damp high frequency errors on the various multigrid levels.
The multigrid technique is particularly well suited for linear problems. However, in the present
context, a non-linear system of ordinary differential equations in time has to be solved. The
method is adapted to the treatment of the non-linear equations, by operating simultaneously on the
solution and on the residual vector. This approach is known as Full Approximation Storage
(FAS) approach.
A. Full Approximation Storage approach
Let us write the Euler or Navier-Stokes system of equations on the fine grid in the following form:
where
denotes the fine grid discretization,
is the Euler/Navier-Stokes operator on the fine
grid,
is the exact solution that we seek, and
are any possible source terms. The residual on
the fine grid is defined by:
where
is the current solution estimation on the fine grid. Taking the difference between
Euler/Navier-Stokes system of equations and the residual on the fine grid, we obtain:
After several smoothing sweeps on the fine grid, using the explicit Runge-Kutta scheme, the high-
frequency errors in the solution are eliminated. The problem then has to be transferred to a coarser
grid to remove lower frequency errors.
Notice that since the Euler/Navier-Stokes system is non-linear, the difference of the operators in
the above equation cannot be replaced by the operator on the difference between the exact and
estimated solutions
. Instead, a new coarse grid variable
is introduced:
where H denotes the coarse grid discretization, and
is the solution restriction operator, which
interpolates the solution from the fine grid h to the coarse grid H.
The equation to be solved on the coarse grid aims to determine the corrections to be transferred
back on the fine grid. Hence it is written as follows:
where
(not to be confused with
) is the residual restriction operator which interpolates
residuals from the fine to the coarse grid. Using the new grid variable
, the system to be
solved on the coarse grid can be rewritten as follows:
The right-hand side of this system is composed of the residual restriction and of the coarse grid
system operator applied once on the solution restriction. It is called the forcing function, and can
be seen as a source term of the system on the coarse grid, which ensures that the solution on the
latter has the accuracy of the fine grid. This system is solved using explicit Runge- Kutta
of the solution on the coarse grid is obtained, in which
smoothing so that a new estimation
the high frequencies on to the coarse grid have been eliminated.
The corrections, i.e. the differences between the computed solution on the coarse grid and the
restricted solution from the fine grid, are then interpolated back to the fine grid, instead of the
solution itself:
If the sequence of coarse grids is optimally generated, this approach requires only little more
memory than that of the baseline explicit scheme used to drive the smoothing process.
Usually, more than two grids are used in the multigrid method, and therefore, various strategies
can be chosen in the sequence of transfers and smoothing sweeps between successive grids. The
most simple strategy is the V-cycle, which consists of a succession of restrictions from the finest
to the coarsest level and prolongations from the coarsest back to the finest level. In addition, the
W-cycle, F-cycle and the sawtooth type of the V/W/F-types are also available. For the sawtooth
cycles, the equations ( momentum and turbulence) are not solved on coarse grids before the
prolongation step to finer grids. The type of multigrid cycle can be selected by the expert
parameter tm_mgCycleType_ (V-cycle by default). Note that on coarse grids, the smoothing may
consist of more than one Runge-Kutta sweep to ensure that the relevant frequency bandwidth of
errors is damped effectively. The number of smoothing sweeps can be chosen by the user for each
grid level (Advanced tab of the Numerical Schemes page, Number of sweep on successive grid
levels).
FIGURE 6.5
The cycle type of multigrid strategy
B. Grid transfer operators
The choice of appropriate transfer operators is of paramount importance to ensure the efficiency
and, most importantly, the robustness of the multigrid method.
Restriction operator
In the FINE™/Open solver, a linear restriction (
) is used. The residual restriction in a
parent cell is equal to the sum of the residuals in its children, and the solution restriction is a
volume-weighted averaging of the solutions in the child cells.
Solution and residuals are "smoothed" prior to the application of the restriction operator, by
interpolation from cells to faces, then from faces back to cells. This improves robustness.
Such a method requires knowledge of the solution and the residuals in dummy cells. The first is
already known through the application of boundary conditions, whereas a boundary treatment
must be applied to evaluate residuals on boundary faces. This is based on the solution boundary
conditions, that is, if the solution can vary in time on the boundary, the residual will be
extrapolated from the interior domain. On the contrary, if the solution is fixed, the residual will
necessarily be equal to zero on the boundary face. This gives the following conditions for the
residuals of the five equations of the RANS system, with 0 designing the outer cell, and 1 the
inner cell:
l subsonic inlet:
l density and momentum:
l energy:
l subsonic outlet:
l density and momentum:
l energy:
l supersonic inlet:
l all equations:
l supersonic outlet:
l all equations:
l mirror or Euler wall:
l density and energy:
l momentum:
l Navier-Stokes wall
l density and energy:
l momentum:
Prolongation operator
For the prolongation of the solution correction from a coarse level to a successive fine level, a
), is used, where corrections are simply injected from a coarse
constant prolongation (
level parent cell to its fine level child cells.
An additional smoothing step is performed, that is, the injected corrections are interpolated on
faces instead, and then transferred back to cells. This method is equivalent to the correction
applied to the solution and residuals before their restriction on a coarser level. The resulting
prolongation operator preserves solution linearity for one- dimensional configurations. This
prolongation operator requires a special treatment of the corrections at the boundaries since these
are needed for the interpolation onto faces. The corrections in outer or "dummy" cells are
calculated by applying boundary conditions on the restricted solution as well as on the solution
computed on the coarse grid. FIGURE 6.6 summarizes the strategy.
FIGURE 6.6
Prolongation operator
6.1.4
Full Multigrid Strategy
In order to create a good initial solution, Full Multigrid is also available.
The structure of Full Multigrid is well explained by FIGURE 6.7. One starts an iteration method,
such as a multi-stage Runge-Kutta explicit scheme, on the coarsest grid. The solution on that level
will not be interpolated to the next finer grid until it converges to a certain accuracy level. Then
the interpolated solution on the finer grid is taken as the initial solution for further iterations run on
that grid level. The process is continued recursively until the finest grid is reached. The initial
solution on the finest grid is called the solution obtained by a Full Multigrid method.
FIGURE 6.7
Scheme of the full multigrid strategy
It should be mentioned that there are two different kinds of prolongation in Full Multigrid. One is
the same as that used in the standard multigrid cycle, the other is the prolongation of solutions,
which replaces the corrections in a standard multigrid prolongation. The same prolongation
operator is used for solution and correction prolongation, see Multigrid Strategy section.
Based upon numerical experiments, it has been found out that it is very important to check the
convergence level of solutions on the coarser grid before switching to the next finer grid. If
solutions do not converge on a coarser grid, it may cause divergence on the next finest grid.
In addition, an initial solution on coarse grids is less sensitive to multigrid convergence than on the
finest grid. A large cell size makes solutions converge quickly and easily. Hence it takes much
less computational time and with a lower risk of calculation divergence to get reasonable solutions
on the finest grid, when compared to the starting directly on the finest grid. A full multigrid
method can therefore improve the robustness and efficiency of numerical iterations methods.
6.1.5
Implicit residual smoothing
Implicit residual smoothing can be used in combination with Runge-Kutta to allow a higher stable
CFL number and speed up the convergence to steady state.
One stage in the explicit Runge-Kutta scheme might be written:
The residual R may then be smoothed first, before applying the update of the explicit Runge-
Kutta scheme. For unstructured grids the smoothened residuals are defined as:
where ϵ is a smoothing coefficient. L represents the Laplacian differential operator. For a discrete
unstructured, cell centered scheme this operator can be represented by a simplified Laplacian
operator:
According to line statistical analysis, the maximum stable CFL number σ* when an implicitly
smoothened residual is used is given by:
(0-1)
where σ*, σ are the maximum stable CFL numbers of the smoothed and unsmoothed Runge-
Kutta scheme, respectively. The result of the residual smoothing is thus that one can run at higher
CFL numbers. The value of ϵ is set by default to 0.75 which means that the CFL number can be
doubled.
Different types of residual smoothing are available. Each one corresponds to a different value of
the expert parameter tm_iResSmoothing_:
l For tm_iResSmoothing_ = 0, no residual smoothing is used.
l For tm_iResSmoothing_ = 1, one uses a smoothing technique of Radespiel & Rossow. The
residual smoothing is performed for all solved equations (including the turbulence model
equations). This option is available for Euler, laminar flow as well as for simulations with one-
equation turbulence models.
l For tm_iResSmoothing_ = 2 (default), one also uses a smoothing technique of Radespiel &
Rossow. However, the residual smoothing is performed only for the continuity, momentum
and energy equations. This option is available for simulations with two-equation turbulence
models.
The residual smoothing during the coarse grid initialization is controlled by the expert parameter
tm_fmg_iResSmoothing_. It has the same possible values as tm_iResSmoothing_, but is by
default equal to 0.
6.2
PRECONDITIONING
In the low subsonic Mach number regime, time marching algorithms designed for compressible
flows show a pronounced lack of efficiency. When the magnitude of the flow velocity becomes
small in comparison with the acoustic speeds, time marching compressible codes converge very
slowly.
The problems faced by compressible codes at low Mach number are:
l High disparity between the convective eigenvalues u and the acoustic eigenvalues u+c, u-c
leading to a much too restrictive time step for the convective waves and causing poor
convergence characteristics.
l Round off errors mostly due to the use of absolute pressure in the momentum equations.
l Impossibility to treat strictly incompressible flows.
This motivated the development of a low speed preconditioner to provide fast convergence
characteristics and accurate solutions as the Mach number approaches zero. Over the past years
and up to now, many attempts have been made to solve nearly incompressible flow problems
within available compressible codes and with minor programming efforts. The corrective action
brought to the discretization of the conservation equations is called preconditioning and is derived
from the artificial compressibility method introduced for incompressible flows by Chorin, (1967).
For steady state applications, solved by time marching algorithms, the time derivatives of the
unknowns in the flow equations are of no physical meaning and can therefore be modified
without altering the final steady state solution. The idea of preconditioning precisely uses this
property and consists of multiplying the time derivatives of the dependent variables with a matrix
called preconditioning matrix. The main property of this matrix is to remove the stiffness of the
eigenvalues. In addition, reduced flow variables such as the dynamic pressure and the dynamic
enthalpy are introduced, reducing drastically the round off errors at low Mach numbers. The
acoustic wave speed c is replaced by a pseudo-wave speed c' of the same order of magnitude as
the fluid speed. To be efficient the selected preconditioning matrix should be valid for inviscid
computations as well as for viscous computations with heat transfer.
6.2.1
Hakimi preconditioning
The preconditioning methodology developed (Hakimi, 1997) is of sufficient generality and can
treat any type of fluids including perfect gases and incompressible Newtonian and non Newtonian
fluids. On the numerical
time
integration and boundary conditions have been adapted to the new transient behavior of the
conservation equations.
the solution procedure including space discretization,
level,
The low speed preconditioner has been validated for inviscid flows, viscous flows, turbulent
flows and unsteady flows. Efficient convergence rates and accurate solution have been obtained
for Mach numbers from M=0.1 to M = 10-6, Reynolds numbers from Re = 106 to 10-6 and aspect
ratios from 1 to 2000.
A. General Form of the Preconditioning Matrix
The Preconditioned Reynolds- Averaged Navier- Stokes equations including turbulence and
species transport equations written in a Cartesian frame of reference and integrated over a control
volume Ω are expressed as:
with
The variable
energy.
is the gauge pressure and the variables
is the total gauge
For a perfect gas with constant
,
is given by:
For an incompressible fluid with constant
,
is given by:
The extension of the preconditioning matrix to the turbulence transport equations is then given in
its general form both for compressible and incompressible fluids by:
* the term -1 should be added in compressible cases only.
We notice from this equation that the preconditioning matrix does not apply to the transport
equations of k and ε. This choice is the simplest and did not cause any particular instability for
turbulent test cases run so far.
B. Eigenvalues of the System
The eigenvalues of the preconditioned system are determined from the Euler part and can be
obtained easily if the equations are written in terms of the primitive variables (p,u,v,w,p or e).
Their expression is given in 3D for compressible fluids by:
The two parameters α and β are chosen so that the stiffness of the eigenvalues is minimised at low
speed.
The corresponding eigenvalues for incompressible fluids are:
Compared to preconditioned system of compressible fluids,
the first three eigenvalues are
unchanged and the eigenvalues of the acoustic waves can be obtained by setting the speed of
sound to infinity. We note in particular that the acoustic eigenvalues are always of opposite sign
showing that the flow remains subsonic with respect to the pseudo-sonic speed. As for the
compressible preconditioner the two parameters α and β are chosen so that the stiffness of the
eigenvalues is minimised at low speed.
Note that if a k-ε model is considered, the corresponding eigenvalues will be:
C. Choice of the Parameters α, β and the Reference Velocity
The user control variables are pref, Tref, α, β.
pref, Tref are accessible through the Numerical Schemes page, by checking the User defined
gauge parameters box, and are referred to as gauge pressure and gauge temperature. By default,
when the box is not checked, they are set equal to the reference pressure and temperature defining
the fluid.
A value of Tref of the order of magnitude of the expected temperature field will reduce the machine
round-off errors influence on the temperature field.
The value of pref fixes the absolute level of the pressure in the field. This value is used in the equation
of state for a compressible fluid and in the second order artificial dissipation term. A value of Pref
close to the real pressure level is therefore recommended.
The parameter α, according to several computations accomplished with the central scheme,
enables to reach good convergence rates for values lying in the range [-1,1]. So far the best value
is found to be α = -1 and is automatically set as default. This optimal value is not surprising since
it increases the spectral radius and therefore adds an additional amount of artificial dissipation.
preconditioning
The
parameters/Numerical schemes page through a coefficient β* and a characteristic velocity
parameter
imposed
user
the Numerical
the
by
in
is
such that
The default value of β* is 3. Based on our experience with the presented low speed
preconditioner the parameter β* can be taken of order unity for inviscid flow computations. For
viscous computations associated with Reynolds numbers greater than about Re=1000, a constant
value β* of order unity is also adequate. If convergence difficulties are encountered at the very
beginning of a computation, it is recommended to increase the value of the parameter β*.
Remember however that a too large value of β* will introduce excessive artificial dissipation into
the solution.
For lower Reynolds numbers the parameter β* has to vary in order to preserve numerical stability
and a good convergence rate. The parameter β* should increase as the Reynolds number
decreases and may vary over several orders of magnitude .
If the local velocity scaling option is activated in the Numerical parameters/Numerical schemes
page, another definition of β is used:
where
is the local velocity.
FIGURE 6.8
Typical variation of the preconditioning parameter β* with Reynolds number
6.2.2 Merkle preconditioning
The motivation for changing from the Hakimi to the Merkle preconditioner is to obtain a solution
scheme with an increased robustness. A further motivation is to get a solution scheme that is not
only efficient at all Mach numbers but also for all Reynolds and Strouhal numbers. The intention
of the change of the preconditioning concept is also to obtain a scheme, which is intuitive,
conceptually simple yet effective and general.
To derive the Merkle preconditioning scheme, the Navier-Stokes equations for compressible in
Cartesian coordinates are used as a basis.
with
.
The set of independent solution variables is changed from the vector of conservative variables U
by splitting up the unsteady
to the vector of viscous, primitive variables
term according to:
The Jacobian
is thereby given as:
The subscripts p and T represent the isothermal derivative with respect to the pressure and the
isobaric derivative with respect to the temperature, respectively.
To ensure efficiency for all Mach numbers the Jacobian is replaced by the preconditioning matrix:
The matrix
differs only from the Jacobian
by the fact that the physical quantities
,
,
and
are replaced by the scaled quantities
and
, respectively.
The parameters
and
are used to control the scaling of the dynamics for both
inviscid and viscous dominated flows. The parameters
and
are set to their physical
values, as these parameters only have a minor effect on the dynamics of the Navier-Stokes
the energy equation in the unscaled Navier- Stokes
equations. In the incompressible limit
equations is decoupled from the continuity and momentum equations. This property should be
should
kept for the preconditioned flow equations, wherefore the preconditioning parameter
be scaled proportional to its physical counterpart. In the FINE™/Open solver, this parameter is set
remains in order to control the
to its physical counterpart. Therefore, only the parameter
preconditioning. This parameter can be written:
where vp is the particle velocity.
The local preconditioning velocity plays a crucial role as it should be as low as possible but not
smaller than the local velocity, and should not be greater than the speed of sound in supersonic
regions. Furthermore, it plays a crucial role in the robustness of the preconditioning method. In the
flow solver the particle velocity vp is defined as:
for compressible fluids
for incompressible fluids
with:
cases.
where the speed of sound is used only for compressible
is set in the Numerical Schemes page.
is a coefficient defined by the expert
parameter preco_pcEpsVLimC_ and
pcEpsVLim_ .
is a coefficient defined by the expert parameter preco_
(turbulent viscosity only used for turbulent cases)
For two equations turbulence models two new limiters should be included:
and
These two limiters are combined in one single limiter:
6.3
TIME CONFIGURATION
Unsteady flow phenomena may arise intrinsically as, for example, in separated flows, wake flows
or may be caused by an external time dependent driving force as, for example, an oscillating
structure. In any case an efficient time- accurate solver has to be employed to obtain time
dependent solutions within a reasonable computational time.
The most common approach is the dual time stepping approach, proposed by Jameson, (1991),
which consist of adding pseudo- time derivative terms to the time dependent Navier- Stokes
equations. At each physical time step, a steady state problem is solved in a pseudo time and all
available acceleration techniques such as multigrid, local time stepping and implicit residual
smoothing can be applied. This approach has been used for compressible flow simulations by
several authors, Arnone, (1995), Melson et al., (1993), Pierce et al., (1997), Eliasson et al., (1995)
and has shown to be an important improvement over the classical global time stepping approach.
6.3.1
Standard Time Accurate Solver (Non-preconditioned
Formulation)
For unsteady flow simulations the Reynolds-Averaged Navier-Stokes equations are expressed as:
where
variables,
is the physical time and
is the volume,
is pseudo time,
are the conservative fluxes and
is the solution vector of the conservative
are the source terms. The time
discretization of the derivative of the conservative variables with respect to the physical time
made to meet the desired accuracy in time. Two formulations are available:
is
A. First Order Backward Method
.
This first order scheme is used only for the first time step of the unsteady computation except for a
restart when the two previous solutions are available.
B. Second Order Backward Method
The implicit second order backward difference scheme to advance the solution in time is given
by:
For general cases, the user specifies the amplitude of the constant physical time step and the
=0.5 (these coefficients
coefficients above are taken as constants, with
=1.5,
=-2,
cannot be modified in the interface). In the case of turbomachinery applications, the solver needs
to consider a physical time step based on the Number Of Angular Positions that the unsteady
algorithm should solve within one period of rotation . If a
variable rotational speed is imposed, the coefficients described above are not taken as constants,
,
but rather dependent on the current and the previous physical time steps,
and
respectively:
All other terms in the Reynolds-Averaged Navier-Stokes equations are computed at the time
. The equation is then treated as a modified steady state problem in the pseudo time :
.
Denoting by
time accurate computations
is given by:
the residual corresponding to the steady state problem, the new residual used for
The new residual contains terms that depend only on the solution of previous time steps, all other
terms depend on the current solution vector
.
When steady state is reached at each physical time step, the left hand side of this new residual
tends to zero and the time accurate solution is obtained.
C. The Time Stepping
When integrating the residual in the pseudo time
Pierce and Alonso (1997) to treat the term
, it is recommended, Arnone et al. (1995),
implicitly. This is done by
developing the solution vector
in a Taylor expansion:
.
Putting this equation into the modified steady state problem, a modified pseudo time step is
introduced:
.
The pseudo time step is modified by an additional term containing the physical time step. This
term becomes dominant if the physical time step is significantly smaller than the pseudo time step.
This situation does not often happen since the physical time step is taken as large as possible.
However, in the far field where mesh dimensions are increased the pseudo time step might reach
high values and the contribution of the physical time step will have a stabilizing effect there.
The physical time step
step is usually taken as a fraction lying between 1/20-1/40 of the expected period.
is limited by the desired level of accuracy. For periodic flows the time
D.
Initial Solution at Each Physical Time Step
The simplest way to obtain an initial solution on the next time level is to choose the latest
available solution:
being the cell volume evaluated at the next time step.
6.3.2 Density Based Time Accurate Solver and
Preconditioning
Application of the dual time stepping approach, along with low speed preconditioning to variable
and constant density flows is presented in Hakimi, (1997). For unsteady flow simulations the
preconditioned Reynolds-Averaged Navier-Stokes equations are expressed as:
,
where t is the physical time and τ is pseudo time, U is the solution vector of the conservative
variables, Q is the solution vector of chosen dependent variables, Γ is the preconditioning matrix,
are the conservative fluxes and ST are the source terms. For all fluids we
Ω is the volume,
have:
.
where
is the gauge pressure (
) and
is the total gauge energy.
The time discretization of the derivative of the conservative variables with respect to the physical
time t is made to meet the desired accuracy in time. The equation is then treated as a modified
steady state problem in the pseudo time τ:
with
,
.
The residual RTA being the preconditioned residual. The new residual contains terms that depend
only on the solution of previous time steps, all other terms depend on the current solution vector
Q. When steady state is reached at each physical time step, the left hand side tends to zero and the
time accurate solution is obtained
A. The Time Stepping
When integrating the residual in the pseudo time τ, we treat the term
implicitly. This is obtained by developing the solution vector U in a Taylor expansion:
Putting this relation into the modified steady state problem we obtain the following updating
procedure:
where I is the identity matrix. The updating procedure has been modified and now includes the
time steps ratios, leading to a stabilizing effect.
B.
Initial Solution at Each Physical Time Step
The initial solution on the next time level is the latest available solution:
Since the dependent variables are Q, these variables have to be computed at the beginning of each
physical time step from the conservative variables U.
CHAPTER 7.
MESH ADAPTATION
This chapter gives some insights about the algorithms governing and performing mesh adaptation in
FINE™/Open with OpenLabs™.
In this section
7.1 H-type adaptation
7.2 Flow feature detection
7.3 Boundary layer insertion/regularization
111
114
117
7.1
H-TYPE ADAPTATION
7.1.1
Anisotropic refinement
First, let us remember that hierarchy is used extensively in the adaptation module data structure.
Hence, when any mesh entity, cell, face or edge, is refined, it is not deleted, but still exists in the
data structure and is connected to any newly created children. This forms the parent- child
connectivity.
The anisotropic refinement algorithm can be split into the following steps, considering that three
directional refinement flags are produced for each cell after the sensor calculation:
1. Propagate the cell refinement flags to their faces and edges.
2. Perform a balance,
i.e. verify that
the current configuration of flags will not produce
configurations which may degrade the code accuracy, such as for example "holes" or edges
with more than one hanging vertex, and if this is the case, to propagate the refinement to
neighboring faces and cells so that such configurations are avoided.
3. Refine the mesh entities according to the flags. The individual cell refinement process begins
with the refinement of the cell faces, itself beginning with the refinement of the face edges.
The refinement balancing function
If the refinement process was just performed according to the flags provided by adaptation
criteria, several cells could remain unrefined whereas their neighbours could be refined several
times. This would lead to very sparse sizes for neighboring elements and to configurations where
one large cell could be the neighbour of n small cells, themselves of different sizes. Such
configurations are not acceptable since they would introduce severe robustness and accuracy
issues in the flow solver.
The role of a balancing function is therefore to "smooth" the refinement by propagating flags so
that certain rules are satisfied, see FIGURE 7.1.
1. Only one hanging node per edge is tolerated
2. In order to avoid large size differences for cells sharing the same face, the difference in
refinement level of two neighboring cells in the direction parallel to their common face cannot
exceed one.
3. "Holes" in the mesh are prevented, i.e., if two opposite faces in a cell are flagged for
refinement, which means that the neighboring cells are flagged, then the cell itself is flagged
for refinement in the corresponding direction.
FIGURE 7.1
Configurations prevented by the balancing function
Solid surface reconstruction
When mesh refinement is performed in the vicinity of curved solid bodies, additional boundary
vertices may be added. It is then necessary to reproject these vertices onto the geometry to avoid
unwanted flow discontinuities due to insufficient geometry resolution compared to mesh
resolution. This operation is performed in the adaptation module after the refinement process, see
FIGURE 7.2. Notice that since the geometry is defined by a set of triangulations, these should be
sufficiently fine compared to the finest mesh cells.
FIGURE 7.2
Solid surface reconstruction during boundary cell refinement
7.1.2 Mesh coarsening
The grid coarsening technique is based on the hierarchical property of the mesh adaptation data
structure. Since the mesh entities' parents are stored during the refinement process, these parents
can be recovered when their children are removed.
The principle of mesh coarsening is less "local" than refinement. Indeed, when analyzing a cell
for refinement, no care is given to its siblings before confirming the cell refinement. When
coarsening is performed, cells are analyzed in families, that is, all the sibling cells are considered.
This property makes the mesh coarsening operation less likely than the refinement one, since for a
set of siblings to be coarsened, several properties must be satisfied, namely:
1. The cells should be flagged only for coarsening. If a cell is flagged for both refinement and
coarsening, which is possible when combinations of adaptation criteria are used,
then
refinement has the priority.
2. All the sibling cells must be leaf cells, otherwise coarsening is cancelled for the whole family.
3. At least 75% of the sibling cells must be flagged for coarsening. Then, the remaining siblings
are also flagged for coarsening, even if they were flagged for refinement.
When all these conditions are satisfied for a set of siblings, they are removed and the parent cell is
recovered. Since the coarsened mesh may contain some of the forbidden configurations
mentioned in the refinement balancing function section, the refinement balancing function is
executed and some cells are refined.
Notice that when cells are removed, their faces, edges and vertices are also removed unless they
belong to other elements that still exist in the mesh. Hence general mesh coarsening consists of the
following steps:
1. The bit vector containing cell coarsening flags is first cleaned, i.e., if cells are flagged for
refinement and coarsening, the latter flag is set off.
2. In three- dimensional cases,
the balancing function removes further
flags because of
problematic configurations potentially encountered for faces after coarsening.
3. Cells are analyzed per family. If a set of leaf sibling cells has more than 75% of its members
flagged for coarsening, the remaining siblings are also flagged for coarsening, else, all the
members are de-flagged.
4. Flagged cells are removed, followed by the faces, edges and vertices that are no longer
referenced.
5. The refinement balancing function is executed to remove forbidden configurations. Hence,
some cells are flagged for refinement.
6. The flagged cells are refined, following the procedure described in the refinement balancing
function section.
The advantage of hierarchical coarsening is obvious in terms of coding, since elements resulting
from mesh coarsening are already stored in the data structure. Furthermore, this approach
guarantees the all-hexahedral configuration of the resulting adapted meshes.
It should also be noticed that initial meshes generated with the all-hexahedra mesh generator
HEXPRESS™ already contain "parent" cells in their data structure, since geometric mesh
adaptation is performed prior to the mesh trimming and body-fitting steps, see the dedicated
manual. It is therefore possible to slightly coarsen the initial mesh using the hierarchical method,
except at the vicinity of boundaries, since parents whose descendants have been removed during
the trimming phase cannot be recovered.
7.2
FLOW FEATURE DETECTION
7.2.1
Introduction
The effectiveness of any adaptation method critically depends on the accurate determination of the
regions to be adapted. The formulation of an efficient universal adaptation criterion is an
extremely difficult task.
In the FINE™/Open solver, flow feature detectors, or sensors, are used to govern adaptation. It is
reasonable to track regions of large flow gradients since they are generally the sites where
significant numerical errors exist. The flow features of interest are "sensed" in order to increase
the solution accuracy in regions where they occur and decrease the resolution in other regions.
Beside sensors, refinement and coarsening thresholds have to be chosen: if a sensor value exceeds
the refinement threshold, then the corresponding part of the domain is flagged for refinement. If
on the contrary, the sensor value is below the coarsening threshold, then the corresponding zone
is coarsened because no significant flow variation is detected.
Flow feature detection can be seen as a three steps procedure:
1. One or more suitable sensors are calculated in each cell for the identification of flow
phenomena.
2. Threshold values a sensor must have to remove or refine the cell are calculated.
3. Cells to be refined or removed are flagged.
7.2.2
Sensor and threshold formulations
Since the flow solution is stored in cell centers, the interesting quantities which are used in the
formulation of flow feature detectors are generally more easily calculated in cell centers than on
faces. Face- centered sensor formulations are however used because they naturally involve
anisotropic refinement. Indeed, when the sensor evaluation in the face exceeds a prescribed
refinement threshold, the neighboring cells are refined in the direction parallel to the face, see
FIGURE 7.3.
FIGURE 7.3
Illustration of sensor calculation and cell flagging
Considering a face k and its two neighbour cells L and R, and denoting by U the quantity used to
detect a given class of phenomena, the following formulation is used for the flow feature detector
evaluated on face k:
where
and
are the flow quantity values in the left and right cells respectively, and
is
its average value over the whole computational domain. This is referred to as a finite difference
formulation. It is non-dimensionalized with respect to the considered flow quantity U by using its
average value over the whole domain. Notice that the behavior of the resulting sensor is
dependent on the mesh and flow configurations. It gives, however, reasonably good indication of
the regions to be refined or coarsened.
Threshold values are necessary to determine which cells should be refined or coarsened. Instead
of relying on completely manual threshold determination, a statistical formulation is used. Making
the assumption that the sensor statistical distribution over the domain is Gaussian, the optimum
are defined by Kallinderis and Baron
threshold values for refinement and coarsening
and
(1989):
where α and β are user-defined parameters, whose default values are equal to 0.3 and -0.3
respectively. This corresponds to a purely Gaussian distribution of the sensor over the
computational domain. The quality of the adapted mesh, and therefore of the solution, depends on
the choice of the threshold values for the sensor. The threshold value determination is very
effective when the sensor has a Gaussian statistical distribution across the whole domain. On two-
dimensional configurations, such a formulation works reasonably well. Unfortunately, when
complex three-dimensional flows are simulated, since many features have to be captured at the
same time, the statistical distribution of the sensor may be completely none Gaussian since the
majority of the cells may be located in regions where a given sensor is not active. The choice of
appropriate parameters is then case and sensor dependent.
7.2.3
Flow quantities used for feature detection
Density, velocity magnitude, pressure and temperature can be used to build the flow feature
detector.
Density should obviously not be used in the case of incompressible flows. It detects strong shocks
very well, reflected shocks less accurately, and expansion fans poorly. By analyzing the Rankine-
Hugoniot relations, see e.g. Hirsch (1990), it can be seen that density is a good candidate for the
detection of contact discontinuities and slip lines
Velocity magnitude can be used for the detection of phenomena as different as shocks, slip lines,
vorticity layers and boundary layers. Its use is inappropriate in expansion fans and contact
discontinuities detection.
Pressure is extremely efficient in detecting shocks, reflected shocks and expansion fans. Its use is
inappropriate in the detection of contact discontinuities, slip lines and boundary layers.
It is very difficult to find a sensor suited for the detection of every flow phenomena. Therefore,
using combinations of these refinement parameters is mandatory when several flow features are
present. Actually, even for the detection of a single phenomenon, there might not always be an
ideal sensor. In most of the cases, a pair of sensors consisting of pressure and velocity magnitude
differences is used for the detection of flow phenomena, since most of the flow features can then
potentially be captured.
7.3
BOUNDARY LAYER
INSERTION/REGULARIZATION
7.3.1
Introduction
This section concerns a module, which is completely transparent to the user. It should however be
read in order to get more understanding of adaptation inside boundary layers.
An additional module exclusively dedicated to mesh adaptation tasks inside the boundary layer
region has been implemented. The objective is to overcome several limitations and problems that
can be caused by classic h-type refinement.
l The first concern is to prevent mesh adaptation produced by flow feature detection inside the
boundary layer region, where the occurrence of hanging vertices can significantly decrease the
robustness and accuracy of the flow computation module of the FINE™/Open solver.
l In addition, if only h-type refinement is performed to capture a boundary layer region, "jumps"
in the point distribution in the direction normal to the boundary layer are unavoidable, as
shown in FIGURE 7.4 . It is furthermore not possible to create a boundary layer with a
constant progression of the cell stretching ratio from the first layer to the outer layer. This is
due to the fact that in classic h-type refinement, mesh edges are divided in two equal parts.
FIGURE 7.4
Evolution of cell stretching in h-type adapted boundary layers
l The third issue to solve occurs when cells located in curved solid boundary regions are refined.
Additional boundary vertices are created, and reprojected onto the boundary surface. When
highly stretched boundary cells are refined, snapping of the new vertices can produce negative
cells, as shown in FIGURE 7.5.
FIGURE 7.5
Limitation of the solid surface reconstruction
7.3.2
Boundary layer insertion and regularization
In order to overcome the above-mentioned problems, the creation of viscous meshes by classic
sensor-based h-type refinement is avoided. Instead, the boundary layer insertion module of the
mesh generator HEXPRESS™ must be used to create the boundary layer. This makes use of
anisotropic refinement to subdivide the first layer of wall boundary cells. However, only a limited
number of hanging vertex configurations are accepted after refinement, and all boundary vertices
are repositioned in order to match a prescribed first layer size and geometric progression of the
stretching ratio. The boundary layer insertion procedure will be briefly outlined here. For more
details, the reader is referred to the HEXPRESS™ manual.
l The first step in the boundary layer insertion consists of the anisotropic refinement of the first
layer of wall cells of the Euler mesh, and of their descendants, until a prescribed number of
layers have been generated. Hence, the whole boundary layer is contained in the original first
wall cell layer of the Euler mesh, which has to be sufficiently coarse. FIGURE 7.6 shows the
refinement process for the creation of ten layers. Boundary layer insertion should be performed
on a mesh whose first layer of wall boundary cells is semi-structured, i.e., does not contain
hanging vertices in the streamwise direction. This is always the case for all- hexahedra
unstructured meshes generated with HEXPRESS™.
FIGURE 7.6
Refinement of the first layer of wall boundary cells
l Once the refinement step is finished, the boundary layer region may contain hanging vertices
the
in the wall normal direction, produced by refinement propagation, for instance at
intersection of two solid surfaces. These vertices are removed through a regularization process,
which propagates refinement normal to the wall from the first to the outer layer inside the
boundary layer region, as shown in FIGURE 7.7 (a). After the regularization step, the
boundary layer region has a semi-structured configuration, with a limited number of hanging
vertices, which cannot be located either in the streamwise direction - since all the cells of the
Euler mesh first wall layer have been refined in the same way - nor in the normal direction -
since regularization has propagated refinement from the wall layer to the outer layer. FIGURE
7.7 (b)
insertion and
regularization.
represents a typical mesh configuration after boundary layer
FIGURE 7.7
Boundary layer regularization (a) and resulting mesh configuration (b)
l It is now possible to move all the vertices located inside the boundary layer region along their
edges normal to the wall, without altering the mesh topological configuration. In particular, the
wall layer cell size and the geometric progression of the stretching ratio are prescribed by the
user, and boundary layer vertices are moved accordingly, as shown in FIGURE 7.8.
FIGURE 7.8
Boundary layer vertices repositioning
Hence, mesh quality is improved by reducing the number of hanging vertices and by allowing a
smooth stretching progression from the wall layer to the outer layer. In addition, the boundary
vertex snapping problem on curved boundaries is also solved. Indeed, all the boundary layer
vertices aligned with the projected boundary vertex are now also moved in order to satisfy the
prescribed stretching ratio progression, thereby avoiding the occurrence of negative volumes, as
shown in FIGURE 7.9.
FIGURE 7.9
Solid surface reconstruction and boundary layer regularization
7.3.3
Viscous mesh adaptation
During the h-type mesh adaptation process, it is necessary to ensure that the boundary layer
remains semi-structured, with a bounded number of elements and without negative volumes.
Therefore, refinement in the direction tangential to the wall is strictly prohibited in the boundary
layer regions, whereas the regularization step is applied to propagate refinement in the normal
direction from wall layers to outer layers, hence avoiding the occurrence of any hanging vertex in
this direction. Finally, newly snapped boundary vertices and their associated aligned vertices are
repositioned according to the original boundary layer properties, i.e. first cell size and stretching
ratio progression, specified in HEXPRESS™.
CHAPTER 8.
OPTIONAL MODELS
This chapter describes the following physical modules in FINE™/Open with OpenLabs™.
In this section
8.1 Combustion Modeling
8.2 Radiation Modeling
8.3 Porous Media Model
8.4 Fluid Structure Interaction
8.5 Fluid-Particle Interaction
8.6 Cavitation
8.7 Multi-Species Framework
122
141
159
162
166
191
200
8.1
COMBUSTION MODELING
This section describes the theory for the simulation of combustion.
8.1.1
Non-premixed Combustion
A. Overview
In general, combustion problems are characterized by a strong variation of density. Since
combustion in most technical applications takes place at low speeds, the density variations are not
caused by the variation in the pressure, but by the heat released from the exothermic reaction
between fuel and oxidizer. Most technical combustion problems can therefore be simulated with
models developed for low Mach number flow. From a mathematical point of view this means,
that the pressure variations in the flow have to be small compared to the thermodynamic
background pressure of the system. Based on this definition, even systems with a transient
background pressure (e.g., internal combustion engines) can be modeled as low Mach number
problems.
In the most general approach, combustion is described as a convection-diffusion-reaction problem
involving n species and m reactions between these species as described by a reaction mechanism.
A direct simulation of the chemistry involved in combustion would therefore lead to a coupled set
of n+4 equations, namely the continuity equation, the momentum equations, the energy equation
and the balance equations for the i = 1, .., n-1 species.
where Yi denotes the mass fraction of the i-th species, Di is it's diffusivity and
source term. Although the solution of this system would describe arbitrary types of combustion
problems (non-premixed, premixed, partially premixed), its solution would be too expensive for
industrially relevant CFD studies:
is the chemical
l The resulting set of partial differential equations can be very large. For instance state-of-the-art
reaction mechanisms for methane contain 53 species subject to 325 elementary reaction steps;
to solve this system a system of 57 transport equations for the flow would need to be solved.
Note that a reaction mechanism for realistic fuels is even bigger.
l Due to the wide range of time and length scales involved the problem is stiff.
l In the case of turbulent flows, the treatment of the averaged source terms in the species
equations is very difficult.
It is therefore much more efficient to exploit certain characteristics of the flame type under
consideration and to simplify the problem in a suitable way. In the case of diffusion flames (i.e.,
non- premixed combustion) fuel and oxidizer are entering the problem domain by separate
streams. In order to react, both components must first be mixed on a molecular level. For many
applications it can be assumed that the chemical reaction is much faster than the mixing process.
In such cases the mixing is the overall rate determining process. With the mixed-is-burned
hypothesis, it is assumed that as soon as mixing is accomplished, reaction takes place in a
practically infinitely fast manner ("mixed=burnt" hypothesis). The idea is now to split the
combustion problem in two subproblems: the first being the global mixing and the second being
the description of the local composition/flame structure. Both subproblems can be described in
terms of the mixture fraction f, which is the central quantity for non-premixed combustion.
B. Mixture Fraction
Non-premixed combustion processes can be parameterised by the mixture fraction variable based
on the assumption that all species involved have equal diffusivities and that the combustion
processes is limited to configurations with two distinct inlet streams – one inlet for the oxidizer
and one inlet for the fuel.
A general way to define the mixture fraction f is to employ the atomic elements. While the mass of
chemical species may change due to chemical reactions, the mass of elements is conserved. The
mixture fraction can be written in terms of the atomic mass fraction as:
where Y i is the mass fraction of element i; The subscript ox denotes the mass fraction at the
oxidizer stream inlet and the subscript fu denotes the value at the fuel stream inlet. If diffusivity of
is identical for all elements. Any linear
the species is assumed equal, then the mixture fraction
combination of atomic elements that distinguishes the fuel stream from the oxidizer stream can be
used to trace the mixing process. An often used definition of the mixture fraction for describing
the combustion of hydrocarbons, is a definition of Bilger (1998), where a linear combination of
the mass fractions of oxygen, hydrogen and carbon is used.
Under the assumption of equi-diffusivities, the species equations can be reduced to a single
. The reaction source term in the species equations vanishes.
equation for the mixture fraction
The transport equation for the mixture fraction f can be expressed as follows:
where D is the diffusivity of mixture fraction. For gaseous fuels, the Schmidt number can be
assumed as constant. In this case, the diffusivity connects to the Schmidt number via the following
relation:
where
.
Defining the Lewis number:
, where α is the thermal diffusivity. If Lewis number
unity is assumed in addition to equi-diffusivity of the species, then the mixture fraction f is not
. For
only a suitable means to represent the transport of species but also the chemical enthalpy
an ideal mixture the chemical enthalpy is defined as:
with
Assuming that the combustion systems are in steady-state, that radiative heat sources can be
neglected and that the work of the viscous forces can be ignored, the energy equation simplifies
to:
After a normalization the transport equation of enthalpy can thus be described by the same PDE
as the transport equation of the species. The mixture fraction can be used to parameterize the
mixing process and thus the combustion process.
C. Chemistry Models
When the mixture fraction approach is used, one needs a description of the flame structure, i.e.,
how the thermochemical properties are related to the mixture fraction variable. In FINE™/Open
with OpenLabs™ two different approaches are available: the equilibrium model and the flamelet
model.
Equilibrium model
The first approach is based on the assumption of chemical equilibrium, where it is assumed that
the time scales related to combustion are infinitely much faster than those of the flow and mixing.
With this approach it is assumed that the fuel/oxidizer mixture in each point is able to reach the
state of chemical equilibrium and the flame is not influenced by the flow. For given conditions of
the fuel and oxidizer streams in an adiabatic combustion chamber, the temperature and chemical
composition as well as all transport coefficients depend solely on the elemental composition and
thus only on the mixture fraction when the equilibrium approach is used:
,
,
,
,
,
, ......
To save computational time, the functional dependencies of the thermo-chemical properties of the
mixture fraction are pre-calculated in a pre-processing step and stored in look-up tables. The look-
up tables of the chemical equilibrium states are read by FINE™/Open with OpenLabs™ at start-
up and the content is stored in memory during the computation. The stored data are accessed
using linear interpolations during the computation of the flow solver.
Flamelet Model
The flamelet model incorporates non-equilibrium effects brought by the influence of the flow on
the combustion. These non- equilibrium effects are mainly important when looking at
the
concentrations of minor species, especially when pollutant formation (NOx, CO, UHC etc.) is of
interest. The underlying idea of the flamelet concept is, that a flame (laminar or turbulent) can be
viewed as an ensemble of flamelets (small flames) embedded in the flow field and are subject to
strain from the flow.
These flamelets are modeled as idealized counter-flow diffusion flames in which fuel and oxidizer
are fed through two opposing nozzles. The flame is then located in the stagnation plane between
the jets. Such a configuration can be simulated as a quasi one-dimensional diffusion flame in a
separate detailed chemistry code. By tabulating the thermo- chemical properties along the
centerline from the oxidizer inlet to the fuel inlet in dependence of the mixture fraction, a look-up
table can be constructed.
The flamelet approach has the advantage over the equilibrium approach, that it can account for the
effect that a strained flow field has on the flame structure. By simulating counter-diffusion flames
for a set of different strain rates, the thermo- chemical properties can be tabulated both in
dependence of the strain rate a and the mixture fraction f:
,
,
,
, ......
,
,
The strain in the simulated flamelets can be varied, by changing the speed of the fuel/oxidizer
streams while keeping the distance between the nozzles fixed. An important parameter to
characterize the influence of the flow field on the flame-structure in non-premixed combustion is
the scalar dissipation rate χ, which either can be interpreted as the inverse of a characteristic
diffusion time scale imposed by the flow field or as the rate with which variations in the scalar
field is destroyed. The scalar dissipation rate is proportional to the strain rate in a flame; for
counter-flow flames where the oxidizer and fuel streams are located sufficiently far away so that
potential flow situation can be assumed, the strain rate and the scalar dissipation rate are related
via
The strain rate is constant for a given flamelet, which makes this parameter suitable to characterize
the flamelets in the flamelet library. The scalar dissipation χ is not a constant but varies with the
mixture fraction within a given flamelet. The local flow field value is related to the combustion
look-up tables via the scalar dissipation rate, as this parameter characterizes the local combustion
process. After that the scalar dissipation rate is calculated for a given point/cell in the flow field,
the flamelet tables are looked up by the local value for the mixture fraction together with a strain
rate that was calculated from the scalar dissipation rate.
For laminar flows the scalar dissipation rate is defined as:
With the steepening of the gradients of the mixture fraction in a flow field, the transport of heat
and intermediate products away from the flame is increased. This causes a reduction of the flame
temperature and reduction of the concentration of the products. If the scalar dissipation rate is high
enough, the straining of the flame will quench the flame and cause local extinction.
D. Turbulent Combustion
In engineering practice the effect of turbulence on the combustion is often modeled by statistical
methods. In the current implementation, non-premixed, turbulent combustion is simulated by the
use of the Reynolds- averaged Navier- Stokes (RANS) in conjunction with two- equation
turbulence models and Reynolds- averaged transport equations for mixture fraction and its
variance.
The Favre-Reynolds averaged transport equation for mixture fraction reads as:
where Dt is the turbulent eddy diffusivity and is determined in dependence of the eddy viscosity
via the turbulent Schmidt number
:
The turbulent Schmidt number is lying in the range between 0.4 and 0.9. In FINE™/Open with
OpenLabs™ the turbulent Schmidt number is by default set to 0.7.
Although the molecular diffusivity of mixture fraction is often small compared to its turbulent
counterpart, it is not neglected as it may have some influence. It should be noted that the transport
coefficients of combusting gaseous fluids typically increase by one order of magnitude in the
course of the reaction due to a temperature increase.
To account for the turbulence-chemistry interaction, the mixture fraction variance needs to be
is solved for
determined. For this reason a transport equation for the mixture fraction variance
turbulent flows. Defining
, a transport equation for the mixture fraction variance can be
expressed as:
The second term on the r.h.s. represents the production of scalar fluctuations due to the presence
of a gradient in the mean mixture fraction field. The third term is the mean scalar dissipation rate,
which for turbulent flows is modeled by:
It is modeled in terms of the inverse of the turbulent time scale τ whose exact definition depends
on the turbulence model employed. For the standard k-ε turbulence model this term is determined
by
The constant
is by default set to 2.
Turbulence-Chemistry Interaction – Presumed PDF
In most technical applications in which combustion processes take place, the governing flow is
turbulent. Turbulent flows are characterized through a cascade of vortices, which is responsible
for the appearance of large spatial and temporal fluctuations in the velocity, density, temperature
and concentrations.
Since combustion has a highly non-linear nature, simple linear averaging of fluctuating variables
in the numerical model would lead to large modeling errors. Due to the non-linear dependence
between the thermo- chemical properties and the mixture fraction, a direct look- up of those
quantities in the combustion tables by means of the Favre-Reynolds averaged value of the mixture
would not be accurate. To both properly account for the fluctuations that
fraction variable
scalars may have in turbulent flow and the non-linear dependence between the scalars and the
mixture fraction, probability density functions (PDF) should be used. A probability density
function P(f) for the mixture fraction variable describes the probability that the flow field takes in
a certain value for the mixture fraction at a given point. As soon such a function is known, these
functions can be used to obtain the proper averaged thermo- chemical states by means of
integrating the state-functions with the probability density function over the complete physical
range
of the mixture fraction:
,
The resulting integral does not need to be normalized, as the integral of the PDF over all possible
states by definition has to equal unity:
The PDF can be obtained by solving PDF transport equations. This method implies the use of
stochastic methods and is computationally very expensive. In FINE™/Open with OpenLabs™
instead a presumed PDF approach is used which is computationally more efficient. As the name
of the method suggests, the shape of the PDF is presumed and the distribution is parameterised via
its statistical moments. In this approach, it is presumed that the functional form of the probability
density function can generally be represented by β-functions. The probability density function is
defined as:
where a and b are given by
.
The probability density function is parameterised in dependence of the mixture fraction and its
variance at each point of the flow field. The β-PDF has the advantage that it can exhibit a bimodal
shape behavior for large variances. This means that the function can account for the coexistence
of fuel and oxidizer in turbulent flows. For typical intermediate values of the variance, the
function represents a Gaussian distribution, while it in the limits of a vanishing variance represents
a Dirac function. The latter property ensures, that the averaged quantities
with
equals the corresponding laminar quantities
in the absence of variances.
In practice, the evaluation of the integral in above equation in each iteration for every cell would
cause a significant computational overhead in the CFD solver. For this reason, the distributions in
the laminar combustion look-up tables are integrated with the corresponding PDF and restored for
discrete values over the complete physical range of the mixture fraction and its variance
. This pre- processing treatment is called pre- integration and
,
results in combustion look-up tables that in addition to the dimensions of the laminar combustion
look-up table have the mixture fraction variance as a new dimension.
8.1.2
Premixed Combustion
A. Overview
Purely premixed combustion takes place when fuel and oxidizer are completely mixed at the
molecular level before combustion is allowed to take place. Premixed flames propagate due to
heat conducted from the burned hot products to fresh cold reactants. This is opposed to non-
premixed flames, where the flame develops due to mixing/diffusion of oxidizer and fuel.
Premixed flames are therefore wave phenomena and non- premixed flames are diffusion
phenomena (and are also often called diffusion flames). In Premixed flames combustion takes
place in a thin reaction zone separating reactants and products.
B. The Bray-Moss-Libby Model
Premixed flames can be modeled by either a G-equation, which tracks the flame front, or by
models based on solving a transport equation for a normalized progress variable, where the flame
front is resolved by means of a convection-diffusion equation. In the current model the latter
approach is chosen. This widely used concept in premixed turbulent flames assumes that chemical
reactions are localized in a thin surface which may be represented as a sheet separating unburnt
mixture from burnt gas. The formulation is based on introducing a progress variable field. In this
approach, the state of the mixture (burnt or unburnt) is expressed in terms of a progress variable .
The progress variable is a normalized quantity which is usually defined as c* = 0 when the
mixture is completely unburnt, and as when the mixture is completely burnt c* = 1. The reactions
are assumed to be fast and the reaction zone therefore to be thin.
The normalized progress variable c* can be defined as a normalized temperature:
where
and
describe the temperature of the unburnt and burnt (adiabatic flame temperature)
mixture.
The general transport equation for the Favre-averaged progress variable reads as:
where
is the source term and D t is the turbulent eddy diffusivity and is determined in
dependence of the eddy viscosity via the turbulent Schmidt number
:
The turbulent Schmidt number is lying in the range between 0.4 and 0.9. In FINE™/Open with
OpenLabs™ the turbulent Schmidt number is by default set to 0.7.
C. Modeling the Source Term
Zimont Model
Zimont et al. (1998) proposed a closure for the reaction source term using the turbulent flame
speed (Turbulent Flame Speed Closure or TFC model) and the gradient of the progress variable.
is density of the unburnt mixture and
In this model,
is the turbulent flame speed. The
Zimont follows the idea that small scale turbulent structures enhance the transfer inside flamelets
and determine their thickness and propagation velocity while large scale turbulent vortices wrinkle
the thickened flamelets and control the width of the average combustion zone. The resulting
expression for the turbulent flame velocity is:
where α is the thermal diffusivity of the unburnt mixture.
is the laminar flame speed, which is
property of the mixture. For a one-stream premixed configuration, the stoichiometry is constant
is turbulent fluctuating velocity
and the temperature of the inlet stream is constant.
and
is the turbulent integral length scale. The constant A=0.52 is recommended and determined
using experiment.
Zimont model with modifications of Dinkelacker
The group of Dinkelacker et al. (S. Pfadler) has proposed an algebraic reaction rate closure based
on a comparison with experimental data on 101 turbulent Bunsen flames. The TFC model by
Dinekelacker determines the turbulent flame speed as follows:
where Le is Lewis number and Ret is the turbulent Reynolds number.
Lindstedt-Vaos Model
The third model offered in FINE™/Open with OpenLabs™ is the Lindsted-Vaos model (2004),
which is read as:
with the constant C
= 2.6 and the Kolmogrov velocity
, where
is the kinematic
viscosity of the unburnt mixture.
In the absence of turbulent fluctuations (
the Zimont model and the Lindstedt-Vaos model give
.
), the Dinkelacker model gives
while both
For laminar simulation, all models are still available by replacing
with
.
D. Calculation of the gas density and the gas temperature
The temperature of the gas is a simple algebraic function of the progress variable that can be
directly obtained from the definition of the progress variable and is given as
where T u is the unburnt 'cold' premixed gas temperature and T ad is the adiabatic flame
is a constant in purely premixed combustion. The
temperature. The expansion ratio
gas density can be calculated by applying the ideal gas law and can be written as:
8.1.3
Partially-premixed Combustion
A. Overview
The mixture fraction modeling approach in conjunction with flamelet tables is recognized as a
reliable and accurate method for the simulation of diffusion flames. As the flame-structure is
calculated in a preprocessing step and thus the chemistry calculations can be kept outside of the
flow solver,
this method has the advantage of being efficient. Due to the fast chemistry
assumption which is only partially relieved by accounting for the effect of strain, this method is
however limited to the use for non-premixed flow. A fruitful approach in the development of a
reliable combustion model that both can handle non-premixed and premixed situations, seems to
be to use a manifold-based modeling technique, like the Flamelet Generated Manifolds (FGM)
method. This approach employs tabulated chemistry in conjunction with transport-equations for
the mixture fraction and one or several progress variables. Solution to dimensional progress
variable is weighted sum of product species. These values are read from tabulated manifold which
are typically chemistry based. In the Hybrid BML/Flamelet partially premixed model solution of
normalized progress variable can be viewed as a normalized temperature. The source term is
modeled as a function of the laminar flame speed, k and epsilon. Laminar flame speed is a
function of equivalence ratio which depends on chemistry. An FGM table can be used, but also
specific "hybrid BML/flamelet" table consisting of a burning and a non-burning flamelet. In the
case that FGM table is used, the source terms are not read from table.
B. Governing Equations
In the present approaches, the RANS-equations are solved together with a transport equation for
the mixture fraction f and its variance g. A transport equation for the progress variable c is solved
to parameterize the evolution of the overall reaction. It is assumed that the variance of the progress
variable plays a negligible role in the turbulence-chemistry interaction compared to the variance of
the mixture fraction.
The governing equations read as
with the velocity vector
, the density r, the effective stress tensor
, the source term of the
progress variable
, the turbulent kinetic energy k and its dissipation rate ϵ. The density ρ, the
source term
, and the molecular dynamic viscosity μ are determined via look-up tables of the
form
For the case that equilibrium or flamelet tables are used, the governing transport equations are the
same, except that no transport equation for the chemical progress is solved. If the latter approach
is used, the combustion tables are looked up with the strain rate a instead of the progress variable
as a parameter.
C. Flamelet Generated Manifolds technique
In this section, the principles behind the construction of the FGM table is explained. The idea of
the FGM method is to construct a manifold based on a set of flamelets. The flamelets can either
represent a non-burning, a premixed propagating or a stretched non-premixed burning flame. The
FGM tables are built either from a library of premixed or from a library of non- premixed
flamelets.
Premixed flamelet generated manifolds
Premixed FGM are based on a library of premixed flamelets, with each flamelet corresponding to
a different mixture fraction. The main step in the construction of the manifolds consists of
mapping the thermochemical states of each flamelet on a grid that spans the complete physical
range of the mixture fraction f and the progress variable c. The progress variable is typically
defined as a linear combination of the intermediate species and the products. Vreman et al. (2008)
suggest using the following definition
where
and
represent the mass fraction and the molar mass of species i, respectively. It is
essential to take a combination of species, so that the progress variable is monotonously increasing
along each flamelet.
It should be noted that since the mixture of fuel and oxidizer in the regular case are not flammable
for the complete range of physical values of the mixture fraction, an interpolation has to be carried
out for the states with a mixture fraction lying between the pure oxidizer (f = 0) and the lower
) as well for the states having a mixture fraction between that of the
flammability limit (
upper flammability limit (
) and that of the pure fuel (f = 0).
Non-premixed flamelet generated manifolds
Non-premixed FGMs are created from a library of burning steady-state non-premixed flamelets
and one unsteady extinguishing flamelet. A steady flamelet library, which is used as a basis for
the construction of a non-premixed FGM, is containing flamelets ranging from a negligible strain
until a strain rate, which lies close to that of the quenching limit. To fill the state-space between
the steady burning flamelet subject the highest possible strain before extinction and the limit of an
unburnt mixture of fuel and oxidizer, the thermochemical states of an unsteady flamelet are used.
The necessary unsteady flamelet for the generation of a non-premixed FGM is created using the
steady flamelet for the highest strain as initial solution and by prescribing a strain rate that lies
slightly above the quenching limit, so that the flame successively dies. After a suitable definition
of the progress variable has been found, the flamelet library is remapped onto a two-dimensional
grid spanned by the mixture fraction and the progress variable.
Filling the non-equilibrium part of the reaction domain with the solution of an unsteady flamelet
leads to non-smoothness in the manifold. However, the incorporation of an unsteady flamelet may
be advantageous, as unsteady flamelets are known to predict intermediate species and slow
chemistry well. In addition, it should be noted, that a library of premixed flamelets in general does
cover a smaller part of the state space than the set of flamelets used for the construction of a non-
premixed FGM.
Turbulence chemistry interaction
To account for the turbulence chemistry interaction, the presumed b-PDF approach is used. In
order to be able to pre-integrate the combustion look-up tables, they must first be transformed onto
a square domain in the independent variables. This is achieved, by re-mapping the flamelets onto
the normalized progress variable:
With this transformation, the thermochemical states are defined on a square domain with mixture
fraction and the normalized progress variable as independent parameterizing variables, both going
from zero to unity on the whole physical domain. In the present approach statistical independence
of the mixture fraction and the normalized progress variable is assumed. It is furthermore assumed
that the fluctuations in the normalized progress variables are negligible. After the pre-integration,
the tables depend consequently on the mixture fraction f, its variance g and the normalized
progress variable c*. Since the transport equations are still solved for the non-normalized progress
variable c, a normalization of the latter solution variable is needed, before the combustion tables
can be looked up.
D. Hybrid BML/Flamelet Technique
The difference between the FGM technique and the hybrid BML/Flamelet model is in the source
term closure. In the Hybrid BML/Flamelet model source term in the transport equation for the
progress variable and variance of the progress variable are closed using a BML type model.
The main difference between a premixed and a partially premixed flame is that in a premixed
flame, the equivalence ratio is constant. In a partially premixed flame the equivalence ratio of the
mixture can vary spatially. This means that the laminar flame speed, the combustion products and
the density are now a function of the local equivalence ratio.
The equivalence ratio can be expressed in terms of the mixture fraction f
where
is the stoichiometric mixture fraction. In partially premixed flames, the transport
equation for the mixture fraction and turbulence-chemistry interaction is taken care by mixture
fraction variance equation.
In Equilibrium chemistry, the thermochemical properties are obtained from an equilibrium table
. In a partially premixed flame these properties
containing the thermochemical properties
are obtained using a linear interpolation between the retrieved states from an equilibrium table and
the retrieved states from a mixing table.
Laminar Flame Speed for Hybrid BML/Flamelet Model
To obtain the laminar flame speed in a partially premixed flame, a possible method is solving the
reaction equations for a one-dimensional premixed configuration and determine the laminar flame
speed as the solution of the eigenvalue problem. Another approach to obtain the laminar burning
velocities is by constructing polynomial fits to experimental data.
The Polynomial is preferred because it is accurate near the flammability limits and does not
depend on the presence of the laminar flame speed in the table. Polynomial fits for several fuel
types have been reported in the study of Metghalchi and Keck. For different pressure and unburnt
temperature, the correlation function of Metghalchi and Keck is being used:
with
=298K,
=1 atm. and where the exponent are computed by:
The coefficients are fuel-independent and are provided by Metghalchi and Keck (1982):
= 2.18,
= -0.8,
=-0.16,
= 0.22
The
coefficients
,
,
,
are
controlled
by
the
expert
parameter
combEquRatioCorrCoefs_.
This model was tested for methane, ethylene and propane fuels with pressures varying between 0.
and 1 MPa. The reference laminar flame speed is given as a function of the equivalence ratio:
with the fuel dependent constants provided by measurement and given in the paper of Metghalchi
and Keck for several fuel types. In this expression, A represents the maximum laminar flame
speed, which occurs at the equivalence ratio ϕ = C. The constant B is found using a nonlinear
least square fit through the experimental data or detailed calculation results.
Gulder proposed an experimental correlation of the form:
where A, B, C and D are constants and correlation for laminar flame speed are fit for different
fuels as function of equivalence ratio based on experimental data. In this case laminar flame speed
is maximum at equivalence ratio 1 and roots at the flammability limits.
Parabolic options can be used for Laminar flame speed for unknown fuel-air mixture. The laminar
flame speed at stoichiometric fuel-air ratio can be obtained from the chemistry table or from
literature. Flammability can also be obtained from literature or experimental data and parabolic
curve can fit for laminar flame speed as function of equivalence ratio.
Flammability limits
When the equivalence ratio ϕ is very high or very low, the flammability limits are reached and the
.
flame can extinguish. (for methane, the flammable region is approximately
Outside of this region, the flame becomes unstable and can extinguish.
The polynomials of Metghalchi and keck gives a flame speed of zero at two equivalence ratio,
which will be taken as the flammability limits. Outside of these limits the flame speed is zero and
no flame can exist.
8.1.4 NOx formation
Overview
In combustion processes, the formation of nitrogen oxides (NOx) is one of the major pollution
sources. Although nitrogen oxides encompasses the three species NO (nitric oxide), NO 2
(nitrogen dioxide) and N2O (nitrous oxide) in high temperature combustion the major pathway to
NOx leads through NO. It is thus the nitric oxide which will be considered in the combustion
model. The nitric oxide can in principle be formed via three mechanisms: (a) Fuel-bound NO,
which is not present for pure hydrocarbon fuels; (b) Prompt NO, which is formed in fuel rich
regions of the flame; (c) Thermal NO, which is the prevailing mechanism in high temperature
combustion. The relative importance of prompt vs. thermal NO can be low in many applications
such as high temperature furnaces with long residence times, but might become large in modern
NOx-reduced combustion devices operating under conditions where much of the thermal NO has
been already eliminated. We focus here on a description of the thermal formation.
Thermal NO formation in laminar combustion
The kinetics of thermal NO formation are described via the Zel'dovich mechanism:
Of these reactions, the first one is the rate determining due to the large energy needed to break up
the triple bonds in the N2 molecules. It becomes relevant only at temperatures above 1700-1800
K, which are often found in near-stoichiometric conditions. Since all of the reactions involved in
here are slow compared to the oxidation of the fuel and the concentrations of the species involved
are very low, the NO formation can be considered decoupled from the main combustion. Based
on a simulated flow field, one can solve an equation for the mass fraction of NO in a
postprocessing mode:
The source term for the formation NO now can be expressed using the kinetic data for reactions 1
to 3. In a homogeneous system with a reaction A+B -> C taking place, the concentrations of the
species involved evolve like:
where [  ] denotes the molar concentration, ρY i /M i and r is the reaction rate. This rate is
proportional to the concentration of the partners involved:
where the rate coefficient k can be expressed as follows by Arrhenius law:
The coefficients involved in this expression are the pre-exponential factor A, the temperature
exponent β and the activation energy E α. Instead of using the activation energy, an activation
temperature
can also be used.
In reversible reactions such as the ones contained in the Zel'dovich mechanism, the respective
forward and backward reactions are governed by forward and backwards rates and their
corresponding coefficients kf and kr.
Employing these relations for the production rate of NO gives:
where now
Many different sets of kinetic data are available in the literature. Here the recent data from
Bockhorn (1990) is chosen and listed in the following table.
Reaction A β TA
1f: N2+O -> NO+N 1.80E+11 0 38367
1r: NO+N -> N2+O 3.98E+10 0 504
2f: N+O2 -> NO+O 6.40E+06 1 3160
2r: NO+O -> N+O2 1.36E+06 1 19235
3f: N+OH -> NO+H 3.00E+10 0 0
3r: NO+H -> N+OH 8.12E+10 0 24125
All of the rates depend besides a respective coefficients only on the temperature, which in turn is a
function of mixture fraction. Since also all the concentrations are functions of mixture fraction,
one can also write
Thermal NO Formation in Turbulent Combustion
For turbulent combustion, the NOx modeling has to be incorporated into the concept of presumed
PDFs applied for the basic combustion model. Since in the turbulent case mean values are being
considered, we also require now the Favre averaged NO formation rate:
Due to turbulence-chemistry interaction, the average NO formation rate cannot be determined by
using the mean NO concentration. Rather, the integration over the joint PDF P(f, YNO) yields the
proper NO source term.
where we already use the normalized NO concentration. The question is now how the joint PDF
of mixture fraction and NO concentration can be modeled. Since the NO chemistry is very low,
the fluctuations of NO are not correlated to the mixture fraction fluctuations, i.e., the joint PDF
can be expressed as the product of the two marginal PDFs of mixture fraction and NO
concentration:
For the mixture fraction it is logical to stick to the β-function formulation. For the NO mass
fraction, the simplest approach here is to neglect fluctuations of NO and employ a δ-function PDF
This approach has the advantage that it does not require the solution of an equation for the
variance of the NO concentration.
Prompt NO and fuel NO Formations
As mentioned above, the thermal NO is dominant in situations where high temperature and near-
stoichiometric conditions prevail. However,
in modern combustion devices (e.g., staged
combustors), the formation of thermal NO is reduced that much that the prompt NO now becomes
important. The prompt pathway involves HCN as an important species for which a concentration
equation will have to be solved. For the time being prompt NO is not included in the NO module.
This means that for certain cases NO might be under predicted if the prompt mechanism plays a
role. Further, fuel NO has not been discussed. This means that the module is not appropriate for
the prediction of the NO formation for the fuels containing NO.
8.2
RADIATION MODELING
This section describes the basic theory for the simulation of the radiation heat transfer.
8.2.1
Overview
Thermal radiative energy may be viewed as electromagnetic waves (electromagnetic wave theory)
or as energy parcels called photons (quantum mechanics). Every medium continuously emits
electromagnetic radiation at a rate depending on the local temperature and the properties of the
material. The radiative heat flux emitted is called the emissive power E. Even though the emissive
power is the natural choice to describe the radiative heat flux leaving a surface, it is not adequate
to describe the directional dependence of the radiation field,
inside an
absorbing/emitting/scattering medium. To overcome this limitation, the intensity I is normally used
and is defined as the radiative energy flow per unit solid angle and unit area normal to the rays.
in particular not
Radiative properties and variables are strongly dependent on the spectrum (frequency), especially
in gases. Therefore, one can normally distinguish between spectral and total properties (i.e.,
spectral or total intensity). The spectral dependence is noted by the frequency ν, wavelength λ or
wavenumber η as a subscript. As an example, the relation of the spectral and total intensity is
expressed as:
Two important definitions regarding the properties of a medium or surface are briefly noted:
l A gray medium or surface is defined as one for which the radiative properties are independent
of the wavelength.
l A diffusive medium or surface is defined as one for which the radiative properties are
independent of the direction.
In contrast to conduction and convection, radiation is a heat transfer mechanism that does not
need a medium for its transfer (electromagnetic waves may travel through a vacuum). Depending
on the temperature and its nature (i.e., chemical species involved, presence of particles), a medium
can be considered participating or non-participating. In combustion environments, radiation heat
transfer may be relevant because of the presence of highly radiative species (i.e., H2O, CO2) and
particles (i.e., soot).
In a participating medium the intensity of the rays that travel through can be absorbed, emitted,
and scattered:
l The absorptivity α is defined as the fraction of the incident energy I on a body that is absorbed
by the body. If the scattering can be neglected, the absorptivity of a homogeneous isothermal
, where κ is the absorption coefficient and s is the
medium can be written as
path length. Absorbed energy is converted to internal energy.
l The emissivity ϵ specifies how well a real body radiates energy as compared with a blackbody
(theoretical emission of a surface that does not reflect any incident radiation-
emission
perfect absorber). The blackbody emission is
, where the Stefan-Boltzmann
constant σ has the value
.
l Scattering occurs when a particle changes the direction in which a photon travels. Out-
scattering (away from the direction under consideration) attenuates the intensity in a given
direction since accounts for the part of the incoming intensity removed from the direction of
propagation. This intensity is simply redirected and appears as augmentation along another
direction, also known as in-scattering. Out-scattering is proportional to the magnitude of the
. On
incident energy I, being in this case the proportional constant the scattering coefficient
the other hand, in-scattering has contributions from all directions and, therefore, is calculated
that describes the probability that a ray
integrating over all solid angles. A function
from one direction
is scattered into the direction under consideration
is required. This
function is known as the scattering phase function. Note that scattering is a redistribution of
energy.
The total attenuation of the intensity by both absorption and out-scattering is known as extinction
and an extinction coefficient β is defined as:
The optical thickness based on the extinction coefficient is defined as the linear integral of the
extinction coefficient along a path s:
This quantity is a good indicator of the model to be chosen for each problem. A very simplified
explanation of it would that a medium for which is difficult (or not possible) to look through is
optically thicker than a medium for which one can look through without difficulty. In order to
make a rough estimation of the optical thickness of a certain problem, it can be approximated by:
where Lref is a reference length of the problem (e.g. diameter of the computational chamber). The
criteria commonly used is that if τ < 1 the medium is considered to be optically thin while if τ > 1
the medium is considered to be optically thick.
Finally, the incident radiation G is defined as the integral over all solid angles 4π:
8.2.2
Radiation with participating media
A. Radiative transfer equation
In order to write an equation for the radiative transfer, a balance on the radiative energy traveling
is done. The change in intensity is found by summing the contributions from
in the direction
emission, absorption, scattering away from the direction
(out-scattering) and scattering into
direction
(in-scattering):
This is an integro-differential equation in five independent variables, three space coordinates and
two direction coordinates. The problem becomes even more complicated if the medium is non-
gray, which introduces an additional variable such as wavelength or frequency and makes the
equation non-linear. This means that the spectral nature of the properties requires also integration
over the spectrum to evaluate the total quantities. Several approaches to solve this equation are
proposed in the literature, with the Discrete Ordinates Method (DOM) being the most popular
one.
In the context of the solution of the Navier-Stokes equations accounting for radiation heat transfer,
the relevant information that is introduced in the energy equation is the radiative heat flux. The
total radiative heat flux vector is defined as an integral of the spectral radiative heat flux over the
entire spectrum:
Radiation can also be seen as a (volumetric) source term ST in the energy equation. In that case,
one can simply take the divergence:
B. P1-Model
The idea behind this method is to convert "" (p. 144) into a set of partial differential equations.
The radiation intensity field
at location
can be viewed as the value of a scalar function
on the surface of a sphere of unity radius, surrounding the point
. Such a function can be
expressed in terms of a two-dimensional generalized Fourier series:
where
are position-dependent coefficients and the
are spherical harmonics,
given by:
that satisfy Laplace's equation in spherical coordinates. Here, θ and ψ are the polar and azimuthal
are associated Legendre
angles describing the direction of the unit vector
, respectively, and
polynomials.
If the Fourier series is truncated beyond l=1 the lowest order approximation of the spherical
harmonics method is obtained. This method is known as P 1 - approximation. The following
expression for the intensity can be written:
The associated Legendre polynomials required are
,
,
.
Using the definition of the incident radiation G and the radiative heat flux , the truncated Fourier
series becomes:
Assuming linear-anisotropic scattering, the phase function can be expressed as:
where C is the linear-anisotropic phase function coefficient. Introducing the result of the intensity
and integrating over all solid angles, the
into the radiative transfer equation, multiplying by
following equation can be written:
Here, the single scattering albedo coefficient ω has been used. This coefficient is defined as
.
Additional equations can be obtained by algebraic manipulation. Here, and for the sake of brevity,
an equation is written without deduction:
Combining the last two equations, an equation for the incident radiation can be obtained:
In contrast, this is a differential equation instead of an integro-differential equation. To be precise,
this is a Helmholtz equation, elliptic in nature, and closely related to Laplace's equation.
Given appropriate boundary conditions, this equation can be used to solve the incident field G.
can be computed. In addition, and using this
From previous equation the radiative heat flux
equation, the divergence of the radiative heat flux
can be also evaluated. As mentioned
above, this is the relevant quantity for the coupling of the radiative heat transfer with the energy
equation.
Boundary conditions need to be specified to solve the incident radiation equation . For wall
boundaries, the following boundary condition is used:
where ε is the local surface emissivity and Ibw is the blackbody intensity at the wall temperature.
is the unity vector normal to the boundary surface. It must be noted that, since
is normal to the
boundary, its dot product with the gradient of G will become the gradient normal to the
.
For inlet and outlet boundaries, the same equation can be used. In that case, the emissivity ε can
be considered, in general, 1.0 (as a black body). The temperature of the fluid at the inflow and
outflow boundaries is taken to compute in this case.
C. Optically Thin Model (OTM)
For media that can be considered optically thin a very simple model can be applied. The model
assumes that each radiation point has an impeded isotropic view of the surroundings. Then, self-
absorption and scattering can be considered negligible compared to the emission. With these
assumptions, the source term for the energy equation can be expressed as follows:
with
absorption coefficient of the mixture and
as the Planck-mean absorption coefficient of the mixture,
as the incident-mean
as the temperature of the surrounding (e.g., the wall
temperature of the combustion chamber).
To evaluate the Planck- mean and incident- mean absorption coefficients of the mixture, the
following relations are applied:
with
as the partial pressure,
as the Planck-mean absorption coefficient and
as the
incident-mean absorption coefficient of species i. An approximate expression for the incident-
mean coefficient is given in dependence of the Planck-mean coefficient:
In combustion environments, the radiative species considered in order of importance are mainly
CO 2 and H 2O, and in less extent CH 4 and CO. Here the contributions of CH 4 and CO are
neglected. The Planck-mean absorption coefficients for these species can be predicted using a
narrow band model. These coefficients are function of the temperature:
For CO2 and H2O:
c0
c1
c2
c3
c4
c5
18.741
-121.310
273.500
-194.050
56.310
-5.8169
-0.23093
-1.12390
9.41530
-2.99880
0.51382
-1.86840e-05
CO2
H2O
D. Finite Volume method (FVM)
The FVM model is a more general approach than the OTM and P1 and it is applicable to all the
range of optical thicknesses. In the limit, and by applying a very low absorption coefficient, it
could even be used for non-participating media problems (for this type of problems the angular
discretization will need to be fine enough).
In the FVM method, the spatial and angular domains are, respectively, divided into a finite
number of control volumes and control solid angles. An important discussion of the finite-volume
method for radiation and its application using 3D unstructured meshes was presented by Raithby.
Radiative transfer equation is then integrated over each control volume and control solid angle.
Volume integrals in a partial differential equation that contains a divergence term are converted to
surface integrals, using the divergence theorem. These terms are then evaluated as fluxes at the
surfaces of each finite volume. The inflow and outflow of radiant energy across a control-volume
face are balanced with attenuation and augmentation of radiant energy within a control volume
and control solid angle. The FVM formulation follows these main steps:
l The domain is divided into a number of control volumes (e.g. mesh from HEXPRESS); the
radiant intensity is located at the centre of the control volumes. The solid angle, 4π steradians,
is discretized into N = Nθ,Nφ directions (Nθ is polar angle and Nφ is the azimuthal angle)
l A set of discretized linear equations is obtained by integrating the radiative heat transfer
equation RTE over the whole domain. To close this set of equations, a spatial differencing
scheme is selected to link the radiation intensities on control volumes faces with those at
control volumes centres.
l The radiative transfer equation is solved for each direction and allows obtaining the directional
intensity Im . These directional intensities Im associated to a control solid angle are used to
evaluate the radiative source terms and wall heat fluxes.
Angular and spatial discretization
The solid angle, 4π steradians around a node centred in a control volume, is discretized into N
non overlapping control solid angles where θ is the polar angle ranging from 0 to π and φ the
azimuthal angle ranging from 0 to 2π. Control solid angles are obtained by dividing the polar
angle in Nθ angles and the azimuthal angle in Nφ angles. So, we have N= Nθ,Nφ control solid
angles. A discrete direction is associated to each control solid angle and defined by:
The subscripts m and n represent, respectively, the number of polar angles and azimuthal angles
associated to the direction. The discretization of the spatial domain may be structured or
unstructured.
Discretized equations
For a given direction, the RTE is integrated over a given control volume ΔV and a given control
solid angle ΔΩmn as follows:
To approximate integrals representing extinction, emission and in- scattering contributions,
radiation intensity and all other variables are considered constant within a given control volume
ΔV and a given control solid angle ΔΩmn. Radiation intensity is evaluated at the centre of control
volumes and at the centre of the control solid angles. All the energy of a given solid angle ΔΩmn
is assumed concentrated in the direction.
By using the divergence theorem, the integrated RTE becomes:
Σ is the control surface. For the first step of the approximation of the left-hand side of this
equation, the surface of the control volume Σ is subdivided into Nf faces of Area Aj (j = 1,…, Nf).
The second step is to consider that the radiant intensity has a unique value on each face. If the
,
radiant transfer through a given face j and within a given solid angle ΔΩmn is denoted by
the left- hand side of this equation is just the sum of
( j = 1,…, N f ). The simplest
approximation for
is:
where the radiant intensity
and the outward unit normal vector
to the surface are
approximated by their values at an integration point centrally located at the face j. The face area
associated with each integration point jp is Ap and the face outward unit normal vector at each jp
. After some intermediate calculations, a simple approximation of Eq. (8- 75) can be
is
obtained:
The directional weight can be written as:
where the control solid angle is defined as
and:
In this model, the angles are defined equidistantly with formulas Eq. (8-80) and Eq. (8-81).
Once the angular limit for each control solid angle is fixed, the directional weight, which
determines an inflow or radiant energy across the control-volume face, is evaluated as follows:
The left hand side of this equation represents the inflow and the outflow of radiant energy passing
in the direction across all the control volume faces. The right hand side denotes the attenuation
and augmentation of energy within the control volume.
For non scattering media, the Eq. (8-78) becomes:
and the Eq. (8-77) becomes:
For a given control volume and a given direction , Eq. (8-84) represents a set of equations in
which the only unknowns are the value of the intensity related to the control volume centre
and the values of the intensities
at its faces. All other variables may be known from previous
calculation. A spatial scheme is used to relate
and
.
Scattering phase function
Chu and Churchill obtained expression for scattering phase function as series in Legendre
polynomials:
Those series converge after a finite number of terms depending on the required accuracy. The
number of terms is determined by anisotropy of the phase function. The more anisotropic it is, the
more terms are required in the expansion.
The great advantage of this formulation is that once the An coefficients are determined, the value
of the phase function Φ is quickly evaluated for all scattering directions.
Isotropic scattering
For the case of the isotropic scattering, one term is considered in Legendre polynomials.
Therefore, the phase function is equal to1. It corresponds to an equal distribution of energy in all
directions. This case can be used to study scattering in mediums including particles with very
small radius compared to the wavelength. As the phase function Φ = 1, normalization condition is
obviously fulfilled:
Linear anisotropic scattering
In this case two terms in Legendre polynomials of scattering phase function are considered.
Therefore, the phase function has the following form:
If a > 0, we have forward scattering. Otherwise, we have backward scattering. With forward
scattering, emerges from the scattering medium traveling predominantly in the same direction as it
entered. Forward scattering is always accompanied by some backscattering, the proportion of the
former increasing with particle size, large particle generally have strong forward scattering peaks
due to diffraction.
Rayleigh scattering
If the particle is non absorbent, the ratio
and the refraction coefficient are arbitrary,
then the scattered intensities in both forward and backward directions are equal. This type of
scattering is called Rayleigh scattering. It applies for gas molecules and small aerosols. They are,
however also some multimolecules solid particles that fall in Rayleigh scattering regime. For
example soot particles with diameter often smaller than 10 nm and that are irradiated in
combustion application by light of approximately 3 μm. Rayleigh scattering is obtained by
considering three terms in Legendre polynomials. The phase function has the following form:
These phase functions depend only on the relative angle Ψ between the two directions (more
precisely on cos(Ψ)). Thus, these phase functions can be pre-processed before iterating and later
used in the iterative process.
E. Radiative Properties of Molecular Gases
As mentioned above, in real gases the radiative properties (i.e., the absorption coefficient) are
strongly dependent on the wavenumber (spectrum). The most accurate technique to compute
these properties is known as line-by-line. As the name suggests, the radiative transfer equation is
solved for each absorption line. However, the computational cost of such techniques is prohibitive
for practical calculations where radiation is coupled with other phenomena.
We are not interested in solving each wavenumber in detail. Therefore, global (or effective or full
spectral) properties are considered here more appropriate since the computational effort is much
lower. For this purpose, the Weighted-Sum-of-Gray-Gases (WSGG) method can be used. In this
method, the non-gray gas is replaced by a number of "fictitious" gray gases, for which the heat
transfer rates are calculated independently. The total heat flux is then found by adding the heat
fluxes of the gray gases after multiplication with certain weighted factors.
For a gray medium with
, the emissivity ϵ and absorptivity α are defined as:
where s is the path length.
Assuming that the emissivity and absorptivity may be approximated by a weighted sum of gray
gases, the following expression can be written:
where p is the sum of partial pressures of radiative species.
The temperature dependence of the coefficients ak is fitted with the following polynomials:
In addition to the temperature dependence, ak may also depend on pressure and composition. The
resulting from complete combustion of methane
following table gives the coefficients
and
(by Smith et al.). The range of validity is
[atm m],
[K].
κk
0.4201
5.516
131.9
6.508
-0.2504
2.718
-5.551
6.112
-3.118
3.029
-3.882
1.221
-5.353
6.528
-1.612
F. Coupling Radiation with Combustion
In the framework of the functionalities implemented in FINE™/Open with OpenLabs™ for non-
premixed combustion based on the mixture fraction approach, the enthalpy-defect method is
implemented to account for heat loss due to radiation or convection. With this approach, an
energy transport equation:
written in terms of the total (sensible and chemical) enthalpy is solved in addition to the mixture
fraction equation (and the variance of the mixture fraction for turbulent flows). Here, h* is the
total enthalpy and ST is the volumetric heat source term that accounts for (radiation) heat loss.
A combustion table computed for a set of heat losses is required, which means that the table has a
dimension that represents the enthalpy defect Δh*.
This energy transport equation is solved using the same method employed for the rest of
the
combustion variables . In the CFD simulation,
(without any heat loss) from
enthalpy defect is evaluated subtracting the adiabatic enthalpy
the actual enthalpy obtained by this energy transport equation:
The adiabatic enthalpy is obtained from the combustion look-up table for
. Once
enthalpy defect is determined, the desired dependent quantities (density, viscosity, temperature,
mass fraction of the species…) can be looked up in the combustion table.
It should be noted that for turbulent flows, the fluctuations of the enthalpy defect are neglected in
the current implementation and only the fluctuations of the mixture fraction are considered. This
can be expressed by the following approximation:
G. Turbulence-Radiation Interaction (TRI)
In the context of RANS turbulence modeling, the governing equation used for radiation must be
Reynolds-averaged.
In the case of P1-approximation, and neglecting scattering, the following equation can be written:
For simplicity, and to avoid extra correlations between the product of the inverse of the absorption
coefficient and the incident radiation, statistic independence is assumed (term on the left hand
side). The same consideration is made for the second term on the right hand side. On the contrary,
in the context of turbulent non-premixed combustion using the mixture fraction approach, the
emission term (first term on the right hand side) can be pre-integrated assuming the PDF of the
mixture fraction. In the following explanation, the dependence of a quantity with the temperature
(which are both direct functions of the mixture fraction), is shown
and radiative species
with
. Three possibilities have been explored for this term:
l No turbulence-radiation interaction. A simple substitution of averaged quantities is considered:
l Weak turbulence radiation interaction. The fourth power of the temperature is pre-integrated
and stored in the combustion table:
l Strong turbulence radiation interaction. The product of the absorption coefficient and the
fourth power of the temperature is pre-integrated with the PDF and stored in the combustion
table:
In the case of OTM, where only the emission term is considered, a similar consideration can be
made:
8.2.3
The S2S model
A. Overview
The S2S radiation model models the radiative heat transfer where the fluid is considered as non-
participating.
Considering the thermal radiation H impinging on a medium of finite thickness. In general, some
of the irradiation (ρH) will be reflected away from the medium, a fraction (αH) will be absorbed
inside the layer, and the rest (τ H ) will be transmitted through the slab. The reflectance,
absorptance and transmittance vary between the value of 0 and 1, which satisfy the relation as,
FIGURE 8.1
Radiation energy balance over a slab
If the medium is sufficiently thick to be opaque, then τ = 0, in which case it is called surface
radiation. The surface radiosity J can be expressed through the irradiation H and the total emissive
power E:
Making an energy balance on the surface, the radiative heat flux is expressed as:
According to Kirchhoff's law,
And assume that the surface is gray, the emittance is independent of the wavelength of the
electromagnetic waves that the surface emits. The total emissive power can be calculated as:
where
the
blackbody
emissive
power
is
calculated
by
,
and
is known as the Stefan-Boltzmann constant.
To describe the directional dependence of the radiation field, the spectral radiative intensity I is
defined. The total emissive power of the surface can be expressed as the integration of the
intensity along the total solid angle,
In which,
is the surface normal, and
is the unit direction vector which may be expressed in
terms of the polar angle θ and the azimuthal angle φ.
If the surface is a diffuse emitter, which means the intensity leaving a surface does not depend on
the direction, then the total emissive power is,
And the directional emissive power E' can be expressed by the following formula, known as the
cosine law:
B. Radiosity irradiosity method
The assumption, considering the surface as gray, diffuse emitter as well as gray diffuse reflector,
simplifies the analysis. The radiative heat transfer rates between surfaces can be calculated by
balancing the net outgoing radiation traveling directly from surface to surface (as opposed to
emitted radiation traveling to another surface directly or after any number of reflections).
The net outgoing radiation heat flux of a surface A at the location
is expressed as,
The irradiation
onto A, can be calculated by integrating the radiosity leaving from all the
other surfaces A' intercepted by A over the entire surface.
where
is view factor. The view factor between two surfaces Ai and Aj is defined as:
where L is the distance between two surfaces and
is the Kronecker delta. Using reciprocity
the irradiation equation reduces to,
Substitution into the net outgoing raidation heat flux, we get the equation relating the heat flux
and temperature:
Assuming that the temperature and heat flux are constant over each surface, the integral equation
becomes,
, i=1,2,3,...,N
It can be expressed by the matrix form,
where,
is
the
heat
flux
vector,
is the temperature vector, and the matrix coefficients are
and
.
C. Boundary Conditions
Since the fluid is radiatively non-participating, the radiative heat flux only appears in the heat
balance of the system only on the level of boundaries.
In the heat balance of
remaining
convection/conduction problem as a nonlinear boundary condition. Specifically, a change in
radiative heat flux disturbs the overall energy balance at the surface, causing a change in
temperature as well as conductive/convective fluxes.
radiative heat
flux enters
system,
the
the
the
For the boundaries with imposed temperature, the convective (or conduction) and radiative heat
fluxes are independent of one another. The radiative heat flux of these boundaries can be
calculated by solving the radiosity equations based on the imposed temperature.
For the boundaries where the temperature is unknown (e.g. imposed heat flux or FNMB), the
convection (or conduction) and radiation must be accounted for simultaneously. In this case, the
radiative heat flux is computed by using the updated boundary temperature in each iteration.
8.3
POROUS MEDIA MODEL
The flow field in the porous media can be solved in FINE™/Open with OpenLabs™. It is done
by adding the additional source terms. Considering the general Navier-Stokes equations:
The source terms can be represented by:
Where
is the gradient of the pressure in the porous media,
is the thermal effects due
to the heat exchanges between the medium and the fluid.
Each porous media defines a separate block in FINE™/Open with OpenLabs™. Hence each
porous block is characterized by its set of parameters. Three models are currently implemented,
namely the Darcy law, the Ergun law and an Integral law.
8.3.1
The Darcy law
The gradient of the pressure in the porous media is given by the following relation:
where the coefficient K' can be defined as follows:
l User defined (homogeneous). The coefficient K' is defined as a constant.
l User defined (non-homogeneous). The coefficient K' is defined by its three components (K'ξ,
K'η , K'ζ) in a local coordinate system (ξ, η, ζ). Then, the flow solver will transform the
coefficient K'ξηζ into the cartesian coordinate system (x, y, z).
l Carman-Kozeny formula. The coefficient K' is defined as K' = μ/κ with μ the viscosity and κ
the intrinsic permeability.
The intrinsic permeability is given by the Carman-Kozeny relation:
where ε is the porosity defined as the volume fraction of the voids from the solid matrix, d is
the mean particle diameter given by the following formula:
where the specific surface area A is the surface area of pores per unit volume of the solid
matrix.
8.3.2
The Ergun law
The Darcy law is valid in the viscous regime, while the Ergun law can be seen as its extension in
the inertial (convective) regime by adding the second source term.
The gradient of the pressure in the porous medium in the Ergun law is given by the following
relation:
where the coefficients K' and K'' can be defined as follows:
l User defined (homogeneous). The coefficients K' and K'' are defined as constant.
l User defined (non-homogeneous). The coefficients K' and K'' are defined by specifying their
three components (K'ξ, K'η, K'ζ) and (K''ξ, K''η, K''ζ) in a local coordinate system (ξ, η, ζ).
Then, the flow solver will transform the coefficient K' ξηζ and K'' ξηζ into the cartesian
coordinate system (x,y,z).
l Carman-Kozeny formula.
The coefficient K' is defined as K' = μ/κ with μ the viscosity and κ the intrinsic permeability.
The intrinsic permeability is given by the Carman-Kozeny relation.
The coefficients K'' is defined as
. CE is the Ergun coefficient defined by:
The constant C proves the dependence of the inertial regime on the roughness of the pore's
surface and takes the following value:
C = 1.8 For smooth walls (Ergun law);
C = 4 For rough walls
8.3.3
The Integral Law
An alternative way often used in industry to define a porous media is to give the relation between
the pressure drop and the mass flow through the porous media of thickness L. Considering the
mass flow uniform over the entire porous media, the pressure drop in the porous medium can be
given by the following relation:
where:
l L [m] is the thickness of the porous media,
l CIL is the proportionality coefficient describing the pressure drop over the porous media,
l n is a user defined exponent (default 2.0).
l Apassage [m²] is defining the effective area through which the fluid flows,
l Atotal [m²] is defining the sum of the area offered to the flow and blocked by inclusions.
8.3.4
Thermal Heat Flux Model
The thermal effects due to the heat exchanges between the media and the fluid are represented by
the following relation:
where Kexch [Wm-2K-1] is the heat transfer coefficient; S'exch [m-1] is the specific surface of the
pores; T is the local temperature and Tskin is the skin temperature of the pores.
For defining completely the local heat source term the specific area of the pores should be given.
For tubular or cylindrical pores the specific surface area S'exch is expressed by:
where M is number f tubes with diameter D and length L that crosses the porous media with
volume Ωpm.
8.4
FLUID STRUCTURE INTERACTION
8.4.1 Modal Coupling
For the modal coupling approach in FINE™/Open with OpenLabs™, a structure file should be
inputted to provide the modal shapes and the eigen frequencies. With these information the flow
solver will compute the deformation of the structure by solving the modal equation , for the
number of modes specified by the user.
Solid mechanics is governed by the following equation:
Where:
l [M] is the mass matrix;
l [C] is the damping matrix;
l [K] is the stiffness matrix;
is the displacement of the structure;
is the external load.
For FSI computation, the external load is applied by the flow. The fluid flow is also influenced by
the deformation of the structure. The FSI resolution needs to solve both the fluid flow and
structure deformation by taking into account their interaction.
Considering the undamped structure without load, we can write:
This equation has not trivial solution only if:
This is an eigen value problem. Its resolution gives the eigen values λk. The eigen values lead to
natural frequencies ωk of the structure and natural mode shapes
:
Mode shapes constitute a basis of deformation modes. The global deformation of the structure can
be written as a composition of these modes:
where qk is the generalized displacement.
Using the global deformation of the structure in the modal equation , assuming a Rayleigh
damping, a stiffness frequency-independent and choosing a proper scale factor for the mode
shape, we can get a set of independent equation for each mode k:
where
is the damping coefficient for each mode shape.
For the coupled simulation, this set of independant equation is solved by the fluid solver at each
physical time step. After reconstruction with the global deformation of the structure, it gives the
new shape of the structure around which the flow is computed.
8.4.2 Mesh deformation
Mesh deformation plays a crucial role in the analysis of physical problems that involve moving
bodies and domain with dynamic boundaries. For example, in Fluid-Structure Interaction (FSI),
the fluid mesh has to be deformed at each time step according to the displacements computed by
the structural solver at the interface of the fluid domain and solid domain.
In FINE™/Open with OpenLabs™, the mesh deformation procedure is a module dedicated to
FSI applications. Two kinds of mesh deformation methodologies are available.
l Mesh deformation with quaternions.
l Mesh deformation with Radial Basis Function (RBF) interpolation.
A. Mesh Deformation with Quaternions
In this method, the mesh deformation is based on the use of quaternions. The methodology works
well when displacements of the boundaries are small but in case of large displacements, the
methodology fails, especially when considering meshes with high aspect ratio and viscous layers.
The approach to mesh deformation includes the following several stages:
First, the initial deformation specified at every point of the boundaries is converted and divided
into two components: translation and rotation. Translation is represented in terms of Cartesian
displacement vectors, while rotation is described in terms of quaternions.
Once the initial deformation is converted into translations and rotations of the boundary faces, an
interpolation procedure is used to propagate the deformation into the volume mesh. The
interpolation procedure is based on weighted Laplacian smoothing approach.
Finally, the interpolated data is converted back into the respective set of Cartesian displacement
vectors, which are used for final relocation of the mesh points.
For more details, please refer to Kovalev K. (2005).
B. Mesh Deformation with RBF
The interpolation function d describing the displacement in the whole domain is approximated by
a sum of basis function:
where
are the coordinates of the boundary nodes for which the value of the displacement is
known, p is a polynomial, Nb is the number of boundary nodes and ϕ is a given basis function
. In the current implementation, a linear polynomial is
with respect to the Euclidian distance
used:
The coefficient
and
are determined by the interpolation conditions:
with
the known values of the displacement at the boundary. To close the system, the
following requirement is added:
for each polynom q of degree less or equal to the degree of p.
The values for the coefficients
and the coefficients
are thus obtained by solving the
following linear system:
where α contains the coefficients
, β contains the coefficients
,
is a
matrix
containing the evaluation of the basis function:
and
is a
matrix with row j given by:
In FINE™/Open with OpenLabs™, the following Radial basis functions are considered:
l Function with compact support d called Wendland function:
l Function with global support called thin plate spline
8.5
FLUID-PARTICLE INTERACTION
The Lagrangian approach is used to simulate the fluid-particle interaction. In the Lagrangian
approach the particle cloud is modeled by a finite number of computational parcels, representing a
group of real physical particles with similar properties. The particles are tracked separately, each
as a single probe particle, through the flow field.
8.5.1
Particle tracking
A. Particle tracking procedure
The particles tracked by the Lagrangian method in FINE™/Open with OpenLabs™ are
computational particles or 'parcels'. This means that each of these parcels represents a given
number of real particles (it has a weight), as a deterministic tracking of a typical application is
prohibitively expensive.
In FINE™/Open with OpenLabs™, a fixed number of particle in the domain are tracked and it is
defined by the number of particles per cell. Since the number of particle are predefined, it is
necessary to use high number of particle in the domain to get good particle statistics. This
algorithm for particle tracking is much more user friendly, since it will stop automatically when all
particles are tracked through the domain.
B. Trajectories Calculation - Integration Method
The calculation of the trajectories is based on the Newton law:
where
is the acceleration vector of the particle of velocity
and
is the sum of the forces
acting on the particles:
where
is the pressure force,
is the drag force,
is the force due to gravity,
is the
buoyancy force,
is the virtual mass force.
Pressure force
The pressure force is a force on the particle that results from a pressure gradient in the fluid
around the particle. The pressure force can be expressed as:
where Ωp is the volume of the particle, ρf is the density of the fluid,
is the Lagrangian time
derivative following the fluid element.
Drag force
is the drag force between the flow and the particles, calculated by:
where mp is the mass of the particles, τp is the Stokes particle response time, Fcorr is a correction
factor, which is chosen in function of the particle Reynolds number, if the user selects Schiller-
Naumann correction as drag law.
The Stokes particle response time writes as:
where dp is the diameter of the particles.
The correction factor Fcorr following the corrections of Schiller-Naumann writes as:
where Rep is the particle Reynolds number defined as:
Force due to gravity
The force acting on the particle due to gravity writes as:
Buoyancy force
The force acting on the particle writes as:
Virtual mass force
The virtual mass force is due to an acceleration of the surrounding fluid by the particle. This force
can be written as:
C. Turbulent Dispersion
In the equation of motion of the particle, the instantaneous fluid velocity at the location of the
in case of large eddy
particle is unknown. Only the mean fluid velocity is available or,
simulations, the filtered fluid velocity. A model for the instantaneous fluid velocity needs to be
constructed that takes into account for the influence of turbulence on the particles. The most
common approach is constructing a Langevin equation for the instantaneous velocity of the fluid
seen by the particle. The Langevin model of Minier and Peirano (2001) is used here.
D. Momentum Two-way Coupling
The presence of a dispersed phase may alter the dynamics of the fluid flow. If particles are
accelerated by the fluid flow, they are slowing down the fluid flow in revenge and vice versa.
This effect
is accounted for in FINE™/Open with OpenLabs™ by a two- way coupling
procedure. During a Lagrangian cycle source terms for the fluid momentum equations are
sampled, which are then introduced in a second simulation of the fluid phase. The volumetric
source term is computed only using the drag force on the particles in the volume
:
The general procedure is the following. First, the Eulerian field is solved (continuous phase), then
based on this simulation the Lagrangian particles are tracked through the flow field and source
terms are sampled. Next, the Eulerian field is recalculated, accounting for these sampled source
terms. This will lead to a change of the continuous velocity fields and this modification will
induce a change in the particle-fluid drift velocities, altering the Lagrangian statistics. In a new
Lagrangian cycle, new source terms are sampled accounting for these modifications and another
Eulerian computation is performed. This has to be repeated until convergence. Unfortunately, nor
clear convergence criterion exists for dispersed two-phase flows, as it does for the continuous
phase. The non-alternation of the particle velocity at a given control point could be used as
convergence criterion.
E. Time Step Calculation
The polydispersion in size or mass of the particles can be taken into account by means of different
then their
size classes. If these size classes represent particles with very different
characteristic times (time to adapt to turbulence) and their velocities might be very different. A
separate time step is used for each of these size classes in order to accelerate the convergence rate.
The statistics taken for the particles account for these different time steps.
inertia,
The local time step is calculated as:
where
and
are the upper and lower bound of the local time step defined by the
expert parameter Lag_MaxLocalTimeStep_ and Lag_MinLocalTimeStep_, respectively.
8.5.2 Heat and mass exchange
A. Heating/Cooling
The droplet heating process is purely a convective heating part and the radiative heating part is not
considered. The droplet heating model is used, where the droplet temperature is uniform, but time
dependent. In this model, all the heat that is supplied from the fluid will be spent in increasing the
droplet temperature. In case of a gas temperature inferior than the droplet temperature, this will
lead to a cooling of the droplet, but the fluid temperature field will not change unless two-way
coupling computation is performed.
where
is the convective heat flux to the particle, the second term
represents heat flux by
radiation. Radiation is not taken into account in this model. The convective heat transfer equation
without considering evaporation (and thus not considering mass transfer from the dispersed phase
to the fluid) is:
Integration of the droplet heating model considering this convective heat transfer equation gives :
the gas temperature infinitely far from the droplet
Where T p is the droplet temperature,
surface, Nu the Nusselt number, λ g the thermal conductivity, t the time, C pL the specific heat
capacity of the liquid phase and the dp droplet diameter.
Considering moving droplets, the heat transfer is of convective nature and the Nusselt number
needs to be corrected. As Sazhin (2006) cites, the correction of the Nusselt number shows to be
(Fuchs 1959). The general formula for the Nusselt number takes thus
proportional to
the following form:
where
is chosen to be 0.552. This is the Ranz-Marshall correlation for the Nusselt number.
Note, if the Reynolds-number is zero, a stagnant droplet is regarded and as a consequence the
Nusselt number equals 2. The Nusselt numbers for moving non-evaporating droplets will be
referred to as Nu0 and is equal to Nusselt Nu in absence of evaporation.
B. Droplet Evaporation
With the droplet evaporation model enabled, the heat balance equation is given by:
is evaporation rate and
the second term expresses the heat flux related to a mass transfer, where
Lv is latent heat of evaporation. The mass transfer equals zero in absence of evaporation and the
second term on the RHS of the heat balance equation is zero and heating/cooling is recovered.
Three evaporation models are implemented, the 'rapid mixing model' and a correction to this rapid
mixing model by Abramzon & Sirignano (1989), in order to account for the blowing effect
(Stefan flow). The third model
is a non- equilibrium Langmuir- Knudsen model, which
incorporates droplet temperature non-uniformity.
Rapid mixing Model
The instantaneous evaporation rate
is given by mass transfer relation:
and droplet temperature Tp is calculated from the heat transfer relation given by:
using the Nusselt and Sherwood number for an evaporating droplets relation:
where BT is the Spalding heat transfer number at equilibrium defined as:
The Spalding mass transfer number at equilibrium B M is calculated based on the fuel mass
fractions on the surface YFP and away from the droplet
as:
Abramzon and Sirignano model
Abramzon and Sirignano (1989) introduced correction factors, which represent the relative
change of the film thickness due to Stefan flow effects.
In the case of an isothermal surface and constant physical properties of the fluid, the correction
factors do not depend on the local Reynolds number and it is found that they are practically
insensible to Schmidt and Prandtl numbers. They can thus be approximated as a function of the
Spalding transfer numbers only:
where F(B) can in either case be written as:
The corrected non-dimensional parameters are then written as:
Those two equations may be termed 'modified' Nusselt and Sherwood numbers respectively and
should not be confused with the actual Nusselt and Sherwood numbers. The actual Nusselt and
Sherwood number is given by:
This model
solves B T iteratively, which adds additional cost. B T is
iterated until
. Therefore, the correction factors F and consequently and are recalculated,
which are then used to determine:
and
Non-equilibrium Lanqmuir-Knudsen Model
Bellan and Harstad (1987) introduced a droplet evaporation model based on the Langmuir-
Knudsen law, which also incorporates droplet temperature non- uniformity. This model is a
modification of infinite thermal conductivity model, thus the droplet temperature is uniform as it is
the case in the above mentioned laws and fits into the frame of the Lagrangian module. The non-
equilibrium Langmuir-Knudsen law is incorporated through the definition of the vapour mole
fraction at the droplet surface, which is obtained from the combination of the vapour mole fraction
at the equilibrium state and a correction term (second term on the RHS of below equation). The
non-equilibrium vapour mole fraction
writes at the droplet surface as:
The Knudsen layer thickness is written as
where
dimensional evaporation parameter is defined as:
is the molecular accommodation coefficient and is assumed equal to unity. The non-
The definition in this equation is implicit for Miller et al. (1998) state that it is not necessary to
calculate β iteratively although the implicit definition, but that it is sufficient to use the previous
time step value, because of the logarithmic form used. The reason is that β varies relatively slowly
even for small droplets when the non-equilibrium contribution is important and is constant for
droplets following the classical d²-law, as β can be written proportional to the time derivative of
D2, which is constant once a constant droplet temperature is reached.
The mass fraction in the non-equilibrium state calculates then as:
The Spalding mass transfer number for the non-equilibrium case writes eventually:
The equation used for the third evaporation model the non-equilibrium Langmuir-Knudsen model
are thus:
C. Determination of droplet diameter
Droplet diameter is given by:
where K is given by:
D. Liquid properties
The liquid phase properties are taken constant over all the heating/cooling and evaporation
process, although the liquid phase temperature (droplet temperature) varies. The liquid properties
should be chosen at some reference temperature between the initial state and the boiling
temperature, such as:
The needed values must be known and are in general easily accessible for a wide range of liquids
or fuels. T0 is the initial temperature at injection and Tboil is the boiling temperature.
E. Vapour and gas phase properties
The vapour and gas phase properties are evaluated as mentioned above in two different ways.
First, using the 1/3-rule and second evaluating the properties at the wet-bulb temperature and
additionally using the 1/3-rule for the mass fractions, in the case of the first two models. The
mixing rules are then applied, except for the Langmuir-Knudsen model for which the model is
based on gas phase properties only.
First, the way to obtain the reference state is explained and then the mixing rules are given with
the corresponding properties that are evaluated at these properties.
Reference state by '1/3-rule'
The 1/3-rule is widely applied to calculate reference values for the temperature T ref and the
vapour mass fraction Yref, which are used to evaluate both the gas phase and vapour properties.
The general rules are:
where A is a chosen equal to 1/3. The coefficient A could taken any value in the range
, but 1/3 has gained the most acceptance.
In the user defined A-rule, the factor A is replaced by any other value given by user in the range
of
.
Reference state by wet-bulb temperature
Miller et al. (1998) propose an alternative approach, which assumes for the purpose of property
evaluations that the droplet surface temperature quickly rises from the initial conditions to the wet-
bulb temperature and that the wet-bulb temperature is the appropriate condition for evaluating
properties of both the gas and vapour phase. They show that this method works quite well in the
cases they investigated. However, if the gas temperature varies strongly over the computation
domain this approach might not be that accurate. If the wet-bulb temperature for a given gas
temperature is not know, Miller et al. (1998) propose an empirical correlation to experimental
results, which is valid for a variety of fuels tested, in function of the boiling temperature Tboil and
the free stream gas temperature
. The correlation is given by the relation:
This correlation is valid for a wide range of fuels, but caution should be taken if applied to
untested fuels.
Mixing Rules
Wilke Rule
The Wilke rule (Poling et al. (2004)) for a quantity ψ = μ, λ, neglecting second effects writes as:
where:
and:
Where the molecular weight is denoted Mi.
Liner mass averaging
The linear mass averaging for the heat capacities given in the form of:
The mean value of the specific gas constant calculates.
F. Evaporation with 2-Way Coupling
Mixture fraction equation quantifies the fuel fraction evaporated from liquid single component
fuel droplets. In 2-way-coupling mode, the Lagrangian evaporation routines will be coupled with
this mixture fraction fields and this allows a more realistic evaporation behavior. Without the
mixture fraction field,
the droplets are always evaporating into a completely unsaturated
environment, which is not a realistic assumption in the core zone of an evaporating liquid spray.
The presence of vapour of the droplets, liquid phase in the gaseous phase will reduce the
evaporation rate in the respective regions. This is physically understandable as a liquid cannot
evaporate into an environment saturated by its vapour. As the only source of vapour is the droplet,
the evaporation rate of the droplets defines the mixture fraction fields.
Mixture fraction equation
The mixture fraction equation is defined as:
The
is mixture fraction source terms which comes from droplet mass evaporation.
8.5.3
Primary atomization and secondary breakup
A. Primary Atomization
The primary atomization (initial breakup) models are employed to determine the conditions of
droplets injected from the nozzle: particle's velocity components and diameters. They compute
necessary properties of droplets for initialization using correlations with flow properties.
Blob model
Blob model, developed by Reitz (1987), is one of the most popular breakup models for high
speed pressure atomizers.
FIGURE 8.2
Schematic of Blob method (Reitz, 1987)
"Blob" denotes the initial monodisperse droplet injected into the domain. This model is quite
simple since the droplet remains spherical with a diameter initially equal to the nozzle diameter.
By mass conservation, the injection speed of the blob is governed by
: where
stands for the mass flow rate and S represents the exit area of nozzle.
LISA model
The Linearized Instability Sheet Atomization (LISA) model has been developed by Schmidt in
order to simulate the effect of primary break-up in pressure-swirl atomizers.
A thin conic liquid sheet is formed as a result of rotational motion. By conservation of the mass
through the inlet, the film thickness is given by:
(0-1)
In addition,
and
where
is the film thickness and
is the diameter of the injector's exit. U is the absolute speed
and u its axial component :
.
The model assumes a two-dimensional, viscous, incompressible liquid sheet with thickness of 2h
and velocity U, moving through a quiescent, inviscous, incompressible gas medium. The sheet
interacts with wave disturbance, with a growth rate approximated by:
where Q is the gas-liquid density ratio and k the wave number.
The surface wave amplitudes are described by:
where
is the initial wave
amplitude and
the complex growth rate.
This
expression is numerically maximized to calculate
the maximum growth rate
considered to be responsible of atomization and used for the evaluation of
breakup characteristic time and length:
where
the amplitude when break-up occurs and
is a constant set to 12.0 by default
according to the work of Dombroski and Hooper 1962 and its value can be changed by means of
the expert parameter Lagr_LISALogAmplitudeRatio.
For long wavelengths (
), the diameter of ligament is given by :
by default,
is the wave number corresponding to the maximum growth rate.
Otherwise, this diameter is
by default and in that case
.
The most probable droplet diameter is determined from :
where
is the usual Ohnesorge number for a droplet. A Rosin-Rammler distribution
is then used to initialize the particles.
In the case of long waves, the atomization distance is computed with :
with in that case
.
B. Secondary break-up
Liquid spray detached from the jet liquid core, continuing their motion through the gaseous
medium, may be disintegrated into smaller droplets. This phenomenon is known as secondary
breakup.
Several break- up regimes are distinguished. Indeed, droplets do not experience the same
phenomenon for two different Weber numbers, but break up in different regimes. Dimensionless
numbers are used to classify the different regimes, mainly the Weber number and Ohnesorge
number :
Weber Number Range
The most commonly distinguished regimes are :
Regime
Vibrational break-up
Bag break-up
Bag-and-stamen break-up
Sheet stripping
Catastrophic break-up
Nevertheless, these criteria are not followed by all models. Some models focus upon specific
Weber number ranges and are inaccurate otherwise. Regimes correspond to the different manners
the droplets break up.
Reitz and Diwakar break-up model
This is a two-regime break-up model based on the work of Reitz and Diwakar. It distinguishes
between bag breakup and stripping breakup. Break-up occurs when critical value of particle
Weber number has been exceeded following the relation :
where
represents droplet radius prior to breakup,
refers to the stable diameter and
is
the characteristic break-up time.
For bag break-up (
) the constants are :
and
For stripping break-up (
) the constants are :
and
The spray angle is computed from :
.
Constants are actually calibrated to match experimental results. Default values are suggested in the
vary strongly from one
following table but the user must retain that the parameter
and
author to another.
Time factor for bag break-up
around
Time factor for stripping
0.5 to 120 ( 1 to 10 in most
cases)
Critical Weber number for Bag break-up
7 to 18
Weber number factor for stripping break-up
around 1.0
Coefficient for angle depending on the geometry and
fluid properties
experimental
Pilch and Erdman model
This model takes viscosity into account. Break-up is based upon empirical correlations developed
by Pilch and Erdman. Break-up occurs if
with :
Five break-up regimes are distinguished each with their dimensionless total break-up times T:
Vibrational break-up
Bag break-up
Bag-and-stamen break-up
Sheet stripping
Wave crest stripping
And the total break-up time and stable droplet diameter are then :
and
with
and the droplet diameter changes as :
Constant calibration :
0.375
0.2274
Hsiang and Faeth model
Hsiang and Faeth developed a model to describe break- up of droplets which undergo a
deformation.
This model is used when We < 1000 and adequate for Diesel engine spray applications. Its
characteristic break-up time is :
The stable diameter is :
Break-up occurs if
and the rate equation for droplet diameter change is :
.
Schmehl break-up model
This model is a combination of Hsiang & Faeth and Pilch & Erdman models.
In
the
Schmehl model,
the
break- up
is exceeded.
happens
if
critical Weber
number
Depending on the Weber number regime at the beginning of the break-up process, different
scenarios are possible :
1. Bag break-up regime :
A random break-up time is computed. Child droplet sizes and normal velocity of children
droplet after break-up are computed. If the particle lifetime is longer than the break-up time
then break-up occurs in the second half of the tl to tbr time frame.
Droplet size after break-up for the bag break-up and multimode regimes is computed from the
following relation :
with
.
The velocity component is given by
and then determined from
where
at
and
is the droplet diameter before break-up.
2. Multimode regime is defined by :
and
computations are the same than previously.
3. Shear break-up regime occurs when
.
Computations are the same except that the breakup can occur at any time of the same time
frame described in bag break-up regime. Children droplet sizes are calculated with :
with
.
Then a root normal distribution is used to distribute diameters with
according to
Simmon's results (1977):
dimension.
are values of mathematical meaning without any physical
Taylor Analogy Break-up model (TAB)
The droplet distorsion was described by Taylor in 1963 as a spring-mass system with a one-
dimensional, forced, damped, harmonic oscillation. The following model based upon that
description is described by O'Rourke and Amsden. It continuously connects the breakup times
found experimentally for bag and stripping breakup regimes.
Deformation motion equation is :
with:
Usually :
so that the droplet have no initial oscillating motion. If
, then the
initial conditions are also set to zero.
Break-up can occur if the particle distortion can exceeds unity. When this happens, oscillation is
. New Sauter mean diameter is calculated from :
set to 1 and :
which derivatives from the fact that parent particles and child particles possess the same energy.
Then, the child diameter is computed from a Rosin-Rammler distribution with a spread of 3.5.
- distribution but Rosin- Rammler (also known as Weibull
The original model uses a
distribution in mathematics) is found to have better accuracy with a probability density function of
:
Break-up can occur if
with
Break-up time is computed from
with
Break-up happens at a specific time, in a following iteration if necessary. Important coefficient are
described in the following table as well as their meaning and calibration method
0.5 Critical amplitude coefficient, breakup occurs if and only if the amplitude of oscillation of the
north and south poles equals the drop radius :
10.0 Damping coefficient for oscillations in the fundamental modes (10 instead of 5 because of
Lamb further development)
1/3
External force coefficient is obtained knowing that CkCbCF=Wecthe critical Weber number
of 12 by default.
8.0 Restoring force coefficient is obtained by matching to the fundamental oscillation frequency
(around 8 but should not be modified)
1.0 New droplet velocity factor, arbitrarily chosen to be of the right order of magnitude and
related to the equator motion of droplets (around 1)
K 10/3 Energy ratio factor (around 10/3)
This model can be enhanced by considering the child droplets rate of creation as a function of the
or
existing number of particles with :
where
if
if
with
the Weber number that separates the two regimes
(bag break-up and stripping break-up). New radius is computed from:
. Then
the velocity component of child droplets is normal and is determined by :
with
and
is the parent droplet drag coefficient at break-up. Break-up times
tend to be too short. In order to solve this problem, the rate
is set to a negative value to
delay the first break-up. This negative value is :
with
It is assigned to initial Lagrangian parcells but not to child particles.
Enhanced bag break-up factor (around 2/9 but should not be modified)
Stripping break-up factor (around 2/9 but should not be modified)
Critical Weber number for stripping break-up (to adjust experimentally)
The main limitation of the breakup model is that only one oscillation mode is kept track of when
many modes actually exist.
Cascade atomization and break-up model (ETAB enhancement)
As previously, the droplet radius is given by :
However,
changes :
where and
Also the expression of ω is modified from TAB and ETAB models with :
which then becomes
to compute break-up properties just as in ETAB.
Enhanced bag break-up factor (around 2/9 but should not be modified)
Stripping break-up factor (around 2/9 but should not be modified)
Critical Weber number for stripping break-up (to adjust experimentally)
Correction of drag force coefficient
Models which relies upon the Taylor analogy compute an oscillation state (noted as y). This state
can be used to take into account the distortion of particles when calculating the drag force. A new
correction model is implemented from Liu:
8.6
CAVITATION
Cavitation is a dynamic process of formation of bubbles inside the liquid, their growth and
subsequent collapse. It appears where the pressure of the liquid falls below its vapor pressure.
Such cavitation often occurs in pumps, propellers and impellers, etc.
The development of the cavitation phenomena is related to the cavitation number σ, defined as:
where Pt,inlet is the absolute total pressure at the inlet of the domain;
Pvap,s is the vapor pressure;
ρ is the density of the liquid phase;
Vref is the reference velocity .
Cavitation develops with decreasing cavitation number, which can be achieved by increasing the
vapor pressure or decreasing the absolute inlet total pressure from an arbitrary non-cavitating state
to the desired cavitating state (defined through σ).
To model the physics of cavitation, the approach used by FINE™/Open with OpenLabs™ makes
use of single fluid approach, characterized with the density ρ that is allowed to vary within the
computational domain.
8.6.1
The Cavitation Model with the Barotropic Law
When the cavitation model with the barotropic law is used, the evolution of density and static
pressure are linked through a barotropic law, enabling macro simulation of the cavitation
phenomena with minimum user inputs.
The barotropic law
is used to evaluate the local density as a function of local static
pressure ps in the cell. According to local value of density and corresponding vapor pressure, the
computational cell can be considered as filled fully with liquid (
), or a
mixture of both. In the latter case, an equivalent density is considered. The corresponding local
fluid velocity is unique, still based on the single fluid approach.
), vapor (
FIGURE 8.3
Sinusoidal barotropic state law
In the biphasic region, the density is written as:
where
is the vapor pressure,
is the minimum speed of sound and
is the local static
pressure.
The parameter AMIN, which represents the slope of the barotropic law, is defined as follows:
Then, the sinusoidal barotropic law is written as:
The dynamic viscosity of the mixture is computed as follows:
and
where
α is defined as:
are the dynamic viscosity of the vapor and liquid, respectively. The void ratio
8.6.2
The cavitation model with the transport equation
model
The Transport Equation Model (TEM) for cavitating flow modeling is based on an Eulerian
homogeneous flow model (phases are assumed to be in kinematic and thermodynamic
equilibrium). The continuity, momentum and energy equations are solved for the mixture (liquid
and vapor) and an additional transport equation is solved for the vapor volume (or mass) fraction.
Derived from the Rayleigh- Plesset equations of vapor bubbles growth, condensation and
evaporation source terms are included in this additional transport equation in order to describe the
phase change. FINE™/Open provides three formulations of the source terms: Singhal et al.
(2002), Zwart et al. (2004) and Tani et al. (2009).
A. Thermal and transport properties for the liquid-vapor
mixture
The relation between the vapor volume and the vapor mass fraction is written as follows:
where f is the vapor mass fraction, α is the vapor volume fraction, ρ is the mixture density and the
subscript V indicates the vapor phase. For the liquid phase the subscript L will be used.
The mixing rule for the mixture density in terms of the vapor volume fraction can be written as:
The mixture density in terms of the vapor mass fraction follows:
In the approach, the speed of sound for the mixture is also needed, for which a harmonic
averaging is applied:
The dynamic viscosity of the mixture is computed as follows:
B. Formulation of the Transport Equation Model (TEM)
The vapor fraction transport equation can be formulated as follows, in a non-conservative form
and in terms of the mass fraction:
where
is the velocity field of the mixture and
is the condensation/evaporation source term.
In the same way, the non-conservative form of the transport equation formulated in terms of the
vapor volume fraction is written as:
The source term
includes the liquid evaporation
and vapor condensation
rates.
FINE™/Open provides three formulations of the source terms:
Singhal et al. (2002)
In vapor mass fraction
if
if
, else 0
, else 0
In vapor volume fraction
if
if
, else 0
, else 0
where σ is the surface tension.
represents the characteristic velocity and it is clipped as max
(1.0,
).
The model constants are set as:
Zwart et al. (2004)
=0.05 ,
= 0.1
if
if
, else 0
, else 0
where
represents the nucleation site volume fraction
,
is interpreted as
the radius of a nucleation site
[m].
The model constants are set as:
=0.001 ,
= 5
Tani et al. (2009)
In vapor mass fraction
if
if
, else 0
, else 0
In vapor volume fraction
if
if
, else 0
, else 0
The model constants are set as:
=0.06 ,
= 0.12
C. The effect of turbulence
Several experimental investigations show a strong impact of turbulence on cavitating flows due to
pressure fluctuations (Singhal et al., 2002). A simplified method to take into account these effects
in the TEM modeling approach is to raise the phase-change threshold pressure as follows:
where
is the saturation pressure of the fluid at a given temperature (thermodynamic
value) and
is a modeling constant with the value 0.39.
The turbulence- cavitation interaction can be used only when the turbulence model is k- based (k-
epsilon, SST, ...).
D. The Transport Equation Model with Thermal Effects
In the transport equation model described above, the saturation pressure in the expressions for the
is defined as a constant. However, for cryogenic fluids such as liquid hydrogen
source term
or liquid nitrogen, the saturation pressure depends on the local temperature. The transport
equation model has been extended with the possibility to take into account the dependence of the
saturation pressure on the temperature. In FINE™/Open, there are two options of modeling the
dependence of the saturation pressure on the temperature.
Option 1: Correction of the saturation pressure based on ideal
temperature depression
The first option of modeling the thermal effect on the saturation pressure is based on the model
presented in Ruggeri and Moore (1969). In this model, the saturation pressure depression is
estimated by performing a heat balance between the heat required for vaporization and the heat
subtracted from the surrounding liquid. The ideal temperature depression due to vaporization is
given by:
is the latent heat of vaporization and
where
liquid. The real temperature drop can be estimated by introducing a non-dimensional factor
given by:
is the heat capacity at constant pressure of the
,
For small changes in temperature, the change in the saturation pressure can be expressed by:
By combining these results, the saturation pressure as a function of the temperature can be
determined as follows:
With this formulation, there is no need for the energy equation to be solved, because an algebraic
expression is used to compute the saturation pressure.
Option 2: Saturation pressure as a polynomial function of the
temperature
The second option of modeling the thermal effect on the saturation pressure is to define the
saturation pressure as a polynomial function of the temperature:
In FINE™/Open, a fourth order polynomial of the temperature is used, which allows a good
match with the saturation pressure curves of typical fluids.
Since the temperature is needed to solve for the saturation pressure, the energy equation needs to
be solved with this option. In addition, a model of the thermal fluid properties of the mixture is
required. The mixing rule for the specific heat capacity of the mixture is given by:
The mixing rule for the thermal conductivity is given by:
The user can define the thermal conductivity for the liquid and the vapor either by supplying the
values directly or by supplying the Prandtl numbers. For the latter option, the thermal conductivity
is computed with the following expression:
The temperature may vary rapidly during the first iterations of the solver. This can cause
difficulties with convergence, because the saturation pressure depends on the temperature. For this
reason, a temperature limiter is included, with which the user can define a temperature range
around the reference temperature between which the solution can evolve.
Because the cavitation source term is very stiff, it causes numerical difficulties. Therefore, sub-
iterations have been introduced in order to obtain a more precise calculation and avoid divergence
or oscillations around the saturation curves. A sub-iteration time step is defined by the user-
controlled parameter
as:
During the sub-iteration process, velocities are neglected and artificial pressure, temperature, and
and
void fraction are updated starting from the initial values
followed by:
The cavitation source term
is computed according to its regular definition depending on the
model selected by the user, but with the values of the artificial variables at each sub-iteration.
Furthermore,
is the cell volume and
is given by:
in which
is the preconditioning parameter.
The final cavitation source term at the next time step is the sum of all the sub-iterations:
8.6.3
The Cavitation Model with Thermodynamic Tables
When the cavitation model with thermodynamic tables is used, the density will depend on the
the
pressure and enthalpy, which is accounted for by thermodynamic tables. Among all
thermodynamic tables, the key table is the one that describes the relation between the density and
pressure. A second variable that will be especially important for thermo-sensitive fluids is the
temperature (or enthalpy). In the present approach, the density depends on both pressure and
enthalpy. This relation is accounted for in the RHP table.
All the thermodynamic tables are generated by using TabGen, which uses REFPROP (NIST) as
engine/database. The tables are generated assuming thermodynamic equilibrium.
The dependence of the saturation pressure on the temperature will give a very important
indication of the thermal sensitivity of the fluid. Actually, TabGen can provide the derivative of
. As an illustrative example, the value
the saturation pressure with respect to the temperature
of this derivative for water (very low thermal-sensitivity) at 300 K is 208 Pa/K. The same
derivative for a highly thermo-sensitive fluid such as N2 at 86 K is 23687 Pa/K. Some fluids are
sensitive to the temperature at which the derivative is evaluated. For example, the derivative for
LH2 at 23 K is 50506 Pa/K while it reduces to 22505 Pa/K at 19 K. One of the advantages of the
use of thermodynamic tables to model cavitating flows is that the thermo-sensitive effect is
included in the table and no other model is needed. Moreover, the thermodynamic tables can also
take into account the variation of the derivative with respect to the temperature at which is
evaluated.
References
Singhal A, Athavale M, Li H, Jiang Y, 2002, Mathematical basis and validation of the full
cavitation model, ASME (2002), Vol. 124 pp. 617 – 624.
Zwart P, Gerber A, Belamri T, 2004, A two- phase flow model for predicting cavitation
dynamics, ICMF (2004), Yokohama,Japan, Paper No. 152.
Tani N, Tsuda S, Yamanishi N, Yoshida Y, 2009, Development and validation of a new
cryogenic cavitation model for rocket turbopump inducer, 7th International Symposium on
Cavitation (2009), Paper No. 63.
Ruggeri R.S and Moore R.D, 1969, Method for prediction of pump cavitation performance for
various liquids, liquid temperatures, and rotative speeds, NASA technical note TN D-5292.
8.7 MULTI-SPECIES FRAMEWORK
8.7.1
Inert multi-species
With the Multi-species framework, mixing and transport of chemical species can be simulated by
solving conservation equations describing convection, diffusion and reaction source terms for
each component species. This framework is currently only available for inert flow (without source
terms).
Inert multi-species framework solves for convection and diffusion without any chemical reaction
source terms. Non- reacting species transport for multi- species framework can be used for
simulation such pollutant tracking and chemical mixing flows.
A. Governing Equations
Governing equation for the multi-species framework is given by:
is the flux of species j caused by mass diffusion. N is the number of species and E represents
the total sensible energy. The energy equation is formulated in dependence of the sensible total
energy to keep the energy in the same form for multi-species simulation as for single-species
computation. In the inert cases heat release due to destruction and creation of species due to
chemical reaction is not considered.
The sensible enthalpy h for ideal gas mixture is given as a mass-weighted sum of the enthalpies of
the all individual mixture:
The sensible energy of species j is defined as:
Thus, In the equation that has only one species is present, the equation are the same as that of
single specie framework.
is the mass fraction of species j. In the species equation, first N-1 species equation are solved
and the concentration of Nth species is determined via the condition, that the sum of all mass
fraction must be equal to 1. Normally the abundant species in mixture is considered as N th
species.
It is assumed that the gas behaves as an ideal mixture. Thus, the thermal equation of state is given
by:
B. Ensuring Mass Conservation
To ensure mass conservation (both for a mixture and real gases), the closure conditions:
has to be ensured. The above equation is enforced by setting the N-th species to:
This is done after each solution update and after each time the solution variable are prolongated in
the multigrid scheme. To see why the closure condition need to be respected to ensure mass
conservation, one may add up the partial densities to yield:
Alternatively, Since the density is determined as:
,
,
It is obvious that the closure condition needs to be respected in order to avoid spurious generation
or destruction of mass.
It should further be noted, that the use Fick's law for determining the diffusive fluxes
according to:
does not guarantee the conservation of the species. To avoid a spurious generation of the species a
correction velocity has to be introduced. This correction velocity reads as:
which leads to the following flux:
By summing over all fluxes, the mass conservativity of the approach can be demonstrated:
as long as the closure condition is simultaneously enforced.
C. Species Diffusion
Species Diffusion is given by Fick's law:
Where
represents the effective diffusion coefficient given by:
where,
represents the laminar diffusion coefficient and
the turbulent one. Diffusion of
species due to the presence of a pressure gradient (pressure diffusion) or temperature gradient
(Soret effect) are not considered. In FINE™/Open with OpenLabs™ the user can either specify a
constant laminar diffusion coefficient for each species or specify that the diffusion coefficient of
each species be calculated from the laminar kinematic viscosity
assuming a constant laminar
Schmidt number
for each individual species, which is a user input:
The turbulent diffusivity is determined assuming Schmidt similarity:
where
denotes the turbulent dynamic viscosity of the mixture.
D. Transport Properties
Determination of the dynamics laminar viscosity of the individual
species
In FINE™/Open with OpenLabs™ the user can either specify a constant viscosity:
for each species or specify that the dynamic laminar viscosity of each species be calculated using
sutherland's Law.
Determination of the dynamic laminar viscosity of the mixture
The viscosity of the mixture is calculated from the viscosities of the individual species either by
taking the mass average:
or applying the simplified form of Wilke's law:
The mole fraction
are calculated from the mass fraction
as follows:
,
Determination of the turbulent dynamic viscosity of the mixture
The turbulence model determines the turbulent dynamic viscosity of the mixture. The presence of
individual species does influence the modeling of the turbulence.
Determination of laminar conductivity of the individual species
In FINE™/Open with OpenLabs™ the user can either specify a constant laminar conductivity:
for each species or specify that the dynamic laminar viscosity of each species be calculated from
the laminar viscosity assuming a constant laminar Prandtl number Pr (Pr is same for all species):
This corresponds to the law used in the single-species framework. Even though the framework
principally allows the use of different state laws for the various species, the framework currently
requires the user to use one single law for all species. Thus, the user needs either to specify a
thermal conductivity for each species or use the Prandtl number to determine
constant
conductivity of each species.
Determination of laminar conductivity of the mixture
The conductivity of the mixture is calculated from viscosity of individual species either by taking
the mass average:
or applying the simplified form of Wilke's law:
Determination of turbulent conductivity
The turbulent conductivity
is determined assuming Prandtl similarity (as for the single species
framework, this is the only option):
where
denotes the turbulent dynamic viscosity (of the mixture),
denotes the turbulent
Prandtl number and
denotes the heat capacity of the mixture.
CHAPTER 9.
ROTATING MACHINE
This chapter describes the theory dedicated to turbomachinery applications.
In this section
9.1 Rotor/Stator Interaction
9.2 Unsteady Turbomachinery Calculations
9.3 Harmonic Method
207
216
219
9.1
ROTOR/STATOR INTERACTION
9.1.1
Introduction
The relative motion between successive blade rows together with boundary layers, wakes, shocks
and tip leakage jets are the major sources of unsteadiness that may affect a turbomachinery flow
locally or as it travels through the next rows. All these interactions are strongly coupled,
increasing in magnitude as the gap between successive blade rows is decreased, and affecting
consequently the performance of the machine.
Solving for such flows requires an unsteady and viscous flow solver with the capability to
manage enormous data storage. One way to optimize the computer memory requirement is to
resolve the steady flowfield on a truncated computational domain. This requires a pitchwise
averaging process to be performed at the so-called rotor/stator interfaces. This particular boundary
condition is available under the FINE™/Open with OpenLabs™ environment as the mixing
plane approach. The rotor-stator interaction is done by exchanging circumferentially averaged
flow quantities. Physically, this means that the blade wake or separation occurring in the blade
passage are mixed circumferentially before entering the downstream component. As a result, the
velocity components and pressure is uniform in the circumferential direction at the rotor/stator
interface. This physical approximation tends to become more acceptable as rotational speed is
increased. This mixing plane technique is by far the most used rotor/stator modeling in industry
approach. See Full Non- matching Mixing Planes and Non Reflecting Boundary Conditions
sections for more details on the mixing plane approach.
The Frozen Rotor approach is another steady method considering the rotor/stator interface. This
method is a simplified full non-matching domain scaling approach. The basic idea at the origin of
the Frozen Rotor technique consists of neglecting the rotor movement
in the connecting
algorithm. The governing equations are solved for the rotor in a rotating frame of reference,
including Coriolis and centrifugal forces; whereas, the equations for the stator are solved in a
absolute reference frame. The two components are literally connected, and hence a rotor-stator
approximation is not required, rather the continuity of velocity components and pressure is
imposed. As a result, the final steady solution will be depending on the relative position of the
rotor and the stator. See Frozen Rotor section for more detail on the Full Non Matching Frozen
Rotor approach.
The second step allowing for a higher level of accuracy consists of considering an unsteady
rotor/stator interaction. Various techniques allowing to treat configurations with an arbitrary
number of blades in the rotor and the stator have been proposed by many authors (Giles, 1990,
Lemeur, 1992, Erdos et al., 1977, He, 1997), each of them having their own advantages and
disadvantages, each of them affecting differently the memory requirement, solution time and the
most important parameter, the accuracy of the computed flow solution. But none of these
techniques allows to resolve on a truncated computational domain all time frequencies present in
the turbomachinery configuration, except if the pitch distance is the same in the successive rotors
and stators. In fact, each of them are affecting the computed time frequencies and Fourier modes
that are propagating the flow information inside the gap region.
The Domain Scaling Method is a kind of unsteady rotor/stator interface treatment (Rai, 1989), that
has been selected and implemented in the FINE™/Open solver. This technique is based on the
constraint that the pitch distance must be identical on both sides of the interface. If the numbers of
blades in the rotor and the stator are different, this implies either to increase the number of
passages modeled or to scale the geometry. The Domain Scaling Method presents the advantage
that it allows to resolve all time frequencies with an error that is proportional to the scaling
coefficient. The accuracy of the computed unsteady flow solution may then be improved at the
expense of more data storage and larger solution time if more blade passages are considered. See
Domain Scaling Method section for more detail on the domain scaling method.
9.1.2
Full Non-matching Mixing Planes
A. Full Non-matching Technique
This technique is based on the concept of image mesh. The purpose of the image mesh is to
eliminate any constraint on the rotor/stator patches configuration. The only remaining geometrical
constraints are the follows:
l the hub and the shroud lines are assumed to be located on a circular arc, and each extremity of
the hub and shroud lines should coincide with one corner of one of the patches.
l all patches constituting a rotor/stator interface should form a filled closed surface with no gap
l the rotor/stator patches should be fully included in the rotor/stator interface: contrary to the full
non matching algorithm, which includes an automatic detection of the connection zone, and in
which the patches can then be partially connected, the rotor/stator module assumes that the
patches are fully connected.
The image mesh is constructed on both sides of the interface, on basis of the real mesh rotor/stator
patches, and respects the following constraints:
l The image is a "concatenation" of all patches constituting the left or right side of the interface.
l The spanwise distributions of the nodes in the left and right image meshes are coincident.
l The pitchwise lines of the image meshes lie on circular arcs.
l The mesh density of the image mesh is similar to the one of the basic mesh.
The creation of the image mesh is illustrated by FIGURE 9.1.
FIGURE 9.1
Creation of the image mesh
B.
Implementation of Mixing Plane Approach with Full Non
Matching Technique
The communication algorithm between rotors and stators is organized in several steps:
1. Extrapolation of the flow solution from the inner cells to the boundary: the cylindrical velocity
components are extrapolated.
2. Sending of the flow solution from the initial mesh to the image (on both sides): an interpolation
tree is built between the image and the initial mesh, by applying the full non matching
connecting algorithm.
3. Application of the mixing plane algorithm between the left and right images, with construction
of flux variables to be imposed on the left and right side.
4. Sending of the fluxes from the image to the initial meshes: this is again performed with the aid
of the full non matching algorithm, which allows for an exactly conservative distribution of the
calculated fluxes throughout the cells. The transformation of the flux variables to the primitive
ones is not required, as the fluxes are directly added to the residuals of the finite volume
scheme, without the use of the dummy cells.
A flux-based mixing plane algorithm is used, mainly because strict conservation of mass flow,
momentum and energy is guaranteed. The algorithm is organized under the following steps:
1. Calculation of the flux variables on both sides
2. For all spanwise positions perform a pitchwise averaging of the flux and of the primitive
variables.
3. For all spanwise positions determine the upstream and downstream side according to the flow
direction, and build the mixing plane fluxes.
The local fluxes on the upstream side are taken from the upstream, with a contribution of the
averaged downstream static pressure.:
On the downstream side the local fluxes are taken as the averaged fluxes on the upstream side
with a contribution of the local static pressure:
9.1.3
Non Reflecting Boundary Conditions
A. Concept
the strong interaction between neighboring rows,
Because of
the flow in multistage
turbomachinery is rather complex. This complexity is increased by the difficulty that CFD codes
have to handle rotor-stator interfaces located close to blade rows. In such configurations, spurious,
non-physical reflections of steady waves - such as shock waves -can occur at boundaries.
A common way to cope with this problem is to use a steady-state non reflecting boundary
condition based upon a characteristic analysis of the linearized Euler equations [Giles, 1988]. The
characteristic variables are imposed on each side of the rotor-stator interface. On a downstream
patch the entropy wave, two vorticity waves and the downstream running pressure wave are
imposed, whereas the upstream running pressure wave is imposed on the upstream patch.
Though the methodology is based on the linearized Euler equations, it could be applied to viscous
flows. Nonetheless, such an approach should be restricted to cases where the pitchwise variations
are much smaller than the pitch average quantities.
It should be noted that this method uses the Full Non- Matching technique. The procedure
described bellow is performed on the image meshes. The turbulent quantities is treated by the full
non-matching mixing plane approach.
B. Characteristic Variables
The characteristic variables (ci) are determined in terms of perturbations to the average flow field:
where ρ is the density, u is the velocity normal to the boundary considered, v and w are the
tangential velocities, and p the pressure. The upper bar designs the averaging procedure. c is the
speed of sound. The characteristic variables are:
l c1: the linearized perturbation in entropy.
l c2 and c3: the tangential velocity.
l c4: the downstream running pressure wave.
l c5: the upstream running pressure wave.
C. Non Reflecting 1D
For the Non Reflecting 1D rotor/stator interface, at an inflow (downstream of the rotor/stator
interface) the first four incoming characteristics are specified, whereas the fifth characteristic is
specified at an outflow (upstream of the rotor/stator interface). For instance if a stator is located
upstream of a rotor, at the stator outflow the imposed characteristic is
and at the rotor inflow the imposed characteristics are
The other characteristics are computed is inverted in order to recompute the new primitive
variables on the boundary.
D. Non Reflecting 2D
For the Non Reflecting 2D rotor/stator interface, the way that the boundary condition is treated
depends on the local Mach number M.
For subsonic inflow, the outgoing fifth characteristic variable is evaluated at each point along
pitchwise direction and its discrete Fourier transform is calculated.
where k can vary in the range [–N/2+1;N/2-1]. Based on the experience already obtained with the
harmonic method, it has been decided to set the range of variation of k as an input parameter,
which is controlled by the expert parameter RS_NbH2DNR_ (default value [-3;3]).
According to the steady-state non-reflecting theory, the correct steady state amplitude of the
Fourier transform of the second characteristic is
where
Transforming back into the physical domain gives
For supersonic inlet, since β is real and defined as
. The
relationship between c5 and c2 is more direct and does not require any Fourier transform
The steady state correction to the local second characteristic variable is the difference between the
one obtained from c2js and c2j and the current value:
Therefore the characteristics for downstream patches are:
For subsonic outflow, the outgoing second and fourth characteristic variables are evaluated at
each point along pitchwise direction and there discrete Fourier transform is calculated.
According to the steady-state non-reflecting theory, the correct steady state amplitude of the
Fourier transform of the fifth characteristic is
Transforming back into the physical domain gives
For supersonic outlet, the relationship between c5 and c2 is more direct and does not require any
Fourier transform
The steady state correction to the local fifth characteristic variable is the difference between the
one obtained from c5js and c5j and the current value:
Therefore the characteristics for downstream patches are:
E. Correction for Enthalpy
As for the time-marching method, the treatment described above leads to a global correction of the
flow variables at the rotor/stator. Due to second order effects, at downstream patches, the local
values of enthalpy could be much different from its average value. It is therefore required to
impose an additional correction in order to eliminate local deviations. This is obtained by driving
the two following residuals to zero:
Where j stands for the grid indices in the pitchwise direction. This can be achieved by imposing
the incoming local characteristic:
Note that only c4 has been changed (control by the expert parameter RS_LocalCorrection_).
Sensitivity tests have proved that this method is more robust and produce better results than the
one with c1 and c4 modified.
Therefore the fourth characteristic for downstream patches are:
9.1.4
Frozen Rotor
The frozen rotor technique consists of a simple connecting boundary condition, ignoring the
rotation of the rotor. The implementation is identical to the one adopted in the full non-matching
domain scaling approach (Domain Scaling Method), except from the fact that no rotation of the
rotor-linked image is performed, allowing the creation of a steady-state solution.
9.2
UNSTEADY TURBOMACHINERY
CALCULATIONS
The unsteady multi-stage calculations with the domain scaling method is available within the
FINE™/Open solver to solve the unsteady flow in the turbomachinery.
9.2.1
Domain Scaling Method
A. Geometry Constraints
The Domain Scaling Method considers in the computational domain respectively K 1 and K 2
blade passages with the following condition to be satisfied:
.
where the indices 1 and 2 refer to the upstream and downstream sides of the interface, and P1 and
P2 are the pitches of the two connected blade rows.
If the numbers of blades in respectively the rotor and the stator are not equal, the user should
make the choice between:
l modeling a higher number of blade passages (or even the entire machine if a common multiple
can not be found). If for instance the numbers of blades are 16 & 24, the numbers of passages
to model are respectively 3 & 2. This permits to avoid the introduction of an error due to the
geometry scaling, at the cost of an increased memory requirement.
l scaling the geometry. The easiest way to proceed in order to obtain the required scaling is to
generate a mesh with a blade number different from the real one. The ratio between the
modified and the real blade numbers should be as close as possible to 1.0.
In some cases the most appropriate treatment may be a combination of the 2 above approaches. If
for instance the numbers of blades are 18 & 24, one could scale the stator by changing the number
of blades from 18 to 16, and then choose to model 2 & 3 passages. The scaling factor is then
1.125, instead of 1.33 in case only one blade passage is modeled.
B. Full Non-matching Approach
The FNMB approach is used for the domain scaling method. This is nearly the same as the
mixing plane approach, except from the fact that the mixing plane technique applied between the
two image must be replaced by an additional full non-matching connection.
C. Rotor/stator interaction treatment
The treatment of the boundary conditions in rotor/stator interface is done in five steps:
l Send solution: during this step, the solution is transferred from the boundary cells to arrays
used to store the solutions on the boundary faces.
l Get image solution: during this step the solution stored on the boundary faces is transferred to
the image patches.
l Apply rotor stator coupling: during this step, the fluxes are computed as well as the values on
the boundary faces. For that, we use the image patches.
l Get fluxes and solutions on patches: during this step, the fluxes and solutions computed on the
image patches are transferred on the real patches.
l Update of the solution in the boundary faces: from the values in the boundary cells and on the
boundary faces, we can compute the solutions in the boundary faces.
D. Solution Strategy
The major advantage of having the same pitch distance on both sides of the interface is that it
permits to avoid considering any time periodicity in the boundary condition treatment. The
boundary conditions to be imposed along the periodic boundaries inside the gap region are given
by
,
where
is the pitch distance on both sides of the interface. The "+" sign is to be used
when imposing boundary conditions on the lower periodic segment (minimum azimuthal
coordinates) and the "-" sign is to be used for the higher periodic segment (maximum azimuthal
coordinates). Along the rotor/stator interface, the boundary condition is defined as
,
where the parameter m is selected such that the point
is part of the computational
domain of row 3-i to allow for the interpolation across the interface. Since only the spatial
periodicity is accounted for in the connecting boundary condition, the periodic surfaces become
simple non- matching rotating boundaries, while the interface is a non- matching connecting
boundary. The solution procedure is then as follows, for each physical time t:
l Rotate the grid in function of the physical time step and of the rotation speed of each row.
l Resolve the flowfield at the given physical time t. The boundary conditions to be imposed
along the periodic segments are defined by this equation . The boundary condition to be
imposed along the interface boundary is defined by this equation.
l Save the flow solution for future post-processing.
This method does not impose any time periodicity in the boundary condition treatment and thus,
allows to capture all time frequencies of the various unsteady interactions, but occurring on a
modified geometry due to the grid scaling. The effect of the grid scaling on the accuracy of the
computed flow solution is of great importance when comparing computational results with the
experimental data, as another one-stage configuration has been truly resolved. These effects may
be summarized as:
l a shift in the spectrum of time frequencies for the blade row that has not been scaled.
l the modification in both blade rows of the Fourier modes that are propagating the flow
information.
The unsteady governing flow equations are resolved in the relative system of each row. Thus, no
grid rotation needs to be performed at each physical time step and only the interpolation data
structure needs to be modified in function of the relative position of each component. For
example, a downstream rotor will see an upstream stator moving in the opposite direction of its
own rotation velocity, while the upstream stator will see the rotor moving in the direction of the
rotor rotation velocity.
9.2.2
Choice of the Physical Time Step
For a general case the user specifies the amplitude of the physical time step. This time step is
constant through the whole calculation.
In the case of turbomachinery applications the user defines the time step in another manner, by
imposing the Number Of Angular Positions that the unsteady algorithm should solve within one
period.
The time to accomplish one full rotation being equal to 2π/
is the rotation speed of the
domain as defined in the Rotating Machinery page), the time step is computed using the
relations:
(
,
where
is the periodicity of the domain.
In case a variable rotational speed is imposed through the OpenLabs™ environment, the solver
takes into account the
profile input in the OpenLabs™ Resource Manager and determines a
different
for each time iteration based on the equation above. A variable physical time step
can also be imposed in the OpenLabs™ environment by directly using the PhysTimeStep
internally defined constant (further details in the Standard Time Accurate Solver page of the
Theory Guide).
9.3
HARMONIC METHOD
An attractive feature of FINE™/Open with OpenLabs™ is the computation of unsteady flows
using the so-called nonlinear harmonic method (He et al, 1998). The main idea is that the flow
perturbations that make the flow unsteady are written about a time-averaged value of the flow and
are Fourier decomposed in time. Casting the unsteady Navier-Stokes system into the frequency
domain, transport equations are obtained for each time frequency. The user controls the accuracy
of the unsteady solution through the order of the Fourier series.
The unsteady Reynolds Averaged Navier- Stokes equations are considered, formulated in
the conservative flow variable
Cartesian coordinates
in a rotating frame for
(x,y,z)
where
is the relative velocity.
The conservative variable is decomposed into a time-averaged value and a sum of periodic
perturbations, which in turn can be decomposed into N harmonics:
The first harmonic being the fundamental associated with the blade passing frequency (BPF) of a
blade row for instance. The harmonic amplitudes
are complex conjugates.
and
A time-mean flow equation is obtained by time-averaging the unsteady equations. This is like
Reynolds averaging, except that the unsteady perturbations are periodic fluctuations, assumed to
be preponderant over the turbulent fluctuations. The resulting time-mean flow equations are in a
conservative form and can be formulated following a finite-volume method as
where i is the cell number and Ωi its volume. Fc and Fv are respectively the discretized convective
and viscous fluxes, and ST is the source term that includes the Coriolis and centrifugal terms.
The nonlinearity makes the deterministic stress terms appear in the time-averaged equation in the
same way as Reynolds stress terms appear in the Reynolds averaged equations. They provide
new contributions Detc and Detv to the advective and viscous fluxes following:
(0-1)
where Dx = (τxx, τxy, τxz), Dy = (τyx, τyy, τyz), Dz = (τzx,τzy, τzz) are the strain terms and .
The deterministic stress contribution is of the form:
and
To compute the stress terms and perform the model closure, a transport equation for the unsteady
perturbations is obtained by retaining the first-order terms in the basic unsteady flow equations.
Considering the first N harmonic components of the periodic fluctuation U', a transport equation is
of the fluctuation. By casting the 1st order linearized
obtained for each complex amplitude
equation into the frequency domain, this harmonic perturbation equation is made space dependent
only like the time-averaged flow equation. It can be made pseudo time dependent and, being in a
conservative form, formulated following the finite-volume method:
9.3.1
Viscous Stresses & Turbulence Model
In the time-averaged and harmonic flow equations, the laminar viscosity is computed from the
averaged flow variables only.
The turbulence can be modeled by the eddy-viscosity models. The eddy viscosity is assumed
undisturbed by the unsteady fluctuations. Therefore, the total viscous terms are in a linear form:
9.3.2
Closure of the Model
The deterministic stress is directly computed from the harmonic values. The stress generated by
two fluctuations f' and g' reads
(0-2)
9.3.3
Rotor/Stator Connection Treatment
Vilmin et al. (2013) present a generalized method to treat the rotor/stator connection. Usually, the
rotor/stator interface is applied the coupling of two boundaries, arbitrarily named left and right.
Each boundary is the inlet or the outlet of a row adjacent to the interface that can be displaced
relatively to the row on the opposite side of the interface. This displacement can be either periodic
in time and space – associated with a rotation speed – or can be periodic in space only as a change
of azimuthal position. Thus, the name rotor/stator is restrictive, because the stator/stator interface
can be taken into account for adjacent stators. By definition, any row which is separated from a
reference row by a periodic motion interface generates a rank-1 periodic disturbance into that row
of reference; and a row which is separated by two periodic motion interfaces creates a rank-2
disturbance into the reference.
FIGURE 9.2
Rank-2 disturbance
Contributions to the quantity in a reference row by surrounding rows that are positioned or
relatively moving in a periodic manner, such as a stator relatively to a stator or a row rotating
relatively to another row. The adjacent row gives a time-varying or space-varying contribution,
which is named a rank- 1 disturbance, and the adjacent of the adjacent produces a rank- 2
disturbance via the adjacent of the reference.
FIGURE 9.3 and FIGURE 9.4 show a general case of the rank-2 harmonic method where two
rows have the same rotation speed (one harmonic per perturbation), whether there are adjacent or
not: there appear harmonics with interblade phase angles that are given by the difference of
number of blades between these two rows. Some of these harmonics have a null frequency,
because of the null relative rotation between the two rows. These are space harmonics that are
associated with the time-mean flow, and a particular case is that of the clocking configuration,
discussed above. The others have the non-null frequency of a time harmonic and are associated
with that time harmonic, which can be called a base time harmonic. Thus, because the mean
solution (in the sense of passage-averaged) must keep the periodicity of the row, and because the
base time harmonics must keep their interblade phase angle in the same row (and in particular
their amplitude keep the periodicity of the row), there are additional space harmonics associated
with the time-mean and also additional time harmonics associated with the time harmonics. The
number of additional harmonics is
harmonics per perturbation.
per base harmonic for
FIGURE 9.3
Rank-2 harmonic method (r1 and r3 have the same rotation speed)
FIGURE 9.4
Rank-2 harmonic method (r2 and r3 have the same rotation speed)
Case where r2 and r3 have the same rotation speed, like a rotor/stator/stator configuration. New
time harmonics and space harmonics are respectively associated with the base time harmonics and
the mean flow in these two rows.
The relation between the harmonics at the left (L) and right (R) sides of the periodic motion
interface is given by a Fourier reconstruction in space, along the azimuthal angle θ, of the
complex amplitudes of the harmonics. This is analogous to the formulation by Giles (1988), and
can be shown to be equivalent to the chorochronic formulation by Gerolymos et al. (2002). It
reads (Vilmin et al., 2013)
where N is the number of harmonics to decompose the disturbances from the left row into the
right row; j is a list of time indices, and f is a list of time indices which is a function of k and j;
corresponds to a spatial frequency along the azimuth, named the azimuthal number or
spatial mode, common to
and
.
The relation between a harmonic and another harmonic gives to this harmonic a spatial mode at
the side of the row interface where the connection is made. At the side of a row interface, a
harmonic has as many modes as it has connections with other harmonics and their conjugates ( k
< 0 ) on the opposite side of the row interface.
CHAPTER 10.
COMPUTED VARIABLES
The flow solution used by the FINE™/Open solver is stored in the ".aout" file, while CFView™ uses
separate solution output files, namely ".d1.s*" for scalar quantities and ".d1.v*" for vector quantities.
CFView™ requires a cell-vertex representation of the flow solution, i.e. the flow variables need to be
provided at the mesh vertices. Since the FINE™/Open solver treats the flow variables at cell centres, an
interpolation process is performed by the flow solver in order to compute the flow variables at the
mesh vertices.
In this section
10.1 Global Performance Output
226
10.1 GLOBAL PERFORMANCE OUTPUT
Surface integrals are approximated by rectangular sums: for any vector quantity
or scalar
quantity q,
The index B indicates a boundary cell face centre value, obtained by averaging the coordinates
of the four corners:
and the solution
0):
in the first inner (index 1) and first outer cell (index
.
All variables, except flow angles, are first computed locally from this consistent representation of
solution and geometry and then summed, multiplied by the appropriate weight
factor
. Averages are calculated for the following variables:
or
.
Static pressure is area averaged, all other variables are mass averaged. Explicitly, q representing
any of the enumerated scalars (other than p) and
its average:
.
The mass flow
is obtained from the above approximation with
, the area A with q =
1. The values of
are also computed from
and the averaged velocity components to be
compared with the directly averaged values.
CHAPTER 11.
REFERENCES
This chapter lists all the references used in FINE™/Open with OpenLabs™.
Abramzon B, Sirignano W.A., 1989, "Droplet vaporization model for spray combustion
calculations", Int. J. Heat and Mass Transfer, 32:1605-18
Adamczyk, J. J., 1985, "Model Equations for Simulating Flows in Multistage-Turbomachinery",
ASME Paper 85-GT-226.
Anker J.E., Claramunt K., Hirsch C., 2009 "Assessment and Modeling Approaches for the
Simulation of Non-premixed and Partially Premixed Turbulent Combustion Processes", ECM
2009 Fourth European Combustion Meeting, Vienna, Austria.
Arnone A., Liou M. and Povinelli L., 1995, "Integration of Navier-Stokes Equations Using Dual
Time Stepping and Multigrid Method", AIAA-Journal, Vol. 33:985-990.
Ashford G. A., and Powell K. G., 1996, "An unstructured grid generation and adaptive solution
technique for high-Reynolds number compressible flow", VKI (Von Karman Institute) Lecture
Series 1996-06.
A. Maltsev, A. Sadiki, and J. Janicka, "A new BML-based RANS modeling for the description
of gas turbine typical combustion processes," *Progress in Computational Fluid Dynamics, An
International Journal *, vol. 4, 2004, pp. 229 - 236.
Balay S., Abhyankar S, Adams M.F., Brown J., Brune P., Buschelman K., Dalcin L., Eijkhout
V., Gropp W.D., Kaushik D., Knepley M.G., Curfman McInnes L., Rupp K., Smith B.F.,
Zampini S., Zhang H. and Hang Z., 2016, PETSc Users Manual, Argonne National Laboratory,
ANL-95/11 – Revision 3.7.
Baldwin B., Lomax H., 1978. "Thin Layer Approximation and Algebraic Model for Separated
Turbulent Flows", AIAA-78-257.
Barth T. J. and Jespersen D., 1989, "The Design and Application of Upwind Schemes on
Unstructured Meshes", AIAA paper 89-0366.
Barlow R. S., Karpetis A. N., Frank J. H., Chen J.-Y., 2001, "Scalar Profiles and NO Formation
in Laminar Opposed-Flow Partially-Premixed Methane/Air Flames," Combustion and Flame,
127:2102-2118.
Berger M., Aftosmis M. J., Murman S. M., 2005 "Analysis of Slope Limiters on Irregular Grids",
AIAA Paper 2005-0490.
Bennett B.A., McEnally C.S., Pfefferle L.D., Smooke M.D., 2000, "Computational and
experimental study of axissymmetric coflow partially premixed methane/air flames", Combustion
and Flame, 123:522-546.
Bouwer. H., 1978, "Groundwater Hydrology", McGraw-Hill.
Chorin A. J. 1967, "A Numerical Method for Solving Incompressible Viscous Flow Problems",
J. of Comput. Phys., Vol. 2:12-26.
Chien K. Y., 1982, "Predictions of Channel and Boundary-Layer Flows with a Low-Reynolds-
Number Turbulence Model", AIAA J., Vol. 20, No. 1.
Chu, C. M., and S. W. Churchill , "Representation of the angular distribution of radiation
scattered by a spherical particles". Journal of the Optical Society of America vol. 45, no 11, pp
958-962. 1955.
Clark, G. C, C. M., Chu, and S. W. Churchill , " Angular distribution coefficients for radiation
scattered by a spherical particles". Journal of the Optical Society of America vol. 47, pp 81-84.
1957.
Claramunt K., Consul R., Carbonell D., Perez-Segarra C.D., 2006, "Analysis of the Laminar
Flamelet Concept for Nonpremixed Laminar Flames", Combustion and Flame, Vol.145:845-862.
Colomer G., Costa M., Consul R., Oliva A., 2004, "Three-dimensional numerical simulation of
convection and radiation in a differentially heated cavity using the discrete ordinates method",
International Journal of Heat and Mass Transfer, 47:257–269.
Coutier-Delgosha O., 2001, "Modélisation des écoulements cavitants : étude des comportements
instationnaires et application tridimensionnelle aux turbomachines", PhD. thesis, Institut National
Polythechnique de Grenoble.
Dannenhoffer J. F., 1988, "A Comparison of Two Adaptive Grid Techniques", in Proc. of the
2nd Conference on Grid Generation in Computational Fluid Dynamics, Eds Sengupta, S.,
Hauser, J., Eiseman, P.R., and Thompson, J.F., pp. 319-328
de Boer A., van der Schoot M.S., Bijl H., 2007, "Mesh Deformation Based on Radial Basis
Function Interpolation", Computers and Structures, Vol.85:784-795.
Eliasson P. and Nordstrom J., 1995, "The Development of an Unsteady Solver for Moving
Meshes", FFA/TN 1995-39.
Erdos J.I., Alzner E. & McNally W., 1977, "Numerical Solution of Periodic Transonic Flow
Through a Fan Stage", AIAA Journal, Vol. 15, No. 11, pp. 1559-1568
Fatsis A., Pierret S., Van den Braembussche R., 1995, "3D Unsteady Flow and Forces in
Centrifugal Impellers with Circumferential Distortion of the Outlet Static Pressure", ASME paper
95-GT-33.
Grosshandler W.L., 1993, "RADCAL: A narrow-band model for radiation calculations in a
combustion environment", NIST Technical Note 1402.
G.D. Raithby, " Discussion of the Finite Volume Method for radiation, and its application using
3D unstructured meshes". Numerical Heat Transfer, Part B, 35:389–405, 1999.
G.D. Raithby and E.H. Chui, " A Finite Volume Method for predicting a radiant heat transfer in
enclosures with participating media". Journal of Heat Transfer, 112:415–423, 1990
Gerolymos, G. A., Michon, G. J., and Neubauer, J., 2002, "Analysis and Application of
Chorochronic Periodicity in Turbomachinery Rotor/Stator Interaction Computations", AIAA
Journal of Propulsion and Power, Vol. 18, No. 6.
Giles, M.B., 1988, "Non-reflecting boundary conditions for the Euler equations", Technical
Report TR-88-1, MIT Computational Fluid Dynamics Laboratory.
Giles M.B., 1990, "Stator/Rotor Interaction in a Transonic Turbine", Journal of Propulsion and
power, Vol. 6, No. 5, pp. 621-627
Hakimi N., 1997, "Preconditioning methods for time dependent Navier-Stokes equations", PhD
Thesis, Dept of Fluid Mechanics, Vrije Universiteit Brussel.
He, L. and Ning, W., 1998, "Efficient Approach for Analysis of Unsteady Viscous Flows in
Turbomachines", AIAA Journal, Vol. 36, No. 11.
Hirsch Ch., 1990, "Numerical Computation of Internal and External Flows. Volume 2", John
Wiley & Sons.
Holmes D. G., Connell S. D., 1989, "Solution of the 2D Navier- Stokes Equations on
Unstructured Adaptive Grids". AIAA Paper 89-1932
Jameson A., Schmidt W., Turkel E., 1981, "Numerical Solutions of the Euler Equations by Finite
Volume Methods using Runge-Kutta Time-Stepping Schemes", AIAA-81-1259.
Jameson A., 1991, "Time Dependent Calculations Using Multigrid, with Applications to
Unsteady Flows Past Airfoils and Wings", AIAA-Paper 91-1596.
Jameson, A., 1995, "Analysis and design of Numerical Schemes for Gas Dynamics, 1: Artificial
Diffusion, Upwind Biasing, Limiters and Their Effect on Accuracy and Multigrid
Convcergence", International Journal of Computational Fluid Dynamics, Volume 4:171-218.
Jameson A., 1995, "Analysis and Design of Numerical Schemes for Gas Dynamics, 2: Artificial
Diffusion and Discrete shock Structure", International Journal of Computational Fluid Dynamics,
Volume 5:1-38.
Jameson A., 1995, "Positive schemes and shocks modeling for compressible flows", International
Journal for Numerical Methods in Fluids, Vol. 20:773-776.
Kalitzin G., Medic G., Iaccarion G., Durbin P., 2005, "Near- Wall Behavior of RANS
Turbulence Models and Implications for Wall Functions", Journal of Computational Physics,
Vol.204, pp265-291.
Kallinderis Y. and Baron J. R., 1989, "Adaptation Methods for a New Navier- Stokes
Algorithm", AIAA Journal, Vol. 27:37-43.
Kaviany M., 1995, "Principles of Heat Transfer in Porous Media", Second Edition, Springer.
Kroll N., Jain R. K., 1987, "Solution of Two-Dimensional Euler Equations – Experience with a
Finite Volume Code", DFVLR-FB 87-41.
Kovalev K., 2005, "Unstructured Hexahedral Non-conformal Mesh Generation", Ph.D. Thesis,
Vrije Universiteit Brussel, Belgium.
Launder B. E. and Sharma B. I., 1974, "Application of the Energy- Dissipation Model of
turbulence to the Calculation of Flow Near a Spinning Disc", Letters in Heat and Mass Transfer,
Vol. 1:131-138.
Launder B. E. and Spalding D. B., 1974, "The numerical computation of turbulent flow",
Comput. Methods App. Mech. Eng., vol. 3:269-289.
Lemeur A., 1992, "Calculs 3D stationnaire et
transonique", AGARD Report CP-510
instationnaire dans un étage de turbine
Livne O.E., Wright G.B., 2006, "Fast Multilevel Evaluation of Smooth Radial Basis Function
Expansions", Electronic Transactions on Numerical Analysis, Vol.23:263-287.
Lorrain E., Tartinville B., Capron A., Hirsch Ch., 2009, "A 3D multigrid algorithm applied to
cavitation for rotating machinery", 8th European Conference on TURBOMACHINERY Fluid
Dynamics and Thermodynamics.
Majda A., Sethian J., 1985, "The derivation and numerical solution of the equations for zero
Mach number combustion", Combust. Sci. Technol. 42 :185-205.
Marques N. P. C., Pereira, J. C. F., 2001, "Comparison of Three Second- order Accurate
Reconstruction Schemes for 2D Euler and Navier-Stokes Compressible Flows on Unstructured
Grids", Commun. Numer. Math. Engng., Vol. 17:309-323.
Martinelli L. ,1987, "Calculations of Viscous Flow with a Multigrid Method", PhD Thesis, MAE
Department, Princeton University.
Melson N. D., Sanetrik M. D., Atkins, H. L., 1993, "Time accurate Navier-Stokes calculations
with multigrid acceleration", AIAA paper, pp. 1041-1042.
Mengüç M., Viskanta R., 1985, "Radiative transfer in three-dimensional rectangular enclosures
Journal of Quantitative
containing inhomogeneous,
Spectroscopy & Radiative Transfer, 33:533-549.
anisotropically scattering media",
Menter F., 1992, "Influence of freestream values on k-ω turbulence model predictions", AIAA J.,
Vol. 30, No. 6, pp1657-1659.
Menter F., 1993, "Zonal two-equation k-ω turbulence model for aerodynamic flows", in AIAA
24th Fluid Dynamics Conference, AIAA paper 93-2906, (Orlando, FL).
Menter F., 1992, "Performences of popular turbulence models for attached and separated adverse
pressure gradient flows", AIAA Journal, vol.30, pp.2066-2072.
Menter F., 1994, "Two-equation eddy viscosity turbulence models for engineering applications",
AIAA Journal, vol.32, pp.1299-1310.
Menter F., Garbaruk A.V., Egorov Y., 2009, "Explicit algebraic Reynolds stress models for
anisotropic wall- bounded flows", EUCASS – 3rd European Conference for Aero- Space
Sciences, Versailles.
Merkle C.L., Sullivan J.Y., Buelow P.E.O., Venkateswaran S., 1998, "Computation of Flows
with Arbitrary Equations of State", AIAA J. Vol.36:515-521.
Minier J.P. and PeiranoE., 2001, "The PDF approach for turbulent polydispersed two-phase
flows", Physics Reports, 352:1-214.
Modest M.F., 2003, "Radiative Heat Transfer", Academic Press.
M. Metghalchi and J.C. Keck, "Burning velocities of mixtures of air with methanol, isooctane,
and indolene at high pressure and temperature," Combustion and Flame, vol. 48, 1982, pp. 191-
210.
Nakamura T., van de Kamp W.L., Smart J.P., 1991, "Further studies on high temperature natural
gas combustion in glass furnaces", IFRF Doc. Number F90/y/7, IJmuiden, The Netherlands.
Nichols R. H., 1990, "A Two-Equation Model for Compressible Flows", AIAA paper 90-0494.
Patel A., 2003, "Development of an Adaptive RANS Solver for Unstructured Hexahedral
Meshes", Ph. D. Thesis, ULB, Belgium.
Peters N. , 2000, "Turbulent Combustion", Cambridge University Press
Pierce N. A., Alonso J. J., 1997, "A Preconditioned Implicit Multigrid Algorithm for Parallel
Computation of Unsteady Aeroelastic Compressible Flows", AIAA paper 97-0444.
Pitsch H., 2000, "Unsteady Flamelet Modeling of Differential Diffusion in Turbulent Jet
Diffusion Flames", Combustion and Flame, Vol.123:358-374.
Poinsot T. , Veynante D., 2001, "Theoretical and Numerical Combustion", R.T. Edwards.
Press W. H., Teykolsky S. A., Vetterling W. T., Flannery B. P., 1992, "Numerical Recipes in C",
2nd ed., Cambridge University Press.
Rai M.M., 1989, "Three- Dimensional Navier- Stokes Simulations of Turbine Rotor- Stator
Interaction; Part I - Methodology and Part II - Results", Journal of Propulsion and power, Vol. 5,
No. 3, pp. 305-319
Radespiel R., Rossow C., Swanson R. C., 1989, "An Efficient Cell-Vertex Multigrid Scheme for
the Three-Dimensional Navier-Stokes Equations", AIAA Paper 89-1953.
Rizzi A., Viviand H., 1981, "Numerical Methods for the Computation of Inviscid Transonic
Flow with Shock Waves", Notes on Numerical Fluids Mechanics, GAMM Workshop.
Saad Y., 2003, "Iterative Methods for sparse linear systems", 2nd edition, Society for Industrial
and Applied Mathematics.
Sarkar S., Erlebacher G., Hussaini M. Y., Kreiss H. O., 1991, "The analysis and modeling of
dilatational terms in compressible turbulence", J Fluid Mech, Vol.227:473-493.
Schiller, L. and Naumann, A., 1935, "A drag coefficient correlation", VDI Zeitung, 77:318-320.
Shur M. L., Strelets M. K., Travin A. K., Spalart P. R., 2000, "Turbulence Modeling in Rotating
and Curved Channels: Assessing the Spalart-Shur Correction", AIAA Journal, Vol 38:784-792.
Smith T.F., Shen Z.F., Friedman J.N., 1982, "Evaluation of coefficients for the weighted sum of
gray model", Transactions of the ASME, 104:602-608.
Spalart P. R. and Allmaras S. R., 1992, "A one equation turbulence model for aerodynamic
flows", AIAA 92-0439.
Stokes, G.G., 1850, "On the effect of the internal friction of fluids on the motion of pendulums",
Trans. Cambridge Phil. Soc., 9:8-23.
S. Pfadler, J. Kerl, F. Beyrau, A. Leipertz, A. Sadiki, J. Scheuerlein, and F. Dinkelacker, "Direct
evaluation of the subgrid scale scalar flux in turbulent premixed flames with conditioned dual-
plane stereo PIV," *Proceedings of the Combustion Institute*, vol. 32, pp. 1723-1730.
Tim Peeters, 1995, "Numerical modeling of turbulent natural-gas diffusion flames", PhD. Thesis.
Truelove J.S., 1975, HTFS Design Report DR33 (Part I:AERE- R8167), Atomic Energy
Authority.
Vandromme D., 1991, "Turbulence Modeling for Compressible Flows and Implementation in
Navier-Stokes Solvers", VKI Lecture Series 1991-02.
Venkatakrishnan V., 1995, "Convergence to Steady State Solutions of the Euler Equations on
Unstructured Grids with Limiters", J. Comp. Phys. Vol 188:120-130.
V.L. Zimont, W. Polifke, M. Bettelini, and W. Weisenstein, "An Efficient Computational Model
for Premixed Turbulent Combustion at High Reynolds Numbers Based on a Turbulent Flame
Speed Closure," Journal of Engineering for Gas Turbines and Power, vol. 120, Jul. 1998, pp.
526-532.
V.L. Zimont, "Gas premixed combustion at high turbulence. Turbulent flame closure combustion
model," Experimental Thermal and Fluid Science, vol. 21, Mar. 2000, pp. 179-186. V.L. Zimont,
F. Biagioli, and K. Syed, "Modeling turbulent premixed combustion in the intermediate steady
propagation regime," Progress in Computational Fluid Dynamics, An International Journal , vol.
1, 2001, pp. 14-28.
Van Leer B., 1985, "Upwind-Difference Methods for Aerodynamic Flows Governed by the
Euler Equation", Lectures in Applied Mathematics, Vol. 23, Part 2, AMS, Providence, pp. 327-
336
Vilmin S., Lorrain E., Hirsch C., Swoboda M., 2006, "Unsteady Flow Modeling Across The
Rotor/Stator Interface Using The Nonlinear Harmonic Method", ASME Paper GT-2006-90210.
Vilmin S., Lorrain E., Hirsch C., Swoboda M. 2009. "Application of a Nonlinear Harmonic
Method to the Simulation of Clocking Effects", ASME Paper GT2009-59475.
Vilmin S., Lorrain E., Tartinville B., Capron A., Hirsch C., 2013. "The nonlinear harmonic
method: from single stage to multi-row effects", International journal of computational fluid
dynamics, Vol. 27: pp. 88-99.
Vilmin S., Lorrain E., Debrabandere F., Tartinville B., Capron A., Hirsch C., 2013. "The
nonlinear harmonic method applied to the combined effects of multi-row unsteady flows", ASME
Paper GT2013-94847.
Vreman A.W., Albrecht B.A., van Oijen J.A., de Goey L.P.H., Baastians R.J.M., 2008,
"Premixed and Nonpremixed Generated Manifolds in Large-eddy Simulation of Sandia Flame D
and F", Combustion and Flame, Vol.153:394-416.
Warnatz J., Maas U., Dibble R.W., 2001, "Combustion", Springer, Berlin, 3rd edition.
Yang Z. and Shih T. H., 1993, "A k-ε model for turbulence and transitional boundary layer",
Near-Wall Turbulent Flows, R.M.C. So., C.G. Speziale and B.E. Launder(Editors), Elsevier-
Science Publishers B. V., pp. 165-175.
Zhang H. S., So R. M. C., Speziale C. G., Lai Y. G., 1991, "A Near- Wall Model for
Compressible Turbulent Flow", ICASE Report 91-82.
Zhu Z. W. 1996, "Multigrid Operation and Analysis for Complex Aerodynamics", PhD Thesis,
Vrije Universiteit Brussel, Belgium.
© NUMECA International, all rights reserved
EN201805172158

CHAPTER 4. FLOW MODEL
4.1 Mathematical Model
Introduction to Turbulence
Euler
Laminar Navier-Stokes
Turbulent Navier-Stokes
4.1.1
4.1.2
4.1.3
4.1.4 Advanced Parameters for Turbulence modeling
Best Practice for Turbulence Modeling
4.1.5
A.
B. First Step: Choosing a Turbulence Model
C. Second Step: Generating an Appropriate Grid
D. Defining Initial and Boundary Conditions
E. Wall Distances
LES/DES models
A. Brief Overview of Models
B. Best Practice
4.1.6
4.1.7 Gravity Forces
4.1.8 Heat Source
4.2 Characteristic Values - Reynolds Number
CHAPTER 5. SOLID MODEL
5.1 Solid Model Interface
5.2 Advanced Parameters for Solid Model
5.3 Best Practice for Conjugate Heat Transfer
5.3.1
5.3.2
5.3.3
Step 1: Determine the Solid and Fluid Blocks
Step 2: Setting the Global Parameters
Step 3: Setting the Thermal Connections
CHAPTER 6. BOUNDARY CONDITIONS
6.1 Boundary Conditions in FINE™/Open with OpenLabs™
Inlet Condition
6.1.1
6.1.2 Outlet Condition
6.1.3
6.1.4
6.1.5 Advanced Parameters for the Boundary Condition
Solid Wall Boundary Condition
External Condition (Far-field)
6.2 Best Practice for Imposing Boundary Conditions
CHAPTER 7. NUMERICAL MODEL
7.1 Numerical Model
7.1.1 Numerical Model in FINE™/Open with OpenLabs™
A. CPU booster
B. Multigrid
C. Numerical Schemes
7.1.2 Advanced Parameters for the Numerical Model
Interfaced Advanced Parameters
A.
B. Non-interfaced Advanced Parameters
FINE™/Open with OpenLabs™ 7.2 User Guide
95
95
95
95
98
100
100
101
102
106
110
111
112
115
122
123
126
128
129
130
131
131
132
134
137
141
143
147
148
149
152
154
154
154
157
161
CHAPTER 1.
GETTING STARTED
Welcome to the FINE™/Open User's Guide, a presentation of NUMECA's F low IN tegrated
Environment for computations on unstructured meshes. This chapter presents the basic concepts of
FINE™/Open with OpenLabs™ and shows how to get started with the program by describing:
l what FINE™/Open with OpenLabs™ does and how it operates,
l how to use this guide,
l how to start the FINE™/Open GUI.
In this section
1.1 Introduction
1.2 How To Use This Manual
1.3 First Time Use
1.4 How to start FINE™/Open GUI
1.5 Required Licenses
10
13
14
16
17
1.1
INTRODUCTION
Components
The resolution of Computational Fluid Dynamics (CFD) problems involves three main steps:
l spatial discretization of the flow domain,
l flow computation,
l visualization of the results.
To perform these steps NUMECA has developed three software systems. The first software
system, HEXPRESS™, is an automated all- hexahedral unstructured grid generation system.
HEXPRESS™ also includes a module HEXPRESS™/Hybrid, which allows to mesh complex
geometries with an isotropic hybrid mesh including mainly hexahedral cells with tetrahedral,
pyramid and prism cells. The second software system, FINE™/Open with OpenLabs™, is a
powerful CFD Flow Integrated Environment dedicated to complex internal and external flows.
The third software system, CFView™, is a highly interactive Computational Field Visualization
system.
These three software systems have been integrated in a unique and user friendly Graphical User
Interface (GUI), called FINE™/Open with OpenLabs™, allowing the solution of complete
simulations of 3D internal and external flows from the grid generation to visualization, without
any file manipulation, through the concept of a project. Moreover, multi-tasking capabilities are
incorporated, allowing the simultaneous treatment of multiple projects.
Multi-tasking
FINE™/Open with OpenLabs™ fully integrates the concept of multitasking. This means that the
user can manage a complete project
in the FINE™/Open GUI; making the grid using
HEXPRESS™, running the computation with the FINE™/Open solver and visualizing the
results with CFView™. Furthermore, the user has the possibility to start, stop and control multiple
computations. Please note that
therefore the
possibility of running computations in the background has been implemented. See the Task
Manager for more details on how to manage multiple tasks through the interface or in
background.
the flow simulation can be time consuming,
Project Management
To manage complete flow analyses, FINE™/Open with OpenLabs™ integrates the concept of
project. A project involves grid generation, flow computation and visualization tasks. The results
of each of these tasks are stored in different files that are automatically created, managed and
modified within FINE™/Open with OpenLabs™:
l The grid files: The grid generation process in HEXPRESS™ (HEXPRESS™/Hybrid)
creates files containing the representation of the geometry, the grid related to the project and
the definition of the boundary conditions types. Five files with respectively extensions ".igg",
".dom", ".bcs", ".hex" (".sph") and ".fnmb" contain all relevant information about the mesh.
Furthermore, two files with extensions ".rep" and ".dist" contain respectively the report of the
grid generation process and the wall distance.
The file with extension ".dist" is only available when the distance criteria is used during surface
adaptation (more details in HEXPRESS™ User Manual).
l The project file: The project file is created by FINE™/Open with OpenLabs™ with the
extension ".iec" and it contains the input parameters needed for the flow computations.
l The result files: FINE™/Open with OpenLabs™ creates a new subdirectory for each
computation where it stores the following files :
l a file with extension ".run" containing all computation input parameters used by the solver
and by CFView™,
l a file with extension ".dtw" containing the distance to the wall for each grid nodes,
l a ".bout" file that contains the solution and is used for restarting the solver,
l a series of ".di.sj" and ".di.vj" files (where respectively i and j stand for the ID number of
the domain and the ID number of the scalar or vectorial quantity) and the ".cfv" file used by
CFView™ in order to visualize the quantities,
l a ".res" file used by the Monitor to visualize the residual history ,
l two files used to visualize the convergence history in the Steering with extensions
".steering" and ".steering.binary",
l a ".mf" file that contains global solution parameters,
l a ".wall" file that contains information on forces and moments,
l a ".std" file that contains global information about the computation history. If the flow
solver encounters a problem, warning/error messages will be described in the std file. The
.std file can be checked quickly by clicking the button View computation std file(s) in the
TaskManager INFO window.
l a set of ".log" files under the sub folder report that contain global information about the
computation history. These files are used for support purposes only. If problems are
encountered, all ".log" files should be sent to your local support office together with the
problem description.
l a ".batch" file used to launch the computation using scripts .
l The CFView™ visualization files: In addition to the ".run" and ".cfv" files, the flow solver
creates a series of files, which can be read by CFView™. These files have different
extensions. For example in the case of a perfect gas compressible flow simulation at moderate
Mach number, density in the first domain will be visualized in CFView™ through reading of
the file with extension ".d1.s1".
FIGURE 1.1
Example of file management for a FINE™/Open with OpenLabs™ project
Through the interface, the user can modify all the information stored in the files associated to the
project.
When creating a new project (e.g. "project.iec"), a new directory is made "\project". In this directory
the project file is stored: "\project\project.iec" and a directory is created called "\project\_mesh\". In
this last sub- directory, the user is invited to store the grid files used for the computations. It is
however also possible to select a grid that is located in another directory. Only one mesh file should
be used for all computations in a project. If computations need to be done on another mesh file, it is
advised to duplicate the existing project or to create a new project for those computations.
The special characters, such as ü, ë and ê et al., are not allowed in the path name.
The white space is not allowed in the path name.
1.2
HOW TO USE THIS MANUAL
Outline
This manual consists of five distinct parts:
l Getting Started and User Interface: Introduction and description of the interface,
l Fluid Model to Initial Solution: Computation definition,
l Outputs and Monitoring & Launching Mode,
l Task Manager,
l Python script
l Annex: File formats,
l Annex: List of advanced parameters.
Before using FINE™/Open with OpenLabs™ for the first time, it is recommended to read this
first chapter carefully. The User Interface chapter gives a general overview of the FINE™/Open
GUI and explains how to manage a project. For each computation, the input parameters can be
defined as described in the chapters Fluid Model to Initial Solution. Outputs and Monitoring &
Lauching Mode describes outputs coming out FINE™/Open with OpenLabs™ as well as the
monitoring tool. Task Manager gives an overview of how to run calculations using the Task
Manager or using a script. Finally, Python script gives a description of all python commands that
allow to automate the settings of the project.
The experienced user can find, in all chapters, a section describing advanced options that are
available in the Advanced tabs of the various pages. Additionally,
the List of advanced
parameters provides a list of all supported non-interfaced advanced parameters, which are located
in the Advanced tab of the Computation Steering/Control Variables page. For each parameter
a reference is given to the section in the manual where it is described.
The use of non- supported parameters is at own user risk and will not guarantee correct and/or
physical results.
Conventions
Some conventions are used to ease information access throughout this guide:
l Commands to type in are in italics.
l Keys to press are in italics and surrounded by <> (e.g.: press <Ctrl>).
l Names of menu, sub-menu items and names of buttons in dialog boxes are in bold.
l Numbered sentences are steps to follow to complete a task. Sentences that follow a step and
are preceded with a dot (•) are substeps. They describe in detail how to accomplish the step.
A text in blue with a blue background indicates an important note.
Keyboard shortcuts are shown in blue italic.
A light bulb indicates a section with a description of advanced parameters.
1.3
FIRST TIME USE
1.3.1
Basic Installation
When using FINE™/Open with OpenLabs™ for the first time it is important to verify that
FINE™/Open with OpenLabs™ is properly installed according to the installation note. The
installation note provided with the installation software should be read carefully and the following
points are especially important:
l Hardware and operating system requirements should be verified to check whether the chosen
machine is supported.
l Installation of FINE™/Open with OpenLabs™,
in a directory chosen by the user and
referenced in the installation note as "NUMECA_INSTALLATION_DIRECTORY", should
respect the described procedure in the installation note.
l A license should be requested that allows the use of FINE™/Open with OpenLabs™ and the
desired component and modules. The license should be installed according to the procedure
described in the installation note.
l Each user wishing to use FINE™/Open with OpenLabs™ or any other NUMECA software
must perform a user configuration as described in the installation note.
When these points are checked the software can be started as described in the installation note.
1.3.2
Advanced Graphics Options
A. Graphics Driver
The graphics area of FINE™/Open GUI uses by default an OPENGL driver that takes advantage
of the available graphics card. When the activation of OPENGL is causing problems, FINE™
uses an X11 driver (on Linux) or MSW driver (for Windows) instead.
It is possible to explicitly change the driver used by FINE™/Open with OpenLabs™ in the
following ways:
On Linux
in csh, tcsh or bash shell:
setenv NI_DRIVER X11
in korn shell:
NI_DRIVER=X11
export NI_DRIVER
The selection will take effect at the next session.
On Windows
l Log in as Administrator.
l Launch regedit from the Start/Run menu.
l Go to the HKEY_ LOCAL_ MACHINE/SOFTWARE/NUMECA International/Fineopen#
register.
l Modify the DRIVER entry to either OPENGL or MSW.
The selection will take effect at the next session.
B. Background Color
The background color of the graphics area can be changed by setting the environment variable
NI_ IGG_ REVERSEVIDEO on Linux platforms or IGG_ REVERSEVIDEO on Windows
platforms. Set the variable to "ON" to have a black background and set it to "OFF" to have a
white background. The variable can be manually specified through the following commands:
On Linux
in csh, tcsh or bash shell:
setenv NI_IGG_REVERSEVIDEO ON
in korn shell:
NI_IGG_REVERSEVIDEO=ON
export NI_IGG_REVERSEVIDEO
The selection will take effect at the next session.
On Windows
l Log in as Administrator.
l Launch System Properties from the Start/Settings/Control Panel/System menu.
l Go in the Environment Variables.
l Modify or add the IGG_REVERSEVIDEO entry to either ON or OFF.
The selection will take effect at the next session.
1.4
HOW TO START FINE™/OPEN GUI
In order to run FINE™/Open with OpenLabs™, the following command should be executed:
On Linux platforms type: fine# <Enter> where # stands for the release version number (i.e.
open211_1).
When multiple versions of FINE™/Open with OpenLabs™ are installed, or if FINE™/Open with
OpenLabs™ is installed with FINE™/Turbo, the installation note should be consulted for advice on
how to start FINE™/Open with OpenLabs™ in a multi-version environment.
On Windows click on the FINEOpen icon in Start/Programs/NUMECA software/Fine#.
Alternatively FINE™/Open with OpenLabs™ can be launched from a dos shell by typing:
<NUMECA_INSTALLATION_DIRECTORY>\fineopen72\bin64\fine_openx86_64.exe
<Enter>
where "NUMECA_INSTALLATION_DIRECTORY" is the directory indicated.
1.5
REQUIRED LICENSES
Standard FINE™/Open with OpenLabs™ License
The standard license for FINE™/Open with OpenLabs™ allows for the use of all basic features
of FINE™/Open with OpenLabs™ including:
l HEXPRESS™ ,
l HEXPRESS™/Hybrid ,
l CFView™ ,
l Task Manager,
l Monitor,
l OpenLabs.
Additional Licenses
Within FINE™/Open with OpenLabs™ the following features require a separate license:
l parallel computations ,
l CATIA v5 importation ,
l conjugate heat transfer ,
l porous media model ,
l combustion model ,
l coupling with MpCCI ,
l coupling with modal approach ,
l coupling with Oofelie ,
l fluid-particle interaction ,
l radiation model ,
l uncertainty quantification ,
l treatment of unsteady rotor-stator interface ,
l thermodynamic tables ,
l TabGen ,
l TabGen/Chemistry .
In addition to FINE™/Open with OpenLabs™, other products are available that require a
separate license:
l FINE™/Turbo (Flow INtegrated Environment using structured mesh technology, see
FINE™/Turbo, IGG™, AutoGrid user manuals),
l AutoBlade™ & FINE™/Design 3D (structured 3D inverse design technology, see
FINE™/Design 3D, AutoBlade™ user manual).
l FINE™/Marine (unstructed mesh generator - solver - visualization software) dedicated to
marine applications.
CHAPTER 2.
INTERFACE
When launching FINE™/Open with OpenLabs™, as described in Getting Started chapter, the interface
appears in its default layout as shown in FIGURE 2.1. An overview of the complete layout of the
FINE™/Open GUI is shown on the next page in FIGURE 2.2. In the next sections the items in this
interface are described in more detail.
Together with the FINE™/Open GUI a Project Selection window is opened, which allows the creation
of a new project or the opening of an existing project. See Project Selection section for a description
of this window.
A File Chooser window is available for browsing through the file system and to select a file. More
detail on the File Chooser window is given in File Chooser section.
To define a profile through the FINE™/Open GUI a Profile Manager is included. The Profile Manager
is described in more detail in Profile Manager section.
FIGURE 2.1
Default FINE™/Open GUI
2.11 File Chooser
2.12 Profile Manager
74
75
2.1
PROJECT SELECTION
When the FINE™/Open GUI is started, the Project Selection window, as shown in FIGURE
2.1, appears together with the interface.
This window allows the creation of a new project or the opening of an existing one as described
in the next sections. To open a project or to create a new one without the Project Selection
window is also possible using the Project menu.
The Project Selection window also suggests the user to start working within the TurboWizard
directly from here. More details about the TurboWizard can be found in the "Using the
Turbowizard" (p. 24) section.
FIGURE 2.3
Project and Grid File Selection window
2.1.1
Create New Project
To create a new project when launching the FINE™/Open GUI:
1. The Open an existing project should be left deactivated. Then after clicking on Ok, a Grid
File Selection menu (FIGURE 2.3) is appearing to assign a grid to the new project. There are
three possibilities:
l Open an existing grid by clicking on Importing a mesh.
l If the required grid is not yet created use Creating a mesh.
l Another possibility is to create a turbomachinery (impeller/volute) setup including the grid
Using the TurboWizard.
2. If the Creating a mesh is selected, a file chooser appears, which allows the selection of a
name and location for the new project (for more detailed information on the File Chooser
window see File Chooser section).
l In the Directories text box a name can be typed or the browser under the text box may be
used to browse to an appropriate location.
l Once the location is defined type a new name in the text box under Files, for example
"project.iec" (it is not strictly necessary to add the extension ".iec", FINE™/Open with
OpenLabs™ will automatically create a project file with this extension).
l Click on Ok (Save on Windows) to accept the selected name and location of the new
project.
3. A new directory is automatically created with the chosen name as illustrated in FIGURE 2.5
indicated by point (1). All the files related to the project are stored in this new directory. The
most important of them is the project file with the extension ".iec", which contains all the
Inside the project directory FINE™/Open with
project settings ( FIGURE 2.5 - (2)).
OpenLabs™ creates automatically a subdirectory "_mesh" (FIGURE 2.5-(3)).
4. Depending on your choice regarding the grid file selection (step 1), there are three possibilities:
l If you have chosen to create a grid file, HEXPRESS™ is launched after defining the new
project. You can then create the mesh and save it in the "_mesh" directory of the new
project. Click on Close icon in HEXPRESS™ to return to the FINE™/Open with
OpenLabs™ project. The new mesh is automatically associated to the project. Mesh scaling
properties can be set using the Mesh/Properties... menu within FINE™/Open with
OpenLabs™ (refer to Mesh Properties section).
l If you have chosen to open a grid file, a file chooser, after defining the new project, allows
you to browse to the grid file with extension ".igg" or ".msh". Select the unstructured grid
file and press OK to accept the selected mesh. The new mesh is automatically associated to
the project and the mesh scaling properties can be set through the Mesh properties window.
Mesh scaling properties can be set afterwards using the Mesh/Properties... menu (refer to
Mesh Properties section).
l If you have chosen to create a project Using the TurboWizard a wizard embedded in
FINE™/Open with OpenLabs™ would guide you through the entire setup of a
turbomachinery (impeller/volute) project.
It is suggested to generate and save meshes in the latest HEXPRESS™. In case that the mesh is not
saved in the latest version, the computation will run correctly but CFView™ may crash when loading
a quantity.
FINE™/Open with OpenLabs™ allows to link a TGrid mesh (".msh") to a project. When linking
a Tgrid mesh, FINE™/Open with OpenLabs™ will automatically create some HEXPRESS™
files (".bcs", ".igg" and ".dom"). These files do not contain any information about topological
entity discretisation. As a consequence, the geometry can not be displayed in the graphic view.
No periodic boundaries are allowed in the TGrid mesh (.msh).
For a project linked with a TGrid mesh, CFView™ is not available for post-processing. The user has
to select Ensight in the Computation Controls / Outputs page to activate the Ensight output and post-
process the results in Ensight.
The computation using HEXPRESS™/Hybrid or TGrid mesh must be launched in parallel mode.
2.1.2
Open Existing Project
To open an existing project, the two following possibilities are available after clicking on Open
an Existing Project:
l Click on Ok and a file chooser appears, which allows the selection of a name and location for
the new project (for more detailed information on the File Chooser window see File Chooser
section).
l Select the project to open by double-clicking on it in the list of Recent Projects, which
contains the most recently used project files. The selected project will then be loaded. If a
project no longer exists it will be removed from the list when selected. Furthermore, by
double-clicking on the More files... line, a file chooser will appear that allows to browse to the
location of the existing project. Automatically the filter in the file chooser is set to display only
the files with extension ".iec", the default extension for a project file.
Once the mesh is opened, the geometry is loaded in the graphics area of the interface. The mesh
itself is not visible, unless it is loaded manually (Mesh/Load Mesh menu).
2.1.3
Using the Turbowizard
To create a new impeller/volute project within FINE™/Open with OpenLabs™ using the
TurboWizard module, the Using the TurboWizard option should be selected.
l After clicking on Ok, the TurboWizard - step 1 window appears, allowing the user to create
a new project or to load a previous case in the first step of the TurboWizard.
l More information about
this embedded wizard dedicated to turbocharger or centrifugal
compressor project setup can be found in the "Turbowizard module" (p. 38) section.
2.1.4 Mesh Properties
The Mesh properties window appears automatically when creating a new project (link a mesh)
or attaching a new mesh to an existing project (Mesh/Link a mesh file). This window can also be
displayed manually (Mesh/Properties... menu)
l Grid Units under the tab General: the user can specify the grid units after importing a mesh
through the Mesh/Properties... menu. A different scale factor may be defined to convert the
units of the mesh to meters. The scale factor is for instance 0.01 when the grid is in
centimeters.
l Information about the number of cells, vertices and periodicity is displayed per block (domain)
under the tab General.
l Information about the global mesh quality is displayed under the tab Quality. FINE™/Open
with OpenLabs™ will check the mesh quality when linking a mesh to the project. If the value
of the quality items is not reached the criteria, the items will be shown in red. In FINE™/Open
with OpenLabs™, the mesh quality criteria is as follows:
Invalid mesh:
l Mesh is not snapped
l Negative cells
l FNMB connections are not computed
l Undefined boundary type
Mesh quality should be improved:
l Existence of concave or twisted cells
l minimum skewness < 5 degree
l averaged skewness < 65 degree
l maximum aspect ratio > 5000
l maximum expansion ratio > 20
Mesh quality is satisfying, but could be improved:
l minimum skewness < 15 degree
l averaged skewness < 75 degree
l maximum aspect ratio > 2000
l maximum expansion ratio > 5
When creating a new project, linking a new mesh, opening an existing project or switching from
HEXPRESS™ to FINE™/Open with OpenLabs™ environment, a warning message will be
shown if the mesh quality is not good enough. In case of invalid mesh, the flow solver can not be
started.
The mesh quality information is only available for the mesh generated/converted in HEXPRESS™
v3.1-1 or higher.
FIGURE 2.4
Mesh properties window
2.2 MAIN MENU BAR
2.2.1
Project Menu
New Project
The Project/New menu allows the user to create a new FINE™/Open with OpenLabs™ project.
When clicking on Project/New , the Project Selection window appears, and the user has the
possibility to create a new project or to open an existing project, see Project Selection section.
During the new project creation, the user has the possibility to choose whether to create a new
grid or to assign an existing grid to the project, through a Grid File Selection box.
A File Chooser window appears, as described in the File Chooser section, allowing to browse in
the Directory list to the directory in which the new project subdirectory will be automatically
created (in the example of FIGURE 2.5 the directory /home was selected). Give a new project
name in the File list, for example "project.iec" and click on OK to create the new project.
When starting a new project a new directory is then automatically created with the chosen name
(1). All the files related to the project are stored in this new directory. The most important of them
is the project file with the extension ".iec" (2), which contains all the project settings. Inside the
project directory FINE™/Open with OpenLabs™ creates automatically a subdirectory "_mesh"
(3). As all the computations of the project must have the same mesh it is advised to store the mesh
in this specially dedicated directory. Finally, each time the user creates and saves a new
computation, a subdirectory is added (4). The output files generated by the flow solver will be
written in the subdirectory of the corresponding running computation.
FIGURE 2.5
Directories managed through FINE™/Open with OpenLabs™
Once the new project name is defined, two possibilities are available:
l If you have chosen to create a grid file (Creating a mesh), HEXPRESS™ is launched. You
can then create the mesh and save it in the "_mesh" subdirectory of the new project. Click on
Close icon to return to the FINE™/Open with OpenLabs™ project. The new mesh is
automatically associated to the project. The mesh is assumed to be in meters. If a different
mesh scaling is required, the Mesh/Properties... menu (refer to Mesh Properties section)
should be used to define a new scaling factor.
l If you have chosen to open a grid file (Importing a mesh), another File Chooser appears,
which allows to browse to the grid file with extension ".igg". Select the grid file and press OK
to accept the selected mesh. The geometry is then automatically loaded in the Graphics Area of
the interface. The mesh is assumed to be in meters. If a different mesh scaling is required, the
Mesh/Properties... menu (refer to Mesh Properties section) should be used to define a new
scaling factor
Open Project
There are three ways to open an existing project file:
Using the Project/New menu item
1. Click on Project/New.
2. Click on Open an existing project.
3. Choose one of the projects in the unfrozen list and double-click on the project, or, if your
project is not in the list, double-click on the More files... line:
l A File Chooser window appears.
l Browse through the directory structure to find the project file to open. This file has
normally the ".iec" extension. If this is not the case, the file filter in the input box named
List Files of Type, has to be modified.
l Select the project file.
l Click on the file.
l Click on OK.
The opened project becomes the active project. All subsequent actions will be applied to this
project.
Using the Project/Open menu item
1. Click on Project/Open.
2. A File Chooser window appears.
3. Browse through the directory structure to find the project file to open. This file has normally
the ".iec" extension. If this is not the case, the file filter in the input box named List Files of
Type, has to be modified.
4. Select the project file.
5. Click on the file name.
6. Click on OK.
The opened project becomes the active project. All subsequent actions will be applied to this
project.
Selecting the project from the list of files in the Project Menu
The Project menu lists the names of the five most recent projects that have already been opened.
Click on a project name from this menu to open the corresponding project.
FINE™/Open with OpenLabs™ will check the write permission of the project directory and of
the project files and will issue a warning if the project and/or directory are read only. In both cases
the project can be modified, but the changes will not be saved.
Only one project can be active. Opening a second project will save and close the first one.
An attempt to open a project that no longer existing will remove its name from the list in the Project
menu.
Save Project
The Project/Save menu stores the project file (with extension ".iec") on disk. The project file is
automatically saved when the flow solver is started, when FINE™/Open with OpenLabs™ is
closed, or when another project is opened.
Duplicate Project
The Project/Duplicate menu is used to store the active project on disk under different name. A
File Chooser opens to specify the new directory and name of the project. A confirmation dialog
box appears, which contains a checkbox to enable/disable the copying of the associated results
files. Clicking on Dismiss will cancel the operation.
Create Run Files
The Project/Save selected 'Run' Files menu is used to store all the information needed for the
flow solver to run the active computation. This menu is mainly useful when the Task Manager is
used .
If more than one computation is selected in the Active Computations list, then all parameters defined
in the Project Parameters area will be assigned to all selected computations (highlighted in blue).
This may be dangerous if the parameters for the currently opened information page are not the same
for all the selected computations. To avoid this, it is recommended to select only one computation at a
time.
The ".run" file is automatically updated (or created if not existing) when starting a computation
through the main menu (Solver/Start or click on
).
Script
Actions executed by the user through the FINE™/Open GUI are recorded in a Python-like script
giving added flexibility for automation of project settings. The template is a python script that will
allow to set-up (i.e. change the default value of the expert parameters, select a predefined fluid,
etc) an initialized project well linked to a mesh.
The Project/Script.../Edit... menu opens a dialog box displaying all the commands performed by
the user since the beginning of its session. The user can easily edit this script (add, remove and
modify commands). The dialog box contains two pull-down menus. The File menu allows to
open a script in a separate dialog box and to save it in a file. The Run menu allows to run the
script shown in the window under the current session ("Rerun on top").
The Project/Script.../Save All... menu is used to save the dynamic recording of all commands
performed by the user since the beginning of its session.
The Project/Script.../Execute... menu is used to run a python script
file containing
FINE™/Open with OpenLabs™ commands. A file chooser is opened to select a file with a ".py"
extension. Upon selection of a valid file, the script is executed in the current session. Depending
on the content of the script, operations will be added to the current project or a new project will be
automatically opened before operations are performed (the previous project is closed). If the script
being run contains a syntactical error it will be aborted and a message will appear in the shell.
The Project/Script.../Re-execute Last menu can be used to rerun the last script that was run
using the Project/Script.../Execute... command. This option is useful when writing own scripts
manually to rapidly test it on the fly.
The Project/Script.../Templates… menu opens a dialog box to add, select, remove and execute
predefined templates. The template is a python script that should respect the format illustrated in
Configuration and Resource Files Used by the FINE™/Open GUI.
The dialog box is divided into two areas: the list of templates on the left and the description of the
selected template on the right.
The lists of templates under respectively the "Templates" and the "My Templates" sections are
updated depending on the templates provided in the software package under the NUMECA_
DIRECTORY/_ python/_ fine/_ hexa/Templates subfolder or stored by the user into its local
subdirectory .numeca/products/Open/My Templates/. The template name that is displayed in the
dialog box is the name of the associated file on the disk (without '.py' extension).
If the file is located into a subfolder in the "Templates" or the "My Templates" subdirectories, this
folder is displayed in the tree allowing to group some templates in the same folder for better
visibility.
When a template is selected in the tree, the associated python script is loaded, and the information
is updated in the right area of the dialog box.
When clicking on the Ok button, the selected template is executed. A message in the bottom of
the GUI informs the user about the status of the execution. If the execution is successful, the
message "Template executed successfully" appears otherwise; an error message is popped up:
l "no mesh is linked to the project" if the project is not well initialized;
l "an error occurred during the template execution" if the script execution failed;
l "the selected template is not implemented" if the "apply(self)" method of the template is not
implemented.
Once a template is executed, its name is stored in the tree under the "Recently Used" section.
Only the five last executed scripts are kept.
When clicking on the Cancel button, the dialog box is closed without applying a template.
When right-clicking on the tree, a pop-up menu allows depending on the selected item:
l Add template… to add a user-defined template selected in the file browser into the tree under
the "My Templates" section.
If another template with the same name already exists, it will be scratched after confirmation.
l Remove selected template… to remove a selected user-defined template from the tree under
the "My Templates" section.
l Clear recent templates to clear the list of templates into the "Recently Used" section.
Preferences
The Project/Preferences menu is used to:
l Select the calculation accuracy for the FINE™/Open solver
l Select the default MPI library to be used for parallel computations launched from the
FINE™/Open GUI
Mixed and double precision modes of the FINE™/Open solver are available. For most cases, the
mixed precision solver (much less demanding in memory consumption) will be sufficiently
accurate and should be considered as the default option. However, some certain types of
problems, such as very long thin pipe and conjugate heat transfer problems, may benefit from
double precision solver.
The choice of the MPI library for parallel computations is also accessible. On Windows, the user
may choose between MPICH2 and IntelMPI; on Linux, OpenMPI and IntelMPI are available.
More details about the MPI library can be found in the "MPI system " (p. 371) page. The MPI
choice selected in the "Project preferences" menu acts only as default. This allows to overwrite
the default proposed by NUMECA. When you create a new project or a new computation, the
MPI choice proposed by default will be the one selected in the "Project preferences" menu.
Quit
Select the Project/Quit menu item to quit the FINE™/Open with OpenLabs™ integrated
environment. If changes have been made in the active project, the user will be asked if these
changes need to be saved.
Note that this action will NOT stop the running calculations. A Task Manager window will
remain open for each running computation. Closing the Task Manager window(s) will kill the
running calculation(s) after confirmation from the user.
Project Names Limitations
The use of non- standard characters in the project name (other than English letters, Arabic
numerals, and underscore symbol "_") is not recommended because it may cause problems when
opening the project on another computer on which such characters may not be defined or
misunderstood (a back slash for example may be understood as a directory name separator, etc.).
If the name of an already existing project is specified, this project file will be overridden. All other
files and subdirectories will remain the same as before.
2.2.2 Mesh Menu
Link a mesh file
When creating a new project, a grid file is automatically assigned. However, if the user wishes to
change the assigned grid file, he should click on Mesh/Link a mesh file menu. A File Chooser
appears, which allows the user to browse to a grid file with extension ".igg". Select the grid file
and press OK to accept
the selected mesh. The mesh units may be changed using the
Mesh/Properties... menu, see Mesh Properties section and click OK to accept.
If a new mesh is linked to the project, the partitions that are present in the computation directory
should be removed. Otherwise, the old mesh will be used if the number of processors is the same.
Load Mesh
By default, when a grid file is assigned to a project, the associated geometry is automatically
shown in the graphics area of the FINE™/Open with OpenLabs™ main window, but not the
mesh. The Mesh/Load Mesh command allows the user to load (and therefore visualize) the mesh
in the graphics area of the FINE™/Open with OpenLabs™ window.
Notice that when large meshes are loaded, motion and zooming tasks in the graphics area may be
slowed down, due to the large amount of memory used by the mesh.
Unload Mesh
The Mesh/Unload Mesh command unloads the mesh and clears it from the memory of the
computer. However, the geometry of the computational domain remains visible in the graphics
area. By default, only solid surfaces are shown (shading).
Properties
Clicking on Mesh/Properties... opens a dialog box that displays global information about the
mesh:
l Mesh file: name and location of the mesh file.
l Grid units: allows the user to impose the units of the mesh.
l Mesh properties: the total number of cells and vertices per block (domain) are automatically
detected from the mesh.
l Mesh quality: the global mesh quality will be checked and shown.
Agglomeration preview
Clicking on Agglomeration preview opens a dialog box that allows the user to preview the
agglomeration results.
Before previewing the results, the user must apply the agglomeration first. Select the option
Agglomerate and specify the number of the levels, then click on the button Apply to agglomerate
the mesh. By default, the maximum number of levels is proposed.
After applying the agglomeration, the Display frame becomes accessible. Specify the Display
level number and then click on the button Apply, the cell in the specified level will be displayed
in the view region. The Options allow to select the display mode. By default, the shaded surface
mesh is displayed. The user may change to wireframe, hidden line or volume cell with/without
shaded.
The information frame shows the number of cells in each grid level.
2.2.3
Solver Menu
This menu gives access to the FINE™/Open solver, a powerful 3D unstructured code dedicated
to Navier- Stokes or Euler computations. The FINE™/Open solver uses the computational
parameters and boundary conditions set through FINE™/Open with OpenLabs™ and can be
fully controlled both from the FINE™/Open Solver Menu and from the Task Manager.
In this section, information is given on how to start, stop, interrupt and restart the flow solver. All
these actions may be performed by using the pull down menu appearing when the button Solver
of the Menu bar is clicked.
Start Solver
To start the flow solver, select the menu item Solver/Start.
It is not recommended to start the flow solver before setting the physical boundary conditions and the
computational parameters.
When launching any computation, the result files produced by a previous calculations on that
computation will be overwritten with the new result values. It also implies that the initial solution
will be created from the values set in the Initial Solutionpage within FINE™/Open with OpenLabs™
(more details in Initial Solution chapter).
If "Parallel" has been chosen in " Launching Mode " (p. 400) page, the user can access the MPI
library choice in "Parallel settings ..." , available after pressing the button "Start".
Stop Solver
There are two different ways to stop the flow solver:
l Solver/Save and Stop interrupts the flow computation after the next iteration. This means that
the flow solver stops the computation at the end of the next iteration and outputs the current
state of the solution exactly as if the computation was finished. This operation may take some
time.
l Solver/Kill allows the user to immediately stop the computation for the active project. In this
case no output is created when stopping and the only solution available is the last output saved
during the run. This may be a dangerous choice if requested during output of the solution. The
output is then corrupted and all the computation time is lost. To avoid this, it is better to use
Solver/Save and Stop or to kill the computation some iterations after the writing operations.
Restart Solver
To restart a computation from an existing solution:
l in the Initial Solution page, an initial solution file should be specified. See Initial Solution
chapter for more details on the available ways to define an initial solution.
l the solver should be started using the Solver/Start menu,
Save Batch File
The Solver/Save batch file menu allows the user save all necessary files to start a computation in
batch mode.
2.2.4
Plugins Menu
The purpose of this menu is to provide to users an access to predefined module provided by
NUMECA within FINE™/Open with OpenLabs™.
The Plugins/TurboWizard... menu gives access to the TurboWizard module, an embedded
wizard capable of guiding the user through the entire setup of a turbocharger or centrifugal
compressor project.
The TurboWizard module, from a structured blade row (s) mesh file from AutoGrid5™ and a
domain file from HEXPRESS™ (or ".stl" file(s)), manages the import of the geometry, converts
the structured AutoGrid5™ mesh, generates the volute's mesh and sets up the steady computation.
More information about this embedded python module can be found in the "Turbowizard
module" (p. 38) section.
The user can also access the TurboWizard module when starting FINE™/Open with OpenLabs™, in
the Project Selection window.
A. Turbowizard module
The TurboWizard module is an embedded python wizard dedicated to guide the user through the
entire setup of a turbocharger or centrifugal compressor project. The TurboWizard, from a
structured blade row(s) mesh file from AutoGrid5™ and a domain file from HEXPRESS™ (or
".stl" file(s)), manages the import of the geometry, converts the structured AutoGrid5™ mesh,
generates the volute's mesh and sets up the steady computation.
The module can be reached in the Plugins menu of FINE™/Open with OpenLabs™, or when
starting a new project, through the Project Selection window.
The TurboWizard module has the following general limitations:
l Dedicated only to turbochargers and centrifugal compressors, not for axial turbomachines.
l The bladed channel(s) and the volute domain (or ".stl") file(s) should have the same units.
l Only the main inlet and outlet are configured. The user must setup all the secondary inlets or
outlets.
l Creates new RANS steady computation without modifying existing computations in the project.
The TurboWizard module consists of the following steps:
1. The project management where the user can create a new FINE™/Open with OpenLabs™
project or load an existing one and select the geometry units.
2. The computation settings where the user can fill in the information needed (inlet conditions,
turbomachinery configuration and fluid/flow modeling details) for the mesh generation and the
project settings.
3. The blade rows mesh import where the user can import the impeller (or impeller + diffuser)
structured mesh file from AutoGrid5™.
4. The volute definition where the user can import the volute's domain (or ".stl") file and request
the automatic cleaning of the geometry.
5. The mesh generation dedicated to the volute's mesh generation in HEXPRESS™, the merging
of the structured and unstructured meshes and finally the setup of a ready-to-run new steady
RANS computation in FINE™/Open with Openlabs™ based on the user inputs to the
previous steps and recommended settings.
Turbowizard Step 1: project management
The first step of the TurboWizard module is the project management: an existing project can be
loaded or a new one can be created.
When a new project is created (e.g. "myproject.iec"), a folder named "myproject" is generated
including the FINE™/Open with OpenLabs™ ".iec" file, a subfolder named "_mesh" (which
will contain the necessary grid files with extensions ".igg", ".dom", ".bcs", ".hex" and ".fnmb"
with relevant information about the mesh to be generated by the wizard, as well as the grid report
and the wall distance data) and finally the "TurboWiz.conf" configuration file (which stores the
data entered by the user throughout the steps of the wizard).
The configuration file "TurboWiz.conf" stores the data entered by the user throughout the steps of
the wizard:
l the path to the AutoGrid5™ structured mesh;
l the path to the volute geometry (the ".dom" file or the folder containing ".stl" files);
l the total pressure and temperature value at inlet;
l the fluid model name, e.g. AIR(Perfect), OXYGEN(Perfect);
l the massflow rate value;
l the rotational speed value of the impeller blade row;
l the turbulence length and intensity (in percentage) at inlet;
l the turbulence model name from interface, e.g. Spalart-Allmaras, SARC, k-epsilon (Extended
Wall Function);
l the maximum radius of rotating parts;
l the target pressure ratio value;
l the desired mesh coarsening for the volute (1 for coarse, 2 for medium, 3 for fine);
l the length units (1 for meters, 2 for millimeters, 3 for inches).
All modifications applied in the TurboWizard module are automatically recorded in the
configuration file.
The "TurboWiz.conf" configuration file can also be used as input file to run the TurboWizard module
in batch mode.
The Geometry Units option allows the selection of the project length units (meters, millimeters or
inches).
Both structured and unstructured meshes used in the project must have the same units.
The Cancel button stops the TurboWizard module without saving.
The Next >> button allows to go to the second step of the TurboWizard module. The button is
not active when no project file is selected.
Turbowizard Step 2: computation settings
The second step of the TurboWizard module allows the user to define the inputs used in the
volute mesh generation as well as used in the steady RANS computation setup in FINE™/Open
with OpenLabs™.
The Cancel button stops the TurboWizard module without saving the input data of the current
step.
The << Back button allows to go back to the first step of the TurboWizard module. Pressing the
Next >> button to go from step 1 to step 2 again shows the last input values of this step.
The Next >> button allows to go to the third step of the TurboWizard module.
Inlet Conditions
The Inlet Conditions section is used to impose the boundary conditions at inlet:
l the total pressure, in [Pa];
l the total temperature, in [K];
l the turbulence intensity, in [%];
l the turbulence length intensity, in [m].
Turbomachinery configuration
The Turbomachinery Configuration section is used to impose general settings of the
turbomachine:
l the mass flow rate, in [kg/s];
l the rotational speed of the impeller, in [rpm];
l the rotating wheel maximum radius, in [m];
l the estimated pressure ratio.
A positive value for the rotation speed indicates a rotation in positive θ-direction with θ positive
according to a right handed coordinate system.
The rotating wheel maximum radius is used to define the portion of the impeller (i.e. hub and
blade patches) which is rotating. If the input value is higher than the geometric value (e.g. 1000
m), it is considered that the whole hub and blade patches rotate.
Fluid & Flow Modeling
The Fluid & Flow Modeling section is used to impose the fluid and turbulence flow models:
for the fluid model
l AIR(Perfect);
l CARBON_DIOXIDE(Perfect);
l NITROGEN(Perfect) or OXYGEN(Perfect).
for the turbulence model
l Spalart-Allmaras;
l Spalart-Allmaras (Extended Wall Function);
l SARC;
l SARC (Extended Wall Function);
l k-epsilon (Extended Wall Function);
l k-epsilon (Low Re Yang-Shih, classic);
l k-omega (M-SST);
l k-omega (M-SST Extended Wall Function);
l S-BSL-EARSM ;
l S-BSL-EARSM (Extended Wall Function).
Turbowizard step 3: blade rows mesh import
The third step of the TurboWizard module allows the user to import the mesh of the bladed
channel(s). The imported mesh must be structured, generated within AutoGrid5™ and respect
one of the following configuration:
l an impeller from one to full periodicity meshed passages without diffuser or,
l an impeller from one to full periodicity meshed passages with a diffuser with full wheel
meshed passages.
Pressing the button
bladed channel(s).
allows the selection of the AutoGrid5™ structured mesh file of the
The limitations regarding the imported structured AutoGrid5™ mesh are:
l A minimum of two grid levels is mandatory;
l ZR technological effects are supported if they are not connected to a rotor/stator interface or to
the interface with the volute;
l 3D technological effects are not supported (e.g. cooling holes);
l Patches with inlet boundary condition (“INL") patches must be defined.
l Patches defined with outlet boundary condition ("OUT") are considered to belong to the interface
with the volute and must belong to the same row.
Once the structured file (e.g. "impeller.igg") is imported, the AutoGrid5 Mesh Report section
shows the number of cells of the imported structured mesh. In addition, information about the
periodicity, the number of meshed passages and the mean first cell size are displayed in the
Interface With Volute - Upstream Side section.
Once the structured mesh file is imported, a set of files is saved in the "_mesh" folder (created at the
step 1 of the TurboWizard). Those files contain the bladed channel(s) geometry, the grid related to the
project and the definition of the boundary conditions types.
The Cancel button stops the TurboWizard module without saving the input data of the current
step.
The << Back button allows to go back to the second step of the TurboWizard module. Pressing
the Next >> button to go from step 2 to step 3 again shows the last imported mesh file and its
properties.
The Next >> button allows to go to the fourth step of the TurboWizard module.
turbowizard step 4: volute definition
The fourth step of the TurboWizard module allows the user to import the volute geometry. Two
options are available:
l Import a domain file from HEXPRESS™ (Import HEXPRESS Domain);
l Import one or multiple ".stl" file(s) (Import STL File(s)).
The following conditions must be respected at
meshes:
the interface between the structured/unstructured
l The relative difference in interface area between the meshes must be less than 1%.
[(Interface area, structured side) - (Interface area, unstructured side)]/(Interface area, unstructured
side) < 1%
l The position along z between the hub for the structured and the unstructured part must be less
than half the first cell width at the wall.
l The position along z between the shroud for the structured and the unstructured part must be less
than half the first cell width at the wall.
For both options, the TurboWizard module allows the cleaning of the geometry through the
Clean Geometry check box. The activation of this check box allows the wizard to try to merge
adjacent faces in the volute geometry if they have edges connected with an angle of less than 20
degrees. In addition, the adjacent faces are only modified if they are not forming a sharp angle of
less than 40 degrees.
When selecting the Import HEXPRESS Domain option, the Read Volute Domain File button
allows to import a domain file from HEXPRESS™. The info icon
opens an information
window presenting the required boundary conditions to be set on different patches of the domain
file:
l An outlet boundary condition ("OUT") must be set.
l There must be at least two patches defined with "UND" boundary condition. These patches
are used as the structured/ unstructured interface.
l All the other patches must be defined with solid ("SOL") boundary condition.
The file with extension “.bcs” must be in the same directory as the volute ".dom" one. Note that this
".bcs" file is automatically generated if the domain is saved within an HEXPRESS™ project.
When selecting the Import STL File(s) option, new buttons allows to import one or multiple
".stl" file(s). These buttons give the user the possibility to add a single file (using the Add File
button) or whole folder (using the Add Folder button). Removing imported files is possible
through the Remove button). If the user loads more than one ".stl" file, the wizard will assemble
together the files and generate a domain once clicking on the Generate Domain button.
Note that the wizard does not have stitching capabilities, therefore, the ".stl" files are considered as
perfectly matching and with a clean triangulation.
Once the volute's domain file is imported, a set of files is saved in the "_mesh" folder (created at the step 1
of the TurboWizard). Those files contain the representation of the volute geometry and the definition of the
boundary conditions types. The unstructured mesh file selected has its name displayed in the step 4 window
(e.g. "volute_HEX.igg").
The Cancel button stops the TurboWizard module without saving the input data of the current
step.
The << Back button allows to go back to the third step of the TurboWizard module. Pressing the
Next >> button to go from step 3 to step 4 again shows the last imported volute's file(s).
The Next >> button allows to go to the fifth step of the TurboWizard module.
turbowizard step 5: mesh generation & COMPUTATION SETUP
The fifth and last step of the TurboWizard module is dedicated to the generation of the volute's
mesh, the merging of the structured and unstructured meshes and the automatic setup of a new
computation in FINE™/Open with OpenLabs™.
The TurboWizard module gives three options of coarsening for the volute mesh refinement level:
coarse, medium or fine. According to the selected level, the volute mesh settings to be used in the
HEXPRESS™ is displayed, including information about the Cartesian cell size, the sharpest
corner angle, the rotor-stator cell size in the radial direction and the first cell size at rotor-stator
interface.
Once one of the mesh refinement levels is selected and clicking on the Generate HEXPRESS
Mesh button, the generation of the volute's mesh in HEXPRESS™ is starting. The inputs of the
mesh generation relies on the data coming from the TurboWizard previous steps, as well as built-
in experience based setup formulations:
Initial mesh
This step is based on the Cartesian Cell Size value. This value is defined based on the spanwise
number of cells at the outlet of the structured mesh. Using the bounding box function of
HEXPRESS™, the span of the outlet is measured through its z-axis edge. This value is then used
to determine the initial cell size of the volute by dividing it by a number that depends on the mesh
refinement level selected as function of the number of points spanwise for the impeller. Then, the
number of cells in the z-direction for the volute is simply the height of the global bounding box
divided by the initial cell size.
Adapt to geometry
This step in HEXPRESS™ refines the initial Cartesian mesh. The wizard checks each corner and
additional refinements (e.g. a cube around the corner) are applied in case the angle is less than 20
degrees. In addition, The curvature criterion refinements is always activated and the alignment of
edges to the Cartesian axis is checked in order to put anisotropic refinements. The interface has a
target cell size calculated based on the bounding box at the impeller outlet and the number of cell
in the z-direction of this patch. The target cell size for each other surface is chosen according to
the formula below:
where
is set to 3, 5 and 7 for the coarse, medium and fine meshes, respectively and
is the surface area. Finally, the maximum number of refinement is set as 20, expressed in the
form of global number of refinement. The wizard computes automatically a level of refinement
related to the geometrical features of the geometry. If this number is below 20, the user will see
that the refinements are activated and set to 20, if the computed number is more than 20, the user
interface will show 1000.
Snap to geometry & Optimize
The wizard sets snapping and optimization as enabled. The default settings of HEXPRESS™ are
kept.
Viscous layers insertion
The wizard inserts viscous layers on all solid surfaces. The first layer thickness value is defined as
the First Cell Size at RS value obtained from the AutoGrid5™ mesh. In addition, the stretching
ratio is the same for all solid surface and takes the value of 1.35, 1.25 and 1.1 for the coarse,
medium and fine meshes, respectively.
After generation of the volute mesh, the Volute Mesh Report section displays the main mesh
statistics of the volute grid: number of cells, orthogonality, aspect ratio and expansion ratio.
When the volute mesh is generated, the TurboWizard module gives flexibility to the user to
modify the mesh settings and regenerate the volute mesh (Switch to HEXPRESS button) or to
directly merge the generated mesh with the imported structured AutoGrid5™ mesh (Merge
Meshes button).
Switch to HEXPRESS
The Switch to HEXPRESS button allows the user to check, modify and customize the volute's
mesh directly in HEXPRESS™. When pressed, the wizard opens the mesh of the volute in
HEXPRESS™ and gives the user access to each of the five steps mentioned above, as illustrated
below.
Once the modifications are done and the mesh regenerated, the project must to be saved either
in the main toolbar of
through the menu Project / Save or through the shortcut icon
HEXPRESS™. Finally, the TurboWizard module can be resumed by clicking on the Resume
button on the TurboWizard dialog box.
The window corresponding to the first step of the TurboWizard is brought to front. The Next >>
button can be used to reach step 5 again.
Note that the TurboWizard module can take some seconds until the unstructured mesh is loaded and
the Volute Mesh Report is shown.
The Merge Meshes button can be clicked in order to merge the structured grid imported from
AutoGrid5™ and the unstructured volute mesh generated by HEXPRESS™. Once completed, a
Global Mesh quality section is displayed in the step 5 windows, displaying the total number of
cells of the full mesh, orthogonality, aspect ratio and expansion ratio statistics.
The Cancel button stops the TurboWizard module saving the last task of the current step.
The << Back button allows to go back to the fourth step of the TurboWizard module.
Clicking on the Finish button finalizes the TurboWizard module by transferring data to
FINE™/Open with OpenLabs™ (as shown in the dialog box below).
If applicable, additional dialog boxes are shown with recommended calculation adjustments and
mesh statistics to be improved, including warnings about the maximum expansion ratio, the
minimum skewness and the presence of twisted, concave or negative cells for example.
Pressing OK for the possible warnings, brings the user to FINE™/Open with OpenLabs™. The
Mesh Properties dialog box is shown, presenting information about the mesh file, grid units and
mesh properties.
Once Ok is clicked, a new computation setup named "design_ point_ 1" is available within
FINE™/Open with OpenLabs™.
The wizard does not overwrite or delete pre-existing computation(s).
The user has the flexibility to check and modify the project parameters before starting the solver if
necessary. The settings of the Project Parameters list are directly linked to the user inputs during
the five steps of the TurboWizard module. A summary of these settings is given below.
Physical configuration
l General Properties: the computation created by the wizard is steady, and the bladed channel
(s) as well as the volute are set as fluid blocks.
l Fluid Model : volute and bladed channel (s) are defined with the fluid selected in the
TurboWizard module's step 2, e.g AIR(Perfect).
l Flow Model: by default, the wizard takes turbulence into account and selects Turbulent
Navier Stokes as mathematical flow model. The turbulence model selection from step 2 of the
wizard is adopted (e.g. Spalart-Allmaras, S-BSL-EARSM, ...) and Reference length is set as
is
the Turbulence Length Scale input. In the equation below, the Reference velocity
estimated using the Mass Flow Rate
pressure
and total temperature
and total quantities from the Inlet Conditions (total
, is
) also specified in step 2. The impeller inlet area
automatically measured by the wizard from the AutoGrid5™ mesh. Both volute and blade
channel(s) have the settings.
l Rotating Machinery: the wizard sets the Rotation speed of the impeller based on the input of
step 2 and unselects the Rotating check box for the volute and the diffuser (if present). In
addition, the Rotor/stator tab presents all the connections detected by the wizard, an adopts
Full non-matching mixing plane treatment for all interfaces.
In HEXPRESS™, the non matching connection between the impeller row and the volute (or
between impeller and diffuser) is set as rotor/stator. If a diffuser is present, a FNMB connection is
adopted in the interface with the volute.
Boundary Conditions
Inlet
inlet flow angle are set
Total quantities with Angle From Axial Direction (V extrapolated) is selected. Tangential and
radial
to zero. Absolute Total Pressure and Absolute Total
Temperature take the values entered by the user in step 2 of the wizard. Depending on the
turbulence model, the Turbulence Viscosity or k and Epsilon are computed. the following table
is the turbulent
summarizes the estimation adopted by the TurboWizard module, where
is the turbulent
viscosity,
is a
specific dissipation ratio,
is the turbulent dissipation ratio,
is the turbulent kinetic energy,
is the reference length and
is the turbulence intensity,
coefficient of the turbulent model.
k-epsilon (Extended
Wall Function)
k-epsilon (Low Re
Yang-Shih, classic)
k-omega (M-SST)
S-BSL-EARSM
k-omega (M-SST
Extended Wall
Function)
S-BSL-EARSM
(Extended Wall
Function)
Spalart-Allmaras
Spalart-Allmaras
(Extended Wall
Function)
SARC
SARC (Extended Wall
Function)
-
-
-
-
-
-
-
-
-
Outlet
The outlet of the volute has a Mass Flow Imposed boundary condition (using the wizard's input
on step 2) and its Initial Pressure is estimated using the following sequence of calculations:
where
,
,
are the impeller inlet static temperature, Mach number and static pressure,
respectively;
and
are the fluid's specific heat and heat capacity ratio, respectively; and
is
the volute outlet static pressure calculated using the pressure ratio estimation
input of step 2.
SOLID
The wizard sets patches as rotating with Area Defined Rotation Speed depending on their name
from AutoGrid5™. In addition, all the solid wall are Adiabatic . For the rotating patches,
Rotation Speed 1 is set as 0 RPM and Rotation Speed 2 takes the input of the wizard's step 2.
The lower and higher radius limits are set to zero and to the Rotating Wheel Maximum Radius
input from step 2, respectively. Finally, for rotating patches, the axial limits are automatically
measured by the TurboWizard module and the option Compute force and torque is activated.
Initial Solution
l If the configuration comprises an impeller + volute with a periodicity higher than one for the
impeller, turbomachinery initialization is used for the structured part of the mesh. The static
) and the inlet pressure is calculate from
pressure at the interface is the same as the outlet (
the isentropic relation, as shown in the equation above. For other configurations, constant
values are used for both the structured mesh, with Relative velocity = 0 m/s, static temperature
and static pressure equal to the values computed at the inlet.
l Regardless of the bladed channel's configuration, the volute takes Constant values for its
initial solution parameters. Constant initial solution with cylindrical coordinate system is used.
is estimated as shown below.
The outlet static temperature
where
is the total outlet temperature,
 is the change in specific enthalpy,
 is the outlet
tangential velocity,
 is the impeller rotating speed (an input from step 2 of the wizard) and
 is the maximum radius of the rotating part. This quantity assumes the value of 90% of the
impeller's maximum radius (measured by the wizard) if the user input to Rotating Wheel
Maximum Radius in step 2 is more than the real value automatically measured. On the other
hand, if the maximum rotating radius given by the user is less than the maximum radius of the
 equals 100% of the value measured by the wizard. Using an auxiliary
impeller, then
velocity
estimation,
 is calculated. Lastly, the radial velocity
 at the volute's outlet is
calculated using the mass flow value and static quantities as shown below.
where
is the surface area of the interface between structured and unstructured meshes.
When a full diffuser is present in the structured mesh, it is recommended to multiply the value of
 given by the wizard by the periodicity of the diffuser.
Numerical Parameters
l General Properties: by default, the wizard activates CPU Booster, multigrid with 4 grid
levels and coarse grid initialization. In the Advanced tab, a linear scheme of sweeps in
successive grid levels is used. The Maximum number of cycles per grid level is set as 30,
with Convergence criteria on each grid level equals -5.
l Numerical Schemes: second order central difference discretization scheme is selected and a
CFL number equals 1000 is applied for both volute and bladed channel(s).
Computation Control
l Outputs: by default, the wizard selects the following quantities as output:
l STATIC_TEMPERATURE
l ABSOLUTE_TOTAL_TEMPERATURE
l STATIC_PRESSURE
l ABSOLUTE_TOTAL_PRESSURE
l DENSITY
l TURBULENT_VISCOSITY
l YPLUS
l SKIN_FRICTION
l VORTICITY_VECTOR
l ABSOLUTE_VELOCITY
l RELATIVE_VELOCITY
l FRICTION_VELOCITY
l ENTROPY
l ABSOLUTE_MACH_NUMBER
l RELATIVE_MACH_NUMBER
l WALL_DISTANCE
l VISCOUS_STRESS
l Control Variables: the Number of iterations is set as 1000, with Convergence criteria set
to -10 and the solution being saved every 100 iterations.
l Launching Mode: by default, the wizard uses serial launching mode.
The computation created by the TurboWizard module can be started by pressing the
button.
2.3
ICON BAR
The icon bar contains twelve buttons that provide a shortcut for menu items in the main menu bar.
File Buttons
The four buttons on the left of the icon bar are shortcuts for items on the Project menu:
The New Project icon is a shortcut for the menu item Project/New.
The Open Project icon is a shortcut for the menu item Project/Open.
The Save Project icon is a shortcut for the menu item Project/Save.
The Save Selected 'Run' Files icon is a shortcut for the menu item Project/Save Selected
'Run' Files.
Solver Buttons
The four central buttons allow the user to start, stop, kill or monitor the active computation:
The Start Flow Solver icon is a shortcut for the menu item Solver/Start.
The Save and stop icon is a shortcut for the menu item Solver/Save and Stop.
The Kill Flow Solver icon is a shortcut for the menu item Solver/Kill.
The Steering icon activates the Convergence History page, which allows the user to follow
the evolution of the active computation.
Module Buttons
The four buttons on the right of the icon bar allow the user to start the pre- and post-processors:
The Start Task Manager icon is used to open the Task Manager software.
The Start HEXPRESS icon is used to open the HEXPRESS™ software.
The Start Monitor icon is used to open the Monitor software.
The Start CFView icon is used to open the CFView™ software.
2.4
COMPUTATIONS
When clicking on the Computations button at the top left of the interface a list of all the
computations of the project is appearing. The active computation is highlighted in blue and the
corresponding parameters are presented in the Project Parameters area (more details in Project
Parameters section). All the project parameters of the computation can be controlled separately by
selecting (from this list) the computation on which all the user modifications are applied.
With the buttons New , Clean , Rename and Delete , computations can be created, cleaned,
renamed or removed. When clicking on New the active computation is copied and the new
computation has the same name as the original with the prefix "new_" as shown in the example
below. In this example "computation_2" is the active computation. When clicking on the New
button, a new computation called "new_computation_2" is created and is presenting the same
project parameters as "computation_2".
FIGURE 2.6
Computations area
The Clean button allows after confirmation to remove the resulting files and to clear the steering
files of the non-running selected computation(s) and sub-computation(s) (if non-deterministic).
For non-deterministic computation when the main computation is selected, in the confirmation
dialog box the Clean non-deterministic results option allows to clean the main computation and
the corresponding sub-computations as well.
FIGURE 2.7
Cleaning confirmation when non-deterministic main computation
For the selected non-running computation (s) or sub-computation (s), the remaining files after
cleaning will be the ".bat" (".batch"), ".run", ".steering", ".steering.binary" and ".ANSYSgeom"
if existing. An information is displayed at the bottom of the graphics area after the cleaning
process and a warning is appearing when some selected computations or sub-computations are
running.
FIGURE 2.8
Warning when cleaning running computation(s) or sub-computation(s)
When cleaning a computation running in batch, as the GUI cannot detect
corresponding files will be removed and cleared.
if it
is running, the
The Rename button allows to rename the active computation after typing a new name and
pressing <Enter>.
The buttons
computations.
allow to move up or down the selected computation (s) in the list of
The reordering cannot be applied on non-deterministic sub-computations.
When right-clicking on an active computation, a pop-up menu is appearing that is giving access to
the New, Clean, Rename and Delete commands.
2.5
PROJECT PARAMETERS
The Project Parameters is the second button on the left of the interface, below the Active
Computations button. When clicking on this button a directory structure appears allowing the user
to go through the available pages of the project definition. The Parameters window (FIGURE
2.2) shows the parameters corresponding to the selected page in the Project Parameters list. To
see the pages available in a directory double-click on the name or click on the
the name.
sign in front of
FIGURE 2.9
Project Parameters area
The graphics area always remains visible, and pages of the Project Parameters list are accessed
through pop-up windows. Two pages cannot be accessed at the same time.
2.6
VIEW
The View subpanel (FIGURE 2.10) controls viewing operations on the geometry and the grid.
FIGURE 2.10
View subpanel
This last subpanel is divided into two rows of buttons:
l The three first buttons on the first row allow to set the selection.
l The three last buttons on the first row allow to modify the way of displaying surfaces in the
graphics area.
l The second row allows to start the distance tool which computes the distance between two
points selected on the screen.
Selection Mode
The button (
) allows the face mode viewing. All the viewing modification are applied on the
currently selected face. The face may be selected interactively by left-clicking on the face into the
graphics area or by right-clicking on the face icon (
(Face Viewer) listing all the faces available.
). This last operation opens a dialog box
The button (
) allows the block mode viewing. All the viewing modification are applied on the
currently selected block (domain). The block may be selected interactively by left-clicking on the
block into the graphics area.
The button (
) allows to apply the viewing modifications on all the blocks
Viewing Mode
The button (
) allows the user to display the faces as wireframe. When clicking on the button
( ), the user can choose to display the wireframe as the triangulation from the geometry surfaces (
) or the mesh faces (
).
The button (
) allows to toggle on/ off the shading of the faces.
Distance Tool
) is useful to measure the distance between two points or between a point
The distance tool (
and a line. The following dialog box will appear, showing the distances computed along principal
directions between the two points:
The following prompt appears, asking to enter the first point:
Enter first point (toggle selection: a = points, c = curves, s = surfaces, l =distance to line)
Once the first point (or line) is entered, a second prompt appears, asking to enter the second point:
Enter second point (toggle selection: a = points, c = curves, s = surfaces, l =distance to line)
To measure the distance between two points, simply select the points with the mouse or enter the
coordinates with the keyboard. For example, to measure the distance between (0,0,0) and (1,1,1),
enter the sequence '0 0 0' in the graphics area, followed by <Enter>. Then enter '1 1 1' followed
by <Enter>. The distance is indicated in the graphics area and in the information area.
To select an existing point, attraction features are available, allowing attraction to points, curves
and surfaces. To activate the attraction to points, press <a> in the graphics area, then move the
cursor to the desired point. Similarly, to activate the attraction to curves or surfaces, press
respectively <c> or 
, then move the cursor to the desired curve or surface. The attraction
works on:
l end points of the curves,
l visible Cartesian points,
l visible curves,
l visible surfaces,
l block vertices and fixed points.
In this last case, the attraction cannot be deactivated. When there is attraction, the corresponding
point is highlighted. Simply press the left mouse button to select it.
To measure the distance between a point and a line, press <l> in the graphics area. Then enter a
line origin (with the mouse or the keyboard) and direction (this one must be entered with the
keyboard). The attraction features are also available for the line origin.
Enter line origin (toggle selection: a = points, c = curves, s = surfaces)
Enter line direction (keyboard only)
>> 1 1 1
This option can be activated before or after having entered the first point. The distance is
measured perpendicularly to the line.
Once a distance is calculated, another distance can be measured by selecting other points.
To quit this tool, press <q> or the right mouse button or close the Distance tool window.
2.7 MESH INFORMATION
When a mesh is assigned to the project, the mesh information area is shown at the bottom on the
left of the interface. It contains the following information:
FIGURE 2.11
Mesh information area
l Number of cells.
l Number of vertices.
2.8
PROJECT PARAMETERS WINDOWS
The Parameters windows are pop-up windows containing the parameters related to the selected
item of the Project Parameters list. The graphics area always remains visible. Two pages cannot
be accessed at the same time.
2.9 GRAPHICS AREA
The graphics area shows the geometry of the mesh assigned to the active project. When the mesh
is loaded, the surface mesh on solid surfaces is also shown. The graphics area always remain
visible. The grid icons can be used to change the visualization of the mesh. These are described
below and in View section.
FIGURE 2.12
Resizing of Graphics Area
2.10 VIEWING BUTTONS
The Viewing buttons are used to perform viewing manipulations on the active view, such as
scrolling, zooming and rotating. The manipulations use the left, middle and right buttons of the
mouse in different ways. The sub-sections below describe the functions associated with each
mouse button for each viewing button.
For systems that only accept a mouse with two buttons, the middle mouse button can be emulated for
viewing options by holding the <Ctrl> key with the left mouse button.
X, Y, and Z Projection Buttons
These buttons allow to view the graphics objects on X, Y or Z projection plane. Press the left
mouse button to project the view on an X, Y or Z constant plane. If the same button is pressed
more than one time, the horizontal axis sense changes at each press.
Coordinate Axes
The coordinate axes button acts as a toggle to display different types of coordinate axes on the
active view using the following mouse buttons:
l Left: press to turn on/off the display of symbolic coordinate axis at the lower right corner of the
view.
l Middle: press to turn on/off the display of scaled coordinate axis for the active view. The axis
surrounds all objects in the view and may not be visible when the view is zoomed in.
Scrolling
This button is used to translate the contents of active view within the plane of graphics window in
the direction specified by the user. Following functions can be performed with the mouse buttons:
l Left: press and drag the left mouse button to indicate the translation direction. The translation is
proportional to the mouse displacement. Release the button when finished. The translation
magnitude is automatically calculated by measuring the distance between the initial clicked
point and the current position of the cursor.
l Middle: press and drag the middle mouse button to indicate the translation direction. The
translation is continuous in the indicated direction. Release the button when finished. The
translation speed is automatically calculated by measuring the distance between the initial
clicked point and the current position of the cursor.
3D Viewing Button
This button allows the user to perform viewing operations directly in the graphics area. Available
operations are 3D rotation, scrolling and zooming.
After having selected the option, move the mouse to the active view, then:
l Press and drag the left mouse button to perform a 3D rotation
l Press and drag the middle mouse button to perform a translation
l Press and drag the middle mouse button, while holding the <Shift> key, to perform a zoom
l To select the centre of rotation, hold the <Shift> key and press the left mouse button on a
geometry curve, a vertex or a surface (even if visualized with a wireframe model). The centre
of rotation is always located in the centre of the screen. So, when changed, the model is moved
according to its new value.
This 3D viewing tool is also accessible with the <F1> key.
Rotate About X, Y or Z Axis
The rotation buttons are used to rotate graphical objects on the active view around the X, Y or Z
axis. The rotations are always performed around the centre of the active view. Following
functions can be performed with the mouse buttons:
l Left: press and drag the left mouse button to the left or to the right. A clockwise or counter
clockwise rotation will be performed, proportional to the mouse displacement. Release the
button when finished.
l Middle: press and drag the middle mouse button to the left or to the right. A continuous
rotation will be performed, clockwise or counter-clockwise. Release the button when finished.
Zoom In/Out
This button is used for zooming operations on the active view. Zooming is always performed
around the centre of the view. Following functions can be performed with the mouse buttons:
l Left: press and drag the left mouse button to the left or to the right. A zoom in - zoom out will
be performed, proportional to the mouse displacement. Release the button when finished.
l Middle: press and drag the middle mouse button to the left or to the right. A continuous zoom
in - zoom out will be performed. Release the button when finished.
Region Zoom
This button allows to specify a rectangular area of the active view that will be fitted to the view
dimensions. After having selected the button:
1. Move the mouse to the active view.
2. Press and drag the left mouse button to select the rectangular region.
3. Release the button to perform the zoom operation.
These operations can be repeated several times to continue zooming.
Press <q> or the right mouse button to quit the option.
This tool is also accessible with the <F2> key.
Fit Button
The fit button is used to fit the content of the view to the view limits without changing the current
orientation of the camera (which can be interpreted as the user's eyes).
This tool is also accessible with the <F3> key.
Original Button
The original button is used to fit the content of the view and to give a default orientation to the
camera.
This tool is also accessible with the <F4> key.
Cutting Plane
This option displays a movable plane that cuts the geometry and the mesh. The surface mesh is
displayed. The plane is symbolically represented by four boundaries and its normal, and is by
default semi-transparent. After a click on the button,
l Press and drag the left mouse button to rotate the plane,
l Press and drag the middle mouse button to translate the plane,
l Press <x>, <y> or <z> to align the plane normal along the X, Y or Z axis,
l Press <n> to reverse the plane normal,
l Press <o> to open the Cutting plane options dialog box:
FIGURE 2.13
Cutting plane options dialog box
Hide cut-away: hide the geometry on the other side of the plane.
Activate transparency: deactivate to make the cutting plane fully transparent
It is advised to deactivate plane transparency when using X11 driver to increase the execution speed.
Show mesh: deactivate to hide the mesh and view geometry only.
Intersecting cutting plane only: active to display only cells intersecting the cutting plane. The
cells are displayed through each side of the cutting plane.
Shading: active to display cells in solid mode. Deactivate for wireframe mode.
Shrink factor: from 0 to 1, the shrink factor reduces the cell size in the X, Y and Z direction.
FIGURE 2.14
Shrink factor from 0.2 to 0.7
2.11
FILE CHOOSER
For file management (opening and saving of files) FINE™/Open with OpenLabs™ uses the
standard File Chooser window. The layout of the File Chooser depends on the operating system
used, but a typical layout is shown in FIGURE 2.15. The Directories list allows the user to
browse through the available directory structure to the project directory.
The Files list can then be used to select the file name. In the case where a file needs to be opened,
an existing file should be selected in the list of available files. When creating a new file, the user
can type a new file name with the appropriate extension.
In the List Files of Type bar the default file type is set by default to list only the files of the
required type. For a description of all available file types in FINE™/Open with OpenLabs™, see
Project Management section.
FIGURE 2.15
Typical layout of a File Chooser window
2.12 PROFILE MANAGER
When a law is defined by a profile, clicking on the button
will invoke a Profile Manager window.
, right next to the pull down menu,
The Profile Manager is used to interactively define and edit profiles for both fluids and boundary
conditions parameters. The user simply enters the corresponding coordinates in the two columns
on the left. The graph is updated after each coordinate (after each coordinate press the <Enter>
key).
FIGURE 2.16
Profile Manager for fluid parameters
The Import button may be used if the profile exists already as a file on the disk. The Export
button is used to store the current data presented in the Profile Manager window as a file (for
example to share profiles between different projects and users). The formats of the profile files are
explained in the File Formats chapter presenting all files formats used by FINE™/Open with
OpenLabs™ and the flow solver.
If the mouse cursor is placed over a point in the graph window, this point is highlighted in blue
and the corresponding coordinates on the left will be also highlighted, giving the user the
possibility to verify the profile.
The button OK will store the profile values and return back to the main FINE™/Open with
OpenLabs™ window.
CHAPTER 3.
FLUID MODEL
Every FINE™/Open with OpenLabs™ project contains a fluid with corresponding properties. In
FINE™/Open with OpenLabs™, the fluid can be defined by:
1. using the fluid defined in the project file of which the properties are shown on the fluid selection
page, or
2. selecting a fluid from the fluid database included in the release, or
3. creating a new fluid.
When opening the Fluid Model page, the user gets all information of the currently used fluid. The
fluid can be edited, using the Edit button, or replaced by another fluid, using the Select button, which
shows the currently available fluid database and gives the user ability to manage the database.
FIGURE 3.1
Fluid Model page
In the next section, the interface is described in detail, including advice for use of the fluid definition.
In this section
3.1 Fluid Properties
3.2 Edit Current Fluid
3.3 Select Fluid from database
3.4 Add Fluid to Database
3.5 Delete Fluid from Database
3.6 Reference Pressure & Temperature
3.7 Expert Parameters
78
FINE™/Open with OpenLabs™ 7.2 User Guide
79
80
81
84
91
3.1
FLUID PROPERTIES
Every FINE™/Open with OpenLabs™ project contains a fluid with the properties displayed in
the interface.
When a new project is created, the used fluid is a default fluid. When an existing project is
opened, the fluid is defined by the properties as given in the project file.
The first listed fluid property is the fluid type. Four fluid types are available. For more detail on
each of these types see the theoretical manual.
l perfect gas,
l real gas
l incompressible gas or liquid,
l condensable gas
For the first three fluid types above, the following properties are listed:
l the reference pressure and temperature at which the properties are defined
l the specific heat
l the heat conduction
l the viscosity
l the density law (for an incompressible fluid)
For the condensable gas, the table path and all other defined properties are listed. The range of the
independent variables of all available tables can be checked by clicking on the symbol
.
3.2
EDIT CURRENT FLUID
All the fluid properties can be modified by clicking on the button Edit.... See section Add Fluid to
Database for how to define fluid properties.
the modifications will be local
the fluid
Notice that
database. To modify the fluid database, the fluid must be removed from the list, see Select Fluid
from Database section, and then recreate it.
to the current project, and will not affect
3.3
SELECT FLUID FROM DATABASE
Another fluid may be selected from the fluid database by clicking the button Select... or a new
fluid may be defined .
After clicking the button Select..., the Fluid Database page appears, which contains the list of
pre-defined fluids and the user-defined fluids. Each fluid has a type and an access permission.
Each fluid is associated with the user who created it and can be removed only by its owner (the
owner has Read Write Delete permissions). All other users have Read Only permissions.
The user may select a fluid from the list. The selection will be highlighted and the properties of
the selected fluid are displayed in the Properties frame below the fluid list. After clicking on the
button Ok, the selected fluid will be used in the project.
FIGURE 3.2
Fluid Selection page
In the Fluid Database page, the user can also add a new fluid into the database (New fluid..., see
Add Fluid to Database section for more details), or delete a fluid from the database (Delete fluid,
see Delete Fluid from Database section for more details).
3.4
ADD FLUID TO DATABASE
To add a new fluid to the database click on the New fluid... button on the Fluid Database page.
A wizard will appear, allowing the user to specify the new fluid's properties.
On the first page of the wizard, the user can enter the name and type of the new fluid. The name
should be entered by moving the mouse to the text box for the Fluid name and typing the name
on the keyboard. By default, a name is proposed.
FIGURE 3.3
New Fluid Wizard - Fluid Type
Then, the user should select Add to NUMECA fluid database or Add to User fluid database.
When selecting Add to NUMECA fluid database, the new fluid will be saved to:
Installation_path/fineopen72/COMMON/euranus.flb (on LINUX)
Installation_path\fineopen72\bin\euranus.flb (on Windows)
When selecting Add to User fluid database, the new fluid will be saved to:
$HOME/.numeca/Common/My_fluids.flb (on LINUX)
%HOMEPATH%\.numeca\Common\My_fluids.flb (on Windows)
If a condensable fluid is defined,
thermodynamic_tables, which is located in the same directory as My_fluids.flb.
the thermodynamic tables will be copied to the folder
If the user selects Add to User fluid database, the other users will not be able to use the
defined fluids.
The fluid type can be entered by selecting the appropriate check boxes. First make a choice for a
compressible, incompressible or condensable fluid. For a compressible fluid select a perfect gas or
a real gas.
To cancel the modifications to the fluid definition and close the wizard, click on the Cancel
button.
Once the fluid name and type are correctly set, click on Next>> to go to the next page of the
wizard. On this page the following properties are defined:
l Reference pressure and temperature at which the properties are defined,
l Specific Heat Law,
l Heat Conduction Law,
l Viscosity Law,
l Density Law (for an incompressible fluid only).
l Thermodynamic tables folder (for condensable fluid only).
The possible values to enter for these laws depend on the selected fluid types as described in the
next paragraphs.
Information linked to fluid creation is stored in the fluid database only when closing the
FINE™/Open GUI. As a consequence, this information will not be available to other users until the
operation is completed.
When defining a fluid law by using a profile, the definition must cover all the range considered in the
simulation. Otherwise the simulation may give a wrong solution or even crash.
Definition of a Perfect Gas
In order to define a perfect gas, the user has to specify:
l The specific heat at constant pressure. For a perfect gas only a constant Cp is allowed.
l The characteristic specific heat ratio (γ = Cp/Cv) of the fluid.
l The heat conductivity, which may be constant, defined by a profile in temperature or specified
through a constant Prandtl number.
l For the viscosity, the dynamic or kinematic viscosity can be specified. The viscosity law which
may be constant, temperature dependent or specified by the Sutherland law. In case the
viscosity law is defined by the Sutherland law, the Sutherland parameters are accessible. The
user can click on the button (
) to view the definition of the Sutherland law.
FIGURE 3.4
New Fluid Wizard - Perfect Gas Properties
Definition of a Real Gas
In order to define a real gas, the user has to specify:
l The specific heat defined by a profile in temperature. For a real gas, cp can only be defined as
a profile.
l The gas constant R of the fluid.
l The heat conductivity, which may be constant, defined by a profile in temperature or specified
through a constant Prandtl number.
l For the viscosity, the dynamic or kinematic viscosity can be specified. The viscosity law which
may be constant, temperature dependent or specified by the Sutherland law. In case the
viscosity law is defined by the Sutherland law, the Sutherland parameters are accessible. The
user can click on the button (
) to view the definition of the Sutherland law.
FIGURE 3.5
New Fluid Wizard - Real Gas Properties
Definition of a Liquid
Presently, only Newtonian liquids, with constant density, can be simulated. The user then has to
specify:
l The specific heat at constant pressure. For liquids only a constant Cp is allowed.
l The heat conductivity which may be constant, defined by a profile in temperature or specified
through a constant Prandtl number.
l For the viscosity, the dynamic or kinematic viscosity can be specified. The viscosity law which
may be constant or defined by a profile.
l The density law follows the Boussinesq law. In this latter case, the density is constant and the
Boussinesq coefficients (compressibility and dilatation coefficients) are taken into account only
if the button Gravity Forces (Flow Model page) is activated. These coefficients are used in
source terms of the momentum equation and the energy equation in order to model the
gravitational effect (i.e. natural convection) although the density is assumed to be strictly
constant.
For liquids, the reference temperature and pressure must lie in the expected range of the static
temperature and pressure of the flow field.
Definition of a Condensable Gas
The aim of the condensable fluid module is to model the real thermodynamic properties of the
fluid by means of interpolation of the variables from dedicated tables.
The module can be used for a single-phase fluid of which the properties are too complex to be
treated with a perfect or real gas model. It can also be used in order to treat thermodynamic
conditions that are close to the saturation line. Note that the model can be used on the liquid or on
the vapour side of the saturation curve. In case that the thermodynamic state lies inside the two-
phase region, a homogeneous equilibrium two-phase mixture of vapour and liquid is considered.
However the hypothesis of an equilibrium mixture is not valid if the dryness (wetness) fraction
exceeds 20%. The module can not be used above these fractions, as it completely ignores
evaporation-condensation phenomena.
The approach that has been adopted in the FINE™/Open solver consists of using a series of
thermodynamic tables, one table being required each time a thermodynamic variable must be
deduced from two other ones. This implies the creation of many tables as an input, but presents
the advantage that no iterative inversion of the tables is done in the solver, with as a consequence
a very small additional CPU time.
two sets of
By default,
thermodynamic tables are provided in the FINE™/Open with
OpenLabs™ package: Refrigerant R134a and Water-Steam tables. The other thermodynamic
tables can be generated using TabGen by the user or provided by NUMECA, upon request.
In order to define a new condensable fluid, the user has to create a new fluid by clicking the
button New fluid.... In the first page of the wizard, select the fluid type Condensable. In the
second page of the wizard, the user needs to specify the folder where the thermodynamic tables
locate. After specifying the location of the thermodynamic tables, the range of the independent
variables will be displayed.
By default, the specific heat, the heat conductivity and the viscosity are defined by the tables, if
the related table is available. The user can also select different definition for these quantities:
l The specific heat can be defined by a constant or by thermodynamic tables.
l The heat conductivity can be defined by a constant, a profile function of temperature, a
constant Prandtl number or by thermodynamic tables.
l The viscosity can be defined by a constant,
the Sutherland law, a profile function of
temperature or by thermodynamic tables.
According to the flow type, the required tables by the flow solver are different. The files used by
FINE™/Open with OpenLabs™ are the .atab files that contain the tabulated information of the
coefficients of the interpolation polynomials. Here lists all the tables that may be used in the
computation:
l The 1D tables:
l PSA.atab: contains the liquid and vapor saturation lines function of the saturation pressure:
liquid and vapor densities, liquid and vapor enthalpies, ....
l The 2D tables:
l AER.atab: Quality function of energy and density
l AHP.atab: Quality function of enthalpy and pressure
l BER.atab: Heat capacity function of energy and density
l BHP.atab: Heat capacity function of enthalpy and pressure
l CER.atab: Speed of sound function of energy and density
l CHP.atab: Speed of sound function of enthalpy and pressure
l DPT.atab: density function of pressure and temperature
l EPT.atab: energy function of pressure and temperature
l HSP.atab: enthalpy function of entropy and pressure
l KER.atab: thermal conductivity function of energy and density
l KHP.atab: thermal conductivity function of enthalpy and pressure
l MER.atab: dynamic viscosity function of energy and density
l MHP.atab: dynamic viscosity function of enthalpy and pressure
l PER.atab: pressure function of energy and density
l PHS.atab: pressure function of enthalpy and entropy
l RHP.atab: density in function of enthalpy and pressure
l RHS.atab: Pressure over density in function of enthalpy and entropy
l SHP.atab: entropy function of enthalpy and pressure
l TER.atab: temperature function of energy and density
l THP.atab: temperature function of enthalpy and pressure
A classification of the tables function of their use follows here:
l Necessary tables for computations without preconditioning: PER.atab, TER.atab
l Necessary tables for computations with preconditioning: RHP.atab, THP.atab
l Necessary tables for computations with initial solution for turbomachinery and/or for inlet
boundary conditions where total enthalpy and dryness fraction are imposed: SHP.atab,
THP.atab, RHP.atab, HSP.atab, EPT.atab, DPT.atab and PSA.atab
l Necessary tables for total quantities (imposed at inlet or as outputs): SHP.atab, THP.atab,
RHP.atab, HSP.atab, EPT.atab, DPT.atab
l Necessary tables for cavitation computation: AHP.atab, AER.atab and PSA.atab
The following tables are optional but we advise to use them:
l Transport properties (viscosity and conductivity): MER.atab, MHP.atab, KER.atab, KHP.atab
l Speed of sound tables: CER.atab, CHP.atab
The .ntb files are not needed to run a computation. They are generated by TabGen and contain all
the tabulation for two independent quantities and all the dependent ones. The .ntb files can be
deleted as well as the .btab (binary counterpart of .atab)
3.5
DELETE FLUID FROM DATABASE
When the user has the permission to delete a fluid (Read Write permission), the button Delete fluid
(FIGURE 3.1) allows the user to remove the selected fluid from the database.
is stored in the fluid database only when closing the
Information linked to fluid removal
FINE™/Open GUI. As a consequence, this information will not be available to other users until this
operation is completed. A message will however warn users that the fluid properties have been
modified (until removal in the present situation) by the owner.
3.6
REFERENCE PRESSURE & TEMPERATURE
The reference pressure and temperature for the fluid are used:
l when defining the fluid viscosity using Sutherland's law.
l in the density law (Boussinesq law) for incompressible fluids, when gravitational effects are
taken into account.
l in the application of an outlet boundary condition for which the mass flow is imposed with
pressure adaptation.
3.7
EXPERT PARAMETERS
All expert parameters are available in the Advanced tab of the Computation Control/Control
Variables page. For these parameters the default values are generally the appropriate ones and
only have to be changed if the user has specific wishes concerning the fluid modeling.
phys_PrandtlTurb_: allows to define the turbulent Prandtl number. Default value is set to 1.0.
iCondTableClip_: The thermodynamic tables are generated in a given range of thermodynamic
variables. When the thermodynamic variable is not in the given range, the expert parameter
iCondTableClip_ can be used to control the computing method of the dependent thermodynamic
variable.
0: the dependent thermodynamic variable is extrapolated from the interior field.
1 (default): a clipping value will be used for the dependent thermodynamic variable.
iHStablesNotUsed_: When a coarse PHS table is used, the computation may produce a very
large error when calculating the total pressure and total temperature from the static pressure and
static temperature, and vice versa. Instead, a SHP table will be more accuracy when the pressure
from enthalpy and entropy is needed. But it needs a bit more CPU time because an iterative
procedure is needed. The expert parameter iHStablesNotUsed_ is used to control which table will
be used.
0: the PHS table will be used.
1 (default): the SHP table will be used.
table_cp_Limit_: When the heat capacity is computed by using thermodynamic table, the heat
capacity shows a singularity at the critical point, where the value becomes infinite. In order to
avoid numerical problems, the parameter table_cp_Limit_ is introduced to clip the heat capacity.
By default, the value is set to 100000. If the heat capacity is clipped, a message is given in the .std
file, indicating the number of cells for which the clipped value is used.
CHAPTER 4.
FLOW MODEL
The Flow Model page, as shown in FIGURE 4.1, can be used to specify several characteristics of the
flow:
l the mathematical model to:
l choose between viscous and non-viscous flow,
l choose between laminar and turbulent flow,
l activate gravity,
l activate pre-conditioning for low speed flow,
l characteristic scales defining the Reynolds number of the flow.
In addition, the heat source term can be specified through the expert parameters.
This chapter is organized in the following way:
l Mathematical Model section describes the interface and best practice for the definition of the
mathematical model and, especially, for the available turbulence models,
l Characteristic Values - Reynolds Number section provides details on the Reynolds number
related information and reference values.
The settings of pre-conditioning for low speed flow can be seen in the Numerical Model Chapter.
FIGURE 4.1
Flow Model page
In this section
4.1 Mathematical Model
4.2 Characteristic Values - Reynolds Number
95
126
4.1
MATHEMATICAL MODEL
4.1.1
Euler
By selecting Euler on the Flow Model page, an inviscid calculation will be performed. In such a
case, all solid walls are considered as Euler walls, i.e. only normal velocity components are set to
zero at the wall.
Note that the Reynolds number has no meaning for Euler calculations.
4.1.2
Laminar Navier-Stokes
When selecting Laminar Navier-Stokes equations, the only effect is on the thermodynamic
property of the flow. The viscosity will be the laminar kinematic viscosity and therefore does not
contain any turbulent component.
4.1.3
Turbulent Navier-Stokes
When selecting Turbulent Navier-Stokes, turbulence is taken into account through the chosen
turbulence model. In FINE™/Open with OpenLabs™, several turbulence models are available:
l Spalart-Allmaras,
l Spalart-Allmaras (Extended Wall Function),
l SARC,
l SARC (Extended Wall Function),
l k-ε (Standard), only available for combustion computations
l k-ε (Extended wall function),
l k-ε (low Reynolds number Yang-Shih),
l k-ω (M-SST),
l k-ω (M-SST, Extended wall function),
l S-BSL-EARSM,
l S-BSL-EARSM (Extended wall function).
The wall functions are used to mimic the presence of the walls by reflecting the effect of the steep,
non-linear variations of the flow properties through the turbulent boundary layer. They define the
shear stress and the heat flux on the cell faces lying on solid boundaries as well as the values of
the turbulent variables in the vicinity of the wall. FINE™/Open provides both standard wall
function (only for k-ε model) and extended wall function. For more details, see Modeling the flow
near the wall.
In the following sections, the interface parameters related to the turbulence models are described.
For all the turbulence models, additional equations are solved and consequently suitable additional
initial and boundaries conditions must be defined in the interface.
Boundary Condition
Inlet or External:
l Spalart-Allmaras and SARC models: the value of the turbulence viscosity must be specified. It
can be constant or varying in space. The user can specify 1D spatial variation using the profile
manager.
l k-ε, k-ω and S-BSL-EARSM models: the values of the turbulent quantities (k and ε) must be
specified. They can be constant or varying in space. The user can specify 1D spatial variation
using the profile manager.
Solid wall
l When using the turbulence models with extended wall function, the wall can be defined as
smooth or rough:
l For a smooth solid wall (default), only the Von Karman constant and a constant Bo have to
be specified.
l When selecting a rough solid wall, two additional parameters have to be specified: the
equivalent roughness height and the zero-displacement plane.
Initial Condition
l Spalart-Allmaras and SARC models: a value of
has to be specified if the constant initial
solution or the turbomachinery initial solution is chosen.
kinematic viscosity of the fluid. The ratio
is the Spalart viscosity, and ν is the
is equivalent to the ratio between the turbulent
eddy-viscosity and the kinematic viscosity
, for values higher or equal to 1. When
decreasing
below 1,
the ratio
decreases more significantly. The value of
corresponds to
. Once this ratio has been specified, the
FINE™/Open solver automatically uses it to initialize the flow field.
l k-ε, k-ω and S-BSL-EARSM models: the initial values of the turbulent quantities (k and ε) are
specified by the user when the constant initial solution is chosen.
4.1.4
Advanced Parameters for Turbulence modeling
Non-interfaced Expert Parameters
All non-interfaced advanced parameters related to the turbulence models are accessible on the
Control Variables page, in the Advanced sub-menu.
All turbulence models
turb_mavRes_: denoted here ζ, allows the user to control the update of k and ε (k-ε and k-ω
(Spalart-Allmaras and SARC models) for each Runge-Kutta stage. The default
models) or of
, the following restrictions are
value is set to 0.95. Denoting the new value of k, ϵ or
as
imposed:
If turb_mavRes_ > 0:
where EPS is equal to 1E-20. EPS is used to avoid possible divisions by zero.
If turb_mavRes_= 0: only the restriction defined is applied.
turb_mavRem_: denoted below as ζ, allows the user to control the multigrid corrections for k
(Spalart-Allmaras and SARC models). The default value is
and ε (k-ε and k-ω models) or of
0.95.
If turb_mavRem_> 0:
If turb_mavRem_= 0: restriction to positive values,
If turb_mavRem_< 0:
turb_mutMuLimit_: controls the maximum allowable value for the ratio
in the flow field
but not on boundary conditions (default value = 50000).
turb_ ProdWithDiamondGrad_ : controls methodology used to compute the gradients when
evaluating the turbulent production term.
0 (default): based on Least Square gradients,
1: based on Diamond gradients.
k-ε models
phys_PrandtlTurb_: the turbulent Prandtl number (default = 1.0)
ke_Ceps1_: Ceps1 constant in the k-ε equations (default = 1.44)
ke_Ceps2_: Ceps2 constant in the k-ε equations (default = 1.92)
turb_KEpsProd_: control the production term in the k-ε model.
0 (default): linearized production term;
1: the non-linear production term.
turb_iYAP_: control the Yap correction in the k-ε (Extended Wall Function) and k-ε (Low Re
Yang-Shih, classic) model.
0: deactivate the Yap correction;
1 (default): activate the Yap correction.
Wall distance
dtw_method_: Controls which algorithm is used for calculation of the distance to the wall.
1 (default): calculates the distance to the wall as the point to the nearest boundary cell center.
2: calculates the distance to the wall using an orthogonal projection of the point on the solid
surface
When changing the method calculating the distance to wall, the .dtw file of the mesh must be
removed manually if it exists.
4.1.5
Best Practice for Turbulence Modeling
A.
Introduction to Turbulence
Turbulence can be defined as the appearance of non-deterministic fluctuations of all variables
(velocity u", pressure p", etc....) around mean values. Turbulence is generated above a critical
Reynolds number that may range in values from 400 to 2000 depending on the specific case. In
95% of industrial applications, the flow Reynolds number lies above that range. This is why it is
in general necessary to predict adequately the turbulence effects on the flow-field behavior.
To model turbulent flow in a satisfactory way, four steps should be performed:
l choosing a turbulence model,
l generating an appropriate grid,
l defining initial and boundary conditions,
l setting expert parameters to produce convergence.
B. First Step: Choosing a Turbulence Model
A turbulence model is chosen based on the specific application. The following table shows the
most appropriate turbulence models to use for different types of flows:
TABLE 4.1 Recommended turbulence models for different flow types and appropriate y+ values
Turbulence Models
High-Re
Spalart-Allmaras (Extended Wall
Function);
SARC (Extended Wall Function);
Low-Re
Spalart-Allmaras;
Spalart-Allmaras (Extended Wall
Function);
k-ε (Standard);
SARC;
k-ε (Extended Wall-function);
SARC (Extended Wall Function);
k-ω (M-SST, Extended Wall
Function);
S-BSL-EARSM (Extended Wall
Function)
k-ε (Extended Wall function);
k-ε (Low Re Yang-Shih, classic);
k-ω (M-SST);
k-ω (M-SST, Extended Wall
Function);
S-BSL-EARSM;
S-BSL-EARSM (Extended Wall
Function)
Most Appropriate
Flows
Quasi-2D;
3D;
Weak pressure gradient;
Strong pressure gradient;
Quick design-cycle calculations
Moderate curvature;
y+
20 - 50
Separating flows
< 10
Two main kinds of turbulence models are present in the FINE™/Open solver:
l one-equation models (e.g. Spalart-Allmaras and Simplified SARC),
l two-equation models (k-ε, k-ω and S-BSL-EARSM models).
When quick turbulence calculations are required, for example, in design-cycle analysis, it is
recommended to use the Spalart-Allmaras model.
Turbulence models with Extended Wall Function are often used in design. These models employ
an empirically based logarithmic function to represent the near-wall physics and require a lower
grid resolution in this region as a result.
The M-SST k-ω turbulence model is another popular two-equation model. This model combines
the advantages of the Wilcox k-ω model and the k-ε model and has higher accuracy in the
prediction of separated flows. The recommendation is to use the M-SST k-ω model in prediction
of the onset and the amount of separation under adverse pressure gradient conditions.
C. Second Step: Generating an Appropriate Grid
Cell Size
When computing turbulence quantities, it is important to place the first grid node away from the
wall within a certain range (ywall). When doing viscous computations (Navier-Stokes equations),
the boundary layer near a solid wall contains high gradients. To properly capture these high
gradients, it is important to have a sufficient number of grid points inside the boundary layer.
When Euler computations are performed, no boundary layer exists and therefore the cell size near
solid walls is of less importance.
To estimate an appropriate cell size ywall for Navier-Stokes simulations including turbulence, the
local Reynolds number based on the wall variable y+is computed.
The value of y+ associated with the first node off the wall will be referred to here as y1
+:
where uτ is the friction velocity:
Note that the value of ywall depends on the desired value of y1
+.
FIGURE 4.2 shows the evolution of u+ against y+ from the measurements of Lindgren (1965)
with:
.
Note that the viscous sublayer extends up to y+=5 but 10 is an acceptable approximation for
design calculations.
FIGURE 4.2
Boundary layer profiles (v*= uτ, from White, F.M., Viscous Fluid Flow, McGraw Hill, 1991).
+ values less than 10
Low-Re models resolve the viscous sublayer and are well suited for y1
+
whereas high-Re models apply analytical functions to the log-layer and are appropriate to y1
values ranging from 20 to 50, even more (depending on the extension of the buffer layer for the
considered flow). When the extended wall function is used, it is strongly advised to locate the first
inner node either in the viscous sublayer or in the log layer (y1
Moreover one can notice that the logarithmic function does not apply for separated flow. So when
a significant amount of separation is expected, a low-Reynolds number turbulence model is more
appropriate.
+<5 or y1
+>20).
+ specific to the different types of
Recommendations are given in the TABLE 4.1 for ranges of y1
models. One way to estimate ywall as a function of a desired y+ value is to use a truncated series
solution of the Blasius equation:
Note that the reference velocity, Vref, can be taken from an average at the inlet. For instance, if
the mass flow is known, the value can be calculated using the density and the cross-sectional area
of the inlet. If the mass flow is not known the reference velocity may be calculated from the inlet
total pressure and an estimated static pressure using isentropic relations. The reference length,
Lref, should be based on streamwise distance since an estimation of boundary layer thickness is
implied in this calculation. For instance, in the case of a turbomachinery simulation one could use
the distance of hub and shroud curves that exist upstream of the first row of blades. This is
approximate, of course, as the thickness of boundary layers will vary widely within the
computational domain. Fortunately it is only necessary to place y+ within a range and not at a
specific value.
Another method of estimating ywall is to apply the 1/7th velocity profile. In this case the skin
friction coefficient Cf is related to the Reynolds number:
where Rex should be based on average streamwise values of Vref and Lref as discussed above.
Since uτ is based on Cf, it may be calculated based on the equation of uτ, and ywall may then be
calculated. Note that either method is not exact but they will yield results that are quite close to
each other. In fact, it can be instructive to calculate ywall using both methods as a check. Since
only one wall distance is being calculated, the particular flow being studied should be kept in
mind. For instance, if it is a diffusing flow Cf, and hence y+, can be expected to drop. Since a
certain range is desired (e.g., 20< y+<50 for high-Re Standard k- ε), the user may choose to base
the calculation of wall distance on an average of that range (e.g., 40).
Verification of y+
These instructions should provide reasonable estimates but it is always wise to plot y+ once a
solution has finished. Hence, color contours on the walls representing y+ over the first layer of
nodes should be represented in CFView™ to check that most y+ values fall within the desired
range.
There are some special cases where such checks do not strictly apply. For instance, skin friction
approaches zero at points of separation so it is expected that y+ will be low in such regions.
General Advice
What grid resolution is adequate?
The resolution method employed in the FINE™/Open solver requires approximately 9 nodes
across a free shear- layer and approximately 15 across a boundary layer to provide grid-
independent results for turbulent flows. If wall functions are used the boundary layer only requires
approximately 9 nodes.
Of course, the flow field under study will realistically consist of shear layers of which the width
varies substantially throughout the flow field. The user must therefore decide what is important to
capture and what is not. The selection of nodes in the streamwise direction should be governed by
what resolution adequately represents the studied geometry. Regions of concentrated high
gradients, such as airfoil leading or trailing edges or any geometrical corners should contain a
relatively high clustering of nodes.
What determines the grid quality?
After the various grid resolution concerns are addressed, the level of skewness must be analyzed.
Providing clustering in a curved geometry can often lead to internal angles of grids cells of less
than 10°. It is important to minimize the number of cells containing such low angles as the
calculation of fluxes can become significantly erroneous under such conditions. More information
concerning how to check the quality of a grid can be found in the HEXPRESS™ User Guide and
the HEXPRESS™/Hybrid User Guide . If the adjustment of the number of nodes and the
clustering does not reduce the level of skewness, local smoothing should be applied. The
expansion ratio, the ratio of adjacent cell sizes, should also be checked. It is particularly important
to keep this value within an absolute range of about 0 - 1.6 in regions of high gradients, such as
boundary layers, free shear-layers and shocks. If it is evident that adjacent cells are different in
size by factors significantly greater than two, the clustering in this region should be reduced or the
number of nodes should be increased.
Things to Look Out For
By following these instructions, it should be possible to generate a grid of reasonable quality for
turbulent flows. It is recommended, however, that the user checks the values of y + within
CFView™ after approximately one hundred iterations on the fine grid to ensure the proper range
has been specified. At the same time, it can be useful to plot contours of residuals (continuity,
momentum, energy and turbulence) over selective planes within CFView™. If the level of
skewness is too high, this will be indicated by local peaks in residuals that are orders of magnitude
greater than the rest of the flow field.
D. Defining Initial and Boundary Conditions
Turbulence is commonly modeled by emulating molecular diffusion with a so-called "eddy-
viscosity" (μT). A standard method for determining μT is based on turbulent-eddy length and time
scales that are modeled through turbulence kinetic energy (k) and dissipation (e.g. ε) equations. It
is important to note that the level of turbulence quantities (i.e. turbulence intensity, μ T, k, ε)
specified at the inlet boundary can have a strong effect on the flow-field prediction for quantities
like the total pressure, velocity profiles, flow angles, total temperature etc. Since the measurement
of turbulence is rarely conducted in a design and test environment, the designer faces the problem
of setting these quantities without knowing the correct values.
Spalart-Allmaras and SARC Models
In the Boundary Conditions page, the turbulent eddy viscosity
in relation to the kinematic viscosity :
at inlet needs to be specified
l For internal flows (e.g. turbomachinery):
= 1 to 5.
l For external flows (e.g. vehicle aerodynamics):
= 1.
The turbulent eddy viscosity is set automatically to zero at the walls and is extrapolated at outlets.
In the Initial Solution page a default value for
of 50 is proposed, where
is the Spalart
viscosity and
estimation. This value is used to initialize the flow field for the Spalart viscosity. The ratio
the kinematic viscosity of the fluid. It is rarely necessary to change this initial
is
depending of the ratio between the turbulent eddy-viscosity and the kinematic viscosity
with the formula
with
,
and
. The ratio
is
very close to the ratio
, for values higher or equal to 10. When decreasing
below 10,
the ratio
decreases more significantly. For example,
for
the ratio
.
k-ε, k-ω and S-BSL-EARSM Models
Recommendation to estimate the turbulent kinetic energy and turbulent
dissipation
If there is no (experimental) data available for the turbulence intensity or the wall shear stress, the
inlet boundary conditions for turbulence can be estimated in the following way.
First an estimation of the ratio of the turbulent viscosity to the laminar viscosity is needed:
l For internal flows (such as turbomachinery flow), typical values are
l For external flows (in aerodynamics computations), typical values are
.
.
The value of the turbulent kinetic energy, k is defined as:
with U the streamwise velocity, L ref the characteristic length of the domain, ν the kinematic
viscosity of the fluid and Cμ=0.09.
The value of ε, the turbulent dissipation is:
with ρref the reference density of the fluid.
Details on the estimation of the turbulent kinetic energy and turbulent
dissipation
The recommendation in the previous section can be used if no further information on the
turbulence is available. More in general several methods exist to determine k and ε exist based on
different assumptions as detailed below. Combination of two of the methods to determine ε have
lead to the above recommendation as further explained at the end of this section.
Estimation of k
The value of the turbulent kinetic energy can be derived from the turbulence intensity Tu or from
the wall shear stress.
l From the turbulence intensity: The turbulence intensity Tu can be expressed as a function of
the streamwise fluctuating velocity u" and the streamwise velocity Uref:
For internal flows the value of Tu is about 5% and for external flows it is reduced to 1%. With
these considerations k can be calculated by considering an isotropic turbulence:
l From the wall shear stress: If the wall shear stress is known, the user can use the wall
functions defined for the fully turbulent flow:
This value of k could be used as an initial value and also for the inlet boundary condition.
Estimation of ε
The value of the turbulent dissipation can be specified through one of the following rules:
l Specify the turbulent length scale (only valid for internal flows).
A typical values is
. where DH is the hydraulic diameter of the inlet section
l Derive ε from the asymptotic turbulent kinetic equation:
In a free uniform flow the turbulent kinetic energy equation reduces to
This relation can be used to specify the value of the turbulent dissipation in the following way:
where U is the inlet velocity, Δk the decay of the turbulent kinetic energy over a length L. For
example, in turbomachinery, L is the maximum geometric length and Δk could be set to 10%
of the inlet value of k. In other words: k is expected to decrease by about 10% over a length L
that is characteristic to the size of the domain.
Using this method, the user must make sure that the value of the turbulent viscosity obtained
. If this
from these values of k and ε is not too big or too small. i.e.
condition is not satisfied, it is advised to scale down or up the value of k inlet or the Δk and
compute again the turbulent dissipation.
l Specify the wall shear stress.
If the wall shear stress is known, the user can use the wall functions defined for the fully
turbulent flow.
l Specify the ratio of the turbulent viscosity to the laminar viscosity
For internal flows (such as turbomachinery flow), typical values are
For external flows (in aerodynamics computations), typical values are
.
.
Any of the above methods can be applied for setting the boundary conditions. However, if the
resulting values of k and ε lead to the damping of the turbulence shortly after the inlet section, we
suggest the user derives ε from the asymptotic turbulent kinetic equation and selects an inlet value
of k such that the ratio of the turbulent viscosity to the laminar viscosity equals 50.
In some cases the different methods to estimate ε may result in very different values. In such a
case it is recommended to re-evaluate k and ε in the following manner:
Combine the asymptotic turbulent kinetic equation:
with the
expression based on the ratio of the turbulent viscosity to the laminar viscosity:
with Cμ=0.09 and μ representing the laminar viscosity of the fluid to obtain k:
Using either of the two expressions for ε then easily leads to an estimation of ε at the inlet.
Initial solution for the turbulent kinetic energy and turbulent dissipation
If there is an initial solution file containing k and ε, the k and ε values of this file are used to
initialize the fields. The values mentioned above can also be used to set the initial conditions for
the k and ε fields. However, to reduce the possibility of oscillations in the skin friction due to non-
physical relaminarization during convergence, it is recommended to set
.
E. Wall Distances
All turbulence models need to compute the wall distances everywhere in the computed domain. It
is a rather time consuming process, so that they are saved in a ".dtw" mesh file at the beginning of
the first computation. These values are read and used for the next computations. If the mesh file
(".hex") is modified, they are erased and will be computed again.
The ".dtw" file is saved in the mesh directory. When launching the computation, the wall distance is
computed once for each concerned grid level. As a consequence, it is recommended not to launch
multiple computations evolving the same mesh when its wall distance has not been yet computed.
Two strategies are available for wall distance calculation. The old algorithm counts the distance
between the cell center and then center of the boundary faces; while the new approach takes the
orthogonal projection.
This behavior is control by the expert parameter dtw_Method_.
4.1.6
LES/DES models
Direct Numerical Simulation (DNS) is the most accurate method for solving turbulence in flows.
In DNS the Navier-Stokes equations are solved on a fine mesh with small physical time-step, to
resolve all the spatial/temporal scales in the entire flow field. However, the computational cost of
DNS is excessively high, even at very low Reynolds numbers.
RANS models have shown remarkable strength in plenty of industrial applications, but it is
incapable to give any information of turbulent spectrum which is essential for many practical
issues. Examples are acoustic simulations where the turbulence generates noise sources.
Large Eddy Simulation(LES) and Detached Eddy Simulation(DES) in which at least a part of
turbulence spectrum is resolved in at least a portion of numerical domain. Such methods bridge
the two extremes of DNS and RANS, providing considerable accuracy and also efficiency with
affordable computational resource.
In FINE™/Open with OpenLabs™, the LES/DES models are available from the page Physical
Configuration/ Flow Model in the Graphic User Interface. To be more clear, these models are
separated from RANS ones.
The following models are available:
l Spalart-Allmaras DDES
l Spalart-Allmaras DDES (Extended Wall Function)
l Spalart-Allmaras IDDES
l Spalart-Allmaras IDDES (Extended Wall Function)
l Smagorinsky-Lilly LES
l WALE LES
The LES/DES models are visible only in Unsteady mode
A. Brief Overview of Models
Large Eddy Simulation (LES)
LES is the most widely used scale resolving model over the last decades. A LES approach
resolves all large turbulent structures which have impact on the flow field up to grid limits. The
dissipation of the energy from Kolgomorov scales is achieved by introduction of Sub-Grid -Scale
(SGS) model.
The main limitation originates from the excessive resolution requirements for wall-bounded flows at
high Reynolds number. Hence LES has remained a research tool in academic community, rather than
a industrial approach.
The most widely used LES model is the Smagorinsky model:
this classical model provides non-zero eddy-viscosity for simple laminar shear flows, negatively
affecting prediction of transition. On top of that, the backscatter (energy injected from small scales
to large eddies) is not taken into account. An improved LES model: Wall-Adapting Local Eddy-
viscosity (WALE) is capable to overcome the limitation. In WALE LES, a new operator that
vanishes in the near-wall regions is constructed:
where
denotes the gradient of velocity tensor. Hence the eddy viscosity is expressed
as:
where
is the strain-rate tensor and Δ is the filter width defined as
.
The Smagorinsky model does not include a near-wall correction, therefore, using the WALE
LES model should be preferred.
Detached Eddy Simulation (DES)
DES is a typical hybrid RANS/LES approach proposed to eliminate the main limitation of LES
models, by introducing a hybrid formulation that switches between RANS and LES based on grid
resolution.
In Sparlart-Allmaras (SA) model, the distance to the closest wall
is defined as the length scale.
When SA is employed for RANS part of DES, then a new length scale is proposed as:
where
is a constant taken equal to 0.65,
indicates the maximum edge length of the
local computational cell. As the grid is refined below the limit, the DES-limiter is activated and
switches from RANS to LES mode.
By this formulation, the attached regions like wall boundary layers, are entirely covered by
RANS model and the detached flow portions are resolved in LES mode.
Grid-Induced Separation (GIS): the DES limiter may be activated by grid refinement in the near-wall
regions, as a result, the flow separates at arbitrary locations, namely grid-induced separation.
Due to the limitation GIS, traditional DES method is not recommended.
In order to avoid the limitation of high sensitivity to grid spacing, the DES concept has been
extended to Delayed-DES (DDES) which provides additional shielding functions to ensure that
the model does not switch to LES within the boundary layer. In DDES, the length scale is
redefined as:
the model yields to RANS if
while it reduces to DES with
. The definition of
parameter
reads:
in which
.
Another variation was developed by Shur et al (2008) with the aim of combining both the
capabilities of DDES and Wall-Modeled LES (WMLES) by attempting at resolving the issue of
mismatch between the modeled and resolved log layer which was first identified by Nikitin et al
(2000).
The method was developed in the course of DESider (Haase et al, 2009) and was named as
Improved DDES (IDDES) . In their original paper, Shur et al (2008) claim that IDDES
significantly broadens the application area of (D)DES by permitting the activation of RANS and
LES in different flow regions.
the implementation of IDDES is
Provided that DDES is already available in a solver,
straightforward, as it only requires embedding a new length scale in place of lDDES. This new
length-scale is defined as:
A description of the new functions,
and
is provided in the Theoretical Manual.
B. Best Practice
Categories of Flows
There is no single LES/DES approach to cover all complex turbulent flows with high efficiency.
To select the optimal model, flows are categorized into various types.
It is notable that the proposed classification is not strictly defined and remarkable overlap is
present among the types. Besides, there are a lot of flows not included in any categories or fall
into more than one. In summary, this best practice only gives a general guideline for application.
Globally Unstable Flows
The most common example is the flow past a bluff body. An unsteady output is available even
computed with a classical URANS model.
A list of typical examples in engineering applications are given by:
l Flow past circular cylinder (von Karman vortex street)
l Landing gears of airplanes
l Stalled airfoils
l Tip gap of turbo-machinery blades
Among all flows solved with LES/DES, global unstable flows are the easiest to handle.
Benefiting from strong instability, this type of turbulence can be captured by DDES. Such model
calculates the attached and mildly separated boundary layers in RANS mode, avoiding heavy cost
of resolving near-wall turbulence.
Locally Unstable Flows
In this case, the flow instability producing turbulence is much weaker compared to globally
unstable flows. Representative examples include:
l Backward-facing step flows
l Free shear flows (jets, wakes, mixing layers)
l Flows with weak swirl
For such configuration, DDES is capable to allow LES manner if high-resolution grid is provided
downstream, as the shielding function reduces eddy-viscosity. The spacing should be sufficiently
small to allow resolution of initial flow instability of the separating shear layer(SSL):
denotes RANS length scale and could be approximated with
where
is the thickness of mixing layer.
Due to strong grid sensitivity of DDES model, LES is favored for locally unstable flows.
Meshing Strategy
Without wall functions,
must be achieved to resolve the boundary layer.
For LES, typical cell size near the wall are:
where the x denotes the stream direction, y is the wall-normal direction and z the spanwise.
For DDES, the estimation of lowest mesh resolution in the detached regions is based on the
characteristic length scale D, which is the diameter of bluff body or the diameter of jet in
crossflow. Experience shows that the minimum resolution is of the order:
For all LES/DES models, low aspect ratio, high orthogonality, low skewness and low stretching
are desirable properties. Away from the solid walls, cubic cells are the preferred option.
LES/DES mesh is intrinsically a 3D mesh.
Configuration of time-Step
LES/ DES computations are inherently unsteady and essentially aim at resolving structures. The
unsteady mode should thus be selected and the choice of the physical time-step is of paramount
importance.
The choice of the time-step is dictated by the following considerations:
l In the areas of interest (i.e. where turbulence structures are present), the time-step is selected
such that
. This is a quantity that can be visualized in CFView™.
l If information on periodic phenomena (e.g. vortex shedding) is available from experiment and/
or theory, the time-step should be small enough to adequately capture the periodicity.
l In the case time-sampling is required to build up spectra, the time-step should be small enough
so that the highest frequency is captured.
l Other criteria that may be dictated by physical considerations belonging to the particular case
considered.
The time-step is thus chosen so that it matches all the requirements described here above.
Discretization scheme for convective fluxes
An important aspect which concerns LES, and LES-zones in hybrid RANS/ LES approaches, is
the possible interference of the numerical errors which can be of the same order as the sub-grid
stresses produced by the model. It is recommended to use the Variable Averaging form for the
convective terms to allow the reduction of the aliasing error as much as possible. This is achieved
by setting the Advanced local parameter iFluxAverage_ to 0 under the Computation Control /
Control Variables page.
Initial and Boundary Conditions
Initialization
It is strongly recommended to initialize the LES/DES computation using a converged RANS
solution, especially for hybrid DES that based on an underlying RANS model.
Boundary Conditions
Inlet Conditions
Inlet conditions should be configured according to flow physics or experimental data, in a similar
manner as RANS computations.
Outlet Conditions
Outlet Mass-flow or Averaged Pressure is more desirable than constant pressure, as turbulent
vortices carry variable pressure distributions across the boundary.
Setting Up the Numerical Dissipation
The default values of parameters controlling the numerical dissipation are only suitable for RANS
computations and lead to much too dissipative schemes in the frame work of LES/DES, thus
damping unnecessarily the turbulence structures.
The 2nd-order Central Scheme should be employed. A list of recommended values for artificial
dissipation are provided in the following table.
Flow Regime
β*
spc_artDiss2ndCoef_
(advanced parameter)
spc_artDiss2ndCoefDES_
(advanced parameter)
Incompressible and
low Mach
30
Compressible
n.a.
0.01~0.025
0.01~0.025
The Multi- grid functionality can be activated on the Numerical Parameters / General
Parameters. At each physical time-step, the multi-grid should perform 100 iterations and this
must be enforced by setting the Maximum number of inner iterations to 100 while configuring
the Convergence criteria low enough so that it will never be reached.
Good practice is to deactivate the residual smoothing by setting the advanced parameter tm_
iResSmoothing_ =0 and give the numerical CFL number to 2 at maximum. Another option is to
activate the CPUBooster, in this case, 10 to 15 inner iterations have to be enforced to guarantee
convergence.
Post-processing
Visualization
One typical approach of visualizing turbulence structures in LES/DES is an iso-surface of the Q
Invariant. The definition of Q is given by:
where S is the absolute value of the strain rate and Ω the absolute value of Vorticity:
Another popular criterion of vortices is Lambda-2 (
), which is defined as the second largest
eigenvalue of
.
Other flow variables can be visualized on the iso-surface of Q-invariant or Lambda 2. Quantities
), or a velocity component not present in RANS, or
of interest are the eddy-viscosity ratio (
CFL number.
121
FINE™/Open with OpenLabs™ 7.2 User Guide
Averaging
LES/ DES is intrinsically unsteady, while usually only time- mean results are of value for
industrial applications, so averaging is required. Restarting from an RANS solution, the settlement
of the flow into new state takes a while for:
l The development and transportation of the turbulence.
l Adaption of flow from initial solution.
l Start-up of multi-physics effects.
Such transition time significantly depends on the flow physics and only rough general guideline
, where L is the length of flow
can be given: estimate with through-flow duration
domain and U ∞the mean-flow velocity. Typically 3~5
turbulence.
is required for the development of
In FINE™/Open, the averaging is configured in Control Variable/General/Output files, where
users can activate the Time averaged solution and set the time step from which the averaging
starts.
4.1.7
Gravity Forces
When gravity should be taken into account, the box marked Gravity Forces (FIGURE 4.1)
should be checked. If gravity is activated by checking this box, two inputs are required from the
user:
l The gravity vector
, which will, in general, be set equal to the gravity on earth.
l The reference altitude
at which a reference pressure is specified to add the hydrostatic
pressure in the initial pressure field. Note that the reference pressure is the reference value in
the Fluid Model page.
When the gravity is taken into account in the Navier-Stokes equations, the source terms
and
respectively are introduced in the momentum and energy conservation equations where
ρ is the density,
the gravity vector and
the velocity vector.
If the fluid is a liquid, the density is constant and there is no influence on the pressure or
temperature of the flow by interaction with gravity. To simulate these interactions, one can use the
Boussinesq approximation in the gravity source terms. With this approximation, the density is
developed in the first order of the Mac Laurin series. It becomes:
with α the compressibility and β the dilatation coefficients specified in the fluid properties (refer to
Fluid Model chapter).
This variation of
the density is only applied to the gravity source term (Boussinesq
approximation). Otherwise, the density is kept constant in the conservation equations. The value
are the
of
is the characteristic density specified in the Fluid Model page.
and
reference values in the Fluid Model page.
4.1.8
Heat Source
When heat source is taken into account, a specific volumetric heat source term
[W/m³] is
introduced in the energy conservation equation. The heat source term is acting in an user-defined
volume (sphere, brick or cylinder) or in the entire domain. Consequently, the specific volumetric
heat source term
is evaluated as follows:
where ϕ (W) is the user-defined heat flux and
is the sum of the volume of the cells
contained in the given shape.
When the volumetric heat source term dominates the other terms in the energy equation, the user may
encounter difficulties in converging to steady state.
The heat source term can be accessed through the Physical configuration / Heat Source page.
The user can activate the heat source terms for the selected blocks by clicking the option Activate
heat source(s).
FIGURE 4.3
Heat source parameters
If the option Global heat source is chosen, the entire domain is considered as a source. In this
case, no additional local heat source can be defined.
If the option Local heat source(s) is chosen, the user can Add, Remove a source and Edit the
is activated in cells
shape and parameters of the source. The specific heat source term
which are located inside the given volume. Let (xcell, ycell, zcell) the coordinates of the center of a
given cell. The source term is activated in this cell if the following conditions are fulfilled:
Note that
may be not equal to the volume of the user-defined shape, because a cell belongs to a
given shape only if its center belongs to the given shape.
FIGURE 4.4
The Editor dialog of Local Heat Source
l Sphere: Center coordinates and radius are specified. For a sphere, only one condition is
required:
where (xspherecenter, yspherecenter, zspherecenter) is the center's coordinates of the sphere and
rsphere is the radius of the sphere.
l Brick: First corner and opposite corner are specified. For a brick, three conditions are required:
where the min and max quantities are computed as follow:
l Cylinder: Center coordinates of the basis, direction axis, radius and height are specified. The
axis of the cylinder can be only the x, y or z axis. For a cylinder, two conditions are required.
For example, if the direction of the cylinder is z, one has:
where
,
. (xorigin, yorigin, zorigin) is the original
center's coordinates of the cylinder and rcylinder is the radius of the cylinder.
The heat flux value for the heat source term is specified in Watt. In steady computation, this value
is constant. In the case of unsteady computation, the heat flux value can be defined by a profile
depending on the time.
4.2
CHARACTERISTIC VALUES - REYNOLDS
NUMBER
The user must specify some characteristic values (length and velocity). These values are used to
calculate the Reynolds Number that provides useful information to choose the suitable model.
Furthermore the characteristic length can be used for other purposes as well in the outlet boundary
condition for which the mass flow is imposed with pressure adaptation.
CHAPTER 5.
SOLID MODEL
The conjugate heat transfer model allows the simulation of the thermal coupling between a fluid flow
the simultaneous calculation of the flow and temperature
and the surrounding solid bodies,
distribution within the solid bodies.
i.e.
The current version of the model assumes that some of the blocks of the multiblock mesh are "solid",
whereas the other ones are "fluid". The connections between the solid and fluid blocks become
"thermal connections" along which the fluid-solid coupling is performed.
The FINE™/Open solver can calculate the temperature distributions in solid bodies meshed with tetrahedra,
hexahedra, pyramids, prism or a mix of them, which gives users the ability to import and run ANSYS meshes
for solid bodies, simultaneously with HEXPRESS™ meshes for fluid bodies with a FNMB connection
between them. For more details on mesh generation, the user can refer to the HEXPRESS™ user manual.
The default solid solver (iSolidImpl_=3) is not compatible with the option Allow multiple domains per
process for parallel computations.
In this section
5.1 Solid Model Interface
5.2 Advanced Parameters for Solid Model
5.3 Best Practice for Conjugate Heat Transfer
127
FINE™/Open with OpenLabs™ 7.2 User Guide
128
5.1
SOLID MODEL INTERFACE
The Conjugate Heat Transfer model can be directly activated from the FINE™/Open GUI under
the General parameterspage. The figure below shows how the General parameters page looks
like. All blocks (domain) in the mesh are listed on the left of the page and all of them are by
default set as Fluid block. The user can activate solid model in some blocks by selecting them on
the left part of the window and by pressing the ratio button Solid block.
For each solid block imposed by the user in the General parameters page,
the thermal
conductivity has to be specified (in W/m.K) in the Solid Model page. The thermal conductivity
may be a constant or defined by a temperature profile (for the format, see Solid Properties
section).
5.2
ADVANCED PARAMETERS FOR SOLID
MODEL
All non-interfaced advanced parameters related to the solid model are accessible on the Control
Variables page, in the Advanced sub-menu.
For all solid solvers
iSolidImpl_: Select the method solving the energy equation in solid blocks.
0: use the explicit Runge-Kutta time integration method. This is an explicit method. In general, the
suggested CFL number is 1. In case of difficulty of convergence, the CFL number should be
reduced (e.g. 0.1).
1: use the classical implicit Gauss-Seidel method. When using this method, the value in all solid
blocks should be set to 1. This implicit method is unconditionally stable in theory. While
experience shows that the GS method is sensitive to the mesh resolution. If the mesh used in the
computation presents some refinements (e.g. viscous layers) or is not uniformly cartesian, then the
convergence of the GS method can become extremely poor and in some cases, the computation
can even diverge.
3 (default): use the Conjugate Gradient (CG) method (Saad, 2003). This method is less sensitive
to the mesh resolution, and is unconditionally stable. When iSolidImpl_=3, the flow solver sets
solidImpl_gamma_ to 1 automatically.
solidImpl_gamma_: Control the level of implicitness of the time-marching scheme. Only apply
to iSolidImpl_=0/1.
0: leading to a purely explicit scheme;
1: leading to a purely implicit scheme (first order Euler method);
0.5 (default): leading to a blended scheme (second-order Cranck-Nicholson method).
solidImpl_omSOR_: Over-relaxation parameter, varies between 0 and 2.
For the CG solver (iSolidImpl_=3)
solidImpl_KSPCFLStart_: a ramp of the CFL is applied at the beginning of the computation to
increase the robustness of the computation. At the beginning of the computation, the CFL applied
is solidImpl_KSPCFLStart_. The CFL is then increased to the value specified in the GUI during
the iterations defined by solidImpl_KSPniterCFL_.
solidImpl_KSPniterCFL_: number of iterations to apply the ramp of the CFL, see solidImpl_
KSPCFLStart_ for more details.
solidImpl_KSPMaxIter_: maximum number of inner iterations for the CG method.
solidImpl_ KSPRelTol_ : relative tolerance applied for the convergence criterion of the CG
method.
solidImpl_KSPAbsTol_: absolute tolerance applied for the convergence criterion of the CG
method.
solidImpl_KSPDivTol_: divergence tolerance applied in the inner iterations for the CG method.
solidImpl_KSPPrecondType_: type of preconditioner applied:
1 (default): Matrix Diagonal scaling preconditioner (available if solidImpl_KSPSolverType_=1)
solidImpl_KSPSolverType_: type of the solver applied:
1(default): Conjugate Gradient.
solidImpl_ KSPComputeOnGrid_ : applied from the finest to the coarsest multigrid in solid
blocks. The first number corresponds to the finest grid level. By default, the parameter is set to 1 0
0 0, which means that the heat equation will be solved only on the finest grid level of the finest
grid.
0: Do not solve the heat equation on the current multigrid.
1: Solve the heat equation on the finest grid level of the current multigrid.
2: Solve the heat equation on each grid level of the current multigrid.
5.3
BEST PRACTICE FOR CONJUGATE HEAT
TRANSFER
This section presents how to set up a project involving the Conjugate Heat Transfer model under
the FINE™/Open user environment. The only action required from the user to set up a
computation involving the Conjugate Heat Transfer model can be decomposed in three steps:
1. Determine the Solid and Fluid Blocks,
2. Set the Global Parameters,
3. Define the thermal connections.
Those steps are described in the following paragraphs in more details.
5.3.1
Step 1: Determine the Solid and Fluid Blocks
The use of the Conjugate Heat Transfer model requires the generation of a multi-block mesh, the
Solid block and Fluid block parts of the domain being discretised with separate blocks. The
good mesh quality at the interface is essential for the accuracy of the results (cells need to be as
much as possible orthogonal to the solid walls for a better convergence of the solver). When
generating the mesh, the user should follow the guidelines in Generate an appropriate grid.
Once the mesh is generated, the first step consists in pointing the Solid block and Fluid block
within the FINE™/Open GUI. In the default configuration of the solver, all blocks are set as the
type Fluid block, so that the Solid Model page does not need to be entered for a classical flow
calculation. The transfer of some of the blocks from fluid to solid is performed by selecting those
blocks on the left part of the window and by pressing the button Solid block.
5.3.2
Step 2: Setting the Global Parameters
For each solid block the thermal conductivity has to be specified (in W/m/K) in the Solid Model
page.
Furthermore, the CFL number used for the time integration of the conduction equation has to be
specified in the Numerical Schemes page (default value 3).
the same CFL number as used for the fluid blocks is
When iSolidImpl_ =3 (default),
recommended for the solid blocks. The user may increase the CFL number (e.g. 100) in the solid
blocks to accelerate the convergence but it will require more CPU time because more inner
iterations are required for solid blocks.
When iSolidImpl_= 0 or 1, the recommended CFL number is 1 for solid blocks. If convergence is
difficult, the CFL number should be decreased (e.g. 0.1).
5.3.3
Step 3: Setting the Thermal Connections
The thermal connection between blocks is a full non-matching connection (refer to full non
matching connections for more details).
Once some blocks of the multi-block mesh are pointed as solid blocks, the connections between
solid/solid and solid/fluid blocks become thermal connections. These connections are solid wall
boundary conditions with a particular thermal condition, along which the heat flux is iteratively
iterated in order to ensure a correct coupling.
These patches appear in the list of patches under the tab Solid on the Boundary Conditions
page. Although the thermal aspect is fully controlled by the coupling procedure, the following
boundary conditions must be imposed by the user:
l the thermal wall boundary condition. In case that the patches are not fully connected, the
remaining part of the patch will use the boundary condition defined through the FINE™/Open
GUI.
l the kinematic wall boundary condition (translation or rotation speed).
CHAPTER 6.
BOUNDARY CONDITIONS
During the mesh generation process, the user must define the type of boundary condition to be imposed
along all boundaries. The parameters associated with these boundary condition types can be fully
defined using the Boundary Conditions page.
If the patches are defined with the same names in HEXPRESS™, the FINE/Open™ GUI will automatically
add 3 indexes in the patch names to distinguish them: B(Block), F(Face) and P(Patch). For example, Inlet-
(B1_F1_P4), where Inlet is the original name, B1, F1 and P4 is the added indexes.
This chapter gives a description of the boundary conditions available on the Boundary Conditions
page. In Boundary Conditions in FINE/Open™ section theBoundary Conditions page is described.
In Best Practice for Imposing Boundary Conditions section advice is provided on the combinations
of boundary conditions to use. For more detailed information, see the theoretical manual.
In this section
6.1 Boundary Conditions in FINE™/Open with OpenLabs™
6.2 Best Practice for Imposing Boundary Conditions
134
149
6.1
BOUNDARY CONDITIONS IN FINE™/OPEN
WITH OPENLABS™
When selecting the Boundary Conditions page the parameters window appears as shown in
FIGURE 6.1. Four tabs are accessible, depending on the boundary condition types defined in the
mesh. There are currently four types of boundary conditions available in the FINE™/Open GUI:
l inlet,
l outlet,
l solid walls,
l external (far-field).
Each of these is described in the next sections.
The mirror boundary conditions (MIR), periodic boundary conditions (PER), periodic non matching
boundary conditions (PERNM) and non matching boundary conditions (NMB) are supported by the
flow solver but don't appear in the interface. The user doesn't need to set any parameters for these
boundary conditions.
Translational PER boundary conditions are not supported.
A common particularity of the four Boundary Conditions pages is their subdivision into two
areas. The left area always contains a list of the different patches that are of the selected boundary
condition type. A patch can be identified by the name of the block face to which it belongs. The
right area is where the boundary condition parameters are specified for the selected patch(es).
FIGURE 6.1
Boundary Conditions page
The option Viewing is used to highlight the seleted patch as Shade or Outline in the Graphics
Area window. If None is selected, nothing will be highlighted.
One or several patches may be selected in the left area by simply clicking on them. Clicking on a
patch deselects the currently selected patch(es). It is possible to select several patches located one
after another in the list by clicking on the first one and holding the left mouse button while
selecting the next. To select a group of patches that are not located one after another in the list, the
user should click on each of them while simultaneously holding down the <Ctrl> key. It is also
possible to select one or several patches by using the Filter string. To select the boundaries, type
full or fraction of the name of the boundaries need to be filtered and press <Enter>.
Several patches can be grouped by selecting them and clicking on the Group button. A name
entry box will appear asking for a group name. The name of the group will appear in red in the
list of patches to indicate that this is a group of patches. Each change to the parameters, when a
group is selected, applies to all patches in that group. The Ungroup button removes the group and
its patches are displayed individually in the list.
The Ungroup button is active only when at least one group is selected.
Clicking with the left mouse button on the plus sign
the patches included in this group.
left of a group name in the list will display
these names will appear in
If some of the patches have been given names in HEXPRESS™,
FINE™/Open with OpenLabs™. If the patches have been grouped in HEXPRESS™, by giving the
same name to many patches, they will appear ungrouped in FINE™/Open with OpenLabs™ to avoid
contradiction between grouping in HEXPRESS™ and FINE™/Open with OpenLabs™.
If the user selects several patches that have different parameters, a warning dialog box will appear.
When clicking on OK all parameters will be set equal to the ones of the first patch. Selecting
Cancel instead will cancel the selection
FIGURE 6.2
Few patches have been grouped into a group called WING.
The right area of all the boundary condition tabs is created in a generic way by means of a
resource file, where all the boundary condition parameters are described altogether with their
default values.
Some boundary conditions are only available for an incompressible or compressible flow.
FINE™/Open with OpenLabs™ will automatically disable the boundary conditions that are not
available, depending on the type of fluid selected in the Fluid Model page. Also the type of
boundary conditions are adjusted according to the selection for Cartesian or Cylindrical boundary
conditions.
6.1.1
Inlet Condition
Available Inlet Boundary Condition Types
The inlet boundary condition page is customized according to the configuration of the project
(Cartesian or Cylindrical) as shown in the following two figures. The user has the freedom to
access both types of configurations in the boundary conditions page independently of the mesh
properties.
The upper part of the inlet boundary condition page allows the user to select the type of inlet
condition to apply to the selected patches through a series of toggle buttons. There are two
categories of inlet conditions: conditions applicable to subsonic inlets and conditions applicable to
supersonic inlets.
Note that to determine whether an inlet (or an outlet) boundary is subsonic or supersonic, the velocity
component normal to the boundary should be considered.
FIGURE 6.3
Inlet boundary conditions page for Cartesian problems.
FIGURE 6.4
Inlet boundary conditions page for Cylindrical problems.
For each inlet condition type, the lower part of the page is adapted to provide input boxes only for
the physical variables that are required to fully determine the selected boundary condition. These
variables are for instance: the pressure and temperature (static or total), the velocity components,
the velocity magnitude, the velocity angles (specified in radians), or the mass flow. In case of a
simulation involving a turbulence model, the inlet values of the turbulence variables are also
required. Please refer to Defining Initial and Boundary Conditions section for more information
on setting the boundary condition of the turbulence variables.
For the inlet boundary conditions:
l The velocity components are defined in the Cartesian or cylindrical coordinate system,
depending on the selected type.
l The required pressure and the temperature values can be the static or the total values.
Four major types of inlet boundary conditions can be identified:
l velocity components and the static temperature,
l total pressure, total temperature and the flow angles,
l Total enthalpy, dryness fraction and the flow angles (only for condensable fluid)
l mass flow, the static temperature and the flow angles (related patches must be grouped).
When using a mirror periodicity, the mass flow specified in the interface equals the mass flow
through only half of the inlet. When using a rotational periodicity, the mass flow specified in the
interface equals the mass flow through the whole inlet (360 degrees).
Imposing Variables as an Interpolation Profile
Each variable can be defined as a constant or as an interpolated profile of the variable. The
imposed boundary condition may be variable in space. Time dependent profile is currently not
supported by the FINE™/Open solver.
To select profile data, rather than the default "Constant Value" click on the down arrow alongside
the relevant input box and select "fct(space)".
A button ( ) will appear to the right of the input box, which down contains the phase "profile
data". To visualize and/or edit the profile data press this button, which opens the Profile
Manager with the existing profile. See Profile Manager section for a detailed description of the
Profile Manager. It allows the user to modify or create a data profile interactively. Click on the
Ok button to set the new profile for the selected patch(es).
FIGURE 6.5
The Profile Manager
If a quantity is defined as a function without the definition of a valid profile a warning message will
appear when saving the project. In such a case a default constant value is used in the computation.
6.1.2
Outlet Condition
The outlet boundary condition page is customized according to the configuration of the project
(Cartesian or cylindrical). The user has the freedom to access both types of configurations in the
boundary conditions page independently of the mesh properties.
For a supersonic outlet all variables are extrapolated. An outlet is considered as supersonic by the
velocity normal to the boundary.
Three types of subsonic outlet boundary condition are available, as shown in FIGURE 6.6. These
different boundary conditions are described in the following paragraphs.
An option for treatment of backflow ( Backflow Control) can be activated. The purpose of this
option is to prevent the flow to re-enter in the domain by applying a slip wall boundary condition
locally to the velocity.
FIGURE 6.6
Outlet boundary conditions page.
Pressure Imposed
There are three different methods to impose the pressure at the outlet:
l Static Pressure Imposed :
the static pressure is imposed on the boundary,
the static
temperature and the absolute velocity components are extrapolated. As described for the inlet
conditions, the static pressure can be constant or defined as a data profile. To define a profile
as a function of space click on the profile button to the right of the input text box. The Profile
Manager will appear.
l Radial Equilibrium: This boundary condition is applicable only to cylindrical problems. The
outlet static pressure is imposed on the given radius and integration of the radial equilibrium
law along the spanwise direction allows calculation of the associated profile of the static
pressure. A constant static pressure is imposed along the circumferential direction.
Please note that the given radius should be between hub and shroud. Otherwise, the outlet static
pressure will be imposed on the corresponding extreme radius of the outlet instead of the given
radius.
l Average Static Pressure Imposed: if imposing a uniform static pressure at the outlet is not an
appropriate approximation of the physical pressure distribution at the outlet, an averaged static
pressure may be used. In this case, only an averaged value for the static pressure is imposed
while the pressure profile (around this average) is extrapolated from the interior field.
Mass Flow Imposed
When imposing the mass flow at the outlet the related patches must be grouped. This allows there
to be several groups of patches, each of which constitutes an outlet through which the mass flow
can be controlled.
The mass flow boundary condition cannot be applied to a group which patches come from different
blocks.
When using a mirror periodicity, the mass flow specified in the interface equals the mass flow
through only half of the inlet. When using a rotational periodicity, the mass flow specified in the
interface equals the mass flow through the whole inlet (360 degrees).
Two different techniques are available to impose the mass flow:
l Velocity Scaling: the pressure is extrapolated and the velocity vector is scaled to respect the
mass flow. This technique is only valid for subsonic flows and is not recommended in case of
significant back flows along the exit boundary.
l Pressure Adaptation: this boundary condition is identical to the "Uniform outlet pressure" or
"Radial equilibrium" (if the option Radial Equilibrium is activated) boundary conditions,
except the fact that the exit pressure is automatically modified during the resolution process so
that after convergence, the prescribed mass flow is obtained. When this boundary condition is
the user has to specified the reference temperature through the expert parameter
used,
TRefBCpAdapt_, see more information in the theoretical manual.
Additionally, the initial pressure which is used to create the initial solution, should be defined by
the user. The option Constant Pressure During FMG Initialization uses a uniform static
pressure outlet condition during the full-multigrid initialization process. For robustness reasons, it
is activated by default.
6.1.3
Solid Wall Boundary Condition
The solid wall boundary condition page is customized according to the type of calculation
(inviscid or viscous).
For Euler cases (i.e. inviscid), no parameter is requested for the wall boundary conditions. For
Navier-Stokes cases, the upper box enables the user to choose the required thermal conditions and
the lower box the associated velocity conditions.
On the SOLID page, FINE™ will group automatically the patches of a same FNMB connections
in order to reduce the list of solid patches displayed. The group name will be the FNMB
connection name. In particular cases, the user can still ungroup them when different settings must
be applied to these patches.
If the project includes AutoGrid5™ meshes converted into HEXPRESS™ format (from v211-1),
FINE™ will group automatically the patches related to turbomachinery elements (Hub, Shroud
and Blade). The grouping is based on the patch names generated by AutoGrid5™. The
connection types PER/PERNM/NMB existing in AutoGrid5™ will be converted into FNMB in
HEXPRESS™. All FNMB connections will also be grouped automatically for each row.
Cartesian Boundary Conditions
The user can define a translation or a rotation velocity vector. In the latter case, the coordinates of
the rotation centre are required. Four options are available for the thermal condition: adiabatic,
constant heat flux (in W/m²), isothermal or constant heat transfer coefficient (in W/m²K). The
imposed heat flux or temperature can be constant on the patch or defined as a profile. Use the pull
down menu to change Constant Value to Fct(space). Click on the profile button to launch the
Profile Manager
FIGURE 6.7
Solid boundary conditions page in case of a Cartesian boundary condition
Cylindrical Boundary Condition
The wall rotation velocity can be constant or area defined . The area defined
option allows the user to attribute a specific rotation velocity to a rectangular zone in the
meridional plane independently of the grid structure. When the area defined option is selected, a
small picture defining the parameters is displayed (the z axis is the rotation axis, the r axis is the
radial axis). The rotation velocity is set to
outside the domain and to
inside the domain.
FIGURE 6.8
Solid boundary conditions page in case of a cylindrical boundary condition
The specified range must be a valid range for the geometry. For example, for an axial machine the
limits for rotation of the hub can be defined by setting the lower and higher axial limit to
appropriate values. In such a case it is important to set the radial limits such that they include the
full solid (hub) patch.
The thermal conditions are similar to those for Cartesian flows (more details in previous section).
Euler or Navier-Stokes Wall for Viscous Flow
If the flow type is selected as laminar or turbulent Navier-Stokes, it is possible to choose between
an Euler wall (zero normal velocity) and a Navier-Stokes wall (no-slip condition). Further details
on the numerical treatment of walls are provided in the theoretical manual: Solid Wall Boundary
Conditions. Note that the default is a Navier-Stokes wall.
Force and Torque
At the bottom of the right page, a "Compute force and torque" button is provided that allows
the user to include the selected patches in the calculation of the global solid boundary
characteristics.
In the case of external flows  the force and torque
are computed as:
l the lift,
l the drag,
l the moment.
The direction of the forces, as well as the reference axis and the location of the point for the
moment are determined in the Computation Control / Outputs page.
In the case of internal flows, the axial thrust and torque at (0,0,0) are computed.
Properties of Solid for Turbulence
In addition, when turbulence models with extended wall function are used, the user has to specify
the type of wall ("Smooth" or "Rough") and the following constants: the Von Karman constant
κ and the Bo constant. If the wall type is rough, the equivalent roughness height k0 and the height
of the zero displacement plane d0 are also required. A description of these constants is provided in
the theoretical manual.
Two methods considering the wall function for roughness is implemented. With the old method
(default, turb_iRoughModel_=0), the constant Bo has to be computed according to the value of
y+. And the value of Bo will also correct y+. The user has to iterate this procedure and converge to
the desired value of Bo. This is not straightforward and a new approach has been introduced in
the flow solver in order to simplify the computations with roughness. To use the new method, the
user has to set the expert parameter turb_iRoughModel_ to 1.
For rough walls, the following limitations are applied:
l the distance from the wall to the cell-centre of the first inner cell should be bigger than k0 + d0.
l the first inner cell should be located within the fully turbulent layer.
The application field of the "law of the wall" imposes restrictions on the grid. The user is strongly
advised to check the conformity of this grid with these conditions (Mathematical Model section).
6.1.4
External Condition (Far-field)
The external boundary condition is provided to treat far-field boundaries when dealing with
external flow computations. An example is given in FIGURE 6.9 . This type of boundary
condition determines whether the flow is locally entering or leaving the flow domain and uses the
theory of Riemann invariants to correctly treat the appropriate variables. Depending on the chosen
turbulence model, five or seven input boxes are provided to specify the free-stream values of the
variables to be used in the boundary condition formulation.
For the external boundary condition, the user can impose the components of the velocity directly,
or impose the Mach number together with the velocity angle.
A negative Mach number can be imposed, relative to the imposed velocity angle.
FIGURE 6.9
External (far-field) boundary conditions page.
Use an external condition rather than an inlet condition for cases for which it is not known whether
the flow enters or leaves the domain.
The external boundary should be far away from the body so that the Riemann boundary condition is
satisfied.
It is not recommended to use an external condition on flat surfaces.
6.1.5
Advanced Parameters for the Boundary Condition
Non-Interfaced Advanced Parameters
iFnmb_treatment: The purpose of this treatment is to avoid the appearance of spurious pressure
spots along curved FNMB connections where the mesh densities on both sides of the interface are
different.
0 (default): the default treatment of the FNMB connections;
1: the improved treatment of the FNMB connections. The fluxes on each faces are computed
using the different normal vectors on both sides instead of using the identical common normal
vector.
iGhostCylindExtrapol_: Control the approach of computing dummy cell coordinates:
0 (default): the old treatment;
1: the coordinates of dummy cells are computed using cylindrical extrapolation.
bc_treatThermoOnFace_: Control where the thermodynamic and state laws are applied when
applying the boundary conditions:
0: apply thermodynamic and state laws in boundary dummy cells;
1 (default): apply thermodynamic and state laws at boundary.
bc_wallCondensableFluid_: Control the type of relation used to compute the density at the wall
in case of condensable fluids.
0 (default): Relation used in versions older than FINE™/Open v5.2;
1: Relation used for iCavitation_ = 2 and iCavTablesNEWALGO_ = 1.
out_forceTorqueAreaDefined_: If the solid patches are defined by using Area Defined Rotation
Speed, the force and torque can be computed only on the central part of the patches with Area
Defined Rotation Speed:
0 (default): the force and torque are computed on the full patch(es).
1: the force and torque are computed only on the central part of the patch(es) with Area Defined
Rotation Speed.
The rotation speed of the central part of the patches with Area Defined Rotation Speed must
be not equal to 0.
out_displayForcePatchOfGroup_: The information of the force and torque is available in the
".wall" file. The expert parameter out_displayForcePatchOfGroup_ is used to control the output
in ".wall" file.
0 (default): the force and torque are given only for the solid boundary groups/ patches.
1: the force and torque are given not only for the solid boundary groups/ patches, but also for each
patch in the solid boundary groups.
6.2
BEST PRACTICE FOR IMPOSING
BOUNDARY CONDITIONS
The quality of the flow simulation rests primarily on the quality of the grid and the imposed
boundary conditions. In this section the most appropriate boundary conditions are proposed
depending on the type of studied flow.
In case of divergence in calculations it is strongly recommended to check, by post processing of the
solution (in CFView™), that appropriate boundary conditions have been imposed.
Compressible Flows
For compressible internal flows it is recommended that the inlet boundary condition fixes either
the static quantities or the absolute total quantities (pressure, temperature) plus the flow angles,
and that the outlet boundary condition fixes the static pressure (exit pressure). This exit pressure
can be imposed as:
l a constant value along the exit,
l an average value at the exit,
l the pressure at mid-span for radial equilibrium (only for an axial outlet).
The static pressure at the exit of the domain is rarely constant. It is thus advised to impose the
pressure as an average value or as initialization data for radial equilibrium.
Even if this value of pressure is known, for numerical reasons it is possible that the computed
mass- flow differs from the expected one. It is thus necessary to modify the exit pressure
repeatedly until obtaining an accurate mass-flow. This procedure can be numerically expensive
especially if the calculations are carried out on a fine grid.
A solution to overcome this drawback is to impose the mass-flow at the outlet. This can be
accomplished by " Pressure Adaptation ": in this case, an automatic procedure introduces a
variation of the imposed exit pressure at each iteration of the calculation. The pressure is then
iteratively updated in order to reach the imposed mass-flow at convergence. This is however not
as robust as imposing the exit pressure, although it is more robust than a " Velocity Scaling"
option.
For external flows, the use of the external boundary condition is recommended.
Incompressible or Low Speed Flow
For incompressible or low speed internal flows it is recommended to impose the mass-flow and
the static temperature at the inlet and a static pressure at the exit. This combination of inlet-outlet
conditions has a stabilizing effect on the calculation.
For external flows, the use of the external boundary condition is recommended.
CHAPTER 7.
NUMERICAL MODEL
This chapter describes the interface and settings that can be used to specify the numerical parameters
and the time configuration for the simulations:
l Numerical Model defines the numerical aspects of the computations,
l Time Configuration defines the time dependence of the equations to solve.
In this section
7.1 Numerical Model
7.2 Time Configuration
152
168
7.1
NUMERICAL MODEL
The Numerical Parameters / General Parameters and Numerical Parameters / Numerical
Schemes pages allow the user to define the numerical aspects of the computation:
l the CPU Booster
l the multigrid parameters,
l the spatial discretization,
l the CFL number,
l preconditioning parameters (if applicable).
These parameters are described in the next section.
FIGURE 7.1
General tab of the general parameters page
Explicit time stepping is available through Temporal discretization parameters. This function
is still at Beta version.
In the Advanced tab of the General Parameters page, additional parameters are available as
shown in FIGURE 7.2: additional multigrid parameters and unsteady parameters.
FIGURE 7.2
Advanced tab of the global parameters page
FIGURE 7.3
Numerical schemes page
7.1.1
Numerical Model in FINE™/Open with OpenLabs™
A. CPU booster
FINE™/Open with OpenLabs™ includes an innovative breakthrough in convergence
acceleration. Based on enhanced implicitness, it leads to a drastic reduction in computational time
with respect to the current advanced technologies in FINE™/Open with OpenLabs™. The user
can activate the option CPU Booster in the Numerical Parameters/General Parameters page.
Then, the default CFL number in the Numerical Parameters/Numerical Schemes page will be
set to 100.
The option CPU Booster is a general parameter. If CPU Booster is switched on, this option will
be activated for all blocks. The applied CFL number can be selected for every block
independently. If one parameter of a block is not compatible with this option, the CPU Booster
cannot be activated.
For the compatibility of the CPU Booster, please refer to the Compatibility Matrix.
B. Multigrid
The multigrid method is used to accelerate convergence. The Multigrid strategy is an important
feature of the FINE™/Open flow solver, which enables convergence acceleration at
low
computational and memory overheads compared to the explicit Runge-Kutta scheme.
In the Global Parameters page under the tab General, the Number of grid levels used by the
multigrid strategy can be specified in the Multigrid parameters frame.
In the Global Parameters page under the tab Advanced, an additional input box permits to
select the number of sweeps to be performed on each grid level through the input box Number of
sweeps on successive grid levels. The amount of sweeps is the number of times the Runge-Kutta
operator is applied . In the default configuration of the
solver, a linear progression is used, the number of sweeps on each level equals the level number
(2 sweeps on the second level,...). It has been observed in many cases that the convergence rate
may be significantly improved by performing a higher number of sweeps on the coarsest levels,
for instance (1,2,16) in case of 3 grid levels. However, it should be noted that more sweeps have
as a consequence more time required for an iteration.
Multigrid Strategy: Agglomeration
Notice that since the FINE™/Open solver deals with unstructured meshes, the generation of
coarse multigrid levels is significantly different from structured meshes, where one point in two is
removed in each direction to create a coarse grid. In the current framework, the agglomeration
technique is used by default. This technique is used to recover coarsening ratios close to 1/8 (1/4
in 2D) between successive multigrid levels. The agglomeration strategy developed in
FINE™/Open with OpenLabs™ is inspired by the "greedy"-type frontal algorithm developed by
Mavriplis and Venkatakrishnan (1995) for mixed element meshes. It has, however, been
significantly modified, in order to take into account the mesh and topological configurations
generated by HEXPRESS™.
It is recommended not to select more than 4 grid levels for the multigrid strategy (default =4).
FIGURE 7.4
Agglomeration strategy on F16
Correction Damping
During the multigrid process, interpolations are performed from coarser grid to finer grid. They
can lead to high discontinuities between iterations and produce numerical instabilities. To avoid
those instabilities, the Correction damping when activated smooths the interpolation results to
remove high discontinuities and thus ensure multigrid robustness.
Coarse Grid Initialization
The option Coarse Grid Initialization enables, before calculating the flow on the mesh, to
perform a preliminary flow calculation on a coarser mesh automatically created by the flow solver
by coarsening the initial one. This provides a rapid estimation of the flow. This technique is
referred to Full Multigrid.
If the option Coarse Grid Initialization is activated, the computation starts on the coarsest grid
level and includes a finer grid level each time if one of the two following criteria is satisfied:
l The maximum number of cycles to be performed on each grid level is reached. This parameter
is specified through the input box in the Coarse grid initialization parameters area under the
Advanced tab as the Maximum number of cycles per grid level.
l The residual on the current grid level has dropped a certain order of magnitude as indicated by
the Convergence criteria on each grid level in the Coarse grid initialization parameters
area.
The applied CFL number on the coarser grid levels can be specified per block in the Numerical
Parameters/Numerical Schemes page. This CFL number can be lower or equal to the one
applied on the finest grid level. By default it is equal to 1.
When the CPU Booster is activated in the Global Parameters page under the tab General, the
Advanced tab allows the user to activate or deactivate the CPU Booster during the coarse grid
initialization. By default, the CPU Booster is not active.
C. Numerical Schemes
Spatial Discretization
Three types of spatial discretization are available under the Numerical Schemes page:
l central scheme (default)
l central matrix scheme
l Roe-type upwind scheme (only under a specific license).
The order of accuracy (1st or 2nd) of the schemes can also be specified. This gives the following
possible combinations:
l 1st-order central: pressure switches in the artificial dissipation are activated everywhere so that
this corresponds to the highly dissipative first-order Lax-Friedrichs upwind scheme. This
scheme is very robust and can be used to obtain a first initialization of the solution before
switching to second-order schemes.
l 1st-order central matrix.
l 1st-order Roe upwind: this 1st-order upwind scheme is less dissipative than the Lax-Friedrichs
scheme.
l 2nd-order central scheme (default): the central scheme with scalar artificial dissipation is the
default choice in FINE™/Open with OpenLabs™.
l 2nd-order central matrix scheme: the central matrix scheme with matrix artificial dissipation is
available for incompressible fluids or perfect gas with and without preconditioning. It is less
dissipative than the central scheme.
l 2nd-order Roe upwind: this 2nd-order upwind scheme is available when compressible fluids
are used and CFL is recommended to be set to 1.0.
In case the central matrix scheme is selected, the central scalar scheme will be applied during the
coarse grid initialization by default. This can be changed by adjusting the expert parameter spc_
artMatDissfmg_.
CFL Number
An explicit 4-stage Runge-Kutta scheme is used to march the governing equations in time
towards the steady state solution and the CFL (Courant-Friedrichs-Levy) number can be tuned by
the user to ensure convergence. This number globally scales the time-step sizes used for the time-
marching scheme of the flow solver. A higher value of the CFL number results in a faster
convergence but will lead to divergence if the stability limit is exceeded.
The user can select a different CFL number during coarse grid initialization and can manage the
CFL number for every block independently.
Preconditioning
This box allows the user to choose the Hakimi or Merkle preconditioners. The parameters are
only available when an incompressible fluid is selected on the Fluid Model page or when the
Low Speed Flow (M<0.3) option is activated on the Flow Model page.
The upwind spatial scheme (Numerical Model page) is not available if the preconditioning
option is chosen.
When the option CPU Booster is active, only the Merkle preconditioning is available.
Hakimi preconditioning
When the Hakimi preconditioning is selected,
information is provided in the theoretical manual.
1. β* coefficient.
the following parameters can be set. More
The default value of β * is 3. Based on our experience with the presented low speed
preconditioner the parameter β* can be taken of order unity for inviscid flow computations.
For viscous computations associated with Reynolds numbers greater than about Re=1000, a
constant value β* of order unity is also adequate. If convergence difficulties are encountered at
the very beginning of a computation, it is recommended to increase the value of the parameter
β * . Remember however that a too large value of β * will introduce excessive artificial
dissipation into the solution.
For lower Reynolds numbers the parameter β* has to vary to preserve numerical stability and a
good convergence rate. The parameter β* should increase as the Reynolds number decreases
and may vary over several orders of magnitude .
FIGURE 7.5
Typical variation of the preconditioning parameter β* with Reynolds number
Too small value of β* may lead to divergence and too big value may lead to a too dissipative
solution.
2. Characteristic velocity and local velocity scaling
The characteristic velocity
should be as low as possible but not smaller than the local
velocity. If the local velocity scaling option is activated (default), the characteristic velocity will
be replaced by
is the local velocity.
, where
In case that the local velocity scaling option is activated (default),
can be taken as the
reference velocity, for example, the free stream velocity in external flows and the inlet velocity
must be
in internal flows. In case that the local velocity scaling option is not activated,
taken as the maximum velocity in the domain.
The choice of
has an influence on the convergence. A bigger value will accelerate the
convergence but introduce more dissipation.
3. User defined gauge parameters
If this option is activated, the user may input the gauge pressure
and gauge temperature
.
When the box is not activated, the gauge pressure and gauge temperature are chosen equal to
the fluid reference pressure and temperature for incompressible fluid, perfect gas and real gas.
In case of a condensable fluid, the gauge pressure and gauge temperature are set to 0.
A value of
of the order of magnitude of the expected temperature field will reduce the machine
round-off errors influence on the temperature field.
The value of
fixes the absolute level of the pressure in the field. This value is used in the
equation of state for a compressible fluid and in the second order artificial dissipation term. A value
of
close to the real pressure level is therefore recommended.
Merkle preconditioning
For compressible flows and condensable fluids, the Hakimi preconditioning can only be used at
the low Mach number (M<0.3). On the other side, the Merkle preconditioning is efficient at all
Mach numbers and also for all Reynolds and Strouhal numbers.
When choosing the Merkle preconditioning,
information is provided in the theoretical manual.
1. Characteristic velocity
the following parameters can be set. More
The characteristic velocity
is used to compute the particle velocity.
can be taken as
the reference velocity, for example, the free stream velocity in external flows and the inlet
velocity in internal flows.
The choice of
has an influence on the convergence. A bigger value will accelerate the
convergence but introduce more dissipation.
2. User defined gauge parameters
If this option is activated, the user may input the gauge pressure
and temperature
.
When the box is not activated, the gauge pressure and gauge temperature are chosen equal to
the fluid reference pressure and temperature for incompressible fluid, perfect gas and real gas.
In case of condensable fluid, the gauge pressure and gauge temperature are set to 0.
A value of
of the order of magnitude of the expected temperature field will reduce the
machine round-off errors influence on the temperature field.
The value of
fixes the absolute level of the pressure in the field. This value is used in the
equation of state for a compressible fluid and in the second order artificial dissipation term. A
value of
close to the real pressure level is therefore recommended.
7.1.2
Advanced Parameters for the Numerical Model
A.
Interfaced Advanced Parameters
Pseudo-time integration
An explicit Runge-Kutta scheme accelerated by a multigrid technique is used to march the
solution in time towards the steady state solution.
When the multigrid strategy is used (i.e. if more than one grid level has been selected in the
Numerical Schemes/ General page), an input box allows the user to select the number of sweeps
to be performed on the coarse grid levels. The number of sweeps is the number of times the
Runge-Kutta operator is applied. In the default solver configuration, the number of sweeps on
each level equals the level number (e.g. 2 sweeps on second level etc.). It has been observed in
many cases that the convergence rate may be significantly improved by performing a higher
number of sweeps on the coarsest levels. Recommended sets of values are, for instance, (1,2,16)
for 3 grid levels or (1,2,8,32) for 4 levels. However, it should be noted that more sweeps imply
that more time is required for an iteration.
If the option Coarse Grid Initialization has been activated in the Numerical Schemes/ General
page, the computation starts on the coarsest grid level and includes a finer grid level each time one
of the two following criteria is satisfied in the Advanced tab of the Numerical Schemes /
General Parameters page:
l The maximum number of cycles to be performed on each grid level is reached. This parameter
is specified through the input box in the Coarse grid initialization parameters area as the
Maximum number of cycles per grid level.
l The residual on the current grid level has dropped by a certain order of magnitude as indicated
by the Convergence criteria on each grid level.
Another feature of the pseudo-time integration scheme is the time stepping technique used to
march the solution in time. At present, only the local time stepping method can be selected. This
self-explanatory approach is used to drive the solution towards the steady state at the fastest rate
compatible with the CFL condition.
If the computation is unsteady, the Dual time step inner-iteration control box is unfrozen in the
Advanced tab of the Numerical Schemes/ General Parameters page. The user can specify the
Convergence criteria and Maximum number of inner iterations for the Dual time stepping
method, which is used to compute the right-hand side of the governing equations at each physical
time step, see Linear Eddy Viscosity Turbulence Models.
B. Non-interfaced Advanced Parameters
rot_iVelSy_: The governing equations for rotating systems, such as turbomachinery problems,
are usually formulated in the relative system and solved for the relative velocity components.
However, experience shows that, for propeller, ventilators or wind turbine problems,
the
formulation based on relative velocities has the disadvantage that the far field relative velocity can
reach high values. This induces an excess of artificial dissipation leading to a non-physical
rotational flow in the far field region, this dissipation is based on the computed variables. So the
governing equations for these cases are often expressed in the relative frame of reference for the
absolute velocity components. In FINE™/Open with OpenLabs™, the user has the ability to
select the solved velocity for rotating systems through the expert parameter rot_iVelSy_.
0: solve the absolute velocity components in the relative frame of reference for rotating block.
1 (default): solve the relative velocity components in the relative frame of reference for rotating
block.
iAsFT_: Since the numerical methods used in the FINE™/Turbo and FINE™/Open solvers are
different, the results obtained with these two solvers are different. The use of the expert parameter
iAsFT_ aims at giving the possibility for a FINE™/Open with OpenLabs™ user to reproduce
results obtained with FINE™/Turbo. If this parameter is set to 0, the user employs the original
version of the FINE™/Open solver. If this parameter is set to 1, the user is attempting to obtain a
version that has the similar behavior with the FINE™/Turbo solver.
There is no guarantee that using the expert parameter iAsFT_ 1 will obtain identical results
between FINE™/Turbo and FINE™/Open.
in FINE™/Open with
_ typeOfBlockID : Each block has a _ typeOfBlockID number
OpenLabs™. The user can modify this number. If the _ typeOfBlockID numbers of the
neighboring blocks that have a FNMB connection, are different, the solver will only consider the
heat flux across the FNMB interface.
agglomerationNEW_: 0: old agglomeration method;
1 (default): new agglomeration method. The treatment approach in the boundary layer is
improved.
tm_iResSmoothing_: Specifies the implicit residual smoothing method during the computation
on the finest grid. The user may always set this parameter to 2 if the residual smoothing module
needs to be activated. The solver will check the settings in the .run file and change to 1
automatically if necessary.
0: Deactivate the residual smoothing procedure,
1: The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed
for all solved equations (including the turbulence model equations). This value is available for
Euler, laminar and turbulent flow with one-equation turbulence models.
2 (default): The smoothing technique of Radespiel & Rossow is used. The residual smoothing is
performed only for the continuity, momentum and energy equations. This value is available for
turbulent flow with two-equation turbulence models.
tm_fmg_iResSmoothing_: Specifies the implicit residual smoothing method applied during the
coarse grid initialization. The user may always set this parameter to 2 if the residual smoothing
module needs to be activated. The solver will check the settings in the .run file and change to 1
automatically if necessary.
0 (default): Deactivate the residual smoothing procedure,
1: The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed
for all solved equations (including the turbulence model equations). This value is available for
Euler, laminar and turbulent flow with one-equation turbulence models.
2: The smoothing technique of Radespiel & Rossow is used. The residual smoothing is performed
only for the continuity, momentum and energy equations. This value is available for turbulent
flow with two-equation turbulence models.
tm_iResSmooVersion_: Specifies the numerical method used in the implicit residual smoothing
method.
0: the residual smoothing coefficient ϵ is computed on cell faces and the boundary conditions are
depending on the boundary type.
1: the residual smoothing coefficient ϵ is computed on cell centers and the boundary conditions
are depending on the boundary type.
2: the residual smoothing coefficient ϵ is computed on cell faces and the Neumann boundary
conditions are used.
3 (default): the residual smoothing coefficient ϵ is computed on cell centers and the Neumann
boundary conditions are used.
tm_mgCycleType_: Applies only for multigrid and selects the type of multigrid cycle
1 (default): V-cycle;
2: W-cycle;
3: F-cycle;
4: V-cycle in sawtooth;
5: W-cycle in sawtooth;
6: F-cycle in sawtooth.
gradientScheme_: Controls the computation of the gradient at cell centers, which is used mostly
for 2 features of the flow solver: the computation of the production term for turbulent models and
the reconstruction of the solution at the face from the cell center:
0: use the least square technique. When the 2nd order Roe upwind scheme is used, the expert
parameter gradientScheme_ must be set to 0. The technique may fail when dealing with highly
stretched meshes, typically in the boundary layers.
1 (default): use the weighted least square technique.
2: use the least square technique with the Singular Value Decomposition (SVD).
4: use the weighted least square technique with SVD.
5: use the Green-Gauss gradient technique.
mg_iPrecondFoF_: When using the multigrid method combining preconditioning, the forcing
function in the Full Approximation Storage (FAS) approach can be computed before/after
applying the preconditioning:
0 (default): compute the forcing function before applying the preconditioning.
1: compute the forcing function after applying the preconditioning.
The other expert parameters related to the numerical model are as follows:
Central Discretization
spc_dissip_ext_: 0 (default): the second order dissipation term is applied at inlet, outlet and
external boundaries.
1: both the second and fourth order dissipation terms are applied at these boundaries.
2: neither the second nor fourth order dissipation are computed at these boundaries.
spc_dissip_wall_: 0: the second order dissipation term is applied at wall boundary.
1: the second order dissipation term is applied at wall boundary, and the second-order difference
in the first inner cell is set to zero in the direction normal to the wall.
2: neither the second nor fourth order dissipation are applied at wall boundary, and the second-
order difference in the first inner cell is set to zero in the direction normal to the wall.
iFluxAverage_ : In the absence of gravity, two discretizations of the fluxes for the Jameson
scheme have been introduced.
0 (default): variable averaging,
1: flux averaging.
iFluxAverageFMG_: Select the method of discretization of the fluxes during the FMG..
0 (default): variable averaging,
1: flux averaging.
spc_artDiss2ndCoef_: Coefficient κ(2) for 2nd order dissipation in the central scheme. Default
value is 1.0.
spc_artDiss4thCoef_: Coefficient κ(4) for 4th order dissipation in the central scheme. Default
value is 0.1.
spc_ expMartinelli_ : Exponent in the multi- dimensional scaling model of Martinelli of the
dissipation used in central schemes. Default value is 0.5.
spc_TswitchInArtDissip_: Defines whether the second order artificial dissipation switch should
be based on both pressure and temperature gradients or on pressure gradients only.
0 (default): only pressure gradients are taken into account.
1: both pressure and temperature gradients can be taken into account.
spc_XhilnArtDissip_: Improve the treatment of artificial dissipation running the second order
central scheme for supersonic and hypersonic applications. This parameter varies between 0.0 and
0.99. The value 0.0 corresponds to the original central scheme of Jameson which is not
monotonous for cases presenting discontinuities like shocks. The value 0.99 makes the scheme
monotonous.
Central matrix discretization
spc_ artMatDiss2ndCoeff_ : Coefficient k (2) for 2nd order dissipation in the central matrix
dissipation scheme. Default value is 1.0.
spc_ artMatDiss4thCoeff_ : Coefficient k (4) for 4th order dissipation in the central matrix
dissipation scheme. Default value is 0.15.
spc_ artMatDissfmg_ : In case the central matrix dissipation scheme is selected, another
dissipation scheme can be applied during the coarse grid initialization:
0 (default): The central scalar scheme is applied during the FMG
1: The central matrix scheme is applied during the FMG
EntrFx_: The parameters Vl and Vn used in the limiter of the central matrix dissipation scheme.
Default value is 0.1 0.1.
merkle_matdisEntrFx_: Entropy fixes for the matrix dissipation with Merkle preconditioner.
The parameters Vl and Vn used in the limiter of the central matrix dissipation scheme. Default
value is 0.3 0.3.
hakimi_matdisEntrFx_: Entropy fixes for the matrix dissipation with Merkle preconditioner.
The parameters Vl and Vn used in the limiter of the central matrix dissipation scheme. Default
value is 0.1 0.1.
Upwind Discretization
upw_dissipEnthalpy: Controls the use of the standard or isenthalpic dissipation. The default
option is the standard dissipation when value set to 0.
upw_dissip_ext_: Controls the calculation of the dissipation at inlet-outlet boundaries. If 1 the
dissipation is computed (0 not computed).
upw_ limit_ : Activate the limiting procedures with the second order upwind scheme for
supersonic and hypersonic applications. For cases presenting shocks, this option has to be
activated by setting the value to 1 so that a monotonous solution is obtained.
upw_limitVenka_: Select to use the Barth-Jespersen limiter or the Venkatakrishnan limiter with
the second order upwind scheme for supersonic and hypersonic applications.
0 (default): the Barth-Jespersen limiter,
1: the Venkatakrishnan limiter.
EntrFx_: Values of the entropy fix for the linear fields and the non-linear fields. EntrFx_ is an
array of two dimensions set by default at (0.1;0.1). For cases presenting shocks, it is advised to
modify the values and set them to (0.3; 0.3).
Time Discretization
tm_nbStage_: Specifies the desired number of stages in the Runge-Kutta scheme. Default set to 4
tm_drcoeff_: Runge-Kutta coefficients. One for each stage, the first one for the first stage, the
second one for the 2nd stage and so on. If all coefficients are set to zero, default values are taken,
depending on the number of stages and the spatial discretization scheme.
spc_iCalcArtifDissip_: One for each Runge-Kutta stage, the first one for the first stage, the
second for the second stage and so on. Set to 1 if numerical dissipation is to be recalculated at the
associated stage, set to 0 if the numerical dissipation is taken from the previous calculation. For
consistency, spc_iCalcArtifDissip_ should be set to 1.
spc_iCalcVFluxes_: One for each Runge-Kutta stage, the first one for the first stage, the second
for the second stage and so on. Set to 1 if viscous fluxes are to be recalculated at the associated
stage, set to 0 if the numerical dissipation is taken from the previous calculation. For consistency,
spc_iCalcVFluxes_ should be set to 1.
Preconditioning
preco_pcEpsVLim_: Coefficient of
when computing
in the Merkle preconditioning
(default value is 0.001).
preco_pcEpsVLimC_: Coefficient of the speed of sound when computing
preconditioning(default value is 0.001).
in the Merkle
7.2
TIME CONFIGURATION
To perform time independent computations it is sufficient to select Steady. For time dependent
simulations, Unsteady should be selected which gives access to additional parameters for
unsteady flow simulation. All parameters in the FINE™/Open GUI related to unsteady
computations are described in the following section. More details can be seen in the theoretical
manual.
7.2.1
The Interface for an Unsteady Computation
When selecting Unsteady time configuration in the General Properties page the following
additional parameters become accessible in the FINE™/Open GUI:
Rotating Machinery
On the Physical Configuration\Rotating Machinery page, under the Rotor/stator tab, the
Domain scaling rotor/stator interface treatment can be activated.
Control Variables
On the Computation Control/Control Variables page under the tab General, the following
parameters appear when selecting an unsteady time configuration:
If Time averaged solution activated, the value indicates the number of iteration from which the
time-averaging of the solutions will be started.
Time step
l Physical time step: in general cases, the user specifies the magnitude of the physical time step
in seconds. This time step is constant
In cases of
turbomachinery applications where Rotor/Stator interfaces are detected, the Number Of
Angular Positions is requested instead of the Physical time step.
through the whole calculation.
A variable physical time is automatically computed by the solver if a variable rotational speed is
imposed in the OpenLabs™ environment using the internally defined rot_Omega_ constant. A
variable physical time step can also be directly imposed in the OpenLabs™ environment using the
internally defined PhysTimeStep constant.
ta_
iVariableTimeStepping_ must be set to 1 in the Global parameters list in the Advanced tab in
order to activate the use of a variable physical time step.
expert parameter
In both cases,
the
l Number of time steps: to define the number of time steps to perform.
Steady initialization
l Number Of Steady Iterations: the number of iterations to initialize the unsteady computation.
Such initialisation is performed with the steady state algorithm, using fixed geometry and mesh
as well as constant inlet/outlet boundary conditions. In case this initialisation procedure is used
the steady state iterations can even be proceeded by a full multigrid process allowing a rapid
initialisation of the flow.
l Save Steady Solution Every : the number of iterations at which the solution of steady
initialisation is saved
Steady initialization is not available when From file is used in the Initial Solution / Initial
Solution page.
Output files
l Save Solution Every: allows to save the solution after a constant number of time steps. By
default the output files will be overwritten, every time the solution is saved. In order to keep
the successive unsteady solutions, the option Visualization files must be set to Multiple files.
l Time averaged solution after # time steps: When activated, the time averaged solution will
be computed and saved in a ".avg" file after the imposed time steps. After the user activates
this option, the user must go to the Computation Control / Outputs page under the category
Unsteady to select the quantities that will be time averaged. All the quantities surrounded by <
> can be selected.
The quantities that can be time averaged appears only when the option Time averaged solution
after # time steps is activated.
The time averaged solution is computed after the imposed time steps on fine mesh. All the
quantities are averaged as follows:
where
is the time step in time step i and T is the period.
l Visualization files: controls the output files for visualization.
l One file: One set of output files for visualization in CFView™ is only saved at the end of
the computation.
l Multiple files: Multiple sets of output files are saved for visualization in CFView™ during
the computation (every x time steps as specified in Save Solution Every).
l Intermediate restart files: controls the output files for unsteady restart. In both cases (One
file/Multiple files), second order restart is possible.
l One file: One set of output files for unsteady restart is only saved at the end of the
computation.
l Multiple files: Multiple sets of output files are saved for unsteady restart during the
computation (every x time steps as specified in Save Solution Every).
Second Order time-accurate scheme
The FINE™/Open solver performs second order accurate simulations in time. When requesting a
restart of an unsteady computation, the FINE™/Open solver will automatically look for a ".btm1"
file containing the solution at previous time steps. If this file exists, a second order restart is
performed. If this file is not found, a first order scheme is used for the first time step.
7.2.2
Advanced Parameters for Unsteady Computations
Numerical Model advanced parameters
In the Numerical Schemes page, two new parameters appear in the Advanced tab. These are the
control variables for the inner iterations of the dual time stepping approach. For each physical time
step a certain number of iterations are performed in pseudo time leading to a converged solution
independent of the pseudo time.
l Convergence criteria of the inner iterations (orders of magnitude of reduction). The inner
iterations are stopped if the reduction of the residuals reaches the specified value.
l Maximum number of inner iterations: it allows the user to define the maximum number of
iterations to perform for each time step. In general the default of 50 iterations per time step is
sufficient (15 in case of using the CPU booster). The inner iterations are automatically stopped
after this maximum number of iterations, even if the convergence criteria has not been
satisfied.
7.2.3
Best Practice on Time Accurate Computations
General advice on how to perform time accurate computations is provided in this section.
General Project Set-up for Time Accurate Computations
1. Create a new project,
2. Select Unsteady in General parameters page,
3. Select the fluid to use in the Fluid Model page,
4. On the Rotating Machinery page, set the parameters for the turbomochinery simulations,
5. Set the boundary conditions. Notice that only steady boundary conditions are presently
available.
6. There are three possibilities for the initial solution:
l to start from a steady solution,
l to start from an unsteady solution,
l to use constant values or for turbomachinery.
For more detail on these initialization procedures see Initialization Procedure.
7. All outputs available in steady mode are also available in unsteady mode .
8. On the Computation Control / Control Variables page set:
l the physical time step and the number of time steps,
l amount of iterations in steady state initialization 
l the Amount of Output files
Initialization Procedure
Start from a Steady Solution
In most cases it is necessary to perform a preliminary steady state computation. The objective
might be to ensure that the problem naturally depicts the unsteady behavior and/or to get an
adequate guess solution before going towards time accurate calculations with periodic behavior.
The steady state initialization may be done in a separate computation, performed in steady mode.
The time accurate calculation is then started using this solution as an initial solution. To set up the
time accurate calculation in this case follow the steps 1 to 8. In step 6 select Initial solution from
file and select the solution of the steady computation.
Start From a Time Accurate Solution
It is possible to start from a previous time accurate solution. For general information about starting
from an initial solution, see Initial Solution from File section.
In order to allow the user to do a second order accurate restart, it is necessary to keep, in the initial
solution directory, the "*.btm1" file which is generated by the flow solver during the unsteady
computations used to initialize the present computation. When requesting a restart of an unsteady
computation, the FINE™/Open solver will automatically use this second solution file. If this file is
not found, a first order scheme is used for the first time step, as if the code was starting from an
initial steady solution.
In the case of a second order restart, the convergence history must be imported, otherwise a steady
solution is computed during the first time step.
Steady State Initialization in Unsteady Computation
The steady state initialization is automatically performed before starting the time accurate
computation (that means within the same computation). To perform a steady state initialization in
an unsteady computation, the number of iterations has to be entered in Steady Initialization
parameters on the Control Variables page.
Physical Time Step
The physical time step should be entered on the Control Variables page. Choice of the correct
time step depends on the expected frequency of the flow phenomena that the user wishes to
capture. In general, it is recommended to compute at least 10 to 20 time steps per period.
Amount of Output
By default only one set of output files for visualization in CFView™ is created, which is
periodically overwritten. It is however possible to save solutions at specified time steps (this
depends on the Save solution Every entry available in the Control Variables page) into separate
files. This is done by setting the option Visualization files to Multiple files in the Control
Variables page.
Multiple sets of files will be generated. The files are automatically renamed accordingly to the time
step computed using the suffix "_t#." that is thus determining the #th physical time step.
CHAPTER 8.
MESH ADAPTATION
FINE™/Open with OpenLabs™ contains an optional module dedicated to solution- based mesh
adaptation at the page Numerical parameters/Mesh adaptation.
This module requires a special license feature. If the model is not accessible due to a missing license it
is displayed in gray. Please contact our local sales or support office for more information about the
possibility of obtaining a license.
The mesh adaptation module is not available with:
l FNMB connection,
l multidomain mesh,
l axisymmetric mesh,
l parallel computation.
In this section
8.1 Introduction
8.2 Driving an adaptive computation in FINE™/Open with OpenLabs™
175
176
8.1
INTRODUCTION
When industrial flows around complex geometries are computed, regions where interesting flow
features are met are generally unknown, or may even vary during the simulation, if the flow is
unsteady. Using a uniformly fine grid to capture all flow phenomena is computationally costly,
whereas using coarser grids degrades the solution accuracy. In this context, the potential of mesh
adaptation is extremely high because it allows the clustering of points only where needed, and
coarse grids where no significant flow variations occur, thereby optimizing computational costs
with respect to accuracy.
Other types of adaptation, like equation, time step and p-type adaptation, can be considered. Their
use is however not widespread compared to mesh adaptation, and their efficiency is often case
dependent. Among mesh adaptation strategies, two approaches can be distinguished, namely grid
redistribution, or r-type adaptation, and grid enrichment, or h-type adaptation.
In the first strategy, the solution of the governing equations is computed on a grid composed of a
fixed number of vertices, redistributed from their original locations in such way that they are
concentrated in the vicinity of flow features. This yields the best possible solution for a fixed
amount of resources. In the second strategy, points are added in the vicinity of flow features. This
yields the least costly solution for a fixed level of accuracy, Dannenhoffer (1988).
On the other hand, h-type adaptation necessitates the use of an appropriate data structure, because
the adapted meshes are unstructured. Since unstructured meshed are used by the FINE™/Open
solver, this method can be used. It offers the possibility of achieving very high accuracy by
clustering points where needed, and is best suited to domains involving complex geometries, since
point movement is generally limited, depending on local geometric configurations.
In the FINE™/Open solver, h- type adaptation is available. The implementation of h- type
adaptation in the flow solver is a natural choice since the code deals with unstructured meshes. In
addition, since adaptation is also a central task in the mesh generator HEXPRESS™, the
dedicated classes are shared by both codes, and a specific data structure is designed to optimize
this task.
FIGURE 8.1
Mesh and Mach number field around NACA0012 when using initial mesh (left) and after four
adaptations (right)
8.2
DRIVING AN ADAPTIVE COMPUTATION IN
FINE™/OPEN WITH OPENLABS™
Basic structure of an adaptive computation
Mesh adaptation can currently be used for steady computations only. Generally, a few adaptations
(e.g. 2) can be performed to optimize the initial mesh with respect to the flow solution.
The basic structure of the adaptive procedure is as follows:
1. The flow solution is calculated on an initial mesh.
2. Using adaptation criteria, directional refinement flags as well as coarsening flags are produced
for each control volume.
3. Mesh adaptation is performed, based on the refinement/coarsening flags. Adaptation starts with
the local mesh coarsening. Then, anisotropic local mesh refinement is performed on the
coarsened mesh, and the flow solution is transferred to the new mesh using the grid hierarchy.
4. A new flow solution is computed using the new adapted grid.
5. If the number of mesh adaptations performed is below a prescribed number of adaptations,
then we go back to Step 2, otherwise the flow computation is terminated.
FIGURE 8.2
Adaptation page (specific license required)
Number of adaptations
In the case of steady flows, two or more mesh adaptations can be performed to optimize the mesh
with respect to the solution. The number of adaptations can be specified by the user, in the
Numerical parameters/Mesh adaptation page.
The number of adaptations depends on the initial mesh properties in terms of clustering and size, and
on the available computational resources. One should be aware that for three-dimensional problems,
the mesh size is often multiplied by two in a single adaptation step. The adapted mesh size is highly
dependent on the adaptation criteria and on the flow computed on the initial grid.
Adaptation criteria
Properties of the mesh resulting from adaptation depend on criteria, which are based on flow
feature detection. These are displayed in the Adaptation criteria section of the Numerical
parameters/Mesh adaptation page. Four flow feature detectors, or sensors, are available. The
first is based on density, the second on velocity magnitude, the third on pressure and the last on
temperature. Sensors will order refinement of regions where significant variations of the
associated physical quantity (density, velocity, pressure and temperature) occur, and order
coarsening in regions of very low gradients of the flow quantities.
By default, only velocity magnitude is used for flow feature detection. It is however possible to
select the other three criteria by ticking the associated activation boxes. Several criteria can be
selected at the same time, e.g. velocity and pressure. Such a configuration is advised when
significantly different flow features have to be captured. One sensor is then often responsible for
refinement in a certain region, and the other sensor may order refinement in other regions.
Certain regions may be flagged for refinement by a sensor, and for coarsening by another one. In this
case, refinement always takes priority.
In addition to the computation of sensors, associated refinement and coarsening threshold values
should be determined in order to specify the regions to be refined or coarsened. When a sensor is
activated in the FINE™/Open GUI, two additional (vector) parameters α and β, corresponding to
refinement and coarsening threshold parameters respectively, should be specified. The size of
these vectors corresponds to the number of adaptations. The first component of the vectors gives
threshold parameters for the first adaptation, the second for the second adaptation, and so on.
Increasing the value of α means that the refinement threshold is increased, hence fewer elements
are refined. Increasing the value of β means that the coarsening threshold is increased, hence more
elements may be coarsened. The default value for α is 0.3, while β is set to -0.3.
It is generally advised to start with low refinement and coarsening threshold for the first refinement,
in order to ensure the capture of relevant flow phenomena. The threshold values can be increased
after each adaptation, so that the refinement regions are captured more accurately, and zones where no
variations occur can be coarsened.
Usual lower and upper bounds for both α and β are -1.0 and 2.0, although lower or higher values can
be selected.
Other adaptation control parameters
In the Adaptation control parameters section of the Numerical parameters/Mesh adaptation
page, two additional parameters can be specified by the user, the maximum number of iterations
and the convergence criteria for the computations on initial and intermediate grids.
The maximum number of iterations and convergence criteria on the final grid are specified in the
Computation control/Control Variables page.
The user has the freedom to specify different convergence criteria for the intermediate grids
compared to the final one. However,
the solution is
sufficiently converged on intermediate grids before proceeding to mesh adaptation, otherwise
transient flow features may be captured, leading to wrong "mesh convergence".
is strongly advised to make sure that
it
Advanced parameters
These parameters are located in the Advanced tab of the Computation control / Control
Variables page.
out_snsOnCFV_: orders output of the selected sensors to CFView™ in order to analyse the
behavior of the adaptation criteria over the computational domain. This helps gaining a better
understanding on how the sensor behave on a certain class of flow configurations. The default
value of the parameter is out_ snsOnCFV_ = 0 (no output). In order to trigger output to
CFView™, the parameter should be set to 1. A "_sns_adap#.cfv" file (how to open?) will be
created for each mesh adaptation step, which includes the results of the selected sensors.
Depending on the selected criteria, the following sensor quantities may appear in CFView™
when post processing:
l sensor 1: Density sensor
l sensor 22: Velocity magnitude sensor
l sensor 13: Pressure sensor
l sensor 19: Temperature sensor
Notice that this parameter should be activated only if adaptation is performed, and if the archiving of
the solution on intermediate adapted meshes has been activated in the Computation Control /
Outputs page, see Advanced section.
CHAPTER 9.
OPTIONAL MODELS
FINE™/Open with OpenLabs™ contains the following physical models.
Each of these modules requires a special license feature. If the model is not accessible due to a missing
license it is displayed in gray. Please contact your local sales or support office for more information
about the possibility to obtain a license.
In this section
9.1 Combustion modeling
9.2 Radiation modeling
9.3 Porous Media Model
9.4 Coupling
9.5 Fluid-Particle Interaction
9.6 Uncertainty Quantification
9.7 Cavitation
9.8 Multi-species Framework
181
203
219
224
238
256
262
279
9.1
COMBUSTION MODELING
9.1.1
Introduction
Combustion is a complex sequence of exothermic chemical reactions between a fuel and an
oxidant accompanied by the production of heat and light. In the most general approach,
combustion is described as a convection-diffusion-reaction problem involving n species and m
reactions between these species as described by a reaction mechanism. In reality, combustion of
even simple fuels involves a large number of intermediate species, which interact through
elementary reactions. A direct simulation of the chemistry involved in combustion would
therefore lead to a coupled set of n+4 equations, namely the momentum equations, the energy
equation and the balance equations for n species. For instance state- of- the- art reaction
mechanisms for methane contain 53 species subject to 325 elementary reaction steps; to solve this
system a system of 57 transport equations would need to be solved.This is unacceptable for
industrially relevant CFD studies.
The combustion module in FINE™/Open with OpenLabs™ allows the user to simulate all kinds
of combustion. In addition, radiation can be taken into account in conjunction with combustion,
please refer to Radiation modeling section for more information.
The combustion module can be directly activated from the FINE™/Open GUI under Physical
configuration. If the combustion module is activated for one block, the combustion model will be
applied for all blocks.
Since the modeling is based on the assumption of a low Mach number flow, preconditioning is
thus selected as a default option for all combustion runs, and it does not longer appear as a user
choice within the graphical user interface.
The following limitations applied to the combustion module:
l Combustion simulations are limited to subsonic flows.
l Only compatible with k-epsilon based turbulence models.
l When simulating combustion with CPU Booster, the following limitations are applied:
l Not compatible with the Hakimi preconditioning,
l Not compatible with the expert parameter CombTimeStep_=1,
l ONLY compatible with the k-epsilon (Extended Wall Function) turbulence model and the
k-epsilon (Low Re Yang-Shih, classic) turbulence model.
l For the compatibility of the combustion model, please refer to compatibility matrix.
9.1.2
Non-premixed Combustion
The modeling techniques applied for the Non-premixed combustion are based on the mixture
fraction approach. Besides a basic combustion model for non-premixed combustion, which can
account for heat loss due to radiation, a post-processing model for the formation of NOx is
available in FINE™/Open with OpenLabs™.
On the Optional Models / Combustion page, the combustion type Non premixed is available.
FIGURE 9.1
Non-premixed combustion parameters
Two chemistry models are proposed as a user choice:
l Equilibrium : This model is based on the chemical equilibrium assumption, where it is
assumed that the time scales related to combustion are infinitely much faster than those of the
flow and mixing. With this approach it is assumed that the fuel/air mixture in each point is in
chemical equilibrium and the flame is not influenced by strain.
l Flamelet: The flamelet model incorporates non-equilibrium effects. These non-equilibrium
effects are mainly important when looking at the concentrations of minor species, especially
when pollutant formation (NOx, CO etc.) is of interest. In this approach, a flame (laminar or
turbulent) is viewed as an ensemble of flamelets (small flames) embedded in the flow field and
that are subjected to strain from the flow. This makes the flamelet model more accurate,
although it requires the generation and the use of a library of flamelets.
A checkbox can be activated to select a specific strain rate. The default value is set to 100/s.
Turbulence-chemistry interaction can be modeled using the Presumed PDF approach. In the
Presumed PDF approach, a probability density function (PDF) for the mixture fraction describes
the probability that the flow field takes in a certain value for the mixture fraction at a given point.
In FINE™/Open with OpenLabs™, it is presumed that the shape of the PDF can be represented
by ß-functions, and the distribution is parameterized via its statistical moments. In practice, the
calculation of the PDF involves integrals and is thus computationally expensive. A pre-integration
of the PDF is done to reduce the overhead, and an additional dimension is stored in the
combustion look up tables for the mixture fraction variance.
For the evaluation of NOx, a dedicated post-treatment restricted to the formation of thermal NO
can be activated.
A combustion look up table must be specified for the determination of the thermochemical
properties of the burnt and unburnt mixture of the fuel and oxidizer. After specifying the table, the
button Preview can be used to view the properties of the table. If needed, the user can click on
the button Create/Edit to create a new look up table. For more information on how to create/edit
a combustion look up table, see TabGen/Chemistry.
The combustion model is limited to two stream problems. If a combustion problem contains three (or
more) streams, then the third stream (or any stream in addition to the first and the second) must
represent a linear combination of the two first ones.
The present approach assumes that the chemistry is much faster than the mixing process. For slow
reactions this assumption may not be valid which results in poor accuracy of the predictions.
The Create/Edit... button is only available on Linux.
The other combustion model parameters in the FINE™/Open GUI can be found in the following
menus:
Fluid model
When the combustion model is activated, the fluid is automatically changed to "Reactive fluid".
The Fluid Model menu gives restricted access to fluid properties. Both density and temperature
field are determined through the interrogation of look-up combustion tables, as function of the
mixture fraction and its variance.
However, reference values, heat conduction and diffusivity related parameters can still be edited.
Flow model
When the combustion model is activated, the turbulence model is by default set to the standard k-ε
model. The other 2-equation turbulence models available for inert flow can also be selected for
the one equation turbulence models cannot be used in
combustion simulations. However,
conjunction with combustion modeling.
Laminar regime can be also modeled.
Boundary conditions
Combustion-dedicated boundary conditions have been introduced at inlets, with entries for the
mixture fraction and NO mass fraction.
l Mixture fraction should range between 0 (oxidizer stream) to 1 (fuel stream).
l NO mass fraction relates to the fraction of NO injected through the inlet patch. The
recommended value is set to 0.
No dedicated condition is required for the treatment of outlets, since combustion variables are
purely convected quantities.
Initial Solution
Minor modifications have been brought to the Initial Solution menu, with the introduction of
initial data for the mixture fraction. As a default, pure oxidizer conditions (Mixture fraction f = 0)
are recommended in most cases.
Numerical parameters
When performing non-premixed combustion computations, the following choices are the best
recommendation:
l In the General Parameters page under the tab General,
l set the Number of grid(s) to 3 or 4 (preferred),
l activate Coarse grid initialization.
l In the General Parameters page under the tab Advanced,
l Increase the Maximum number of cycles per grid level to 400 - 600,
l Reduce Convergence criteria on each grid level to -6,
l Possibly increase Number of sweeps on successive grid levels to 1 2 16 (3 grid levels), or
1 2 3 32 (4 grid levels)
l In the Numerical Schemes page,
l The recommended CFL number is 1.5. This is also set as default.
The non-premixed combustion module can be used together with CPU Booster. In order to get
the best performance, the following settings are recommended when combining CPU Booster and
combustion:
l In the Flow Model page,
l Set the Turbulence model to k-epsilon (Extended Wall Function) or k-epsilon (Low Re
Yang-Shih, classic),
l In the General Parameters page under the tab General,
l set the Number of grid(s) to 3 or 4 (preferred),
l activate Coarse grid initialization.
l In the General Parameters page under the tab Advanced,
l Increase the Maximum number of cycles per grid level to 400 - 600,
l Reduce Convergence criteria on each grid level to -6,
l Deactivate the CPU Booster during coarse grid initialization,
l In the Numerical Schemes page,
l The recommended CFL number is 100. This is also set as default. In case of convergence
problem, reduce the CFL number.
l Keep the Merkle preconditioning selected.
l In the Control Variables page under the tab Advanced,
l Increase the density relaxation coefficient to 0.1 (the fifth dimension of the local expert
parameter RelaxCombVars_). In case of convergence difficulty, set the density relaxation
coefficient to 0.01 (default value).
l In case that heat flux solid boundary condition is defined, set the local expert parameter
IterScalingFuncHeatFlux_ to 10.
l In case that the S2S radiation model is activated, set the local expert parameter RadFVM_
IterationNumber to 2.
Outputs
When performing non-premixed combustion computations, the following quantities are available
for output
/ Outputs / General under the category
Combustion.
in the page Computation Control
l Comb_MixtFrac: mixture fraction
l Comb_VarianceMixtFrac: mixture fraction variance
l Comb_EnthDefect: Enthalpy defect
l Comb_TempDefect: Temperature defect
l Comb_TemperatureClipping: Flag to plot whether temperature was clipped or not. 0: Not. 1:
Yes.
l Comb_SDissipRate: scalar dissipation rate
When NOx post-processing is activated, the following variables can be selected for output:
l Comb_NOxPost: mass fraction (
) of NO
l Comb_SourceTermNO: source term of the mass fraction (
) equation
Depending on the lookup table specified for the non- premixed computation, the following
quantities may be available:
l LookUpTable_RHO: density of the mixture [kg/m³]
l LookUpTable_TEMP: absolute temperature of the mixture [K]
l LookUpTable_DYNVISC: dynamic viscosity of the mixture [Pa.s]
l LookUpTable_ENTHALPY: specific chemical enthalpy of the mixture [J/Kg]
l LookUpTable_CP: isobaric heat capacity of the mixture [J/K/Kg]
l LookUpTable_SCNO: first source term of the NO equation
l LookUpTable_SPNO: second source term of the NO equation
l LookUpTable_MMW: molar weight of the mixture [kg/ kmol]
l LookUpTable_QOTM: source term for OTM model, only if applicable
l LookUpTable_Temp4: absolute temperature in fourth power
l LookUpTable_LAM: laminar heat conductivity coefficient (
)
l LookUpTable_##: mass fraction of the species ##
Expert parameters
All non- interfaced advanced parameters related to the non- premixed combustion model are
accessible on the Control Variables page under the tab Advanced.
combSDissConst_: Specify the constant
for the mean scalar dissipation rate. The default
value is 2.0.
combSchmidtTurb_: The turbulent Schmidt number (default value 0.7).
RelaxCombVars_: The relaxation coefficient in combustion module. This parameter is an array
of seven dimensions, corresponding to the relaxation coefficients for the mixture fraction f, the
mixture fraction variance g, the enthalpy defect, the NO variable, the density update, the
molecular viscosity and progress variable update respectively (Default value: 1 1 1 1 0.01 1 1).
Note: The progress variable relaxation factor is used by the premixed model.
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied
to scale the heat fluxes boundary condition(s). During the course grid initialization the heat flux
(es) is/are set to zero. The idea of this switch is to ensure that the flow field and/or the combustion
process is developed before extracting/adding heat.
combTimeStep_: By default (value=0), the time step solving all the combustion equations is
determined by using the acoustic propagation speed (u+c). When setting the expert parameter
combTimeStep_ to 1, the time step is determined by using the advective propagation speed (u).
9.1.3
Premixed Combustion
Premixed combustion occurs whenever fuel and air are mixed at the molecular level prior to
ignition. Reaction takes place in a combustion zone that separates unburnt reactants and burnt
combustion products. This combustion mode is found in classical spark ignition engines, in many
household appliances and in Bunsen burners.
A. Premixed Combustion in FINE™/Open GUI
On the Optional Models / Combustion page, the combustion type premixed is available. Only
the BML type model can be selected as Premixed combustion model. These model assume that
chemical reactions are localized in thin surface which may be represented as a sheet separating
unburnt mixture from burnt gas. The formulation is based on introducing and solving progress
variable equation. The progress variable equation has source terms which can be modeled using
chemistry mode. Chemistry modes are the Zimont model, the Zimont model with the modification
of Dinkelacker and the Lindstedt-Vaos Model. The Laminar flame speed, the adiabatic flame
temperature of burnt mixture and density, the temperature, the kinematic viscosity of the unburnt
mixture are inputs to the model.
FIGURE 9.2
Premixed Combustion parameters
Fluid model
When the combustion model is activated, the fluid is automatically changed to "Reactive fluid".
The Fluid Model menu gives restricted access to fluid properties.
Flow model
When the combustion model is activated, the turbulence model is by default set to the standard k-ε
model. The other 2-equation turbulence models available can also be selected for combustion
simulations. However, one equation turbulence models, such as the Spalart-Allmaras model, that
are available for inert flow can not be used in conjunction with combustion modeling.
Laminar regime can also be modeled. In the absence of turbulence, the laminar speed is taken as
the effective flame speed.
In the absence of turbulent fluctuations (
TFC model gives
. Hence, the modified TFC model is recommended in laminar simulations.
), the modified TFC model gives
while the
Boundary conditions
Combustion-dedicated boundary conditions have been introduced at inlets, with entries for the
Normalized progress variable.
l The Normalized progress variable should range between 0 (unburnt state) to 1 (burnt state), the
default value is set to 0.
No dedicated condition is required for the treatment of outlets, since combustion variables are
purely convected quantities.
Initial Solution
Initial data for progress variable has been introduced to the Initial Solution menu. As a default, a
value of unity is recommended for the Normalized progress variable. This value corresponds to a
fully burnt state type initialization.
Numerical parameters
When performing premixed combustion computations,
recommendation:
the following choices are the best
l In the General Parameters page under the tab General,
l set the Number of grid(s) to 3 or 4 (preferred),
l activate Coarse grid initialization.
l In the General Parameters page under the tab Advanced,
l Increase the Maximum number of cycles per grid level to 400 - 600,
l Reduce Convergence criteria on each grid level to -6,
l Possibly increase Number of sweeps on successive grid levels to 1 2 16 (3 grid levels), or
1 2 3 32 (4 grid levels)
l In the Numerical Schemes page,
l The recommended CFL number is 1.5. This is also set as default.
The premixed combustion module can be used together with CPU Booster. In order to get best
performance,
the following settings are recommended when combining CPU Booster and
premixed combustion:
l In the Flow Model page,
l Set the Turbulence model to k-epsilon (Extended Wall Function) or k-epsilon (Low Re
Yang-Shih, classic),
l In the General Parameters page under the tab General,
l set the Number of grid(s) to 3 or 4 (preferred),
l activate Coarse grid initialization.
l In the General Parameters page under the tab Advanced,
l Increase the Maximum number of cycles per grid level to 400 - 600,
l Reduce Convergence criteria on each grid level to -6,
l Deactivate the CPU Booster during coarse grid initialization
l In the Numerical Schemes page,
l The recommended CFL number is 100. This is also set as default. In case of convergence
problem, reduce the CFL number.
l Keep the Merkle preconditioning selected.
l In the Control Variables page under the tab Advanced,
l Increase the density relaxation coefficient to 0.1 (the fifth dimension of the local expert
parameter RelaxCombVars_). In case of convergence difficulty, set the density relaxation
coefficient to 0.01 (default value).
l In case that heat flux solid boundary condition is defined, set the local expert parameter
IterScalingFuncHeatFlux_ to 10.
l The relaxation coefficient of the progress variable (the seventh dimension of the local
expert parameter RelaxCombVars_) should be kept as 1. In case of convergence difficulty,
set this relaxation coefficient to 0.1.
l In case that the S2S radiation model is activated, set the local expert parameter RadFVM_
IterationNumber to 2.
Outputs
When performing partially- premixed combustion computations,
the following quantities are
available for output in the page Computation Control / Outputs / General under the category
Combustion.
l Comb_NormalizedProgressVariable: normalized progress variable
l Comb_SourceProgressVariable1: source term of the normalized progress variable equation
l Comb_Temperature: temperature of the mixture
l TurbulentFlamespeed: turbulent flame speed
Expert parameters
All non- interfaced advanced parameters related to the non- premixed combustion model are
accessible on the Control Variables page under the tab Advanced.
combSDissConst_: Specify the constant
for the mean scalar dissipation rate. The default
value is 2.0.
combSchmidtTurb_: The turbulent Schmidt number (default value 0.7).
RelaxCombVars_: The relaxation coefficient in combustion module. This parameter is an array
of seven dimensions, corresponding to the relaxation coefficients for the mixture fraction f, the
mixture fraction variance g, the enthalpy defect, the NO variable, the density update, the
molecular viscosity and progress variable update respectively (Default value: 1 1 1 1 0.01 1 1).
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied
to scale the heat fluxes boundary condition(s). During the course grid initialization the heat flux
(es) is/are set to zero. The idea of this switch is to ensure that the flow field and/or the combustion
process is developed before extracting/adding heat.
combTimeStep_: By default (value=0), the time step solving all the combustion equations is
determined by using the acoustic propagation speed (u+c). When setting the expert parameter
combTimeStep_ to 1, the time step is determined by using the advective propagation speed (u).
9.1.4
Partially-premixed Combustion
FINE™/Open with OpenLabs™ provides
to simulate partially- premixed
combustion: Manifold technique (FGM) and Hybrid BML/Flamelet. The difference between
the FGM technique and the hybrid BML/Flamelet model is in the source term closure. In the
Hybrid BML/Flamelet model, the source term in the transport equation for the progress variable
and variance of the progress variable are closed using a BML type model.
two methods
The partially-premixed combustion model can be selected in the Optional Models / Combustion
page. The following part explains how to set up a partially-premixed combustion computation
using the Manifold technique (FGM) or the Hybrid BML/Flamelet method.
Flamelet Generated Manifold Model
FIGURE 9.3
FGM Partially-premixed combustion parameters
Turbulence-chemistry interaction is modeled using the Presumed ß-PDF approach. In the
Presumed PDF approach, a probability density function (PDF) for the mixture fraction and the
progress variable describes the probability that the flow field takes in a certain value for the
mixture fraction and the progress variable at a given point. In practice, the calculation of the PDF
involves integrals and is thus computationally expensive. A pre-integration of the PDF is done to
reduce the overhead, and an additional dimension is stored in the combustion look up tables for
the mixture fraction.
For the evaluation of NOx, a dedicated post-treatment restricted to the formation of thermal NO
can be activated.
The NOx information is contained in the combustion look- up table. Please make sure your table
including the NOx information.
A combustion look up table must be specified for the determination of the thermochemical
properties of the burnt and unburnt mixture of the fuel and oxidizer. After specifying the table, the
button Preview can be used to view the properties of the table. If needed, the user can click on
the button Create/Edit to create a new look up table. For more information on how to create/edit
a combustion look up table, see TabGen/Chemistry.
The Create/Edit... button is only available on Linux.
Hybrid BML/Flamelet Model
FIGURE 9.4
Hybrid/BML Flamelet Partially-premixed combustion parameters
When the Hybrid/BML Flamelet model is selected, additional parameters are needed for the
closure of the source terms of the progress variable and variance of the progress variable.
The available BML models are the Zimont model and the Dinkelacker model.
In Flamelet definition, the user has to choose one fuel-air mixture used in chemistry model for
combustion.
The Laminar flame speed correlation can be defined by Constant, Metghalchi-keck, Gulder
or Parabolic . The default option Gulder is recommended. The laminar flame speed at
stoichiometric fuel- air ratio can be obtained from the chemistry table or from literature.
Flammability limits can also be obtained from literature or experimental data
The other parameters of partially premixed combustion model in the FINE™/Open GUI are:
Fluid model
When the combustion model is activated, the fluid is automatically changed to Reactive fluid.
The Fluid Model page gives restricted access to fluid properties. Both density and temperature
field are determined through an interrogation of look-up combustion tables, as function of the
mixture fraction and its variance.
However, reference values, heat conduction and diffusivity related parameters can still be edited.
Flow model
When the combustion model is activated, the turbulence model is by default set to the standard k-ε
model. The other 2-equation turbulence models available can also be selected for combustion
simulations. However, one equation turbulence models, such as the Spalart-Allmaras model that
are available for inert flow cannot be used in conjunction with combustion modeling.
Laminar regime can also be modeled.
Boundary conditions
Combustion-dedicated boundary conditions have been introduced at inlets, with entries for the
mixture fraction and progress variable.
l Mixture fraction should range between 0 (oxidizer stream) to 1 (fuel stream).
l progress variable, the default value is set to 0.
No dedicated condition is required for the treatment of outlets, since combustion variables are
purely convected quantities.
Initial Solution
Initial data for the mixture fraction and progress variable has been introduced to the Initial
Solution menu. As a default, a value 0 is recommended for the mixture fraction and progress
variable.
FIGURE 9.5
Initial solution for partially-premixed combustion simulations
If the user activates the option Initialization with fully burned state, the combustion is looked
up for a value of the progress variable that corresponds to a fully burned state in the first N
iteration. If On finest grid is activated, the progress variable is initialized with fully burned state
after Number of iteration specified on the fine grid level.
Numerical parameters
When performing partially-premixed combustion computations, the following choices are the best
recommendation:
l In the General Parameters page under the tab General,
l set the Number of grid(s) to 3 or 4 (preferred),
l activate Coarse grid initialization.
l In the General Parameters page under the tab Advanced,
l Increase the Maximum number of cycles per grid level to 400 - 600,
l Reduce Convergence criteria on each grid level to -6,
l Possibly increase Number of sweeps on successive grid levels to 1 2 16 (3 grid levels), or
1 2 3 32 (4 grid levels)
l In the Numerical Schemes page,
l The recommended CFL number is 1.5. This is also set as default.
The partially-premixed combustion module can be used together with CPU Booster. In order to
get the best performance, the following settings are recommended when combining CPU Booster
and partially-premixed combustion:
l In the Flow Model page,
l Set the Turbulence model to k-epsilon (Extended Wall Function) or k-epsilon (Low Re
Yang-Shih, classic),
l In the Initial Solution page,
l Keep Initialization with fully burned state activated,
l Reduce the Number of iterations to 10.
l In the General Parameters page under the tab General,
l set the Number of grid(s) to 3 or 4 (preferred),
l activate Coarse grid initialization.
l In the General Parameters page under the tab Advanced,
l Increase the Maximum number of cycles per grid level to 400 - 600,
l Reduce Convergence criteria on each grid level to -6,
l Deactivate the CPU Booster during coarse grid initialization
l In the Numerical Schemes page,
l The recommended CFL number is 100. This is also set as default. In case of convergence
problem, reduce the CFL number.
l Keep the Merkle preconditioning selected.
l In the Control Variables page under the tab Advanced,
l Increase the density relaxation coefficient to 0.1 (the fifth dimension of the local expert
parameter RelaxCombVars_). In case of convergence difficulty, set the density relaxation
coefficient to 0.01 (default value).
l The relaxation coefficient of
the progress variable (the local expert parameter
RelaxCombProgVars_) should be kept as 0.1. In case of convergence difficulty, set this
relaxation coefficient to 0.01.
l In case that heat flux solid boundary condition is defined, set the local expert parameter
IterScalingFuncHeatFlux_ to 10.
l In case that the S2S radiation model is activated, set the local expert parameter RadFVM_
IterationNumber to 2.
Outputs
When performing partially- premixed combustion computations,
the following quantities are
available for output in the page Computation Control / Outputs / General under the category
Combustion.
l Comb_MixtFrac: mixture fraction
l Comb_VarianceMixtFrac: mixture fraction variance
l Comb_EnthDefect: Enthalpy defect
l Comb_TempDefect: Temperature defect
l Comb_TemperatureClipping: Flag to plot whether temperature was clipped or not. 0: Not. 1:
Yes.
l Comb_SDissipRate: scalar dissipation rate
l Comb_ProgressVariable1: progress variable
l Comb_SourceProgressVariable1: source term of the progress variable equation
When NOx post-processing is activated, the following variables can be selected for output:
l Comb_NOxPost: mass fraction (
) of NO
l Comb_SourceTermNO: source term of the mass fraction (
) equation
Depending on the lookup table specified for the non- premixed computation, the following
quantities may be available:
l LookUpTable_RHO: density of the mixture [kg/m³]
l LookUpTable_TEMP: absolute temperature of the mixture [K]
l LookUpTable_DYNVISC: dynamic viscosity of the mixture [Pa.s]
l LookUpTable_ENTHALPY: specific chemical enthalpy of the mixture [J/Kg]
l LookUpTable_CP: isobaric heat capacity of the mixture [J/K/Kg]
l LookUpTable_SCNO: first source term of the NO equation
l LookUpTable_SPNO: second source term of the NO equation
l LookUpTable_MMW: molar weight of the mixture [kg/ kmol]
l LookUpTable_QOTM: source term for OTM model, only if applicable
l LookUpTable_Temp4: absolute temperature in fourth power
l LookUpTable_LAM: laminar heat conductivity coefficient (
)
l LookUpTable_##: mass fraction of the species ##
Expert parameters
All non- interfaced advanced parameters related to the non- premixed combustion model are
accessible on the Control Variables page under the tab Advanced.
combSDissConst_: Specify the constant
for the mean scalar dissipation rate. The default
value is 2.0.
combSchmidtTurb_: The turbulent Schmidt number (default value 0.7).
RelaxCombVars_: The relaxation coefficient in combustion module. This parameter is an array
of seven dimensions, corresponding to the relaxation coefficients for the mixture fraction f, the
mixture fraction variance g, the enthalpy defect, the NO variable, the density update, the
molecular viscosity and progress variable update respectively (Default value: 1 1 1 1 0.01 1 1).
Note: The progress variable relaxation factor is used by the premixed model.
RelaxCombProgVars_: The relaxation coefficient of the progressive variable in the partially-
premixed combustion module, the default value is 0.1.
combInitHybrid_: It is used when the fully burned state is active for the Hybrid-BML partially
premixed model (Default value 1). By setting this expert parameter to 1, in the fully burned state
the flammability limits are extended and
is set to
.
combReInitProgVar_: Only used by FGM and Hybrid-BML models in conjunction with the
"Initialization with fully burned state" option. Two new reinitialization methods of the progress
variable can be selected via this expert parameter.
0: No reinitialization.
1: Reinitialization of the progress variable based on its initial condition (constant value applied to
the entire domain).
2: Reconstruction of the progress variable based on the current temperature field.
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied
to scale the heat fluxes boundary condition(s). During the course grid initialization the heat flux
(es) is/are set to zero. The idea of this switch is to ensure that the flow field and/or the combustion
process is developed before extracting/adding heat.
combEquRatioCorrCoefs_ : controls the Metghalchi-Keck coefficients [Default:2.18 -0.8 -0.16
coefficients of the
0.22]. In the Hybrid-BML/Flamelet model it allows to change
,
,
,
linear fit, for alpha and beta exponents respectively, in the equivalent ratio correlation.
iPartPremNonAdiabEffOnFlameSpeed_
the
laminar/turbulent flame speed calculation in Hybrid-BML model. By default, the value of this
expert parameter is set to 0. If active, the unburned quantities are looked-up in table accounting
for heat gains and losses
non- adiabatic
: Activate
effect
on
combTimeStep_: By default (value=0), the time step solving all the combustion equations is
determined by using the acoustic propagation speed (u+c). When setting the expert parameter
combTimeStep_ to 1, the time step is determined by using the advective propagation speed (u).
9.2
RADIATION MODELING
FINE™/Open with OpenLabs™ provides four radiation models which allow the user to include
radiation in the heat transfer simulations:
l Optically Thin Model (OTM) and the 1st order spherical harmonics model (P1-Model):
The OTM and P1-Model are good for modeling the radiative heat transfer where the media
should be considered participating. For these two radiation models, the optical thickness,
, is a good indicator of which model to choose in your problem. Here,
defined as
is a reference length of your domain is the extinction coefficient. If
, the media
can be considered to be optically thin. For this kind of problems, the OTM radiation model is
, the media can be considered to be optically thick. For this kind of
appropriate. If
problems, the P1-Model is recommended.
l Finite Volume Method (FVM): The FVM model is a more general approach than the OTM
and P1 and it is applicable to all the range of optical thicknesses. It is primary used for
modeling the radiative heat transfer where the media should be considered participating.
Applying a very low absorption coefficient, it could even be used for non-participating media
problems also.
l Surface-to-Surface model (S2S): The S2S radiation model is appropriate for modeling the
radiative heat transfer between surfaces within non-participating media.
The radiation module can be activated in the FINE™/Open GUI under the page Physical
configuration / General Properties.
For multi-block with fluid-fluid connection(s), the radiation model should be activated for all
connected fluid blocks and the same radiation model should be selected for those blocks.
After activating Radiation, the user can select a radiation model in the page Optional Models /
Radiation . In the following sections the settings related to each radiation model
in the
FINE™/Open GUI are described.
Please refer to Compatibility Information for the compatibility between radiation and other models.
9.2.1
P1-Model
The interface of the P1-model is shown in FIGURE 9.6.
FIGURE 9.6
P1-model in the FINE™/Open GUI
The first order spherical harmonics (P1-model) is based on a truncation of a Fourier series beyond
the first term (lower order approximation). The method is powerful (allowing non-black surfaces,
non-constant properties, anisotropic scattering, etc.). The model performs best for optically thick
media, while it may lead to substantially modeling errors in optically thin media with strongly
anisotropic intensity distribution; in particular, in multidimensional geometries with large aspect
ratios (i.e., long and narrow configurations) and/or when surface emission dominates over
medium emission. Although this model requires the solution of a Helmholtz (diffusion) equation
and it is more costly than OTM, it is still considered to be a computationally cheap method to
solve radiation heat transfer, especially when compared to more general methods such as the
Discrete Ordinates Method.
Radiative properties of gases are strongly dependent on the electromagnetic spectrum. Therefore
particular care must be taken to evaluate the optical properties. Due to their atomic disposition,
CO2 and H2O are the most important species to account for in radiative heat transfer simulations.
Obviously, these two gases are very important for combustion applications. The following models
can be used to evaluate the absorption coefficient of a mixture of CO2 and H2O:
Radiative species are restricted to CO2 and H2O.
l Constant: Default value is set to 1
l Planck-Mean absorption coefficient: Relevant user inputs are related to CO2 and H2O mole
fractions. Default values are respectively set to 0.1 and 0.2. In combustion simulations (Non-
premixed), the CO2 and H2O mole fractions are computed based on the mixture fraction. In
this case, no user inputs are needed.
l Weighted-Sum-of-Gray-Gases (WSGG): This approximation is based on the substitution of
the media by a number of "fictitious" gray (spectrum independent) gases. Relevant user inputs
are related to CO2 and H2O mole fractions. Default values are respectively set to 0.1 and 0.2.
In combustion simulations (Non-premixed), the CO2 and H2O mole fractions are computed
based on the mixture fraction. In this case, no user inputs are needed. This model is a good
compromise in terms of simplicity, computational cost and accuracy, and is recommended in
most circumstances.
In the context of RANS turbulence modeling, the governing equation used for radiation must be
Reynolds-averaged. The different assumptions can be made to simplify the Turbulence-Radiation
Interaction (TRI). Three models are available:
l No turbulence-radiation interaction,
l Weak turbulence-radiation interaction,
l Strong turbulence-radiation interaction.
For more information on the turbulence- radiation interaction, please refer to the theoretical
manual.
The other P1-model parameters in the FINE™/Open GUI can be found in the following menus:
Boundary conditions
For the SOLID boundaries, the following boundary conditions are available as options:
l Adiabatic
l Temperature Imposed
l Heat Flux Imposed, only in case that combustion is not activated.
l Heat Transfer coefficient Imposed, only in case that combustion is not activated
For each solid wall, the emission coefficient must be specified. It can be defined as a Constant or
a 1D profile.
Numerical parameters
When simulating radiation, the suggested CFL number is 1.5.
Outputs
All the available output variables are listed in the Computation control / Outputs page. When
the P1-model is activated, the following variables can be selected for post-processing:
Under the Radiation category:
l Incident radiation (Rad_GP1Rad)
l Absorption coefficient (Rad_AbsorptionCoefficient)
l Radiation heat flux (Rad_HeatFlux)
Under the Monitors for other variables category:
l Residual for the G equation (Residual_Rad_GP1Rad)
Under the Combustion category in case of radiation modeling in conjunction with combustion:
l Temperature defect (Comb_TempDefect). This parameter represents the difference between
) and the actual
the corresponding adiabatic temperature retrieved from the table (
temperature using the computed enthalpy defect.
l Enthalpy defect (Comb_EnthDefect)
9.2.2 OTM
The interface of the optically thin model is shown in FIGURE 9.7.
FIGURE 9.7
OTM in the FINE™/Open GUI
The Optically thin model (OTM) assumes that the emission of the media is dominant while
absorption and scattering contributions to the radiative heat
transfer are negligible. This
approximation can only be used in the context of radiation heat transfer in participating media.
The model performs best for "small" flames where the radiation heat loss is not a dominant effect.
It is computationally cheap since only a source term must be computed and added to the energy
equation.
Models available for the evaluation of optical properties restricts to Planck-mean absorption
coefficient model in case the optically thin radiation model is selected. In this case, relevant user
inputs are related to the surrounding temperature, together with CO 2 and H 2O mole fractions.
Default values are respectively set to 298K, 0.1 and 0.2. In combustion simulations (Non-
premixed), the CO2 and H2O mole fractions are computed based on the mixture fraction.
Radiative species are restricted to CO2 and H2O.
In the context of RANS turbulence modeling, the governing equation used for radiation must be
Reynolds-averaged. The different assumptions can be made to simplify the Turbulence-Radiation
Interaction (TRI). Three models have been implemented:
l No turbulence-radiation interaction,
l Weak turbulence-radiation interaction,
l Strong turbulence-radiation interaction.
For more information on the turbulence- radiation interaction, please refer to the theoretical
manual.
The other OTM model parameters in the FINE™/Open GUI can be found in the following
menus:
Boundary conditions
For the SOLID boundaries, the following boundary conditions are available as options:
l Adiabatic
l Temperature Imposed
l Heat Flux Imposed, only in case that combustion is not activated
l Heat Transfer coefficient Imposed, only in case that combustion is not activated
For each solid wall, the emission coefficient must be specified. It can be defined as a Constant or
a 1D profile.
Numerical parameters
When simulating radiation, the recommended CFL number is 1.5.
Outputs
All the available output variables are listed in the Computation control / Outputs page. When
the OTM model is activated, no quantities are available under the Radiation category.
Under the Combustion category in case of radiation modeling in conjunction with combustion:
l Temperature defect (Comb_TempDefect). This parameter represents the difference between
) and the actual
the corresponding adiabatic temperature retrieved from the table (
temperature using the computed enthalpy defect.
l Enthalpy defect (Comb_EnthDefect)
9.2.3
Finite Volume Method
The interface of finite volume method is shown in FIGURE 9.8.
FIGURE 9.8
FVM model in the FINE™/Open GUI
In the FVM method, the spatial and angular domains are, respectively, divided into a finite
number of control volumes and control solid angles. Radiative transfer equation is then integrated
over each control volume and control solid angle. Volume integrals in a partial differential
equation that contains a divergence term are converted to surface integrals, using the divergence
theorem. These terms are then evaluated as fluxes at the surfaces of each finite volume. The
inflow and outflow of radiant energy across a control-volume face are balanced with attenuation
and augmentation of radiant energy within a control volume and control solid angle. By default
the solid angle θ in polar direction and ϕ azimuthal direction is 4 respectively. The values of solid
angles can changed by modifying the expert parameter RadFVM_Ntheta and RadFVM_Nphi
respectively.The expert parameter Rad_ RelaxHeatFluxBC controls the relaxation factor for
radiative heat flux at the boundaries and this parameter can relaxed to reduce the intensity of
radiated heat flux at boundaries.
Radiative properties of gases are strongly dependent on the electromagnetic spectrum. Therefore
particular care must be taken to evaluate the optical properties. Due to their atomic disposition,
CO2 and H2O are the most important species to account for in radiative heat transfer simulations.
Obviously, these two gases are very important for combustion applications. The following models
can be used to evaluate the absorption coefficient of a mixture of CO2 and H2O:
Radiative species are restricted to CO2 and H2O.
l Constant: Default value is set to 1
l Planck-Mean absorption coefficient: Relevant user inputs are related to CO2 and H2O mole
fractions. Default values are respectively set to 0.1 and 0.2. In combustion simulations (Non-
premixed), the CO2 and H2O mole fractions are computed based on the mixture fraction. In
this case, no user inputs are needed.
l Weighted-Sum-of-Gray-Gases (WSGG): This approximation is based on the substitution of
the media by a number of "fictitious" gray (spectrum independent) gases. Relevant user inputs
are related to CO2 and H2O mole fractions. Default values are respectively set to 0.1 and 0.2.
In combustion simulations (Non-premixed), the CO2 and H2O mole fractions are computed
based on the mixture fraction. In this case, no user inputs are needed. This model is a good
compromise in terms of simplicity, computational cost and accuracy, and is recommended in
most circumstances.
In the context of RANS turbulence modeling, the governing equation used for radiation must be
Reynolds-averaged. The different assumptions can be made to simplify the Turbulence-Radiation
Interaction (TRI). Three models are available:
l No turbulence-radiation interaction,
l Weak turbulence-radiation interaction,
l Strong turbulence-radiation interaction.
For more information on the turbulence- radiation interaction, please refer to the theoretical
manual.
The other FVM model parameters in the FINE™/Open GUI can be found in the following
menus:
Boundary conditions
For the SOLID boundaries, the following boundary conditions are available as options:
l Adiabatic
l Temperature Imposed
l Heat Flux Imposed, only in case that combustion is not activated.
For each solid wall, the emission coefficient must be specified. It can be defined as a Constant or
a 1D profile.
Numerical parameters
Recommendations for Global Numerical Parameters are the same to the ones suggested for
combustion modeling.
Outputs
All the available output variables are listed in the Computation control / Outputs page. When
the FVM model is activated, the following variables can be selected for post-processing:
Under the Radiation category:
l Incident radiation (Rad_GFVMRad)
l Absorption coefficient (Rad_AbsorptionCoefficient)
l Radiation heat flux (Rad_HeatFlux)
l Radiation Surface heat flux (Rad_SurRadiationHeatFlux)
Under the Monitors for other variables category:
l Residual for the Radiation Inentsity equation (Residual_Rad_GFVMRad)
Under the Combustion category in case of radiation modeling in conjunction with combustion:
l Temperature defect (Comb_TempDefect). This parameter represents the difference between
) and the actual
the corresponding adiabatic temperature retrieved from the table (
temperature using the computed enthalpy defect.
l Enthalpy defect (Comb_EnthDefect)
9.2.4
S2S Model
Introduction
In many engineering applications the exchange of radiative energy between surfaces is virtually
unaffected by the medium that separates the surfaces. Such radiative heat transfer is referred to as
the surface-to-surface radiation.
The main assumption of the Surface-to-Surface (S2S) radiation model in FINE™/Open with
OpenLabs™ is that the radiative heat transfer transports in non-participating media, and all the
surfaces are gray and diffuse. Emissivity and absorptivity of a gray surface are independent of the
wavelength. The energy exchange between two surfaces depends in part on their size, separation
distance, and orientation. These parameters are accounted for by a geometric function called
"view factor''. In FINE™/Open with OpenLabs™, the Stochastic Ray Tracing method is used to
calculate the view factors.
The following limitations apply for the S2S radiation model:
1. The S2S model is not compatible with periodic boundaries and mirrors that are considered as
participating surfaces. Which means, the radiosity cannot be transformed/ reflected on the
surfaces. In 2D cases, the periodic or mirror boundaries in the virtual direction should not be
activated.
2. It is not yet available to impose external radiation, such as solar radiation.
3. The full non matching mixing plane method for radiation on fluid-fluid R/S connections is not
available.
S2S model in the GUI
When the Surface to surface model is selected in the Optional Models / Radiation page, the
radiation parameters dialog box is shown below.
The parameters in the S2S radiation page must be identical for all the blocks where the S2S
radiation is activated.
First, the user should define how to compute the view factor. The view factor can be calculated or
read from file:
l Calculate: the view factor will be calculated based on the mesh and the radiation settings. In
case of 2D configurations, the option 2D has to be activated and the Virtual direction
(perpendicular to the 2D plane) has to be specified. After the computation is launched, the
view factor will be calculated and saved in the computation folder with the extension .bvf.
For 2D axis-symmetric simulations, the middle-θ plane must be placed in xz or yz plane so that
the Virtual direction can be y or x.
l Read from file : the user specifies a view factor file computed by FINE™/Open with
OpenLabs™. When reading view factor from a file, the format and settings of the view factor
will be checked automatically. If they are not compatible with the current computation, the
view factor calculation will be launched automatically.
In many cases the radiative heat transfer is only considered in a part of the domain. The concept
of Partial enclosure is introduced to disable the radiation calculation of some boundaries. In case
of Partial enclosure, the average temperature of the non-participating boundaries must be given.
When Partial enclosure is activated, the periodic and mirror boundaries are automatically
disabled for the radiation calculation.
Partial enclosure must be activated and a surrounding temperature must be given if the
activated radiation surfaces don't form an enclosure.
The other S2S radiation model parameters in the FINE™/Open GUI can be found in the
following pages:
Boundary conditions
In the Boundary Conditions / Boundary Conditions page, the radiation boundary condition
must be defined at each boundary. The user needs to select Activate patch for S2S radiation for
the boundaries that participate in radiation. For FNMB fluid-fluid connections, if both sides are
not selected, it is transparent to radiation. If one or both sides are selected, it is opaque to radiation.
Note: When one side of a FNMB connection contains multiple patches, they have to be treated in
the same way: either active or non-active.
For 2D/2D axis- symmetric simulations, the option Activate patch for S2S radiation cannot be
activated for the boundaries in the third direction.
For each solid boundary, the Emission coefficient should be specified. It can be a constant or a
1D profile  for the data format).
In case of partial enclosure, the option Activate patch for S2S radiation should be activated
only for the radiative boundaries.
When simulating S2S radiation, the FNMB connection can connect a stationary block and a
rotating block  for more information on Multiple Reference
Frame).
l If the rotating block is a fluid block, the "frozen rotor" method is applied for radiation. The
view factor is calculated between the activated surfaces of non-rotating block and the activated
surfaces of the rotating block based on their current positions.
l If the rotating block is a solid block, the "mixing plane" method is applied for radiation. The
radiative heat flux is averaged over the tangential direction.
Outputs
All the available output variables are listed in the Computation control / Outputs page. When
the S2S model is activated, the following variables can be selected for post-processing:
Under the Radiation category:
l Surface radiation heat flux (Rad_SurfRadiationHeatFlux)
9.2.5
Advanced Parameters for Radiation Model
Non-interfaced Expert Parameters
All non-interfaced advanced parameters related to the radiation model are accessible on the
Control Variables page, in the Advanced tab.
P1-model
GP1Free_: Initial value for the G-field of the P1 radiation model.
S2S model
S2S_nbRayPerFace_: The number of the rays per face used in view factor calculation. The
drawback of the stochastic ray tracing method is that the accuracy is dependent on the number of
the rays. In some special cases, the user can increase the value of the expert parameter S2S_
nbRayPerFace_ to improve the accuracy. Note, the computational cost solving the view factors is
proportional to the number of the rays.
S2S_iLevelCoarse_: The S2S radiation model can be quite memory and CPU consuming. A
coarsening of the boundaries, based on the agglomerated mesh, has been introduced in the
FINE™/Open solver in order to reduce the computational cost. The choice of the multigrid level
can be set through the expert parameter S2S_iLevelCoarse_. Note, the value of 0 means that the
view factor is computed in the coarsest grid level and 1 means the second coarsest level.
S2S_NbIter_: The radiosity equations will be solved at every S2S_NbIter_ iterations.
S2S_BCCycle_: Number of cycles of solving the radiosity equation at each Runge-Kutta stage.
In each cycle, the flow solver solve the radiosity equation based on the boundary temperature, and
then updates the boundary temperature. Iterating more cycles means deeper convergence of the
coupling but needs more CPU time.
S2S_ InnerIter_ : The radiosity equation is solved by a Gauss- Seidel iteration. The expert
parameter S2S_InnerIter_ is used to define the number of the Gauss-Seidel iterations.
S2S_RelaxFactor_: The relaxation factor used in the Gauss-Seidel iteration solving the radiosity
equation.
FVM model
RadFVM_ AreMirrorsSpecular : FVM for radiative heat transfer at mirror boundaries as
Specular or Diffuse.
0: Diffuse
1 (default): Specular.
RadFVM_ FixedIterationNumber : Use the criterion of maximum number of Gauss- Seidel
iterations to solve the radiative transfer equation. (default value 1)
RadFVM_IterationNumber: Number of Gauss-Seidel iterations to solve the radiative transfer
equation at each global iteration (default value 1).
RadFVM_NbIter: Iteration frequency to compute radiation heat transfer with FVM. Number of
flow iterations per radiation iteration (default value 1: means that they are synchronized )
RadFVM_NodalInt_AngularErrorTol: Tolarance to solve the radiative transfer equation at
each iteration (default value 0.1)
RadFVM_Nphi: Angular discretization in Phi direction (default value 4).
RadFVM_Ntheta: Angular discretization in Theta direction (default value 4).
Rad_AnisotropicScatteringCoeff: Anisotropic scattering coefficient (default value 0.0).
If Rad_ScatteringModel = 2; this parameter is the linear anisotropically scattering coefficient
If Rad_ScatteringModel = 4; this parameter is the asymmetry scattering coefficient of the Henyey-
Greenstein phase function
Rad_ RelaxHeatFluxBC : Relaxation factor for the radiation heat flux calculation at
boundaries (default value 0.2)
the
Rad_ScatteringCoeffValue: Scattering coefficient value (default value 0.0)
Rad_ScatteringModel: Scattering model.
0 (default): No scattering model
1: Linear Isotropic scattering
2: Linear Anisotropic scattering
3: Rayleigh scattering
4: Henyey-Greenstein scattering
5: F1 Forward scattering phase function
6: F2 Forward scattering phase function
7: B1 Backward scattering phase function
8: B2 Backward scattering phase function
9.3
POROUS MEDIA MODEL
Introduction
A porous medium is a solid permeated by an interconnected network of pores filled with a fluid.
Usually both the solid matrix and the pore network are assumed to be continuous, so as to form
two interpenetrating continua such as in a sponge. Many natural substances such as rocks and
soils, and man made materials such as foams and ceramics can be considered as porous media.
When simulating the flow in porous medium the user has to use a porous media model because
the geometry is too complex to resolve with a grid.
The Porous Media Model in FINE™/Open with OpenLabs™ allows the user to simulate the
flow in porous media. The source terms are added in both the momentum and energy equations
for the porous media flow simulation with the objective to mimic:
l Pressure drop through the medium
l Thermal effects due to heat exchanges between the medium and the fluid
In the next section the settings related to the porous media model in the FINE™/Open GUI are
described.
Porous Media Model in the FINE™/Open GUI
The porous media model can be directly activated from the FINE™/Open GUI under Physical
configuration. This model can be activated for each block individually. The interface of the
porous media model parameters is shown in FIGURE 9.9.
FIGURE 9.9
Porous media page in FINE™/Open with OpenLabs™
Three models are available to model the pressure drop through the porous media:
l Darcy law : for low Reynolds number regimes. When selecting the Darcy law , the K'
coefficient can be estimated by using the Carman- Kozeny formula or directly inputted
(homogeneous or non-homogeneous).
l Carman-Kozeny formula: if the option Carman-Kozeny formula is selected, the user has to
input the Porosity, defined as the volume fraction of the voids from the solid matrix, and the
Specific area, defined as the surface area of pores per unit volume of the solid matrix. In
addition, a preferential direction for the flow in the porous media can be set up. The
direction is specified by a vector in the Cartesian frame. In case that the flow direction is
specified, the fluid will be forced to flow along the specified direction.
l User defined (homogeneous): if the option User defined (homogeneous) is selected, the
user has to input the K' coefficient. In addition, a preferential direction for the flow in the
porous media can be set up. The direction is specified by a vector in the Cartesian frame. In
case that the flow direction is specified, the fluid will be forced to flow along the specified
direction.
l User defined (non- homogeneous): if the option User defined (non- homogeneous) is
selected, the user has to specify the local frame of reference (ξ,η,ζ) and input the K'
coefficient in each direction. For the definition of the local frame of reference (ξ,η,ζ), the
user needs to specify only the ξ and >η directions in Cartesian frame. The flow solver will
compute the third orthogonal direction ζ.
l Ergun law: for high Reynolds number regimes. When selecting the Ergun law, the K' and K"
coefficient can be estimated by using the Carman- Kozeny formula or directly inputted
(homogeneous or non-homogeneous).
l Carman-Kozeny formula: if the option Carman-Kozeny formula is selected, the user has to
input the Porosity, defined as the volume fraction of the voids from the solid matrix, and the
Specific area, defined as the surface area of pores per unit volume of the solid matrix. The
pore's surface can be treated as Smooth surface or Rough surface. In addition, a preferential
direction for the flow in the porous media can be set up. The direction is specified by a
vector in the Cartesian frame. In case that the flow direction is specified, the fluid will be
forced to flow along the specified direction.
l User defined (homogeneous): if the option User defined (homogeneous) is selected, the
user has to input the K' and K" coefficients. In addition, a preferential direction for the flow
in the porous media can be set up. The direction is specified by a vector in the Cartesian
frame. In case that the flow direction is specified, the fluid will be forced to flow along the
specified direction.
l User defined (non- homogeneous): if the option User defined (non- homogeneous) is
selected, the user has to specify the local frame of reference (ξ,η,ζ) and input the K' and K"
coefficients in each direction. For the definition of the local frame of reference (ξ,η,ζ), the
user needs to specify only the ξ and η directions in Cartesian frame. The flow solver will
compute the third orthogonal direction ζ.
l Integral law : When selecting the Integral law ,
the user needs to input the following
parameters:
Proportionality constant CIL: describing the pressure drop over the porous media,
Thickness L [m]: the thickness of the porous media,
Area ratio Atotal/Apassage: where Apassage [m²] is defining the effective area through which the
fluid flows and Atotal [m²] is defining the sum of the area offered to the flow and blocked by
inclusions.
Exponent n: a user defined exponent (default 2.0).
Thermal effects can be included so as to account for the heat exchange between the media and the
fluid. The user has to specify the following parameters for the thermal effects:
l Heat transfer coefficient: the heat transfer coefficient between the fluid and the media.
l Specific area surface: the surface of exchange.
l Skin temperature: the temperature at the surface of the media, can be constant value or defined
by a profile.
The present model are valid assuming the porous media is considered isotropic and no highly non-
linear heat transfer phenomena occur. In particular, heat transfer phenomena are properly modeled as
long as their effects on the density and pressure remains limited (liquids).
As explained previously, the parameters are set by block. It is possible to select several blocks
(multiselection) by pressing <CTRL> key and left clicking the mouse. In this case, the parameters
settings apply to all selected blocks. If several blocks are selected, any parameters, which are not
identical for all selected blocks, are highlighted in red, with no value. Then if a value is set, it
applies to all blocks from the selection and the entry is unhighlighted.
9.4
COUPLING
Multi-physics problems, including Fluid-Structure Interaction (FSI), are becoming more important
for industrial applications. FINE™/Open with OpenLabs™ has integrated several modules,
which allows the user to perform multi-physics simulations, including thermal and mechanical
simulations.
9.4.1
Coupling with MpCCI
Introduction
For multi-physics problems, many commercial codes, such as FINE™/Open with OpenLabs™
and Abaqus etc., can be used to solve only one aspect of the physical problem. One way to
perform the multi-physics simulations is to use two or more dedicated codes coupled through the
exchange of data.
MpCCI (Mesh-based parallel Code Coupling Interface) is a coupling interface developed by the
Fraunhofer Institute (SCAI) and used to perform multi-physics simulations. It consists in a server,
which handles physical quantities exchanges between two or more heterogeneous solvers (for
example a Computational Fluid Dynamics solver and a solid mechanics solver).
FINE™/Open with OpenLabs™ includes a MpCCI code adapter in order to solve the thermal
and/or mechanical coupling problems. The adapter takes in charge all communication processes
with the MpCCI coupling server. About the settings in MpCCI, please refer to the MpCCI
manual. For the coupling quantities with MpCCI, FINE™/Open with OpenLabs™ can send the
following quantities:
l Global values:
l Physical time;
l Time step count;
l Time step size;
l Reference pressure.
l Face node values:
l Absolute pressure;
l Overpressure
l Density
l Velocity;
l Temperature.
l Face element values:
l Absolute pressure;
l Overpressure
l Density
l Velocity;
l Temperature;
l Heat flux;
l Relative wall force.
FINE™/Open with OpenLabs™ can receive:
l Face node values:
l Displacements;
l Nodal position.
l Temperature
l Face element values:
l Temperature;
The limitations coupling with MpCCI are as follows:
l Only surfaces (3D) and lines (2D) coupling are supported by FINE™/Open with
OpenLabs™. Volume coupling is not yet supported.
The coupling with MpCCI uses the mesh deformation module. For the limitations related to mesh
deformation, see Mesh Deformation Methods section.
The Settings in the FINE™/Open GUI
The Coupling with MpCCI can be accessed in the Optional Models / Coupling page.
Selecting Coupling with MpCCI in the option Coupling method, then the user will be able to
set the parameters for the MpCCI code adapter. The user needs to specify the reference pressure
for the exchange of coupling data, which is used to calculate quantities such as overpressure
(absolute pressure - reference pressure).
In order to couple with MpCCI, the user needs to activate the option Coupling activation for the
coupling solid boundaries. Three kinds of coupling simulations can be performed:
l Thermal coupling: the wall heat load (temperature or heat flux) is sent to structural code, the
wall temperature is sent to the FINE™/Open solver;
Thermal coupling is only compatible with MpCCI v4.
l Mechanical coupling: the fluid loads (pressure or forces) are sent to structural code, the solid
deformation (position or displacement) is sent to the FINE™/Open solver;
l Thermo-mechanical coupling: both the fluid loads (pressure or forces) and the wall heat load
(temperature or heat flux) are sent to structural code, the solid deformation (position or
displacement) and the wall temperature are sent to the FINE™/Open solver.
Thermo-mechanical coupling is only allowed for unsteady computations.
The coupled boundaries can be moving or fixed:
l Moving grid points: The points of the selected boundary are moving. In this case, a mesh
deformation module, which is dedicated to the applications related to Fluid- Structure
Interaction (FSI), is automatically activated. The mesh deformation method is selected through
the expert parameter mov_iMovingGridMeth_, see Advanced Parameters for Coupling with
MpCCI for more detail.
l Fixed grid points: The points of the selected boundary are fixed.
Advanced Parameters for Coupling with MpCCI
The following non- interfaced advanced parameters related to Coupling with MpCCI are
available:
iMpCCISteadyMode_: For the FSI simulations, the CFD solver computes a transient solution.
However, a special steady coupling mode is implemented in the FINE™/Open solver. It does not
use the steady solver but forces the unsteady solver to compute a steady solution. To force such a
computation, one has to set the parameter iMpCCISteadyMode_ to 1 instead of 0.
mpcci_Relax_: In order to avoid convergence problems for steady computations, the received
temperature can be relaxed through the following formula:
where
and
are the previous temperature and the received temperature,
respectively. The coefficient
is the relaxation parameter. By default, the relaxation
parameter is equal to 1.
iMpCCIIterCoupling_: for steady computations, the data exchange is performed at the iteration
number N if (N / iMpCCIIterCoupling_)=0
iMpCCIzSize_: This parameter is used to specify the size of the cell in the third direction (z) in
2D cases. By default, it is 1.0 [m].
9.4.2
Coupling with modal approach
Introduction
FINE™/Open with OpenLabs™ includes a modal coupling module in order to perform Fluid-
Structure Interaction (FSI) simulations. For modal coupling simulations, an external structural
analysis software should be used first to compute the modal shapes and the eigen frequencies of
the structure. With the computed modal shapes and the eigen frequencies, the FINE™/Open flow
solver will consider the interaction between the flow and the structure and compute the
deformation of the structure by solving the modal equations.
The limitations on the modal coupling are as follows:
l For unsteady computation, the time step should be less than one third of the period of the
highest mode to avoid divergence.
l Structure file containing mode shape definition must be written in SI units.
The coupling with modal approach uses the mesh deformation module. For the limitations related
to mesh deformation, see Mesh deformation methods section.
The Modal Coupling in the FINE™/Open GUI
The Coupling with modal approach can be accessed in the Optional Models / Coupling page.
FIGURE 9.10
Coupling with modal approach
Selecting Coupling with modal approach in the option Coupling method, then the user will be
able to set the parameters for the modal coupling. The user needs to specify the reference pressure
for the exchange of coupling data, which is used to calculate quantities such as overpressure
(absolute pressure - reference pressure).
All solid patches and groups in the fluid mesh are listed on the left of the page. The user has to do
the settings as follows:
1. select the patches/groups that belong to the same structure. One structure can consist of
multiple patches/groups. To select multiple patches/groups, keep the key <Ctrl> pressed and
left-click on the patches/groups.
2. activate the option Coupling activation and select the structure (by Structure name) where
the patches/groups are located.
At the first time the coupling is activated for a patch, the structure name is <Select a
configuration> by default. In this case, the user must select "New configuration..." item (only
choice) from the drop-down menu. Then, the modal structure configuration window appears.
FIGURE 9.11
Structure properties
The user has to specify a Structure name and set the corresponding parameters.
A Structure file, including the modal properties and the initial deformation (optional), has to
be imposed for each structure. The modal properties (eigen frequencies and modes shapes) are
needed by the flow solver in order to compute the elastic deformation of the structures. These
properties can be computed by a CSM code or measured experimentally. As the modal
resolution is a linear method, an initial deformation can be specified. This is useful to take into
account non-linear effects independent of fluid load, such as centrifugal load effect.
The structure file must be written in ASCII format. First, this file includes the number of
dimensions of the structure, the number of modes, the number of structure nodes at which the
modes are defined and a flag to specify if an initial deformation is specified. Then, the eigen
frequencies are listed in increasing order. The frequencies have to be written in Hz. Finally, the
initial deformation and the mode shape information are written node by node. For each node
one line contains the three (or two for 2D computation) coordinates, the initial deformation (if
the parameter Initial deformation is set to 1) and the components of each mode sorted in
increasing frequency order. The coordinates and the mode shapes have to be written in SI unit
system and in cartesian system. For mode shape the conversion factor is the inverse of the
square root of mass conversion factor.
Mode shape must be scaled for a generalized mass equal to 1.
FIGURE 9.12
The format of structure file
After specifying the structure file, the Number of Modes used in the computation must be
specified. The number of used modes must be less than or equal to the number of modes
defined in the structure file. For each used mode, a damping coefficient needs to be specified.
These damping coefficients will be used to solve the modal equations and compute the
deformation of the structures. The user can select one or multiple modes by keeping the key
<Ctrl> pressed, or select All or None modes in the list by using the button Select, then set the
damping coefficient for all selected modes.
Note that only used modal structures (referenced by a patch) are saved. This means that during the
computation setup, the user can define several modal structures and each of them are selectable
(even those that are not used). But when the project is saved and re-open, modal structures that
were not used are lost.
3. After selecting the structure (by Structure name), the button Edit is available to view or edit
the structure properties, as shown in FIGURE 9.11.
Output
With the modal approach, an output file is generated with the extension ".generalized_motion".
This file has the following format:
l for steady computations: the iteration number, q for each mode and each structure defined in
the interface, where q is the generalized displacement.
l for unsteady computations: the time step, q,
,
for each mode and each structure defined
in the interface, where q is the generalized displacement.
9.4.3
Coupling with Oofelie
Introduction
A very important concept for multi-physics unsteady problems is the strong coupling. Such a
coupling requires that the solutions for all the physics must be synchronized at every time step.
When using two dedicated codes coupled through the exchange of data (staggered approach),
strong coupling can be achieved if several fluid and structure computations are performed at every
time step, until synchronization is obtained between the solutions (Strongly-Coupled Staggered
Approach). The disadvantage of such a method is that, as several computations are done at each
time step, the computational cost is much larger. However, strong coupling allows to ensure a
better energy and momentum conservation at the fluid-structure interfaces, provides second order
time accuracy and increases the stability of the coupled algorithm. It is then highly recommended
for problems with large deformations where both domains influence each other, especially with
quite large time step.
FINE™/FSI- OOFELIE is a fully integrated solution for strongly coupled Fluid- Structure
Interaction (FSI) simulations, which combines the CSM software Oofelie developed by Open
Engineering and the CFD software FINE™/Open with OpenLabs™ developed by NUMECA
International. The exchange of information at the coupled interfaces is done by using the MPI
(Message Passing Interface) protocol. With FINE™/FSI-OOFELIE, the user is able to get faster
convergence and more accurate results for the thermal and/or mechanical coupling problems. To
get the FINE™/FSI-OOFELIE package, please contact your local support office.
Within FINE™/Open with OpenLabs™, a module Coupling with Oofelie is included in order to
couple with Oofelie. In the following section, the interface coupling with Oofelie will be
explained.
The limitations coupling with Oofelie are as follows:
l This feature is not compatible with multi-block projects.
l This feature is not applicable for projects with R/S or FNMB connections.
The coupling with Oofelie uses the mesh deformation module. For the limitations related to mesh
deformation, see Mesh deformation methods section.
The Settings in the FINE™/Open GUI
The Coupling with Oofelie can be accessed in the Optional Models / Coupling page.
Selecting Coupling with Oofelie in the option Coupling method, then the user will be able to set
the parameters for the coupling.
First, the user has to specify the Oofelie coupling file (with the extension .stl.fsi). The Oofelie
coupling file, generated by Oofelie, contains all the information of the coupled boundaries in the
fluid domain. All the boundaries coupled with Oofelie are hidden in the interface. The user does
not need to set anything for the coupled boundaries.
For the uncoupled boundaries, the deformation type can be defined through the interface:
l Fixed grid point: the points of the selected boundary are fixed during the iteration.
l Floating grid point: The points of the selected boundary can move. That means the boundary
may deform during the iteration. This option is usually activated for the boundaries that
connect to the coupled boundaries in order to avoid negative cell.
l Free grid point: The points of the selected boundary can move. That means the boundary
may deform during the iteration. This option is usually activated for the boundaries that
connect to the coupled boundaries in order to avoid negative cell.
Floating grid point and Free grid point deformation types will give exactly the same results for the
RBF mesh deformation technique. There will be a difference for the treatment of sliding nodes
introduced in the IDW mesh deformation technique (feature still in BETA).
9.4.4 Rigid Motion
Introduction
The Rigid Motion model allows to simulate the flow in a domain where the solid boundary can
move according to a translation law.
The limitations for the Rigid Motion model are as follows:
l For applications with periodic boundary conditions,
the motion is restricted to axial
displacement (along z-axis).
l Not compatible with PERNM and periodic FNMB.
The Rigid Motion model uses the mesh deformation module. For the limitations related to mesh
deformation, see Mesh deformation methods section.
The Settings in the FINE™/Open GUI
The Rigid Motion can be accessed in the Optional Models / Coupling page.
The Coupling activation has to be enabled for the moving solid boundaries. The motion of the
solid boundary is defined through OpenLabs™. Three keywords to define the translating motion
are available in the constant list:
l FSI_RigidTranslation_X_
l FSI_RigidTranslation_Y_
l FSI_RigidTranslation_Z_
The translation motion is defined relatively to the original position of the geometry. The unit of
the displacement is the same as the unit of the mesh.
Here is an example of a lab where the motion is a translation along the z-axis and fluctuates over
time:
For the uncoupled boundaries, the deformation type can be defined through the interface:
l Fixed grid point: the points of the selected boundary are fixed during the iteration.
l Floating grid point: The points of the selected boundary can move. That means the boundary
may deform during the iteration. This option is usually activated for the boundaries that
connect to the coupled boundaries in order to avoid negative cell.
l Free grid point: The points of the selected boundary can move. That means the boundary
may deform during the iteration. This option is usually activated for the boundaries that
connect to the coupled boundaries in order to avoid negative cell.
Floating grid point and Free grid point deformation types will give exactly the same results for
the RBF mesh deformation technique. There will be a difference for the treatment of sliding nodes
introduced in the IDW mesh deformation technique (feature still in BETA).
9.4.5 Mesh deformation methods
Introduction
Mesh deformation plays a crucial role in the analysis of multi-physics problems that involve
moving bodies and domain with dynamic boundaries. For example, in Fluid-Structure Interaction
(FSI), the fluid mesh has to be deformed at each time step according to the displacements
computed by the structural solver at the interface of the fluid domain and solid domain.
In FINE™/Open with OpenLabs™, two kinds of mesh deformation methods are available: mesh
deformation based on quaternions and mesh deformation based on Radial Basis Function (RBF).
The user can select the method through the expert parameter mov_iMovingGridMeth_. By
default, the mesh deformation based on Radial Basis Function (RBF) is used.
The limitations of the mesh deformation module are:
l Only available for mono-block projects.
l FNMB is not taken into account during the process.
l Not compatible with HEXPRESS™/Hybrid mesh.
l Mesh deformation module is not compatible with the coarse grid initialization feature. The
coupled simulations are suggested to start from a pre-computation solution (without coupling).
Mesh deformation based on quaternions
In this method, the mesh deformation is based on the use of quaternions. The methodology works
well when displacements of the boundaries are small but in case of large displacements, the
methodology fails, especially when considering meshes with high aspect ratio and viscous layers.
The approach to mesh deformation includes the following several stages:
First, the initial deformation specified at every point of the boundaries is converted and divided
into two components: translation and rotation. Translation is represented in terms of Cartesian
displacement vectors, while rotation is described in terms of quaternions.
Once the initial deformation is converted into translations and rotations of the boundary faces, an
interpolation procedure is used to propagate the deformation into the volume mesh. The
interpolation procedure is based on weighted Laplacian smoothing approach.
Finally, the interpolated data is converted back into the respective set of Cartesian displacement
vectors, which are used for final relocation of the mesh points.
Radial Basis Functions
The mesh deformation based on quaternions works only when the mesh deformation is very
small. When performing a mechanical coupling simulation, the structure deformation may be very
large. In this case, the mesh deformation method using Radial Basis Function (RBF) can be used.
The RBF method gives deformed meshes keeping very good quality even for large deformation.
For more information on the RBF method, please refer to the theoretical manual.
The main limitations for the RBF mesh deformation method are as follows:
l The mesh deformation method using RBF is not compatible with:
l FNMB connections,
l SNG boundary condition,
l Upwind scheme,
l Rigid body motion,
l Adaptive wall.
Please note that memory usage can become higher when the number of boundary nodes increases.
Expert Parameters
The following non-interfaced advanced parameters related to the mesh deformation module are
available:
mov_iMovingGridMeth_: Choice of the mesh deformation procedure:
1: Mesh deformation based on the use of quaternions.
2 (default): Mesh deformation based on the use of Radial Basis Function (RBF).
The parameters related to the mesh deformation with RBF:
mov_iMatSave_: controls the solving of the mesh deformation matrix in RBF.
0 (default): the matrix will be recomputed automatically.
1: the flow solver will try to read and use the file "projectName.mat" in the computation folder. If
the file format is not correct or if the size of the matrix does not correspond to the mesh, the flow
solver will automatically recompute the mesh deformation matrix.
In case of ISVMAT=2, an inverse matrix computed in single precision can not be used in a
double precision computation. Otherwise, negative cells may appear after mesh deformation.
mov_rad_: Radius of the support of the Wendland function (RBF).
mov_rbf_: Function used for RBF mesh deformation:
1: Wendland function.
2 (default): Thin plate spline.
mov_iFromInitMesh_: A way to improve the CPU performance of the methodology is, for a
given time, to perform deformation starting from the initial mesh instead of starting from the mesh
computed at the previous time step. Indeed, if we choose to perform the deformation from the
initial mesh, the matrix of the linear system is constant during all computation and can be inverted
one time and stored in a file. The expert parameter mov_iFromInitMesh_ controls if deformation
is performed starting from the initial mesh:
0: False
1 (default): True
mov_iLevelCoarse_: The RBF mesh deformation methodology can be quite memory and CPU
consuming. If one considers a computational domain which contains few thousands of boundary
nodes, for example 25 000 boundary nodes, therefore the memory required to store half of the
matrix (since it is symmetric) is 4.5 GigaBytes. Moreover, the resolution of the linear system will
take several hours, which is not acceptable for an unsteady computation with thousands of
physical time-steps. A coarsening of the boundaries has been introduced in the FINE™/Open
solver in order to reduce the size of the system and therefore increase the speed of the mesh
deformation procedure. The coarsening consists at taking into account the nodes that belong to a
given multigrid level. The choice of the multigrid level can be set through the expert parameter
mov_iLevelCoarse_. By default, mov_iLevelCoarse_=3. This means that the mesh deformation is
performed in the finest grid level (with 4 multigrid levels). When setting mov_iLevelCoarse_=0,
the mesh deformation will be performed in the coarsest grid level.
9.5
FLUID-PARTICLE INTERACTION
The Fluid-Particle Interaction module in FINE™/Open with OpenLabs™ allows the user to
simulate dilute inertial dispersed two-phase flows by using a Lagrangian particle tracking method.
What are dilute inertial two-phase flows?
First, the dilute inertial two-phase flows are characterized by the presence of two different phases
(gas-solid, gas-liquid, liquid-solid or liquid-gas). These flows can be characterized by the density
ratio of the continuous and dispersed phase. If the density ratio is much larger than one, then the
drag force is often the only force considered to act on the particles or droplets, as it is much larger
than all other forces. On the other hand, if the density ratio is smaller than one (bubbles) then the
added mass force becomes very important. It should be noted that the Lagrangian module in
FINE™/Open with OpenLabs™ has been developed for spray applications, thus for a density
ration much larger than one.
Second, the second phase must be dispersed, i.e. consisting of single isolated elements, like
particles, droplets or bubbles (or everything that can be modeled by one of these). For example,
this method is not applicable to mixing of two fluids.
Third, the module has been developed for dilute cases, which means that the volume fraction of
the dispersed phase should be small (smaller than 0.0001 for the theoretical limit). If this limit is
exceeded, additional physical effects become important. The influence of the dispersed phase on
the continuous phase cannot be neglected anymore and two-way coupling should be used. Two-
way coupling is included in FINE™/Open with OpenLabs™ and can be activated by selection in
the GUI.
important physical effect, which is not accounted for
Another
in FINE™/Open with
OpenLabs™, is particle/droplet collisions, coalescence or agglomeration. These effects are not
negligible for higher volume fractions. Nevertheless, the Lagrangian module in FINE™/Open
with OpenLabs™ might also be used for higher volume fraction if this lack of modeling is kept in
mind. However, much larger values (larger than 0.1) for the volume fraction might lead to
stability problems of the two-way coupling. These regimes are largely out of the scope of dilute
flows.
Fourth, the dispersed phase might possess its own inertia. In function of the relative velocity at the
inlet between the continuous and disperse phase, different sized or weighted particles adapt with
different speed to the fluid flow field. Very small particles injected at the same speed as the fluid
will follow very much the fluid flow, whereas particles with high inertia might take completely
different trajectories across the fluid flow compared to a fluid element.
The physical effects accounted for in FINE™/Open with OpenLabs™
In FINE™/Open with OpenLabs™, the following physical effects are accounted for:
l Polydispersion: Particles of different sizes (or with different masses) can be followed through
the flow. This is of particular importance for inertia effects, as particles might react very
differently in function of their weight. Low inertia particles will provide a solution field very
similar to the one predicted the Eulerian solver, while high inertia particles will show distinct
different trajectories.
l The drag force is the most dominant particle force if the particle-fluid density ratio is high.
Two different correlations can be used for the drag coefficient: the Stokes drag for low particle
Reynolds number particles and the drag correction from Schiller & Naumann for higher
particle Reynolds numbers.
l Other forces in FINE™/Open with OpenLabs™ include gravity, buoyancy, pressure gradient
and added mass.
l Turbulent dispersion is taken into account, considering the inertia of the particles. The
dispersion model imitates the influence of turbulence on the particle trajectories in function of
their inertia.
l Wall collisions: When the particles reach the walls, the particles can be deposited on the wall
(Deposition ) or re-bounce from the wall (Re-bound ). In case of re-bound, a reflection
coefficient can be set for each solid wall. Its default value is 1.0 and it indicates that the
collision is elastic, i.e. there is no energy dissipation during the collision. If this value is
lowered, the wall normal velocity component of the particles will be altered, such that it re-
bounces with a lower normal velocity.
l Heating/Cooling of droplet is subdivided into a convective heating part and a radiative heating
part. The radiative heating part is not considered in this model but could be added to the
convective heating. In the droplet heating/cooling model the droplet temperature is uniform,
but
in
increasing/decreasing the droplet temperature. In case of a gas temperature inferior than the
is supplied from the fluid will be spent
time dependent. All
the heat
that
droplet temperature, this will lead to a cooling of the droplet, but the fluid will not heat up
unless heat two-way coupling computation is performed.
The thermal properties of droplets are accessible only when the evaporation model activated
(expert parameter iLagr_Evaporation_ set to 1). And the Inlet Boundary Conditions tab in FPI
Parameter window is the only place to configure these properties.
l Evaporation accounts for mass transfer from liquid to gaseous phase due to droplet heating.
In order to account for the convective transport caused by the droplet motion relative to the
gas, the so-called film theory is used. The evaporated vapour is tracked with mixture fraction
variable when coupled with continuos phase. Evaporation models implemented are the 'rapid
mixing model' and a correction to this rapid mixing model by Abramzon & Sirignano (1989),
in order to account for the blowing effect (Stefan flow). The third model is a non-equilibrium
Langmuir-Knudsen model.
l Primary atomization is implemented in order to solve the initial conditions for the droplets
injected from the nozzle. Two types of injectors are processed by different models: Blob model
for plain orifice and LISA model for pressure swirl.
l Secondary breakup enables to compute the evolution of diameters of droplets undergoing
aerodynamic forces. Such forces fragment the droplets into smaller particles and seven models
are provided.
Limitations
The following are the known limitations of the Lagrangian module in FINE™/Open with
OpenLabs™:
l The Lagrangian module is available only when INLET boundary condition exists. Therefore,
for some cases regarding external flow field such as isolated airfoil, the Lagrangian solver is
not applicable.
l The Lagrangian module in parallel mode is not compatible with NMB connections.
l If virtual mass is selected, only the first order scheme for Lagrangian Integration (expert
parameter iLag_IntegrationScheme_ = 0) can be used. The exact integration scheme is not
possible.
l The virtual mass coefficient is selected to 0.5, which is the value for a Stokes flow. Corrections
for much higher particle Reynolds numbers are not implemented at the moment.
l Using a pressure force or particle dispersion modeling, the expert parameter iCstInterpol_ has
to be set to its default value 0, which means that linear interpolation is used.
l The simulations with the Lagrangian module are currently not suited for the simulations of
bubbles because transverse lift force as well as a momentum two-way coupling source term
due to forces other than drag are currently not included.
l Only the drag force accounts for momentum two-way coupling effects at the moment.
l If dispersion is selected for the Lagrangian module, a k-ε turbulence model needs to be
selected.
l Lagrangian simulations with evaporating particles are not compatible with incompressible fluid
and condensable gas.
l The evaporation rate is limited to 5% of the remaining mass for stability reasons.
l No condensation is accounted for.
l Single component evaporation is considered only (so for example no distillation).
l Evaporation of droplets, not suitable for evaporation of wall films.
l Lagrangian 2-way coupling is not compatible with initial solution from file (restart).
Below is the known limitations of the Primary Atomization and Secondary Breakup models in
FINE™/Open with OpenLabs™:
l The Primary Atomization/ Secondary Breakup models are available only in serial mode.
9.5.1
Fluid-Particle Interaction in the FINE™/Open GUI
The Fluid-Particle Interaction module can be accessed through the Optional Models / Fluid-
Particle Interaction page. In the parameters panel click on Fluid-particle calculation to activate
this model. The user needs to enter the main features of the Lagrangian simulations in this page.
Global parameters
When the fluid-particle interaction module is activated, the user needs to set the global parameters
first.
The top frame Main parameters allows to choose the degree of influence of the particles on the
flow. The calculation of the carrier flow and of the particles can be fully (2-way coupling) or
weakly (1-way coupling) coupled:
l in the 1-way coupling approach the flow calculation (ignoring the influence of the particles on
the flow field) is followed by a calculation of the trajectories of particles. In this case, there is
no influence of the particles on the flow.
l in the 2-way coupling approach the calculation of the trajectories of particles is followed by a
second flow calculation, taking into account the presence of the particles in the flow (the
interphase forces are introduced as source terms in the flow calculation). The sequence can be
repeated several times (defined by Number of global cycles) until no changes are observed in
the results.
The parameter Number of particles per cell is used to define the number of computational
particles per class and per cell (default value 30).
When NMB connections are used and the mesh in the upstream side is much coarser than the mesh in
the downstream side, the Number of particle per cell should be increased. Otherwise, holes may
appear in the statistical fields in the downstream side of the NMB.
In the frame Particle forces, the following forces can be activated:
l Pressure: the pressure force is a force on the particle that results from a pressure gradient in
the fluid around the particle.
l Drag: due to the velocity difference of the particle and the fluid. Two different correlations can
be used for the drag coefficient: the Stokes drag for low particle Reynolds number particles
and the drag correction from Schiller-Naumann for higher particle Reynolds numbers.
l Virtual mass: the inertia added to the particle because the accelerating or decelerating of the
particle must move (or deflect) some volume of surrounding fluid.
l Gravity: the force acting on the particle due to gravity.
l Buoyancy : the buoyancy force acts against the direction of gravity and thus in opposite
direction of the gravity force on a particle. The buoyancy force is accessible only when the
gravity forces are selected in the Physical Configuration / Flow Model page.
l Dispersion: while moving through a turbulent flow, each particle faces a sequence of random
turbulent eddies that result in a lack of accuracy in particle velocity and position. A model for
the instantaneous fluid velocity is constructed that takes into account the turbulent dispersion of
the particles. The treatment is only available for the k-based turbulence models.
In the frame Particle temperature evolution, the following options can be activated:
l Heating/Cooling: Injected particles can exchange energy with the continuous phase and it can
be heated up or cooled down based on thermal gradients in the vicinity of particles. It can also
influence the thermal field of the continuous phase by 2-way coupling. If the evaporation
model is enabled using the expert parameters, the evaporated droplet mass is added to
continuous field as mixture fraction variable in 2-way coupling.
Initialize the parcels
To start the fluid-particle interaction simulation, the first step is to initialize the parcels. This will
define the starting positions, velocities, and other parameters of the parcels. In FINE™/Open and
OpenLabs™, there are three ways to initialize the parcels.
Injection from inlet boundary
The user can access this functionality from the Optional Models / Fluid-Particle Interaction
page under the tab Boundary conditions / Inlet. In this way, the parcels are injected from the
selected inlet patch/group. In the list of patches, the user can group patches or select multiple
patches at the same time to apply the same boundary conditions to all of them. To select multiple
patches hold the <Ctrl> key while selecting them.
The user can add a number of classes of particles for the selected inlet patch(es) by clicking on the
button Add class. Each class represents a different type of particles. For each class the inlet
boundary conditions have to be specified. Select the class on the right top frame, then the
corresponding boundary conditions will be displayed. All the inlet boundary conditions can be
specified by a constant value or a profile.
The inlet boundary conditions are the following:
l Velocity of the particles: Select the coordinate system (Cartesian or Cylindrical) and the
frame of reference (Absolute or Relative), then define the 3 components. The absolute/relative
particle velocity refers only to the selected frame of reference.
l Volume fraction: volume of particles divided by the total volume of the control volume.
l Density: density of the particles.
l Diameter: mean diameter of the particles.
l Turbulent kinetic energy (k): turbulent kinetic energy of the particles.
l Temperature: Temperature of particles
l Molecular Weight: molecular weight of particles
l Boiling temperature: boiling temperature of particles
l Freezing temperature: freezing temperature of particles
l Critical temperature: critical temperature of particles
Molecular weight, boiling, freezing and critical temperature of the particles are available only when
the evaporation model is enabled using the expert parameter (iLag_Evaporation=1)
In case that the evaporation model is activated (iLagr_Evaporation_=1), the user needs to define
the Lagrangian mixture fraction at inlet (LagrMixtureFraction) in the Boundary conditions page
for the carrier flow. Please refer to Fluid-Particle Interaction for the information regarding mixture
fraction.
Use primary atomization and secondary breakup models
FINE™/Open provides multiple primary atomization and secondary break- up models. The
primary atomization models are available for different types of injectors: plain orifice and
pressure-swirl. Secondary breakup enable to compute the evolution of diameters of droplets
undergoing aerodynamic forces. Such forces break up the droplets into smaller particles.
These atomization and break-up models play the role of two-phase flow initialization for spray
simulations with the Lagrangian solver. Instead of providing profiles at the inlet, the user will
configure injector and injection characteristics required by the models which will initialize
Lagrangian parcels accordingly.
There is no GUI available for the primary atomization and secondary breakup models. All the
settings are imposed by expert parameters. Refer to "For primary atomization and secondary
breakup models" (p. 253) for the expert parameter settings and Primary atomization and
secondary breakup for the theoretical part.
Define injection from file
In some cases, the user has for example experimental data of the particles or droplets at given
location(s). The user may want to inject the particles or droplets into the domain from these given
location(s). FINE™/Open allows the user to initialize the parcels from given injection points
through an external file.
To define the injection points from an external file, the user has to follow the steps below:
1. activate the Optional Models / Fluid-Particle Interaction module in the GUI,
2. define the global parameters under the tab Boundary conditions / Parameters,
3. under the tab Boundary conditions / Inlet , define injections (classes) from the inlet
boundaries,  for more details,
The parcels indicated in the external file will be initialized in addition to the ones coming from
the inlets. In case that the user only wants to initialize the parcels from the external file, the
Volume fraction of that class in all inlets has to be set to 0.
The number of classes defined in the GUI must be equal to the number of classes defined in the
external file.
It is very important to note that the physical properties of each class are given in the GUI:
l Density,
l Molecular weight, Boiling temperature, Freezing temperature and Critical temperature if
heating/cooling (GUI) + evaporation (expert parameter iLagr_ Evaporation_ =1) is
activated.
4. set the global expert parameter iLagrInjectionPoints_ to 1 in the page Computation Control /
Control Variables under the tab Advanced.
5. put the injection points file (.lagrInjPoints) in the computation folder with the same name as the
computation: <nameOfComputation.lagrInjPoints>.  for the format of the injection points file.
If the injection points file is not present, the flow solver will stop with an error message in the .std
file.
6. define other parameters for the Lagrangian simulation: solid wall boundary condition, output,
...
Solid Wall Boundary Condition
Two solid wall treatment methods are available:
l Rebound: When the particles reach the walls, the particles are reflected from the wall. In this
case, a reflection coefficient (default value 1) is required. The Reflection ratio is only used to
consider the loss of normal velocity of the particles. If the ratio is zero, the normal velocity of
all the particles will be zero after collision with the walls. Whereas if it is 1.0, all particles are
reflected, without any loss of energy.
l Deposition: When the particles reach the walls, the particles deposit on the wall.
Outputs
Under the Outputs tab, the user can select the type of averaging procedure for outputs: mass
averaged or number averaged.
The option Select output of classes is used to select the output of the statistics of the particle
classes:
l All classes: the average over each class will be outputted individually.
l Mean over all classes: the average over all classes together will be computed and outputted.
l All classes and mean over all classes: a combination of the first two.
For the available outputted variables, please refer to Lagrangian section.
9.5.2 How to set up/restart a Lagrangian simulation
Set up a new Lagrangian simulation
The Lagrangian simulations are based on a standard fluid simulation and are executed after the
Eulerian simulation. It is therefore recommended to do a fluid simulation first and restart the
particle simulation based on this fluid simulation.
The usual way to proceed is:
1. perform a pure flow study without activating the Fluid- Particle Interaction model in a
computation.
2. while this computation is active in the list of Computations subpanel on the top left of the
interface, create a new project by clicking on the New button.
3.
in this new computation activate the Fluid- Particle interaction model and perform a
computation with Lagrangian coupling.
Restarting from a saved solution
When a simulation has successfully finished, two files will be written in addition to the regular
single phase flow files for each block. The files are given with the extension name
.lagrangian.aout.# and .lagrangian.bin.#, where # is the index of the block. The aout file contains
the mean particle information (this data is only used for initialization of sampled Lagrangian
statistics at restart). The bin file contains the instantaneous particle data (location, velocities, etc.,
only used for restart purposes).
When you restart from a saved solution, these files are expected to be in the directory from which
you restart. When the files are found, the information will be read and used. When the aout file is
not found, the mean data will be initialized to zero. When the bin file is not found, you start with
zero particles in your domain. Note that when one file is not found, it will still use the information
of the other file.
9.5.3
Advanced Parameters for Fluid-Particle Interaction
For all Lagrangian models
Lag_MaxLocalTimeStep_: Upper global bound for particle time step (default value 1.0e-4).
Lag_MinLocalTimeStep_: Lower global bound for particle time step (default value 1.0e-6).
iLag_IntegrationScheme_: Integration schemes for particles.
0 (default): First-order Euler scheme
1: Exponential Integration Scheme
iLagr_CellResidenceTime_: Controls the number of Lagrangian time steps a particle may stay in
a cell before it is deleted (default value is 1000).
iLagr_TimeStepCriteria_: Controls the time step criteria for the Lagrangian method, if iLagr_
Method_ is set to 1. 0 means deactivated and 1 means activated. (default value 1 1).
First: Using the particle response time as time step criterion.
Second: Using a time step criterion if droplet evaporation is activated, which limits evaporation to
10% of the mass to evaporate during one time step.
LagrMixFracSchmidtsTurb_: Turbulent schmidt number used in the modeling of the turbulent
contribution to the diffusion coefficient for the lagrangian mixture fraction. The laminar
contribution of the diffusion coefficient is calculated (default Value 0.7).
LagrRelaxSourceTerms_: Relaxation factor for Lagrangian source terms. The number of the
Lagrangian cycles must be chosen such that the product of the number of cycles and relaxation
factor is larger or equal to one, in order to account for the full source term at the end of the two-
phase simulation (default value 1).
iLagr_Evaporation_: Selects evaporation for the Lagrangian.
0 (default): not selected
1: selected
iLagr_EvapModel_: Selects the evaporation model to be used.
0 (default): Rapid Mixing model
1: Abramzon-Sirignano model
2: Non-Equilibrium model of Miller, Harstand and Bellan
iLagr_HeatReferenceTemp_: Selects the model for calculation of the reference temperature.
0 (default): 1/3-rule
1: Wet-bulb -temperature
2: A-rule
iLagragian_ Max_ Iterations_: Defines the maximum number of
Lagrangian cycle (default value is 1000000).
iterations during one
Lagr_ NbOfEstimatedStepsPerCell_: Controls
a particle does
approximately per cell. The higher the value, the better the resolution of the statistics sampled, but
computational cost will increase. The minimum value is 3.0. Any lower value is corrected by the
solver to 3.0 (default value is 3.0).
the number of
steps
LagrHeatReferenceFactor_ :
the
iLageHeatReferenceTemp (default value is 0.5).
Provides
value
of
the A- rule
selected with
Lagr_ HeatCapacity_ liquid_ : Heat capacity of the dispersed phase for the particle/droplet
evaporation models (default value 4180 J/kg/K).
Lagr_SumAtomicDiffVol_: Diffusion coefficient in droplet evaporation models. The values are
sum of atomic diffusion values. The first value corresponds to the carrier phase and the second
value to the vapour phase of the dispersed droplet (default values 19.7 13.1).
Lagr_ CoeffConductivityVap_ : Polynomial Coefficients for the conductivity of evaporated
vapour for the droplet evaporation models (default values 0.007341 -1.013e-05 1.801e-07 -
9.10001e-11).
Lagr_CoeffcpVap_: Polynomial Coefficients for the heat capacity of evaporated vapour for the
droplet evaporation models (default values 33.76336 -5.945958e-03 2.235754e-05 -9.962009e-09
1.097487e-012).
Lagr_ CoeffDynViscVap_ : Polynomial Coefficients for the dynamic viscosity of evaporated
vapour for the droplet evaporation models. It has three coefficients (default values -0.003189
4.145e-05 -8.272e-1).
Lagr_ LatentHeatVaporization_ : For droplet evaporation models this is latent heat of
vaporization of the Lagrangian liquid (default value 2257000 J/kg).
iLagrOutputIterations_ : Intermediate output
is written during the particle tracking every
iLagrOutputIterations_ iteration. The mean fields cannot be directly visualized in CFView, but the
end of the simulation must be waited for in One-Way coupling mode and an output in the
Eulerian cycle in Two-Way coupling mode. This expert parameter is mostly of interest if iLagr_
Method == 0 is used. (default value 5000).
For injection points from file
iLagrInjectionPoints_: activates the functionality of adding Lagrangian injection points from a
file.
0: No injection points file
1: Use injection points file (.lagrInjPoints)
LagrInjectionPointsDistanceTol_: tolerance in meters to check if injected parcels are inside or
outside the computational domain when iLagrInjectionPoints_=1. If the distance of the injection
point to the closest boundary face coordinates is smaller than the value of the parameter, then the
injection point coordinates are changed to the closest boundary face coordinates. Otherwise, the
flow solver will stop with an error message in the .std file.
For primary atomization and secondary breakup models
iLagr_ PrimaryAtomization_:
FINE™/Open in combination with Fluid-Particle Interaction.
(default: 0) Activates primary atomization capabilities in
0: Deactivated
1: Activated
iLagr_PrimaryAtomizationModel_: (default: 0) For primary atomization models. Controls the
primary atomization model used.
0: Blob model (for liquid core atomization)
1: LISA model (for liquid sheet atomization)
iLagr_ SecondaryBreakup_:
FINE™/Open in combination with Fluid-Particle Interaction.
(default: 0) Activates
secondary break- up capabilities
in
0: Deactivated
1: Activated
iLagr_SecondaryBreakupModel_: (default: 4) For secondary break-up models. Controls the
secondary break-up model used.
0: Reitz and Diwakar model
1: Pilch and Erdman model
2: Hsiang and Faeth
3: Schmehl
4: Taylor Analogy Break-up (TAB)
5: Enhanced Taylor Analogy Break-up (ETAB)
6: Cascade Atomization and Break-up (CAB)
iLagr_ AtomizationAndBreakupParameters_:
atomization and secondary break-up modeling.
(default: 10000 0 1 0) Used for spray
First: Number of Lagrangian parcels to initialize from injector.
Second: Number of child parcel creations per parcel allowed.
Third: Number of new child parcels to initialize at each breakup.
Fourth: Activates delay of first breakup for Taylor analogy based models if set to 1.
Lagr_AtomizationInjectionCoordAndDirection_: (default: 0.0 0.0 0.0 0.0 0.0 1.0) Used for
spray atomization modeling. Coordinates of injection nozzle exit [m] and vector indicating the
direction of injection [-].
First three: Coordinates of injection nozzle (x,y,z).
Second three: Direction of injection (u,v,w).
Lagr_AtomizationNozzleDiameter_: (default: 0.001) Used for spray atomization modeling with
Blob model or LISA model. Diameter of the nozzle exit [m].
Lagr_AtomizationMassFlow: (default: 0.0) Used for spray atomization. Mass flow through the
nozzle in kilograms per second [kg/s].
Lagr_ AtomizationPressureDifference_:
modeling. Pressure difference between the nozzle exit and domain [Pa].
(default: 1000000) Used for spray atomization
Lagr_ Atomization_ InjectionTemperature_: (default: 293.15) Used for spray atomization
the temperature
modeling. Injection static temperature of parcels [K]. (Inside the parcels,
distribution is uniform)
Lagr_AtomizationModel_LISA: (default: 12.0 3.5) Used for spray atomization in the LISA
model.
First: Logarithm of the amplitude ratio of disturbances.
Second: Exponent used in the Rosin Rammler method.
Lagr_Atomization_HalfConeAngle_: (default: 0.5) Used for spray atomization modeling in
LISA model. Half cone angle of the spray [rad].
Lagr_SecondaryBreakUpModel_CAB_: (default: 80 350.0 0.05) Specific parameters for CAB
model.
First: Critical Weber number for stripping breakup.
Second: Critical Weber number for catastrophic breakup.
Third: Energy ratio factor k1 (default: 0.05)
Lagr_ SecondaryBreakUpModel_ ETAB_:
parameters for ETAB model.
(default: 80 0.222222 0.222222) Specific
First: Critical Weber number for stripping breakup.
Second: Bag breakup coefficient for the energy ratio factor.
Third: Stripping breakup coefficient for the energy ratio factor.
Lagr_SecondaryBreakUpModel_PilchErdman_: (default: 0.375 0.2274) Specific parameters
for Pilch and Erdman model.
First: Coefficient for T.
Second: Coefficient for T*T.
Lagr_ SecondaryBreakUpModel_ ReitzDiwakar_: (default: 12 3.14158 1.0 10.0) Specific
parameters for Reitz and Diwakar model.
First: Critical Weber number for bag breakup regime.
Second: Modeling constant for the characteristic time of bag breakup.
Third: Criterion for the second regime.
Fourth: Modeling constant for the characteristic time of stripping breakup.
Lagr_SecondaryBreakUpModel_Schmehl_: (default: 1.0 0.238 1.2) Specific parameters for
Schmehl model.
First: Expected value for the root-normal distribution.
Second: Variance for the root-normal distribution.
Third: Simmons mass median mean-Sauter mean ratio.
Lagr_SecondaryBreakUpModel_TAB_: (default: 3.5 3.333333 1.0) Specific parameters for
TAB model.
First: Exponent used in the Rosin-Rammler distribution k.
Second: Energy ratio factor K.
Third: Velocity factor Cv.
9.6
UNCERTAINTY QUANTIFICATION
9.6.1
Introduction
Nowadays, the analysis and design methods in aeronautical industry, particularly the aerodynamic
simulation tools relying on CFD and their multidisciplinary extensions are based on simulations
with a unique set of input data and model variables. In spite of that, the actual operating
conditions are a superposition of numerous operational and geometrical uncertainties, under
which the industrial products operate, representing a major source of risk in the design decision
process.
Uncertainties must be incorporated into the simulation tools in order to improve the predictive
reliability of
the simulation tools become non
deterministic.
the simulation process. This means that
FINE™/Open with OpenLabs™ provides an uncertainty quantification module, which is using
the non-intrusive probabilistic collocation method (NIPCM) and is able to manage operational
uncertainties.
The next sections will describe the way to set-up and manage the non deterministic computation
in detail.
The uncertainty quantification module is not compatible with OpenLabs™.
9.6.2 Uncertainty Quantification in the FINE™/Open GUI
Create non deterministic computation
Before creating a non deterministic computation,
the user has to create a deterministic
computation (normal FINE™/Open with OpenLabs™ computation). Then, the non deterministic
computation will be created based on the deterministic computation.
The non deterministic module can be activated in the Optional Models / Non-Deterministic
Data page. Select the button Non Deterministic Data to activate the non deterministic module,
then the user will be asked to select uncertainty for quantities in the Boundary Conditions page.
Go to the Boundary Conditions page, a button uncertainty will appear at the right side of each
boundary condition entry. Check the uncertainty button will select the corresponding boundary
condition as uncertainty.
The recommended maximum number of the uncertainties is 4. More than 4 uncertainties will lead to a
huge number of sub-computations and thus may lead to problems of memory consumption.
FIGURE 9.13
Boundary Conditions page for non deterministic computation
After selecting the uncertainties in the Boundary Conditions page, switch back to the Optional
Models / Non-Deterministic Data page, the settings for the non deterministic computation
appear, as shown in FIGURE 9.14.
In the left side of the Non-Deterministic Data page, all the selected uncertain input quantities are
listed. The right side lists all the parameters of the selected uncertainty entry. The user has to set
the parameters for each uncertainty entry. First, the Polynomial Chaos Order needs to be
specified. Then the user should select
the corresponding
parameters. Four uncertainty types are available:
the Uncertainty Type and set
l Gauss: the Gaussian distribution is used to compute the collocation points.
l In case that the uncertainty entry is a constant, two parameters need to be specified, one is
the mean of the distribution (Average value) and one is the Variance.
l In case that the uncertainty entry is a profile, only one parameter, Variance, needs to be
specified. For each point of the profile, the variance is common while the mean of the
distribution (Average value) is set to the value of the point.
l Truncated Gauss: the truncated Gaussian distribution is used to compute the collocation
points.
l In case that the uncertainty entry is a constant, two parameters need to be specified, one is
the mean of the distribution (Average value) and one is the Variance.
l In case that the uncertainty entry is a profile, only one parameter, Variance, needs to be
specified. For each point of the profile, the variance is common while the mean of the
distribution (Average value) is set to the value of the point.
l Beta: the Beta distribution is used to compute the collocation points.
l In case that the uncertainty entry is a constant, three parameters need to be specified, the
Minimum value, the Maximum value and the Most Likely value.
l In case that the uncertainty entry is a profile, only two parameters need to be specified, the
Minimum value and the Maximum value. The Minimum value and the Maximum
value must be defined relative to a Most likely value of 0. For each point of the profile, the
Minimum value, the Maximum value and the Most likely value will be shifted based on
the value of the point.
l User defined: the user inputs a probability density function, which is used to compute the
collocation points. The format of the probability density function file can be found in User
defined PDF section.
l In case that the uncertainty entry is a constant, the imported PDF is directly used to
compute the collocation points.
l In case that the uncertainty entry is a profile, the imported PDF must be defined relative to a
reference value of zero. Then, for each point of the profile, the PDF will be shifted based
on the value of the point. The shifted PDF is used to compute the collocation points of the
point of the profile.
The specified uncertainty probability density function will be displayed. The user can export the
probability density function into a file by using the button Export.
FIGURE 9.14
Settings for non deterministic computation
After setting the parameters for all the uncertainty entries, click the button Calculate to calculate
the collocation points. Then click the button Ok to create the non deterministic computation.
The non deterministic computation is organized as shown in FIGURE 9.15 . Here,
the
computation "Ps110k" is the deterministic computation, which was created before making the non
deterministic computation. Three sub-computations are the non deterministic computation runs.
FIGURE 9.15
Management of non deterministic computation
After creating the non deterministic computation,
the user should not modify the sub-
computations any more. Otherwise, the results of the non deterministic computation may be
changed.
Launch non deterministic computation
The deterministic computation and the non deterministic computation can be launched
individually. When selecting the deterministic computation and clicking on the button Start Flow
Solver, a window will appear, see FIGURE 9.16:
FIGURE 9.16
Launch non deterministic computation
l Select Start deterministic run,the deterministic computation will be launched.
l Select Start non-deterministic run and then select Start sub-computations one by one, all
the sub-computations will be launched one by one.
l Select Start non-deterministic run and then select Start sub-computations simultaneously,
all the sub-computations will be launched at the same time.
In case that the launching mode of the deterministic computation is set to Parallel, a button
Parallel settings appears, allowing the user to specify the parallel settings. Note, the
launching mode of the sub-computation will follow the launching mode of the deterministic
computation.
Post processing
The results of the non deterministic computation can be found in the Computation Control /
Non-Deterministic Results page, as shown in FIGURE 9.17.
When selecting the deterministic computation, the .mf file of the deterministic computation will be
shown at the lower part of the page. At the upper part of the page, all available quantities are
listed,
their Mean Value ,
together with their Value from the deterministic computation,
Variance, Skewness and Kurtosis from the non deterministic computation.
If the mean and variance are needed for any output quantity, a level 1 produces sufficient accuracy. If
the skewness and kurtosis (For example the output PDF reconstruction) are needed, a level 2 is
recommended.
When selecting a sub-computation (one of the non deterministic computation runs), the page will
show only the mf file of the selected sub-computation.
FIGURE 9.17
Non deterministic computation results
9.7
CAVITATION
Cavitation occurs when in a liquid flow, the pressure falls below its saturation pressure, and as a
consequence, gas filled or gas/vapor filled cavities are formed. This phenomenon is observed in
applications such as pumps, nozzles, injectors, propellers and impellers. Cavitation is, in many
cases, an undesirable occurrence since it can produce structural damage as soon as the bubbles
implode, and can also cause instabilities, a loss in efficiency and an increase of the noise level.
The Cavitation model in FINE™/Open with OpenLabs™ allows the user to simulate cavitating
flows by using incompressible liquid or thermodynamic tables. In the following sections, the
settings and guidelines performing a cavitation simulation will be described.
9.7.1
Cavitation with the barotropic state law
A. Overview
The first cavitation model is based on the barotropic state law which describes the density change
when the pressure falls below the liquid saturation pressure. Barotropic means that the density
depends only on the pressure. This model can only be used with incompressible fluids. Both pure
phases (liquid and gas) are considered incompressible. The barotropic law is used to describe the
density variation in function of pressure from the liquid density to the gas density. Thermo-
sensitive effects will NOT be taken into account when using the barotropic law.
The limitations for the cavitation model with the barotropic law are:
l The cavitation model with the barotropic law should be used when the derivative of the
saturation pressure with the temperature is small.
l The cavitation model with the barotropic law is ONLY compatible with Hakimi
preconditioning.
B. Settings and Guidelines in FINE™/Open with OpenLabs™
There is no access of the Cavitation Model with the barotropic law through the graphical user
interface. The user has to activate this model by setting the expert parameter iCavitation_ to 1.
The other expert parameters setting the cavitation model with the barotropic law are:
Define liquid properties:
cavRhoL_: Density of the liquid phase [kg/m3] (default value 1000)
cavMuL_: Dynamic viscosity of the liquid phase [Pa.s] (default value 1.001E-3)
Define vapor properties:
cavMuV_: Dynamic viscosity of the vapor phase [Pa.s] (default value 9.73E-6)
cavRhoV_: Density of the vapor phase [kg/m3] (default value 1)
cavPv_: Vapor pressure [Pa] (default value 2000)
cavPrV_: Prandtl number of the vapor phase (default value 0.74)
Define the barotropic law:
cavAmin_: User parameter related to the maximum slope of the barotropic law (default value 50).
The convergence rate can be quite sensitive to this parameter. Low cavAmin_ value implies large
derivative of density with pressure. For values of lower than 20,
the solver might have
convergence difficulties.
The other parameters of the cavitation model with the barotropic law in the FINE™/Open GUI
are:
Fluid model
Incompressible liquid MUST be used in the Physical Configuration / Fluid Model page in order
to use the cavitation model with the barotropic law.
Boundary conditions
It has been observed that the following combination of boundary conditions is more robust when
the cavitation model with the barotropic law is activated:
l Static quantities or mass flow imposed at the inlets (velocity, temperature and turbulence
variables)
l Static pressure is imposed at the outlet. Imposing the static pressure at the outlet actually means
) at the outlet. However, for most of the test cases, the
imposing the cavitation number (
) at the inlet. Then,
known parameter of the operating conditions is the cavitation number (
the idea is to modify the static pressure at the outlet until we obtain the desired cavitation
number at the inlet.
Initial Solution
When the cavitation model with the barotropic law is activated, the cavitating flow field can be
initialized by Constant values or From file.
When the cavitating flow field is initialized by Constant values, it is recommended to use an initial
pressure value significantly larger than the saturation pressure. This enforces the computation to
start with a pure liquid flow solution.
In some cases, the cavitation simulation initialized by Constant values may have convergence
problem. In this case, it is recommended to start the cavitating flow simulation from a converged
incompressible simulation without cavitation. The incompressible flow solution will have an
extremely low pressure where cavitation is supposed to occur. Experience shows that it is more
robust to moderate the intensity of cavitation as an initial solution. In FINE™/Open with
OpenLabs™, the strategy used is to start a cavitating flow simulation from an incompressible
simulation result but modifying the pressure inside the two-phase region. To use this strategy, the
user needs to select From file and deactivate the option Import convergence history in the
Initial Solution page.
Numerical parameters
When the cavitation model with the barotropic law is activated, the CFL number MUST be set to
1.0. In case of convergence problems, it can be even reduced to 0.5 or 0.2.
The Multigrid method is compatible with the cavitation model. Four multigrid levels can in
general be used. However, in case of convergence difficulties, the user might consider reducing
the number of grid levels to 3 or even 2.
Control Variables
In order to improve the robustness of the cavitating flow simulation, the following expert settings
are recommended:
cavPreFactorRhoDissip_: Controls the first order density differences term added to the artificial
dissipation of the continuity equation in case of cavitation modeling (default value 1.0)
spc_RhoswitchInArtDissip_: By default this parameter is set to 0, meaning that the only sensor
used to activate second-difference dissipation in regions of strong gradients is a pressure switch.
When the cavitation model is used, this parameter should be set to 1 in order to activate a density
switch in addition to the pressure switch.
tm_iResSmoothing_ : By default this parameter is set to 2, meaning that the residual smoothing
is only applied to the first 5 equations (continuity, momentum and energy). When the cavitation
model is used, this parameter should be set to 0.
spc_dissip_wall_: The default value of this parameter is 2, meaning that there is no artificial
dissipation at the wall boundaries. When a cavitation model is used and is difficult to get
convergence, the value can be changed to 1 in order to activate the computation of the artificial
dissipation at the wall boundaries.
turb_mutMuLimit_: By default this parameter is set to 50000, meaning that the ratio between
the turbulent viscosity and the molecular viscosity is limited to 50000. In order to avoid an
unphysical behavior of the turbulence model, it is recommended to set this parameter to a higher
number, for example 200000.
9.7.2
Cavitation with the Transport Equation Model
A. Overview
The Transport Equation Model (TEM) for cavitating flow modeling is based on an Eulerian
homogeneous flow model (phases are assumed to be in kinematic and thermodynamic
equilibrium). The continuity, momentum and energy equations are solved for the mixture (liquid
and vapor) and an additional transport equation is solved for the vapor volume (or mass) fraction.
Derived from the Rayleigh- Plesset equations of vapor bubbles growth, condensation and
evaporation, source terms are included in this additional transport equation in order to describe the
phase change. FINE™/Open provides three formulations of the source terms: Singhal et al.
(2002), Zwart et al. (2004) and Tani et al. (2009). By means of OpenLabs™, the user will be able
to modify one of the existing source terms or completely change it by a new one. With the
transport equation model, it is possible to model cavitation including or excluding thermal effects.
The limitations for the cavitating flow modeling with the TEM are:
l Can be used only with incompressible fluids.
l The cavitation model with the TEM without thermal effects should only be used when the
derivative of the saturation pressure with the temperature is small.
l ONLY compatible with the Merkle preconditioning.
l The Singhal model is not compatible with the following flow models
l Laminar Navier-Stokes
l The turbulence model Spalart-Allmaras
l The turbulence model Spalart-Allmaras (Extended Wall Function)
l The turbulence model SARC
l The turbulence model SARC (Extended Wall Function)
l The turbulence model S-BSL-EARSM
l The turbulence model S-BSL-EARSM (Extended Wall Function)
B. Settings and Guidelines in FINE™/Open
There is no access of the Cavitation Model with the TEM through the graphical user interface.
The user has to activate this model by setting the expert parameter iCavitation_ to 3. The other
expert parameters setting the cavitation model with the TEM excluding thermal effects are as
follows.
Define the used transport equation:
cavFCM_iVaporMassFracEqs_: Select the vapor equation type used in the transport equation
model.
0 (default): Solve for the vapor volume fraction equation.
1: Solve for the vapor mass fraction equation.
cavFCM_iFullPreconditioning_: Control to consider the volume or mass transport equation in
the preconditioning matrix when the transport equation cavitation model is activated.
0: Do not consider the transport equation in the preconditioning.
1 (default): Consider the transport equation in the preconditioning.
Define liquid properties:
cavRhoL_: Density of the liquid phase [kg/m3] (default value 1000).
cavMuL_: Dynamic viscosity of the liquid phase [Pa.s] (default value 1.001E-3).
cavFCM_cL_: Speed of sound of the liquid phase [m/s] (default value 1481.7).
Define vapor properties:
cavMuV_: Dynamic viscosity of the vapor phase [Pa.s] (default value 9.73E-6).
cavRhoV_: Density of the vapor phase [kg/m3] (default value 1).
cavPv_: Vapor pressure [Pa] (default value 2000).
cavPrV_: Prandtl number of the vapor phase (default value 0.74).
cavFCM_cV_: Speed of sound of the vapor phase [m/s] (default value 423.08).
cavFCM_MinDensClip_: The mixture density could vary between the limiting states of pure
liquid and pure gas. However, and especially for industrial cases, it has been found that allowing
the density to reach the pure gas value heavily destabilizes the convergence and even, very often,
leads to divergence of the flow solver. It is for this reason that the minimum mixture density
allowed is clipped. When the fluid used is water, it has been found that a clipping density value of
60 kg/m3 produces satisfactory convergence rates without significantly damaging the solution. If
the value of cavFCM_MinDensClip_ is set to -1, no clip is activated. If the value is set to a
positive number, the density is not allowed to be lower than this number. The default value is set
to 60.
Define source terms describing the phase change:
cavFCM_SourceTerm_: Select the formulation used in the source term that describes the phase
change.
1 (default): Singhal.
2: Zwart.
3: Tani.
cavFCM_ SourceRelaxFactor_ minus_ : Relaxation factor
(condensation) when the transport equation cavitation model is activated. Default value is 0.2.
the negative source term
for
cavFCM_ SourceRelaxFactor_ plus_ : Relaxation factor
(evaporation) when the transport equation cavitation model is activated. Default value is 0.02.
the positive source term
for
cavFCM_Singhal_Cc_: Modeling constant (default value 0.05) that multiplies the condensation
part of the source term. Used when iCavitation_=3 and the Singhal model is used (cavFCM_
SourceTerm_=1).
cavFCM_Singhal_Ce_: Modeling constant (default value 0.1) that multiplies the evaporation
part of the source term. Used when iCavitation_=3 and the Singhal model is used (cavFCM_
SourceTerm_=1).
cavFCM_Zwart_Fc_: Modeling constant (default value 0.001) that multiplies the condensation
part of the source term. Used when iCavitation_=3 and the Zwart model is used (cavFCM_
SourceTerm_=2).
cavFCM_Zwart_Fe_: Modeling constant (default value 5) that multiplies the evaporation part of
the source term. Used when iCavitation_ =3 and the Zwart model
is used ( cavFCM_
SourceTerm_=2).
cavFCM_Tani_Cc_: Modeling constant (default value 0.06) that multiplies the condensation part
of the source term. Used when iCavitation_ =3 and the Tani model is used ( cavFCM_
SourceTerm_=3).
cavFCM_Tani_Ce_: Modeling constant (default value 0.12) that multiplies the evaporation part
of the source term. Used when iCavitation_ =3 and the Tani model is used ( cavFCM_
SourceTerm_=3).
cavFCM_ Cturb_ : Modeling constant (default value 0.39) to account for the turbulence-
cavitation interaction. Used when iCavitation_=3 and the turbulence model is k-based (k-epsilon,
SST, ...).
cavFCM_SurfTension_: Surface tension used in Singhal model (default value 0.072759). Used
when iCavitation_=3 and the Singhal model is used (cavFCM_SourceTerm_=1).
Settings and Guidelines for the Transport Equation Model with
Thermal Effects
In addition to the parameters described above, modeling cavitation with the transport equation
model including thermal effects requires setting additional expert parameters.
Define the method used to take into account the thermal effects:
cavFCM_iThermo_: Select the option of modeling the dependency of the saturation pressure on
the temperature that is used in the transport equation model.
0 (default): No thermal effects taken into account.
1: Model the saturation pressure based on the ideal temperature depression. Solving the energy
equation is not required.
2: Model the saturation pressure as a polynomial function of the temperature. Solving the energy
equation is required.
Define the model parameters specific to cavFCM_iThermo_=1:
cavFCM_Gsat_: Derivative of the saturation pressure with respect to the temperature [Pa/K].
The default value is 143.75, which is the value for water at 293 K and a saturation pressure of
0.023 bar.
Define the model parameters specific to cavFCM_iThermo_=2:
cavFCM_PvPolynomial_: Coefficients defining the polynomial used to model the dependency
of the saturation pressure [Pa] on the temperature [K]. 5 coefficients need to be provided, starting
from order 0. The default values are [1.131871e7 - 1.483606e5 7.342645e2 - 1.628494e0
1.367673e-3], which are the values for water between 280 K and 450 K.
cavFCM_TRange_: Temperature range used for the calculation of the saturation pressure. 2
bounds need to be provided. If the temperature exceeds the bounds, the saturation pressure will be
evaluated at the bound. The default values are [0 5000], which implies that the temperature is not
bounded by default.
Define general model parameters:
cavFCM_ NSubiterations_ : Number of sub- iterations used per time step to calculate the
cavitation source terms (default value 1). At least 20 sub- iterations are required, but it is
recommended to use 50 sub-iterations to ensure better convergence of the computation.
Define additional liquid properties:
cavFCM_Latent_: Latent heat of vaporization [J/kg]. The default value is 2,453,900, which is
the value for water at 293 K and a saturation pressure of 0.023 bar.
Define additional vapor properties:
cavFCM_cpV_: Heat capacity at constant pressure of the vapor [J/(kg K)]. The default value is
1,905.9, which is the value for steam at 293 K and a saturation pressure of 0.023 bar. The heat
capacity at constant pressure of the liquid will be taken from the Fluid Model page.
Define the thermal conductivity. The user can define the thermal conductivity for the liquid and
the vapor either by supplying the values directly or by supplying the Prandtl numbers. This is
determined by the selection of the Heat conduction law made in the Fluid Model page.
In case the Heat conduction law is defined by Constant K:
cavKappaL_: Thermal conductivity of the liquid phase [W/(m K)]. The default value is 0.59843,
which is the value for water at 293 K and a saturation pressure of 0.023 bar.
cavKappaV_ : Thermal conductivity of the vapor phase [W/ (m K)]. The default value is
0.018228, which is the value for steam at 293 K and a saturation pressure of 0.023 bar.
In case the Heat conduction law is defined by Prandtl:
The Prandtl number of the liquid phase is set by the user in the Fluid Model page.
cavPrV_: The Prandtl number of the vapor phase is described in the section excluding thermal
effects.
General guidelines for modeling cavitation using the transport equation model with thermal effects
are as follows:
l It
is recommended to use the Zwart model
( cavFCM_ SourceTerm_ =2 ) as the
condensation/evaporation source term. This model gives the best overall results for TEM with
thermal effects. In practice, the Zwart model gives the closest estimate of cavitation pockets.
l It is recommended to set the minimum allowable density cavFCM_MinDensClip_ to 10% of
the liquid density (which is given by the expert parameter cavRhoL_ ). Doing this will
considerably help the convergence of the simulation without significantly impacting the results.
l The temperature may vary strongly during the first iterations of the solver. This can cause
difficulties with convergence, because the saturation pressure, and thus the phase change
source terms, will depend on the temperature. It is recommended to define an interval of
temperatures inside which the solution is allowed to evolve, in order to avoid difficulties with
convergence. At the end of the simulation, it is necessary to verify that the temperature of the
converged results never reaches the bounds defined in the interval cavFCM_ TRange_ .
Otherwise, the results of the simulation may be affected.
l If the temperature is an important output of the simulation, it is recommended to use the second
option of modeling the dependency of the saturation pressure on the temperature (cavFCM_
iThermo_=2). The first option (cavFCM_iThermo_=1) converges faster and gives a good
estimate of the pressure. This option is not recommended for accurate computations in which
the temperature is of interest, or if it is expected to have regions of gas only.
l The mass flow error must be carefully verified after a simulation with cavitation.
The other general parameters and guidelines of the cavitation model with the transport equation
model in the FINE™/Open GUI are:
Fluid model
Incompressible liquid MUST be used in the Physical Configuration/Fluid Model page in order
to use the cavitation model with the transport equation model.
Note, the density and viscosity of the fluid will be overwritten by the expert parameter cavRhoL_ and
cavMuL_, respectively.
Initial Solution
When the cavitation model with the transport equation model is activated, the cavitating flow field
can be initialized in different ways:
l Start from a uniform initial solution of pressure and velocities (Constant values). When
initializing by Constant values, it is recommended to use an initial pressure value significantly
larger than the saturation pressure. This enforces the computation to start with a pure liquid
flow solution.
l For
turbomachinery applications, start
from the 'initial
turbomachinery solution'
(For
turbomachinery).
l Start from a converged solution from a pure incompressible simulation or from another
cavitating condition. For high cavitating pockets (low cavitation numbers) it might be difficult
to start from a uniform solution. In those cases it is recommended to use the restart option.
Further, in order to produce a performance curve for a pump or inducer, the restart option can
also reduce the computation (and engineering) time.
Numerical parameters
When the cavitation model with the transport equation model is activated, the CFL number
MUST be set to 1.0. In case of convergence problems, it can be even reduced to 0.5 or 0.2.
The multigrid method is compatible with the cavitation model. Four multigrid levels can in
general be used. However, in case of convergence difficulties, the user might consider reducing
the number of grid levels to 3 or even 2.
Outputs
the available output variables for cavitating flow are listed in the Computation
All
control/Outputs page. Please refer to the Cavitation section for more details.
Control Variables
In order to improve the robustness of the cavitating flow simulation, the following expert settings
are recommended:
spc_RhoswitchInArtDissip_: By default this parameter is set to 0, meaning that the only sensor
used to activate second-difference dissipation in regions of strong gradients is a pressure switch.
When the cavitation model is used, this parameter should be set to 1 in order to activate a density
switch in addition to the pressure switch.
tm_iResSmoothing_: By default this parameter is set to 2, meaning that the residual smoothing is
only applied to the first 5 equations (continuity, momentum and energy). When the cavitation
model is used, this parameter should be set to 0.
spc_dissip_wall_: The default value of this parameter is 2, meaning that there is no artificial
dissipation at the wall boundaries. When a cavitation model is used and is difficult to get
convergence, the value can be changed to 1 in order to activate the computation of the artificial
dissipation at the wall boundaries.
turb_mutMuLimit_: By default this parameter is set to 50000, meaning that the ratio between
the turbulent viscosity and the molecular viscosity is limited to 50000. In order to avoid an
unphysical behavior of the turbulence model, it is recommended to set this parameter to a higher
number, for example 200000.
9.7.3
Cavitation with thermodynamic tables
A. Overview
The derivative of the saturation pressure with the temperature indicates the thermo-sensitivity of
the fluid. For example, for water this parameter is around 130Pa/K. Therefore water can be
considered as non thermo-sensitive. However, for LH2 (~50000Pa/K) this parameter is quite
large and therefore it should be considered as thermo-sensitive. It should also be noted that this
parameter can strongly depend on the temperature at which it is evaluated.
Thermodynamic tables provide a precise description (in equilibrium) of the density in function of
pressure and enthalpy. The description of the states provided by the thermodynamic tables will be
used both for the pure phases (liquid or gas) and for the biphasic states. Thermo-sensitive effects
will automatically be taken into account when thermo-sensitive fluid is used.
For the cavitating simulation with thermodynamic tables and Hakimi preconditioning,
following tables are essential:
the
l RHP.atab - density in function of enthalpy and pressure
l THP.atab - temperature in function of enthalpy and pressure
Moreover, tables for the transport properties are strongly recommended:
l MHP.atab - dynamic viscosity in function of enthalpy and pressure
l KHP.atab - thermal conductivity in function of enthalpy and pressure
For the cavitation modeling, a table for the quality χ is used to detect the state (liquid, gas or
mixture).
l AHP.atab - quality in function of enthalpy and pressure. The quality χ can take the following
values: 0 for liquid phase, 1 for gas phase and from 0 to 1 for biphasic/mixture.
When using thermodynamic tables to model cavitating flows, the thermodynamic tables should cover
all the thermodynamic states that are present in the converged solution.
The limitations for the cavitation model with thermodynamic tables are:
l The cavitation model with thermodynamic tables is ONLY compatible with Hakimi
preconditioning.
B. Settings and Guidelines in FINE™/Open with OpenLabs™
There is no access of the Cavitation Model with thermodynamic tables through the graphical user
interface. The user has to activate this model by setting the expert parameter iCavitation_ to 2.
The other Expert Parameters setting the cavitation model with thermodynamic tables are:
cavPreFactorRhoDissip_: Controls the first order density differences term added to the artificial
dissipation of the continuity equation in case of cavitation modeling (default value 1.0)
spc_RhoswitchInArtDissip_: By default this parameter is set to 0, meaning that the only sensor
used to activate second-difference dissipation in regions of strong gradients is a pressure switch.
When the cavitation model is used, this parameter should be set to 1 in order to activate a density
switch in addition to the pressure switch.
tm_iResSmoothing_ : By default this parameter is set to 2, meaning that the residual smoothing
is only applied to the first 5 equations (continuity, momentum and energy). When the cavitation
model is used, this parameter should be set to 0.
turb_mutMuLimit_: By default this parameter is set to 50000, meaning that the ratio between
the turbulent viscosity and the molecular viscosity is limited to 50000. In order to avoid an
unphysical behavior of the turbulence model, it is recommended to set this parameter to a higher
number, for example 200000.
iCondTableClip_ : By default this parameter is set to 0, meaning that the access to the
thermodynamic tables is not clipped. With the cavitation model with thermodynamic tables is
activated, it is recommended to set this parameter to 1 in order to activate the clipping when the
tables are looked-up.
The other parameters of the cavitation model with thermodynamic tables in the FINE™/Open
GUI are:
Fluid model
Thermodynamic tables MUST be used in the Physical Configuration / Fluid Model page in
order to use the cavitation model with thermodynamic tables.
Boundary conditions
It has been observed that the following combination of boundary conditions is more robust when
a cavitation model is activated:
l Static quantities or mass flow imposed at the inlets (velocity, temperature and turbulence
variables)
l Static pressure is imposed at the outlet. Imposing the static pressure at the outlet actually means
). However, for most of the test cases, the
imposing the cavitation number at the outlet (
known parameter of the operating conditions is the cavitation number at the inlet (
). Then,
the idea is to modify the static pressure at the outlet until we obtain the desired cavitation
number at the inlet.
Initial Solution
When the cavitation model with thermodynamic tables is activated, the cavitating flow field can
be initialized by Constant values or From file.
When the cavitating flow field is initialized by Constant values, it is recommended to use an
initial pressure value significantly larger than the saturation pressure. This enforces the
computation to start with a pure liquid flow solution.
In some cases, the cavitation simulation initialized by Constant values may have convergence
problem. In this case, it is recommended to start the cavitating flow simulation from a converged
solution without cavitation for which the fluid state is pure liquid in the entire computational
domain. In order to apply this strategy, a pure liquid solution has to be obtained first for a higher
pressure in the domain than the one to be used for the cavitating simulation (avoid zones with
pressures below the saturation one). Usually, this can be simply obtained by increasing the
pressure at the outlet boundary. Afterwards, the cavitating computation can be started using this
pure liquid computation as initial solution.
In order to accelerate the convergence, the pressure field in the whole domain of this starting
solution can be reduced by the difference of the pressure level between the pure liquid
computation and the cavitating one. Two expert parameters can be used to control this restarting
strategy:
iRestartCav_PressDiff_: This expert parameter is by default 0. In case the user sets it to 1, the
initial pressure field will be reduced by the expert parameter DeltaPress_RestartCav_.
DeltaPress_RestartCav_: value used to reduce the initial pressure field when the parameter
iRestartCav_PressDiff_ is activated.
Numerical parameters
When the cavitation model with thermodynamic tables is activated, the CFL number MUST be
set to 1.0. In case of convergence problems, it can be even reduced to 0.5 or 0.2.
The Multigrid method is compatible with the cavitation model. Four multigrid levels can in
general be used. However, in case of convergence difficulties, the user might consider reducing
the number of grid levels to 3 or even 2.
9.8 MULTI-SPECIES FRAMEWORK
9.8.1
Introduction
The Multi-species framework in FINE™/Open with OpenLabs™ allows the user to simulate
mixing of chemical species by solving conservation equations describing convection, diffusion
and reaction of the species. Please refer to Multi-Species Framework for more information of the
theoretical part.
The limitation of the multi-species framework in FINE™/Open with OpenLabs™ is as follows:
l The multi- species environment
is not available for
the simulation of a mixture of
incompressible fluids.
9.8.2
Settings and Guidelines in the FINE™/Open GUI
To set up a multi-species simulation, the user should follow the steps below:
1. Enable multi-species framework, define a multi-species fluid.
2. Define multi-species parameters.
3. Define boundary condition of each species.
The details of each step are explained in the following sections.
Before FINE™/Open with OpenLabs™ v6.1, the multi-species framework could be defined
only by expert parameters. When opening an existing project created before v6.1, the interface
will keep the multi-species settings (Everything is defined by expert parameters). Please see
How to maintain a Multi-species Framework by expert parameters for more details.
A. Define a multi-species fluid
To simulate a multi-species flow, the first step is to define a multi-species fluid. Go to the
Physical Configuration / Fluid Model page, click the button Edit to open the edit panel of the
fluid properties. Enter a fluid name and select the fluid type Multi-Species, the entries defining a
multi-species fluid appears.
First, the user should specify the reference pressure and temperature at which the properties are
defined. Then, a mixture file should be specified. The mixture file defines all the species and their
properties. After specifying the mixture file, the user may be able to select the definition of each
property, depending on the contents of the mixture file.
Multi-species simulations can be performed by using either perfect gas or real gas model. The user
can select the model in the option Mixture type.
The mixture file is an external file that provides the information of the species and their properties.
Example of a mixture file
# Version number
Version 1.0
# Atomic elements description: symbol + atomic mass (kg/mol)
NI_BEGIN ELEMENTS
H 0.0010079
O 0.0159996
N 0.01401
C 0.01201
NI_END ELEMENTS
# define the species. The molar mass is computed automatically
NI_BEGIN SPECIES
O2
N2
C3H8
NI_END SPECIES
# Mixture type: Real gas mixture (Cp defined by the NASA polynomials)
NI_BEGIN THERMO
C3H8 300 1000 0.93355381 2.6424579E-2 6.1059727E-6 -2.1977499E-8 9.5149253E-12 -
13958.520 19.201691 1000 5000 7.5341368 1.8872239E-2 -6.2718491E-6 9.1475649E-10 -
4.7838069E-14 -16467.516 -17.892349
N2 300 1000 3.298677 1.4082404E-3 -3.963222E-6 5.641515E-9 -2.444854E-12 -1020.8999
3.950372 1000 5000 2.926640 1.4879768E-3 -5.684760E-7 1.0097038E-10 -6.753351E-15
-922.7977 5.980528
O2 200 1000 3.78245636 -2.99673416E-3 9.84730201E-6 -9.68129509E-9 3.24372837E-12 -
1.06394356E+3 3.65767573 1000 3500 3.28253784 1.48308754E- 3 - 7.57966669E- 7
2.09470555E-10 -2.16717794E-14 -1088.45772 5.45323129
NI_END THERMO
# Mixture type: Perfect gas mixture (Cp defined by a constant)
NI_BEGIN THERMO_CP_CONST
C3H8 1670
N2 1039
O2 909
NI_END THERMO_CP_CONST
# Heat conduction law: Constant K
NI_BEGIN THERMAL_CONDUCTIVITY_CONST
C3H8 0.015198
N2 0.02583
O2 0.0238
NI_END THERMAL_CONDUCTIVITY_CONST
# Heat conduction law: Prandtl
NI_BEGIN THERMAL_CONDUCTIVITY_PRANDTL
C3H8 0.72
N2 0.72
O2 0.72
NI_END THERMAL_CONDUCTIVITY_PRANDTL
# Viscosity law: Constant Viscosity
NI_BEGIN DYNAMIC_VISCOSITY_CONST
C3H8 1.1e-05
N2 1.657e-05
O2 1.909e-05
NI_END DYNAMIC_VISCOSITY_CONST
# Mass diffusion law: Constant diffusion
NI_BEGIN DIFFUSIVITY_CONST
C3H8 1.119e-05
N2 2.23e-05
O2 1.98e-05
NI_END DIFFUSIVITY_CONST
# Mass diffusion law: Schmidt
NI_BEGIN DIFFUSIVITY_SCHMIDT
C3H8 1
N2 1
O2 1
NI_END DIFFUSIVITY_SCHMIDT
Syntax of the mixture file
The mixture file is subjected to the following conventions:
l The mixture file starts with keyword Version following the version number 1.0.
l Each property is defined inside a section, which starts with NI_BEGIN following a keyword
and ends with NI_END following the same keyword.
l Each line in a section defines one species or one property.
l Blank spaces (Blank lines) are ignored.
l All lines starting with the symbol # are comment lines.
l The element symbol is case-sensitive.
Define species and properties
In the mixture file, the user needs to specify the species and their properties. A description of these
parameters is presented below.
Elements
The section starts and ends with the keyword ELEMENTS. This section defines the basic atoms
used in the species and its atomic mass (kg/mol). Each line defines one atom following its atomic
mass.
Species
The section starts and ends with the keyword SPECIES. This section defines the species. Each
line defines one species. The molecular mass is computed automatically based on the atoms in the
species and its number.
Specific heat
The specific heat at constant pressure can be defined by a constant or by the 7-coefficient NASA
polynomials. In the mixture file, the user can provide both definitions and then select one in the
GUI under the option Mixture type.
l When the specific heat is defined by a constant, the section starts and ends with the keywords
THERMO_CP_CONST. In each line, one species should be given following the value of its
specific heat. When the specific heat is defined as constant, the species are considered as
perfect gas. In the GUI under the option Mixture type, the option Perfect gas mixture will be
available for selection.
l When the specific heat is defined by the 7-coefficient NASA polynomials, the section starts
and ends with the keywords THERMO. In each line, one species should be given following
18 numbers. The first 9 numbers define the low-temperature range following its 7 coefficients
and the second 9 numbers define the high-temperature range following its 7 coefficients. When
the specific heat is defined by the 7-coefficient NASA polynomials, the species are considered
as real gas. In the GUI under the option Mixture type, the option Real gas mixture will be
available for selection.
Thermal conductivity
The thermal conductivity can be defined by a constant or by the Prandtl number. In the mixture
file, the user can provide both definition and then select one in the GUI under the option Heat
conduction law.
l When the thermal conductivity is defined by a constant, the section starts and ends with the
keywords THERMAL_CONDUCTIVITY_CONST. In each line, one species should be
given following the value of its thermal conductivity. When the thermal conductivity is defined
as constant, the option Constant K will be available in the GUI under the option Heat
conduction law for selection.
l When the thermal conductivity is defined by the Prandtl number, the section starts and ends
with the keywords THERMAL_CONDUCTIVITY_PRANDTL. In each line, one species
should be given following the value of its Prandtl number. When the thermal conductivity is
defined by the Prandtl number, the option Prandtl will be available in the GUI under the
option Heat conduction law for selection.
Viscosity
The viscosity can be defined only by a constant. The section starts and ends with the keywords
DYNAMIC_VISCOSITY_CONST. In each line, one species should be given following the
value of its dynamic viscosity. In the GUI under the option Viscosity law, the option Constant
Viscosity will be available and selected by default.
Mass diffusivity
The mass diffusivity can be defined by a constant or by the Schmidt number. In the mixture file,
the user can provide both definitions and then select one in the GUI under the option Mass
diffusion law.
l When the mass diffusivity is defined by a constant, the section starts and ends with the
keywords DIFFUSIVITY_CONST. In each line, one species should be given following the
value of its mass diffusivity. When the mass diffusivity is defined as constant, the option
Constant Diffusion will be available in the GUI under the option Mass diffusion law for
selection.
l When the mass diffusivity is defined by the Schmidt number, the section starts and ends with
the keywords DIFFUSIVITY_ SCHMIDT . In each line, one species should be given
following the value of its Schmidt number. When the mass diffusivity is defined by the
Schmidt number, the option Schmidt will be available in the GUI under the option Mass
diffusion law for selection.
B. Define multi-species parameters
In the page Optional Models / Multi-Species, the user can define the parameters used for multi-
species simulations.
In the section General properties, the user should select the reaction type. Currently, only Inert
is available. The inert multi-species simulation does not take any reactions between the species
into account.
In the section Mixing laws, the user should select the mixing law (how to compute the heat
conductivity and viscosity of the mixture based on the definition of each species). Two methods
are available:
l Averaged: the property of the mixture is computed by a mass weighted average.
l Wilke: the property of the mixture is computed by using the Simplified form of the Wilke's
law, see Multi-Species Framework for more details.
C. Boundary Conditions
In the Boundary Conditions / Boundary Conditions page, the mass fraction of each species
has to be specified at all inlet and external boundaries.
The mass fraction of each species should be specified and the sum of all species mass fraction should
be 1 on any given boundary.
The other settings related multi-species are explained below:
Numerical Parameters
The CPU Booster can be activated when using the multi-species framework. In case that the
multi-species simulation does not converge with the CPU Booster, the following parameters can
be modified:
l Switch off the CPU Booster during the coarse grid initialization,
l Decrease the CFL number.
CPU Booster is compatible only with the Merkle preconditioning.
CHAPTER 10.
ROTATING MACHINERY
The Rotating Machinery page contains the following tab pages:
l Rotating Domains, defining if the domain is rotating and its rotating speed.
l Rotor/Stator , defining the properties of each rotor/stator interface. This page is only available
interfaces are computed in
interfaces. Rotor/Stator
when the mesh contains Rotor/Stator
Hexpress™.
In this section
10.1 Rotating Blocks
10.2 Rotor/Stator Interaction
10.3 How to Set-up a Simulation with Rotor/Stator Interfaces?
10.4 Harmonic Method
289
291
294
303
10.1 ROTATING BLOCKS
FIGURE 10.1
Rotating Blocks on Rotating Machinery Page
When selecting the Rotating Domains tab the page appears as shown in FIGURE 10.1. On the
left a list of all blocks is displayed. If the mesh has been generated by AutoGrid5™ and converted
into HEXPRESS™ format, a default grouping per row is proposed. It is also possible to manually
group the blocks that have the same properties:
1. Clicking on a block de-selects the currently selected block(s). It is possible to select several
consecutive blocks in the list by clicking on the first one and holding the left mouse button
while selecting the next. To select a group of blocks which are not situated next to each other,
click on each of them while keeping the <Ctrl> key pressed.
2. Click on the Group button. A text box will appear just below the Group button. Place the
cursor in the text box and type the name of the group and press <Enter>. The name of the
group will appear on the list of blocks with a plus sign on the left of the name. To see the
blocks that are included in a certain group double click on the name of the group or click on
the
symbol in front of the name.
3. To remove a group of blocks select the group and click on the Ungroup button. The group
will be removed and the blocks that were in this group will be listed again in the list as separate
blocks.
On the right of the list with blocks, the information for the selected block is given. If multiple
blocks are selected the information is only displayed for the first selected block.
By default, the rotation axis should be the z-axis.
FINE™/Open with OpenLabs™ also allows to use Multiple Reference Frame (MRF). This is
useful for some applications, such as automotive applications to model the car wheels. The user
can specify a rotation axis for a block that is different from the axis z. The entry specifying the
rotation axis and rotation center can be accessed only if all patches of the block are of type
"SOLID" or connect to another patch through a FNMB connection.
Periodic FNMB by repetition is not allowed.
The FNMB connecting a rotating block and a non-rotating block will be treated by using the Frozen
Rotor approach.
FIGURE 10.2
Set Rotation axis and Rotation center
When a block is set as rotating, a message dialog box will appear to inform the user. After
confirmed, a series of modifications will be automatically performed:
l The boundary "INLET", "OUTLET" and "SOLID" will be changed to "Cylindrical".
l All FNMB patches attached to the rotating block will be set as rotating with the same rotation
speed as the block.
The FINE™/Open solver solves the equations in a relative frame of reference. This implies that
the mesh blocks surrounding rotating blades rotate with the blades and should therefore be set as
"rotating" in this page. The Rotational Speed of the block has to be given in Revolutions Per
Minute (RPM). A positive value for the rotation speed indicates a rotation in positive θ-direction
with θ positive according to a right handed coordinate system. In FIGURE 10.3 this is illustrated
for the case where the z-axis is the axis of rotation.
FIGURE 10.3
Positive rotation speed
It is important to notice that the FINE™/Open solver allows only one rotation speed (combined with
a zero rotation speed) for the simulations using the Domain Scaling method.
10.2 ROTOR/STATOR INTERACTION
10.2.1 Overview
The Rotor/Stator tab gives access to the definition of the rotor/stator interfaces as shown in
FIGURE 10.4 . This tab is only accessible when the mesh contains rotor/stator interfaces.
Rotor/stator interfaces are computed in Hexpress™. Consult the Hexpress™ User Manual for
more detailed information on how to set this boundary condition.
The limitations using rotor/stator interfaces are as follows:
l The Full non-matching frozen rotor method is not compatible with rotor/stator interfaces
containing periodic boundary condition with staircase mesh.
l When the rotor/stator connection is a fluid-solid connection, only the Full non-matching
mixing plane approach can be used. The frame of the Flow direction will be hidden since
there is no flow through the rotor/stator interface.
l The Non reflecting 1D/2D methods are not compatible with unstructured mesh containing
periodic boundary conditions.
l In case the rotor/stator patches include regions where r=0, the limitations are listed in the below
paragraph.
FIGURE 10.4
Rotor-Stator interface definition in steady mode
Zero radius rotor/stator interface
In case a rotor/stator interface is present including regions where r=0, the user must change the
value of the expert parameter RS_iCorrectionFactor to 1. The expert parameter will apply a
correction factor for the cell face area between the image and actual mesh. The change is
necessary to have consistent results at zero radius.
Note that the expert parameter change of RS_iCorrectionFactor may lead to small discrepancies in
mass flow.
Furthermore, following limitations apply in case of a zero radius rotor/stator interface:
l All zero-radius configurations that are not full-circle, are assumed to have a patch corner at
zero radius.
l If the zero-radius configurations are full-circle and do not have a patch corner at zero radius,
two additional limitations exist:
l The slope of the rotor-stator meridional profile must not be zero at any point, and it must
not change sign. In other words, it must always be possible to start from a point on the
shroud, and march toward the axis of rotation by following a path with decreasing radius.
l All the patches on each side of the interface must be connected at their corners with
matching connections along the adjacent edges.
10.2.2 Settings of rotor/stator interfaces
On the left frame, the list of all rotor/stator interfaces is displayed. Multiple rotor/stator interfaces
can be treated in one single project. The user can click on sign (
) to view the left and the right
patches of the rotor/stator interfaces.
On the right, the treatment method must be specified for each rotor/stator connection. Also, it
should be specified the flow direction for the rotor/stator connection. Note that the flow direction
(upstream/downstream patches) is set automatically if the mesh comes from AutoGrid5™. If the
mesh comes from HEXPRESS™, left patches are set as "upstream" and right patches as
"downstream". The default settings can be modified if necessary.
Each time the user is passing from steady to unsteady, and vice-versa, the settings of rotor/stator
interface are kept if possible. If not, the default settings will be used.
Up to now, five rotor/stator interface treatment methods are provided in FINE™/Open with
OpenLabs™:
Steady state:
1. The Full non-matching mixing plane approach is respecting an exact conservation of mass
flow, momentum and energy through the interface and has fewer constraints on the interface
geometry.
2. The Full non-matching frozen rotor approach is considering the rotor/stator interface as a
perfect connection and is neglecting the rotor movement in the connecting algorithm. In this
approach, the periodicities between rotor stator must be equal.
3. The Non Reflecting 1D approach is based upon a characteristic analysis of the linearized
Euler equations. The characteristic variables are imposed on each side of the rotor/stator
interface. Such a treatment is recommended when wave reflection is observed at the interface,
which can occur when the interface is close to the blade.
4. The Non Reflecting 2D approach is the extension of the Non Reflecting 1D approach. The
Non Reflecting 2D approach is also based upon a characteristic analysis of the linearized Euler
equations. The characteristic variables are imposed on each side of the rotor/stator interface.
The Non Reflecting 2D approach will produce a better representation of the shock wave
crossing a R/S interface.
Unsteady state:
5. The Domain scaling approach is an unsteady simulation technique for the rotor/stator
interfaces. The effect of displacement due to rotation, is taken into account. In this approach,
the periodicities between rotor stator must be equal.
10.3 HOW TO SET-UP A SIMULATION WITH
ROTOR/STATOR INTERFACES?
Three different approaches are available in FINE™/Open with OpenLabs™ to simulate the
interaction between rotating and non-rotating blocks:
Steady:
l Mixing plane approach : a pitchwise averaging of the flow solution is performed at the
rotor/stator interface and the exchange of information at the interface depends on the local
direction of the flow. See Mixing Plane Approach for more detail on how to use this approach.
l Frozen rotor approach: a steady simulation of one specific position of the rotor with respect
to the stator. For more information on how to set up a project according to this method see
Frozen Rotor section.
Unsteady:
l Domain scaling method: unsteady simulation in which the mesh periodicities are constrained
to be identical on both sides of the interface. See Domain Scaling Method for more details on
how to use this approach.
Harmonic:
l Harmonic method: this method needs only one inter-blade channel per blade row. No special
requirement on the periodicities is required. The interaction between two adjacent blade rows
is modeled by computing the time harmonics of the fluctuating part of the unsteady flow along
the two sides of the rotor/stator interface as well as the time-averaged flow. The values are
calculated with respect to the matching of the unsteady flow on both sides of the interface and
are treated locally by a non-reflective treatment. A mixing-plane approach is applied to the
eddy-viscosity if the Spalart-Allmaras model is used. See Harmonic Method section for more
details on how to use this approach.
10.3.1 Mixing Plane Approach
In the mixing plane approach the flow solution at the rotor/stator interface is azimuthally averaged
and the exchange of information at the interface depends on the local direction of the flow. In this
section it is described how to use this approach in FINE™.
Geometrical and Mesh Constraints
The full non matching mixing plane method (Full Non Matching Mixing plane, Non Reflecting
1D and Non Reflecting 2D ) is based on the full non- matching algorithm and has clear
advantages:
l The only remaining constraint being that the rotor/stator patches belonging to a given interface
should lie on the same common axisymmetric surface.
l An exact conservation of the mass flow, momentum and energy is guaranteed.
Only one blade passage needs to be meshed for both the rotor and the stator, regardless of their
respective periodicities.
FINE™ Settings
1. The mixing plane approach is a steady simulation technique which requires to set the Time
Configuration to Steady on the General properties page.
2. For each rotating block the rotation speed is defined under the Rotating Domains tab on the
Rotating Machinery page.
3. Under the Rotor/Stator tab on the Rotating Machinery page, the user has to specify for each
of the rotor/stator connections:
l the rotor/stator connection treatment method:
l Full Non Matching Mixing plane,
l Non Reflecting 1D.
l Non Reflecting 2D.
The Non Reflecting 1D/2D approach can not be used when the flow perpendicular to the
rotor/stator interface is supersonic.
The use of the Non Reflecting 1D/2D approach is limited to steady simulations without
preconditioning.
The Non Reflecting 1D/2D approach is only compatible with perfect gas or real gas.
l the flow direction.
Illustrative Example
To illustrate the mixing plane approach the flow in Aachen turbine is considered as shown in
FIGURE 10.5. Due to the pitchwise averaging process one can see that the wake occurring
slightly downstream the trailing edge of the first stator blade is spread when entering in the rotor
blade passage. If the rotational speed of the rotor blade is high, this approximation is acceptable
since one can consider that the rotor blade "sees" a more statistically averaged flow. If the
rotational speed is low, this approximation is essentially invalid and thus another method should
be considered.
the rotor/stator
In some cases, i.e. in low pressure ratio compressors or turbines, the losses at
interfaces are in the order of magnitude of the overall gain in the machine. In such cases, it is
recommended to use an unsteady approach
FIGURE 10.5
Aachen turbine: Mixing Plane approach
Non-interfaced Advanced Parameters
Additional parameters related to the mixing plane method are available in the list located in the
Advanced tab of the Control Variables page.
RS_NbH2DNR_: sets the number of harmonics used for DFT and inverse DFT when using the
non-reflecting 2D Rotor/Stator interface. The default value is 3.
RS_LocalCorrection_: In some particular cases, a problem of mass flow conservation through a
non reflecting 1D or 2D rotor-stator interface can arise. This can be improved by deactivating the
local enthalpy correction through the expert parameter RS_LocalCorrection_.
0: local enthalpy correction deactivated
1 (default): local enthalpy correction activated
10.3.2 Frozen Rotor
The basic idea at the origin of the frozen rotor technique consists of neglecting the rotor
movement in the connecting algorithm.
The governing equations are solved for the rotor in a rotating frame of reference, including
Coriolis and centrifugal forces; whereas, the equations for the stator are solved in a absolute
reference frame. The two components are literally connected, and hence a rotor- stator
approximation is not required, rather the continuity of velocity components and pressure is
imposed. As a result, the final steady solution will be depending on the relative position of the
rotor and the stator. Unsteady 'history effect' (such as shedding separated zones) are neglected.
It is usually well accepted that the frozen rotor approach is an appropriate solution for the
treatment of rotor-volute interactions, where pitchwise variations of the flow cannot be neglected.
However, it requires the meshing of the complete impeller (all passages). Another drawback is
that the flow solution depends on the rotor position, relative to the stator.
Mesh Constraints
For the Full non-matching frozen rotor approach a constraint must be satisfied on the mesh
periodicity. The pitchwise distance must be the same for both sides of the rotor/stator and
coincident (no gap allowed between rotor and stator components in the pitchwise direction). For
each different position of the rotor with respect to the stator a new mesh will have to be created
and a new steady calculation has to be performed.
FINE™ Settings
1. The frozen rotor approach is a steady simulation technique which requires to set the Time
Configuration to Steady on the General properties page.
2. For each rotating block the rotation speed is defined under the Rotating Domains tab on the
Rotating Machinery page.
3. Under the Rotor/Stator tab on the Rotating Machinery page, the user has to specify for each
of the rotor/stator connections:
l the rotor/stator connection treatment method: Full non-matching frozen rotor.
l the flow direction.
Illustrative Example
Results obtained from frozen rotor calculations usually look similar to unsteady ones. A more
detailed analysis shows that the approximation introduced in the connection algorithm induces a
deviation of the wake when passing through the interface. As an illustration the flow in Aachen
turbine is considered as shown in FIGURE 10.6.
FIGURE 10.6
Aachen Turbine: Frozen Rotor approach
10.3.3 Domain Scaling Method
The Domain Scaling Method is an unsteady simulation technique for rotor/stator interfaces. The
effect of displacement due to rotation is taken into account. At each time step, the rotor is set at its
correct position and equations are solved for that particular time step for the whole computation
domain. The final solution is therefore a succession of instantaneous solutions for each increment
of the rotor position.
Mesh Constraints
The blade passages of each blade row to include in the mesh should cover the same pitch distance
(have the same periodicity). If the periodicity of the rotor and the stator is not the same this can be
solved in three different ways:
l modeling a higher number of blade passages on each side to find a common periodicity,
l scaling the geometry (with the scaling being as close to 1 as possible). The common way to
scale the geometry is to modify the number of blades during the mesh generation process. The
time frequencies are resolved with an error that is proportional to the scaling coefficient.
Apart from this constraint on the periodicity, there is no constraint on the patches and mesh nodes
configurations.
FINE™ Settings
1. The Domain Scaling Method is an unsteady simulation technique. The Time Configuration
in the General properties page should thus be set to Unsteady.
2. For each rotating block, the rotation speed is defined under the Rotating Domains tab on the
Rotating Machinery page.
3. Under the Rotor/Stator tab on the Rotating Machinery page, the user has to specify for each
of the rotor/stator connections:
l the rotor/stator connection treatment method: Domain scaling.
l the flow direction.
4. The initialization process can be performed in two ways:
l A steady state initialization is performed in a separate computation with Steady as Time
Configuration. It is suggested to model all rotor/stator interfaces in this case using frozen
rotor approach. The unsteady domain scaling computation is using the result of this steady
computation as initial solution. See Initial Solution chapter for more information on how to
start a computation from an initial solution file.
l The steady initialization is automatically performed before starting the time accurate
computation (that means within the same computation). To use steady initialization, specify
the Steady
in the interface an appropriate Number of steady iterations under
Initialization parameters in the Control Variables page.
5. The Number Of Angular Positions is defined in the Control Variables page. When
working with the Domain Scaling method, using a Number Of Angular Positions of 10 points
per blade passage is giving a coarse but reasonable result. To have a more accurate (but more
CPU consuming) result choose 20 to 30 points per blade passage.
The physical time step will be calculated based on the imposed Number Of Angular
Positions and the information will be given below.
6. The Number Of Time Stepsis defined in the Control Variables page. In general, it is
recommended to repeat the period at least 20 times. Usually after 20 periods, the flow becomes
periodic.
For example, considering a 1-1/2 turbine with the blade number of 43, 64 and 16. The user
can generate a scaled multi-row mesh including 8 stator passages, 12 rotor passages and 3
stator passages with a common periodicity of 5. In this case, the user needs at least 10 time
steps for each rotor passage and that is really a coarse result. So the minimum Number of
Angular Positions is 120. Usually, 20 periods are needed to reach periodic flow. The user
will have to set the Number Of Time Steps to 2400.
7. For more info on the Steady initialization and Outputs Files available in the Control
Variables page, see Control Variables section.
Illustrative Example
The example case of the flow in Aachen turbine is considered as shown in FIGURE 10.7. With
the domain scaling approach, one can observe a strong interaction between the wake and main
flow, leading to a correct physical simulation of the unsteady phenomenon (at the expense of
much higher CPU time compared to mixing plane approach).
FIGURE 10.7
Aachen turbine: Domain Scaling method
Non-interfaced Advanced Parameters
Additional parameters related to the Domain Scaling Method are available in the list located in the
Advanced tab of the Control Variables page.
RS_OutputMultiple_: In case that Multiple files is selected for visualization and/or restart in the
Computation Control / Control variables page under the General tab, the multiple files can be
corresponding to the last period or the whole iteration procedure when Domain Scaling Method is
used:
0: The FINE™/Open solver will only save the solution corresponding to the last Number of
Angular Position physical time steps.
1: The FINE™/Open solver will save the solution from beginning.
10.4 HARMONIC METHOD
10.4.1
Introduction
FINE™/Open with OpenLabs™ allows to compute unsteady flows at minimum costs thanks to
the so-called nonlinear harmonic method (NLH). This approach, introduced by He and Ning
(1998), can be considered as a hybrid method that conjugates the advantages of classical steady
state and full unsteady calculations.
The method is based on solving steady flow transport equations for the time-mean flow and the
time harmonics. In particular, in a turbomachinery configuration, due to the relative motion, the
blade passing frequencies (BPF) of the blade rows are the fundamentals in time of the periodic
disturbances entering the adjacent blade rows. Solving the periodic perturbation in a row is
performed in the frequency domain by a time-marching to the pseudo-steady state of the solution
of the transport equations associated with the BPFs and their harmonics, the number of these
being a user input. One important advantage of the method is that the effect of the periodic
unsteadiness onto the time-averaged flow, the deterministic stresses, is calculated directly from the
in-phase and out-of-phase components of the solved harmonics. Thanks to the transposition to the
frequency domain, only one blade channel is required like a steady flow simulation. More details
about the harmonic method can be found in the theoretical manual.
The harmonic method in FINE™/Open with OpenLabs™ is a generalized multi-rank method,
which considers the unsteady effects provoked by the relative rotation of the direct adjacent blade
row(s) on a reference row, as well as the interactions between the harmonics on that reference
row. The maximum rank is currently limited to 2:
l In case of 1-rank, the harmonic method deals with rotor/ stator interaction of only adjacent
rows.
l In case of 2-rank, the harmonic method considers not only the perturbation from the direct
adjacent row(s) of the reference row, but also the interaction of harmonics between the direct
adjacent rows. In this case, the harmonic can simulate the effects between consecutive rotors or
stators (including clocking effect), or the effects between two adjacent rows that have the same
rotation speed (such as configuration stator-stator-rotor). For example, for a contra-rotating
open rotors (CROR) case, if the pylon of the CROR mounted on the fuselage is taken into
account, then the reproduction of its unsteady effects on the flow in the rotor that is not
adjacent to the pylon can be performed by the rank-2 harmonic method.
Limitations
The harmonic method can be used only in case of:
l perfect gas1;
l no preconditioning or Merkle preconditioning;
l no inlet distortion;
l no CPU Booster;
l the Spalart-Allmaras2 model in case of turbulent simulations;
l Adiabatic wall;
l The effects are limited to 2-rank;
l The maximum number of harmonics in each row is limited to 40;
l The nonlinear harmonic method can only be used for turbomachinery applications. This
method cannot be used for cascade configurations with translational periodic boundaries;
l The flow perpendicular to the inlet (INL), outlet (OUT), external boundary (EXT) and rotor/
stator interface (ROT) has to be subsonic;
l The number of frequencies per perturbation in a row is the same all over the multistage
machine.
10.4.2 Interface and best practices
The harmonic method can be switched on through the radio button Harmonic in the Physical
Configurations / General Properties page.
1Compatibility with a fluid defined by thermodynamic tables is available but requires additional
calibration.
2Compatibility with two equations turbulent models is available but requires additional
calibration.
FIGURE 10.8
General properties
Then, the user can access the Physical Configuration / Harmonic Model page to set all
parameters for the harmonic computation.
Mesh constraints
The rotor/ stator interface treatment in the harmonic method is based on the full non-matching
algorithm, which requires the rotor/ stator patches belonging to a given interface to have the same
spanwise extension.
Although the harmonic method does not impose a specific azimuthal position for the blade, it is
recommended for post-processing purposes to align the adjacent rows in the circumferential
direction. Visualization of the flow across the interface is much clearer.
Mesh resolution in the tangential direction
The harmonic method is based on the spatial Fourier decomposition of the time-averaged flow
and the harmonics in the tangential direction.
It is suggested to guarantee at least 30 grid nodes in the azimuthal direction to represent in space
the first harmonic (or fundamental) of a periodic disturbance at the inlet/ outlet of a row. Then, the
number of nodes in the tangential direction of the row channel should be at least 30 times the
number of blades of the adjacent blade row generating this harmonic divided by the number of the
blades of the row. The narrower the adjacent blade row channels, the more refined the channel
should be.
It is assumed that the amplitude of the subharmonics decreases very quickly. The constraint can
thus be relaxed for the other harmonics. In general, at least 30 grid notes for the first harmonic and
15 for the other harmonics are suggested.
Example
For a stator/ rotor/ stator configuration in case of 1-rank, where the number of blades in the rotor
and stators are Nbrotor, Nbstator 1 and Nbstator 2 and NH is the number of harmonics:
Number of Points in Azimuthal Direction in stator 1:
30 x
15 x
if(NH=1)
x NH if(NH>1)
Number of Points in Azimuthal Direction in rotor:
max(30 x
, 30 x
) if(NH=1)
max(15 x
x NH, 15 x
x NH) if(NH>1)
Number of Points in Azimuthal Direction in stator 2:
30 x
15 x
if(NH=1)
x NH if(NH>1)
Harmonic Model
FIGURE 10.9
Harmonic settings
In the frame Harmonic Settings, the number of Maximum rank should be specified. The
maximum rank of the perturbations is limited to 2. After setting the number of Maximum rank,
the user needs to set the Number ofharmonics per perturbation (Default value: 3). Note, the
Number ofharmonics per perturbation is common to all perturbations.
When the Maximum rank is set to 2, the option Clocking position becomes accessible to
control if the clocking position is Fixed or Variable:
l Variable: From this simulation, all the harmonics from different perturbations in the same row
will be resolved, whether the harmonics have the same properties or not. The user can
reconstruct the flow in time or in space. For both time and space reconstructions, the initial
relative position of the rows can be defined by the user. In case of clocking effect, it allows to
display the solutions for different azimuthal offset of one stator relatively to the other.
l Fixed: From this simulation, all the harmonics from different perturbations in the same row
will be merged if the harmonics have the same properties (phase angle and angular velocity).
In this case, the user can only reconstruct the flow solution in time. Unlike the option
"Variable", the relative initial position of the rows can only be changed by a multiple of the
pitch. The rank-2 effects are also limited to the initial position of the rows in the input mesh.
In addition to the perturbations coming from the rows adjacent to the reference row, the multi-
rank harmonic method can also consider the interaction between the harmonics.. By default, the
multi-rank harmonic method does not consider the interaction of harmonics between the upstream
row and the downstream row of the reference row (No interaction). But in some applications, this
interaction may have important influence on the flow in the reference row. In this case, the user
can activate the interaction of harmonics by checking the option Interaction in the frame
Harmonics Range. The Max order in interaction is set by default to 1. This number can be
increased but cannot be larger than the number of harmonics per perturbation. For example, a max
order in interaction of 3 will introduce the interaction of the first three harmonics from the
upstream row and the downstream row into the reference row.
In the harmonic method, the perturbations are linearly combined. All harmonics and their conjugate
harmonic are taken into account. Only harmonics having a non-negative frequency will be kept for
the computation.
In the frame Harmonics Results, the harmonics defined in each group can be inspected and their
status updated.
FIGURE 10.10
Check harmonics in each row
Each group listed in the left-tree menu can be expanded with the symbol "+"/"-". Selecting an
harmonic in the expanded menu displays its characteristics (name, angular velocity, phase angle,
aliases properties and base – these parameters are detailed later on in this section) on the right side
of the window.
For each group, the list of disturbers and associated harmonics can be displayed by expanding the
menus Disturbers and Harmonics, respectively.
The expandable menu Disturbers indicates the number of harmonics considered for the modeling
of the perturbation originated from the adjacent row(s).
The expandable menu Harmonics allows to modify the harmonics to be solved. Thanks to the
flexibility of the NLH method, each harmonic displayed in a group can be disabled, i.e. not
solved by the solver, by unchecking the checkbox on the left of its name.
When deactivating an harmonic (for example "1G2" in row 1), all other conjugate harmonics
defined as a linear combination of the one unselected (e.g. "(-3G3;1G2)") will be ignored by the
solver even if they appear checked in the interface.
Note that changing the settings in the menus Disturbers or Harmonics will display a warning
message:
Some global harmonics settings have changed. Harmonics need to be recomputed.
If the change is global, the harmonics results are all hidden. If the modification is local (for example,
a modification in the number of harmonics for a disturber), a warning sign icon is displayed in front
of the affected group in the left-tree menu. In both cases, the set of harmonics to be considered for
the simulation must be updated by clicking the button Update.
The maximum number of harmonics in each group is limited to 40. If this limits is exceeded, a
specific warning message is displayed in the interface, asking to decrease the number of harmonics in
the group(s) exceeding this limit:
Warning ! The number of harmonics exceeds the limit of 40 for some groups. 
Please modify the settings to decrease the number of harmonics, or deactivate some
harmonics.
FIGURE 10.11 illustrates the information displayed when selecting an harmonic from a given
group. The following information is displayed:
l The Name of the harmonic indicates where it is originated. For example, the name " (-
3G3;1G2)" means that the harmonic is a linear combination of the third harmonic from G3
(row 3) and the first harmonic from G2 (row 2), where the symbol ";" should be considered as
the operator "+". The frequency of this harmonic will be given by the algebraic sum of the
individual frequencies. For example, if 3G3 has 10000 Hz and 1G2 has 15000 Hz, then
frequency of "(-3G3;1G2)" will be -10000+15000 = 5000 Hz.
l The Angular Velocity shows the angular velocity of the harmonics.
l The Phase Angle depends on the differences between the circumferential angles due to the
differences in blade count.
l It may happen that harmonics of different origins have the same properties. In this case, the
harmonics having the same properties can be merged by using the fixed clocking position.
Then, the Number of aliases of a harmonic can be larger than one (alias could be understood
as 'name' of the harmonic). For example, a Stator-Rotor-Stator configuration with 36/41/36
blades will have number of aliases greater than 1 if the simulation has only one set of
azimuthal positions of the stators (fixed clocking). Indeed, in this case, for one harmonic per
perturbation, the harmonic in the central rotor from the second stator has the same frequency
and phase angle as the harmonic from the first stator, because the two stators have identical
numbers of blades. Therefore, the harmonic from the first stator is an alias of the harmonic
from the second stator and only one harmonic will be resolved in the rotor instead of two.
l Alias name gives the name of all the harmonics that have the same properties and are merged.
l The Base can be:
l -999: if the harmonic is a LONE TIME HARMONIC (no clocking impact at the frequency
of this harmonic).
l (-1)*Harmonic number: if the harmonic is a BASE TIME HARMONIC with associated
clocking harmonics.
l associated base time harmonic number: if the harmonic is a CLOCKING HARMONIC
(note that a particular case is zero, which means that the harmonic is associated with the
time-averaged flow).
FIGURE 10.11
Check properties of each harmonic
The other parameters for the harmonic method in the FINE™/Open GUI can be found in the
following menus:
Flow Model
When Harmonic is checked in the Physical Configurations / General Properties page, the
turbulence model is set by default to Spalart-Allmaras. The Euler flow and the Laminar flow
can also be selected.
Rotating Machinery
In the Physical Configurations / Rotating Machinery page under the tab Rotor/stator, the
rotor/ stator connection treatment parameters will be set automatically by the flow solver when the
harmonic method is activated.
Boundary Conditions
The boundary conditions of the NLH computation are non-reflective at the far inlet and far outlet.
They are based on 1D non-reflective treatment that computes the flow variables on the boundary
as a resulting combination of incoming and outgoing characteristics. The flow at the far inlet and
far outlet is assumed to be the time-averaged without the deterministic stress terms.
Initial Solution
It is recommended to use a previous steady flow simulation as the initial solution. This can be
done by using the option from file in the Initial Solution page.
Outputs
The Harmonics category in the Computation Control / output page allows to select the
harmonic variables for output.
The user can select to output the Real & Imaginary parts of the harmonic variables (such as
Harmonic Pressure) and/ or the Amplitude of the harmonic variables (such as Harmonic Pressure
Amplitude).
Note, the reconstruction in time/ space is based on the Real & Imaginary parts of the outputted
harmonic variables. If no harmonic variables are outputted, it is not possible to reconstruct the flow in
time/ space.
Reconstruction in time/ space
The harmonic simulations can be reconstructed in time or in space in CFView™. For more
information, see the CFView user manual.
Control Variables
NLH computations need more CPU time and memory, in comparison with a steady mixing-plane
method, due to the additional transport equations associated with each harmonic. If N harmonics
of a perturbation are to be modeled, then there are 10N additional transport equations to be solved
(5 for the real part and 5 for the imaginary part of the complex amplitude of each harmonic).
Then, the ratio R of the required CPU time or memory between the harmonic method and the
steady method is:
where
is the number of the grid nodes in the blade row bi (i in range of [1,B]),
is the
number of harmonics per perturbation,
is the number of the equations in the steady
computation (5 for Euler, Laminar and turbulent flow with the 0-equation turbulence models; 6
for the turbulent flow with the 1-equation turbulence models).
As an approximation, the number of the grid nodes can be assumed to be the same for all the
blade rows. The ratio R can be simplified as:
For example, for a 3-harmonic (
) simulation of a one-stage turbine (B=2) and using the
Spalart- Allmaras model (
=6), the CPU time is therefore 6 times that of a steady
simulation.
10.4.3 Troubleshooting in rotor/ stator interface
Convergence
In case of convergence issues when using the NLH with perfect gas and Merkle preconditioning,
the following parameters may be modified:
l set preco_NLH_Vunst2Factor_ to 1
l set NLH_HarmoPressureInit_ to (10,10) or (1,1)
Conservation of flow variables
In some cases, the conservation of the flow variables such as entropy may not be accurately
respected through the rotor-stator interface, even with more than 3 harmonics per perturbation.
This situation is often due to a strong wake or shock wave on one side of the rotor-stator interface.
Within the NLH method, the conservative variable is decomposed into a time-averaged value and
a sum of periodic perturbations, which in turn are decomposed into N harmonics. In some special
cases, the perturbation can not be accurately reconstructed by using the decomposed harmonics.
The error is depending on the number of the used harmonics.
FIGURE 10.12 shows how a square wave signal
is captured by using a Fourier series
(harmonics) and the influence of the number of harmonics on the reconstructed signal. One can
see that the accuracy of the reconstruction increases with the number of harmonics. However, it is
impossible to reproduce the vertical line in the signal. This can only be reached if the number of
harmonics is infinite.
FIGURE 10.12
The first four Fourier series approximations for a square wave
As an example, FIGURE 10.13 shows the iso-radius contours of entropy in a contra rotating
propeller using the 1-rank harmonic method. In this case, there is a strong peak in entropy
upstream the rotor-stator interface due to the wake of the front blade. To capture such a sharp
signal with Fourier series (that is what non-linear harmonics computations do) is indeed very
difficult. As shown in the image, the signal is better captured when increasing the number of
harmonics. This is in agreement with the theory: increasing the number of harmonics will improve
the accuracy, but with higher computation costs.
FIGURE 10.13
The contours of the entropy at a constant r surface for a contra-rotating propeller
CHAPTER 11.
INITIAL SOLUTION
A FINE™/Open with OpenLabs™ computation is started from an initial solution. The following initial
solution types are available:
l Constant values,
l From file,
l For turbomachinery,
l Techno effects.
Each of these types is described in the next sections ('Techno effects' is described in the section 'For
turbomachinery').
It is possible to initialize a multi-domain computation by combining different initial solution types. For
example, for an impeller and volute configuration, the impeller can be initialized by using For
turbomachinery and the volute by Constant values, or the impeller can be initialized by From file and
the volute by Constant values.
In this section
11.1 Initial Solution Defined by Constant Values
11.2 Initial Solution from File
11.3 Initial Solution for Turbomachinery
11.4 Expert Parameters
317
FINE™/Open with OpenLabs™ 7.2 User Guide
318
319
11.1
INITIAL SOLUTION DEFINED BY CONSTANT
VALUES
When selecting Constant values on the Initial Solution page, the user can modify the physical
values used for the initial solution on the page as shown in FIGURE 11.1.
FIGURE 11.1
Constant initial solution
The physical values are uniformly used as initial solution over all the domain, except on the
boundaries. The variables for which initial values need to be specified are the static pressure, the
static temperature, the velocity components and the turbulence-based variables k and ε, if a two-
equation turbulence model is used. Note that the velocity components specified by the user are the
Cartesian or cylindrical ones depending on the chosen system of coordinates in the Initial
Solution page. When the cylindrical coordinate system is select, the user has ability to define the
initial velocity field in the relative frame of reference.The circumferential component of the
velocity will then vary as a function of the radius.
11.2
INITIAL SOLUTION FROM FILE
11.2.1
General Restart Procedure
To continue using the results from a previous computation, the user must select From file in the
Initial Solution page. Clicking on the browser button (
to select the ".run" file of a computation.
) will open a File Chooser window
To restart from a solution the computation definition file with extension ".run" is not sufficient. It is
required that
the saved
quantities.
the solution file with extension ".bout" is present, which contains all
The toggle button Import convergence history can be selected. When selecting this button the
".res" file, which contains all the residuals from the previous computation, will be used. The new
residuals will be calculated with respect to the last iteration of the previous computation and will
be appended to the ".res" file.
If the computation is initialized with different files (or combined with Constant values / For
turbomachinery), the Import convergence history will not work.
If the initial solution From file is used, the option Coarse grid initialization will be disabled.
FIGURE 11.2
Restarting from a file
When a computation is initialized by the solution of a previous simulation, the user has the
possibility to change the fluid model. To keep a robust initialization, it is recommended that the
fluid model of the previous computation, used as initial condition, be simpler than the fluid nature
of the new computation. To summarize, one of these fluid changes can be applied:
l from incompressible to perfect gas
l from incompressible to real gas
l from incompressible to condensable gas
l from perfect gas to real gas
l from perfect gas to condensable gas
l from real gas to condensable gas
is not possible to restart a computation using incompressible fluid from a previous non-
It
preconditioned computation using condensable gas.
11.2.2 Restart in Unsteady Computations
To enable a second order restart for unsteady computations it is necessary for the ".btm1" file to
be present in the computation directory. This is the case if an unsteady computation is being
restarted from an existing unsteady solution.
If the FINE™/Open solver can not find the solution of the previous time step, a first-order time
accurate computation will be made during the first time step.
In case of an unsteady computation restarted from a steady one, it is not possible to import the
convergence history.
11.2.3 Advanced control of the restart
When a computation is running, the computation will save the solution at a constant interval . However, the convergence history (.res file, .fmperit file, ctl_
out file ......) are saved at every iteration in case of steady computations and at every time step in
case of unsteady computations. If the computation is abnormally stopped (machine shutdown,
crash, ......), the user can restart the computation from the saved solution but cannot keep the
convergence history, because the solution and the convergence history are saved at different
iterations/time steps.
FINE™/Open with OpenLabs™ provides the user a smart restart procedure, allowing the user to
restart a computation from an abnormally stopped computation, from a given time step or from a
given adaptation step, and keep the convergence history without the user having to edit any files.
With this smart restart procedure, the user may:
l restart an abnormally stopped computation. This smart restart procedure is controlled by the
expert parameter iSmartRestart_ . When settings iSmartRestart_ = 1, the FINE™/Open
solver will make a backup of all required files under the folder "backup" in the computation
folder at each intermediate save. If the computation abnormally stops and the user restarts the
computation, the flow solver will read the proper files from the computation folder or the
"backup" folder, depending on the moment that the computation had ended.
l restart an unsteady computation from a given time step provided that the solution of the
specified time step is available. The time step can be specified by the expert parameter ta_it_
restart_.
l restart an mesh adaptation computation from a given adaption step provided that the adapted
mesh is saved . The adaptation step is
specified by the expert parameter adapt_id_restart_.
The parameter iSmartRestart_ must be activated prior to the unexpected termination in order to
have the backup files.
The smart restart procedure is valid only for a restart from the same computation.
If turbulence models with extended wall functions are applied, a jump in the convergence history may
appear because the wall shear velocity is not saved in the restart files and has to be recomputed.
11.3
INITIAL SOLUTION FOR TURBOMACHINERY
The initial solution for turbomachinery is dedicated to the cylindrical rotating machinery. This
type of initial solution respects the inlet and outlet boundary conditions and assumes a constant
rothalpy along axisymmetric stream surfaces. In addition, the velocity field is automatically
aligned with the blade passage.
The initial solution for turbomachinery can be applied for meshes generated in AutoGrid5™. If a
mesh combines an AutoGrid5™ mesh and a HEXPRESS™ mesh, the initial solution for
turbomachinery can be applied only for the AutoGrid5™ mesh part.
The limitations using initial solution for turbomachinery are:
l Only available for internal flow.
l Supersonic inlet boundary condition at the main channel entrance is not allowed.
l Cartesian inlet boundary condition at the main channel entrance is not allowed.
l For a combined AutoGrid5™/HEXPRESS™ mesh, it is possible to use the initial solution for
turbomachinery on the AutoGrid5™ part. However, when the HEXPRESS™ mesh connects
to the original inlet and/or outlet of the AutoGrid5™ mesh (for example, an impeller/volute
configuration), the initial solution for turbomachinery will be possible only if the connection
between the meshes is a Rotor/Stator interface.
The orientation of the rotor/stator interfaces (from left to right or from right to left) must be
defined correctly in order to use the initial solution for turbomachinery.
11.3.1 Methodology
The initial solution for turbomachinery is computed on the 2D meridional view divided into
different parts named "meridional sectors". The control sections of the meridional mesh in
AutoGrid5™ that correspond to the main entrance, main outlet and rotor-stator interfaces define
these meridional sectors as showed in FIGURE 11.3. Note that the main entrance/exit could be a
rotor/stator interface when the main channel of the first/last row defined in AutoGrid5™ is
connected to a 3D effect meshed in HEXPRESS™. In a combined AutoGrid5™/HEXPRESS™
mesh, the FINE™/Open GUI and solver will detect the AutoGrid5™ mesh part depending on the
2D meridional mesh.
FIGURE 11.3
Additional data necessary for computing initial solution
The conservation of mass and rothalpy is applied on the streamlines of each meridional sector.
Then the initial solution computed in the meridional view is interpolated in the 3D mesh.
Such initial solution 'For turbomachinery' can also be used for the blocks defining technological
effects. For example the axisymmetric elements such as seal leakages that are not included in the
general meridional view can be treated easily. If the cell centre is not located in the meridional
view, the pressure will be the pressure in the closest cell of the meridional mesh (idem for the
temperature). The components of the velocity will be set to zero. This special treatment can be
applied as well to the blocks included in 3D effects located in the main passage (cooling holes,
…). Selecting the page Techno effects uses this initial solution.
Before converting the mesh in HEXPRESS™, modifying afterwards the AutoGrid5™ mesh in IGG™
can lead to a mismanagement of the blocks grouping. If some blocks are added, they are not included
in the turbomachinery group, which is detected automatically by the interface. If some blocks are
removed or renamed, the initial solution 'for turbomachinery' will be stopped.
11.3.2 Grouping & Parameters
The turbomachinery-oriented page displays two major frames: one for the channel parameters and
one for the turbulence parameters . On the left of the page, a tree shows by
default the grouping.
FIGURE 11.4
Example of Turbomachinery-oriented initial solution
Select the Main Entrance in the left side of the Channel Parameters frame, all the existing inlet
patches/groups that belong to the first row will be listed. The user has to specify the main entrance
of the channel. Then, an input dialog box is provided in order to select the type of static pressure
specification: constant distribution or radial equilibrium. One or two input boxes are provided in
order to define the static pressure value to be used and, if radial equilibrium is chosen, the radius
(in meters [m]) on which this radial equilibrium will be based. If the inlet of the first row is a
rotor/stator interface, the name of the rotor/stator interface is displayed. For this case, the user has
to set all the estimated inlet boundary conditions (static pressure, static temperature and velocity).
An inlet patch must be defined for the first row for which a 'for turbomachinery' initial solution
has been chosen. If there is no inlet patch for the first row, a warning message is displayed in the
FINE™/Open interface asking the user either to check the orientation of the rotor/stator connections
or to change the type of initial solution.
Select the Internal R/S connections in the left side of the Channel Parameters frame, all the
existing rotor/stator interfaces between rows in the main channel will be listed. For each
connection, the user must select it and set the corresponding parameters, depending on the
selected type of static pressure specification. The specified values of the static pressure will be
shown.
Select the Main Exit in the left side of the Channel Parameters frame, all the existing outlet
patches/groups that belong to the last row will be listed. The user has to specify the main exit of
the channel. Nothing needs to be set for the exit if this is an actual outlet. If the outlet of the last
row is a rotor/stator interface, the name of the rotor/stator interface is displayed. For this case, the
user has to set the corresponding parameters at the rotor/stator interface, depending on the selected
type of static pressure specification. For a bypass configuration, the fourth zone Main Up Exit
(bypass) appears, allowing the user to specify the second exit of the bypass configuration.
The channel main exit frame does not appear in special configurations where the main channel exit is
connected to the main channel entrance by a Rotor/Stator interface (for example, a torque converter).
In this case, all boundary conditions are specified at the channel main entrance.
When clicking
at the right side of the frame Channel Parameters, an information dialog box
will appear, which remind the user to specify the corresponding boundary conditions at channel
main entrance/exit. If the channel main entrance/exit contains a few patches and they are not
grouped, the user can select one of the patches and set the corresponding parameters. The
specified parameters will automatically be applied to the whole main entrance/exit.
If a Spalart-Allmaras or SARC turbulence model is selected, a initial value of
has to be
specified. For advice on the initial values see Turbulent Navier-Stokes section. If a k-ε or k-ω
turbulence model is selected, the initial values for the turbulent kinetic energy ( k ) and the
turbulent dissipation rate (epsilon) must be specified.
11.4 EXPERT PARAMETERS
iSmartRestart_: Activate the option of saving backup files at each intermediate save and the
possibility of a smart restart.
0 (default): no backup files will be saved. When restarting a computation that had ended
unexpectedly, the flow solver will read the files from the computation folder. The convergence
history cannot be kept.
1: the flow solver will save backup files at each intermediate save. When restarting a computation
that had ended unexpectedly, the flow solver will read the proper files from the computation
folder or the "backup" folder, depending on the moment that the computation had ended, thus
allowing the user to restart while keeping the convergence history
ta_it_restart_: the time step at which the unsteady computation will be restarted.
-1 (default): inactive
#: allow to restart from the same directory an unsteady computation from the solution saved at the
time step #.
adapt_id_restart_: the adaption step at which the mesh adaptation computation will be started.
-1 (default): inactive
#: allow to restart a mesh adaptation computation from the saved intermediate solution on adapted
mesh #, see Save solution on intermediate adapted meshes.
The following expert parameters are dedicated to initialization procedure for the simulation of
supersonic and hypersonic flows (no preconditioning):
HypInit_: If HypInit_=1, a first order upwind discretization scheme is applied during the coarse
grid initialization process and HypInitItMax_ iteration on the finest grid before switching
automatically to second order scheme.
If HypInit_=0, the solver will apply the selected scheme in Numerical Scheme menu from the
beginning to the end of the simulation.
HypInitItMax_: Gives the number of iteration that the first order upwind scheme will be applied
on the finest grid before the solver switches automatically to the second order scheme. Taken into
account only if HypInit_=1.
HypInitCfl_: The CFL number used during the hypersonic initialization. Taken into account only
if HypInit_=1.
HypInitResSmoo_ : Allow to activate the residual smoothing during the first order upwind
initialization. Taken into account only if HypInit_=1.
CHAPTER 12.
OUTPUTS
This chapter is dedicated to outputs:
l The page Computation control / Outputs is described in Outputs . The user can select
the
quantities that will be outputted and visualized in CFView™.
Furthermore CFView™ allows the user to calculate derived quantities, which limits the memory size of
the output.
l Global performance data is outputted by the FINE™/Open solver. The output is written in an
ASCII file with the extension ".mf", see Global Performance Output section.
l The FINE™/Open solver can create an ANSYS compatible input file (.cdb), more details can be
found in Ansys output section.
l The FINE™/Open solver can create an FINE™/Acoustics input file, more details can be found in
FINE™/Acoustics Output section.
In this section
12.1 Outputs
12.2 Global Performance Output
12.3 Ansys Output
12.4 FINE™/Acoustics Output
328
345
350
358
12.1 OUTPUTS
Management of outputs in FINE™/Open with OpenLabs™ is performed through the
Computation control/Outputs page. The Computation control/Outputs page contains three
tabs: General, External Flow and Advanced.
12.1.1
General
Using the General tab, the user can choose which format will be used and which physical
variables have to be included in the output generated by the flow solver, see FIGURE 12.1.
FIGURE 12.1
Output Parameters - General
In the Flow configuration frame, the configuration choice for the output can be selected:
Internal flow , External flow or Turbomachinery. Depending on the choice, the selectable
quantities in the Quantities selection frame will be adapted automatically.
In the Output file format frame, the format of the output file can be selected. By default, the
CFView™ format is activated. The user has to select at least one format for output. In case that
none of them is selected, the CFView™ format will be used.
l CFView: This is the native format used by FINE™/Open with OpenLabs™. The format is
fully supported by CFView™. By default (out_newCfv_=0), all output generated by the flow
solver for CFView™ are written in ".d1.s*" files for scalar quantities and in "d1.v*" files for
vector quantities. The flow solver can also write all output into one single ".cfview" file, which
can be done by setting the expert parameter out_newCfv_ to 1.
In case of harmonic simulations, the expert parameter out_newCfv_ is set to 1 automatically by
the flow solver.
To compare the outputted derived quantities by the flow solver and the derived quantities
computed by CFView™, the user must set the expert parameter out_derQntFromNode_ to 1 in
order to compute the derived quantities in the flow solver after interpolating the primitive
variables to nodes.
l Ensight: The flow results can be exported in EnSight format. Thus, the user can post-process
the FINE™/Open with OpenLabs™ solution in EnSight. For the use of EnSight, please refer
to the EnSight manual.
Validation tests are performed with EnSight v9.1.2.
For unsteady computations, the intermediate solutions can not be saved.
l CGNS: The flow results can be exported in CGNS v3.3.1 format.
When exporting results in CGNS format, the following limitations exist:
l No information on FNMB or R/S interfaces in CGNS file.
l No Solid Data in CGNS file.
l For sliding mesh cases, the mesh is not rotated.
l For PER boundary condition, one layer of extra cells is added in case of serial
computations.
The Quantities selection frame is split up into three parts. On the left side, the different
Categories of output are listed. If no variable can be selected, the category will be gray out. On
the right side, there are two lists: Available quantities and Selected quantities. The user can
click on the button Add to move a selected variable from Available quantities to Selected
quantities, or click on the button Remove to move a selected variable from Selected quantities
to Available quantities. All the selected variables will then be automatically available when
launching CFView™ in order to visualize the results.
The selection of variables is global. If a variable is selected, it will be computed for domains that
match the conditions. For the other domains, the value will not be computed (field appears blank
in CFView™).
If the user changes the flow configuration, the previous selection is kept. The selected variables,
which are not compatible with the new configuration, are hidden. The new selectable variables
are added to the list Available quantities.
By default, the following variables are selected, whatever the flow configuration is:
l Static temperature
l Static pressure
l Density
l Vxyz
l Turbulent viscosity
All the variables that can be selected for output are listed in the following sections.
Thermodynamics
For all the flow configurations, the following variables can be selected for output.
l Static/Total temperature
l Static/Total pressure
l Over static pressure
l Static/Total enthalpy
l Density
l Entropy
When computing the Entropy, the reference pressure, reference temperature and reference density
are the averaged values of the static pressure, static temperature and density averaged on all INL
patches, respectively. If there are no INL patches, all reference values must be defined in the
Advanced tab.
l Static Energy (only for condensable gas)
l Dynamic viscosity
l Dryness fraction (only for condensable gas)
l Generalized dryness fraction (only for condensable gas): the generalized dryness fraction is
. Where ρ is the local density, ρL and ρv are the liquid density and vapor
defined as:
density computed from the pressure saturation table, respectively.
l Void fraction
l HeatCapacity (not available for combustion)
l Thermal conductivity
l Gamma (only for perfect gas and real gas, not available for combustion)
TABLE 12.1 Thermodynamics quantities generated by the FINE™/Open solver
Quantity
Incompressible
Perfect gas
Static
temperature
Total
temperature
Static
pressure
Total pressure
(The term k only exists when the two or four equation
turbulence models are applied)
Density
Entropy
Dynamic
viscosity
Thermal
conductivity
Heat capacity
Gamma
-
The heat capacities cp and cv are function of the temperature for real gas and condensable gas.
When real gas or condensable gas is used, the total pressure and total temperature are computed
by the following equations:
In case of condensable gas, some thermodynamic variables are selected by default for output.
These variables are used to compute derived quantities in CFView™, for example, the "static
energy" and "density" in case of non-preconditioning. If these variables are deselected, a
warning will be pop-up for confirmation:
The following five definitions of the pressure coefficient are available for fluid blocks with inlet
and outlet boundary conditions:
where
corresponds to the averaged value of the variable X on the inlet. vref is defined as
in case of Turbomachinery activated in the General tab ( L ref the reference length
defined in the Advanced tab). In case that Turbomachinery is not activated in the General tab, vref
is defined as Reference velocity in the Advanced tab.
Furthermore the following definition of the pressure coefficient is available for fluid blocks:
where
,
and
are the reference pressure, reference density and reference velocity
defined in the Advanced tab, respectively.
For turbomachine computation (when Turbomachineryactivated in Flow configuration frame),
the following additional quantities can be selected for output:
l Absolute/Relative total temperature
l Absolute/Relative total pressure
l Absolute/Relative total enthalpy
l Rothalpy: the rothalpy is defined as
. Where h is the static
enthalpy, w the relative velocity, u the entrainment velocity defined as:
.
Vorticity
For all the flow configurations, the following variables can be selected for output:
l Vorticity components in the
axes:
l Vorticity magnitude
l Vorticity vector
Velocities
For all the flow configurations, the following variables can be selected for output:
l Velocity components in the xyz axes:
,
,
l Velocity magnitude:
l Mach number
l Velocity vector:
l Velocity vector with projection of the velocity field in the wall boundary cells onto the surface.
This enables visualisation of oil flow traces on solid boundaries with surface streamlines.
For turbomachine computation (when Turbomachinery activated in Flow configuration frame),
the following additional quantities can be selected for output:
l Absolute Velocity components in the
axes:
,
,
l Absolute Velocity m-component:
l Relative velocity components in the
axes:
,
,
l Relative Velocity component in the θ axes:
l Relative velocity magnitude:
l Relative Mach number
l Relative velocity vector:
Residuals
The residuals are computed in FINE™/Open with OpenLabs™ by a flux balance (the sum of the
fluxes over all the faces of each cell). The absolute value |RES| resulting from the flux balance is
written as output for each cell.
For all the flow configurations, the following residuals can be selected for output:
l mass conservation
l x-component of the momentum equation
l y-component of the momentum equation
l z-component of the momentum equation
l energy conservation
l Spalart viscosity
equation, for the Spalart-Allmaras and SARC models
l turbulent kinetic energy k equation, for the k-ε and k-ω models
l turbulent energy dissipation rate ε equation, for the k-ε models
l Specific dissipation rate ω equation, for the k-ω models
For combustion computations, the following additional residuals may be selected for output:
l Residual_Comb_NormalizedProgressVariable
l Residual_Comb_MixtFrac
l Residual_Comb_VarianceMixtFrac
l Residual_Comb_EnthDefect
l Residual_Comb_NOxPost
l Residual_Comb_ProgressVariable1
For radiation computations using the P1-model, the following additional residuals can be selected
for output:
l Residual_Rad_GP1Rad
Turbulence
For all the flow configurations, the following variables can be selected for output:
l Spalart viscosity , for the Spalart-Allmaras and SARC models
l turbulent kinetic energy k, for the k-ε and k-ω models
l turbulent energy dissipation rate ε, for the k-ε models
l Specific dissipation rate ω, for the k-ω models
l Distance to wall
l Ratio between turbulent eddy viscosity and molecular viscosity
l Dimensionless distance to wall y+
l Turbulence production term
Data
For all the flow configurations, the following solid data can be selected for output:
l Cf: Skin friction coefficient (only the wall boundary cells are considered. Set to 0 elsewhere).
is the local wall shear stress (magnitude of the vector Viscous
, where
stress),
and
are the reference density and reference velocity, respectively (set in the
Output page under the tab Advanced).
The quantity Cf =
used in your existing script.
before FINE™/Open v5.2. Please update your Python script if Cf is
l Viscous stress (wall to fluid): local wall shear stress (vector).
l Heat flux (wall to fluid)
l Heat transfer coefficient:
. Where
is the heat flux (wall to fluid);
is the
local wall temperature;
is defined as the averaged absolute total temperature on all inlets
in case of the expert parameter out_htcDef_=1 and defined as the reference temperature in the
Advanced tab in case of the expert parameter out_htcDef_=2.
Unsteady
For all the unsteady flow configurations, the following variables can be selected for output:
l CFL_phys: the unsteady CFL number, defined by
, where v is the local velocity,
is
the physical time step and
is the characteristic cell size.
l Q_criterion:
, where S is the absolute value of the strain rate and Ω the
absolute value of Vorticity.
l Lambda_2: is defined as the second largest eigenvalue of
.
Combustion
For output of non-premixed combustion simulation, .
For output of partially-premixed combustion simulation, .
For output of premixed combustion simulation, .
Radiation
For all the flow configurations, the following variables can be selected for output:
l Rad_GP1Rad: Incident radiation
l Rad_AbsorptionCoefficient: Absorption coefficient
l Rad_SurfRadiationHeatFlux: Surface radiation heat flux
l Rad_HeatFlux: Radiation heat flux
Cavitation
For all the flow configurations, the following variables can be selected for output:
l Cav_VaporFraction: the vapor mass fraction or the vapor volume fraction, depending on the
solved transport equation (cavFCM_ iVaporMassFracEqs_). This output is available only
when using the cavitation model with the TEM model.
Harmonics
For harmonic output, see output.
Lagrangian
Depending on the settings of Lagrangian computations, the following variables may be selected
for output:
l Lagr_ParticleVelocity: the velocity of the particles.
l Lagr_VolumeFraction: the volume of the particles / m³.
l Lagr_TurbulentKineticEnergyK: the turbulent kinetic energy of the particles.
l Lagr_NumberConcentration: the number of the particles / m³.
l Lagr_MassConcentration: the mass of the particles / m³.
l Lagr_ArithmeticMeanDiameter: the arithmetic mean diameter of the particles.
l Lagr_ArithmeticDiameterVariance: the variance of the Arithmetic Mean Diameter.
l Lagr_Deposition_Rate: the deposition rate on the solid walls where the option Deposition is
selected.
l Lagr_InterphaseForces: the components of the interphase force. These are all source terms
activated going to the Eulerian equations, thus mass, momentum and energy source terms from
the Lagrangian phase to the Eulerian phase. They are also sampled.
l Lagr_ReynoldsStress: these are the stresses of Lagrangian particle velocities (again ensemble
averaged), ie.: u'u', v'v', w'w', u'v', u'w', ... and so on, where u', v', and w' are the fluctuations
of the averaged Lagrangian particles velocities. It is the same as for the fluid, but for the
particle velocities.
The output can be computed for each class of particle. The number of classes is defined during the
computation settings. All sections concerning Lagrangian quantities are expanded during the saving of
the run file, so that it contains as many sections as the number of classes for each quantity.
Deformation
The deformation output is available only when the mechanical coupling method (MpCCI and
Modal Approach) is activated:
The output quantities available are:
l Dx, Dy, Dz : scalar quantities of mesh deformation in X, Y and Z respectively.
l Magnitude of D : magnitude of deformation
l Dxyz : mesh deformation vector
OpenLabs
The available variables depend on the definition in OpenLabs, see Output by OpenLabs section.
12.1.2
External Flow
The tab External flow contains the output parameters for the external flow applications. It is
accessible only if the External flow configuration has been selected in the General tab.
When External flow is activated, the flow solver will calculate the lift, drag and moment. The
user can set the direction of the lift, drag and moment under Outputs parameters.
FIGURE 12.2
Output Parameters - External flow
If the option Output force and moment coefficients is activated, the lift, drag and momentum
will be expressed as dimensionless coefficients. These coefficients will be stored in the ".wall" file
instead of lift, drag and moment. The coefficients are defined as:
Lift coefficient
Drag coefficient
Moment coefficient
where L, D and M are the lift, drag and moment, respectively;
is the reference density;
is the reference velocity;
is the reference area;
is the reference length. All reference
values should be defined under the Advanced tab.
12.1.3 Advanced
The tab Advanced contains advanced output parameters and the control points definition.
FIGURE 12.3
Output Parameters - Advanced
When mesh adaptation is performed with FINE™/Open with OpenLabs™, the user can save the
meshes and solution files on each intermediate, adapted mesh, by activating the Save solution on
intermediate adapted meshesoption. In this case, the FINE™/Open solver outputs at the end of
each computation a "*_a#.cfv" file for the intermediate project, a "*_a#.hex" file containing mesh
information related to the current grid, and associated solution files for CFView™. The number
following "*_ a" corresponds to the number of adaptations performed before archiving the
solution. It is therefore possible in CFView™ to visualize intermediate adapted meshes and
solutions. This is accomplished by opening the ".cfv" file corresponding to an intermediate project
and is possible even when the flow computation is terminated on a different ("adapted") final
mesh.
In the frame Reference parameters , all required reference parameters in the computation,
depending on the settings, are listed. The user should specify correct value for the available
parameters. When the parameters is not used by the computation, it is disabled.
In the Control points definition frame, the user can define "control points". These are specific
locations where the user can follow the evolution of the solution or to extract the final solution.
The Add Point button is used to add a new control point definition in the control points area.
After adding a new control point, the control point coordinates can be modified. It is possible to
remove control points by selecting the control point to be removed and then clicking on the
Remove point button. The Import and Export buttons are used to import or export control
points definition to file, which has the extension ".ctl" and the format as follows:
Two header lines, e.g.:
#List of control points (X Y Z)
#Created on 07/21/2003 15:08:43
This is followed by a line containing the number of control points required, e.g.:
There then follows a list of x,y,z coordinates of each control point, each on a separate line, e.g.:
0.5 0.5 1
0.55 0.55 1.1
Note that all coordinates should be defined in meters irrespective of the mesh units.
The evolution of the solution at the defined control points can be followed at each iteration
in the
(steady computations) or at each physical
time update (unsteady computations)
Convergence History page or in the Steering (
out" file.
). The evolution is also outputted in a ".ctl_
Note that it is impossible to change the control points definition during a computation.
12.1.4 Advanced Parameters
iCstInterpol_: Select the method of interpolation to get the nodal values.
0 (default): the linear interpolation is used,
1 : the constant interpolation is used.
out_allRes_ta_: Specify the frequency that the residual is outputted in the .res file when running
unsteady computations. When using the dual time stepping method, the frequency is applied to
the inner-iteration cycle only. For each inner-iteration cycle, the residuals of the first iteration,
every # iteration (# is the frequency) and the last iteration will be outputted. When using the
explicit time stepping method, the frequency is applied to the time steps. The residuals of the first
time step, every # time step (# is the frequency) and the last time step will be outputted.
out_ copyFiles_ : by default (value 1), the FINE™/Open solver copies the mesh files to the
computation folder. When settings out_copyFiles_ to 0, the FINE™/Open solver will create links
instead of copying the mesh files in order to save disk space.
out_copyFiles_=0 only works on LINUX.
out_CPUperIteration_: Control the output of the CPU time per iteration.
0 (default): no information on the CPU time of per iteration is outputted.
1: the CPU time of per iteration will be outputted in the .log and .std file. For each iteration, the
following information will be outputted:
MainSolver::main-->Iteration performed in 0h 0m 15s
MainSolver::main-->Comm time is 0.5 construction 0.04
The first line gives the CPU time information. The second line gives the time communication
between the processors during the calculation (Comm time) and the time to construct links
between the processors for the communication (construction).
out_derQntFromNode_: When exporting the results to CFView™, the derived quantities can be
computed before or after interpolating the primitive variables to nodes:
0 (default): derive quantities before interpolation to nodes;
1: derive quantities after interpolation to nodes.
out_ gaugeForceTorque_ : For some applications, for example automotive applications, the
outputted lift depends on the far-field value of the static pressure, because the car surface is not a
closed one due to the presence of the contact patch between ground and the tyre. Using the expert
parameter out_ gaugeForceTorque_ will allow the user to get
the lift and drag that are
independent of the farfield value of the static pressure.
0 (default): the force and torque are computed by integrating the static pressure.
1: the force and torque are computed by integrating the (static pressure - reference pressure).
Where the reference pressure is defined in the Advanced tab.
out_globQuantPerIt_: Allow to export the global results in function of the number of time steps
on the finest grid level. This function only works in case of unsteady computations. If setting to 1,
a ".globalout" file will be saved in the computation folder, which contains the exported data, see
The globalout file for more details.
out_mfFileVersion_: Control the content of the MF file.
0 (default): This is the default format used in FINE™/Open.
1: The global performance will be written using the same format as in FINE™/Turbo.
out_periodicForcesAndMoments_ : Control the integration when computing the forces and
moments in the .wall output file.
0 : the forces and moments are computed on specified solid patches without taking into account
the periodicity.
1 (default): the forces and moments are computed on specified solid patches taking into account
the periodicity.
out_resCluster64_: Control the save of the .res file in the parallel computation. Sometimes, the
.res file generated on 64 bits Cluster can not be read by Monitor. In this case, the user can set
out_resCluster64_ to solve the problem.
0 (default): each processor is writing data in .res file.
1: only the first processor is writing data in .res file.
out_saveAHEX_: If setting this parameter to 0, the partitioning data (".ahex", ".fmf", ".fnmb",
".pmf", ".vmf" and ".dtw") will not be saved to disk. This parameter has an effect in combination
with the parallel partitioner (PartitionerParallel_=1) only. Note, the required memory when out_
saveAHEX_=0 will be ~10% more than the one when out_saveAHEX_=1.
out_wallForcesPerIt_: Allow to export the lift, drag and moment on per patch or per group of
patches in function of the number of iterations on the finest grid level. If setting to 1, a ".fmperit"
file will be saved in the computation folder, which contains the exported data, see The fmperit file
for more details.
out_ writeAllCtrlPts_ ta_ : Control the output of the solution on the control points in inner
iteration cycles when using the dual time stepping method.
0 (default): the flow solver will save the solution only at the last inner iteration.
1: the flow solver will save the solution at each inner iteration.
out_writeCtrlPts_ta_: Control the interval of the time steps at which the solution on the control
points is written in unsteady mode. By default, the value is set to 1, which means that the solution
will be written at each time step.
out_ writeForces_ ta_ : Control the interval of the time steps at which the forces  and the global results  are written in unsteady mode.
By default, the value is set to 1, which means that the forces and the global results will be written
at each time step.
12.2 GLOBAL PERFORMANCE OUTPUT
The main global performance data are output in an ASCII file with extension ".mf".
The content of the file depends on the flow configuration. The user should specify on the
Computation control/Outputs page whether the current problem deals with an internal flow, an
external flow or a turbomachinery flow configuration.
FINE/Open provides two format of the .mf file, depending on the expert parameter out_
mfFileVersion_.
12.2.1 mf file when out_mfFileVersion_ =0
External configurations
When External flow configurations are computed with FINE™/Open with OpenLabs™, the
following global quantities are output in the ".mf" file:
l Lift
l Drag
l Moment
these quantities are selected in the
The solid surfaces used for
SOLID/Boundary Conditions page, by activating the Compute force and torque when a
relevant solid patch is treated.
the computation of
Lift and drag directions, as well as moment reference axis and center, can be specified in
dedicated input fields on the Computation control/Outputs page. These fields are unfrozen only
when External flow configuration is selected on the same page.
Internal configurations
In the case of internal configurations, Internal flow configuration should be selected on the
Computation control/Outputs page. Quantities referring to inlet and outlet boundaries are also
output in the ".mf" file:
l Mass flow
l Static pressure (area averaged)
l Static temperature (mass averaged)
l Enthalpy (mass averaged)
l Total pressure (mass averaged)
l Total temperature (mass averaged)
l Total enthalpy (mass averaged)
Turbomachinery configurations
In the case of turbomachinery configurations, Turbomachinery configuration should be selected
on the Computation control/Outputs page. Additional quantities referring to inlet and outlet
boundaries are also output in the ".mf" file as well as global performances:
l Hub/Shroud radius
l Total pressure ratio
l Isentropic efficiency (total to total)
l Rotational speed
l Power
Other information
Additional information is available in the ".mf" file, independent of the flow configuration.
Fluid properties
Information on the fluid used in the computation is given:
l Specific heat at constant pressure (Cp)
l Specific heat at constant volume (Cv)
For compressible fluids:
l Gas constant (R)
l Ratio of specific heats (
)
For incompressible fluids:
l Density (ρ)
Momentum & energy balance
For each individual patch, the following quantities are output:
l Mass flow
l Momentum flux
l Pressure contribution to momentum flux
l Torque flux
l Enthalpy flux
This enables the user to check flux and mass flow balance at boundaries. For viscous
computations, we have, in addition:
l Friction force
l Friction torque
l Heat generated by friction
l Heat flux by conduction
Again the balance on boundaries can be checked for these quantities.
12.2.2 mf file when out_mfFileVersion_ =1
If the expert parameter out_mfFileVersion_ =1, the FINE™/Open solver is able to output the
global performance into .mf files using the same format as FINE™/Turbo.
Mesh data
l Number of blocks
l Total number of nodes
Fluid properties
l Fluid type
l Specific heat
l Density
Weight factors used for averaging
l For static pressure
l For all other variables
Geometrical data
The geometrical data are computed at inlet/outlet.
When there are multiple inlets or outlets with different periodicities, only one "number of blades"
is reported in the .mf file.
Fluid properties
The specific heat and the specific heat ratio are computed at inlet/outlet.
Absolute/Relative velocities
Both absolute and relative velocities, including the flow angles, are computed at inlet/outlet.
Static/Total conditions
The density, the absolute/relative static/total pressure and temperature are computed at inlet/outlet.
Mass Flow
Mass flow and Absolute Mass flow are output at inlet/outlet.
Absolute Mass flow is different in case of Backflow.
Global performance
Global performance data, available in the ".mf" file, are calculated using the results at the inlet and
outlet boundaries of the computational domain.
Global performance output for incompressible fluid
The outputted global performance is depending on the type of the fluid. In case of incompressible
fluid, the following data will be written:
l Static pressure rise
l Absolute total pressure rise
l Static Head
l Absolute total Head
l Static temperature rise
l Absolute total temperature rise
l Efficiency
Global performance output for compressible fluid
In case of compressible fluid, the following data will be written:
l Static pressure ratio
l Absolute total pressure ratio
l Static temperature ratio
l Absolute total temperature ratio
l Isentropic efficiency
l Polytropic efficiency (for Perfect Gas only)
Turbomachinery Outputs
With out_mfFileVersion_ =1, some quantities are written in .mf file only if Turbomachinery
checked in Outputs/General.
FIGURE 12.4
Turbomachinery Outputs
l Relative total enthalpy (for Condensable Fluid only)
l Hub radius and Shroud radius
l Axial thrust, Torque and Power (available if at least one rotating block exists)
Flow variables at Rotor/Stator interfaces are not available.
12.3 ANSYS OUTPUT
The FINE™/Open with OpenLabs™ environment provides the user with a specific ANSYS
output. The objective is to export results of the CFD computation on solid surfaces (nodes and
elements) into ANSYS as a boundary condition for the finite element model. This approach is
called FEM loading method for loading the CFD results on a F inite E lement M odel. The
transferred results on the interface fluid-structure can be the pressure field for a structural analysis
and the temperature field, the heat fluxes or heat transfer coefficients for a thermal analysis in the
structure.
The FEM approach needs to have the finite element mesh of ANSYS. If this mesh does not exist
before the CFD computation, it is impossible to create directly a file that can be imported in ANSYS
to apply the suitable boundary condition. Consequently the best way to manage the interface between
FINE™/Open with OpenLabs™ and ANSYS can be a new post-processing tool. The post-processing
tool is needed with the specification of the ANSYS mesh, the common surfaces where the data must
be interpolated and the type of boundary condition on each surface. The transfer will be carried out
through the ANSYS file saved with the command CDWRITE ("project_ANSYS.cdb") in ANSYS.
This file will be modified and read again in ANSYS to impose the CFD results as boundary
conditions .
The ANSYS file is dedicated to a fully defined ANSYS project. It cannot be imported in another
project with different meshes or geometries (even if the geometries of the interface fluid-structure are
unmodified). A new ANSYS project requires a new data transfer.
The application is restricted to steady analysis.
FIGURE 12.5
Data transfer diagram
12.3.1 ANSYS Pre-Processing
Before completing the Computation control/Ansys output pages, the user must create an Ansys
file with the extension ".cdb" saved with the command CDWRITE in ANSYS, for example
"project_ANSYS.cdb". Furthermore before the save in ANSYS, some operations are needed to
allow the identification of the common surface between the fluid model and the structural model.
The ANSYS project must be completely defined with a special treatment for the surface
loads that will be replaced by the interpolated CFD results. On each common surface, a
coded constant value is specified. The default coded values are given in the TABLE 12.2 for the
different types of boundary condition. The value is incremented by one for each different surface
so that for example the pressure imposed on the first surface is set to 1000001 and it is set to
1000002 on the second,...
TABLE 12.2 Default code for different type of boundary conditions imposed from CFD results
Boundary Condition
Pressure field
Temperature field
Heat transfer coefficient
Heat flux
Code
1000001
2000001
3000001
4000001
The coded value can be modified in order to avoid confusion with physical values.
Validation tests are performed with ANSYS release v8.0. Please refer to ANSYS user manual for
more details on the ".cdb" file format
12.3.2 Global Parameters
The user can complete the Computation control/Ansys output pages when the file "project_
ANSYS.cdb" has been created.
FIGURE 12.6
GeneralParameters of ANSYS outputs
Firstly, the user needs to specify under the tab Global Parameters in Boundary Conditions
(FIGURE 12.6 - (1))the coded constant value used in the file "project_ANSYS.cdb". The default
coded values are given in the TABLE 12.2 for the different types of boundary condition.
Furthermore, the user has to specify the required units of the data for each type of boundary
condition. The units will be specified next to the coded value.
Convection type boundary condition in Ansys consists in specifying the heat transfer coefficients,
which are defined by:
where
Q heat flux per unit surface (W/m²)
h heat transfer coefficient or film coefficient (W/m²K)
T temperature at the surface of the model (K)
Tbulk Bulk temperature of the adjacent fluid or temperature bulk (K)
The bulk temperature plays a crucial role in the definition of the heat transfer coefficient. The bulk
temperature can be specified by the user through the Ansys interface or extracted from the CFD
results. If the toggle Compute non- uniform temperature bulk ( FIGURE 12.6 - (1)) is
activated, the bulk temperature will be computed by the FINE™/Open solver.
Then, the user needs to load the file "project_ANSYS.cdb" (FIGURE 12.6 - (2)) created in
ANSYS ) in Ansys Input File.
The data transfer between the CFD mesh and the structural mesh requires matching common
boundaries. The following settings must be set correctly in order to have matching common
boundaries.
l Units: the units used in the ANSYS mesh must be specified in Ansys Mesh Units. The
conversion Factor will be deduced automatically (FIGURE 12.6 - (2)).
l Reference system: The user must specify the used coordinate systems (FIGURE 12.6 - (3)).
For example, the original geometry can be rotated for the CFD model so that the axial
direction corresponds to the Z axis. The necessary conversion of coordinates will be done
through the specification of the position of the coordinate center of the ANSYS mesh in the
coordinate system of the CFD mesh and the specification of the location of three common
points in both meshes in Reference System.
Note that these points cannot be located on a line or a plane including the zero point (not
linearly dependent).
The coordinates are specified in their respective units.
The origin of the ANSYS mesh should be at (0,0,0).
Finally in Ansys Output File ,
the user specifies the new output file "project_ CFD.cdb"
(FIGURE 12.6 - (4)) containing the transferred CFD results on the solid boundaries coded in
ANSYS.
12.3.3 Surface Selection
After completion of the page under Global Parameterstab page, the user has to complete the
Surface Selection page before creating the ANSYS output file.
When the ANSYS input file is read in Ansys Input File (FIGURE 12.6 - (2)), the common
surfaces on which the data must be transferred are identified in the ANSYS mesh. The
FINE™/Open GUI lists each surface with the corresponding coded value (FIGURE 12.7 - (1)).
By clicking on Selected Surface Properties button ( FIGURE 12.7 - (2)), a new window
( FIGURE 12.8 ) allows the user to specify the solid patches from which the data will be
interpolation type
interpolated. Following interpolation parameters can also be defined:
(Interpolation type) and the allowed maximal distance (Maximum distance).
For the moment, only a non-conservative transfer is available. In the non-conservative approach,
each node of a surface of the Ansys mesh is projected on the face of the corresponding selected
Hexpress patches. Since for a face, the vertices are not necessary coplanar, the face has to be
triangulated. The projection direction of the Ansys node is the normal of the tested triangle. The
nearest triangle is used to interpolate the CFD values at the location of the projection. When the
projection of the node of a surface of the Ansys mesh is not on the selected solid patches, the
nearest triangle is found. The value at this point will be an interpolation of the CFD values on the
nearest edge. An allowed Maximum distance can be specified to check if the triangle used in the
interpolation process is closed enough.
FIGURE 12.7
Surface Selection of ANSYS outputs
The maximum distance of the ANSYS output on the surface selection page, is always expressed in
meters (independent from the mesh units or project preferences)
FIGURE 12.8
Add solid patches to ANSYS surface
Then, the user specifies the solid CFD patches in the list of Selected Solid Patches by <Ctrl> or
<Shift> and left-click. When the solid patches are well selected, the window has to be closed (Ok)
and the patches will appear in the list Connected Solid Patches(FIGURE 12.7 - (3)).
To ensure a complete data transfer, the selected Hexpress™ solid patches have to completely overlap
the ANSYS surface. The area of the selected Hexpress™ solid patches can be larger than the area of
the ANSYS surface.
The Ansys surfaces must be totally overlapped by the selected Hexpress patches in order to
ensure a complete data transfer. Therefore, a periodic shift of the Hexpress patches can be
necessary to match the common ANSYS surface.This shift must be specified for each solid patch,
highlighted in Connected Solid Patches list, by activating Periodic solid patch (FIGURE 12.7 -
(4)). The rotation and translation shifts are respectively specified in degrees and Hexpress™ mesh
units.
Moreover one ANSYS surface can be covered by a group of solid patches and by the same group
which is rotated (or translated). Consequently, the Number of repetition has to be specified
(FIGURE 12.7 - (4)). The toggle Partial indicates that the patch is copied by rotation or transition
or both.
Launching the CFD computations will create the new Ansys file. The transfer is performed at the
end of the computation, before the creation of the Cfview files.
12.3.4 Import Results in ANSYS
The new output file "project_CFD.cdb" (FIGURE 12.6 - (4)) containing the transferred CFD
results on the solid boundaries coded in ANSYS is now available. When reading this file in
ANSYS with the command CDREAD, following rules need to be respected:
l Only the FE model (file ".cdb") has to be imported.
If the coded values have been prescribed by using the solid model, the solid model has not to be
saved in the original ".cdb" input file . If the solid model is saved,
conflicting values are set on the fluid-structure boundaries and the initial coded values will be
kept. Moreover these artificial boundary conditions have to be removed in the ANSYS project
before importing the modified archive file with the suitable boundary conditions. If they are not
removed, the coded values will replace the transferred values.
(continued in FINE™/Acoustics output)
12.4 FINE™/ACOUSTICS OUTPUT
FINE™/Open with OpenLabs™ is now able to output the absolute static pressure on solid
patches to files in FINE™/Acoustics format, thus allowing the user to perform noise predictions
with the static pressure computed by FINE™/Open with OpenLabs™.
There is no interface available. The user has to set the expert parameter out_writeFINEAcoustics_
to 1 to activate the FINE™/Acoustics output.
For steady computations, after the computation finished, two files will be created in a new folder
FINEAcoustics under the computation directory.
l A mesh file "_mesh.vnx" storing the mesh of the solid patches.
l A data file "_data.vnx" containing the value of the absolute static pressure on the solid patches.
For unsteady computations, after the computation finished, one mesh file and one/multiple data
file(s) will be created in a new folder FINEAcoustics under the computation directory.
l A mesh file "_mesh.vnx" storing the mesh of the solid patches.
l One/multiple data file(s) "_data#.vnx" containing the value of the absolute static pressure on
the solid patches. Where # is the index of the data file.
In case of unsteady computations, the expert parameter out_writeFINEAcousticsInterval_ta_ is
used to specify the save frequency. If the value is set to 0, the FINE™/Acoustics output will be
generated as for a steady computation: only the mesh file and the data file corresponding to the
last time step. If the value is set to an integer larger than 0, then a data file will be created at each
out_writeFINEAcousticsInterval_ta_ time step. The name of the data file will be named with the
extension _data#.vnx, with the index # being 0, 1, 2, 3…
If the computation is a restart from a previous computation with the import of the convergence,
the previous computation will be copied in the
the FINE™/Acoustics output
computational directory of the new computation.
files of
CHAPTER 13.
TASK MANAGER
Using the Solver menu in FINE™/Open with OpenLabs™, computations can be started, saved and
stopped or killed. For basic task management these menu items are sufficient.
The Task Manager provides more advanced features for the management of (multiple) tasks. It allows
the user to manage tasks on different machines on a network, to define parallel computations or to
delay tasks to a given date and time.
Before using the Task Manager for the first time it is important to first read the next section. This
section provides important information for getting started with the Task Manager. The user should read
this section carefully to fully benefit of the capabilities of the Task Manager.
From FINE™/Open with OpenLabs™ the Task Manager can be accessed by clicking on the Switch to
TASK MANAGER button (     ) on the main icon bar. The interface, as shown in FIGURE 13.1, will
appear.
In the Task Manager Interface section the Task Manager interface is described in detail including a
description of all
limitations of the Task Manager are listed in the
Limitations section.
its capabilities. The current
Task management through the use of scripts is also possible and has the benefit that it is not necessary
to remain logged on to the machine on which the tasks are launched. See Task Management Using
Script section for more detail on the scripts to use to launch NUMECA software.
In this section
13.1 Getting Started
13.2 The Task Manager Interface
13.3 Parallel Computations
13.4 Task Management Using Scripts
13.5 Limitations
361
366
378
382
395
13.1 GETTING STARTED
The PVM Daemons
The Task Manager is based on the PVM library. It allows FINE™/Open with OpenLabs™ to
control processes and the communication between processes on all the machines available to the
user. PVM works with a virtual machine managed through a pvm daemon. In this section the way
the PVM daemons work and their limitations under Windows are described.
What PVM Daemons Do
If a user starts the FINE™/Open GUI on a given computer where no PVM daemon is running,
FINE™/Open with OpenLabs™ will automatically start the process pvmd on this machine that
becomes the virtual machine server for the user. When adding a host in the Task Manager (on the
Hosts definition page) a pvmd is started on the remote computer and this machine is added to the
virtual machine. If the user now starts FINE™/Open with OpenLabs™ on this second computer
the host list will contain the original machine on which the pvmd was first started. The original
machine remains the server for all the associated virtual machines.
If the user logs on a third computer on which no pvmd is running and starts the FINE™/Open
GUI, FINE™/Open with OpenLabs™ will start a pvmd on this machine and this will become the
server of a new virtual machine. If the user attempt to add a machine already controlled by a
different virtual machine (for example contained in the list controlled by machine 1), he will see
the message "can not connect the virtual machine".
If the user wants to have the three computers in the same virtual machine, one of the virtual
machines servers must be shut down (on the Hosts definition page) and this machine can then be
added to the existing virtual machine.
Limitation under Windows
On windows only one pvmd can run and therefore, only a single user can connect to the virtual
machine. If another user wants to use the NUMECA software on the PC as server (FINE™/Open
with OpenLabs™) or as client (the FINE™/Open solver), the first user must shut down the pvm
daemons on this machine. To shut down go to the Hosts definition page and click on Shutdown.
This will close the interface and removes all the pvm daemons on the machine. Remove the files
pvml.<userID> and pvmd.<userID> from the directory defined by the PVM_TMP (by default
C:\tmp).
Multiple FINE™/Open with OpenLabs™ Sessions
During a FINE™/Open with OpenLabs™ session all the tasks defined by the user are stored in
the "hexatasks" file in the NUMECA tmp directory. This is the ".numeca/tmp" directory in the
home directory of the user. On Linux the home directory corresponds to the HOME environment
variable. This is also true on Windows if this variable is defined and, if it is not the case, it is set to
the concatenation of HOMEDRIVE and HOMEPATH environment variables.
On Windows, the home directory can not contain white spaces: if the HOMEPATH variable of the
user contains white spaces, a HOME variable must be defined corresponding to a directory that does
not contain white spaces.
When FINE™/Open with OpenLabs™ is started more than once using the same virtual server, it
can cause conflicts with the other FINE™/Open with OpenLabs™ sessions. For example, the
user can define tasks in both interfaces but the task definitions saved when exiting FINE™/Open
with OpenLabs™ can be overwritten by the other sessions. Therefore, it is not advised to open
multiple FINE™/Open with OpenLabs™ sessions when the Task Manager is used.
Machine Connection from Linux Platforms
The Task Manager allows the user to control processes on all the machines connected to the
network. The rsh command is used by the PVM library to access the machines. Before using the
Task Manager, the following actions must be done:
1. Modify the .rhosts file in the home directory in all the machines which can be used by the Task
Manager. i.e.: if the machines machine1 and machine2 will be used by the users tasks from
machine_master, the file in machine1 and machine2 must be modified as follows:
line1: machine_master <login1>
where machine_master is the host name. login1 is optional. If the login on machine_master is
different from login1, the user in machine_master will be asked to supply a password when
connecting to machine1 and machine2.
The rhosts file needs to be ended by a blank line.
The file permission must be set to 'rw' (on Linux: chmod 600 ~/.rhosts).
2. Test the rsh command on the desired machine: an external check that the .rhosts file is set
correctly is to enter the following command line:
rsh remote_host ls <Enter>
where remote_host is the name of the machine to connect to. If the login on the remote host is
not the same, ensure that the .rhosts file contains the line:
remote_hostlocal_login
and in this case the command line is:
rsh remote_host -l local_login ls <Enter>
If the rhosts file is set up correctly, a listing of the files is shown on the remote host.
Due to a limitation of the PVM library, FINE™/Open with OpenLabs™ can not be connected to a
machine where FINE™/Open with OpenLabs™ has already been started. When PVM tries to establish
the connection, it detects that a FINE™/Open with OpenLabs™ server is already running and/or pvm
daemons are still running and refuses the connection. To solve this problem, the PVM daemons must
be stopped on the machine on which FINE™/Open with OpenLabs™ must be connected:
1. Log on the machine where the connection must be established.
2. Start FINE™/Open with OpenLabs™ and open the Task Manager
through Modules/Task
Manager and use the button Shutdown of the page Hosts Definition. The button Shutdown can
be used to stop all the PVM daemons of all the machines connected to this FINE™/Open with
OpenLabs™ virtual server. This action will stop all the daemons on all the machines connected,
kill all the tasks and exit FINE™/Open with OpenLabs™.
3. Remove all the /tmp/pvmd.<userID> and /tmp/pvml.<userID> files.
4. Repeat this operation for all the machines on which the problems appear.
5.
If PVM still has a problem obtaining a connection, it will print an error message either to the
screen, or in the log file /tmp/pvml.<userID>. Please send this log file to our local support office.
All these operations apply only to the user's daemons and user's files. Multiple users can use the Task
Manager simultaneously. There is no interaction between the PVM daemons and the PVM log files of
different users.
The Task Manager does not allow the user to launch processes from a Linux platform on a Windows
platform.
Machine Connection from Windows Platforms
1. The Numeca RSH Daemon has to be started. The user is referred to the installation note for
more details.
2. Modify the rhosts.txt file in C:\WINDOWS in all the machines which can be used by the Task
Manager. i.e.: if the machines machine1 and machine2 will be used by the users tasks from
machine_master, the file in machine1 and machine2 must be modified as follows:
line1: machine_master <login1>
where machine_master is the host name. login1 is optional.
The rhosts file needs to be ended by a blank line.
3. Test the rsh command on the desired machine: an external check that the rhosts.txt file is set
correctly is to enter the following command line:
rsh remote_host dir <Enter>
where remote_host is the name of the machine to connect to. If the login on the remote host is
not the same, ensure that the .rhosts file contains the line:
remote_hostlocal_login
and in this case the command line is:
rsh remote_host -l local_login dir <Enter>
If the rhosts file is set up correctly, a listing of the files is shown on the remote host.
On Windows,
DIRECTORY>/fine#/bin/
the rsh.exe executable is
located in < NUMECA_ INSTALLATION_
Due to a limitation of the PVM library, FINE™/Open with OpenLabs™ can not be connected to a
machine where FINE™/Open with OpenLabs™ has already been started. When PVM tries to establish
the connection, it detects that a FINE™/Open with OpenLabs™ server is already running and/or pvm
daemons are still running and refuses the connection. To solve this problem, the PVM daemons must
be stopped on the machine on which FINE™/Open with OpenLabs™ must be connected:
1. Log on the machine where the connection must be established.
2. Start FINE™/Open with OpenLabs™ and open the Task Manager
through Modules/Task
Manager and use the button Shutdown of the page Hosts Definition. The button Shutdown can
be used to stop all the PVM daemons of all the machines connected to this FINE™/Open with
OpenLabs™ virtual server. This action will stop all the daemons on all the machines connected,
kill all the tasks and exit FINE™/Open with OpenLabs™.
3. Remove all the pvmd.<userID> and pvml.<userID> files. Under Windows these files should be in
the directory defined by PVM_TMP (by default this directory is C:\tmp).
4. Repeat this operation for all the machines on which the problems appear.
5.
If PVM still has a problem obtaining a connection, it will print an error message either to the
screen or the log file pvml.<userID> in the directory defined by the environment variable PVM_
TMP (by default C:\tmp). Please send this log file to our local support office.
All these operations apply only to the user's daemons and user's files. Multiple users can use the Task
Manager simultaneously. There is no interaction between the PVM daemons and the PVM log files of
different users.
When a user stops the pvmd on a remote host (using Remove Host button on the Hosts Definition
page) and immediately try to restart it (using the Add Host... button), a message will appear stating
that it is not possible to connect. This problem does not occur in general since there is no need to
remove a host and add it immediately after. When it occurs the only solution is to wait until the
host is available again (after 5 to 10 minutes).
From time to time, when a user tries to connect on a remote host, an error message can appear very
briefly: "Can not connect to RSH Port!!!" This may happen on a Windows machine connecting to
a host, disconnecting, and trying to reconnect again to the same host. This will stop the FINE™/Open
GUI. Windows contains a socket release time parameter which keeps the connection for some time.
Remote Copy Features on Linux
All the tasks defined by the user are associated with files used or created by the NUMECA
software. When the files are not visible from the machine on which the task will be launched (i.e.
the files are on the local disk of the host where FINE™/Open with OpenLabs™ is running), the
user can use the remote copy feature available in the Task Manager. All the files needed by the
tasks will be transferred into a directory (specified by the user) on the remote machine and at the
end of the computation all created or modified files are transferred back to the host machine. By
default, the remote directory is "/tmp". The user can specify any other directory, as long as it is
visible from the remote host and has write permission.
This feature uses by default the scp command (encapsulated in the nircp script) unless the
environment variable NI_RCPCMD is set to rcp or scp. In this case, the command defined by
this environment variable will be launched.
l for csh or tcsh:
setenv NI_RCPCMD rcp
l for bash or ksh:
export NI_RCPCMD = rcp
Before using the remote copy feature when the environment variable NI_RCPCMD is set to rcp,
it is advised to first check if the rcp command works correctly between the machines:
l Type the command: touch test; rcp -p -r test destination_machine:/tmp/test. If no error is
returned by the system, the remote copy works between the local host and the "destination_
machine". Errors may appear if the .cshrc file contains an stty command. To be able to use the
remote copy feature, remove all the stty commands from the .cshrc file.
l If the login on the local host is different from the login on the remote host, type the command:
touch test; rcp -p -r test remote_login@destination_machine:/tmp/test.
13.2 THE TASK MANAGER INTERFACE
13.2.1 Hosts Definition
The Hosts definition page shows the hosts in the virtual machine, the operating system of the
machine and their connection status. For an explanation of the virtual machine see the PVM
Daemons section. If the connection is not OK, it means that the corresponding computer is no
longer in the virtual machine. This may occur, for example, if the computer has been rebooted.
FIGURE 13.1
Hosts definition page
Add a Host
When the user clicks on the Add host... button, the interface asks for a host name and a login
name. The login name is optional. It is needed only if the user login on the local host and the one
on the remote host are different.
FIGURE 13.2
Add a host pop-up window
When the user presses the Accept button, the host name appears in the host list, with type of
operating system and its connection status. At this point, the host is in the virtual machine, and is
ready to receive a task.
if the connection can not be established, check for more detail in the PVM Daemons , Machine
Connection from Linux Platforms and Machine Connection from Windows Platforms sections.
Remove Host
When the user clicks on the Remove Host button, the selected host is removed from the list, and is
no longer available in the virtual machine. This operation is not allowed when a task is running on
the host to be removed, or when the local host is selected.
Shutdown
When the user clicks on the Shutdown button, all hosts in the virtual machine are removed.
FINE™/Open with OpenLabs™ exits and the virtual machine halts. All running tasks are killed.
This option is useful when the user wants to change the machine on which FINE™/Open with
OpenLabs™ is running.
13.2.2 Tasks Definition
A task is a collection of subtasks where a subtask is one of the program with its arguments (".run"
file for HEXSTREAM and macro file ".py" for CFView™). The different subtasks of a given
task can be run simultaneously if the output of one subtask is not needed by other ones (for
example: several CFView™ subtasks with different macro files or several HEXSTREAM
subtasks with different run files started on different computers). If the output of one subtask is
needed by another, it must be run sequentially. For example: the output of a FINE™/Open
computation is used for starting CFView™.
FIGURE 13.3
Tasks definition page
Task List
In this section, the user can visualize the defined tasks and their status. To create a task, click on
the New Task button. The defaults task name can be modified by clicking on the Rename Task
button. The selected task can be removed by clicking on the Remove Task button.
Once a task has been created and defined , it can be started or stopped by
clicking on the Start, or Stop buttons, respectively.
After a subtask is defined, the Save button can be used to save all necessary files to start a parallel
computation in batch mode. When a queuing system is used, a set of default templates is available
in order to submit the job to the queue. New templates can also be created by the user.
A task can be delayed: click on the Delay button and enter the date and time for when the task
should be launched in the dialog box. The delayed task can be disabled using the Cancel button.
FIGURE 13.4
Task Delay pop-up window
When the user validates the data, a small watch in the task list indicates that the task is scheduled:
FIGURE 13.5
Task List with Delay window to start a task at a later moment
their starting times are reached. When starting the FINE™/Open GUI again, all
When exiting Task Manager, all the delayed tasks are automatically started and stay in sleep mode
the task
until
managers relating to the delayed tasks, still in sleep mode are killed, and the FINE™/Open Task
Manager recovers control of these tasks.
Task Definition
In this section, the subtasks of the selected task in the Task Listare discussed. A subtask is
defined by its type (hexstream or cfview), its status and the host on which it is launched. To add a
subtask click on the New button in the subtask section. Select the executable name (hexstream or
cfview) and the host on which the process should be started in the two pull-down boxes beneath
the task list. The host name list contains the hosts that are in the virtual machine as set in the Hosts
definition page.
Subtask Arguments
Definition of Input and Output
Once a subtask is created, input and/or output files must be defined in the Subtask arguments
section:
l The FINE™/Open solver (hexstream) requires one argument file: the name of the run file.
This files must be created using the menu Project/Save Selected 'Run' Files in the
FINE™/Open GUI.
FIGURE 13.6
FINE™/Open solver Subtask Arguments
l The flow visualization system CFView™ requires two files: the run file and a macro file 
FIGURE 13.7
CFView™ Subtask Arguments
The ".run" file is automatically opened by CFView™ before starting the macro. The macro file
may open other ".run" files to perform flow comparisons .
Simultaneous or Sequential Mode
A process may be executed simultaneously with the other subtasks (by selecting Run
Simultaneously with Previous Subtask ) or sequentially (by selecting Run After Previous
Subtask). In the second case (set by default), the process waits until the previous subtask has
finished before starting. This option is only available for the hexstream subtasks. Only a limited
number of tasks may be performed at the same time, depending on the available licenses. The
subtasks related to postprocessing with CFView™ are always executed in sequential mode.
Remote Copy
The Remote copy to button allows the user to specify that the necessary files are not available on
the remote machine and must be transferred. This option is only available for the hexstream
subtasks.
Parallel settings
MPI system
The FINE™/Open flow solver has an integrated multiprocessor machine concept. The button
Flow solver parallel settings is used to set up the parallel computation if the computation was set
up to be launched in parallel (more details in the Launching Mode Chapter).
When the dialog box is opened, the block list displays all the blocks of the mesh defined in the
Launching Mode page within the FINE™/Open GUI.
The parallel processing can only be used on multiprocessor machines (shared memory mode) or on
machines with the same operating systems (homogenous distributed memory mode), see the Parallel
Computations section for more detailed information on parallel computations.
Two types of license keys can be used to trigger parallel computations: either a seat-locked type
(MPROC) whose associated cores cannot be shared between several simultaneous parallel
computations or flexible type (FFLEX) whose associated cores can be distributed between several
simultaneous parallel computations. The flow solver uses the seat- locked type in priority.
Checking the button Flexible Cores Type from License forces the flow solver to use the flexible
license key type in priority.
For the MPI libraries, the user has the possibility to use MPICH2 and IntelMPI (libraries v5.0.3)
on Windows, while OpenMPI (librairies v2.1.2) and IntelMPI (libraries v5.1.3) are available on
Linux. The MPI choice is set for each subtask; each subtask may have a different MPI choice.
SGE system
Within the Task Manager provided in FINE™/Open with OpenLabs™, the parallel process can
be set using the SGE (Sun Grid Engine) batch system.
This last system includes the possibility to add a SGE type host and to define arguments needed to
launch the computation within the Task Manager.
Host Definition
In the page Hosts definition the user needs to add hosts. When adding a host, automatic checks
are performed:
1.
2.
3.
it will detect if the "sge_qmaster" is running on the platform. If not, it means that the platform
does not have SGE capabilities or the platform is not the SGE master processor.
it will detect all parallel environments defined in SGE.
it will detect all parallel environments that the user is allowed to use. If no parallel environment
could be accessed by the user, his login should be added to the user list by the SGE
administrator.
When all checks are successful, the SGE capability of the added host is activated and the user can
see if the host added is a SGE platform within the Task Manager GUI.
Task Definition
In the page Tasks definition, if the user select a SGE platform when launching an hexstream task
in parallel, he has the access to the MPI system or the SGE system.
When the SGE system is used, the SGE environment has to be specified. Depending on the
settings in the .run file, the number of processors will be set automatically.
The number of processors defined in the option Queuing system is currently restricted to the
Total number of processes defined in the Launching mode page.
Two types of license keys can be used to trigger parallel computations: either seat-locked type
(MPROC) whose associated cores cannot be shared between several simultaneous parallel
computations or flexible type (FFLEX) whose associated cores can be distributed between several
simultaneous parallel computations. The flow solver uses the seat- locked type in priority.
Checking the button Flexible Cores Type from License forces the flow solver to use the flexible
license key type in priority.
Process Management
Once the process is starting, a script file ".sge" is created in the computation folder.
is thus chosen
The name of the SGE job is limited to 8 characters and the following format
"comp####" where #### stands for a any number depending of the number of SGE jobs already
running under the same environment.
There are no communication between the flow solver and the task manager because the flow
solver is not launched using PVM daemon. To test if a computation is running, the "qstat"
command with the job-ID number of the SGE job should be used.
To save and stop the SGE job, the user could use the Stop function of the Task Manager. It will
create a ".stop" file in the running computation directory that will enable the flow solver to stop
after saving the solution at the next iteration or after the full multigrid initialization.
To kill the SGE job, the user could use the Kill function. The Task Manager will then use the
SGE™s function "qdel" to kill the computation without saving the solution.
To kill the flow solver properly, the SGE™s "execd parameters" variable should be set to "NOTIFY_
KILL=TERM" and the "notify time" variable of nodes should be set to a sufficient value to allow the
flow solver to exit properly. We invite the user to ask the SGE administrator to check these variables.
User-defined Templates on Queuing System
If the option Queuing system in the Task Definition page is activated, the user needs to select a
template in order to submit the computation to the queue. By default, a set of templates is
available for the supported queuing system SGE (with corresponding extension .sge).
The user can also create a new template to customize the settings: queuing system environment,
OpenMPI, etc. In order to use an user-defined template, the user has to:
l name the new template using the extension .sge,
l copy the template to the queuing templates folder:
l On Linux systems:
"NUMECA_
templates/"
INSTALLATION_
DIRECTORY/fineopen72/COMMON/queuing_
l On Windows systems:
"NUMECA_INSTALLATION_DIRECTORY\fineopen72\bin\queuing_templates\"
It is strongly suggested to create a new template based on the existing templates. All the existing
templates can be found in the queuing templates folder mentioned above. The Figure shows the
contents of the default SGE template. Based on this template, the user can customize the SGE
environment, the OpenMPI settings and the command launching the computation. Please refer to
How to Launch the flow solver in Parallel using SGE on LINUX for the detailed explanation of
the template contents.
The user must obey the following rules when creating a new template:
l Any line beginning with # (except #! and #$) is a comment.
l The first blank line MUST be placed after the section defining queuing system environment
and before the section defining the OpenMPI settings. Here, TaskManager will define the
SGE environment variables (number of processors, name of the computation, etc.) and the
NUMECA variables (NI_VERSION_DIR and NUMECA_SOFT_VERSION), depending
on the user-settings in TaskManager.
l The comment line "# COMPUTATION SETTINGS" MUST be kept and placed before the
command launching the flow solver. Here, TaskManager will define the computation settings
(variables RUN_ FILE, STEERING1, STEERING2 and PREC, which are used in the
command launching the flow solver).
FIGURE 13.8
The default template for SGE (default_hexstream.sge)
Message Window
When a task is started, a Task Manager process is launched to manage the task: process
communication, automatic launching of the sequential and parallel subtasks. A message window
linked to the Task Manager is opened. In this window the user can follow the evolution of the
status of all the subtasks of the current task. For flow solver computations the iterations are also
displayed in this window.
At the bottom of the Task Manager window a Refresh Rate can be chosen. This rate determines
how frequently the Task Manager window is updated. A higher refresh rate will update the
information in the window more frequently but will use more of the available CPU.
FIGURE 13.9
Task Manager information window
If the user quits the FINE™/Open GUI, all the message windows will remain open and the tasks will
continue. Closing a message window will immediately kill all the subtasks of the corresponding task.
13.3 PARALLEL COMPUTATIONS
13.3.1
Introduction
Parallel computations can be defined through the FINE™/Open GUI using the Task Manager
and the Launching Mode page that allows to split the unstructured mesh into the required
number of partitions. Parallel computation reduces the calculation time of a given problem by
splitting the task among a number of processes, each of which works on part of the problem.
Communication between these different processes is necessary at the partition interfaces to ensure
that the solution near the boundaries is consistent across the different partitions.
A domain decomposition approach is taken to the parallelization of the flow solver. The METIS
library from the University of Minnesota is used to perform the serial partitioning. This library
uses the graph of the mesh to perform the partitioning, with the goals of minimizing the
communication cost, using a selection of metrics, and balancing the number of grid cells in each
partition. For multigrid meshes, partitioning operations are performed on the finest available level,
this ensuring optimal load balancing for computations on this level. Coarse multigrid level
partitions are then constructed successively using the hierarchy mesh data structure. For parallel
partitioning, the library ParMETIS is used. This library ParMETIS extends the functionality
provided by METIS and is designed to run in parallel. After partitioning the mesh in parallel, the
multigrid agglomeration will be performed based on the partitions. The parallel partitioner and
significantly accelerate the preprocessing and reduce the memory
agglomeration will
consumption. The drawback of agglomeration based on the partitions is that the multigrid will not
remain identical when the number of processors is different, therefore the convergence history of
global quantities will not remain identical, too. For the selection of the sequential or parallel
partitioner, please refer to Launching Mode section.
At the interfaces between partitions, the meshes are overlapped by a single cell to facilitate inter-
partition communication. Data in these ghost cells is replaced with the correct value at various
points in the computation procedure where an incorrect value of solution would adversely
influence the calculation. In addition to the cells that share faces, cells that share nodes need to be
communicated in the case of viscous calculation due to the diamond control volume interpolation
technique.
The FINE™/Open solver allows an arbitrary number of processes (at least equal to the number of
blocks in case of multiblock computation) to be assigned to a given problem. One processor
should be defined, within the Task Manager, for each of the available partitions. Each processor
will launch a self- contained instance of the solver using the MPI parallel message passing
interface. Both shared memory and distributed memory are supported as are shared/non-shared
disk configurations.
By default, FINE™/Open uses the MPICH2 libraries on Windows operating systems and the
OpenMPI libraries v1.6 on Linux operating systems.
Generally, each cluster has its own characteristics and we recommend to use a local version of
OpenMPI which has been compiled for supporting infiniband connection. This library is generally
provided by the cluster manufacturer. The OpenMPI provided in the installation package does not
support infiniband connection. For example in order to use a local version of OpenMPI, please refer
to "Use an External OpenMPI Library on Linux" (p. 381).
The parallel implementation is available under Linux and Windows platform. Currently, each
partition constructed is of equal size by default, which is the optimal configuration for
homogeneous systems.
13.3.2 Management of Inter-block Communication
Each partition must be assigned to a separate process. Any number of processes can be assigned
to a single processor, but each must be defined separately. When starting the computation each
process has a self-contained instance of the solver referencing its own input and output files.
Communication between overlapping ghost cells of the different processes occurs at various
points in the calculation, when updated values in the ghost cells are required.
The partitions have been optimized to balance the computational load, by ensuring the same
number of cells are located in each partition by default, and to reduce the inter- process
communication, by minimizing the number of connections between the partitions.
A number of global communications are also necessary during the calculation to make global
variables, such as the residuals, available to all processes.
At the end of the computation the outputs from the different processes are collected and the full
solution is reconstructed, by the 0th (i.e. host) process, for visualization and post-processing.
13.3.3 How to Run a Parallel Computation
The settings required for running a parallel computation from the Task Manager are described in
Subtask Arguments section and the equivalent batch commands in Launch the FINE™/Open
solver in Parallel using Scripts section. The general stages for running a parallel computation are
as follows:
1. Create the required number of partitions in the FINE™/Open Launching Modepage. This
number should be strictly equal to the number of processes required.
2. Set up the necessary PVM daemons on the host machines using the Hosts definition window
of the task manager.
3. Follow the instruction in Subtask Arguments section for interactive, and Launch the
FINE™/Open solver in Parallel using Scripts section for batch computations.
13.3.4 OpenMPI Options
The FINE™/Open solver uses the default OpenMPI options on Linux. The user can change the
OpenMPI options in order to get a higher performance. In general, all the MCA parameters can
be defined by the user. The MCA parameters may be set in several different ways:
l add the options in the command line, .
l set the options in the user profile ($HOME/.profile). For example:
l for csh or tcsh:
setenv OMPI_MCA_btl_sm_eager_limit 9192
l for bash or ksh:
export OMPI_MCA_btl_sm_eager_limit=9192
l create
file
".default_ mpi'"
folder <NUMECA_ INSTALLATION_
the
DIRECTORY>/fine#/_mpi/, where # is the FINE™/open version. Then edit the file ".default_
mpi" and set the options. For example:
under
l for csh or tcsh:
setenv OMPI_MCA_btl_sm_eager_limit 9192
l for bash or ksh:
export OMPI_MCA_btl_sm_eager_limit=9192
l create a file "default_mpi'" under the folder $HOME/.numeca/, where $HOME is the home
directory of the user account. Then edit the file "default_ mpi" and set the options. For
example:
l for csh or tcsh:
setenv OMPI_MCA_btl_sm_eager_limit 9192
l for bash or ksh:
export OMPI_MCA_btl_sm_eager_limit=9192
The following MCA parameters may be required to tune:
l OMPI_MCA_mpi_leave_pinned: When mpi_leave_pinned is set to 1, OpenMPI aggressively
leaves user memory registered with the OpenFabrics network stack after the first time it is used
with a send or receive MPI function. This allows Open MPI to avoid expensive registration /
deregistration function invocations for each send or receive MPI function. When the value is
set to 0, it is disable. -1 (default) let the system decides. Setting this parameter to 0 has helped
to performed a parallel partitioning on a cluster.
l OMPI_MCA_btl_###_eager_limit (### being tcp, openib,sm,...): This argument controls the
size of the message above which the processor must wait a confirmation from the other
processor that the message has been properly delivered. If the message is smaller than the
specified value, the message is sent and the processor does not wait any confirmation of
reception. If the message is bigger than this value, the message is split in sub-packets of fixed
size and each sub- packet is sent one by one and the processor waits a confirmation of
reception from the other processor before sending the next packet. By removing this
parameter, the size is reduced to the default one (4096 b= 4 Kb) and the processors must wait a
confirmation from the other processors in order to go on for all messages bigger than 4 Kb.
This may have an impact on the speed up but it secures the communication.
13.3.5 Use an External OpenMPI Library on Linux
By default, FINE™/Open with OpenLabs™ uses the OpenMPI library on Linux operation
systems. FINE™/Open with OpenLabs™ also allows to use an external OpenMPI library, which
may be a tuned, customized or hardware specific OpenMPI library. In order to use an external
library, the user has to re-define the runtime environment, which can be done in two ways:
l create
file
".default_ mpi'"
folder <NUMECA_ INSTALLATION_
the
DIRECTORY>/fine#/_mpi/, where # is the FINE™/Open with OpenLabs™ version. Then
edit the file ".default_mpi" and specify the external OpenMPI library in the file ".default_mpi"
(here the external library is located in /tmp/libs/OpenMPI/ompi1.4):
under
l for csh or tcsh:
setenv NI_MPI_DEFAULT ompi
setenv NUMECA_MPI_DIR /tmp/libs/OpenMPI/ompi1.4
l for bash or ksh:
export NI_MPI_DEFAULT=ompi
export NUMECA_MPI_DIR=/tmp/libs/OpenMPI/ompi1.4
In this way, the FINE™/Open flow solver will use the specified external library when launching
computations.
l create a file "default_mpi'" under the folder $HOME/.numeca/, where $HOME is the home
directory of the user account. Then edit the file "default_ mpi" and specify the external
library is located in
OpenMPI
/tmp/libs/OpenMPI/ompi1.4):
library in the file "default_ mpi" (here the external
l for csh or tcsh:
setenv NI_MPI_DEFAULT ompi
setenv NUMECA_MPI_DIR /tmp/libs/OpenMPI/ompi1.4
l for bash or ksh:
export NI_MPI_DEFAULT=ompi
export NUMECA_MPI_DIR=/tmp/libs/OpenMPI/ompi1.4
In this way, all the NUMECA flow solvers running in this user account will use the specified
external library.
13.3.6 Limitations
l The distributed memory mode is restricted to homogeneous system. While not strictly
necessary, it is recommended that machines of the same speed are used, as all partitions are of
equal size by default and therefore, require the same computational cost.
l The number of processors should be strictly equal to the number of partitions. It is possible to
run more than one process on a single machine, but each process must be defined separately.
l When running parallel computations, the path to the project has to be identical on both the
local and remote machines. For example, for distributed memory parallel computations, a
folder must be mounted on the remote machine and share the same disk, in order to store the
project directory that will be run in parallel on multiple hosts.
l The blank space is not allowed in the path name and the computation name.
13.4 TASK MANAGEMENT USING SCRIPTS
This section provides information on how to launch the installed NUMECA Software from a
shell, without using HEXPRESS™, FINE™/Open with OpenLabs™ or CFView™ interfaces.
Every time a task is started (Task Manager) a script file is automatically created. On Linux the
name of this file has the extension ".batch" and under Windows the extension is ".bat". Such files
contain text lines with the commands to launch the software with the appropriate command
arguments. To launch a task from a shell simply execute the automatically generated file by typing
its name.
In the next sections the commands available to launch NUMECA software are described in more
detail.
13.4.1
Launch HEXPRESS™ Using Scripts
How to Launch HEXPRESS™ on Linux
1. Create a template and geometry files (".igg", ".bcs" and ".dom") using the HEXPRESS™
interface.
2. Start HEXPRESS™ to create a mesh from these files by typing:
hexpress -batch -project /user/test.igg -niversion <version>
The command line to start the grid generator HEXPRESS™ contains its name, the full path name
of the mesh that will be saved (geometry ".dom" should be located in the same directory and
should have the same name) and the HEXPRESS™ release that will be used (i.e. open211_1).
The "-batch" option avoids the display of the HEXPRESS™ graphical user interface.
How to Launch HEXPRESS™ on Windows
1. Create a template and geometry files (".igg", ".bcs" and ".dom") using the HEXPRESS™
interface.
2. Start HEXPRESS™ to create a mesh from these files by typing:
<hexpress_path>\hexpressx86_64.exe -batch -project c:\users\mesh.igg
The command line to start the grid generator HEXPRESS™ contains its name, the full path name
of the mesh that will be saved (geometry ".dom" should be located in the same directory and
should have the same name) and the HEXPRESS™ release that will be used. The "-batch"
option avoids the display of the HEXPRESS™ graphical user interface.
13.4.2 Launch the FINE™/Open Solver in Sequential Mode
Using Scripts
How to Launch the flow solver in Sequential mode on Linux
1. Create a script file (for example, with the name "batch.sh"). Such a script file must be created
with execution permission in order to launch a series of computations. An example of a
"batch.sh" file for a series of computations on Linux:
#! /bin/csh
hexstreamdp "<project_path>/computation_1/computation_1.run" -steering "<project_
path>/computation_1/computation_1.steering" -niversion "<version>"
The script is started in a C-shell due to its first line: "#! /bin/csh". The command line, to start
the FINE™/Open solver, contains its name (hexstreamdp is the double precision version of the
FINE™/Open solver), the full path name of the ".run" and the corresponding ".steering" files
to launch, and the FINE™/Open with OpenLabs™ release that will be used (for example,
open211_1).
Mixed and double precision versions of the FINE™/Open solver are available.
2. Set Permission for execution for the script file "batch.sh" by typing the command: "chmod
755 batch.sh".
3. Create an input file (".run") for each computation. To create these files through the
FINE™/Open GUI, click on the Project/Save Selected 'Run' Files menu to save the ".run"
file of the activated computation, after opening the corresponding project.
4. Launch the script "batch.sh" by typing the script file name: "./batch.sh".
Clicking on the menu Solver/Save batch file, a script "computation_name.batch" can be created
in the corresponding computation subfolder. This script enables the user to launch the same
computation in batch.
How to Launch the flow solver in Sequential mode under Windows
1. Create Script File ".bat". An example of ".bat" file for a series of computations on Windows:
<NUMECA_install_dir>\fineopen72\bin64\hexstreamdpx86_64.exe "<project_
path>\computation_1\computation_1.run" -steering "<project_path>\computation_
1\computation_1.steering"
The command line, to start the FINE™/Open solver, contains its name (hexstreamdp is the
double precision version of the FINE™/Open solver), the full path name of the ".run" and the
corresponding ".steering" files to launch.
Mixed and double precision versions of the FINE™/Open solver are available.
2. Set Permission for Execution of "*.bat" file
3. Create an input file (".run") for each computation. To create these files through the
FINE™/Open GUI, click on the Project/Save Selected 'Run' Files menu in order to save the
".run" file of the activated computation, after opening the corresponding project.
4. Launch the script ".bat" by typing the script file name: "*.bat" in a DOS-shell or double click
on the ".bat" file from the Windows Explorer.
Clicking on the menu Solver/Save batch file, a script "computation_name.bat" can be created in
the corresponding computation subfolder. This script enables the user
to launch the same
computation in batch.
13.4.3 Launch the FINE™/Open Solver in Parallel Using
Scripts
Do not forget to partition the mesh first in FINE™/Open Launching Mode page. The number of
partition should be strictly equal to the desired number of processes.
How to Launch the flow solver in Parallel using MPI on Linux
1. Create a script file "batch.sh" with permission for execution. An example of a "batch.sh" file
for a parallel computation on Linux:
#! /bin/csh
hexstreamdp_parallel -mca=btl=openib,sm,self "<project_path>/computation_
1/computation_1.run" -steering "<project_path>/computation_1/computation_
1.steering" -niversion "open72" -p4pg "<project_path>/computation_1/computation_
1.p4pg" -fullflex
The script is started in a C-shell due to the line: "#! /bin/csh". The command line, to start the
flow solver in parallel, contains the script name that enables parallel computation,
the
OpenMPI options that configures the used OpenMPI library or runs the runtime tools, the full
path name of the ".run" and the corresponding ".steering" files to launch, the FINE™/Open
with OpenLabs™ release version and the full path name of the file "computation.p4pg" file
containing the definition of the machines that will be used to launch the computation in
parallel. The argument -fullflex is optional, which forces the flow solver to use the FFLEX-
type license keys in priority (For more details, see Flexible Cores Type from License).
Mixed and double precision versions of the FINE™/Open solver are available.
The OpenMPI options can be used to configure OpenMPI. In general, all the MCA options
can be imposed in the script.
Please note, when the OpenMPI options are following the NUMECA executable, the
spaces in the original MCA parameters MUST be replaced by "=".
If OpenMPI is built with the support of CPU affinity, it is possible to configure this feature
through the script by adding the option -rf=<rankfile>, with a rankfile written like described in
http://www.open-mpi.org/faq/?category=tuning#using-paffinity.
The OpenMPI options can also be used to call the runtime tools that permit to scan the host
machine, get runtime information, etc. For example, the following options can be added in the
command line to obtain the corresponding information:
-param=btl=openib to run ompi_info --param btl openib;
-param=btl=all to run ompi_info --param btl all;
-param=mpi=all to run ompi_info --param mpi all;
-param=all=all to run ompi_info --param all all;
etc.
All these runtime information is written in a hidden file located in the working directory, with
the extension .rtm.
2. Create Hosts Definition File "computation.p4pg". A file needs to be created to define the hosts
(e.g. hosts.p4pg). This file specifies the machine information of the various processes and is
automatically created when starting the computation in parallel within the Task Manager. An
example of a "hosts.p4pg" file:
Example 1:
Hostname1 4 hexstreamdpopen211_1
Hostname2 2 hexstreamdpopen211_1
where master host on Hostname1 and 5 process on Hostname1; 2 processes on Hostname2.
Example 2:
Hostname1 0 hexstreamdpopen211_1
Hostname2 2 hexstreamdpopen211_1
where master host on Hostname1 and 1 process on Hostname1; 2 processes on Hostname2.
For each machine, a line must be added containing the machine name (the machine hostname),
the number of processes to run on the machine,
the name of the executable and the
FINE™/Open with OpenLabs™ release version (i.e. open211_1):
hostname 4 hexstreamdp<version>
If additional machines are to be used, subsequent lines are required for each machine. For the
first machine, a process is automatically launched. Therefore, the number specified in the
"hosts.p4pg" file should be equal to the number of processes required on this machine, minus
one.
The first machine (hostname) specified in the file "hosts.p4pg" should be the one from which the
script will be launched.
The total number of processes defined in the file "hosts.p4pg" should be equal to the number of
partitions minus one (since one process is launched automatically on the Hostname specified on
the first line of the file).
The Hostname specified on the first line will be used for solution reconstruction.
3. Set permission for execution "batch.sh" by using the command: "chmod 755 batch.sh"
Create input files ".run" to launch the computation. The parallel settings of the computational
file (".run" and ".steering") are managed by the Task Manager. Therefore before launching the
parallel computation script, the following steps must be performed through the FINE™/Open
GUI:
4. Create computational file (".run") by activating the corresponding computation and clicking on
the Project/Save Selected 'Run' Files menu in the interface.
5. To set the final parallel settings:
l create a task in the Task Manager,
l define the parallel settings of HEXSTREAM subtask (parallel computation),
l save the task through the Task manager by clicking on Save button.
These operations are mandatory in order to have all the parallel settings correctly imposed in
the computation file (".run").
6. Launch the script "batch.sh" by typing the script file name: "./batch.sh".
When saving the ".run" file of the computation (Project/Save Selected 'Run' Files) and clicking
the Save button as explained in step 5 through the Task Manager (Modules/Task Manager), a new
script ".batch" and a file ".p4pg" are created in the corresponding computation subfolder that enable
the user to launch the same parallel computation in batch.
How to Launch the flow solver in Parallel using MPI on Windows
1. Create a script file "batch.bat" with permission for execution. An example of a "batch.bat" file
for a parallel computation on Windows:
<NUMECA_install_dir>\fineopen72\bin64\mpiexec.exe -n "#" -machinefile "<project_
path>\computation\computation.p4pg" "<NUMECA_install_
dir>\fineopen72\bin64\hexstreamdpx86_64.exe" "<project_
path>\computation\computation.run" -steering "<project_
path>\computation\computation.steering" -fullflex
The command line, to start the flow solver in parallel, contains the full path to the script that
enables parallel computations (mpiexec.exe), the number of the processors, the full path of the
p4pg file containing the definition of the machines that will be used to launch the computation
in parallel, the full path to the flow solver (hexstreamdpx86_64.exe) and the corresponding
".steering" files to launch. The argument -fullflex is optional, which forces the flow solver to
use the FFLEX-type license keys in priority (For more details, see Flexible Cores Type from
License).
Mixed and double precision versions of the FINE™/Open solver are available.
2. Create Hosts Definition File "computation.p4pg". A file needs to be created to define the hosts
(e.g. hosts.p4pg). This file specifies the machine information of the various processes and is
automatically created when starting the computation in parallel within the Task Manager. An
example of a "hosts.p4pg" file:
hostname1:4
hostname2:2
where master host on hostname1 and 5 processes (including the master host) on hostname1; 2
processes on hostname2.
For each machine, a line must be added consisting of the machine name (the machine
hostname) and the number of processes to run on the machine. If the number of processors is
set to 0 for the first machine (first line of the ".p4pg" file), only the master host process will run
on that machine while the nodes will run on the next machines declared in the following lines.
The first machine (hostname) specified in the file "hosts.p4pg" should be the one from which the
script will be launched.
The total number of processes defined in the file "hosts.p4pg" should be equal to the number of
partitions minus one (since one process is launched automatically on the Hostname specified on
the first line of the file).
The Hostname specified on the first line will be used for solution reconstruction.
3. Set permission for execution "batch.bat"
Create input files ".run" to launch the computation. The parallel settings of the computational
file (".run" and ".steering") are managed by the Task Manager. Therefore before launching the
parallel computation script, the following steps must be performed through the FINE™/Open
GUI:
4. Create computational file (".run") by activating the corresponding computation and clicking on
the Project/Save Selected 'Run' Files menu in the interface.
5. To set the final parallel settings:
l create a task in the Task Manager,
l define the parallel settings of HEXSTREAM subtask (parallel computation),
l save the task through the Task manager by clicking on Save button.
These operations are mandatory in order to have all the parallel settings correctly imposed in
the computation file (".run").
6. Launch the script "batch.bat" by typing the script file name: "batch.bat" in a DOS-shell.
When saving the ".run" file of the computation (Project/Save Selected 'Run' Files) and clicking
the Save button as explained in step 5 through the Task Manager (Modules/Task Manager), a new
script ".batch" and a file ".p4pg" are created in the corresponding computation subfolder that enable
the user to launch the same parallel computation in batch.
How to Launch the flow solver in Parallel using SGE on Linux
1. Create a script file "batch.sge" with permission for execution. An example of a "batch.sge" file
for a parallel computation on Linux:
#!/bin/sh
# request Bourne shell as shell for job
#$ -S /bin/sh
#$ -notify
# Specify a MPI job on 4 processors
#$ -pe mvapich 4
#$ -N ahmed
# standard output redirection
# -j y standard error redirected in the same file as the standart output
#$ -o /tmp/ahmed/ahmed_computation_1/ahmed_computation_1.std -j y
NI_VERSIONS_DIR=/home/fineopen72
export NI_VERSIONS_DIR
NUMECA_SOFT_VERSION=open72
export NUMECA_SOFT_VERSION
TMP_DIR=~/.numeca/tmp/
NUMECA_DIR=${NI_VERSIONS_DIR}/fine$NUMECA_SOFT_VERSION
export NUMECA_DIR
NUMECA_BIN=${NUMECA_DIR}/LINUX
export NUMECA_BIN
MPIR_HOME=${NUMECA_BIN}/_mpi/_ompi1.6/
export MPIR_HOME
OPAL_PREFIX=$MPIR_HOME
export OPAL_PREFIX
PATH=${MPIR_HOME}/bin:${PATH}
export PATH
LD_LIBRARY_PATH=$MPIR_HOME/lib64:$MPIR_HOME/lib:${NUMECA_BIN}/ _
lib_sx86_64gcc4.4:${NUMECA_BIN}/_lib_sx86_64:${LD_LIBRARY_PATH}
export LD_LIBRARY_PATH
ompi_options=
RUN_FILE=/tmp/ahmed/ahmed_computation_1/ahmed_computation_1.run
PREC=hp
BIN=${NUMECA_BIN}/hexa/hexstream${PREC}x86_64_ompi
ompi_info
$MPIR_HOME/bin/mpirun --display-map --display-allocation ${ompi_options} -np
$NSLOTS -hostfile $TMPDIR/machines ${BIN} $RUN_FILE -fullflex
where:
#$ -S /bin/sh requires Bourne shell to be used by SGE for job submission and hence, only the
".profile" file of the user is executed if exists on each computation host. There is nothing
specific to NUMECA software that must be written in the ".profile" file.
#$ -notify gives a delay between the send of the SIGKILL signal and SIGUSR2 signal. The
delay is defined in the SGE interface.
#$ -pe mvapich 4 requests 4 slots (processors) to the SGE system for executing the job using
the mvapich parallel environment. This must correspond to the number of computation
processes (partitions).
#$ -N ahmed is the name of the job given to SGE and that will be seen when monitoring the
job with the graphical monitoring utility qmon (Job Control button) or with the qstat SGE
command. SGE has a limitation of 8 characters for the job name.
#$ -o /tmp/ahmed/ahmed_computation_1/ahmed_computation_1.std -j y tells SGE system
that the standard output has to be redirected in the ".std" in the computation directory, the
option "-j y" indicates that the standard error is redirected into the same file.
NI_VERSIONS_DIR=/home/fineopen72
export NI_VERSIONS_DIR
NUMECA_SOFT_VERSION=open72
export NUMECA_SOFT_VERSION
specifies the installation directory and version of FINE™/Open with OpenLabs™.
MPIR_HOME=${NUMECA_BIN}/_mpi/_ompi1.6/
export MPIR_HOME
OPAL_PREFIX=$MPIR_HOME
export OPAL_PREFIX
PATH=${MPIR_HOME}/bin:${PATH}
export PATH
LD_LIBRARY_PATH=$MPIR_HOME/lib64:$MPIR_HOME/lib:${NUMECA_BIN}/ _
lib_sx86_64:${LD_LIBRARY_PATH}
export LD_LIBRARY_PATH
are the environment variables indicating respectively the OpenMPI directory (FINE™/Open
with OpenLabs™ allows to use an external OpenMPI library, which may be a tuned,
customized or hardware specific OpenMPI libraries.) and the library directories that are used in
the command launching the flow solver.
ompi_options= specifies the OpenMPI options. If nothing is specified, OpenMPI will choose
the most efficient interconnect supported by the pointed library (OPAL_PREFIX)
ompi_info is a OpenMPI tool, which is used to call the runtime tools that permit to scan the
host machine, get runtime information, etc. For example, the following options can be added in
the script to obtain the corresponding information: ompi_info --param all all.
Independently of OpenMPI, the following commands can be used in the sge script:
ldd - v $NUMECA_ BIN/hexa/hexstreamhpx86_ 64_ ompi
environment is loaded before launching the flow solver.
to check which runtime
/lib64/libc.so.* or /lib/libc.so.* to get the version of the libc.
etc.
All these runtime information is written in a hidden file located in the working directory, with
the extension .rtm. Once a parallel computation using OpenMPI is launched, each process is
hosted on a node and the rank of each process is contained in the environment variable OMPI_
COMM_ WORLD_ RANK. As a consequence, each process can also check the loaded
runtime environment and the libs of the host, and write the information in a hidden file located
in the working directory, with the extension .rtm$OMPI_COMM_WORLD_RANK.
$MPIR_HOME/bin/mpirun --display-map --display-allocation ${ompi_options} -np
$NSLOTS -hostfile $TMPDIR/machines ${BIN} $RUN_FILE -fullflex
is the command to launch the parallel computation. --display-map --display-allocation is the
OpenMPI options that are used to display the process map before launching the job and the
allocation being used by this job. $NSLOTS is the number of slots (processors) that have been
allocated by SGE for the job. $TMPDIR is generated by SGE for providing the machines file
used by the mpirun script. ${BIN} is the defined mixed precision solver compiled with the
OpenMPI library. $RUN_FILE is the argument to the flow solver. The argument -fullflex is
optional, which forces the flow solver to use the FFLEX-type license keys in priority (For
more details, see Flexible Cores Type from License).
For sequential runs, the line "#$ -pe mvapich 4" must be removed and the final command must
be: ${BIN} $RUN_FILE
2. Set permission for execution "batch.sge" by using the command: "chmod 755 batch.sge"
Create input files ".run" to launch the computation. The parallel settings of the computational
file (".run") are managed by the Task Manager. Therefore before launching the parallel
computation script, the following steps must be performed through the FINE™/Open GUI:
3. Create computational file (".run") by activating the corresponding computation and clicking on
the Project/Save Selected 'Run' Files menu in the interface.
4. To set the final parallel settings:
l create a task in the Task Manager,
l define the parallel settings of HEXSTREAM subtask (parallel computation),
l save the task through the Task manager by clicking on Save button.
These operations are mandatory in order to have all the parallel settings correctly imposed in
the computation file (".run").
5. Launch the script "batch.sge" by typing the script file name: "./batch.sge".
When saving the ".run" file of the computation (Project/Save Selected 'Run' Files) and clicking
the Save button as explained in step 4 through the Task Manager (Modules/Task Manager), a new
script ".sge" is created in the corresponding computation subfolder that enables the user to launch the
same computation in batch and in parallel.
13.4.4 Launch CFView™ Using Scripts
How to Launch CFView™ on Linux
1. Create a macro file ".py". See the CFView™ user manual for more details on the format of a
macro file and the commands that it can contain.
2. Launch the macro ".py" by typing:
cfview -macro <py_path>/test.py -batch -niversion <version>
The command line to start CFView™ contains its name, the full path name of the macro ".py" file
to launch, and the CFView™ release that will be used (i.e. open211_1). The "-batch" option
disables the display of the CFView™ graphical user interface.
How to Launch CFView™ on Windows
1. Create a macro file ".py". See the CFView™ user manual for more details on the format of a
macro file and the commands that it can contain.
2. Launch the macro ".py" by typing:
<cfview_path>\cfviewx86_64.exe -macro <py_path>\test.py -batch
The command line to start CFView™ contains its full path name and the full path name of the
macro ".py" file to launch. The "-batch" option disables the display of the CFView™ graphical
user interface.
Command Line Arguments
The command cfview may be followed by a set of command line arguments. These command line
arguments allow the user to override some system defaults (driver used, display, double-buffering
and update abort options) or to specify files to be loaded immediately (project, macro, defaults
settings, macro module). The supported command line arguments are:
-help prints a summary of the command line arguments,
-version prints the CFView™ version number,
-date prints the CFView™ version date,
-defaults <file name> starts CFView™ with the default settings from the specified file,
-project <file name> starts CFView™ and immediately opens the specified project,
-macro <file name> starts CFView™ and execute the specified macro script,
-macromodule <file name> starts CFView™ and load the specified macro module,
-display <display name> starts CFView™ on the specified display device,
-doublebuffering on (off) enables (disables) double buffering,
-updateabort on (off) enables (disable) update aborting ,
-driver <driver name> starts CFView™ with the specified graphics accelerator,
-reversevideo on (off) starts CFView™ with black (white) background color ,
- facedisplacement <n> starts CFView™ with the specified face displacement ,
-loaddata all (none, ask) when opening a project the quantities fields are loaded in the computer
memory (are not loaded, a specific dialog box is raised where the user choose the field variables
to be loaded). The defaults is to load all field quantities. ,
-batch on (off) starts CFView™ without graphical user interface. This mode can be used in
combination with the -macro command line option in order to perform the execution of a macro
script without user interaction,
-hoops_relinquish_memory off this option disables the hoops garbage collection feature that is
activated when CFView™ is idle for a long period of time.
13.5
LIMITATIONS
The task manager have some limitations due to the current PVM and MPI libraries:
l Linux to Windows connections are not allowed.
l The remote copy works only if there is enough disk space on the remote machine. Currently,
no check is performed to identify the available disk space and the flow solver crashes with
"undefined reason".
l The remote copy option is not available in batch mode. Therefore, all processes must have
access to the same disk system (e.g. NFS) when running in batch.
l When a user launches FINE™/Open with OpenLabs™ on different machines, the connection
between these machines is not allowed as described in What PVM Daemons Do section.
CHAPTER 14.
MONITORING & LAUNCHING MODE
This chapter
is dedicated to monitoring and launching mode parameters in FINE™/Open with
OpenLabs™. The Steering (
control/Control
Manager/Convergence History are described.
) and Monitor (
Variables , Computation
) tools as well as the pages Computation
Task
control/Launching Mode
and
l The Computation control/Control Variables page is described in the Control Variable section.
l The launching mode (sequential or parallel) is explained in the Launching Mode section.
l The built- in Steering tool (
) and the Task Manager/Convergence History page of
FINE™/Open with OpenLabs™ are described in the Steering section.
l The Monitor external tool (
) is described in the Monitor section.
l In the Best Practice for Computation Monitoring section, advice is provided on how to use the
monitoring tools for analysing the progress of a computation.
In this section
14.1 Control Variables
14.2 Launching Mode
14.3 Steering
14.4 Monitor
14.5 Best Practice for Computation Monitoring
397
400
404
411
414
14.1 CONTROL VARIABLES
The General tab of Computation Control/Control Variables page allows the user to define
some global parameters for the selected computation.
For steady computations:
l the maximum Number of iterations on the finest grid level (i.e. not including the iterations
performed during coarse grid initialization), or, when adaptive computations are performed, the
maximum number of iterations on the final "adapted" grid.
l the Convergence criteria corresponding to the (negative) number of orders of magnitude the
norm of the residuals must decrease before stopping the calculation. If this criteria is not
reached the calculation proceeds until the maximum number of iterations has been performed.
l the frequency for saving output: every x iterations the solver saves the flow solution and
creates the output files to be read in CFView™ (where "x" is the number of iterations defined
in the FINE™/Open GUI).
FIGURE 14.1
General tab of the Control Variables page, steady case
For unsteady computations,
initialization and Output files, see Control Variables section for more details.
the user needs to set
the parameters for Time step , Steady
FIGURE 14.2
General tab of the Control Variables page, unsteady case
When restarting a computation, the user needs to increase the Number of iterations (steady) or
Number of time steps (unsteady) in the Computation control
/ Control variables page,
otherwise the computation will not continue because the imposed number through the interface is an
absolute number of iteration linked to the computation.
In the Advanced tab of this page, a list of non-interfaced expert parameters is displayed. In
FINE™/Open, the expert parameters are separated into two categories: Global parameters which
are applied to all blocks in the project and Local parameters which are block-dependent. The user
can choose Global parameters or Local parameters in the option Select category. In case of
Local parameters, a list of the blocks in the project will be shown in the left of the window. The
user can select a block and set the corresponding block-dependent expert parameters, as shown in
FIGURE 14.4.
FIGURE 14.3
Advanced tab of the Control Variables page - Global parameters
FIGURE 14.4
Advanced tab of the Control Variables page - Local parameters
Only the expert parameters that are described in the manual are supported. Use of the other
parameters is not recommended. For a summary of all supported expert parameters, see the List of
Advanced Parameters section.
14.2
LAUNCHING MODE
The Computation Control/Launching Mode page allows the user to define if the computation
will be launched in sequential or in parallel.
The computations using HEXPRESS™/Hybrid in sph format or TGrid mesh must be
launched in parallel mode.
launching a computation,
After
the FINE™/Open solver will automatically allocate memory
depending on the computation. Please note, there is a limitation coming from the operating system on
the amount of memory that can be used. In case of large computations, it is suggested to run the
computation in parallel mode.
FIGURE 14.5
Launching Mode page
The Launching Mode page allows the user to select between Serial (sequential mode) or
Parallel. By default the computation will be launched in sequential mode.
When activating the Parallel option, the user should define the parameters for the load balancing.
With Allow multiple domains per process
activated, it is possible to group and handle more
than one block in one single process. This is useful in case there are multiple small blocks in the
project.
When multiple blocks are treated by one process, these blocks must not be partitioned.
After the user specifies the Total number of processes to be used, the load balancing between
blocks will be automatically computed.
FIGURE 14.6
Parallel Settings
After setting the Total number of processes, the user can still modify the Number of partitions
and Weight(%) (if the option Weighted is active) for each block/group. In this case, the Total
number of processes will be automatically updated.
The button Default balancing allows to re-set the weight using the default value.
After selecting the number of partitions and their respective weight, FINE™/Open with
OpenLabs™ allows the user to visualize the cells composing a selected partition by left-clicking
on the "eye" button ( ).
FIGURE 14.7
Visualize the cells composing a selected partition
For parallel computations, FINE™/Open provides two partitioners:
l Serial partitioner (default): guaranties the same convergence history whatever the number of
processors is. It is slow and limited by the maximum memory that can be allocated on a
processor.
l Parallel partitioner: can be activated by settings the expert parameter PartitionerParallel_=1.
It is fully parallelized and thus faster and without memory restriction.
One disadvantage of the parallel partitioner is that the convergence history of the computation
depends on the number of processes, because there is no communication between the
processes when performing agglomeration. In order to overcome the disadvantage, a new
agglomeration method is introduced, which can be activated by settings the expert parameter
newParallelAgglomeration_ =1. This new agglomeration method allows to get the same
convergence history whatever the number of processors is. However, this new agglomeration
method needs more CPU time because of the communication between the processes.
In case of a structured grid, the expert parameter newParallelAgglomeration_ is automatically
set to 0.
For parallel computations with ".hex" mesh (HEXPRESS™ format), by default, the mesh will be
partitioned in serial (by only one processor). If the user wants to partition the ".hex" mesh in
parallel, the user must set the expert parameter PartitionerParallel_ to 1 to activate the parallel
partitioner.
For parallel computations with ".sph" mesh (HEXPRESS™/Hybrid format) or ".msh" mesh
(TGrid format), the mesh will be automatically partitioned in parallel.
When option Allow multiple domains per process checked,
automatically activated.
the parallel partitioner
is
14.3 STEERING
The Steering button (
) on the main icon bar or Task Manager/Convergence History allow
the user to load the Convergence History page. It is possible here to define quantities to be
followed during the convergence process of the FINE™/Open solver. This pages is divided into 5
areas as shown in FIGURE 14.8:
1. The steering files selection (Select Computations) and the curves export (Export Curves To
File...) only available in Task Manager/Convergence History page.
2. The available variables (Available Variables).
3. The parameters (Parameters type).
4. The selected variables (Selected Variables).
5. The graphics view (Convergence History).
When the FINE™/Open solver is invoked, communication is automatically established within
FINE™/Open with OpenLabs™ allowing the user
to follow selected quantities. Two
representations of the quantities are currently available: the convergence curves displayed in area
4 and the quantity value at the last iteration in area 3. All these data are stored in files with
extension ".steering" and ".steering.binay". These files are created and managed automatically by
FINE™/Open with OpenLabs™
If the communication between the FINE™/Open solver and the FINE™/Open GUI is interrupted (e.g.
a network problem), parts of the convergence curves can be lost.
Steering data cannot be outputted in batch mode.
FIGURE 14.8
The five areas of the Convergence History page
14.3.1 Steering Files Selection and Curves Export
FIGURE 14.9
Steering files selection area
Different mode exists for the selection of the current steering results stored in the steering files:
1. When a project is opened, the active computation steering file is automatically selected and
appears in the Add or select computations window when clicking on Select Computations
button (a). Each time a new computation is selected,
the associated steering file is
automatically loaded and becomes the active one.
2. All the steering files already loaded can be selected by <Ctrl>-leftclick and <Shift>-leftclick in
the list of available computations.
3. The file can also be loaded manually using the button Add Computation (c). A file chooser
prompts the user to select the file.
4. The button Remove Computation allows the user to remove from the memory the selected
computation (the file is not removed and remains available for selection).
5. Additionally, when a task is started, the steering files of the flow solver computation called in
the task are automatically loaded and become available through the list (b).
The Export Curves To File... button enables the user to save in an ASCII file ".cvh" all the curves
plotted in the Graphics View.
14.3.2 Available Quantities Selection
By default, the global residual, the inlet and outlet mass flow, the efficiency, the pressure ratio, the
axial thrust and the torque are computed during the convergence process. During the convergence
process, the Available Variables list (b) allows the user to select and the Add for Selection
button allows the user to add new quantities to the computed list.
FIGURE 14.10
Available Variables selection area
All quantities can be added before or during the computation.
When a quantity has been added, it appears in the selection list and becomes the selected quantity.
If the flow solver is running, the value and the convergence curve of the new quantity is displayed
after a few seconds. The convergence curve begins at the iteration corresponding to the moment
when the new quantity was added.
When a quantity is added for selection it appears in the selection list with a number after the name.
This number is only added to avoid that the same variable name appears twice in the list. This is
necessary when, for example, the static pressure is monitored at two different points in the
domain.
14.3.3 New Quantity Parameters Definition
When a new quantity has been added, it becomes available for selection in the Selected
Variables list (area 4 in FIGURE 14.8). The user can select the way the flow solver computes the
quantity through the parameter type area (area 3 in FIGURE 14.8). Several types of parameters
can be chosen using the parameter type list box (FIGURE 14.11).
A description of the available types of parameters that can be defined to computed the selected
quantities is given below:
1. global: the computed variable is averaged over all the domain.
2. control point: the user specify the control point ID. Control points are defined in the
Computation control/Outputs page, or in a ".ctl" file, see Advanced section for more details.
FIGURE 14.11
Parameter type definition
Care should be taken when using the steering of a parameter on a control point. It should be carried
out in the following way:
l select the parameter (relative velocity u, static pressure etc.) and Add for Selection. It becomes
available in the Selected Variables list.
l select the new variable in the list and set the ID of the control point on which the evolution of the
selected parameter will be visualized.
All the user modifications can also be done (and changed) during the computation run.
14.3.4 Quantity Selection Area
When a quantity has been added, it becomes available for selection in the Selected Variables list.
The list is divided into 3 columns as shown in FIGURE 14.12: the variable name (a) which can
be changed using the Rename button (c), the quantity value and the units (b) which respectively
displays the last computed value and the units. The Remove button (d) is used to remove the
selected variable.
FIGURE 14.12
Selected Variables area
When a quantity has not yet been computed, the value is indicated as undefined.
Selecting a quantity will show its history in the graphics view as described in the next paragraph.
To select multiple quantities click on them (with the left mouse button) in the list while holding
the <Ctrl> key. To select quantities that are next to each other in the list simply left-click on the
first one and keep the mouse button pressed while moving to the last variable.
14.3.5 Definition of Global Residual
The residuals are computed by the FINE™/Open solver as a flux balance (the sum of the fluxes
on all the faces of each cell):
The root mean square of the residuals is computed using the following formula:
.
and the maximum of the residuals in the same way:
,
,
with log the logarithm to the base ten.
the first
On the Convergence History page the global root mean square of the residuals normalized by its
value at
iteration is shown. These values are stored in the file with extension
".steering.binary". Additionally the global residuals are shown in numerical values in the Task
Manager window. The RMS ("avRes") value listed in the Task Manager window is the global
root mean square normalized by its value at the first iteration. The maximum ("maxRes") value is
the maximum residual normalized by the RMS residual at the first iteration.
The equation associated to the displayed residuals is specified through the expert parameter out_
toDisplay_ located in the Advanced tab of the Computation control/Control Variables page. By
default, the mass equation is used.
If the initial solution is already quite close to the final solution, the obtained residual values are not as
low as they would have been when the initial solution is far from the final solution. The obtained
residuals values depend on the difference of the used initial solution with the final solution.
14.3.6 The Graphics View
FIGURE 14.13
Graphics view area
The convergence history of the selected curves are displayed inside the graphics view as shown in
FIGURE 14.13 . The color of the curves is different for each curve (up to 8 curves can be
selected). Colours used for the displayed value are automatically selected (a). Additionally, the
error between the two first selected quantities is also indicated (b). This is useful for checking the
difference between the mass flow at inlet and outlet.
In the Task Manager/Convergence History page, the color of the curves is the same (but with
different markers) if related to the same computation and is different for each curves if related to
different computations (up to 10 selected quantities).
14.4 MONITOR
14.4.1
Introduction
The Monitor can be launched is an external tool, and can be launched from FINE™/Open with
OpenLabs™ by clicking on the Start Monitor button (
) on the main icon bar.
FIGURE 14.14
The Monitor window
The monitor is generally used to facilitate batch mode control, but also contains additional
visualization features.
l the convergence history per equation and per block (domain) of one or several computations
(RMS and maximum residuals) can be displayed,
l the evolution of global quantities, such as lift, drag and moment for external flow, and mass
flow, axial thrust, torque, efficiency and pressure ratio for internal and turbomachinery flows,
FINE™/Open with OpenLabs™ allows multi- process analyses. Therefore, the convergence
histories of multiple (running) projects can be visualized at the same time. It is also possible to
compare the convergence history associated with different computational parameters for the same
project.
The monitored variables are displayed as a x-y graph in the upper part of the window. The x-axis
represents the number of multigrid cycles computed by the flow solver. The y- axis is a
logarithmic axis representing the power of ten of the residual values. The user can choose to
display the residual of any of the equations solved, as well as a number of global parameters,
using the buttons located in the lower part of the graphic control window, as shown in FIGURE
14.14.
The lower part of the graphic control window contains four boxes.
The small box located on the left side contains a Print button (which allows to save the current
graph as a postscript file) and a Quit button. Three radio buttons are also located in this area. Only
the Convergence history button (selected by default) is relevant.
The three other boxes are described in the next sections.
14.4.2 The Residual File Box
Three buttons are provided in this box to Add, Remove or Activate residual files through a file
chooser. The residual files describe the iteration process of previous or current computations.
They contain the history of the axial thrust, mass flow, torque, pressure ratio (if internal or
turbomachinery flows), lift, drag (if external flow) and the residuals of five (six or seven if
respectively the 1-equation or 2-equation turbulence models are used) physical variables.
The activation of one or more of the residual files has the effect of deactivating the other loaded
residual files. When a file is deactivated, its associated convergence history is not displayed. The
selective activation of the files allows the user to display only the convergence histories of
required files.
When opening the graphic control window, the residual files associated with the running applications
is automatically active.
The input boxes File and Block, visible just below the three buttons Add, Remove and Activate,
allow the user to select which file and block the choice of the monitored variables, selected in the
Quantities to display, menu should be applied.
14.4.3 Quantities to Display
Residuals
Buttons are provided to select the type of residuals: rms or maximum as shown in FIGURE
14.14. Residuals relative to all transport equations of the problem are available: these are the
continuity, the momentum, the energy, and possibly the Spalart-Allmaras or the k and ε equations.
While the Convergence History page displays only the RMS global residual for one equation,
the monitor gives the RMS and maximum residuals for each equation. Residuals are given per
block. Computation of the RMS RES and MAX RES values is performed.The values shown in the
monitor for the RMS are normalized by the value of RMS RES at the first iteration: RMS RES-
(RMS RES)it=1. The values shown for the maximum residuals are normalized by the maximum
residual at the first iteration: MAXRES-(MAXRES)it=1.
Since the RMS and maximum residuals are normalized differently it may occur that the RMS value
shown is higher than the maximum residual.
Global Quantities
Several buttons are provided to visualize the additional global quantities available in
FINE™/Open with OpenLabs™:
l Internal or turbomachinery flow problems (select Internal flow or Turbomachinery in the
Computation control/Outputs page): The axial thrust, the (inlet and outlet) mass flows, torque,
pressure ratio, and efficiency.
l External flow problems (select External flow in the Computation control/Outputs page): The
drag, the lift and the moment. The user must specify the axis that is to be used for these global
quantities, as described in the External Flow section.
If several computations are performed at the same time, the curves associated with the different
projects are drawn in different colors. The buttons of the present box act only on the curves of the
file and block selected through the File and Block menu.
14.4.4 Display Options
The Legend button is used to display which files are currently activated. In addition, if the mass
flow button is activated, the relative errors between the inlet and the outlet are indicated.
The Work Unit button is provided to set the type of unit used on the horizontal axis for the
monitor window: multigrid cycles or work units. Ifthe Work Unit button is unchecked the abscissa
will show the number of iterations. The Work Unit option is currently not supported by
FINE™/Open with OpenLabs™ outputs.
The Update now button updates the graph for the active residual file and the selected block.
The Auto update button can be checked on to follow the iteration processes automatically. It is
however a rather time-consuming option and this button is not active by default.
14.4.5 Zooming Option
This option allows the user to interactively zoom in and out:
1. In the drawing window, press the left mouse button to initiate a zooming operation,
2. Drag the mouse to the left or to the right to zoom in, the zooming window number is displayed
on the screen,
3. Click again on the left button when finished,
4. To zoom out (the previous zoom level), click on the right button of the mouse.
14.5 BEST PRACTICE FOR COMPUTATION
MONITORING
Introduction
Several tools are available in the FINE™/Open with OpenLabs™ package to follow the
evolution of a calculation:
l the Convergence History page available in FINE™/Open with OpenLabs™ by pressing the
Steering button (
evolution of a calculation.
) on the main icon bar, which allows the user to easily follow the
l The monitor (
) can be used to compare the evolution of multiple computations and of the
RMS or maximum residuals associated with all equations.
l CFView™ to enter even into more detail.
Each option has its own specific features, but they are complementary. This section describes how
to use those tools to monitor a computation. For a detailed description of the use of CFView™
see the CFView™ user manual.
When a computation has been launched for the first time, and the initialization steps have been
properly passed, the solver writes a first solution file. In fact, it is not yet a solution but only the
result of the initialization. This first output is useful to check if all boundaries conditions have
been set correctly. It is recommended that the user check the velocity profiles at inlet, outlet and
external boundaries. This operation aims to detect a user mistake, which could cause a loss of
time, due to, for example, a forgotten patch. To check this first output use CFView™. Using the
Representation menu the velocity can be displayed on the selected patches.
Convergence History
The global residual on the Convergence History page allows the user to quickly see whether the
computation is running properly. The residuals should initially decrease on the coarser grid levels
of the Full Multigrid strategy as shown in FIGURE 14.15. See Numerical Model chapter for
more detail on Full Multigrid. When moving to a finer grid level the global residual suddenly
increases and then immediately begins to decrease again. When the computation reaches the finest
grid, the curve of the global residual normally should decrease gradually. In general a fall of 3
orders with a stabilization of this curve is considered as a good convergence. But it is important to
check if other global quantities such as lift and drag are also stabilized.
FIGURE 14.15
Example of convergence history for global residuals
Monitor
The monitor follows the same quantities as the Convergence History, but its main advantage is
to allow the user to follow the convergence for each equation and for each block, and to compare
multiple computations.
Control points
During the steering, it is possible to get a deeper control, locally, by adding control points
(Computation control/Outputs page). These points allow the user to track behavior of the
speed, the pressure and turbulent quantities in important parts of the domain. The user may also
require convergence or time histories at specific points in the flow, for example at a experimental
measurement location, which can be accomplished using control points. In the case of steady
computations, the values associated to these points should converge to a constant value.
CFView™
One additional advice is to use CFView™ during the computation with intermediate and non-
converged solutions. When having convergence problems for example CFView™ may be used
to look for the zones were the residuals are too high values compared to other regions or at an
incorrect turbulence field. The cells where the residuals are the highest are displayed at each
iteration in the taskmanager window, and can be found in CFView™ by opening the Cells box in
the Geometry menu. Combining this information and using CFView™ may help the user find
the cause of convergence problems in the computations.
TaskManager information
After a computation (or a subtask) is terminated, the TaskMakager INFO window will appear,
which displays the summary of the computation and its status. In case that the computation
crashes, the user can quickly check the .std file by clicking the button View computation std file
(s). The std file contains a summary of the computation as well as warnings and/ or error
messages.
After clicking the button View computation std file(s), a new window computation std file(s)
the name of the
appears. The tab contains the name of the computation. At the bottom,
computation corresponding to the active tab is displayed. When moving the cursor to this area, the
full path and name of the <std> file is shown in a balloon help.
In case that several computation status are shown in the TaskManager INFO window, the
associated std files will be displayed in separate tabs. If a computation is run several times
successively, the status are appended in the TaskManager INFO window. In this case, only one
std file will be displayed because only one std file exists in the computation folder.
CHAPTER 15.
PYTHON SCRIPT
FINE™/Open provides a new powerful scripting tool that enables the user to automate project settings
for applications. More details on the python commands are available in the files "FHX.py" provided in
the NUMECA distribution after installation (i.e. under Windows, the file is available in "~/_python/_
fine/_hexa/").
All actions for which a python command exists will be automatically recorded in FINE™/Open. The
menu Project/Script/Edit... can be used to edit the current record of the commands. The menu
Project/Script/Save All... can be used to save the current record of the commands.
Script files can be run from the graphical user interface or from the command line.
l From the interface, the option is accessed with the Project/Script/Execute... menu. It opens a file
is executed by
chooser prompting to select a ".py" script file. After acceptation,
FINE™/Open.
the script
l From the command line, a script can be run by launching FINE™/Open with the -script option. For
example:
fine -niversion <version> -script my_script.py
FINE™/Open will execute the script and then open the graphical user interface.
When running a script from the command line, it is possible to execute a process in batch mode,
avoiding to open the GUI. To do so, the -batch option should be specified:
fine -niversion <version> -script my_script.py -batch.
In this section
15.1 Python Language Overview
15.2 FINE™/Open with OpenLabs™ Script Commands
419
424
15.1
PYTHON LANGUAGE OVERVIEW
Scripts are available in FINE™/Open through the object-oriented Python language. Python is a
popular scripting language designed to be easily extendible to a specific application. It provides
the major functionalities classically found in languages such as C or C++, in a dynamic,
interpreted environment.
By default, French accents cannot be included in a script except if the string # coding=utf-8 is added
as first line of the script.
This section provides a brief overview of the basic features of the Python language. Interested
readers should consult the tutorial documents or the systematic description of the language
available on the Python web site (http://www.python.org).
Scripts are evaluated line by line. However, line evaluation continues on the next line if the
character '\' is the last character of the line.
Adding Commented Lines
The '#' character specify that the rest of the line is a comment and will be skipped while the macro
is executed.
Support for Mathematical Operations
l the operators +, -, * and / are defined,
l parenthesis can be used and nested to any level,
l functions abs(x), int(x), floor(x), ceil(x) and sqrt(x) for square root are available,
l trigonometric functions sin(x), cos(x), tan(x), acos(x), asin(x), atan(x) are available, atan2(x,y)
returns atan(x/y),
l logarithmic functions log(x) for neperian logarithm, log10(x) for base 10 logarithm, exp(x),
sinh(x), cosh(x), tanh(x), asinh(x), acosh(x) are available,
l x to the power y is obtained by the function pow(x,y),
l boolean values are returned by the operators >, <, <=, >=, ==, !=, and, or,
l the constants pi and e are predefined.
String Handling
Strings are handled in Python in the following way:
l they are enclosed in single <'> or double <"> quotes,
l concatenation is obtained with the operator +,
l duplication is obtained by the multiplication by an integer (operator *),
l access to the ie element is obtained by the suffix '[i]' and access to a substring is obtained by
the suffix [i:j] for a substring starting from the ie character to the je,
l numerical values contained in variables can be inserted in a string by enclosing the variable
name with reverse quotes (') or by using a formatting specification:
Example:
s = 'The Value of x is' +'x'
s = 'The Value of x is %3d' %(x)
The formatting symbols are interpreted as follows:
l %d formats in an integral value (rounded if necessary)
l %nd (where n is an integer) in an integral value having a length of exactly n characters
(space characters are inserted on the left if necessary)
l %n.mf (where n and m are integers and n>m) formats into a floating point value having at
most n characters length and a fractional part of m characters exactly
l %n.me(where n and m are integers and n>m) formats into a scientific representation having
at most n characters length and a fractional part of m characters exactly
l stripping of the leading or trailing white spaces is obtained by the function strip.
Example:
myStrippedString = strip(myString)
Lists Handling
A list is an ordered set of items.
l a list is defined by enclosing the comma separated items by square brackets. A list may be
empty,
Example:
my_list = [a,b]
empty_list = []
Note that list definition can be extended over several lines without the '\' terminating character.
l an item is accessed by adding the suffix [i] to the list name (ex: my_list[1]). Note that list
indices start at 0,
l lists can be nested to any level,
l appending is obtained by the operator + (ex: my_list + my_list2) or by the function append
(ex:my_list.append([c, d])),
l multiplication (appending oneself n times) is obtained by the multiplication operator (ex: my_
list*3),
l the functions insert(index, value) inserts value at position index, the elements at upper position
are shifted,
l the function index(value) returns the index of the first item of which the value is value,
l the function remove(value) removes the first item of which the value is value,
l the functions sort(), reverse() and len() are, respectively, sorting, reversing the elements and
returning the number of elements in the list.
Control Flow
The body part of these instructions is defined by the indented lines and the specific control lines
are terminated by a colon. The end of the loop body is marked by the first line that does not start
by a tab character. Nested loop are obtained by heading lines with multiple characters.
l if statement:
Example:
if x < 0 :
print 'x is negative'
elif x==0 :
print 'x is null'
else :
print 'x is positive'
elif and else clauses may be omitted.
l loop statements: the for loop iterates on the elements of a list and the while loop iterates as long
as the condition is met. A break statement may be inserted to step out of the loop.
Example:
for x in a[:] :
for x in range(0,10) :
while x>0 :
where the range function returns a list of integers starting from the first argument value to the
second argument value with a step indicated by the third argument if existing (default value is
1).
Function Definition
Function definition starts with the standard header:
def function_name (arg1, arg2, arg3 = default_value, ...)
where def is a reserved keyword. The arguments can be of any type (it is a user responsibility to
provide meaningful ones) and last arguments may have a default value (as arg3 in the above
example).
Each line of the function's body is indented with a TAB character. The function definition ends
with the first line which is not indented by a TAB character.
All arguments are passed by value. Thus, if an argument value is modified, the new value is not
available to the caller.
A returned value may be specified using the 'return' statement followed by the name of the
variable or by a value. In any case, a value is returned and not a reference on a local variable or
object. The type of the returned value is a list, this means that appending a new element in the
returned list is obtained by the statement 'return.append(x)'.
Global scope variable can be accessed if they are declared as such by a statement 'global' (e.g.
'global x' specifies that the x variable is a global variable for the current function).
File Handling
Files can be opened for reading and writing. A file is associated to a variable which is initialized
at its opening:
f = open(fileName, mode, bufferSize)
where fileName is the full file name including its path. The parameter mode is a character string of
which the value may be:
l 'r' or 'rb': file opened for reading,
l 'w' or 'wb': file opened for writing, creates it if not existing or the previous content is discarded,
l 'a' or 'ab': file opened for appending, creates if not existing or writes at the end of the file.
The 'b' character is used only on Windows systems to indicate that the file is in binary mode, on
Linux system, it is neglected.The parameter bufferSize is the integer value of the size of the
buffer, the system default size is chosen if the value is negative, the file is opened in the
unbuffered mode if the value is 0, a value of 1 specifies a line-buffered mode.
The following functions can be used to handle the file content:
l f.close(): closes file,
l f.flush(): flushes file's internal buffer,
l f.read(n): reads at most n bytes from the file and returns as a string. If n is omitted, reads to the
end of the file,
l f.readline(): reads one entire line,
l f.readlines():reads until the end of the file and returns a list of lines,
l f.seek(offset, whence=0): sets file position, if whence =0 or is omitted, offset is the absolute
position, if whence=1 offset is relative to the current position and if whence = 2, offset is
relative to the file end,
l f.tell(): returns file current position,
l f.write(string): writes string to file.
Error Handling
FINE™/Open performs continuous checks during the running of a script to insure that functions
can be normally executed, check of arguments validity during calls to functions or object access.
When a check fails, FINE™/Open raises an exception which stops the execution of the script.
Create & Use Modules (library of functions)
The python language provides the concept of module for grouping a set of functions in a same
file. The module name is the name of the file containing the functions.
The functions can be made available into a script in a similar way to the large set of utility
functions provided with FINE™/Open. If a set of functions is defined in a file called
MyModule.py, and the file is located in the directory /people/myself/open_scripts, they can be
made available in another
sys.path.append
('/people/myself/open_scripts')
through the following instructions:
script
This declares to the system that some python files are available in that directory. Then, two
different ways can be used to import the functions: from MyModule import * or import MyModule
The first one sets all the functions defined in MyModule directly available, while the second form
makes them available with the MyModule. prefix (e.g. if a function f is defined in MyModule, it is
invoked by the command MyModule.f()).
The standard python modules may be imported with both of the above mentioned forms. The
directory declaration is not necessary.
15.2 FINE™/OPEN WITH OPENLABS™ SCRIPT
COMMANDS
All FINE™/Open commands are available from the FHX module ( under INSTALL_DIR/_
python/_fine/_hexa/). This means that they must be accessed by default by using the FHX prefix.
Example:
import FHX
FHX.open('myfile.iec')
Alternatively, the prefix can be omitted by using the statement "from FHX import *". However,
in that case, the user must insure that no other module contains a same command being used.
Example:
from FHX import *
open('myfile.iec')
15.2.1 Global functions
A. Project management
l create_project(directory_name)
Create directory structure on disk:
projectName/
projectName/_mesh/
l new_project()
Destroy current project (data structure reset to default).
l open_project(project_name)
Open an existing project.
l save_project()
Save current project:
projectName/projectName.iec
l link_mesh_file(mesh_filename)
Link the project with a mesh file.
l set_unit_ratio(ratio)
Set unit ratio. Parameter 'ratio' can be any real. The following constants can be used as 'ratio':
METER (ratio=1.0)
CENTIMETER (ratio=0.01)
MILLIMETER (ratio=0.001)
INCH (ratio=0.0254)
Example:
set_unit_ratio(MILLIMETER)
B. Computation management
l get_nb_computations()
Return the number of computations.
l set_computation_name(index,name)
Modify the name of computation specified by its index (0<= index <nb of computations).
l set_active_computations(indexList)
Select computation(s) by specifying their indices.
Example:
set_active_computations([0,2,3])
l new_computation(name)
Create a new computation. This will have the name specified by 'name'. The new computation
will be automatically selected. All its parameters take the same value than the computation
previously selected.
l clean_selected_computations(flag)
Clean the selected computations. If flag is set to 1, any sub-computations are also cleaned.
l move_up_selected_computations()
Change the position of the selected computations in the list of computations (one step up).
l move_down_selected_computations()
Change the position of the selected computations in the list of computations (one step down).
l remove_selected_computations(flag)
Remove the selected computations. If flag is set to 1, all the related files on the disk are also
deleted.
l save_selected_computations()
Save selected computations:
projectName/projectName_computationName/projectName_computationName.run
l save_batch_file()
Save the batch file associated to the active computation.
C. Project preferences
l get_precision_mode()
Return the precision setting of the solver as a string. Values are "hybrid" or "double"
l set_precision_mode(precision_string)
Set the precision setting of the solver as a string. Valid values are "hybrid" or "double"
D. Domain properties
l get_nb_domains()
Return the number of domains contained in the linked mesh.
l get_domain_name(index)
Return domain name from its index.
l get_domain_index(name)
Return domain index from its name.
l get_all_domains()
Return the list of index corresponding to each domain.
l get_nb_domain_patches(index)
Return the number of patch for the specified domain.
E. General properties
l get_block_type(index)
Return the type of block from its index as a string "FLUID" or "SOLID"
l set_block_type(index,type_string)
set the type of block from its index as a string. Valid values are "FLUID" and "SOLID"
F. Fluid model
l select_fluid_from_database(domain_index,fluid_name)
Select a fluid from the fluid database. This fluid will be attached to the domain(s) specified
either by an index, either by a list of index.
l get_fluid_name(domain_index)
domain_index is the index of the domain. Return the fluid name for the specified domain.
l get_fluid_type(domain_index)
domain_index is the index of the domain. Return the fluid type for the specified domain.
G. Flow model
l get_time_configuration()
Return the time configuration (0:steady / 1:unsteady)
l set_time_configuration(value)
Following constants can be used as 'value':
STEADY (value=0)
UNSTEADY (value=1)
Example:
set_time_configuration(UNSTEADY)
This parameter is global: it applies to all blocks.
l get_mathematical_model(domain_index)
domain_index is the index of the domain. Return the mathematical model for the specified
domain.
l set_mathematical_model(domain_index,value)
domain_index can be either an index, a list of index. Set the mathematical model for the
specified domain(s).
Following constants can be used as 'value':
EULER (value=100)
LAMINAR (value=200)
SPALART_ALLMARAS (value=401)
SARC (value=402)
SPALART_ALLMARAS_EXT_WALL_FUNCTION (value=403)
SARC_EXT_WALL_FUNCTION (value=404)
K_EPSILON_EXT_WALL_FUNCTION (value=501)
K_EPSILON_LOW_RE_YANG_SHIH_CLASSIC (value=503)
K_EPSILON_LOW_RE_YANG_SHIH_DIST_FREE (value=504)
K_OMEGA_M_SST (value=505)
K_OMEGA_WILCOX (value=506)
K_OMEGA_LOW_RE (value=507)
K_OMEGA_LOW_RE_WITH_COMPRESSIBILITY_CORR (value=508)
K_OMEGA_M_SST_EXT_WALL_FUNCTION (value=511)
Example:
set_mathematical_model(SPALART_ALLMARAS)
l get_gravity_flag(domain_index)
domain_index is the index of the domain. Return the gravity activation flag (0:off / 1:on)
l set_gravity_flag(domain_index,value)
domain_index can be either an index, a list of index. Set the gravity activation flag (0:off /
1:on)
l get_gravity_h0(domain_index)
domain_index is the index of the domain. Return the gravity h0 (type Point)
l set_gravity_h0(domain_index,value)
domain_index can be either an index or a list of index. Set the gravity h0 (type Point)
l get_gravity_vector(domain_index)
domain_index is the index of the domain. Return the gravity vector (type Vector)
l set_gravity_vector(domain_index,value)
domain_index can be either an index or a list of index. Set the gravity vector (type Vector)
l get_preconditioning(domain_index)
domain_index is the index of the domain. Return the preconditioning activation flag (0:off /
1:on)
l set_preconditioning(domain_index,value)
domain_index can be either an index or a list of index. Set the preconditioning activation flag
(0:off / 1:on)
l get_reference_length(domain_index)
domain_index is the index of the domain. Return the reference length for the specified domain.
l set_reference_length(domain_index,value)
domain_ index can be either an index or a list of index. Set the reference length for the
specified domain(s)
l get_reference_velocity(domain_index)
domain_ index is the index of the domain. Return the reference velocity for the specified
domain.
l set_reference_velocity(domain_index,value)
domain_index can be either an index or a list of index. Set the reference velocity for the
specified domain(s).
H. Solid model
l get_solid_conductivity_type(index)
Return the type of conductivity as a flag: 0 for scalar value, 1 for profile
l get_solid_conductivity_value(index)
Return the conductivity as a floating point scalar value
l get_solid_conductivity_profile(index)
Return the law of conductivity as a list of coordinates
Format is [t1, k1, t2, k2, ..., tn, kn]
l set_solid_conductivity_type(index,flag)
Set the type of conductivity as a flag: 0 for scalar value, 1 for profile
l set_solid_conductivity_value(index,value)
Set the conductivity as a floating point scalar value
l set_solid_conductivity_profile(index,data_list)
Set the law of conductivity as a list of coordinates
Format for the list is [t1, k1, t2, k2, ..., tn, kn]
I. Rotating machinery
l get_rotating_machinery_flag(domain_index)
domain_index is the index of the domain. Return the rotating flag for the specified domain
(0:off / 1:on).
l set_rotating_machinery_flag(domain_index,flag)
domain_index can be either an index or a list of index. Set the rotation flag for the specified
domain(s) (0:off / 1:on).
l get_rotating_machinery_rotation_speed(domain_index)
domain_index is the index of the domain. Return the rotation speed for the specified domain.
l set_rotating_machinery_rotation_speed(domain_index, speed)
domain_index is the index of the domain. Set the rotation speed for the specified domain(s).
l get_rotating_machinery_rotation_axis(domain_index)
domain_index is the index of the domain. Return the rotation axis for the specified domain
(type Vector).
l set_rotating_machinery_rotation_axis(domain_index, axis)
domain_index can be either an index or a list of index. Set the rotation axis for the specified
domain(s) (type Vector).
l get_rotating_machinery_rotation_center(domain_index)
domain_index is the index of the domain. Return the rotation center for the specified domain
(type Point).
l set_rotating_machinery_rotation_center(domain_index, center)
domain_index can be either an index or a list of index. Set the rotation center for the specified
domain(s) (type Point).
J.
Initial solution
l get_turbo_channel_nb_entrance_patches()
Return the number of entrances of the channel (patch or group of patches).
l get_turbo_channel_nb_internal_patches()
Return the number of internal R/S connections.
l get_turbo_channel_nb_exit_patches()
Return the number of exits of the channel (patch or group of patches).
l get_turbo_channel_nb_exit_up_patches()
Return the number of up exits of the channel (patch or group of patches).
l get_turbo_channel_entrance_patches()
Return the list of BCPatch instances of the channel entrance. If some patches are grouped, the
first patch of the group is added to the list.
l get_turbo_channel_internal_patches()
Return the list of BCPatch instances internal to the channel. If some patches are grouped, the
first patch of the group is added to the list.
l get_turbo_channel_exit_patches()
Return the list of BCPatch instances of the channel exit. If some patches are grouped, the first
patch of the group is added to the list.
l get_turbo_channel_exit_up_patches()
Return the list of BCPatch instances of the channel up exit. If some patches are grouped, the
first patch of the group is added to the list.
K. Numerical model
l get_CPU_booster_flag()
Return the CPU Booster activation flag (global parameter, 0:off / 1:on).
l set_CPU_booster_flag(flag)
Set the CPU Booster activation flag (global parameter, 0:off / 1:on).
l get_MG_CFL_number(domain_index)
Return the applied CFL number during coarse grid initialization for the specified domain. If no
argument is defined, the CFL number of the first domain will be returned.
l set_MG_CFL_number(domain_index,value)
Set the CFL number during coarse grid initialization for the specified domain. If no domain is
defined, the CFL number will be applied to all domains.
l get_CFL_number(domain_index)
domain_index is the index of the domain. Return the CFL number for the specified domain.
l set_CFL_number(domain_index,value)
domain_index can be either an index or a list of index. Set the CFL number for the specified
domain(s).
l get_MG_level_number()
Return the number of multigrid levels (global parameter).
l set_MG_level_number(value)
Set the number of multigrid levels (global parameter).
l get_MG_flag()
Return the multigrid activation flag (global parameter, 0:off / 1:on).
l set_MG_flag(value)
Set the multigrid activation flag (global parameter, 0:off / 1:on).
l get_MG_number_of_sweeps()
Return the sweeps on each MG level (global parameter).
l set_MG_number_of_sweeps(value)
Set the sweeps on each MG level (global parameter).
l get_MG_correction_damping()
Return the correction damping (global parameter).
l set_MG_correction_damping(value)
Set the correction damping (global parameter).
l get_MG_number_of_cycles()
Return the max number of cycles per grid level (global parameter).
l set_MG_number_of_cycles(value)
Set the max number of cycles per grid level (global parameter).
l get_MG_convergence_criteria()
Return the convergence criteria (global parameter).
l set_MG_convergence_criteria(value)
Set the convergence criteria (global parameter).
l get_MG_dual_number_of_iterations()
Return the maximal number of inner iterations for dual time step inner-iteration control
l set_MG_dual_number_of_iterations(value)
Set the maximal number of inner iterations for dual time step inner-iteration control
l get_MG_dual_convergence_criteria()
Return the convergence criteria for dual time step inner-iteration control
l set_MG_dual_convergence_criteria(value)
Set the convergence criteria for dual time step inner-iteration control
l get_numerical_scheme(blockId)
Return the numerical scheme for specified block (1:Central, 2:Central matrix, 4:Roe upwind).
l set_numerical_scheme(blockId, scheme)
Set the numerical scheme for specified block (scheme=1:Central, scheme=2:Central matric,
scheme=4:Roe upwind).
Constant value CENTRAL_ SCHEME, CENTRAL_ MATRIX_ SCHEME or ROE_ UPWIND_
SCHEME can be used instead of 1, 2 or 4.
l get_numerical_scheme_accuracy(blockId)
Return the numerical scheme accuracy for specified block (1:1st order, 2:2nd order).
l set_numerical_scheme_accuracy(blockId, accuracy)
Set the numerical scheme accuracy for specified block (accuracy=1:1st order, accuracy=2:2nd
order).
Constant value FIRST_ORDER or SECOND_ORDER can be used instead of 1 or 2.
l get_preconditioning_method(blockId)
Return the preconditioning method for specified block (0: Hakimi, 1:Merkle)
l set_preconditioning_method(blockId, method)
Set the preconditioning method for specified block (method=0: Hakimi, method= 1:Merkle)
Constant value HAKIMI or MERKLE can be used instead of 0 or 1.
l get_preconditioning_beta(domain_index)
domain_index is the index of the domain. Return beta for the specified domain.
l set_preconditioning_beta(domain_index,value)
Set beta for the specified domain(s).
l get_preconditioning_characteristic_velocity(domain_index)
domain_index is the index of the domain. Return the characteristic velocity and the local
scaling flag for the specified domain.
l set_preconditioning_characteristic_velocity(domain_index,vel,flag)
Set the characteristic velocity and the local scaling flag (0:off / 1:on) for the specified domain
(s).
l get_preconditioning_gauge_parameters_activation(domain_index)
domain_index is the index of the domain. Return the gauge activation flag for the specified
domain.
l set_preconditioning_gauge_parameters_activation(domain_index,value)
Set the gauge activation flag for the specified domain(s).
l get_preconditioning_gauge_pressure(domain_index)
domain_index is the index of the domain. Return the gauge pressure for the specified domain.
l set_preconditioning_gauge_pressure(domain_index,value)
Set the gauge pressure for the specified domain(s).
l get_preconditioning_gauge_temperature(domain_index)
domain_index is the index of the domain. Return the gauge temperature for the specified
domain.
l set_preconditioning_gauge_temperature(domain_index,value)
Set the gauge temperature for the specified domain(s).
L. Output parameters
l get_outputs_flow_configuration(domain_index)
domain_index is the index of the domain. Return the flow configuration for the specified
domain.
l set_outputs_flow_configuration(domain_index,value)
domain_index can be either an index or a list of index. Set the flow configuration for the
specified domain(s).
l get_outputs_external_lift(domain_index)
domain_index is the index of the domain. Return the lift direction for the specified domain
(type Vector).
l set_outputs_external_lift(domain_index, liftDir)
domain_index can be either an index or a list of index. Set the lift direction for the specified
domain(s) (type Vector).
l get_outputs_external_drag(domain_index)
domain_index is the index of the domain. Return the drag direction for the specified domain
(type Vector).
l set_outputs_external_drag(domain_index, dragDir)
domain_index can be either an index or a list of index. Set the drag direction for the specified
domain(s) (type Vector).
l get_outputs_external_moment(domain_index)
domain_index is the index of the domain. Return the moment center (Point) and direction
(Vector) for the specified domain.
l set_outputs_external_moment(domain_index, center, direction)
domain_index can be either an index or a list of index. Set the moment center (Point) and
direction (Vector) for the specified domain(s).
l get_outputs_reference_flag(domain_index)
domain_index is the index of the domain. Return the user-defined parameters activation flag
(0:off / 1:on) for the specified domain.
l set_outputs_reference_flag(domain_index, flag)
domain_ index can be either an index or a list of index. Set the user-defined parameters
activation flag for the specified domain(s) (0:off / 1:on).
l get_outputs_reference_density(domain_index)
domain_ index is the index of the domain. Return the reference density for the specified
domain.
l set_outputs_reference_density(domain_index, density)
domain_index can be either an index or a list of index. Set the reference density for the
specified domain(s).
l get_outputs_reference_velocity(domain_index)
domain_ index is the index of the domain. Return the reference velocity for the specified
domain.
l set_outputs_reference_velocity(domain_index, velocity)
domain_index can be either an index or a list of index. Set the reference velocity for the
specified domain(s).
l get_outputs_reference_length(domain_index)
domain_index is the index of the domain. Return the reference length for the specified domain.
l set_outputs_reference_length(domain_index, length)
domain_ index can be either an index or a list of index. Set the reference length for the
specified domain(s).
l get_outputs_reference_area(domain_index)
domain_index is the index of the domain. Return the reference area for the specified domain.
l set_outputs_reference_area(domain_index, area)
domain_index can be either an index or a list of index. Set the reference area for the specified
domain(s).
l select_output(variable_name)
Select the output variable, specified by the variable name.
l unselect_output(variable_name)
Unselect the output variable, specified by the variable name.
M. Launching parameters
l get_launching_mode()
Return the launching mode (global parameter, 0:serial / 1:parallel).
l set_launching_mode(value)
Set launching mode (global parameter, 0:serial / 1:parallel). The following constants can be
used as 'value':
SERIAL (value=0)
PARALLEL (value=1)
Example:
set_launching_mode(PARALLEL)
l get_number_of_processors()
Return the total number of processors, for parallel mode.
l set_number_of_processors(value)
Set the total number of processors, for parallel mode.
N. Control variables
l get_nb_iter_max()
Return the maximum number of iterations (steady mode).
l set_nb_iter_max(value)
Set the maximum number of iterations (steady mode).
l get_convergence_criteria()
Return the convergence criteria (steady mode).
l set_convergence_criteria(value)
Set the convergence criteria (steady mode).
l get_physical_time_step()
Return the physical time step (unsteady mode).
l set_physical_time_step(value)
Set the physical time step (unsteady mode).
l get_nb_of_time_steps()
Return the number of time steps (unsteady mode).
l set_nb_of_time_steps(value)
Set the number of time steps (unsteady mode).
l get_output_writing_frequency()
Return the output writing frequency.
l set_output_writing_frequency(value)
Set the output writing frequency.
O. ANSYS Module
l get_ANSYS_coupling_flag()
Return the ANSYS module activation flag (0:off ; 1:on).
l set_ANSYS_coupling_flag(flag)
Set the ANSYS module activation flag (flag=0:off ; flag=1:on).
l get_ANSYS_pressure_code()
Return the 'Pressure' identification code.
l set_ANSYS_pressure_code(code)
Set the 'Pressure' identification code.
l get_ANSYS_temperature_code()
Return the 'Temperature' identification code.
l set_ANSYS_temperature_code(code)
Set the 'Temperature' identification code.
l get_ANSYS_heat_transfer_coefficient_code()
Return the 'Heat transfer coefficient' identification code.
l get_ANSYS_heat_flux_code()
Return the 'Heat flux' identification code.
l set_ANSYS_heat_flux_code(code)
Set the 'Heat flux' identification code.
l get_ANSYS_pressure_unit()
Return the 'Pressure' unit system and conversion factor.
l set_ANSYS_pressure_unit(unit)
Set the 'Pressure' unit system. Conversion factor is computed internally.
unit =1: [Pa] factor: 1.0
unit =3: [lbf/ft2] factor: 47.88025898
unit =4: [psi] factor: 6894.757293
l get_ANSYS_temperature_unit()
Return the 'Temperature' unit system and conversion factor.
l set_ANSYS_temperature_unit(unit)
Set the 'Temperature' unit system. Conversion factor is computed internally.
unit =1: [K] factor: 1.0
unit =3: [R] factor: 0.555555555
l get_ANSYS_heat_transfer_coefficient_unit()
Return the 'Heat transfer coefficient' unit system and conversion factor.
l set_ANSYS_heat_transfer_coefficient_unit(unit)
Set the 'Heat transfer coefficient' unit system. Conversion factor is computed internally.
unit =1: [W/(m2.K)] factor: 1.0
unit =3: [lbf/(s.ft.R)] factor: 26.269025
unit =4: [lbf/(s.in.R)] factor: 315.2283
l get_ANSYS_heat_flux_unit()
Return the 'Heat flux' unit system and conversion factor.
l set_ANSYS_heat_flux_unit(unit)
Set the 'Heat flux' unit system. Conversion factor is computed internally.
unit =1: [W/m2] factor: 1.0
unit =3: [lbf/(s.ft)] factor: 14.59390294
unit =4: [lbf/(s.in)] factor: 175.1268352
l get_ANSYS_temperature_bulk_flag()
Return the temperature bulk computation flag (0:off ; 1:on).
l set_ANSYS_temperature_bulk_flag(flag)
Set the temperature bulk computation flag (flag=0:off ; flag=1:on).
l get_ANSYS_input_filename()
Return the ANSYS input file name.
l set_ANSYS_input_filename(filename)
Set the ANSYS input file name. This filename is read to initialize the surface parameters.
l get_ANSYS_output_filename()
Return the ANSYS output file name.
l set_ANSYS_output_filename(filename)
Set the ANSYS output file name. This filename will be created afterwards by the solver.
l get_ANSYS_grid_units()
Return the grid units.
l set_ANSYS_grid_units(unit)
Set the grid units.
unit =0: Millimeters
unit =1: Centimeters
unit =2: Meters
unit =3: Inches
unit =4: User-defined scale factor
l get_ANSYS_scale_factor()
Return the scale factor. Used if 'User-defined scale factor' is selected as grid units.
l set_ANSYS_scale_factor(factor)
Set the scale factor. Used if 'User-defined scale factor' is selected as grid units.
l get_ANSYS_fluid_mesh_reference_system()
Return the FLUID mesh reference system (Origin and three points).
l set_ANSYS_fluid_mesh_reference_system(orig, pnt1, pnt2, pnt3)
Set the FLUID mesh reference system.
l get_ANSYS_solid_mesh_reference_system()
Return the SOLID mesh reference system (Origin and three points).
l set_ANSYS_solid_mesh_reference_system(orig, pnt1, pnt2, pnt3)
Set the SOLID mesh reference system.
l get_ANSYS_fluid_reference_system()
Return the SOLID mesh reference system (Origin and three points).
l set_ANSYS_fluid_reference_system(orig, pnt1, pnt2, pnt3)
Set the SOLID mesh reference system.
l get_ANSYS_solid_reference_system()
Return the FLUID mesh reference system (Origin and three points).
l set_ANSYS_solid_reference_system(orig, pnt1, pnt2, pnt3)
Set the FLUID mesh reference system.
l initialize_ansys_surfaces()
Just to ensure backward compatibility with scripts generated for version 4.2
l clear_ansys_surfaces( sID )
Clear list of solid patches connected to ANSYS surface sID.
l connect_ansys_solid_face_to_patch( *args )
Set list of connected patches to a given ANSYS surface.
*args may be:
sID,b,f,p
sID: ANSYS surface id
b: FLUID block ID
f: always 1
p: FLUID patch ID
The patch (b,f,p) is added to the patches connected to the ANSYS surface SID.
sID, [[b0,p0],[b1,p1],...[bn,pn]]
sID:ANSYS surface id
[bi , pi] : FLUID patch specified from block ID patch ID
The list of couples [bi,pi] replace the patches connected to the ANSYS surface SID.
l get_ANSYS_connected_fluid_patch_periodic_flag(surfID, patchID)
Return the 'Periodic' flag of patch patchID connected to ANSYS surface surfID (0:off ; 1:on).
l set_ANSYS_connected_fluid_patch_periodic_flag(surfID, patchID,flag)
Set the 'Periodic' flag of patch patchID connected to ANSYS surface surfID (flag=0:off ;
flag=1:on).
l get_ANSYS_connected_fluid_patch_rotation_angle(surfID, patchID)
Return the rotation angle around Z [degree] of patch patchID connected to ANSYS surface
surfID.
l set_ANSYS_connected_fluid_patch_rotation_angle(surfID, patchID,angle)
Set the rotation angle around Z [degree] of patch patchID connected to ANSYS surface
surfID.
l get_ANSYS_connected_fluid_patch_translation_vector(surfID, patchID)
Return the translation vector of patch patchID connected to ANSYS surface surfID.
l set_ANSYS_connected_fluid_patch_translation_vector(surfID, patchID,vector)
Set the translation vector of patch patchID connected to ANSYS surface surfID.
l get_ANSYS_connected_fluid_patch_nb_repetitions(surfID, patchID)
Return the number of repetitions of patch patchID connected to ANSYS surface surfID.
l set_ANSYS_connected_fluid_patch_nb_repetitions(surfID, patchID,nRepet)
Set the number of repetitions of patch patchID connected to ANSYS surface surfID.
l get_ANSYS_connected_fluid_patch_partial_flag(surfID, patchID)
Return the 'Partial' flag of patch patchID connected to ANSYS surface surfID (0:off ; 1:on)
l set_ANSYS_connected_fluid_patch_partial_flag(surfID, patchID,flag)
Set the 'Partial' flag of patch patchID connected to ANSYS surface surfID (flag=0:off ;
flag=1:on).
l get_ANSYS_solid_surface_list()
Return the list of ANSYS surfaces.
l get_ANSYS_solid_surface_interpolation_type(sID)
Return the interpolation type of ANSYS surface sID.
l set_ANSYS_solid_surface_interpolation_type(sID, interpType)
Set the interpolation type of ANSYS surface sID.
interpType =0: "non-conservative"
interpType =1: "conservative" (NOTE: not implemented in solver).
l get_ANSYS_solid_surface_maximum_distance(sID)
Return the maximum distance of ANSYS surface sID.
l set_ANSYS_solid_surface_maximum_distance(sID, maxDistance)
Set the maximum distance of ANSYS surface sID.
P. Porous media parameters
l enable_porous_media_computing(domain_index)
domain_index is the index of the domain. Activate porous media computing for the specified
domain.
l disable_porous_media_computing(domain_index)
domain_index can be either an index or a list of index. Disable porous media computing for
the specified domain(s)
l get_porous_media_model(domain_index)
domain_ index is the index of the domain. Get the porous media model for the specified
domain.
l set_porous_media_model(domain_index,value)
domain_index can be either an index or a list of index. Set the porous media model for the
specified domain(s). The following constants can be used as 'value':
DARCY_LAW (value=1)
ERGUN_LAW (value=2)
INTEGRAL_LAW (value=3)
Example:
set_porous_media_model(0,DARCY_LAW)
l get_porous_media_darcy_option(domain_index)
domain_index is the index of the domain. Get the darcy law option for the specified domain.
l set_porous_media_darcy_option(domain_index,value)
domain_ index can be either an index or a list of index. Get the darcy law optionfor the
specified domain(s). The following constants can be used as 'value':
CARMAN_KOZENY_FORMULA (value=0)
USER_DEFINED_HOMOGENEOUS (value=1)
USER_DEFINED_NON_HOMOGENEOUS (value=2)
Example:
set_porous_media_darcy_option(0,CARMAN_KOZENY_FORMULA)
l get_porous_media_darcy_carman_kozeny_parameters(domain_index)
domain_index is the index of the domain. Get the Carman-Kozeny parameters for the specified
domain:
Porosity
Specific surface area
l set_ porous_ media_ darcy_ carman_ kozeny_ parameters (domain_ index, porosity, spec_ surf_
area)
domain_index can be either an index or a list of index. Set the Carman-Kozeny parameters for
the specified domain(s).
l get_porous_media_darcy_homogeneous_parameters(domain_index)
domain_index is the index of the domain. Get the parameter 'kPrim' for the specified domain.
l set_porous_media_darcy_homogeneous_parameters(domain_index,kPrim)
domain_index can be either an index or a list of index. Set the parameter 'kPrim' for the
specified domain(s).
l get_porous_media_darcy_nonhomogeneous_parameters(domain_index)
domain_index is the index of the domain. Get the Darcy law parameters for the specified
domain:
kPrim
ksi direction
eta direction
l set_porous_media_darcy_nonhomogeneous_parameters(domain_index,kPrim,ksi_dir, eta_dir)
domain_index can be either an index or a list of index. Set the Darcy law parameters for the
specified domain(s).
l get_porous_media_ergun_option(domain_index)
domain_index is the index of the domain. Get the Ergun law option for the specified domain.
l set_porous_media_ergun_option(domain_index,value)
domain_index can be either an index or a list of index. Get the Ergun law option for the
specified domain(s). The following constants can be used as 'value':
CARMAN_KOZENY_FORMULA (value=0)
USER_DEFINED_HOMOGENEOUS (value=1)
USER_DEFINED_NON_HOMOGENEOUS (value=2)
Example:
set_porous_media_ergun_option(0,CARMAN_KOZENY_FORMULA)
l get_porous_media_ergun_carman_kozeny_parameters(domain_index)
domain_index is the index of the domain. Get the Carman-Kozeny parameters for the specified
domain:
Porosity
Specific surface area
Surface type ('ROUGH' or 'SMOOTH')
l set_ porous_ media_ darcy_ carman_ kozeny_ parameters (domain_ index,porosity, spec_ surf_
area,surface_type)
domain_index can be either an index or a list of index. Set the Carman-Kozeny parameters for
the specified domain(s).
l get_porous_media_ergun_homogeneous_parameters(domain_index)
domain_ index is the index of the domain. Get the parameters 'kPrim' and 'kSec' for the
specified domain.
l set_porous_media_ergun_homogeneous_parameters(domain_index,kPrim, kSec)
domain_index can be either an index or a list of index. Set the parameters 'kPrim' and 'kSec'
for the specified domain(s).
l get_porous_media_ergun_nonhomogeneous_parameters(domain_index)
domain_index is the index of the domain. Get the Ergun law parameters for the specified
domain:
kPrim
kSec
ksi direction
eta direction
l set_ porous_ media_ ergun_ nonhomogeneous_ parameters (domain_ index,kPrim,kSec, ksi_
dir,eta_dir)
domain_index can be either an index or a list of index. Set the Ergun law parameters for the
specified domain(s).
l get_porous_media_integral_law_parameters(domain_index)
domain_index is the index of the domain. Get the 'Integral law' parameters for the specified
domain:
Proportionality constant
Thickness
Area ratio
Exponent
l set_ porous_ media_ integral_ law_ parameters (domain_ index,propor_ cst,thickness,
area_
ratio,exponent)
domain_index can be either an index or a list of index. Set the 'Integral law' parameters for the
specified domain(s).
l get_porous_media_flow_direction(domain_index)
domain_index is the index of the domain. Get the flow direction parameters for the specified
domain:
Impose direction flag (0:off / 1:on)
Flow direction
l set_porous_media_flow_direction(domain_index,impose_flag,flow_dir)
domain_index can be either an index or a list of index. Set the flow direction parameters for
the specified domain(s).
Q. Coupling
Global settings
l get_coupling_mode()
Return the coupling activation mode (0:no coupling, 1:coupling with modal approach).
l set_coupling_mode(mode)
the coupling activation mode (mode=0:no coupling, mode=1:coupling with modal
Set
approach).
Following constants can be used as 'mode' :
NO_COUPLING (mode=0)
MODAL_APPROACH_COUPLING (mode=1)
l get_coupling_reference_pressure()
Return the reference pressure.
l set_coupling_reference_pressure( value )
Set the reference pressure.
Manage coupling boundary patch(s)/group(s)
l get_coupling_nb_groups()
Return the number of coupling boundary patch(s)/group(s).
l get_coupling_group_index( name )
Return the index of the coupling boundary patch/group specified by its name.
l add_coupling_patch_to_group( bcPatch, groupName )
Add a patch (BCPatch type)to the group specified by its name. For example, add_coupling_
patch_to_group(get_bc_patch(0,12),"NewGroup"). If groupName does not exist, it will be
created.
l remove_coupling_patch_from_group( bcPatch )
Remove a patch (BCPatch type) from the group that belongs to.
Activate modal coupling for a patch/group
l get_coupling_patch_modal_structure_ID( item )
Return the modal structure ID attached to a coupling patch/group.
The patch/group (item) can be specified by its index (integer) or by its name (string).
l set_coupling_patch_modal_structure_ID( item , ID)
Activate modal coupling for the patch/group (item) and set the modal structure ID which will
be attached to the patch/group (item).
The patch/group can be specified by its index (integer) or by its name (string).
Manage modal structure
l get_coupling_nb_modal_structures()
Return the number of modal structures.
l create_coupling_modal_structure( ID, name, filename, dampingCoefficients )
Create a new modal structure.
ID: integer to identify the modal structure. If already existing, it will be updated with specified
parameters.
name: string to identify the name of this structure.
filename: string to identify the structure file.
dampingCoefficients: vector of floats to identify the damping coefficients of each mode. Note
that the number of coefficients should not exceed the number of modes of the structure file.
l get_coupling_modal_structure_ID( index )
Return the ID of the modal structure specified by its index.
l get_coupling_modal_structure_index( ID )
Return the index of the modal structure specified by its ID.
Return -1 if no modal structure with this ID exists.
l get_coupling_modal_structure_name( ID )
Return the name of the modal structure specified by its ID.
l set_coupling_modal_structure_name( ID, name )
set the name of the modal structure specified by its ID.
l get_coupling_modal_structure_filename( ID )
Return the name of the structure file for the modal structure specified by its ID.
l set_coupling_modal_structure_filename( ID, filename )
set the name of the structure file for the modal structure specified by its ID.
l get_coupling_modal_structure_nb_modes( ID )
Return the number of modes of the modal structure specified by its ID.
l get_coupling_modal_structure_damping_coefficients( ID )
Return the damping coefficients of the modal structure specified by its ID.
l set_coupling_modal_structure_damping_coefficients( ID, coefficients )
set the damping coefficients of the modal structure specified by its ID.
R. Expert parameters
l get_expert_parameter(domain_index,param_name)
domain_index is the index of the domain. Return the value of the expert parameter for the
specified domain.
l set_expert_parameter(domain_index,param_name,param_value)
domain_index can be either an index or a list of index. Set the value of the expert parameter,
for the specified domain(s).
15.2.2 Classes
A. Boundary conditions
class BCPatch
l BCPatch(blockID,patchID)
Construct a BCPatch object from the block and patch ids. The ids must correspond to a valid
block/patch.
l get_block_patch()
Return the block and patch ids.
l get_name()
Return the name of the patch.
l get_bc_name()
Return the B.C. name.
l get_bc_type()
Return the B.C. type.
l set_bc_type(value)
Set the B.C. type. The following constants can be used as 'value':
INLETs:
SUPERSONIC_CARTESIAN_VELOCITY_COMPONENTS [23,0]
SUPERSONIC_CYLINDRICAL_VELOCITY_COMPONENTS [23,1]
SUBSONIC_CYLINDRICAL_VELOCITY_COMPONENTS [23,2]
SUPERSONIC_ CARTESIAN_ MACH_ NUMBER_ AND_ VELOCITY_ ANGLE_
IMPOSED [23,3]
SUBSONIC_CARTESIAN_STATIC_PRESSURE_EXTRAPOLATED [24,1]
SUBSONIC_CARTESIAN_MACH_NUMBER_EXTRAPOLATED [24,2]
SUBSONIC_ CARTESIAN_ MAGNITUDE_ OF_ ABSOLUTE_ VELOCITY_
EXTRAPOLATED [24,3]
SUBSONIC_CARTESIAN_MACH_NUMBER_AND_VELOCITY_ANGLE_IMPOSED
[24,4]
SUBSONIC_CARTESIAN_VELOCITY_DIRECTION [28,3]
SUBSONIC_CYLINDRICAL_ANGLE_FROM_AXIAL_DIRECTION [124,1]
SUBSONIC_ CYLINDRICAL_ ANGLE_ FROM_ AXIAL_ DIRECTION_ V_
EXTRAPOLATED [124,2]
SUBSONIC_ CYLINDRICAL_ ANGLE_ FROM_ AXIAL_ DIRECTION_ VZ_
EXTRAPOLATED [124,3]
SUBSONIC_CYLINDRICAL_VELOCITY_DIRECTION_V_EXTRAPOLATED [124,4]
SUBSONIC_ CYLINDRICAL_ ANGLE_ FROM_ MERIDIONAL_ DIRECTION_
STATIC_PRESSURE_EXTRAPOLATED [124,5]
SUBSONIC_ CYLINDRICAL_ TANGENTIAL_ VELOCITY_ AND_ MERIDIONAL_
ANGLE_VM_EXTRAPOLATED [124,6]
SUBSONIC_ CYLINDRICAL_ VELOCITY_ COMPONENTS_ STATIC_ PRESSURE_
EXTRAPOLATED [124,7]
SUBSONIC_ CYLINDRICAL_ RELATIVE_ ANGLE_ FROM_ AXIAL_ DIRECTION_
VZ_EXTRAPOLATED [124,8]
SUBSONIC_ CYLINDRICAL_ RELATIVE_ VELOCITY_ DIRECTION_ W_
EXTRAPOLATED [124,9]
SUBSONIC_CYLINDRICAL_MERIDIONAL_FLOW_ANGLE_AND_TANGENTIAL_
VELOCITY [ 28,1]
SUBSONIC_CYLINDRICAL_VELOCITY_DIRECTION [ 28,2]
OUTLETs:
SUBSONIC_CARTESIAN_STATIC_PRESSURE_IMPOSED [ 25, 10]
SUBSONIC_CARTESIAN_RADIAL_EQUILIBRIUM [125, 10]
SUPERSONIC_EXTRAPOLATION [ 22, 0]
SUBSONIC_CARTESIAN_VELOCITY_SCALING [ 27, 21]
SUBSONIC_CARTESIAN_PRESSURE_ADAPTATION [ 27, 30]
SUBSONIC_CYLINDRICAL_STATIC_PRESSURE_IMPOSED [ 25,110]
SUBSONIC_CYLINDRICAL_RADIAL_EQUILIBRIUM [125,110]
SUBSONIC_CYLINDRICAL_VELOCITY_SCALING [ 27,121]
SUBSONIC_CYLINDRICAL_PRESSURE_ADAPTATION [ 27,130]
SOLIDs:
NS_CARTESIAN_ADIABATIC [ 13,0]
NS_CARTESIAN_HEAT_FLUX_IMPOSED [ 10,0]
NS_CARTESIAN_TEMPERATURE_IMPOSED [ 14,0]
EULER_EULER_SOLID_WALL [ 16,0]
NS_CYLINDRICAL_ADIABATIC_CONSTANT_ROTATION_SPEED [113,0]
NS_CYLINDRICAL_ADIABATIC_AREA_DEFINED_ROTATION_SPEED [113,1]
NS_ CYLINDRICAL_ HEAT_ FLUX_ IMPOSED_ CONSTANT_ ROTATION_ SPEED
[110,0]
NS_ CYLINDRICAL_ HEAT_ FLUX_ IMPOSED_ AREA_ DEFINED_ ROTATION_
SPEED [110,1]
NS_CYLINDRICAL_TEMPERATURE_IMPOSED_CONSTANT_ROTATION_SPEED
[114,0]
NS_ CYLINDRICAL_ TEMPERATURE_ IMPOSED_ AREA_ DEFINED_ ROTATION_
SPEED [114,1]
EXTERNALs:
STATIC_QUANTITIES [21,1]
MACH_NUMBER_AND_VELOCITY_ANGLE [21,2]
l get_parameter_value(parameter_name)
Return the parameter value, specified by its name.
l set_parameter_value(parameter_name,value)
Set the parameter value, specified by its name.
l get_compute_force_and_torque_flag()
Return the "force and torque" computation flag (0:off / 1:on).
l set_compute_force_and_torque_flag(value)
Set "force and torque" computation flag (0:off / 1:on).
Besides this class, here are some global functions dealing with B.C management:
l get_bc_patch_by_name(patch_name)
Return the BCPatch object from the patch name.
l get_bc_patch_list(pattern)
Return a list of BCPatch object from the pattern. The pattern is a string containing Linux shell-
style wildcards:
Pattern Meaning
* Matches everything
? Matches any single character
[seq] Matches any character in seq
[!seq] Matches any character not in seq
Example:
get_bc_patch_list('front*')
Return the list of BCPatch objects which name begin by 'front'
l create_group(group_name,value)
Create a group. The name of group will be 'group_name'. 'value' can be either the exhaustive
list of BCPatch objects to group or a pattern as described above.
l ungroup(group_name)
Remove all patches from specified group.
B.
Initial solution
class InitialSolution
l InitialSolution(blockID)
Construct a InitialSolution object from the block id. The id must correspond to a valid block.
l get_mode()
Return the starting mode.
l set_mode(mode)
Set the starting mode. The following constants can be used for the mode:
FOR_TURBOMACHINERY= "turbo"
CONSTANT_VALUES = "const"
FROM_FILE = "file"
TECHNO_EFFECTS= "auto"
l get_coord_system()
Return the coordinate system.
l set_coord_system(coord_system)
Set the coordinate system. The following constants can be used for the coordinate system:
CARTESIAN_COORDS = 'abs'
CYLINDRICAL_COORDS = 'rel'
Constant Value
l get_pressure()
Return the initial pressure.
l set_pressure(pressure)
Set the initial pressure.
l get_temperature()
Return the initial temperature.
l set_temperature(temperature)
Set the initial temperature.
l get_velocity_type()
Return the initial velocity type.
l set_velocity_type(velocity_type)
Set the initial velocity type. The following constants can be used for the velocity type:
ABSOLUTE_VELOCITY = 'abs'
RELATIVE_VELOCITY = 'rel'
l get_velocity()
Return the initial velocity.
l set_velocity(velocity)
Set the initial velocity. The velocity must be a vector. For example, Vector(100,0,0).
l get_turb_viscosity()
Return the initial turbulent viscosity.
l set_turbulent_viscosity(turb_visc)
Set the initial turbulent viscosity.
l get_k_epsilon()
Return the initial k and epsilon.
l set_k_epsilon(k,epsilon)
Set the initial k and epsilon.
Initialisation from file
l get_restart_filename()
Return the filename for restart.
l set_restart_filename(filename)
Set the filename for restart.
l get_restart_mode()
Return the restart mode.
l set_restart_mode(mode)
Set the restart mode. The following constants can be used as 'mode':
RESET_CONVERGENCE_HISTORY (value=1)
IMPORT_CONVERGENCE_HISTORY (value=2)
Example:
set_restart_mode(0,RESET_CONVERGENCE_HISTORY)
Turbomachinery initialisation
l get_turbo_entrance_patch()
Return the BCPatch instance which is selected as main entrance.
If a group of patches is selected as main entrance, then the first patch of this group is returned.
If no channel entrance exists, None is returned.
l set_turbo_entrance_patch(bcpatch)
Set the BCPatch instance to be selected as main entrance.
If it is part of a group, then all patches of this group will be selected.
l get_turbo_exit_patch()
Return the BCPatch instance which is selected as main exit.
If a group of patches is selected as main exit, then the first patch of this group is returned.
If no channel exit exists, None is returned.
l set_turbo_exit_patch(bcpatch)
Set the BCPatch instance to be selected as main exit.
If it is part of a group, then all patches of this group will be selected.
l get_turbo_exitup_patch()
Return the BCPatch instance which is selected as main up exit (in case of bypass).
If a group of patches is selected as main exit, then the first patch of this group is returned.
If no channel up exit exists, None is returned.
l set_turbo_exitup_patch(bcpatch)
Set the BCPatch instance to be selected as main up exit (in case of bypass).
If it is part of a group, then all patches of this group will be selected.
l get_turbo_patch_pressure_type(bcpatch)
Return the pressure type (CONSTANT_PRESSURE=0 / RADIAL_EQUILIBRIUM=1) for
the specified bcpatch.
l set_turbo_patch_pressure_type(bcpatch, pressureType)
Set the pressure type (CONSTANT_PRESSURE=0 / RADIAL_EQUILIBRIUM=1) for the
specified bcpatch.
l get_turbo_patch_pressure(bcpatch)
Return the initial pressure value for the specified bcpatch.
l set_turbo_patch_pressure(bcpatch, pressure)
Set the initial pressure for the specified bcpatch.
l get_turbo_patch_radius(bcpatch)
Return the radius value for
EQUILIBRIUM).
the specified bcpatch (to be used with RADIAL_
l set_turbo_patch_radius(bcpatch, radius)
Set the radius for the specified bcpatch (to be used with RADIAL_EQUILIBRIUM)
l get_turbo_patch_temperature(bcpatch)
Return the initial temperature value for the specified bcpatch.
l set_turbo_patch_temperature(bcpatch, temperature)
Set the initial temperature for the specified bcpatch.
l get_turbo_patch_velocity_type(bcpatch)
Return the velocity type for the specified bcpatch (0:absolute ; 1:relative).
l set_turbo_patch_velocity_type(bcpatch, velocityType)
Set the velocity type for the specified bcpatch (0:absolute ; 1:relative).
l get_turbo_patch_vr(bcpatch)
Return the radial velocity for the specified bcpatch.
l set_turbo_patch_vr(bcpatch, vr)
Set the radial velocity for the specified bcpatch.
l get_turbo_patch_vt(bcpatch)
Return the tangential velocity for the specified bcpatch.
l set_turbo_patch_vt(bcpatch, vt)
Set the tangential velocity for the specified bcpatch.
l get_turbo_patch_vz(bcpatch)
Return the velocity (z component) for the specified bcpatch.
l set_turbo_patch_vz(bcpatch, vz)
Set the velocity (z component) for the specified bcpatch.
CHAPTER 16.
OPENLABS™
OpenLabs™ is a module of FINE™/Open with OpenLabs™ environment, which allows the user to
customize the internal physical models in FINE™/Open and/ or add external physical models. Here,
"internal" means that
the physical models have already been implemented in FINE™/Open and
"external" means that the physical models will be defined by the user through OpenLabs™.
OpenLabs™ gives the user ability to access the physical model in the FINE™/Open solver. OpenLabs™
transforms the user-defined physical models to a library that will be loaded by the flow solver when
launching the computation. To describe a physical model, the user need to write a resource file that lists
a set of objects (including constants, transport equations, algebraic relations, source terms and so on)
and their math expressions in a metalanguage as described below. OpenLabs™ will transform the
resource file to a C++ file and build it to a dynamic library. What user need to do is to set a
FINE™/Open project, write the resource and build the library, then launch the computation.
In this section
16.1 Get Started
16.2 Functionalities
16.3 Limitations
16.4 OpenLabs in the FINE™/Open GUI
16.5 OpenLabs Language
455
456
457
458
471
16.1 GET STARTED
FIGURE 16.1 gives the illustration how OpenLabs works.
FIGURE 16.1
Illustration of OpenLabs
In general, OpenLabs is used through the following steps.
Create a FINE™/Open with OpenLabs™ project
The starting point is to prepare a project as usual: first create a mesh and then create a
FINE™/Open project. The settings of the project (fluid model, flow model, optional models,
boundary conditions, initial conditions, numerical parameters…) have to be defined.
It is recommended to set-up the FINE™/Open project as similar as possible to the final modeling
approach. For example, if user wants to modify an internal k-ε turbulence model, a project with
the internal k-ε turbulence model should be set-up. A complete customized turbulence model can
be added in a Laminar Navier-Stokes simulation. However, it might be easier to start from an
internal turbulent framework and modify it according to the specific needs.
Analyze your project to get potential input parameters
Once the project is ready, the user can activate OpenLabs for each block. Before writing the
resource, it is recommended to analyze your project to get the potential input parameters, see
Analyze section. The project analysis results contain the list of internal constants, variables,
algebraic expressions, transport equations with their corresponding source terms and diffusion
coefficients, as well as the internal boundary conditions.
Write resource and build library
The resource can be written in the Resource Manager , please refer to OpenLabs in the
FINE™/Open GUI on how to use the Resource Manager and OpenLabs Language on how to
write the resource in OpenLabs language.
After the resource is written, the user need to Build Library for each block,
which will save the resource to a ".rc" file, transform the ".rc" file to a C++ file and compile the
C++ file to generate the dynamic library.
Run computation and post-process results
After the dynamic library has been created, the flow solver can be launched as usual. The created
dynamic library will be called during the runtime. The external variables added with OpenLabs
can also be post-processed in CFView™ (Outputs by OpenLabs).
16.2 FUNCTIONALITIES
The user-defined functionalities mainly concern the physical models. The numerical algorithm
and schemes are not considered.
With OpenLabs, the user can:
l modify/add constants of physical models.
l modify/add algebraic expressions. For example, the user can modify the definition of the
turbulence time scale.
l add an arbitrary number of transient-convection-diffusion-source equations (PDE). For the
PDE equations, the user has to provide the following information: source terms, diffusion
coefficient definition, boundary conditions, initial conditions, settings related to the numerical
scheme to be used for the convective term, other numerical parameters related to the relaxation,
clipping, etc.
l modify/add source terms for the internal/external PDEs.
l modify/add diffusion coefficients for the internal/external PDEs.
l modify/add initial fields for internal/external PDEs. It is possible to use cylinder coordinates in
expressions and to specify the initial solutions for the polar velocity vector.
l add boundary conditions for external PDEs and modify internal boundary conditions. The user
can define Dirichlet conditions, Neumann conditions with zero gradient and Robin conditions
for external variables. The user can also modify the internal boundary conditions by giving
algebraic expressions to the imposed physical variables.
16.3
LIMITATIONS
For the moment, the following limitations exist in the OpenLabs™ module:
1. Compiler requirements of OpenLab™:
Windows
Customization of the CFD models using OpenLabs™ requires the possibility for compilation.
On Windows 64 bit, Microsoft Visual C++ Build Tools 2015 must be installed: make sure to
select the component Windows 10 SDK 10.0.10240 during the installation.
Linux
Customization of the CFD models using OpenLabs™ requires the possibility for compilation:
On Linux 64 bit, the GNU C and C++ compiler (g++) must be installed. The gcc version
should be between 4.8.# and 5.3.# (type the command gcc -v in a shell to get your gcc
version). The officially tested version is g++ 4.8.5.
When opening an existing OpenLabs™ project in a newer FINE™/Open version, it is strongly
recommended to recompile the library before launching the computation.
2. OpenLabs™ uses only SI units.
3. OpenLabs™ is compiled with the OpenMPI library. It is not compatible with the IntelMPI
library.
4. When customizing internal boundary conditions, the following limitations apply:
l Cannot customize the radius when the outlet boundary condition is defined by Pressure
Imposed - Radial Equilibrium.
l Cannot customize the initial pressure when the outlet boundary condition is defined by
Mass Flow Imposed.
l Cannot customize Backflow Control at outlets.
l Cannot customize the Von Karman constant κ, the Bo constant, the equivalent roughness
height k0 and the height of the zero displacement plane d0 used for the wall functions.
l Cannot change the type of the boundary condition. For example, the user cannot change
the inlet boundary condition from Static Quantities Imposed to Total Quantities
Imposed in OpenLabs™.
5. OpenLabs™ cannot define different physical models which have different new variables in
connected fluid blocks.
6. The customized convection speed is not compatible with the convection scheme
UpwindHighOrderConservative as well as with FNMB, NMB, PERNM, PER, R/S
boundaries.
7. Vector can be used in OpenLabs™. But it cannot be outputted or used to define coupled
equations.
8. When using control points, the following limitations apply:
l The value of the control point is only updated on the finest grid level.
l The control point must be inside the current block.
l The control point should be given by using Cartesian coordinates with the same grid unit as
the project.
l UTau, TTau, other variable defined only on boundaries and geometric variables are not
available in control points.
l The local value of the control point defined in OpenLabs™ cannot be visualized via
steering and not be written in .ctl_out file.
16.4 OPENLABS IN THE FINE™/OPEN GUI
The OpenLabs Resource Manager is a basic editor that allows the user to write/edit the resource
and build the dynamic library. When opening the Resource Manager, the default layout appears,
as shown in FIGURE 16.2. An overview of the complete layout of the Resource Manager is
shown in FIGURE 16.3.
FIGURE 16.2
Default Resource Manager layout
FIGURE 16.3
Complete overview of the Resource Manager
OpenLabs can be activated or deactivated from the block list, as shown on the top-left frame in
FIGURE 16.2. OpenLabs is block-dependent. The user can activate OpenLabs for part of the
blocks or all the blocks in the project. To activate/deactivate OpenLabs for a block, left-click on
before the block name. After activate
the block name to select it, then left-click on the sign
OpenLabs for a block, the resource frame, as shown on the top-right in FIGURE 16.2, becomes
accessible.
at the left side of the name Resource
If OpenLabs is activated in the computation, the mark
Manager will become green or red, depending on the status of the library. If the color is red, the
user will have to check and re-build the library.
16.4.1 Menu Bar
File menu
New / Empty Resource
Creates an empty resource, containing only the titles of all sections.
New / From Template
Creates a resource from a template. When clicking on this menu, the OpenLabs Resource
Templates window appears. The user can select the provided template and confirm by clicking
the button Ok. Then the template will be loaded. Currently only one template is provided, which
is called "default".
FIGURE 16.4
OpenLabs resource template window
Import
Selects an existing resource file to import.
Export
Exports the content of the resource of the selected block to a file.
Close
Saves the content of the resource in the project file ".iec" and close the window.
Edit menu
Undo (<Ctrl>+<Z>)
Undoes the last modification made in the resource.
Cut (<Ctrl>+<X>)
Cuts the selected text.
Copy (<Ctrl>+<C>)
Copies the selected text.
Paste (<Ctrl>+<V>)
Pastes the copied text to the position of the cursor.
Find (<Ctrl>+<F>)
Finds and selects the specified string in the resource.
If the option Match Case is activated, the search will be case sensitive. The option Direction
controls the direction of the search. Search starts at the current cursor position and goes Up/Down
in the file.
The button Find Next is used to find and select the next occurrence of the specified string.
Find next (<F3>)
Finds and selects the next occurrence of the specified string.
Replace (<Ctrl>+<G>)
Replaces a string in the resource.
If the option Match Case is activated, the search will be case sensitive. The option Direction
controls the direction of the search. Search starts at the current cursor position and goes Up/Down
in the file.
The button Find Next is used to find and select the next occurrence of the specified string. The
button Replace is used to replace the selected string that you search for, and then search for the
next occurrence. The button Replace All is used to replace all of the occurrences of the specified
string that you want to replace.
Select All (<Ctrl>+<A>)
Selects all the content of the resource.
Build menu
Build Current
Builds the dynamic library for the current selected block.
When clicking on this menu, the interface will save the resource to a ".rc" file, transform the ".rc"
file to a C++ file (".C") and compile the C++ file to generate the dynamic library for the current
selected block.
Build All
Builds the dynamic library for all blocks.
When clicking on this menu, the interface will save the resource to a ".rc" file, transform the ".rc"
file to a C++ file (".C") and compile the C++ file to generate the dynamic library for each block.
Preferences
When clicking on this menu, a dialog box appears:
l Auto list keywords : allowing to enable/disable the automatic completion when typing a
special character "=>", "@" or "->", see Write Resource section for more details. By default,
the automatic completion is enabled.
l Stop process after a compilation error: For a multiblock case, all libraries may be generated
at once. This preference allows the resource manager to stop or keep building libraries after a
compilation error. By default, the resource manager will keep building libraries after a
compilation error.
Tools menu
Analyze
The project analysis results will automatically be saved into the ".ana" file and displayed in the
Analysis frame, as shown on the top-middle in FIGURE 16.3. The project analysis file consists
of the following sections:
l CONSTANTS: In this section all the modeling constants and the reference conditions used in
the computation are listed. Typical quantities such as Prandtl number ( phys_ Prandtl_ ),
reference density (rhoRef_), reference temperature (TRef_), etc are listed in this section.
l CFD_ VARAIBLES : In this section all the computed CFD variables (pressure, velocity,
temperature, etc) are listed.
l GEOMETRIC_VARIABLES: In this section all the geometry related quantities which are
used in the computation are listed.
l FLUID_ PROPERTIES : In this section the equation of state and the state relations of
thermodynamic properties can be seen. Information related to the transport properties such as
viscosity and thermal conductivity are also displayed in this section.
l EQUATIONS: In this section all the internal PDEs that are solved in the computation are
listed.
l INTERNAL_BOUNDARY_CONDITIONS: In this section all the boundary patches and
corresponding patch IDs are listed.
l ALGEBRAIC_DIFFUSION_COEFFICENTS: In this section all the diffusion coefficient
that are used in the internal PDEs are listed.
l SOURCETERMS: In this section all the source term related to the turbulence model, porous
media, gravity and rotation source term if used in the computation are listed.
Analyze in detail
The detailed project analysis results will automatically be saved into the ".ana" file and displayed
in the Analysis frame, as shown on the top-middle, in the FIGURE 16.3.
The detailed project analysis results will have the list of the objects name in each section along
with their math expression. Detailed analysis results also include all the auxiliary terms with their
math expression in the section AUXTERMS.
In detailed project analysis results, implementation details of the porous media, turbulence,
rotation and the gravity models can be seen when these models are activated from the
FINE™/Open GUI. This can be used to customize the physical models using OpenLabs.
Customization can effectively be done in two different ways:
Modification of existing physical model using OpenLabs
the physical model has to be activated for the relevant block (s),
First,
in the Physical
Configuration/General Properties page. In the FINE™/Open GUI, the physical model that is
closest to the one the user wants, needs to be selected. In OpenLabs/Resource Manager it is now
possible to see the details of the selected model using the Tools/Analyzein detail menu item.
In the CONSTANTS section of the detailed project analysis results all the constants used in the
computation will be listed. These constants can be copied into the resource area and their
definition can be changed.
Constant can be redefined by a new value or a function of other constants in the resource area. In case
the constant is function of other variables e.g. the temperature, it is no longer a constant and therefore
should be defined in appropriate section in resource area. In that case same name cannot be used as it
is already reserved for the constant in the solver.
If any physical models (e.g porous media) are activated in the FINE™/Open GUI, a source term
is added to energy or momentum equation based on the type of the model selected. In the
SOURCETERMS section of the detailed project analysis results, the source terms related to the
physical model will be listed. To modify the definition of the source terms, copy it into the
resource section and modify it if needed. As long as the same name for the source term is kept, the
definition in the resource area overwrites the one in the FINE™/Open solver.
Example given below shows the SOURCETERMS section of detailed project analysis results
when the porous media is enabled and the Darcy model with Carmen-kozeny formula is selected
from the FINE™/Open GUI:
@ Source: PorousMedia
->EXPRESSION(MomentumXEquation): -(Viscosity+EddyVisc)*Vx/Permeability
->EXPRESSION(MomentumYEquation): -(Viscosity+EddyVisc)*Vy/Permeability
->EXPRESSION(MomentumZEquation): -(Viscosity+EddyVisc)*Vz/Permeability
->EXPRESSION(EnergyEquation):-(Viscosity+EddyVisc)/Permeability* \
(Vx*Vx+Vy*Vy+Vz*Vz)
If the name of the source term ("PorousMedia" in the above example) is changed, an additional
source term is added to the one already activated through the FINE™/Open GUI. Hence it is very
important to either keep exactly the same name or to deactivate the porous media model through the
FINE™/Open GUI.
The flow direction as it can be defined in the FINE™/Open GUI for porous media model, is not
accessible for modification in OpenLabs. Nonetheless, if a flow direction is defined through the GUI,
it will be taken into account even when making modifications to the constant(s) or source terms of
the porous media model in OpenLabs.
The AUXILIARY section in the detailed project analysis results has a list of all the auxiliary
terms used in the computation along with their math expression. If any auxiliary terms are used in
defining the source terms then these auxiliary terms need to be copied to resource area. If required
the user can change the expression of these terms.
Define of a new physical model from scratch
Instead of activating the physical model through the GUI and modifying in Openlabs, physical
model can be defined from scratch.
In this case it is not important what is the name of the added source terms and their definition. In
such cases, user has to make sure to have the physical model in the GUI deactivated to use only
the created Lab instead of any of the already existing models. Otherwise the source terms may be
added twice and hence leading to incorrect results.
View menu
Analysis
Shows or hides the Analysis frame, see FIGURE 16.3.
Output
Shows or hides the Output frame, seeing FIGURE 16.3.
16.4.2 Write Resource
After OpenLabs is activated for a block, the resource linked to this block can be edited. The user
can start to write the resource from an empty resource file, from template or from an imported
resource file.
When writing the resource, an automatic contextual completion window will appear if typing a
special character "=>", "@" or "->". The contents of the automatic completion window are
depending on the cursor position. For example,
the section
"=>EQUATIONS", the following list will appear:
typing "@" under
if
@NONDIFFEXPR:
@PDE:
The keyword will be inserted in the cursor position after selected by moving the cursor on the
keyword and left-clicking, or by using the up/down arrow and confirming by the key <Enter>.
The user can also quit the automatic completion window by pressing the key <Esc> or left-
clicking inside the resource manager, then type the keyword manually.
When writing the resource, the user can also call the contextual completion window by pressing
on the key <Ctrl>+<space>. Depending on the cursor position, the window will show the defined
keyword (sections, objects and attributes). The keyword will be inserted in the cursor position
after selected.
16.4.3 Building Status and Building/Loading Information
. If
If building a library is successful, the check mark before the block name will be green
building a library has failed, the check mark will be red
. The status of the library will be
checked and updated when opening a project, selecting a computation, launching the flow solver,
saving a batch run file or changing the project settings.
The information of building a library is also outputted in the Output frame on the bottom in
FIGURE 16.3. If building a library fails, error messages will be given in the Output frame.
16.4.4 Outputs by OpenLabs
If new transport properties ( Customized transport properties ), new algebraic expressions
(Algebraic Expressions) or new PDEs (Convection-diffusion-source transport equations: PDE)
in the
have been defined in OpenLabs,
Computation Control / Outputs page under the tab General after building the library. By
default, all new variables are selected for output.
the new variables will be available for output
16.4.5 Monitor the Convergence History
The convergence history of external variables is saved in the.res file, which can be visualized in
monitor. To launch monitor, the user can click on the Start Monitor button (
from the FINE™/Open GUI, see Monitoring & Launching Mode for more details on monitor.
) on the icon bar
FIGURE 16.5
Monitor external variables
Click the button Other variables, all external variables defined by external PDEs will be listed.
Then select a variable and its convergence history will be shown.
16.4.6 Files Generated by OpenLabs
OpenLabs is block-dependent. Each block in the project has its own resource file and library. All
the files generated by OpenLabs are saved in the computation folder.
On LINUX, the files generated by OpenLabs are as follows (i is the index of the block):
l project_name_bi.ana contains the list of properties and equations that are defined in the
project.
l ResourceFile_bi.rc contains the resource written by the user.
l compileOpenLabs_bi.C contains the transformed C++ file from the resource.
l compileOpenLabs_bi.o is the object file of the compilation from the C++ file.
l compileOpenLabs_bi.log contains all the log information related to "Build Library".
l libOL_bi.so is the generated dynamic library.
On Windows, the files generated by OpenLabs are as follows (i is the index of the block):
l project_name_bi.ana contains the list of properties and equations that are defined in the
project.
l ResourceFile_bi.rc contains the resource written by the user.
l compileOpenLabs_bi.cpp contains the transformed C++ file from the resource.
l compileOpenLabs_bi.obj is the object file of the compilation from the C++ file.
l compileOpenLabs_bi.exp and compileOpenLabs_bi.lib are the files generated by Microsoft
Visual C++.
l compileOpenLabs_bi.log contains all the log information related to "Build Library".
l libOL_bi.dll is the generated dynamic library.
16.4.7 Build library in batch on Linux
In some cases, the user may want to prepare the FINE™/Open project locally. Then, copy the
project to a HPC machine and launch in batch. If OpenLabs™ is activated in the project, the user
needs to rebuild the library on the HPC machine. FINE™/Open also provides possibility to
rebuild the library in batch for Linux systems.
To rebuild library in batch under Linux, follow the steps below:
1. Prepare project locally. Edit OpenLabs™ resource file and build library.
This step will save required files (.rc) in the computation folder. Each block where OpenLabs™ is
activated will have one .rc file (ResourceFile_b#.rc).
2. Copy the project to your HPC machine.
3. On your HPC machine, open a shell, go to the computation folder.
4. Launch the command: openLabsCreator_open72 computation_name.run -print
OpenLabs™ will convert each .rc file into a .C file (compileOpenLabs_b#.C).
5. Compile each .C file using the command: compileOpenLabs_ open72 compileOpenLabs_
b#.C -print
OpenLabs™ will build one library file (libOL_ b#.so) for each block where OpenLabs™ is
activated.
16.5 OPENLABS LANGUAGE
16.5.1 General Frame
In general, a resource includes the following sections (or a part of them). Each section starts with
the symbol "=>" and a keyword.
In each section, there could be several objects. Each object is defined by a keyword with the
symbol "@" before and ":" after.
In each object, there are a set of attributes (some are optional) and each attribute is defined by a
keyword with the symbol "->" before and ":" after.
=>CONSTANTS
@ ...
=>EQUATIONS
@ NONDIFFEXPR: <name1>
->EXPRESSION: <math expression 1>
@ PDE:
->...
=>CUSTOMIZED_BOUNDARY_CONDITIONS
@ CUSTOMIZED_BOUNDARY_CONDITION:
->…
=>ALGEBRAIC_DIFFUSION_COEFFICIENTS
@ ALGDIFFCOEFF:
->...
=>INITIAL_PROFILES
@ INITIAL_FIELD:
=>SOURCETERMS
@ SOURCE:
->…
=>AUXTERMS
@...
=>GLOBAL_QUANTITIES
@...
=>ADDITIONAL_INFORMATION
@...
Math expressions should be closed. All variables must be defined. Their definitions are sequence
independent. Spaces are allowed in math expressions.
The keywords and their definition of the sections, objects and attributes will be explained in the
following sections.
16.5.2 Nomenclature principle
Within the sections defined in the resource, the user needs to define the corresponding objects to
describe the physical model. Each object generally consists of name of the object, name of
variables, math expression, as well as a set of keywords. To define the object names and variable
names, the following rules must be obeyed:
l Only Latin alphabet characters, numbers, underscore can be used;
l No space is allowed in a name;
l Characters are case sensitive;
l A name cannot contain the keywords described in OpenLabs Language section. For example,
as CONSTANT_ alpha, or AUXTERM1, or
a name
the user can not define
EXPRESSIONforBeta;
l A name cannot be the same as the math operators, logical operators and so on, e.g. sin;
l To modify the internal objects, the exact names given in the project analysis results have to be
used.
16.5.3 Encrypt resource file
OpenLabs™ allows the user to encrypt part or all contents of the resource file. This allows the
users to distribute their OpenLabs™ resource file but keep its contents confidential.
To encrypt part or all contents of the resource file, the user should add the keyword " $OL_
TOENCRYPT_ BEGIN$ " before the section to be encrypted and " $OL_ TOENCRYPT_
END$" after the section to be encrypted. For example:
=>INITIAL_PROFILES
$OL_TOENCRYPT_BEGIN$
@INITIAL_FIELD: Velocity_x
->EXPRESSION: 800
->ExistingField: Vx
$OL_TOENCRYPT_END$
After building library, the resource file ".rc" located in the computation directory will give the
following encrypted contents:
=>INITIAL_PROFILES
$OL_
ENCRYPTED_
BEGIN$448DF19046C82F43E136FF284C7B05B96EF8D1692D4A8BB3699631C944593983
E2F42D9769245497FF45FDA3323BB2526E2C3A1306FC078FCFA8137B99E66E13606125
731722$OL_ENCRYPTED_END$
Please note, when encrypting resource file, the resource saved in .iec file and shown in the
OpenLabs™ resource manager will not be encrypted. So that the user can keep the resource in
the original project. OpenLabs™ only encrypts the contents of the resource file ".rc" saved in the
computation directory.
If a user gets an encrypted resource file ".rc", the user can import it in the OpenLabs™ resource
manager and build library with the encrypted resource. However, the user cannot check and edit
the encrypted part of the resource.
16.5.4 Variables, Operators and Control Statements
Comment Lines
The character "#" is used to comment out complete lines or part of the lines. For example:
# This line will be ignored
@ CONSTANT: <constant name 1> # Everything after this symbol will be ignored
Line Break
In some cases, in order to avoid too long lines, it might be useful to break them (for example, in
case that a very long formula needs to be introduced). The character "\" is used to break a line.
For example:
->EXPRESSION: sigma * StaticTemperature + \
+ beta * (StaticTemperature–Ref_Temp)
The expression above is equivalent to:
->EXPRESSION: sigma * StaticTemperature + beta * (StaticTemperature–Ref_Temp)
If a line break is used, all the text written in the same line after the symbol "\" will be ignored. For
example, the text "This is a source" will be ignored in the following example:
->EXPRESSION: sigma * StaticTemperature \ This is a source
+ beta * (StaticTemperature–Ref_Temp)
Implicit Expression
Sometimes, the relation between variables may be implicit. In this case, the variable must be
solved iteratively. In OpenLabs, the implicit expression can be solved by using the Newton-
Raphson method or by using the user defined iterative expression.
The Newton-Raphson Method
To solve the implicit expression, the relation can be re-written as a zero function f(x)=0 and is
solved by:
To formulate the iterative equation, the user has to provide the jacobian
of the function, either
analytically (keyword Jacobian) or numerically (keyword Disturbance), and some other
informations. The format of giving an implicit expression in the resource file is as follows:
->EXPRESSION: SOLVE(<name of variable, for example x>):{
Zero_Function: <f(x)>
Jacobian: <dfdx> #(Optional)
or
Disturbance: <dx> #by default
InitializeTo: <x0> # by default 0 (Optional)
LowerLimit: <xmin>
Upper Limit: <xmax>
Iteration_Number: <max number of iterations> # by default: 30 (Optional)
Converge_Criterion: <eps> # by default:
(Optional)
}
If the domain of the implicit expression does not cover all real number, e.g. the domain of log(x) is
x >0, it's necessary to either rewrite the expression so that the domain covers all real number, or
provide limiters in order to improve the robustness.
For example, to solve x at a given y0, where y=f(x) and f is a monotonically increasing function in
the region of [xmin,xmax], the Newton-Raphson method could be used:
->EXPRESSION:SOLVE(x):{
Zero_Function: f(x)-y0
Jacobian: dfdx
InitializeTo:x0
}
User Defined Iterative Expressions
Alternatively, the implicit expression can be solved by an user defined iterative expression:
In this case, the keyword "ITERATIVE" must be used. The iterative function should be given
by the user with the keyword "Iterative_Function". The format of giving an implicit expression
in the resource file is as follows:
->EXPRESSION:SOLVE(<name of variable, for example x>):ITERATIVE{
Iterative_Function: <x>=<f(x)>
InitializeTo: <x>=<x0>
Iteration_Number: <max number of iterations> # by default: 30 (Optional)
}
Besides the variable to be solved, there could be several auxiliary terms being iterative. These
auxiliary terms cannot be used in the other expressions and should be defined in SOLVE {} of
the current expression. The user-defined iterative expressions can be written as:
->EXPRESSION:SOLVE(<name of variable, for example x>):ITERATIVE{
Iterative_Function: <aux name1> = <aux expression 1>
...
Iterative_Function: <aux nameN> = <aux expression N>
Iterative_Function: <x>=<f(x)>
InitializeTo: <aux name1> = <initial value of aux1>
...
InitializeTo: <aux nameN> = <initial value of auxN>
InitializeTo: <x>=<x0>
Iteration_Number: <max number of iterations> # by default: 30 (Optional)
}
For example, to solve x at a given y0, where y=f(x) and f is a monotonically increasing function in
the region of [xmin,xmax], the Newton-Raphson method could be used:
->EXPRESSION:SOLVE(x):ITERATIVE{
Iterative_Function:y=f(x)
Iterative_Function: xLower=IF(y<y0) x ELSE xLower
Iterative_Function: xUpper=IF(y<y0) xUpper ELSE x
Iterative_Function:x=0.5*(xLower+xUpper)
InitializeTo:xLower=xmin
InitializeTo: xUpper=xmax
InitializeTo:x=x0
}
Discrete Expression
Discrete expressions are introduced into OpenLabs so that the user can impose a profile data to a
variable. According to the dependency, the profiles can be divided into three types:
l Profiles dependent on geometric variables, for example, Vx (x). They are usually used in
boundary conditions.
l Profiles dependent on CFD variables, for example, Cp(T). They are usually used in defining
fluid properties.
l Profiles dependent on physical time, for example, a time dependent source term.
The user has the flexibility to add a profile dependent on arbitrary variable names. The name of the
dependent variables must be written explicitly (in the resource or the .dat file).
The profile data can be inputted by file or defined in the resource.
Import Discrete Expression by File
When importing the discrete expression by a file, the user should give the file name after the
keyword "->EXPRESSION: PROFILE":
->EXPRESSION: PROFILE<File name>
The inputted file can be in the .p format or .dat format:
l The format with the extension .p has the fixed possibilities and recognized by the identity
number inside the file. The data must be given in structured format, see File Format for more
details about the .p format.
l The format with extension .dat is shown below:
<abscissa1> <abscissa2> ...
<number of point of abscissa1> <number of point of abscissa2> ...
<data>
The data in the .dat format should be given in structured format, except for 2-dimensional profile
that can be given in both structured/unstructured formats.
In case that the interpolated point exceeds the data range, the value will be clipped by default
(LIN_INTERPOLATE_CLIP). However, it is possible to use extrapolation at boundary by
using the keyword (LIN_INTERPOLATE_EXTRAPOLATE):
->EXPRESSION: PROFILE: LIN_INTERPOLATE_EXTRAPOLATE<File name>
The linear interpolation of the profile to find the value at a given point in the domain may be time
consuming. A preprocessing can be taken for the structured profiles to save time. The profile data
are remapped as an equidistant mesh. The borders in each dimension can be obtained via a
formula instead of a bisection searching loop. However, please note that this preprocessing is not
recommended for the high non-linear profiles since the accuracy would be lost in the remapping
process. It is deactivated by default. To activate this preprocessing, the profile expression can be
written as:
->EXPRESSION: PROFILE: REGULARIZE_EQUIDISTANT<File name>
In case that the data are loaded from a file, the profile data can be reloaded from this file at every
certain iterations:
->EXPRESSION: PROFILE: RELOAD_EVERYITER(number_iteration)<File name>
Define Discrete Expression in the Resource
When defining the discrete expression in the resource, the user can give the complete data after
the keyword "->EXPRESSION: PROFILE" with following format:
->EXPRESSION: PROFILE(abscissa1, abscissa2, ..., abscissaN) { 
nbPoint_abscissa1 nbPoint_abscissa2 ... nbPoint_abscissaN
data1_min data2_min … dataN-1_min dataN_min ordinate
data1_min data2_min … dataN-1_min dataN_min+ ordinate
...
data1_min data2_min … dataN-1_min dataN_max ordinate
data1_min data2_min … dataN-1_min+ dataN_min ordinate
...
data1_min data2_min … dataN-1_min+ dataN_max ordinate
…
...
data1_max data2_max … dataN-1_max dataN_min ordinate
...
data1_max data2_max … dataN-1_max dataN_max ordinate
}
In particular, 2-dimensional profile can be given in points cloud:
->EXPRESSION: PROFILE(abscissa1, abscissa2) {
data1_1 data2_1 ordinate
data1_2 data2_2 ordinate
...
data1_N data2_N ordinate
}
When defining the discrete expression in the resource, the user can also give the expression,
instead of giving the data, after the keyword "->EXPRESSION: PROFILE". The expression
and the ranges should be provided with following format:
->EXPRESSION: PROFILE(abscissa1, abscissa2, ..., abscissaN){
Function: <expression>
NumberOfPoint: <abscissa1>, <number of point in abscissa1>
Range: <abscissa1>, <minimum value>, <maximum value>
...
NumberOfPoint: <abscissaN>, <number of point in abscissaN>
Range: <abscissaN>, <minimum value>, <maximum value>
OutToFile: <name of the file> # (optional, the path is by default the computation folder)
}
The discrete expression defined by an expression will be computed only once before the flow
iteration. The build discrete expression could be outputted into a file by using the optional
keyword OutToFile. This function is usually used to reduce the CPU time is case that the
expression is quite complex, such as an user defined EOS.
In case that the interpolated point exceeds the data range, the value will be clipped by default
(LIN_INTERPOLATE_CLIP). However, it is possible to use extrapolation at boundary by
using the keyword (LIN_INTERPOLATE_EXTRAPOLATE):
->EXPRESSION: PROFILE: LIN_INTERPOLATE_EXTRAPOLATE{
...
}
The linear interpolation of the profile to find the value at a given point in the domain may be time
consuming. A preprocessing can be taken for the structured profiles to save time. The profile data
are remapped as an equidistant mesh. The borders in each dimension can be obtained via a
formula instead of a bisection searching loop. However, please note that this preprocessing is not
recommended for the high non-linear profiles since the accuracy would be lost in the remapping
process. It is deactivated by default. To activate this preprocessing, the profile expression can be
written as:
->EXPRESSION: PROFILE: REGULARIZE_EQUIDISTANT{
...
}
Mathematical Operators
The following mathematical operators can be used. An example is included to illustrate the use.
Mathematical Operator
Keyword
sine
cosine
tangent
arc sine
arc cosine
arc tangent
arc tangent of y/x
hyperbolic sine
hyperbolic cosine
hyperbolic tangent
area hyperbolic sine
area hyperbolic cosine
area hyperbolic tangent
Base-e exponential function
Base-2 exponential function
Cubic root
Hypotenuse of a right-angled triangle whose
legs are x and y
Natural logarithm (base-e)
Binary logarithm (base-2)
Common logarithm (base-10)
Raise to power
Square root
Returns the floating-point remainder of
numer/denom
sin
cos
tan
asin
acos
atan
atan2
sinh
cosh
tanh
asinh
acosh
atanh
exp
exp2
cbrt
hypot
log
log2
log10
pow
sqrt
fmod
Example
sin(angle)
cos(angle)
tan(angle)
asin(x/r)
acos(y/r)
atan(y/x)
atan2(y,x)
sinh(angle)
cosh(angle)
tanh(angle)
asinh(y/r)
acosh(x/r)
atanh(y/x)
exp(-TA/StaticTemperature)
exp2(-TA/StaticTemperature)
cbrt(x)
hypot(x,y)
log(x)
log2(x)
log10(x)
pow(StaticTemperature,4.0)
sqrt(TurbK)
fmod(numer,denom)
Mathematical Operator
Keyword
Example
Maximum of two reals
Minimum of two reals
Largest integer less than or equal to x
Smallest integer greater than or equal to x
Round x to the nearest integer
Absolute value
Gradient of a variable in x direction
MAX
MIN
floor
ceil
round
fabs
GRAD
MAX(TurbK,0.0)
MIN(1.0,yfrac)
floor(x)
ceil(x)
round(x)
fabs(x)
GRAD(Vx,x)
(VariableName,x)
Gradient of a variable in y direction
GRAD
GRAD(Vx,y)
(VariableName,y)
Gradient of a variable in z direction
GRAD
GRAD(Vx,z)
1D integration
2D integration
3D integration
Variable at the first fluid cell next to a
boundary face. This operator should be only
used to define boundary conditions.
Dot product
Note:
(VariableName,z)
INTEG1D(expression,
variable name,
min, max)
INTEG1D
(cp,T,Tref_,StaticTemperature)
INTEG2D(expression,
boundary name)
INTEG2D(Density*Vx,
ALLINLETS)
INTEG3D
(expression)
INTEG3D(1)
upcell(VariableName)
upcell(StaticTemperature)
DOT(vector1, vector2) DOT(velocity,velocity)
1. When using the operator INTEG1D(), the bounds min and max can be given by a variable
name which means it equals to the variable value at the position where the expression is
analyzed (in cell, on boundary face...). For example:
INTEG1D(cp_prof, StaticTemperature, TRef_, StaticTemperature)
2. When using the operator INTEG2D()
l ALLINLETS / ALLSOLIDS / ALLOUTLETS refer to all inlets/solids/outlets in the
current block.
l In case that the expression inside INTEG2D is a vector, the normal vector should be
written in the expression, for example,
INTEG2D( Density*(Vx*NormalX+Vy*NormalY+Vz*NormalZ) , ALLINLETS)
3. The following limitations apply for the INTEG1D/INTEG2D/INTEG3D operators:
l The indefinite integration is not doable.
l The INTEG2D is used only for the integral over boundary patches.
l The INTEG3D is used only for the integral over computational domains.
l The INTEG1D is used only for the physical variable dependent profiles/expressions.
l Integration over time is not available.
l The INTEG2D/3D cannot be computed over the boundaries/domains that involve both
solid and fluid blocks.
Logical Operators
The following logical operators can be used.
Logical Operator
Keyword
Alternative Syntax
&&
||
!
==
!=
>
<
>=
<=
Logical AND
Logical OR
Logical negation
Equal to
Not equal to
Greater than
Less than
AND
OR
NOT
EQ
NOTEQ
GREATER
LOWER
Greater than or equal to
GREATEREQ
Less than or equal to
LOWEREQ
Conditional Statements
The following conditional statements can be used.
Conditional Operator
IF
ELSEIF
ELSE
The condition of the "IF" and "ELSEIF" must be written inside a parenthesis. See the following
example:
The expression in the resource will be written as follows:
->EXPRESSION: A = IF (B>=10) 250 ELSEIF (B>5 AND B<10) 50 ELSE 100
By using the line breaks, the same expression can be written as follows:
->EXPRESSION: A = IF (B>=10) 250 \
ELSEIF (B>5 AND B<10) 50 \
ELSE 100
More complex structures can be used. For example:
The expression in the resource will be written as follows:
-> EXPRESSION: A = IF(C>5) IF (B>=5) 15 \
ELSEIF (B>3 AND B<5) 19 \
ELSEIF (B>1 AND B<=3) 17 \
ELSE 18 \
ELSE IF (B>=10) 28 \
ELSE 33
The same expression can be written in a less intuitive form:
-> EXPRESSION: A = IF(C>5) (IF (B>=5) 15 ELSEIF (B>3 AND B<5) 19 \
ELSEIF (B>1 AND B<=3) 17 \
ELSE 18) ELSE (IF (B>=10) 28 ELSE 33 )
A conditional statement with several conditions must start with an IF and end by ELSE . The
keyword ELSEIF is optional.
A conditional statement can only be used with the keyword EXPRESSION. It can not be used to
define constants. For example:
# This is wrong
=>AUXTERMS
@ invYWall = IF (CellVolume>=1e-20) (2*BFaceSurface)/(CellVolume) \
ELSE (2*BFaceSurface)/(CellVolume+1e-20)
# This is right
=>AUXTERMS
@ AUXTERM: invYWall
->EXPRESSION: IF (CellVolume>=1e-20) (2*BFaceSurface)/(CellVolume) \
ELSE (2*BFaceSurface)/(CellVolume+1e-20)
Geometrical quantities
The following geometrical quantities can be used.
Geometrical Quantities
Cartesian coordinates
Cylindrical coordinates
Volume of the cell
Surface area of a boundary face
Keyword
xCoord, yCoord, zCoord
rCoord, tCoord, aCoord
CellVolume
BFaceSurface
Components of surface area vector of a boundary face
xfaceN, yfaceN, zfaceN
Components of unit surface area vector of a boundary face
NormalX, NormalY,
NormalZ
Distance to wall of a cell (used, for example, for turbulence models)
distanceToWall
Normal distance of a boundary cell from the boundary (used to define
boundary conditions)
dn
Time variable
The time variables are used to define temporal dependent terms (e.g. time dependent source terms,
time dependent boundary conditions,…). These variables are used for unsteady computations
only.
Time Variable
Physical Time
Time accurate iteration number
Maximum time accurate iteration number
Vector variable
Keyword
Time
TA_IteNum
TA_IteMax
A vector variable can be defined by its three scalar components enclosed by square brackets, for
example [Vx,Vy,Vz]. The vector can directly be used in any expressions.
Alternatively, to simplify the writing, the user can also define the vector in the section auxiliary
terms starting with the line "=>AUXTERMS".
=>AUXTERMS
@Velocity=[Vx,Vy,Vz]
Then, the vector name can directly be used in any expressions. The user can also use only one of
three components of the vector. For example, Velocity[0] indicates that this is the first component
of the vector Velocity.
Control point
In OpenLabs™, the user can use the local value on a control point. The control point can be an
internal control point defined in the FINE™/Open graphical interface, or an user defined control
point in OpenLabs™.
The variable value on a local control point is expressed by the variable name following with a
control point:
l In case of an internal control point, the expression should be written as:
VarName[<ID of control point>] #for example Density[CTRL_POINT_b0_1]
l In case of an user defined control point, the control point should be expressed by its three
Cartesian coordinates enclosed by square brackets. The expression should be written as:
VarName[<coordinates of control point>] #for example Density[0.5, 1, 1]
The coordinates of the control point must be given by values. For example, the expression Density
[x,y,z] is wrong.
The control point should be used only for the CFD variables (that are not boundary only variables). It
is not suggested to be used for Time and geometrical variables.
The VarName can be the name of an internal quantities or an auxiliary quantities.
The variable value on a local control point can be used in any expressions, except when using a
control point value in SOLVE and PROFILE, it has to be defined as an auxiliary term.
16.5.5 Constants
Constants are used to define the modeling coefficients (e.g. spc_artDiss2ndCoef_), numerical
parameters (e.g. CFL) and so on. These existing constants can be customized or new constants
added in OpenLabs™, and both types can be defined with either a static value or a dynamic
expression. The section to modify and/ or add constants must start with the line =>
CONSTANTS. Each internal or external constant is written by giving a name and its value/
expression.
Detailed nomenclature
=> CONSTANTS
@CONSTANT: <constant name 1>
->Value: <constant value 1>
@CONSTANT: <constant name 2>
->EXPRESSION: <expression 2>
->ExportHistoryToFile: <file name> (optional)
->AddToSteady: <YES (by default) or NO> (optional)
When the constant is defined by an expression, the expression can depend on internal numerical
parameters (e.g. iteration number, Time), internal global parameters (e.g. rotation speed) or any
constants and global quantities (e.g. lift defined in the Lab).
The expression of a constant cannot depend on a geometric variable (e.g. xCoord) or physical
variable (e.g. StaticPressure). Otherwise, OpenLabs™ will abort with an error message.
In order to modify an internal constant, the exact name must be written. For the name of the
internal constant, refer to the project analysis results .
It is important to pay attention to the spelling of the internal constants. In case of a misspelling,
OpenLabs™ will create a new constant instead of modifying the internal one!
The keyword ->AddToSteady is optional. If the keyword ->AddToSteady is not defined,
OpenLabs™ by default updates the constant at each iteration for both steady and unsteady
computations. If the expression depends only on time in case of unsteady computations,
OpenLabs™ will update the constant at every time step. Optionally the keyword -
>AddToSteady can be used: YES - update the constant in each iteration (for both steady and
unsteady cases), and NO - update the constant in each time step (for unsteady cases only).
The keyword - >ExportHistoryToFile: is optional, and allows to check the history of the
customized constant with respect to the iteration number or the time step. If the absolute path for
the file is not specified, OpenLabs™ will save the file in the computation folder with the provided
file name.
Simplified nomenclature
Alternatively, a simplified nomenclature is also available:
=> CONSTANTS
@ <constant name 1> = <constant value 1>
@ <constant name 2> = <expression 2>
…..
Examples
Example 1: modify the Prandtl number
Modify the Prandtl number by adding the following lines in the resource:
=> CONSTANTS
@CONSTANT: phys_Prandtl_
->Value: 0.9
In the simplified nomenclature:
=> CONSTANTS
@phys_Prandtl_ = 0.9
Example 2: change of the rotational speed
The rotational speed of a block is increased linearly from the initial value of 752.5 RPM (≈ 78.80
rad/s) to 1.2 times the initial value.
The following lines should be added in the resource:
=> CONSTANTS
@CONSTANT: rot_Omega_
->EXPRESSION: 78.80 + delta
=> AUXTERMS
@delta = (omega2-omega1) * Time/Period
@omega1 = 78.80
@omega2 = omega1 * 1.2
@Period = 1/omega1
In the simplified nomenclature:
=> CONSTANTS
@rot_Omega_ = 78.80 + delta
=> AUXTERMS
@delta = (omega2-omega1) * Time/Period
@omega1 = 78.80
@omega2 = omega1 * 1.2
@Period = 1/omega1
If the boundary rotation speed is initially set with the same value as the domain rotation speed from
the GUI, it is automatically customized by OpenLabs™ according to the customized rotation speed
expression of the domain.
Two numerical parameters are added in the project analysis results: TA_IteNum (the time accurate
iteration number) and TA_IteMax (the maximum time accurate iteration number). They can be used
to define time dependent expressions. In addition, the lift and drag direction vectors are present in the
project analysis results, allowing user customization.
Example 3: a variable physical time step
The following lines should be added in the resource:
=> CONSTANTS
@CONSTANT: PhysTimeStep
->EXPRESSION: 1.61611e-5*cos(TA_IteNum*2*3.141592/108)+3.23223e-5
->ExportHistoryToFile: <timestep.dat>
In the simplified nomenclature:
=> CONSTANTS
@PhysTimeStep = 1.61611e-5*cos(TA_IteNum*2*3.141592/108)+3.23223e-5
The user should ensure that the time step is never equal or smaller than zero.
It is important to pay attention to the spelling of the internal constant. In case of a misspelling,
OpenLabs™ will create a new constant instead of modifying the internal one.
16.5.6 Algebraic Expressions and PDEs
The user can add or modify algebraic formulas or add external transient-convection-diffusion-
source equations. The section must start with the line "=> EQUATIONS".
Algebraic Expressions
A variable defined by an algebraic formula can be added or modified (e.g. turbulent viscosity in
k-epsilon turbulence models). The section to add algebraic expressions should be added in the
section of "=>EQUATIONS" and must start with "@ NONDIFFEXPR:". Then, each algebraic
expression must be written by adding a given name to the formula. Finally, the variable name and
the expression are written and separated by "=". See the structure below.
=>EQUATIONS
@ NONDIFFEXPR: <Name of the formula 1>
->EXPRESSION: <Name of the variable 1>= <mathematical expression/formula >
->BOUNDARY_FACE: Extrapolation (Optional)
->AddToBoundaryOnly: <Patch num/name>, … (Optional)
->ExportBoundaryProfileToFile: (Abscissas split by ","), <File name>, Patch num (Optional)
@ NONDIFFEXPR: <Name of the formula 2>
->EXPRESSION: <Name of the variable 2>= <mathematical expression/formula >
->BOUNDARY_FACE: Extrapolation (Optional)
->AddToBoundaryOnly: <Patch num/name>, … (Optional)
->ExportBoundaryProfileToFile: (Abscissas split by ","), <File name>, Patch num (Optional)
The boundary values of algebraic expressions can be computed in three ways:
l compute expression at boundary.
l use the extrapolated value from the first inner cell. In order to add this option, the following
line must be added "->BOUNDARY_FACE: Extrapolation".
l set the expression to 0 on the NS wall. In order to add this option, the following line must be
added "->BOUNDARY_FACE: Extrapolation_With_ZERO_On_NSWall".
The attribute line of algebraic expressions with the keyword " ->AddToBoundaryOnly:" is
optional. When this attribute line exists, the algebraic expression will be computed only along the
specified boundaries. To specify the boundaries, the keywords ALLSOLIDS, ALLINLETS
and ALLOUTLETS can be used.
of
line
attribute
algebraic
expressions
The
" -
>ExportBoundaryProfileToFile:" is optional. When this attribute line exists, the value of the
algebraic expression on the specified boundary will be exported to a file. Where, the Abscissas
(split by ",") is used to specify the abscissas. If the user does not specify the absolute path for the
file, OpenLabs™ will save the file in the computation folder. For example, the following line
exports the value of the algebraic expression with respect to xCoord on the patch 4 to a file
/tmp/export.dat.
keyword
with
the
->ExportBoundaryProfileToFile: (xCoord), </tmp/export.dat>, 4
The attribute ExportBoundaryProfileToFile is not available in case of parallel computations.
It is important to note that the name of the formula must be spelled correctly. Otherwise, OpenLabs™
will create a new algebraic expression instead of modifying the internal one.
It is not allowed to modify the value of an internal PDE variable by algebraic expression.
Convection-diffusion-source transport equations: PDE
The transport equation must have the form of a transient-convection-diffusion-source equation:
where ϕ is the variable to be solved,
is the diffusion coefficient and
is the source term.
The section to add a transport equation (PDE) should be added in the section of
"=>EQUATIONS" and must start with "@ PDE:". Each PDE has to be added by giving a name
to the equation, and writing the expression of the equation with the following keywords:
l DDT(<VarName>)
l CONV(<Name of the convection speed, optional>, <VarName>)
l DIFF(<name of the diffusion coefficient >)
l SOURCE(<Name of the source term1> + <Name of the source term2> + …)
The keyword CONV() may have two arguments: the name of the convection speed and the name
of the variable. The first argument, the name of the convection speed, is optional. If the first
, depending on the
argument is not defined, OpenLabs will by default use the expression
or
conservative or non-conservative convection scheme. If the first argument is specified, OpenLabs
will use the user customized convection speed, see Customized convection speed for more details.
The transport equation definition in the resource is as follows:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION:DDT(<VarName>)+CONV(<VarName>)= \
DIFF(<name of the diffusion coefficient >)+ \
SOURCE(<Name of the source term1>+…)
In order to solve the transport equation, a number of properties/attributes need to be defined (e.g.
convective scheme, initial and boundary conditions, relaxation…). In the following table, a list of
possible properties/attributes is shown. If the attribute is not added,
the default value is
automatically set.
Property
Convective scheme:
- Non-conservative form of first order upwind
- Conservative form of first order upwind
- Conservative form of high order upwind
Initial value:
- Constant value for the whole field
- Expression to initialize the field
Upper and lower clipping of the field:
- Clip the field to a minimum value
- Clip the field to a maximum value
Relaxation type:
- No relaxation
- Constant relaxation factor
- Limit the variation of the variable
- Limit upper and/or lower variation of the variable (same as
previous case but being able to limit different upper and lower
variations):
l Limit the upper variation
l Limit the lower variation
Keyword
->Convective_Scheme:
UpwindFirstOrderNonConservative
->Convective_
Scheme:UpwindFirstOrderConservative
(default)
->Convective_Scheme:
UpwindHighOrderConservative
->INITIAL_VALUE: <value> (default:
0.0)
->InitializeTo: <name of initialization
expression>
->LowerLimit: <value> (default: -
1e30)
->UpperLimit: <value> (default: 1e30)
Nothing should be added
->ConstantRelaxFactor: <value>
(default:1.0)
->LimitVariation: <value>
(default:0.95, corresponds to 5%)
->UpperRelaxationFactor: <value>
(1.05, corresponds to 5%)
->LowerRelaxationFactor: <value>
(0.95, corresponds to 5%)
Property
Boundary conditions at solids:
Boundary conditions at inlets:
Boundary conditions at outlets:
Boundary conditions at externals:
Keyword
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
or
->UseCustomBC: <name of bc
expression>, ALLSOLIDS
or
->UseCustomWallFunction: <name of
wall function>, <Patch num/name>, …
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
or
->UseCustomBC: <name of bc
expression>, ALLINLETS
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
or
->UseCustomBC: <name of bc
expression>, ALLOUTLETS
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
In case that the equation added is for the turbulent kinetic
energy, the term
needs to be added
->AddTwoThirdsRhoK (this should
not be used unless a
turbulent kinetic energy equation is
being added)
The following is the complete structure of a transport equation definition with its attributes:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION: DDT(<VarName>)+CONV(<VarName>)= \
DIFF(<name of the diffusion coefficient >)+ \
SOURCE(<Name of the source term1>+…)
->Convective_Scheme: <Convection scheme keyword>
->InitializeTo: <Name of expression to initialize the field>
or
->INITIAL_VALUE: <value>
->LimitVariation: <value between 0 and 1> (Optional)
or
->ConstantRelaxFactor: < value between 0 and 1> (Optional)
or
->UpperRelaxationFactor: < value larger than 1> (Optional)
->LowerRelaxationFactor: < value between 0 and 1> (Optional)
->LowerLimit: <value> (Optional)
->UpperLimit: <value> (Optional)
->UseCustomBC: <name of solid BC expression>, <Patch num>,<Patch num>,…
->UseCustomWallFunction: <name of wall function>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of inlet BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of outlet BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of external BC expression>, <Patch num>,<Patch num>,…
->AddTwoThirdsRhoK (Optional only in case that a turbulent kinetic energy equation is being
added)
Conservative vs. non-conservative convection schemes
A transient-convection-diffusion-source transport equation can be written, in a conservative form.
For this kind of equations, two numerical convection schemes can be chosen in OpenLabs:
l Conservative first order upwind: UpwindFirstOrderConservative
l Conservative high order upwind: UpwindHighOrderConservative
The conservative form of the transport equation is highly recommended, especially when large
density gradients are expected.
The UpwindHighOrderConservative is significantly more computationally costly.
In some particular cases, when the transport equations are source term dominated and very stiff
(e.g. k and epsilon equations), the non-conservative form can be used to gain in robustness. The
equation in the non-conservative form can be written as follows:
In this case, one numerical convection scheme can be chosen in OpenLabs:
l Non-conservative first order upwind: UpwindFirstOrderNonConservative
Warning: In case the non-conservative scheme is selected, the source terms and diffusion coefficients
formulas must be written accordingly (division by density).
Boundary conditions
To specify the boundaries where a certain boundary condition is applied, two options are
possible:
l In case all SOLIDS, INLETS or OUTLETS have the same boundary condition (e.g. the
epsilon at the wall), the keywords ALLSOLIDS, ALLINLETS or ALLOUTLETS can be
used.
l In case that each SOLID (INLET, OUTLET or EXTERNAL) has a different boundary
condition (e.g. a case with different variable value at different inlet), the corresponding <patch
number> or <group name> is required, which can be obtained in the project analysis results.
An example is shown below, where BC_periodic and BC_inlet are the group names that
defined in the GUI by the user. The numbers in the square brackets are the patch numbers that
belong to the group. The physical variables that are imposed to the boundaries in the GUI are
listed after "->Imposed_Physical_Variables:".
# This is ana file
…
=>INTERNAL_BOUNDARY_CONDITIONS
@ InternalBC_PERIODIC: BC_periodic[0,1]
@ InternalBC_INL: BC_inlet [2]
->Imposed_Physical_Variables: "Vr", "Vt", "Vz", "NormalizedProgressVariable"
@ InternalBC_OUT: BC_outlet [3]
->Imposed_Physical_Variables: "StaticPressure"
A group name should never be defined as a number in the GUI, e.g. a group of boundaries cannot be
named as "0". Otherwise it will be mistaken as the patch number.
For the boundaries where no customized boundary conditions are applied, the Neumann (null
gradient of the variable) boundary condition will be automatically imposed.
Diffusion transport equation: PDE
The parabolic PDEs, such as diffusion equations, have the following form.
For parabolic PDEs, the explicit schemes are generally unsuitable because their region of absolute
stability is small. Implicit scheme with a generalized Gauss-Seidel method is available for solving
diffusion equation. It is set as the default method for the transient-diffusion-source PDEs added in
OpenLabs™. The transient-diffusion-source PDE of scalar ϕ is formulated as,
where, R is a function of ϕ and its spatial derivatives. The Crank-Nicolson scheme can be
obtained by applying trapezoidal rule to the time integration,
A general implicit scheme can be achieved by introducing a blending factor γ,
Finally, the solution is updated by,
The general implicit scheme is a combination of the explicit forward Euler scheme (corresponding
to γ=0) and the implicit backward Euler scheme (corresponding to γ=1). And only when γ=0.5
(Crank-Nicolson scheme), it is second-order in time accurate. The value of γ is set using the
keyword -> IMPLICIT_BLENDING. The over-relaxation factor
is set using the keyword -
>IMPLICIT_SOR. The default value for the over-relaxation factor is 1 but a range of values
between 0 and 2 can be used for this parameter. A higher relaxation factor (>1) will accelerate the
convergence of a slow-converging process, it helps to reach a super-linear convergence for some
problems but may fail for the others (divergence).
Alternatively,
>ForceExplicitRungeKutta.
the explicit Runge- Kutta method is still available by using the keyword -
The transport equation definition in the resource file is as follows:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION: DDT(<VarName>)= DIFF(<name of the diffusion coefficient >)+ SOURCE
(<Name of the source term1>+…)
->InitializeTo: <Name of expression to initialize the field>
->IMPLICIT_SOR: <value>
->IMPLICIT_BLENDING: <value>
->UseCustomBC: <name of solid BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of inlet BC expression>, <Patch num>,<Patch num>,…
->UseCustomBC: <name of outlet BC expression>, <Patch num>,<Patch num>,…
It is not obliged to have DDT term for diffusion PDEs in case of the absence, the attribute "->
VARIABLE_NAME:" has to added with given name. In the absence of transient term in the
scalar PDE following structure can be used:
=>EQUATIONS
@ PDE: < Name of the transport equation >
->EXPRESSION: 0= DIFF(<name of the diffusion coefficient >)+ SOURCE(<Name of the
source term1>+…)
->VARIABLE_NAME: GP1
The properties/attributes need to be defined for diffusion PDEs are listed below.
Property
Initial value:
- Constant value for the whole field (Default)
- Expression to initialize the field
Upper and lower clipping of the field:
- Clip the field to a minimum value
- Clip the field to a maximum value
Keyword
->INITIAL_VALUE: <value>
(default value: 0.0)
->InitializeTo: <name of initialization
expression>
->LowerLimit: <value> (default: -
1e30)
->UpperLimit: <value> (default:
1e30)
Property
Keyword
Relaxation type when using the explicit Runge-Kutta method:
- No relaxation (Default)
- Constant relaxation factor
- Limit the variation of the variable
- Limit upper and/or lower variation of the variable (same as
previous case but being able to limit different upper and lower
variations):
l Limit the upper variation
l Limit the lower variation
Relaxation type when using the implicit method:
- blending factor γ in the implicit scheme
- the over-relaxation factor used to update the solution
Boundary conditions at solids:
Boundary conditions at inlets:
Boundary conditions at outlets:
Boundary conditions at externals:
498
FINE™/Open with OpenLabs™ 7.2 User Guide
Nothing should be added
->ConstantRelaxFactor: <value>
(e.g. 0.5)
->LimitVariation: <value> (e.g. 0.95,
corresponds to 5%)
->UpperRelaxationFactor: <value>
(e.g. 1.05, corresponds to 5%)
->LowerRelaxationFactor: <value>
(e.g. 0.95, corresponds to 5%)
-> IMPLICIT_BLENDING (Default:
0.5)
->->IMPLICIT_SOR (Default: 1)
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
or
->UseCustomBC: <name of bc
expression>, ALLSOLIDS
or
->UseCustomWallFunction: <name
of wall function>, <Patch
num/name>, …
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
or
->UseCustomBC: <name of bc
expression>, ALLINLETS
->UseCustomBC: <name of bc
expression>, <Patch num/name>, …
or
->UseCustomBC: <name of bc
expression>, ALLOUTLETS
16.5.7 Customized convection speeds
The user can customize convection speeds for external PDEs. The section defining the convection
speeds must start with the line "=>CUSTOM_CONVECTION_SPEEDS".
To define convection speeds for external PDEs, each convection speed has to be written by
giving
after
the
name
"@CUSTOMCONVSPEED:".
expression.
should
given
name
The
be
to
=>CUSTOM_CONVECTION_SPEEDS:
@ CUSTOMCONVSPEED: <expression name of the convection speed>
->EXPRESSION: <mathematical expression of the convection speed>
Note, the mathematical expression of the convection speed must be a vector expression, for
example, Density*[Vx,Vy,Vz] or Density*Velocity, where Velocity is a vector.
If the user defines a customized convection speed, the defined customized convection speed must
be used at least in one of the external PDEs.
16.5.8 Customized boundary conditions
The user can customize boundary conditions or wall functions. The section must start with the
line "=>CUSTOM_BOUNDARY_CONDITIONS".
Customized boundary conditions
Add boundary conditions for external PDEs
To add boundary conditions for external PDEs, each expression has to be written by giving a
name to the expression, writing the expression and defining the type (Dirichlet by default). The
name should be the one that is defined in the PDE section, after " ->UseCustomBC:". This
boundary condition will be applied to the patches or the group defined in the PDE section.
@CUSTOMIZED_BOUNDARY_CONDITION: <Name of boundary condition expression>
->EXPRESSION: <mathematical expression of the boundary condition>
->TypeBC: Dirichlet
To define the type of the boundary condition, the following keywords can be used:
l Dirichlet: the value of the variable is specified.
l Neumann: the gradient in the normal direction of the variable is specified.
l Robin: the linear relation of the variable and its gradient in the normal direction is specified.
In case of Robin type, the expression of the boundary condition must be written as follows:
->EXPRESSION: ROBIN_DERIV+ROBIN_COEF(a)=ROBIN_FUNC(b)
where, both a and b can be an expression.
l RiemannInvariants: the value of the variable is specified.
where λ is the eigenvalue of the local one dimensional flow equations in the direction that is
perpendicular to the boundary;
is the value of the variable in the first inner cell.
Modify internal boundary conditions
Internal boundary conditions can be modified in two ways:
l Modify the existing boundary condition entries that can be obtained from the project analysis
results. The keywords "->ExistingBC:" must be used to specify the physical entries and the
groups/patches. The boundaries can be specified by group name or patch number. If the
boundary condition is imposed to multiple groups/patches, the group names/patch numbers
should be separated by comma.
@ CUSTOMIZED_BOUNDARY_CONDITION: VzInlet
->EXPRESSION: IF(rCoord>=0.0125) 0 ELSE 1
->ExistingBC: "Vz" , BC_inlet
or
->ExistingBC: "Vz" , 2
When customizing internal boundary conditions, the following limitations are applied:
l Cannot customize the radius when the outlet boundary condition is defined by Pressure
Imposed - Radial Equilibrium.
l Cannot customize the initial pressure when the outlet boundary condition is defined by Mass
Flow Imposed.
l Cannot customize Backflow Control at outlets.
l Cannot customize the Von Karman constant κ, the Bo constant, the equivalent roughness
height k0 and the height of the zero displacement plane d0 used for the wall functions.
l Cannot change the type of the boundary condition. For example, the user cannot change the
inlet boundary condition from Static Quantities Imposed to Total Quantities Imposed in
OpenLabs™.
l Modify the boundary conditions of
the existing PDE variables. The keywords " -
>ExistingVariable:" must be used to specify the PDE variable and the groups/patches. The
boundaries can be specified by group name or patch number. If the boundary condition is
imposed to multiple groups/patches, the group names/patch numbers should be separated by
comma.
#define the inlet BC for multi-species
@ CUSTOMIZED_BOUNDARY_CONDITION: Y1
->EXPRESSION: 0
->ExistingVariable: Yspec1, Block_1_group_0
or
->ExistingVariable: Yspec1, 2
The keyword "->ExistingVariable:" is used to customize the boundary conditions of the additional
scalar equations, for example the multi-species equation. It cannot be used to customize the boundary
. For the temperature and enthalpy defect, only
,
conditions of the PDE variables
the wall boundary conditions with heat flux imposed or adiabatic can be modified.
and
, ρ,
Customized wall functions
The viscous effects are important in the thin near-wall sublayer. To obtain an accurate resolution
of this layer, the most reliable way is to use a fine grid and a low-Re-number model. In industrial
applications, the low-Re-number models can be very expensive and the high-Re-number models
with wall functions are usually used. Wall functions reproduce the effects of near-wall turbulence
on flow and thermal development. For the theory of the internal wall functions, please refer to the
Modeling the flow near the wall section of the Theoretical Manual.
Add new wall functions for external PDEs
To add wall functions for external PDEs, each wall function has to be written by giving a name to
the expression. The name should be the one that is defined in the PDE section, after " -
>UseCustomWallFunction:". This boundary condition will be applied to the patches or the
group defined in the PDE section.
=>CUSTOM_BOUNDARY_CONDITIONS
@CUSTOM_WALL_FUNCTION: <name of the external wall function>
->EXPRESSION: <expression of the wall function>
Modify internal wall functions
Internal wall functions can be modified in three ways:
l Using the identical name as that in the project analysis results. In this case, the customized wall
function will be applied to all the original related patches.
=>CUSTOM_BOUNDARY_CONDITIONS
@CUSTOM_WALL_FUNCTION: <name of the internal wall function>
->EXPRESSION: <expression of the wall function>
l Using the keywords "->ExistingWallFunction:". In this case, the customized wall function
will be applied to the specified patches among the original patches,
=>CUSTOM_BOUNDARY_CONDITIONS
@CUSTOM_WALL_FUNCTION: <name of the wall function>
->EXPRESSION: <expression of the wall function>
->ExistingWallFunction: <name of the internal wall function>, <patches>
l Using the keyword "->ExistingVariable:". In this case, the customized wall function will be
applied to the specified variable and patches,
=>CUSTOM_BOUNDARY_CONDITIONS
@CUSTOM_WALL_FUNCTION: <name of the wall function>
->EXPRESSION: <expression of the wall function>
->ExistingVariable: <name of the internal variable>, <patches>
16.5.9 Diffusion Coefficients
The section to add diffusion coefficients in an external PDE or modify the diffusion coefficient of
an internal PDE must start with the line "=>ALGEBRAIC_DIFFUSION_COEFFICIENTS".
l To add diffusion coefficients in an external PDE, each expression must be written by giving a
name to the expression, and writing the formula.
=>ALGEBRAIC_DIFFUSION_COEFFICIENTS
@ ALGDIFFCOEFF: <name of the diffusion coefficient>
->EXPRESSION: <mathematical expression/formula of the diffusion coefficient>
l To modify the diffusion coefficient of an internal PDE, besides the name of the internal
diffusion coefficient and its expression, the name of the internal PDE is also needed. The user
can refer to the project analysis results to get the name of the internal PDE. Then, the name of
the PDE could be specified in two alternative ways: by the attribute line with the keyword "-
>AddToExistingPde:", or by parentheses after the keyword " EXPRESSION ", see the
following example
=>ALGEBRAIC_DIFFUSION_COEFFICIENTS
@ ALGDIFFCOEFF: <Name of internal diffusion coefficient>
->EXPRESSION(<Name of the internal PDE>): <mathematical expression of the diffusion
coefficient>
…
or
@ ALGDIFFCOEFF: <Name of internal diffusion coefficient>
->EXPRESSION: <mathematical expression of the diffusion coefficient>
->AddToExistingPde: <Name of the internal PDE>
…
In case that several PDEs have the same diffusion coefficient:
@ ALGDIFFCOEFF: <Name of internal diffusion coefficient>
->EXPRESSION: <mathematical expression of the diffusion coefficient>
->AddToExistingPde: <Name of the internal PDE1>, <Name of the internal PDE2>, …
16.5.10 Initial solution
The section to add customized initial solutions must start with the line " =>INITIAL_
PROFILES".
l When an external PDE is added and the external variable needs to be initialized by an
expression (keyword "->InitializeTo" as explained in Convection-diffusion-source transport
equations: PDE ), the expression must be defined in this section. Each expression must be
written by giving a name to the expression, and writing the formula.
=>INITIAL_PROFILES
@ INITIAL_FIELD: <Name of expression to initialize the field>
->EXPRESSION: <mathematical expression/formula >
l In order to modify the initialization of an internal variable, the keyword "->ExistingField:"
must be used. The name of the internal variables can be found in the project analysis results. It
is possible to impose initial solution for cylindrical velocity vector. In this case, all of three
components must be imposed, see the example below.
@ INITIAL_FIELD: VelocityRInit
->EXPRESSION: 0.0
->ExistingField: VrCylinder
@ INITIAL_FIELD: VelocityThetaInit
->EXPRESSION: 0.0
->ExistingField: VtCylinder
@ INITIAL_FIELD: VelocityAInit
->EXPRESSION: IF(rCoord>=0.0125) 1.0 ELSE 0.0
->ExistingField: VaCylinder
16.5.11 Source Terms
The section to add source terms in a PDE must start with the line "=>SOURCETERMS".
Each source term object has to start with the keyword " @ SOURCE: ". There are three
possibilities to define a source term, which includes adding external source terms for external
PDEs, adding external source terms for internal PDEs, modifying internal source terms.
l To add external source terms for external PDEs, each expression has to be written by giving a
name to the expression (the name also appears inside the PDE expression), and writing the
formula. The source terms of each external PDE should be defined individually. That means
for one source term name there is only one expression, as well as one PDE to correspond to.
=>SOURCETERMS
@ SOURCE: <Name of external source term >
->EXPRESSION: <mathematical expression/formula of the source term>
->AddToViscous: NO (Optional)
->AddToBoundaryOnly: <Patch num/name>, … (Optional)
l To add external source terms for internal PDEs, besides the name of expression and the
formula, the name of the internal PDE, which the source terms is added to, is also needed. The
user can refer to the project analysis results to get the name of the internal PDE. Then, the
name of the PDE could be specified in two alternative ways: by the attribute line with the
keyword "->AddToExistingPde:", or by parentheses after the keyword "EXPRESSION",
see the following example.
@ SOURCE: <Name of external source term>
->EXPRESSION: <mathematical expression/formula of the source term >
->AddToExistingPde: <Name of the internal PDE>
->AddToViscous: NO (Optional)
->AddToBoundaryOnly: <Patch num/name>, … (Optional)
or
->EXPRESSION(<Name of the internal PDE>): <mathematical expression of the source
term>
->AddToViscous: NO (Optional)
->AddToBoundaryOnly: <Patch num/name>, … (Optional)
l To modify a source term that already exists in the project, both the name of the source term to
be modified and the name of the PDE which the source term is affecting need to be known.
The names should be the same as that in the project analysis results. Since for the internal
source terms of FINE™/Open, a name could correspond to more than one PDE and thus one
object of source term could have more than one expression. For example, the internal source
term ProductionDissipationKE affects the PDEs: TurbulentKineticEnergyEquation and
DissipationOfTurbulentKineticEnergyEquation. Then, the following structure must be written.
=>SOURCETERMS
@ SOURCE: <Name of internal source term>
->EXPRESSION(<Name of the internal PDE 1>): <mathematical expression of the source
term 1>
->EXPRESSION(<Name of the internal PDE 2>): <mathematical expression of the source
term 2>
…
The Jacobian of the source term can be provided using the keyword -> Jacobian followed by
the math expression.
->Jacobian:<math expression>
It is not mandatory to provide the Jacobian of the source term but to have the implicit
discretized source term in diffusion PDE, the Jacobian of the source term should be provided.
The attribute line of source terms with the keyword "->AddToViscous:" is optional. In the 4
stage Runge-Kutta solution algorithm, the source terms can be updated at each stage (added to the
convective residual) or at selected stages (added to the viscous residual). The expert parameter
spc_iCalcVFluxes_ can be used to control at which Runge-Kutta stages, the viscous residual is
updated. When a source term is added by means of OpenLabs, the default option is to update the
source at the same stages as the viscous terms. However, in the case that user wishs to update the
source at each Runge-Kutta stage, the line "->AddToViscous: NO" has to be added.
The attribute line of source terms with the keyword " ->AddToBoundaryOnly:" is optional.
When this attribute line exists, the source term will be added only along the specified boundaries.
To specify the boundaries, the keywords ALLSOLIDS, ALLINLETS and ALLOUTLETS
can be used.
16.5.12 Customized Fluid Property
The fluid properties (equation of state (EOS) and transport properties) can be customized. The
section must start with the line "=>CUSTOM_FLUID_PROPERTIES''.
Customized EOS
All the state variables of the fluid can be customized. The section to customize the EOS must be
added in the section " =>CUSTOM_ FLUID_ PROPERTIES " and must
start with
" @EQUATION_OF_STATE:". A name of the EOS has to be provided by the user. The
keyword "->UseDatabase" is used in case that the existing EOS needs to be customized. This
keyword can be omitted when creating a new EOS. To change the state relation, the user is
required to provide the name of the relation using the keyword "->EOS_RELATION" followed
by the keyword "->EXPRESSION" to define the relation. The name of the relation must be the
same as that given in the project analysis results. See the structure below.
@ EQUATION_OF_STATE: <name of the EOS>
->UseDatabase: <name of the internal EOS> #optional
->EOS_RELATION: <relation name1>
->EXPRESSION: <math expression>
->EOS_RELATION: <relation name2>
->EXPRESSION: <math expression>
...
The following basic EOS types have been defined and can be used:
l Ideal gas: The EOS of an ideal gas follows the perfect gas law with a constant specific heat
capacity. This EOS will also be adapted corresponding to the "Perfect gas" settings in the
FINE™/Open GUI. The following EOS are implemented based on the ideal gas EOS:
l For premixed combustion: Combustion BML. In this EOS, the density depends on the
normalized progress variable. The fluid type will be automatically adapted to "Reactive
Fluid" settings in the FINE™/Open GUI when the premixed combustion model
is
activated.
l For non-premixed/partial-premixed combustion: Combustion Tables. In this EOS, the
thermal quantities are coming from a table. The fluid type will be automatically set to
"Reactive Fluid" settings in the FINE™/Open GUI when non- premixed or partially-
premixed combustion model is activated.
l Real gas: The EOS of a real gas follows the perfect gas law with the specific heat capacity as
a function of temperature. This EOS will be adapted when "Real gas" in the FINE™/Open
GUI is selected.
l Incompressible fluid: The EOS of an incompressible fluid assumes a constant density and a
. This EOS will be adapted corresponding to the settings in the FINE™/Open
constant
GUI:
l Barotropic law: dedicated to cavitation model type 1
l Full Cavitation: dedicated to cavitation model type 2
l VOF: dedicated to VOF model
l Condensable gas: In this EOS, the thermodynamic quantities depend on thermodynamic
table.The fluid type is set to "Condensable gas" in the FINE™/Open GUI.
The fluid type defined in OpenLabs should be the same or the upper level as the one defined in the
FINE™/Open GUI. For example, when Combustion BML is used in the computation, the user can
use " - >UseDatabase: Ideal gas", but cannot use " - >UseDatabase: Incompressible fluid" in
OpenLabs™
If the user wants to define a new EOS which is not available in the FINE™/Open, the user has to
define all the necessary state relations required to define the EOS.
The following limitations apply to the customized EOS:
l The customized EOS is not compatible with turbo initial solution.
l The customized SoundSpeed is not compatible with Mach number imposed External boundary
condition (Riemann BC).
l The customized EOS is not compatible with FSI (fluid structure interaction).
l The customized gas constant RGas is not compatible with Lagrangian.
l The customized RGas/SoundSpeed/Temperature based on "Real gas" framework is not
compatible with CPUBooster.
l The customized EOS is not compatible with R/S connections.
l The visualization of customized Pt, Tt is not compatible with the expert parameter out_
derQntFromNode_ = 0.
Guidelines on how to customize the EOS
The equation of state (EOS) is used to close the system of Navier- Stokes equations. Five
independent variables, including 2 thermodynamic variables & 3 velocity components, are solved
through RANS. The other thermodynamic variables are computed from the EOS. There are
various ways to compute the thermodynamic variables, either by thermodynamic EOS or by
. In more general situation, it could
caloric EOS, for example,
or
be dependent on additional scalars, such as the mixture fraction. To customize the EOS in the
solver, the user is strongly recommended to follow the following guidelines:
(1) Always select the closest fluid model as database. For example, a mixture behaves as ideal
gas, the ideal gas framework is recommended as the database. Then, the user could refer to the
detailed ana file, to decide which relations need to be modified.
(2) Decide to use expressions or tabulation. When the EOS is quite complex, the computational
cost may not be acceptable because the EOS is calculated at each flow iteration. In this case, the
user can firstly tabulate the EOS into several profiles. Then the EOS can be calculated by the
interpolation of those profiles at each flow iteration. The tabulation of the EOS works with the
same behavior as the fluid type condensable gas. For the tabulation of the EOS, please refer to
Discrete Expression section on how to define a discrete expression by an expression.
(3) The EOS relations should be given by using the independent variables, which can be found in
the ana file. For example, the following is the EOS of a premixed combustion model:
and
,
where Tu is the temperature of the unburned mixture, Tad is the adiabatic temperature of the burnt
mixture. The "ProgVariable" c is resolved from a PDE and the "CombTemp" T is dependent on
the variable c. In this case, the user should define the density as a function of the independent
variable (variable resolved from a PDE) c rather than using the function "CombTemp" T itself.
Use of dependent variables (derived from independent variables) may lead to a wrong solution or
divergence.
The resource file below demonstrates how to use the independent variables when defining the
density relation for a premixed combustion model.
The correct approach, where ProgVariable is an independent variable:
=>CUSTOM_FLUID_PROPERTIES
@EQUATION_OF_STATE: MyEOS
->EOS_RELATION: Density
->EXPRESSION: StaticPressure/ phy_RGaz/ \
(1-ProgVariable)*unburnedTemp+ProgVariable*premixedFlameTemp
The incorrect approach, where CombTemp is a dependent variable:
=>CUSTOM_FLUID_PROPERTIES
@EQUATION_OF_STATE: MyEOS
->EOS_RELATION: Density
->EXPRESSION: StaticPressure/ phy_RGaz/CombTemp
(4) Since the independent variables are different according to whether the project uses
preconditioning or not, the EOS are usually formulated in different way for the case with/without
preconditioning.
- Without preconditioning, (ρ, p) are the independent variables. The pressure relation should be
given in terms of (ρ, E ) (which are resolved from the continuity & energy equations) and/or
additional independent variables. The other thermodynamic variables, T, H, E, cp, ..., should be
given in terms of the independent variables, i.e. ρ, p and the additional independent variables.
- With preconditioning, (p, T) are the independent variables. The temperature relation should be
given in terms of (p, H ) (which are resolved from the continuity & energy equations) and/or
additional independent variables. The other thermodynamic variables, ρ, E, H, cp, ..., should be
given in terms of the independent variables, i.e. p, T, and the additional independent variables.
TABLE 16.1 List of the dependent and independent thermodynamic variables
Without Preconditioning
With Preconditioning
Incompressible
Compressible
Independent variables Density (ρ) and
Pressure (p) and
Pressure (p) and
Pressure (p)
Temperature (T)
Temperature (T)
Without Preconditioning
With Preconditioning
Incompressible
Dependent Variables
Temperature (T)
Energy (E)
Enthalpy (H)
Compressible
Density (ρ)
Energy (E)
Density (ρ)
Energy (E)
Enthalpy (H)
Enthalpy (H)
Heat Capacity (cp) and Specific
heat ratio (γ)
Heat Capacity (cp),
Gamma (γ)
Speed of Sound (c)
Speed of Sound (c)
Independent Variable
relation
Pressure p=f(E) and Density =f
(p,T) ρ
Temperature T=f(H)
Heat Capacity (cp
and cv)
Speed of Sound (c)
Temperature T=f
(E)
(5) Since the EOS is also used for initialization, applying boundary conditions, visualization and
some numerical procedures, the relation of independent variables are also needed. To formulate
the independent variables, the user certainly may use some dependent variables.
(6) For the thermodynamic quantities like static energy, enthalpy and other quantities, the values
computed in CFView™ are not consistent with the values from the FINE™/Open solver. It is
advised to redefine these quantities in OpenLabs and use them in CFView™.
(7) The consistency of the EOS should be maintained by the user. For example, given the energy
function E=f(p,ρ), the pressure function has to be the inverse function p=f-1 (E,ρ). The non-
consistent relations will result in a wrong solution and divergence. Therefore, in case that the user
modifies one relation from the database, the user should check all other relations for consistency
(check in the ana file).
Customized transport properties
All the transport properties of the fluid (e.g., Viscosity and Conductivity) can be customized. The
section to customize the transport properties must be added in the section of " =>CUSTOM_
FLUID_PROPERTIES".
l To add a new transport property: it must start with "@TRANSP_PROPERTY:". Then, the
name of the transport property has to be given by the user and the expression of the transport
property has to be defined. See the structure below.
@TRANSP_PROPERTY: <transport property name1>
->EXPRESSION: <math expression>
...
The new transport property can be outputted for post-processing, see Outputs by OpenLabs.
l To modify an internal transport property: it must start with " @TRANSP_PROPERTY:".
The name of the transport property has to be given by the user and the expression of the
transport property has to be defined. Then, the keywords "->ExistingCalculator:" has to be
used and the name of the internal property calculator must be given. The name of the internal
property calculator must be the same as that in the detailed project analysis results. See the
structure below.
@TRANSP_PROPERTY: <transport property name1>
->EXPRESSION: <math expression>
->ExistingCalculator: <name of the internal transport property>
...
16.5.13 Auxiliary Definitions
Auxiliary definitions can be used to simplify the writing of long formulas, and/or to re-use parts of
a formula. For example, the following expression
can be written by adding an auxiliary definition (S) in the following way:
The section to add auxiliary definitions must start with the line "=>AUXTERMS". Then, each
auxiliary definition must be written by giving a name and expression.
The auxiliary expressions can be used anywhere in the resource (e.g. to define a source term) by
simply writing the given name. Auxiliary expressions can be useful to simplify the way to write a
very long equation.
=> AUXTERMS
@ AUXTERM: < name of auxiliary definition 1 >
-> EXPRESSION: <mathematical expression/formula 1>
@ AUXTERM: < name of auxiliary definition 2 >
-> EXPRESSION: <mathematical expression/formula 2>
….
Alternatively, a simplified nomenclature is also available:
=> AUXTERMS
@ < name of auxiliary definition 1 > = <mathematical expression/formula 1>
@ < name of auxiliary definition 2 > = <mathematical expression/formula 2>
….
16.5.14 Global Quantity
Global quantities can be defined in the section "=>GLOBAL_QUANTITIES:".
For the moment, the global quantity can only be an integral (INTEG1D, INTEG2D and
INTEG3D) or a variable value on a control point. Other type of global quantity is not available.
To define a global quantity, it should start with "@GLOBAL_QUANTITY:". The name of the
global quantity has to be given by the user and the expression of the global quantity has to be
defined (can only be an integral or a variable value on a control point).
=>GLOBAL_QUANTITIES:
@ GLOBAL_QUANTITY: <name>
->Expression: INTEG1D(<expression>, <variable name>, <min>, <max>)
->ExportHistoryToFile: <file name> (optional)
Alternatively, the global quantity can be defined by:
@ <name> =INTEG1D(<expression>, <variable name>, <min>, <max>)
->ExportHistoryToFile: <file name> (optional)
The attribute ExportHistoryToFile is optional and used to output the value of the global quantity
into a file with respect to the output settings.
In case the integration region involves several blocks, OpenLabs has to be activated in each involved
block and exactly the same definition (same name and same expression) should be used for each
block. The example given below in the table illustrates the usage of integrals in multi-block.
In case the global quantity is defined in one block but applied in another block, OpenLabs has to be
activated in both blocks. The global quantity is given with the complete definition in the block where
it is defined, whereas given with only its name and the keywords "EXTERN" in the block where it is
applied. In the example given below in table, illustrates the use of keyword "EXTERN" in multi-
block.
Block1 Resource file
Block2 Resource file
=>GLOBAL_QUANTITIES
=>GLOBAL_QUANTITIES
@massflow_in=INTEG2D(Vx*Density,2)
@massflow_in=INTEG2D(Vx*Density,2)
@m_0To1=INTEG2D(Vy*Density,connection_1)
@m_1To0=INTEG2D(Vy*Density,connection_1)
@ m_1To0:EXTERN
=>EQUATIONS
@NONDIFFEXPR: massBalance
->EXPRESSION:mExc=m_0To1+ m_1To0
16.5.15 Special Information
A section to introduce special information can be added. At present time, this section is used to set
a wall-function turbulence model. The section to add special information must start with the line
"=> ADDITIONAL_INFORMATION".
For the case a k-epsilon model with wall function is to be added, the following line must be
included in this section:
=> ADDITIONAL_INFORMATION
@ K-E_TURBMODEL_WITH_WALLFUNC: <Name of k variable > , <Name of epsilon
variable >
The K-E_TURBMODEL_WITH_WALLFUNC option is only used in case that the turbulence
model is completely added from a Laminar Navier-Stokes simulation. For the high Reynolds number
models existing in FINE™/Open, the wall functions are already built-in and additional information
should not be added.
In case a Rough wall-type is to be used, the following procedure can be used (this is temporal and
it will be improved in the future):
l In the FINE™/Open GUI, set Flow Model to "Turbulent Navier-Stokes" and Turbulence
model to "k-epsilon (Extended Wall Function)" in the Physical Configuration / Flow Model
page.
l In the Boundary conditions / Boundary conditions page under the SOLID tab,
the
possibility to select a "Smooth" or a "Rough" wall-type is available. Select the "Rough" type
and adapt the corresponding parameters.
l Go back to the Physical Configuration / Flow Model page, select the desired choice, for
example, "Laminar Navier-Stokes". In this case, the option for wall-type disappears in the
Boundary conditions / Boundary conditions page under the SOLID tab. However, the
adapted parameters for the "Rough" wall have been stored.
CHAPTER 17.
FILE FORMATS
This appendix describes the files used by FINE™ and the flow solver. It is divided into two parts. The
first one gives the file format information needed to use FINE™/Open with OpenLabs™, while the
second one describes the format of the files used and produced by the flow solver. As FINE™/Open
with OpenLabs™ is intended to handle the file treatment for the user, knowing the exact format of all
the files used in a simulation process is not required. This Appendix is therefore written for advanced
users.
In the following description, it is assumed that all the files are related to a generic project called
'project'. The chapter is divided in six sections:
In this section
17.1 Files Produced by HEXPRESS™
17.2 Files Produced by FINE™/Open with OpenLabs™
17.3 Files Produced by the FINE™/Open Solver
17.4 Input Files Used by the FINE™/Open GUI
17.5 Input Files Used by the FINE™/Open solver
17.6 Configuration & Resource Files Used by the FINE™/Open GUI
516
516
518
522
525
526
17.1
FILES PRODUCED BY HEXPRESS™
This section describes the files produced by the grid generator HEXPRESS™ and used by
FINE™/Open with OpenLabs™:
l project.igg contains all
relevant parameters about
the grid generation process
in
HEXPRESS™.
l project.dom contains the computational domain definition (geometry and topology).
l project.hex contains the mesh and its connection to the computational domain.
l project.bcs contains boundary conditions information. As described in Boundary Conditions
chapter, the settings of the boundary condition type is performed in HEXPRESS™ while the
physical boundary condition parameters are set in FINE™/Open with OpenLabs™. The
settings of HEXPRESS™ are stored in the file project.bcs. This file is used by FINE™/Open
with OpenLabs™ to initialize the boundary condition types for each patch. It is updated each
time the boundary condition type is changed in HEXPRESS™.
l project.fnmb contains information on FNMB and/or the rotor-stator interface.
For more details about these files, the user is referred to the HEXPRESS™ user manual.
17.2
FILES PRODUCED BY FINE™/OPEN WITH
OPENLABS™
This section describes the files produced and used by FINE™/Open with OpenLabs™ (or used
by the flow solver
launched from FINE™/Open with OpenLabs™). Please note that
FINE™/Open with OpenLabs™ acts as a file manager between different software systems.
Therefore, it is important that the read, write and execute permissions are set properly for all the
files and directories used by FINE™/Open with OpenLabs™.
Manual modification of these files is not supported since it may corrupt the file or provide incorrect
results. Such a modification should only be done on explicit advice of the NUMECA support team.
The Project File: project.iec
This file contains all the information related to the project. It is used by FINE™/Open with
OpenLabs™ to save and recover all the user settings. This file is subdivided into several blocks.
Each block contains data and/or other subblocks. The beginning of each block is identified by the
key word NI_BEGIN and a name and the end of the block are identified by the key word NI_
END and the name of the block.
File Header
The file always has the following header containing the version number and the project type:
NUMECA_PROJECT_FILE VERSION 5.0
PROJECT_TYPE HEXA
APPLICATION_TYPE OPEN
After the header, 3 lines are used to store the name of the files linked to the project:
GRID_FILE /usr/_open_tutorials/_multielement/_mesh/multielement.igg
TRB_FILE /usr/unknown (irrelevant)
GEOMETRY_FILE /usr/unknown (irrelevant)
These are respectively the mesh, the template and the geometry files. The template and the
geometry files are not used by FINE™/Open with OpenLabs™ and are only there for backward
compatibility reasons.
The Computation Block
The project file contains the settings of all
computation block is identified by the following keywords:
the computations defined by the user. Each
NI_BEGIN computation
...
NI_END computation
The computation block contains the following subblocks:
l The Initial Solution and Boundary Condition block contains initial solution parameters and
boundary conditions definition.
l The Blade-to-Blade block contains turbomachinery flow hub/shroud definition.
l The Open Parameters block contains all the parameters for the FINE™/Open solver.
l The Grid Parameters block contains irrelevant information (backward compatibility).
The Computation File: project_computationName.run
When the solver is started, FINE™/Open with OpenLabs™ creates a new directory using the
name of the active computation. A subproject file (".run" extension) containing the settings of the
active computation is saved in this new directory. This file is used as input to the flow solver
FINE™/Open with OpenLabs™ and by the flow visualization system CFView™.
17.3
FILES PRODUCED BY THE FINE™/OPEN
SOLVER
This section describes the files produced and used by the FINE™/Open solver. The flow solver
uses most of the files described above and produces the following files:
The bout file: project_computationName.bout
This binary file contains the flow solution. It is used to restart the flow solver.
The mf file: project_computationName.mf
This ASCII file contains global performance data.
The .wall file: project_computationName.wall
This self-explained ASCII file gives information about forces and torques on the patches/groups
for which the Compute force and torque option is activated on the Boundary Conditions page
in the Solid tab. In the first part of the .wall file, the force and torque on all patches/groups for
which the Compute force and torque option is activated is given. Then, the force and torque on
each individual patch/group for which the Compute force and torque option is activated is
given.
The res file: project_computationName.res
This file contains the residual values for each iteration of a computation. It is continuously
updated during the computation. It is used by the monitor to visualize the convergence history.
The header format for this file is the following:
l line 1: Version line.
l line 2: Number of blocks (1 in FINE™/Open with OpenLabs™ projects)
l line 3: 2D or 3D.
l line 4: NO-K-E, SPL-ALM or K-EPS (5-equation, 6-equation or 7-equation problem)
l line 5: Number of chemistry species (not used, for backward compatibility only).
l line 6: STEADY or UNSTEADY.
l line 7: AERO or TURBO (external or internal flow configuration).
The core file format is the following:
For iteration i=1 to itmax
l 4 numbers (5 numbers for unsteady) corresponding to:
l For steady computations, the total iteration number, the number of adaptations performed,
the number of iterations on current grid and 0.
l For unsteady computations,
the total number of
subiterations, the number of subiterations at the current time step, 0 and the physical time
step
the number of physical time steps,
l 7 numbers corresponding to:
l For internal configurations, 0, Force [Y], Force [X],
irrelevant number, pressure ratio
between inlet and outlet, Mass flow at inlet, Mass flow at outlet.
l For external flow configurations, Lift, Drag, Moment, 0, 0, 0, 0
l Finally, first the maximum and then the RMS residual for the mass equation, the 3 momentum
components, the energy equation, the turbulent variables
or k and ε.
The log & std files: project_computationName.log (.std)
These ASCII files contain all the information related to the current computation. It contains a
summary of the computation variables as well as any warnings and/or error messages. If the flow
solver encounters a problem, this is described in the log file. This file is used for support purposes
only. When a problem appears please send this file together with a detailed problem description to
our local support office. The log file is written directly by the FINE™/Open solver, whereas the
std file is written through the Task Manager when launching the flow solver from the
FINE™/Open GUI. Both files have the same content.
For parallel calculations a ".log" file is written for each process with the filename _ p<process_
number>.log. The 0th process contains all output information as given in the serial case. The log files
for the other process only contains a limited subset of the information specific to that process. If
problems are encountered during a parallel computation all ".log" files should be sent to our local
support office.
The cfv file: project_computationName.cfv
This ASCII file contains information for flow field visualization under CFView™. A complete
description of the contents of this file is given in the CFView™ manual.
The ctl_out file: project_computationName.ctl_out
This file is only written if the user has specified output control points on the Computation
control/Outputs page. The file has slightly different formats depending
on if the calculation is steady or unsteady.
Steady Computations
A header is outputted at the beginning of the file. The header contains the coordinates of the
control point and the explanation of the variables which are exported to the ".ctl_out" file. In case
that preconditioning is activated,
the reference quantities used by preconditioning are also
outputted.
Below the header section, each iteration on fine mesh exports a separate line that contains the five
primitive flow variables at the specified location. In the case of turbulent computations, the
, k and ϵ/ω) are also stored. The five primitive flow variables are
relevant turbulent quantities (
depending on the fluid and settings in the computation:
l Incompressible fluid: Pressure, velocity components and temperature. Note, as preconditioning
is used by default for incompressible fluid, the pressure is replaced by the difference between
the pressure and the gauge reference pressure.
l Compressible fluid without preconditioning: Density, velocity components and pressure.
l Compressible fluid with preconditioning: Pressure, velocity components and temperature.
Note, as preconditioning is used, the pressure is replaced by the difference between the
pressure and the gauge reference pressure.
l Condensable fluid without preconditioning: Density, velocity components and total energy.
l Condensable fluid with preconditioning: Pressure, velocity components and total enthalpy.
Note that for parallel calculations only one ctl_out file is written which contains the data for all
control points on all partitions.
Unsteady Computations
In case of unsteady computations, more information is outputted in each iteration. Below the
header section, each physical time step exports a separate line. In unsteady cases, each line
contains the global time step, the physical time, the number of iterations and the five primitive
flow variables at the specified location. In the case of turbulent computations, the relevant
turbulent quantities (
, k and ϵ/ω) are also stored. The order of these variables is the same as
described in the section steady computations above. Data for each point is written on a separate
line.
Note that for parallel calculations only one ctl_out file is written which contains the data for all
control points on all partitions.
The fmperit file: project_computationName.fmperit
This file is written only if the user sets the expert parameter out_wallForcesPerIt_ to 1. The file
has slightly different formats depending on if the computation is steady or unsteady.
Steady Computations
A header is outputted at the beginning of the file. The header contains the explanation of the
variables which are exported to the ".fmperit" file. Below the header section, each iteration on
fine mesh exports a separate line that contains the iteration number, the force along x/y/z direction
and the moment along x/y/z direction.
Unsteady Computations
A header is outputted at the beginning of the file. The header contains the explanation of the
variables which are exported to the ".fmperit" file. Below the header section, each physical time
step exports a separate line that contains the physical time, the time step, the force along x/y/z
direction and the moment along x/y/z direction.
The globalout file: project_computationName.globalout
This file is written only if the computation is unsteady and the user sets the expert parameter out_
globQuantPerIt_ to 1. The file has slightly different formats depending on the flow configuration
of the computation.
Internal flow or Turbomachinery
A header is outputted at the beginning of the file. The header contains the explanation of the
variables which are exported to the ".globalout" file. Below the header section, each physical time
step exports a separate line that contains the time step, the physical time, 0, the axial thrust, the
torque, theefficiency the pressure ratio, the inlet/outlet mass flow rate.
External flow
A header is outputted at the beginning of the file. The header contains the explanation of the
variables which are exported to the ".globalout" file. Below the header section, each physical time
step exports a separate line that contains the time step, the physical time, the lift, the drag, the
moment, 0, 0, 0, 0.
17.4
INPUT FILES USED BY THE FINE™/OPEN
GUI
This section describes the files created by the user and used as input data for the boundary
conditions and for the real gas characteristics. Once these files are read by the interface, they are
imported into the ".iec" file. The flow solver does not read these files directly, it retrieves the
profiles from the computation definition file with extension ".run". Profiles may also be specified
by entering the coordinates directly into the profile viewer.
The imported values will be interpreted in SI units, as used by the flow solver.
The values for 1D profiles should be given in increasing order of the x-coordinate. For example,
when entering a profile of temperature as a function of X, FINE™/Open with OpenLabs™
checks whether the two first points are in increasing order. If this is not the case, the profile will
be inverted automatically in order to ensure compatibility with the flow solver. The next time the
Profile Manager is opened, the profile will be shown in increasing order, contrary to what was
initially entered.
Time profiles cannot be defined in the FINE™/Open GUI. Instead, the user can use OpenLabs™ to
specify a time profile.
Boundary Conditions Data
When defining the inlet (or outlet) boundary condition parameters, the user has the option of
specifying one or several input files each containing a data profile. These profiles are used to
interpolate the corresponding physical variables at the inlet (or outlet).
The file containing the profile must be created by the user and its name must possess the ".p"
extension. The values of the physical variable stored in this file can come from any source:
experiments, previous computations, etc.
The following is a description of the format used to create this file.
l Line 1: Two strings defining the name of the coordinate axes.
l Line 2: Type of interpolation and number of points of the profile curve.
The types are: 0 for data given at each cell centre
1,2,3,4 and 5 for 1D interpolation respectively along x, y, z, r and θ.
11 for interpolation with respect to static temperature .
12 for interpolation with respect to static pressure.
51 for 2D interpolation along x and y.
52 for 2D interpolation along x and z.
53 for 2D interpolation along y and z.
54 for 2D interpolation along r and θ.
55 for 2D interpolation along r and z.
56 for 2D interpolation along θ and z.
The theta angle is defined as θ = arctg (y/x). The θ profile should cover the patch geometry, so it
may take negative values.
When using a 2D interpolation along r and θ, the profile has to be circular and defined from
origin (0,0,0), normal to z-axis.
l The next lines contain the coordinate(s) of each point and the associated physical value.
The following lines give an example of the data profile format:
x pressure
1 5
0.5 101000
0.6 102000
0.6 103000
0.7 102000
0.8 101000
This example is related to the interpolation of the pressure along the X-axis. There are 5 point
coordinates in the file. This is a space profile.
If there are less coordinates supplied than the number of points specified, FINE™/Open with
OpenLabs™ will put zero for the missing coordinates.
Solid Properties
The solid property heat conductivity can be inputted in the solver as constant but can also be
inputted as variables in function of the temperature.
The format used is the following:
l Line 1: Comment line.
l Line 2: Contains two integers:
l the first number is the type of interpolation: 11 for Temperature,
l the second one defines the number of points on the profile curve.
l The next lines list the data of each point: temperature and the solid heat conductivity.
Example:
T k
11 5
300.0 12.8638
350.0 13.8726
400.0 14.8814
450.0 15.8902
500.0 16.899
It is recommended to cover the whole temperature range of the considered problem.
User defined PDF
The format of the user defined PDF is the following:
l Line 1: Contains one string and one integer:
l the string is "number_of_points",
l the integer defines the number of points on the PDF.
l The next lines list the data of each point: variable and its function.
Example:
number_of_points 100
0 0
0.010101010101010102 1.4613474490780709e-005
0.020202020202020204 0.00011601194732412229
0.030303030303030304 0.00038850903048303503
0.040404040404040407 0.00091370627391922316
0.050505050505050511 0.0017704751368160471
0.060606060606060608 0.0030349384765434905
......
17.5
INPUT FILES USED BY THE FINE™/OPEN
SOLVER
The solver accepts additional files that must be explicitly written by the user.
The snap file:project_computationName.snap
This file is used to specify time steps where full outputs are required during an unsteady
computation.
This file contains a list of the time steps for which the users requires full output during an
unsteady calculation. The file contains a simple list of time steps at which output is required, either
space, tab or line separated. The number listed in the file starts from 1 not 0 as output in the Task
Manager window during the computation.
Note that requesting output at a large number of time steps can lead to very large amounts of output
data.
Also note that the results files for these intermediate time steps are not reconstructed during a parallel
computation. If the user wishes to reconstruct these files please contact our local support office.
The Lagrangian injection points file : project_
computationName.lagrInjPoints
This file is used to define the injection points for Lagrangian simulations when the global expert
parameter iLagrInjectionPoints_ to 1.
A first line with the number of points per class and the number of classes is needed. It is not
possible to use different number of points for different classes. Then, the information of all the
points for one class is given line-by-line, then for the points of the second class, and so on.
<NumberOfPointsPerClass> <NumberOfClasses>
x y z vx vy vz d T k m
x y z vx vy vz d T k m
x y z vx vy vz d T k m
x y z vx vy vz d T k m
…..
Here x,y,z are the coordinates of the injection point, vx vy vz are the absolute velocity
components of the parcels, d is the diameter, T is the temperature, k is the turbulent kinetic energy
and m is the mass flow.
The number format can be decided by the user. However it is strongly advised to use scientific format
with sufficient number of decimals, e.g. 6.
17.6 CONFIGURATION & RESOURCE FILES
USED BY THE FINE™/OPEN GUI
This section describes the files created by the user and used as the configuration or resource files
by the GUI.
Template File
The template file is a python script that will allow to set-up an initialized project (more details in
Project/Script.../Templates...). In the script, some global TCL variables are set, so that the dialog
box can display some information and get the status of the template execution. This mechanism is
encapsulated in the "Generic Template" class from which all templates should inherit. The class is
described in the "GenericTemplate.py" file provided into NUMECA_INSTALLATION_DIR/_
python/_fine/_hexa/ subdirectory.
The template file should contain a section about general information to be displayed in the GUI, a
section containing the python commands to be executed to set-up the project and finally a
template execution status to be displayed in the GUI.
Example: a template allowing to set up the fluid model, some expert parameters and the CFL
values for all the domains of the project with a display in the GUI.
#
###################################
#######
# ADJUST SOLVER PARAMETERS
FOR
# AN EXTERNAL HYPERSONIC
FLOW.
#
# VERSION 1.1
# (C) NUMECA INT
#
###################################
#######
import GenericTemplate
from GenericTemplate import *
#
###################################
#######
class HypersonicSettings
(GenericTemplate):
def __init__(self):
self.author = "NUMECA
International"
self.version = "1.1"
self.description = "Adjust default
parameters for an external
hypersonic flow."
self.detail = ". Fluid: AIR (real gas)
\n"
self.detail += ". Set CFL 1.0 \n"
self.detail += ". Expert parameters:
\n"
self.detail += " . tm_
iResSmoothing_ : 0 \n"
self.detail += " . hypInit_: 1 \n"
self.detail += " . hypInitCfl_: 1.0
\n"
def apply(self):
# Select fluid from database for all
domains
FHX.select_fluid_from_database
(FHX.get_all_domains(),'AIR')
# Set CFL for all domains
FHX.set_CFL_number(FHX.get_
all_domains(),1.0)
# Set expert parameters for all
domains:
FHX.set_parameter_value_('tm_
iResSmoothing_',FHX.get_all_
domains(),0)
FHX.set_parameter_value_('hypInit_
',FHX.get_all_domains(),1)
FHX.set_parameter_value_
('hypInitCfl_',FHX.get_all_domains
(),1.0)
# Don't forget to update the status
self.status = "OK"
print 'Template executed
successfully.'
# Template instantiation
thePreSetter = HypersonicSettings()
Resource Files
All the resource files are located in the same directory, which is /COMMON under Linux and
\bin under Windows. It is not possible to start FINE™/Open with OpenLabs™ if any of these
files is missing.
Default Parameters File hexstream.def
This file contains the default values for all parameters related to a computation. The parameter
values displayed when creating a new project in FINE™/Open with OpenLabs™ are read from
this file by the interface. This file is not edited by FINE™/Open with OpenLabs™.
Boundary Conditions Resource File hexstream_bc.def
This file contains the default values for all parameters of the available boundary conditions. The
same file is also used to create the graphical layout of the page Boundary Conditions in
FINE™/Open with OpenLabs™. FINE™/Open with OpenLabs™ only reads from this file so
this file is not modified while using FINE™/Open with OpenLabs™.
Fluids Database File euranus.flb
This file contains all the data relative to the fluids created by the users. This file is overwritten
each time a user quits FINE™/Open with OpenLabs™ after modifying the fluids database (add,
remove, or modify a fluid). All the users should have read and write permissions for this file. It is
not recommended to modify this file manually.
Steering defaults file hexstream_steering.def
This file contains information on which data will be displayed in the Convergence History page,
which is loaded when pressing the Steering button on the main Icon tab.
CHAPTER 18.
LIST OF ADVANCED PARAMETERS
Under the Advanced tab of the Computation control/Control Variables page is a list of non-
interfaced expert parameters. As stated in the interface, these parameters should not be used unless
explicitly stated in this manual. This chapter contains a list of all non-interfaced expert parameters
that are described in this manual. For each parameter a reference is given to the corresponding
section. If more information is desired, please contact our local support office.
List of Advanced Parameters
_typeOfBlockID : the type ID of the block
agglomerationNEW_ : the agglomeration method
bc_treatThermoOnFace_ : control applying thermodynamic and state laws
bc_wallCondensableFluid_ : control the type of relation used to compute the density at the wall in
case of condensable fluids
cavAmin_ : user parameter AMIN related to Cavitation
cavFCM_cL_: Speed of sound of the liquid phase used in the transport equation model.
cavFCM_cL_: Speed of sound of the vapor phase used in the transport equation model.
cavFCM_Cturb_: Modeling constant to account for the turbulence-cavitation interaction.
cavFCM_iFullPreconditioning_: Control if consider the volume or mass transport equation in the
preconditioning matrix when the transport equation cavitation model is activated.
cavFCM_iVaporMassFracEqs_: Select the vapor equation type used in the transport equation
model.
cavFCM_MinDensClip_: The allowed minimum mixture density used in the transport equation
model.
cavFCM_Singhal_Cc_: Modeling constant in Singhal model.
cavFCM_Singhal_Ce_: Modeling constant in Singhal model.
cavFCM_ SourceRelaxFactor_ minus_ : Relaxation factor
(condensation) when the transport equation cavitation model is activated.
for
the negative source term
cavFCM_SourceRelaxFactor_plus_: Relaxation factor for the positive source term (cavitation)
when the transport equation cavitation model is activated.
cavFCM_SourceTerm_: Select the formulation used in the source term.
cavFCM_SurfTension_: Surface tension used in Singhal model.
cavFCM_Tani_Cc_: Modeling constant in Tani model.
cavFCM_Tani_Ce_: Modeling constant in Tani model.
cavFCM_Zwart_Fc_: Modeling constant in Zwart model.
cavFCM_Zwart_Fe_: Modeling constant in Zwart model.
cavMuL_ : dynamic viscosity of the liquid phase
cavMuV_ : dynamic viscosity of the vapor phase
cavPreFactorRhoDissip_ : control the artificial dissipation of the continuity equation
cavPrV_ : Prandtl number of the vapor phase
cavPv_ : vapor pressure
cavRhoL_ : density of the liquid phase
cavRhoV_ : density of the vapor phase
combEquRatioCorrCoefs_ : constant for equivalence ratio correlation
combInitHybrid_ : Intiallize with fully burned state for partially premixed model
combReInitProgVar_ : reinitialization methods of the progress variable
combSchmidtTurb_ : the turbulent Schmidt number
combSDissConst_ : constant for the mean scalar dissipation rate
combTimeStep_: select the method used to compute the combustion time step
DeltaPress_RestartCav_ : Initial pressure difference when restart for cavitation
dtw_method_ : the algorithm is used for wall distance calculation
EntrFx_ : values of the entropy fix for the linear/non linear fields or the parametersVl and Vn used
in the limiter of the central matrix dissipation scheme
GP1Free_ : Initial value for the G-field of the P1 radiation model
gradientScheme_ : compute gradient at cell center
HypInit_ : activate 1st order upwind scheme initialization
HypInitCFL_ : CFL number of 1st order upwind initialization
HypInitItMax_ : the number of iteration of 1st order upwind initialization
HypInitResSmoo_ : activate residual smoothing for 1st order upwind initialization
iAsFT_ : reproduce the results obtained with FINE™/Turbo
iCavitation_ : parameter to activate cavitation
iCondTableClip_ : the computing method of the thermodynamic tables
iCstInterpol_ : the method of interpolation to get the nodal values
iFluxAverage_ : the discretization of the fluxes for the Jameson scheme
iFluxAverageFMG_ : the discretization of the fluxes for the Jameson scheme
iFnmb_treatment : computes the fluxes at FNMB interface
iGhostCylindExtrapol_ : computes dummy cell coordinates
iHStablesNotUsed_ : use PHS table or SHP table
iLagr_EvapModel_ : evaporation model for the Lagrangian
iLagr_Evaporation_ : activation of evaporation for the Lagrangian
iLagr_HeatReferenceTemp_ : model for calculation of the reference temperature
iLag_IntegrationScheme_ : select the Lagrangian integration scheme
iLagr_TimeStepCriteria_ : time step criteria for the Lagrangian method
iLagragian_Max_Iterations_ : maximum number of iterations for one Lagrangian cycle
iLagrInjectionPoints_: activates the functionality of adding Lagrangian injection points from a file.
iLagrOutputIterations_ : frequency of writing intermediate Lagrangian output
iMpCCIIterCoupling_ : iteration interval for steady MpCCI coupling
iMpCCISteadyMode_ : force to compute a steady solution with MpCCI coupling
iMpCCIzSize_ : specify the size of the cell in the third direction in 2D cases
iPartPremNonAdiabEffOnFlameSpeed_: control the non-adiabatic effect when calculating the
laminar/turbulent flame speed in partially-premixed combustion.
iRestartCav_PressDiff_ : control restart for cavitation
iSolidImpl_ : select the time-marching method for solid blocks
iSmartRestart_ : activate the option of saving backup files in case of crash and the possibility of a
smart restart.
IterScalingFuncHeatFlux_: Number of iterations on the finest grid, for which a ramp is applied to
scale the heat fluxes boundary condition(s)
ke_Ceps1_ : Ceps1 constant in the k-eps equations
ke_Ceps2_ : Ceps2 constant in the k-eps equations
Lag_MaxLocalTimeStep_ : Maximum particle time step
Lag_MinLocalTimeStep_ : Minimum particle time step
Lagr_CoeffConductivityVap_ : Coefficients for the conductivity of evaporated vapor
Lagr_CoeffcpVap_ : Coefficients for the heat capacity of evaporated vapor
Lagr_CoeffDynViscVap_ : Coefficients for the dynamic viscosity of evaporated vapor
Lagr_HeatCapacity_liquid_ : heat capacity of the dispersed phase
Lagr_LatentHeatVaporization_ : latent heat of vaporization of the Lagrangian liquid
Lagr_NbOfEstimatedStepsPerCell_ : Number of step a particle does per cell
Lagr_SumAtomicDiffVol_ : diffusion coefficient in droplet evaporation models
LagrHeatReferenceFactor_ : value for A-rule to calculate reference temperature
LagrInjectionPointsDistanceTol_: tolerance in meters to check if injected parcels are inside or
outside the computational domain when iLagrInjectionPoints_=1.
LagrMixFracSchmidtsTurb_ : Turbulent schmidt number for mixture fraction
LagrRelaxSourceTerms_ : relaxation factor for Lagrangian source terms
Lagr_CoeffcpVap_ : Coefficients for the heat capacity of evaporated vapor
MSP_cpConstSpecies_ : isobaric heat capacity of each species for a mixture
MSP_cpSpeciesNASACoeff1_ : NASA polynomials for heat capacity of species
MSP_iConductivityLaw_ : parameter to steer the thermal conductivity law of species
MSP_iConductivityMixingLaw_ : mixing law for thermal conductivity of species
MSP_iCpSpeciesLaw_ : law for isobaric heat capacity of each species
MSP_iDiffusionLaw_ : law for calculating viscosity of each species
MSP_iMultispecies_ : activation of the multi-species environment
MSP_iSpeciesEOSModel_ : law for determining Cp for each species
MSP_iViscosityLaw_ : law for calculating viscosity of each species
MSP_lambdaConstSpecies_ : thermal conductivity of each species
MSP_massDiffCoeffConstSpecies_ : laminar diffusivity of each species
MSP_molarMassSpecies_ : molar mass of each species
MSP_muConstSpecies_ : dynamic viscosity coefficient for each species
MSP_NUM_YSPEC_ : number of species
MSP_schmidtSpecies_ : laminar Schmidt number of each species
MSP_Talpha_ : coefficient of limiting thermodynamic variables
MSP_Tinf_ : lower bound of the temperature
MSP_TinfSpecies_ : for each species in Sutherland's law
MSP_Tsup_ : upper bound of the temperature
MSP_yspecFree_ : initial value of each species mass fraction
mg_iPrecondFoF_ : compute forcing function
mov_iFromInitMesh_ : deformation starting from a initial mesh
mov_iLevelCoarse_ : choose the multigrid level for MpCCI coupling
mov_iMatSave_: controls the solving of the mesh deformation matrix in RBF.
mov_iMovingGridMeth_ : Choice of the mesh deformation procedure
mov_rad_ : radius of the support of RBF
mov_rbf_ : function used for RBF mesh deformation
mpcci_Relax_ : temperature relaxation coefficient for MpCCI coupling
newParallelAgglomeration_ : switching this parameter
agglomeration is independent of the number of processors.
to 1 will ensure that
the parallel
NLH_HarmoPressureInit_: Real and imaginary part of the initial harmonic pressure values set for
all harmonics.
out_allRes_ta_ : the interval of the residual outputs
out_copyFiles_: avoid to copy mesh files to computation folder
out_CPUperIteration_ : output of the CPU time of per iteration
out_derQntFromNode_ : control how to compute derived quantities
out_displayForcePatchOfGroup_ : output force and torque for each individual patch
out_forceTorqueAreaDefined_ : output area-defined force and torque
out_gaugeForceTorque_ : get lift and drag independent of the farfield static pressure
out_htcDef_: define reference temperature used to compute heat transfer coefficient
out_mfFileVersion_ : control the structure of .mf output file.
out_periodicForcesAndMoments_ : control the integration limits when computing the forces and
moments in the .wall output file.
out_resCluster64_ : output of the convergence history in parallel computation
out_saveAHEX_ : save partitioned files
out_snsOnCFV_ : output of adaptation criteria to CFView™
out_toDisplay_ : select equation for global residual display
out_wallForcesPerIt_ : output lift, drag and moment per iteration on the fine mesh
out_writeAllCtrlPts_ta_: write the control points at every time-step or sub-iteration
out_writeCtrlPts_ta_: the interval of the outputs at control points
out_writeForces_ta_: the interval of the force outputs
PartitionerParallel_ : activate the parallel partitioner
preco_NLH_Vunst2Factor_: coefficient controlling the unsteady preconditioning velocity of the
Merkle preconditioning in order to be able to run harmonic method for low speed flow
applications. Can take the value 0 or 1.
preco_pcEpsVLim_: Coefficient of Vref when computing vlim in the Merkle preconditioning.
preco_pcEpsVLimC_: Coefficient of the speed of sound when computing vlim in the Merkle
preconditioning.
phys_PrandtlTurb_ : turbulent Prandtl number (k-ε model)
rot_iVelSy_ : select the solved velocity for rotating systems
Rad_AnisotropicScatteringCoeff : Anisotropic scattering coefficient
Rad_ScatteringCoeffValue : Scattering coefficient value
Rad_ScatteringModel : Scattering model
RadFVM_AreMirrorsSpecular : radiative heat transfer boundary condition at mirror
RadFVM_FixedIterationNumber : maximum Gauss-Seidel iterations to solve RTE
RadFVM_IterationNumber : No. of Gauss-Seidel iterations per global iteration
RadFVM_NbIter : Number of flow iterations per radiation iteration
RadFVM_NodalInt_AngularErrorTol : Tolerance level to solve RTE
RadFVM_Nphi : angular discretization in Phi direction
RadFVM_Ntheta : angular discretization in Theta direction
RelaxCombProgVars_ : relaxation factor for the progressive variable equation
RelaxCombvars_ : relaxation factor for combustion variables
RS_iCorrectionFactor_ : Correction factor for zero radius rotor/stator interface
RS_LocalCorrection_ : local enthalpy correction in non-reflecting R/S
RS_NbH2DNR_ : number of harmonics used in non-reflecting 2D R/S
RS_OutputMultiple_ : control saving of the solutions in R-S simulations
S2S_iLevelCoarse_ : choose the multigrid level for S2S
S2S_NbIter_ : iteration interval solving S2S
S2S_nbRayPerFace_ : the number of the rays per face
S2S_BCCycle_: number of cycles of solving the radiosity equation at each Runge-Kutta stage.
S2S_InnerIter_: number of the Gauss-Seidel iterations solving the radiosity equation.
S2S_RelaxFactor_: the relaxation factor used in the Gauss-Seidel iteration solving the radiosity
equation.
solidImpl_gamma_ : implicitness of the time-marching scheme
solidImpl_omSOR_ : over-relaxation parameter
solidImpl_KSPCFLStart_: starting CFL number used in the CFL ramp.
solidImpl_KSPniterCFL_: number of iterations to apply the ramp of the CFL.
solidImpl_KSPMaxIter_: maximum number of iterations for the CG method.
solidImpl_ KSPRelTol_ : relative tolerance applied for the convergence criterion of the CG
method.
solidImpl_ KSPAbsTol_ : absolute tolerance applied for the convergence criterion of the CG
method.
solidImpl_KSPDivTol_: divergence tolerance applied for the CG method.
solidImpl_KSPPrecondType_: type of preconditioner applied.
solidImpl_KSPSolverType_: type of the solver applied.
solidImpl_KSPComputeOnGrid_: solve or not the heat equation on the current multigrid level.
spc_artDiss2ndCoef_ : Coefficient k(2) for 2nd order dissipation (central scheme coefficient)
spc_artDiss4thCoef_ : Coefficient k(4) for 4th order dissipation (central scheme coefficient)
spc_ artMatDiss2ndCoef_ : Coefficient k (2) for 2nd order dissipation (central matrix scheme
coefficient)
spc_ artMatDiss4thCoef_ : Coefficient k (4) for 4th order dissipation (central matrix scheme
coefficient)
spc_artMatDissfmg_ : applied spatial numerical scheme during coarse grid initialization if the
central matrix scheme is selected
spc_dissip_ext_ : space discretization (dissipation on boundaries)
spc_dissip_wall_ : space discretization (dissipation on boundaries)
spc_expMartinelli_ : the Martinelli exponent of the dissipation
spc_iCalcArtifDissip_ : strategy for dissipation calculation in Runge-Kutta
spc_iCalcLim_limiters calculation at each stage of the Runge-Kutta
spc_iCalcVFluxes_ : strategy for viscous flux calculation in Runge-Kutta
spc_RhoswitchInArtDissip_ : add density switch to compute artificial dissipation
spc_TswitchInArtDissip_ : type of computing of the second artificial dissipation
spc_XhilnArtDissip_ : limiter with the second central scheme
ta_it_restart_ : the iteration at which the computation is restarted
ta_iVariableTimeStepping_ : activation of variable time step
table_cp_Limit_: the Cp limit when using thermodynamic tables
tm_drcoeff_ : coefficients for the Runge-Kutta scheme
tm_iResSmoothing_ : implicit residual smoothing scheme
tm_fmg_iResSmoothing_ : implicit residual smoothing scheme during coarse grid initialization
tm_mgCycleType_ : the type of multigrid cycle
tm_nbStage_ : number of stages in the Runge-Kutta scheme
turb_iRoughModel_ : select the rough wall model
turb_iYAP_ : control the Yap correction in the k-ε (Extended Wall Function) and k-ε (Low Re
Yang-Shih, classic) model.
turb_KEpsProd_ : the production term in k-eps equations
turb_mavRem_ : limiter for turbulent quantities time update
turb_mavRes_ : limiter for turbulent quantities time update
turb_mutMuLimit_ : limiter for Mut/Mu
turb_ProdWithDiamondGrad_ : gradient computing for turbulent production term
TRefBCpAdapt_ : the reference temperature
upw_dissipEnthalpy_ : controls the use of the standard or isenthalpic dissipation
upw_dissip_ext_ : controls dissipation calculation at inlet-outlet boundaries
upw_limit_ : activate limiter for the second order upwind scheme
upw_limitVenka_ : select limiter for the second order upwind scheme
CHAPTER 19.
CHARACTERISTICS OF THERMODYNAMIC
TABLES
As described in Definition of a Condensable Gas section, the Condensable Fluid module aims at
modeling the real thermodynamic properties of a given fluid by means of interpolation of the variables
from dedicated tables.
The approach that has been adopted in the FINE™/Open solver consists of using a series of
thermodynamic tables, one table being required each time a thermodynamic variable must be deduced
from two other ones. This implies the creation of many tables as input, but presents the advantage that
no iterative inversion of the tables is done in the solver, with as a consequence a very small additional
CPU time.
Information related to
l the range of variation of admissible values for thermodynamic variables
l the discretization of the grid
l the nature of the interpolation algorithm selected
l the relative mean error (mean and maximum) on thermodynamic variables
l the size of the table
is discussed here below for the by default available thermodynamic tables.
In this section
19.1 Main Characteristics for Water (Steam)
19.2 Main Characteristics for R134a
540
542
19.1 MAIN CHARACTERISTICS FOR WATER
(STEAM)
Water (steam) tables come in the form of 11 tables, described as follows:
TER: interpolates static temperature as a function of internal energy and density
PER: interpolates static pressure as a function of internal energy and density
DPT: interpolates density as a function of static pressure and temperature
EPT: interpolates internal energy as a function of pressure and static temperature
SHP: interpolates entropy as a function of total enthalpy/total pressure or relative enthalpy/relative
pressure
PHS: interpolates static or total pressure as a function of entropy and static or total enthalpy
RHS: interpolates static pressure over density as a function of entropy and enthalpy
HSP: interpolates static or total enthalpy as a function of entropy and static or total pressure
MER: interpolates dynamic viscosity as a function of internal energy and density
KER: interpolates thermal conductivity as a function of internal energy and density
PSA: defines the saturation line
TABLE 19.1 Admissible range of variations for thermodynamic variables
Tables
Variables
Minimum
Maximum
TER / PER
Energy [J/kg]
Density [kg/m³]
Pressure [bar]
Temperature [K]
DPT / EPT
Pressure [bar]
Temperature [K]
Density [kg/m³]
Energy [J/Kg]
Enthalpy [J/kg]
500,000
0.001
0.0003
237
0.002
250
0.00032
-187,568
-99,726
4,000,000
1,020
26,600
1,630
24,000
1,350
1,432
4,212,000
5,500,000
Tables
SHP
Variables
Enthalpy [J/kg]
Pressure [bar]
Entropy [J/kg/K]
Minimum
Maximum
1,500,000
4,500,000
0.002
-1,582
24,000
12,733
PHS / RHS
Enthalpy [J/kg]
1,850,000
4,500,000
HSP
Entropy [J/kg/K]
Pressure [bar]
Enthalpy [J/kg]
Entropy [J/kg/K]
Pressure [bar]
MER / KER
Energy [J/Kg]
Density [kg/m³]
Viscosity [Pa.s]
2,000
0.00021
-1,655
0.002
500,000
0.001
10,500
46,700
50,000,000
13,000
24,000
4,000,000
500
0.0000085
0.00013
Conductivity [W/m/K]
0.015
0.58
TABLE 19.1 lists the range of admissible variations for the thermodynamic variables, in the
different tables proposed.
TABLE 19.2 Main characteristics of water (steam) thermodynamic tables
Tables Grid
Interpolation
Error RMS [%] Error Maximum [%] Size [MB]
PER
71 x 71
bi-cubic (double table)
0.02
TER
71 x 71
bi-cubic (double table)
0.014
DPT
101 x 101 bi-cubic (single table)
101 x 101 bi-cubic (single table)
-
-
41 x 41
bi-cubic (single table)
0.0015
81 x 81
bi-cubic (single table)
0.005
EPT
SHP
PHS
RHS
81 x 81
bi-cubic (double table)
0.026
HSP
81 x 81
bi-cubic (single table)
0.0003
MER 41 x 61
bi-cubic (double table)
0.126
KER
41 x 61
bi-cubic (double table)
2.02
PSA
120
cubic
-
541
FINE™/Open with OpenLabs™ 7.2 User Guide
80.7
1.7
< 0.1
< 0.1
0.008
5.8
9.7
0.01
8.7
27.2
-
3.2
3.2
3.3
3.3
0.5
2.1
4.2
2.1
1.6
Both RMS (root mean square) and maximum errors should be interpreted as relative errors. RMS
error does not exceed 2%, while in most tables it is ranging from 0.0001% to 0.1%. Maximum
relative errors are located nearby the saturation line, where the interpolation naturally degrades
despite the use of bi-cubic interpolations and double table strategy.
Tables DPT and EPT have been tuned so as to guarantee maximum accuracy in the vapor phase
(< 0.1% at maximum). However, run performed in the liquid phase are consequently prohibited
since they would lead to large relative errors (> 100%) in that area. A dedicated set covering DPT
and EPT tables balancing maximum relative errors both on vapor and liquid phases can however
be obtained upon request. Please contact our local support office for any question on this purpose.
19.2 MAIN CHARACTERISTICS FOR R134A
The tables for the refrigerant R134a come in the form of 9 tables, described as follows:
TER: interpolates static temperature as a function of internal energy and density
PER: interpolates static pressure as a function of internal energy and density
DPT: interpolates density as a function of static pressure and temperature
EPT: interpolates internal energy as a function of pressure and static temperature
SHP: interpolates entropy as a function of total enthalpy/total pressure or relative enthalpy/relative
pressure
PHS: interpolates static or total pressure as a function of entropy and static or total enthalpy
RHS: interpolates static pressure over density as a function of entropy and enthalpy
HSP: interpolates static or total enthalpy as a function of entropy and static or total pressure
PSA: defines the saturation line
TABLE 19.3 Admissible range of variations for thermodynamic variables
Tables
Variables
Minimum
Maximum
TER / PER
Energy [J/kg]
170,000
520,000
Density [kg/m³]
Pressure [bar]
Temperature [K]
0.14
0.075
176
1450
3,850
590
Tables
Variables
Minimum
Maximum
DPT / EPT
Pressure [bars]
SHP
Temperature [K]
Density [kg/m³]
Energy [J/Kg]
Enthalpy [J/kg]
Pressure [bar]
Entropy [J/kg/K]
PHS / RHS
Enthalpy [J/kg]
HSP
Entropy [J/kg/K]
Pressure [bar]
Enthalpy [J/kg]
Entropy [J/kg/K]
Pressure [bar]
0.05
180
0.14
75,000
170,000
0.05
744
272,000
1,000
0.00028
125,000
700
0.05
500
430
1,620
515,000
550,000
500
2,538
550,000
2,100
5,400
1,030,000
2,500
500
TABLE 19.3 lists the range of admissible variations for the thermodynamic variables, in the
different tables proposed.
TABLE 19.4 Main characteristics of the R134a thermodynamic tables
Tables Grid
Interpolation
Error RMS [%] Error Maximum [%] Size [Mb]
PER
71 x 71
bi-cubic (double table)
0.0125
TER
71 x 71
bi-cubic (double table)
0.0022
DPT
101 x 101 bi-linear (single table)
18.9
EPT
SHP
PHS
101 x 101 bi-linear (single table)
8.28
41 x 41
bi-cubic (single table)
0.00027
81 x 81
bi-cubic (single table)
0.0081
RHS
81 x 81
bi-cubic (double table)
0.273
HSP
PSA
81 x 81
bi-cubic (single table)
0.00009
120
cubic
-
64.16
0.15
99.99
> 100
0.008
> 100
> 100
0.0079
-
3.2
3.2
0.9
0.9
0.5
2.1
4.2
2.1
0.1
Both RMS (root mean square) and maximum errors should be interpreted as relative errors.
Maximum relative errors are located nearby the saturation line, where the interpolation naturally
degrades despite the use of bi-cubic interpolations and double table strategy.
CHAPTER 20.
TABGEN
Currently,FINE™/Open with OpenLabs™ offers several modelizations of fluid properties, including
incompressible fluid, perfect gas, real gas and condensable fluid. The use of condensable fluid is done
by means of pre-processed thermodynamic tables that are loaded at the beginning of a CFD simulation
and looked- up during run time. Depending on the type of the simulation (pre- conditioning or non-
preconditioning) and the type of the boundary conditions, a different set of tables is used.
The objective of TabGen is to manage the generation of these thermodynamic tables. For the given user
input parameters, such as the name of the fluid, the equation-of-state used, the type of tables generated
(e.g. temperature-pressure PT, energy-density ER,…), the dimension of each of the tables, etc, this tool
calculates the thermodynamic state at each grid point and writes the resulting table files in a special
format. The
from NIST
(http://www.nist.gov/srd/nist23.htm).
code of REFPROP v8.0
engine of
source
tool
this
the
is
In order to run TabGen, the following command should be executed:
On Linux platforms type: tabgen -niversion <version> -print <Enter>
On Windows click on the TabGen icon in Start/Programs/NUMECA software/fine<version>.
Alternatively TabGen can be launched from a dos shell by typing:
<NUMECA_INSTALLATION_DIRECTORY>\fine<version>\bin\TabGen <Enter>
where NUMECA_INSTALLATION_DIRECTORY is the directory and # is the number corresponding
to the version to be used.
TabGen expects an uniform phase of different components. It does not take into account the fact that one of
the components changes phase at a different conditions than the others. For instance, if considering a mixture
of water and alcohol, the alcohol will evaporate first if increasing the temperature at the same pressure.
In this section
20.1 Graphical User Interface
20.2 Launch TabGen in Batch Mode
545
554
20.1 GRAPHICAL USER INTERFACE
20.1.1 Start Program
When starting the program, a Start window (FIGURE 20.1) allows the user to create a new
mixture, load an existing one or exit TabGen.
FIGURE 20.1
Start window of TabGen
Create New Mixture
The creation of a new mixture is possible by clicking on the button Create New Mixture in the
Start window. Then a Mixture window will appear, as seen in Figure below. The user can modify
the name of the mixture, which will be displayed in the top of the main window.
FIGURE 20.2
Create new mixture
In the section Available Fluids, several fluids can be selected. The
buttons are
used to transfer the selected fluids to and from the mixture. Multi-selection is also possible to ease
the process. Three buttons at the bottom of the window allows the user to load directory with
fluids, load one fluid or unload a fluid.
and
After adding fluids to the mixture, the user needs to set the molar fraction for each fluid of the
mixture. The sum of mixture component should be 100%. In order to change molar fraction, a
double click on the dedicated fluid is needed.
The maximum number of decimals of the molar fraction is 4.
For each fluid in the mixture, the user is able to see its properties and to choose its equation of
state. In order to do it the user needs to select the fluid inside the mixture and click on the button
See Fluid Properties at the bottom of the Mixture of fluids section. A new window will be
opened, as seen in Figure below. Inside there are general properties of the fluid and a combo box
with currently selected equation of state. Just below the application ranges and description related
to the selected equation are shown.
FIGURE 20.3
The properties of the selected fluid
For every user action, the current state of the mixture is displayed at the bottom of the Mixture
Properties section. If the mixture is not possible for any reasons, this issue is written inside this
field. When the mixture is possible the mixture values and application ranges are displayed.
After setting all the parameters and clicking on the button Ok, the main window of TabGen will
appear.
Open Mixture
The user can open an existing mixture by clicking on the Open Mixture button in the Start
window. Then a Load Mixture window will appear that allows the user to browse to the location
of the existing mixture. The filter in the Load Mixture window is automatically set to display only
the files with extension ".xml", the default extension for a mixture file. After opening the existing
mixture, the main window of TabGen will appear.
Exit
Clicking on the button Exit will exit TabGen.
20.1.2 Main Window
FIGURE 20.4
Main window of TabGen
In the left part of the main window, the current mixture information is displayed: Mixture Fluids,
Mixture Values and Applicability Ranges. Just at the bottom of this information part, the Edit
Mixture button allows the user to go back to edit the mixture.
The central part of the main window is dedicated to the list of tables available. Several actions can
be applied on all the available thermodynamic tables using the bottom buttons. The actions are
adapted
applied
(enabled/disabled/transformed) according to the current selection(s) of the table(s) as well as the
table's status.
table (s) within
list. The
selected
actions
are
the
the
for
The central part is subdivided in three columns: Independent Variable (or table type), Dependent
Variables, Status:
l Independent Variables are fixed and cannot be changed.
l Dependent Variables are editable .
l Status reflects the current status of the table.
The status of the table can be:
l EMPTY if nothing is generated on disk
l GENERATED if generated on disk according to the specified parameters
l MISMATCH if the current definition of the table does not correspond to the table generated
on disk
l PT TABLE NOT AVAILABLE if the table PT is not generated. Any table cannot be
generated unless the PT table is GENERATED since all 2D Tables depends on the PT table.
Thus, if the PT table is not generated, all other 2D Tables are not available for generation (but
available for editing and clearing).
If the saturation table is not generated or mismatched when the user selects to generate the PT table,
the saturation table will be generated automatically before starting the PT table generation.
In the right part of the main window, the PT ranges which are defined by default based on the
mixture applicability ranges is displayed. The user is allowed to define the Pressure-Temperature
ranges for the generation of the tables.
The user can in principle use the recommended range or a more restricted one (to have a finer grid in
the range it will be really used). However,
the user will NOT be allowed to go beyond the
applicability range.
Edit Table
When selecting one non-generated table, the user is able to edit its definition by clicking on the
Edit button. It will open a new window related to the type of the table.
Edit 1D Saturation Table
For 1D Table there is no dependent variables selection. When generating it, all dependent
variables are selected: Temperature (T), Density_liq (Dl), Density_vap (Dv), Enthalpy_liq (Hl),
Enthalpy_vap (Hv), Entropy_liq (Sl), Entropy_vap (Sv), Energy_liq (El), Energy_vap (Ev).
Linear or Cubic interpolation types can be chosen.
FIGURE 20.5
Edit 1D saturation table
Edit PT Table
The user is able to select dependent variables for this table. Temperature and pressure dependent
variables are disabled because they are already independent ones. Bilinear or bicubic interpolation
type can be chosen.
To go to the expert mode the user needs to click on the Expert button.
In the Pressure-Temperature tables, a physical discontinuity exists since the saturation is a single
line. And therefore, a sudden jump physically exists from the liquid to the gas phase. In order to
avoid a non-physical interpolation between the two states, a preferential phase can be used with
the following possibilities:
l NONE
l GAS
l LIQUID
In the Independent variables section, the user can select the scale type of the first and second
independent variable directions. The scale can be either linear or logarithmic. The user can also
specify the number of grid points in each independent variable direction. a default value 101x101
is given.
In the clustering section, The type of clustering in the first and second independent variable
direction can be set. Different grid clustering options are available:
l none
l at the beginning
l at the beginning with a small extension
l at the end
l at the end with a small extension
FIGURE 20.6
Edit PT table
Edit 2D Tables
In the normal mode the edit table 2D window is the same as the PT table edition.
In the expert mode, the user can accept the ranges automatically defined from the PT ranges in the
main window or define them by deactivating the option Obtain from PT. It activates the ranges
below and the user is free to impose their own ranges for independent values.
FIGURE 20.7
Edit 2D tables
Generate Tables
To start a generation process for one or several selected tables, the user clicks on the Generate
Tables button. If the generation action is not allowed for at least one of the selected tables, the
Generate Tables button is disabled. The same rule is applied for the other action buttons. If there
are more than one selected tables and the generation is allowed for all of them, clicking on the
button Generate Tables will open a submenu just below the button where the user can choose
between sequential generation or parallel generation of these tables.
If several tables are selected, launching sequential generation disables the Generate Tables button for
any other tables till the end of this generation, while parallel generation leaves the possibility to
generate tables which are not generated at the moment.
If only one table is selected, clicking on the button Generate Tables will automatically launch this
table generation like a parallel one.
In the case of parallel generation the tasks are really independent, so, they will share the RAM
memory and other resources (and the generation process for complex mixtures will require a lot of
resources).
If the user selection includes the PT table and a parallel generation is started, then, first of all, the
PT table will be generated sequentially and afterwards all selected tables will be generated in
parallel.
During the generation process in the status column the progress bar appears to show the
generation progress for the corresponding table. The user is able to stop the generation by clicking
on the Stop button. In the case of sequential generation it will stop all the current generation
processes. In the case of parallel generation, it will stop the generation only for the selected table
(s).
When generating a table the user can edit neither the current mixture nor the PT ranges. The user
can not create new mixture or load another mixture too (all these fields are disabled).
Stop
The user can click on the Stop button to stop the generation of the tables.
Clear Tables
The button Clear Tables is used to remove the selected table/tables that have been generated in
the list.
Mismatch Status / Fix
MISMATCH status for the table appears when its definition inside the interface differs from the
generated and saved on disk definition. The table acquires the MISMATCH status when the
definition (Edit Table button) of the generated table is changed.
Even with the MISMATCH status, the tables can be regenerated with new definitions (the
previous tables are then lost).
The user can also select the MISMATCH table and click on Fix button. In this case the table
definition is restored based on the table saved on disk. The Fix button works for multi-selection if
all the selected tables are presenting a MISMATCH status.
Visualization
FIGURE 20.8
Visualization of the selected table
If the single selected table is generated, the Visualize button is activated and allows to plot the 3D
surface corresponding to the selected generated table.
In the bottom part of the window, the view can be customized thanks to the following items:
l dependent variable surface to visualize
l logarithmic scales for any axis
l saturation lines
l colormap
l viewing buttons
In order to rotate the plot, press the mouse left button on the 3D scene and move the mouse while
it is pressed. Zoom can be performed using the mouse wheel. Translation of the surface inside the
view plane can be made by analogy to rotation holding <Ctrl> button.
It is also possible to print the current view by pressing the Export TIFF button.
20.2 LAUNCH TABGEN IN BATCH MODE
In order to execute the table generation in batch mode, the XML project file should exist before.
One or several tables can be generated in one execution depending on the arguments that are
given to the execution file. The keywords of the different table types are as follows:
l SAT : saturation table. The saturation pressure is the independent variable
l PT : tables that have pressure-temperature as independent variables (e.g. EPT.atab)
l HP : tables that have enthalpy-pressure as independent variables (e.g. THP.atab)
l ER : tables that have energy-density as independent variables (e.g. TER.atab)
l SP: tables that have entropy-pressure as independent variables (e.g. HSP.atab)
l HS : tables that have enthalpy-entropy as independent variables (e.g. THS.atab)
Then, the command to generate the tables is:
l On Linux:
tabgen <XML File> <List of keywords of the tables types separated by spaces>
l On Windows:
Installation path\bin64\tabgenx86_64.exe <XML File> <List of keywords of the tables types
separated by spaces>
Example: tabgen r114.xml SAT PT HP ER SP
In order to remove the tables, the similar command with the keyword <clear> at the end should be
typed.
Example: tabgen r114.xml SAT PT HP ER SP clear
It should be noticed that the generation of HP, ER SP and HS requires the previous generation of
the PT table. Actually, in the generation of the PT tables, a file containing the ranges of the
variables is written. This file is called "ranges.dat" and contains the maximum and minimum
values of temperature, pressure, enthalpy, energy, entropy and density.
CHAPTER 21.
TABGEN/CHEMISTRY
TabGen/Chemistry is a tool that generates, retabulates and preintegrates combustion tables according to
the user settings. The tool contains the 1D chemistry solver CHEM1D of TU Eindhoven to generate
flamelet or equilibrium tables.
TabGen/Chemistry can be used to:
l Generate equilibrium tables (non-premixed combustion),
l Generate flamelet tables or flamelet libraries (non-premixed combustion),
l Generate tables for the Hybrid BML/flamelet method (partially premixed combustion),
l Generate tables for the Flamelet Generated Manifold method (partially premixed combustion),
l Extend a given flamelet or equilibrium table so that it accounts for situations with large heat losses.
The limitations using TabGen/Chemistry are:
l TabGen/Chemistry is currently only available for Linux platforms,
l In a directory several projects can be stored and run. However,
the projects are run
simultaneously in the same directory, they might interfere with the log-file of CHEM1D, which is
used for monitoring of the convergence status,
if
l The chemical composition of the streams can only be specified using mole fractions in the steering
files (mass fractions are not yet supported),
l All flamelets are generated assuming constant pressure. The influence of compressibility effects is
not accounted for in the table generation process,
l FGM tables are based on a counter-flow diffusion flamelets (the table can however also be used for
premixed cases) and does not account for differential diffusion effects,
l FGM tables with large heat losses assumes a frozen chemistry.
In this section
21.1 Graphical User Interface
21.2 Launch TabGen/Chemistry in batch mode
21.3 Steering File
21.4 Format of look up tables
557
562
563
568
21.1 GRAPHICAL USER INTERFACE
In the Optional Models / Combustion page, the user can create a new table , load an existing
table or visualize the selected/generated table.
Create/Edit Table
The creation of a new table is possible by clicking on the button Create/Edit... in the Combustion
Parameters window. Then a new window will appear, as seen in the following figure. A template
can be selected according to the combustion parameters.
After selecting the template and clicking on the button Ok to confirm, the selected template is
loaded in the TabGen/Chemistry editor.
The fuel and oxidizer stream should be edited before the generation of the table .
The editor is split into four parts. At the top of the editor is the toolbar: File / Edit / Build. The
Resource section (under the toolbar) contains the content of the <*.tgc> input file. The Output
section contains output created by the TabGen/Chemistry tool while the table generation. The
bottom displays the cursor current position (line and column), and the status of the table
generation: Pending /In progress / Killed / Successful.
In the File menu, the user might:
l Open a new empty steering or a template
l Rename the current steering file
l Import or Export a steering file
l Close the File menu.
The Edit menu contains the following items:
l Undo: undo last resource modification
l Cut: cut selected text
l Copy: copy selected text
l Paste: paste selected text
l Find: find a string in the text
l Find next: find next occurrence of string
l Replace: replace the selected text by another one
l Select All: select all the content of the resource.
The Build menu has the following items:
l Generate table: launch the TabGen/Chemistry tool in background to generate the table.
l Abort: kill the table generation process.
Generate Table
To start a generation process, click on the Build /Generate table button. A folder _ table is
automatically created in the computation folder of the current project. Inside the _table folder, a
subfolder with the same name as the table is created, which contains the *.tab and *.tgc files. At
the end of the generation, TabGen/chemistry give a message that
the table was created
successfully. In case that the run is not successful, you will get an error message. In case that the
steering file contains errors, you will be informed on which line(s) the error(s) occurred.
The generated table is automatically linked to the computation.
To abort a generation process, click on the Build/Abort button.
Visualization
The Preview button in the Combustion Parameters windows allows to plot distribution of the
temperature (by default) or density as a function of the mixture fraction in the Combustion table
preview windows.
21.2
LAUNCH TABGEN/CHEMISTRY IN BATCH
MODE
In order to run TabGen/Chemistry, the following command should be executed:
On Linux platforms:
tabgenchem -niversion <version> -project <Steering_file> -print <Enter>
In the command line, the release version (for example, open72) needs to be specified, together
with the following arguments:
l -project followed by the full path of the steering file ".tgc". The steering file contains some
informations about the operational conditions, which are needed by TabGen/Chemistry .
l -print. This is an optional argument. If the argument is specified, the output information will
be printed on the screen.
TabGen/Chemistry can be run in an arbitrary directory as long as a valid steering file is provided.
If the run is successful, TabGen/Chemistry will end with the message "TabGen/Chemistry
terminated successfully. A look up table "_ pre.tab" (preintegrated table) or ".tab" (non
preintegrated table in case of laminar case) will be generated. The root of the name of the file
containg the look-up table (".tab"/"_pre.tab") is the same as the root of the name of the steering
file ".tgc".
In case that the run is not successful, you will get an error message. In case that the steering file
contains errors, you will be informed on which line(s) the error(s) occurred.
21.3 STEERING FILE
The steering file contains all informations that are needed by TabGen/Chemistry to generate the
look up table.
Here is an example of the steering file:
<tabgenchem>
<flamelet/>
<CHEM_MECHANISM file=gri30.chm/>
<Pressure value=2.0E5/>
<stream name=fuel>
<Composition unit=mole>
<Species>CH4=1</Species>
</Composition>
<Temperature value=368./>
</stream>
<stream name=oxidizer>
<Composition unit=mole>
<Species>O2=0.21</Species>
<Species>N2=0.79</Species>
</Composition>
<Temperature value=623./>
</stream>
</tabgenchem>
This example demonstrates how to generate a preintegrated flamelet table for methane-air non-
premixed combustion under the conditions: Absolute pressure of 2E5 Pa, air at 623 K and
methane at 368 K. As chemical mechanism the GRI-3.0 is used, which is read from the file
'gri30.chm'.
Syntax of the Steering File
In general, a steering file contains 4 levels:
l Level 1. In this level, the user can use only the following records.
Records: tabgenchem
l Level 2. In this level, the user can use the following commands or records.
Commands: flamelet, flameletlibrary, equilibrium, hybrid, pressure (attr.: value), chem_
mechanism (attr: name),
laminar, nonadiabatic, nonadiabatic_ extrapolation, heatloss (attr:
value), definitionpv (attr: name), initial_strain_unsteady_flamelet (attr: value), ichem1d_nr_
iter_max (attr.: value), nodes_pv (attr.: value), nodes_f (attr.: value), fgm_keep_original_pv_
sourceterms (attr.: value), fixed_pv_variance (attr.: value).
Records: stream (attr.: name),
l Level 3. In this level, the user can use the following commands or records.
Commands: temperature (attr.: value)
Records: composition (attr.: unit)
l Level 4. In this level, the user can use only the following entries.
Entries: Species
The steering file is subjected to the following conventions:
l In general, the xml-format applies, except:
l The user may add comment lines starting with "<!--" and ending with "-->". Alternatively,
the user may add comment lines by adding a hash-sign "#" in the first column of the line.
l Steering files are case-insensitive.
l Each command/record/entry needs to start with a sign '<'.
l A command can have an attribute. All commands are closed in the same line (ended with a
sign '/>'). Only one command is allowed per line. Examples for commands:
<flamelet/>
<Pressure value=2.0E5/>
l A record can have an attribute. All records are not closed in the same line. There can be
multiple entries/commands between the record starting line and closing line. Example for a
record:
<Composition unit=mole>
<Species> ...<Species/>
<Species> ...<Species/>
</Composition>
l An entry is opened and closed in the same line. Example for an entry:
<Species> CH4=0.5<Species/>
l Blanks (Blank lines) are ignored. However, a blank between "/" and a "<" or a ">" is not
allowed.
l The contents of each line should be written between the column 1 and the column 132.
Commands do not need to be indented.
l Commands/entries/records are order independent.
l The steering file must contain specifications for one fuel-stream and one oxidizer stream.
l Concentrations can only be specified in mole fractions and need to sum up to unity.
l Temperature can only be specified in K and need to be positive.
l Pressure can only be specified in Pa and needs to be positive.
Define Parameters
In the steering file, the user needs to specify and edit some parameters to generate a table. A
description of these parameters is presented below.
Type of tables
The following commands can be used to define the type of the tables:
l <equilibrium/>: Generation of an equilibrium table
l <flamelet/>: Generation of table with two flamelets, one for a strain of 100 1/s and the other
for a strain of 101 1/s
l <flameletlibrary/>: Generation of a flamelet library with the following strain rates a = 20, 30,
…, 90, 100, 125, 125, …, 475, 500 1/s
l <hybrid/>: Generation of a hybrid BML/flamelet table (mixing line and flamelet for a strain
rate of a = 100 1/s)
l <fgm_ nonpremixed/>: Generation of an FGM table based solely on an unsteady, non
premixed counter-flow diffusion flamelet
l <fgm_nonpremixed_wflamlib/>: Generation of an FGM table based on a library of steady,
counter flow diffusion flamelets and one unsteady counter-flow diffusion flamelet
l <fgm_nonpremixed_ignition/>: Generation of an FGM table based solely on an unsteady,
non-premixed counter flow diffusion flamelet (auto-ignition).
Laminar or turbulent
By default, a preintegrated table (turbulent case) is generated. If the user wants to generate a table
for a laminar case, the keyword <laminar/> should be added into the steering file.
Chemical mechanism
The user needs explicitly to define the chemical mechanism, which is done by the following entry
in the steering file:
<chem_mechanism file=gri30.chm/>
the user needs
to specify 'gri30.chm'
The GRI- 3.0 mechanism is provided in FINE™/Open with OpenLabs™. When using this
entry. When launching
mechanism,
TabGen/Chemistry, this GRI- 3.0 mechanism will automatically be copied into the working
directory. In GRI-3.0 mechanism, the following species are included: H2, H, O, O2, OH, H2O,
HO2, H2O2, C, CH, CH2, CH2(S), CH3, CH4, CO, CO2, HCO, CH2O, CH2OH, CH3O,
CH3OH, C2H, C2H2, C2H3, C2H4, C2H5, C2H6, HCCO, CH2CO, HCCOH, N, NH, NH2,
NH3, NNH, NO, NO2, N2O, HNO, CN, HCN, H2CN , HCNN, HCNO, HOCN, HNCO,
NCO, N2, AR, C3H7, C3H8, CH2CHO, CH3CHO. For more information on the GRI-3.0
mechanism, please refer to GRI-Mech.
in the
The user can also use another mechanism. In this case, the user must manually copy the
mechanism in the working directory and specify the mechanism name in the entry. Please note,
the chemical mechanism needs to be preprocessed. Please contact your local NUMECA support
for specific preprocessed chemical mechanisms.
Adiabatic or non-adiabatic
To account for heat losses, the user may generate a table that contains flamelets for non-vanishing
values of the enthalpy defect.
If the user specifies the command <nonadiabatic/> in the steering file, a flamelet is generated for
the values of the enthalpy defects corresponding to 0, 50000, …, 200000 J/kg. This option can
only be used with the command <flamelet/>.
If the user specifies the command <nonadiabatic_extrapolation/>, a flamelet or equilibrium table is
generated with a high heat loss (default value is 2.4E6 J/kg). The user can modify the value of the
heat loss with the command <heatloss value=Value of heat loss/>. This option can only be used
with the option <flamelet/> or <equilibrium/> or <fgm_nonpremixed/>.
Pressure
The user needs to specify the pressure level of the flamelets to be generated. This pressure applies
to both streams. When using tabulated chemistry approaches, it is assumed that the combustion
process takes place under isobaric conditions. An ambient value of the pressure is prescribed
using the following command:
<pressure value = 1.01325E5/>
Define the streams
A flamelet table for non-premixed combustion is generated by simulating a counter- diffusion
flame where an oxidizer stream is flowing against a fuel stream. In this way, the thermochemical
properties can be determined for the mixture fraction f between 0 (representing pure oxidizer) and
1 (fuel). To prescribe these streams the user has to specify the mole fractions of the species in each
of the streams as well as the temperature.
To define the conditions of a stream the records <stream name=fuel> and <stream
name=oxidizer> should to be used. The record has a name as its attribute: either "fuel" or
"oxidizer". In the sub-level of the record, the user has to specify the composition and temperature
of the stream. For example, if the fuel stream consists of 25 Vol% hydrogen (molecular), and of
75 Vol% propane (C3H8) and it has a temperature of 293.15 K, the user can define the conditions
of the fuel stream as follows:
<stream name=fuel>
<composition unit=mole>
<Species>C3H8=0.75</Species>
<Species>H2=0.25</Species>
</Composition>
<Temperature value=293.15/>
</stream>
Commands related to FGM tables generation
Some expert parameters are available for the generation of the FGM tables:
l <initial_strain_unsteady_flamelet/>: Initial value of the strain rate for the generation of an
unsteady flamelet. Default value: a0 = 100 1/s. Minimum value allowed a0 = 0.01 1/s. This
parameter is compatible with the option <fgm_nonpremixed/>
l <definitionpv/>: This option allow to change the definition of the progress variable. Default: If
following definition will be used
. If no C-atoms, but H-atoms are present, the following definition will be
contained in the
C- atoms
streams,
are
the
used
. If neither H nor C-atoms are present, the used needs to define the progress
variable explicitly. The progress variable definition is to be entered by first providing the
in mol/kg. Example:
chemical symbol on each line and then weighting coefficient
, the corresponding defintion in the steering file is:
<definitionpv>
<compositionpv unit=mole_per_kg>
<Speciespv> CO2 =22.</Speciespv>
<Speciespv> H2 =55.</Speciespv>
<Speciespv> H2O =35.71</Speciespv>
</compositionpv>
</definitionpv>
l <ichem1d_ nr_ iter_ max/>: Upper limit of the number of iterations performed by chem1d.
Default value: 50000
l <nodes_pv/>: Number of points in the progress variable direction in the un-preintegrated FGM
table. Default value: 201
l <nodes_f/>: Number of points in the mixture fraction direction. Default value: 51
l <fgm_keep_original_pv_sourceterms/>: If you have auto-ignition conditions and want to use
regular FGM tables. Please beware that using this keyword on non-autoignition, premixed
cases can lead to false ignition in the simulation
l <fixed_pv_variance/>: The table is pre-integrated along the progress variable direction.
21.4 FORMAT OF LOOK UP TABLES
Combustion look up tables are stored in a special format (ASCII) defined by NUMECA. Tables
include both a Header and Data Block.
Header
The header includes the following keywords:
l nfMean is the number of nodes in the direction of the mixture fraction
l nfVar is the number of nodes in the direction of the mixture fraction variance
l nSD is the number of nodes in the direction of the strain rate
l nED is the number of nodes in the direction of enthalpy defect
l nSI is the number of scalars stored in each data block (Z,RHO,…,<VAR>nSl-1, <VAR> nSl)
Data Block
Format attached to each data block is shown below.
Several entries are considered as mandatory, depending upon the objectives.
The following scalars are mandatory as soon as combustion is involved:
l Mixture fraction Z [-]
l Density RHO [kg/m³]
l Absolute temperature TEMP [K]
l Dynamic viscosity DYNVISC [Pa.s]
l Specific chemical enthalpy ENTHALPY [J/Kg]
l Isobaric heat capacity CP [J/K/Kg]
Similarly, the following scalars are mandatory for use with NOx post-processing:
l Source terms for NOx post-treatment (SCNO, SPNO)
Finally, the following set of scalars is additionally required for the simultaneous modeling of
combustion and radiation:
l Molar weight of the mixture (MMW, kg/ kmol)
l Source term for OTM model, only if applicable (QOTM)
l Absolute temperature in fourth power (Temp4, K4)
l Mass fraction of CO2 (CO2)
l Mass fraction of H2O (H2O)
© NUMECA International, all rights reserved
EN201805172203

CHAPTER 1.
SYSTEM REQUIREMENTS
For proper installation and use of FINE™/Open with OpenLabs™ please consult the following
sections detailing the system requirements for your operating system.
In this section
1.1 Windows
1.2 Linux
1.1 WINDOWS
1.1.1
Supported platforms and operating systems
NUMECA software is supported in 64 bits on x86_64 processors only (64 bits processors that are
compatible with Intel 8086 set of instructions).
Formally tested on
Windows 7 Professional
Windows 8.1 Professional
Windows 10 Professional
Windows HPC 2012
-
-
-
-
Also known to run ona
-
-
-
VISTA Business
VISTA Ultimate
Windows Server 2008 b
Windows Server 2012 b
a. Known from partners and/ or customers. No official support offered on these combinations.
b. Not for HEXPRESS™/Hybrid.
Please also notice that the following limitations apply:
l Computations under Windows (except Windows Server) are limited to one PVM daemon
running at a time. As a consequence, access to multiple users on a given machine is not
allowed,
l Parasolid uses SSE2 instruction for high performance. If your platform is not supporting the
SSE2 instruction, the FINE™ GUI cannot be started.
Your platform of preference is not in the list?
Contact NUMECA local sales or support office. NUMECA software does however explicitly not
run on the following configurations:
l Power PC based systems,
l WINDOWS 2000 server workstations,
l WINDOWS 95, 98 or ME workstations.
1.1.2 Multiprocessors calculations
Multiprocessors calculations are allowed on shared and homogeneous distributed platforms. Non-
homogeneous configurations are not allowed.
The following limitations additionally apply:
l Multiprocessors calculations are allowed on distributed platforms in local user configurations
provided that the same account is used for all machines,
l Domain administrators are not allowed to run multiprocessors calculations.
l MPICH2 library needs Microsoft
.net Framework package before installing NUMECA
software otherwise execution of mpiexec.exe will lead to a Windows error message.
1.1.3
Hardware requirements
Next to the standard hardware (monitor, keyboard and mouse), some specific recommendations
apply in the use of NUMECA software:
l a mouse with scroll wheel is strongly recommended.
l the monitor should support 24-bit color graphics and have a 1280 x 1024 pixel resolution for
adequate visualization.
l an Ethernet card should be installed and properly configured.
l NUMECA Software does not support CXFS (Clustered XFS) and IBRIX disk file systems.
1.1.4 Memory and disk space requirements
The Random Access Memory (RAM) required to run NUMECA software depends upon several
factors, in particular including the number of grid points inserted in the grid, the physical models
selected (turbulence, adaptation,...), the introduction of non-matching boundary conditions and the
selected calculation mode (mixed or double precision).
Similarly, a minimum disk space is required on the hard disk to allow the storage of the project
files. The size of these files largely depends upon the number of grid points generated.
More product specific details:
HEXPRESS™
The use of minimum 1 GB RAM is strongly recommended. As a general guideline, about 0.5 to
0.7 GB RAM are required to run a one million nodes project. The suggested swap space should
be equivalent to at least 3 times the RAM installed.
As a general guideline, a minimum of 300 MB is required to store the project files (provided that
the geometry is not defined by Parasolid™ or CATIA v5 files) for a one million nodes project.
HEXPRESS™/Hybrid
The Random Access Memory (RAM) required to run HEXPRESS™/Hybrid depends upon
several factors. In particular, the complexity of geometries and the settings of the CONF file. As a
general guideline, the Random Access Memory (RAM) required to run HEXPRESS™/Hybrid
are:
l for mesh without viscous layers - between 500 MB and 700 MB RAM per million of cells
l for mesh with viscous layers - between 700 MB and 900 MB RAM per million of cells
The use of minimum 4 GB RAM is mandatory, but the installation of 8 GB is recommended. The
suggested swap space should be equivalent to at least three times the RAM installed.
About 1 GB is required to store a two-millions nodes mesh in SPH format.
FINE™/Open with OpenLabs™
The use of minimum 1 GB RAM is mandatory, but the installation of 2 GB is recommended. As
a general guideline, about 1.5 GB RAM is generally required to run a one million nodes project in
double precision mode. The suggested swap space should be equivalent to at least 3 times the
RAM installed.
Mesh partitioning for parallel computations requires about 1 GB memory per million cells. When
using serial partitioner, the user must ensure that the memory on the head node is sufficient,
because the partitioning is performed only on the head node in case of serial partitioning.
As a general guideline, a minimum 1.4 GB is required to store the mesh and solution files (one
file, no full non-matching connections, solution stored after one iteration) when running a one
million nodes project.
CFView™
The use of minimum 1 GB RAM is strongly recommended. As a general guideline, about 250
MB RAM are required to visualize a one million nodes project. The suggested swap space should
be equivalent to at least 3 times the RAM installed.
No specific disk space is required on the hard disk for CFView™ except if images or data files
are saved or if the meridional average is created in CFView™ (turbomachinery application).
NTFS file system is recommended for installation and working directories under Windows.
1.1.5
Graphics requirements
NVidia graphics cards are fully supported, installed together with the latest drivers.
NUMECA software makes use of the advantages of the available Graphics Card. Some trouble
may however come up with the default driver OPENGL since it may not be supported by the user
host computer and machine display. In order to set the system compatible with a more portable
driver, typically MSW driver is used under Windows instead. Note however that the proposed
drivers are usually less efficient in terms of graphical speed than the default driver.
To change the used driver
1. Log in as administrator.
2. Launch regedit from the Start/Run menu.
3. Go to the HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International register.
4. Go into the folder of the package for which to modify the driver, e.g.: Fine# where # is the
version number.
5. Modify the DRIVER entry to either OPENGL or MSW.
The selection will take effect at the next session.
1.1.6
Compilation requirements for OpenLabs™
Customization of the CFD models using OpenLabs™ requires the possibility for compilation.
On Windows 64 bit, Microsoft Visual C++ Build Tools 2015 must be installed: make sure to
select the component Windows 10 SDK 10.0.10240 during the installation.
1.2
LINUX
1.2.1
Supported platforms and operating systems
NUMECA software is supported in 64 bits on x86_64 processors only (64 bits processors that are
compatible with Intel 8086 set of instructions).
Formally tested on
Fedora Core 22.x, 25.x
(K)Ubuntu 14.04bcd, 16.04bcd
CentOS 7.0.1406
Also known to run ona
-
-
-
-
-
-
-
SuSe 10.1, 10.2, 11.0
Enterprise 3.x, 4.x, 5.x
Fedora Core 5.x, 7.x, 8.x, 12.x, 17.x, 18.x, 20.x
(K)Ubuntub 7.x, 8.x, 9.x, 10.x, 11.xc, 12.xc, 13.xc
a. Known from partners and/ or customers. No official support offered on these combinations.
b. Debian based operating systems like Ubuntu, even if LSB compliant, are not recommended as a license
server as it is known to diverge occasionally from the LSB standard.
c. For HEXPRESS™/Hybrid pay attention to the changed NVIDIA driver location. It is necessary to specify its
location defining the environment variable LD_LIBRARY_PATH to /usr/lib/nvidia-current/.
d. The OpenLabs™ module cannot be compiled with C++ compiler g++ 4.7.3.
FlexLM requires LSB (Linux Standard Base) compliance. The list of Linux distributions and
applications
on
http://www.linuxfoundation.org/lsb-cert/productdir.php?by_lsb.
compliance with
available
standard
certified
LSB
the
for
is
When launching NUMECA software, if an error message appears when loading shared libraries,
contact NUMECA local sales or support office.
Your platform of preference is not in the list?
Contact NUMECA local sales or support office. NUMECA Software does however explicitly
not run on the following configurations:
l x86_64 processors running Linux SuSe 10.3,
l IBM PowerPC running Linux.
Optimal use of an Infiniband connection
The default Open MPI version provided in the package does not support Infiniband usage. An
Open MPI library specific to the machine(s) is required.
Use an External OpenMPI Library on Linux
1.2.2 Multiprocessors calculations
Multiprocessors calculations are allowed on shared and homogeneous distributed platforms. Non-
homogeneous configurations are not allowed.
1.2.3
Hardware requirements
Next to the standard hardware (monitor, keyboard and mouse), some specific recommendations
apply in the use of NUMECA software:
l a mouse with scroll wheel is strongly recommended.
l the monitor should support 24-bit color graphics and have a 1280 x 1024 pixel resolution for
adequate visualization.
l an Ethernet card should be installed and properly configured.
Specific to HEXPRESS™/Hybrid
l HEXPRESS™/Hybrid makes direct use of OpenGL libraries. These libraries must thus be up-
to-date, properly installed and configured before HEXPRESS™/Hybrid can be started.
l Tests have only been performed on NVIDIA graphical cards.
HEXPRESS™/View is not supported with the integrated graphics card that comes with Intel i7
processors machines. In such cases users need to modify the default settings. For example, if the
NVIDIA graphics card is available on the machine:
1. Go to the NVIDIA control panel/Manage 3D settings,
2. and select High- performance NVIDIA processor from the drop- down menu under Preferred
graphics processor.
1.2.4 Memory and disk space requirements
The Random Access Memory (RAM) required to run NUMECA software depends upon several
factors, in particular including the number of grid points inserted in the grid, the physical models
selected (turbulence, adaptation,...), the introduction of non-matching boundary conditions and the
selected calculation mode (mixed or double precision).
Similarly, a minimum disk space is required on the hard disk to allow the storage of the project
files. The size of these files largely depends upon the number of grid points generated.
HEXPRESS™
The use of minimum 1 GB RAM is strongly recommended. As a general guideline, about 0.5 to
0.7 GB RAM are required to run a one million nodes project. The suggested swap space should
be equivalent to at least 3 times the RAM installed.
As a general guideline, a minimum of 300 MB is required to store the project files (provided that
the geometry is not defined by Parasolid™ or CATIA v5 files) for a one million nodes project.
HEXPRESS™/Hybrid
The Random Access Memory (RAM) required to run HEXPRESS™/Hybrid depends upon
several factors. In particular, the complexity of geometries and the settings of the CONF file. As a
general guideline, the Random Access Memory (RAM) required to run HEXPRESS™/Hybrid
are:
l for mesh without viscous layers - between 500 MB and 700 MB RAM per million of cells
l for mesh with viscous layers - between 700 MB and 900 MB RAM per million of cells
The use of minimum 4 GB RAM is mandatory, but the installation of 8 GB is recommended. The
suggested swap space should be equivalent to at least three times the RAM installed.
About 1 GB is required to store a two-millions nodes mesh in SPH format.
FINE™/Open with OpenLabs™
The use of minimum 1 GB RAM is mandatory, but the installation of 2 GB is recommended. As
a general guideline, about 1.5 GB RAM is generally required to run a one million nodes project in
double precision mode. The suggested swap space should be equivalent to at least 3 times the
RAM installed.
Mesh partitioning for parallel computations requires about 1 GB memory per million cells. When
using serial partitioner, the user must ensure that the memory on the head node is sufficient,
because the partitioning is performed only on the head node in case of serial partitioning.
As a general guideline, a minimum 1.4 GB is required to store the mesh and solution files (one
file, no full non-matching connections, solution stored after one iteration) when running a one
million nodes project.
CFView™
The use of minimum 1 GB RAM is strongly recommended. As a general guideline, about 250
MB RAM are required to visualize a one million nodes project. The suggested swap space should
be equivalent to at least 3 times the RAM installed.
No specific disk space is required on the hard disk for CFView™ except if images or data files
are saved or if the meridional average is created in CFView™ (turbomachinery application).
1.2.5
Graphics requirements
NUMECA software makes use of the advantages of the available Graphics Card. By default, the
driver OPENGL is used.
In case a problem appears with the default driver OPENGL, the user should change to the X11 driver
under Linux. Note however that the X11 driver is usually less efficient in terms of graphical speed
than the default driver.
The drivers OPENGL and OPENGL2 may not work when using VNC or remote access by
"ssh". In case of problems, the X11 driver should be used.
To change the used driver
To change the driver permanently for every next launch of the software:
1. Open the file ~\.numeca\.drivers
2. Type: host_name display_name possible_drivers chosen_driver e.g. gauss.numeca.be gauss
OPENGL:X11 X11
The selection will take effect at the next session.
Alternatively, the driver can be manually specified in a shell for that shell session only through the
following commands:
l in csh or tcsh shell:
setenv NI_DRIVER X11
l in bash or korn shell:
NI_DRIVER=X11 export NI_DRIVER
1.2.6
Compilation requirements for OpenLabs™
Customization of the CFD models using OpenLabs™ requires the possibility for compilation:
On Linux 64 bit, the GNU C and C++ compiler (g++) must be installed. The gcc version should
be between 4.8.# and 5.3.# (type the command gcc -v in a shell to get your gcc version). The
officially tested version is g++ 4.8.5.
CHAPTER 2.
INSTALLATION
Prior to installation it is important to consult first the "System requirements" (p. 3).
2.1 Windows
2.2 Linux
14
34
2.1 WINDOWS
The user is strongly advised to consult the "Windows" (p. 4) system requirements prior to the
installation. Problems may indeed appear during the installation and configuration phases in case
the listed hardware and software requirements would not be fully satisfied.
Please do notice that the documentation package attached to NUMECA software is not installed
during the installation procedure and can be downloaded from the Products page of the Customer
Area of www.numeca.be.
In case of trouble: .
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
At the end of the "Troubleshooting" (p. 31) the information to provide is listed.
2.1.1
Installation
Install FINE™/Open with OpenLabs™ under Windows
1. Log in as administrator or as a user with administrator privileges on the machine. If the user
the NUMECA software installation will not be
does not have administrator privileges,
performed successfully.
2. Check and make sure that the necessary disk space is available prior to starting the installation
process.
For the disk space requirements, see also: "Windows" (p. 4) system requirements.
3. Get the installation package from the Products page of the Customer Area (www.numeca.be).
4. Unzip the installation package.
5. Exit all the other active applications and launch the setup.exe executable.
6. During the installation, the user will be asked to accept the terms of the License Agreement.
7. Enter the installation directory (referred to as NUMECA_INSTALLATION_DIRECTORY)
in function of one of the following scenarios:
l If NUMECA software was not installed before on the machine, choose a directory of your
preference. Providing a directory name that does not exist will create it automatically.
l If NUMECA software was already installed before, choose the same NUMECA_
INSTALLATION_DIRECTORY to use the multiple versions and/ or products in one
multi-version environment.
It is important to notice that a common NUMECA_INSTALLATION_DIRECTORY
should be shared by all NUMECA installations (e.g. C:\numeca_software\), otherwise
the multi-version installation will not be set up adequately. This is important e.g. for the
good functioning of PVM when launching several products or versions one after the
other.
8. At the end of the installation process, instructions to obtain information required for license
generation will be prompted. To this end, the following steps must be performed:
a. Click on Yes.
b. The license information is stored in the file license.info located in NUMECA_
INSTALLATION_DIRECTORY automatically. Once it is saved, send this text file to
NUMECA local sales or support office.
Alternatives to get the license information
the installation process
The information can also be obtained using the NUMECA Administration Tool (Launching at
the end of
from Start/Programs/NUMECA
software/<product_name>/Administration Tool menu) or recovered as Ethernet Address
by clicking on the System Settings tab after launching lmtools.exe located in the directory
NUMECA_INSTALLATION_DIRECTORY\<product_name>\flexlm.
(step 8) or
9. After the package is installed, the NUMECA Administration Tool is launched automatically.
This is a tool for license management and provides a graphical user interface for the
management of the license server and client machines. The tool offers a guide through the
process of setting up and configuring a license server.
Alternatives to access the Administration Tool
installation,
from
After
Start/Programs/NUMECA software/<product_name>/Administration Tool menu. Click
on Finish to leave the tool and to finalize the installation.
the Administration
started
Tool
also
can
be
Tasks that can be performed in the NUMECA Administration Tool
l License Management: to configure the machine as license server and/ or client.
l User Configuration: to set user MPI configuration.
l Diagnostics: to assess and fix problems with license management, graphics, Windows
registry and parallel configuration.
l Network Configuration: to clean and reinitialize PVM, to setup RSH connections to other
machines/ users.
10. When receiving the license file from NUMECA, perform the license installation and user
configuration:
l "License management" (p. 17)
l "User Configuration" (p. 23)
During an installation and license specification, the administrator must launch the software once to
properly initialize flexlm.
In case of installation problems, right-click on setup.exe, select the option Run as... and then either
run as the true Windows Administrator account, or if and only if the user account with Administrator
privileges, run as user, but remove the option to run the program with restricted access. On
WINDOWS 7 it may also be necessary to disable the User Account Control feature (UAC) at least
during the installation process and the configuration steps.
In order to run distributed memory parallel computations, NUMECA software must be installed in the
same directory on different machines.
Install HEXPRESS™ v7.2 standalone
The installation of FINE™/Open with OpenLabs™ v7.2 includes HEXPRESS™ v7.2.
The latest release of HEXPRESS™ standalone v7.2 can be downloaded from the Products page
of the Customer Area (www.numeca.be ) and used in combination with FINE™/Open with
OpenLabs™ v7.2. This standalone version contains significant improvements:
New Features in v7 of HEXPRESS™
New Features in v7 of HEXPRESS™/Hybrid
2.1.2
License management
Introduction
Before using NUMECA software, a valid floating license is required.
What is a floating license?
With a floating license each software component is managed by an independent maximum
number of concurrent accesses (number of processes). Floating licenses are managed by a license
server which checks if process access is free. If so, when launching a software component, license
access is given to the user process or access is denied otherwise. The license can be accessed on
the same computer but also on other computers (clients) with Linux or Windows, connected
through a network to the license server. The license server can be a Linux or a Windows
machine.
l NUMECA updates the security ID of license files with each major release. License files
with old security ID cannot be used with the latest NUMECA software. Please send your
old license file to NUMECA local sales or support office for an upgrade of the license file.
l Redundant license server can be delivered allowing to manage a floating license by several
servers. For more information, contact NUMECA local sales or support office.
l Machines used as license server must have a fixed first IP address. For example, when
using VPN on Windows, VPN will become the first network interface. In this case, the
license server will not work properly.
l By default it is not possible to use a virtual machine as a license server. To install a license
server on a virtual machine, contact your account manager.
l Running Windows 64-bits, an additional Windows security patch is required to enable
CATIA v5 import with Datakit. For more details, link to the Microsoft official website.
NUMECA software must be installed on the license server. At the end of the installation, the
license information (the HostName and HostID of this computer) must be sent to NUMECA local
sales or support office in order to get a license file.
Before using NUMECA software, the license daemon should be configured on the license server.
See also: "Installation" (p. 14)
To set up the license server it is necessary to prepare the license file and launch the server either
though the NUMECA Administration Tool or in LMTools.
Access to the NUMECA Administration Tool
At the end of the installation of NUMECA software the Administration Tool is launched
automatically.
It can also be started anytime from the Start/Programs/NUMECA software/<product_name>
menu: right-click on the Administration Wizard item and select Run as administrator.
It is required to run the Administration Tool as administrator for its proper functioning.
Prepare the license file
To install the license service:
1. Rename the license file as license.dat
2. Copy the license.dat file in the directory that all users are able to access.
3. Check that the license file has the read-execute access privileges:
l select the license file license.dat using Windows Explorer.
l while keeping the mouse on the selected file right-click and select from the appearing
menu: Properties. This will open a properties window.
l on the General page the Read-only box of the Attributes should not be selected. Unselect
this box if necessary.
l click on Apply and click on Close to close the window.
The "license.dat" file must be readable by every user.
When using a TCP port for the license server, the port number (check the free port with the
command: C:\\netsat -an) has to be added in the license file on the server/ vendor line:
1. SERVER hostname hostid and VENDOR numeca should be replaced by SERVER hostname
hostid portnumber1 and VENDOR numeca portnumber2;
2.
3.
reread the license file,
start NUMECA software and specify the license server writing portnumber@hostname . All
specified ports should be opened and free.
It is no more required to copy the license files on every client workstation if the variables NUMECA_
LICENSE_FILE defined as @license_server or port_number@license_server are added in the registry
database for each client. This allows to update the license file only on the license server.
License set-up in NUMECA Administration Tool v12
Start floating license service
To start the license service:
1. Select License Management.
2. On the line Activate from license file browse to the license file.
3. Click on Apply.
The manual start operations must be repeated each time the server machine is rebooted. Alternatively
it would be possible to define an automatic start of the license service from lmtools or using the
NUMECA Administration Tool.
Automatic start at machine boot
After the manual start of the license service, it is possible to have it automatically start at machine
boot:
1. In License management click on the Advanced button.
2. Go to the License server tab.
3. Press the Set autostart server button.
A Windows service called NUMECA License server is used.
Verify license service status
To verify that the license server is correctly running do the following:
1. From the NUMECA Administration Tool home page, click on License Management .
2. Click on the Advanced button at the bottom of the Activate Product tab.
3. Select the License server status tab.
4. Select the license server on the left-hand side drop down menu.
5. Information regarding the available features, the number of available licenses and the number
of used licenses is shown under the License server info section.
Update of license file
When a license file is expired, contact NUMECA local sales or support office to obtain an
updated license file.
Replace the active license file license.dat with the update license provided by NUMECA
(renamed as license.dat).
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
1. Go to the NUMECA Administration Tool home page, click on License Management .
2. Click on the Advanced button at the bottom of the Activate Product tab.
3. Select the License server tab.
4. Click on the Re-read license button.
5. The words "SUCCEEDED" or "Failed" are shown depending on the update success or
failure, respectively.
If the version of the Flexlm tool is upgraded or the version of the license file security ID is
upgraded, an update of the license file is not sufficient. The user must shutdown the running
license server and start a new license server with the latest Flexlm tool and the latest license file.
Alternative: license set-up in lmtools
Start license service
1. In Windows Explorer,
browse
to
the
directory NUMECA_ INSTALLATION_
DIRECTORY/<product_name>/flexlm and double click on lmtools.exe.
2. On the Service/License File page select Configuration using Services.
3. Select the Config Services tab.
4. Enter for Service Name any name indicating that it is related to a NUMECA license (e.g.,
numeca_license).
5. To enter the Path to the lmgrd.exe file click on Browse right next to the text box and browse
select
to NUMECA_ INSTALLATION_ DIRECTORY/<product_ name>/flexlm and
lmgrd.exe.
6. To enter the Path to the license file, click on Browse right next to the text box and browse to
the license file license.dat to select it (files of type from license files (".lic") to license files
(".dat")).
7. Enter HOME_DIRECTORY/.numeca/debug.log to access the path of debug log file. This
file is automatically created when starting the license service.
8. Click on Save Service.
9. Select Use Services and Start Server at Power Up. In this way the license service will be
automatically starting when booting under Windows.
10. To start the server now manually select the tab Start/Stop/Reread.
11. Select
the NUMECA license service under Flexlm license Services installed on this
computer.
12. Click on Start Server.
If the license service was correctly started, numeca.exe and lmgrd.exe should be visible in the list
of processes or services in Windows Task Manager. If these executables are not running verify the
debug.log file.
See also: "Troubleshooting" (p. 31)
13. If NUMECA software is used on the license server, the user should first perform a user
configuration as described in the section "User Configuration" (p. 23).
14. Launch the software a first time.
15. Click on Specify the License Server.
16. Enter the name of the license server or its IP address.
17. Click on Finish.
Update of license file
When a license file is expired, contact NUMECA local sales or support office to obtain an
updated license file.
Rename this license file to license.dat and follow the instructions below.
1. Replace the active license file license.dat with the update license provided by NUMECA
(renamed as license.dat).
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
2. Go to the directory NUMECA_INSTALLATION_DIRECTORY/<product_name>/flexlm.
3. Start the LMTools by double clicking on lmtools.exe
4. Select the tab Start/Stop/Reread.
5. Select the NUMECA license service in the list and click on ReRead License File.
If the version of the Flexlm tool is upgraded or the version of the license file security ID is upgraded,
an update of the license file is not enough. The user must shutdown the running license server and
start a new license server with the latest Flexlm tool and the latest license file.
Verify license service status
To verify that the license server is correctly running do the following:
1. Open the Windows Task Manager.
2. Select the Processes or Services.
3. Check that the processes numeca.exe and lmgrd.exe are running.
or:
1. In Windows Explorer
browse
to
the
directory NUMECA_ INSTALLATION_
DIRECTORY/<product_name>/flexlm and double click on lmtools.exe.
2. Select Configuration using Services.
3. Select the tab Server Status.
4. Click on Perform Status Enquiry and wait to see the server status and the available features.
Floating license on Windows client
When a floating license is installed on a license server, this license may be used by other
computers with a network connection to the license server. In this section, it is assumed that the
license server is running. On each Windows client, the user must:
1. Install NUMECA software.
2. Perform a user configuration on this machine before first use as described in the section "User
Configuration" (p. 23).
3. Click on Specify the License Server when first starting the software.
4. Enter the name of the license server or its IP address.
5. Click on Finish.
Optional: ask software to wait for license
To request that NUMECA products wait for an active license, define it in the "Home directory"
(p. 26) in .numeca/preferences.dat using the keyword LICENSE_WAIT. This functionality is
available for all products.
Example
PRODUCT FINE/Marine
LICENSE_WAIT
END_PRODUCT
Student version with activation ID
In general a license certificate (text file) is provided to give access to NUMECA software.
Alternatively the NUMECA Administration tool allows to use an activation ID to start the license
server. For example, the free student version is based on an activation ID and the instructions how
to use it are provided together with the activation ID. Use of an activation ID requires the use of
Trusted storage and installation of an anchor service. Hence this terminology can be found in the
NUMECA Administration Tool but can be safely ignored in case of a license certificate in text
file format.
Example of an Activation ID: C2a9-561f-7895-435b-acb5-3520-c166-4bcc
2.1.3
User Configuration
A. Optional user configuration
Without the optional steps in this section it is still possible to launch a simulation on one processor
on the local machine with a default location of the home directory.
Configure account to perform parallel computations
Provided that the parallel capabilities have been adequately installed and valid licenses can be
accessed,
the user will be able to perform parallel computations. Launching a parallel
computation, the system will by default request the user login and password. Before the first
launch, the user can register his/ her name and password once and for all, by doing the following
steps:
1. Open a DOS shell,
2. Type
the
command
NUMECA_
INSTALLATION_
SOFTWARE/fineopen72/bin64/mpiexec.exe -register<Enter>.
3. Enter the user login and password and confirm.
If the user does not register his/ her name and password before launching the parallel computation,
the FINE™ GUI will prompt the user to enter credentials (Windows login account) if needed.
Currently, it is not possible to launch the computation without the registering/ providing the user's
credentials. Thus, if no password has been defined during the registration, it will be necessary to set
the password on the machine in any case.
Domain administrators are not allowed to run parallel computations under Windows.
PVM does not support domain accounts.
Parallel computations under Windows (except Windows Server) are limited to one PVM daemon
running at a time on the machine. Consequently, access to multiple users on a given machine is not
allowed.
MPICH2 library needs Microsoft .net Framework package before installing NUMECA software.
When running parallel computations, the path to the project must be identical on both the local and
remote machines. For example, for distributed memory parallel computations, a folder must be
mounted on each machine and share the same drive name, in order to store the project directory that
will be run in parallel on multiple hosts.
Configure account to allow remote computations
It is possible to launch tasks on remote machines by using the Task Manager capabilities. To be
able to perform remote launches, NUMECA software must be installed and explicit permission
must be specified on the remote machine. To this end, the following operation must be checked
and/ or performed on the remote machine:
1. Open the Windows Control Panel window (Start/Settings/Control Panel).
2. Click on the Services icon under System and Security/Administrative tools.
3. Select from the list of services NUMECA RSH Daemon.
4. Click on Stop and leave the Services window open.
5. Edit the file rhosts.txt in the directory C:\WINDOWS on both the host and client machines.
This can be done through the FINE™/Admin tool. Launch it from All Programs-
>NUMECA software-><product_name>->Administration Wizard and select Configure
the TaskManager in this machine.
Alternatively edit the rhosts.txt file
Edit the text file and add the following line for each host user you want to give access
permission:
hostname username:
These lines typically give right to the user username, working on the machine hostname, to
connect to the machine containing the rhosts.txt file.
6. Select the NUMECA RSH Daemon from the list of services in the Services window.
7. Click on Start. Starting this service may take approximately 5 minutes.
Use of the Task Manager under Windows with a Linux host may lead the remote copy to option to
fail. See also: "Cannot connect to other hosts" (p. 33) in the Troubleshooting section for more detail
on this problem.
In addition to that, the firewall should also allow remote computations. To do so, follow the steps
below:
1. Add a Port inbound and outbound rule for a TCP protocol with the number 514. The
connection should be allowed for all type of profiles.
2. Allow the following programs to bypass the firewall inbound and outbound rules: smpd,
mpiexec, hexstream#x86_64 and hexstream#_impix86_64 (# stands for sp, hp and dp) located
in <NUMECA_INSTALLATION_DIRECTORY>\fineopen72\bin64; lib\win32\pvmd3.exe,
<NUMECA_
bin\rsh.exe,
INSTALLATION_DIRECTORY>\pvm.
bin\win32\hoster.exe
bin\rsh_ vista.exe
located
and
in
Home directory
On Windows, NUMECA software saves some data (preferences, user fluid database, ...) in the
folder %HOME%\.numeca\, or in the %HOMEDRIVE%%HOMEPATH%\.numeca\ folder in
case %HOME% is not defined. If the user wants to customize the path of the .numeca folder, the
user can redefine the system environment variable HOME.
Note:
l The variable HOME must be defined as a system environment variable.
l Defining HOME to a network disk may significantly slow down the NUMECA software
GUI.
the
runtime, NUMECA software writes
During
directory
%HOME%\.numeca\tmp. This tmp directory can be redefined by defining the environment
variable TMP_DIR.
temporary
data
the
in
B. Software launch
After configuring,
software\<product_name>\ menu.
the product can be
started from the Start\Programs\NUMECA
It is not allowed to start NUMECA software under Windows as administrator in a user domain
environment. This limitation does not apply to user login.
In case the license has not been configured adequately at this stage of the installation process, it is still
possible to launch the product by selecting a license file (server) when prompted after first launch.
The UAC (User Account Control) should be disable for running the solver in parallel otherwise it
prevents mpiexec to record the encrypted login and password in the registry database and the Task
Manager remains open forever without any evolution.
NUMECA software can be launched directly from the user desktop by copying shortcuts from
~\AllUsers\StartMenu\Programs\NUMECA software\<product_name>\ to ~\AllUsers\Desktop.
It is not suggested for one user to simultaneously open (and therefore launch tasks in) more than one
FINE™ environment.
2.1.4
Uninstallation
Before removing a product, the license service and PVM should be stopped as detailed in the
following section. As a next step the product can be removed.
Uninstall license service
In case the license service is defined based on a version of NUMECA software to uninstall, the
license service should be stopped and removed first. Of course further use of remaining
NUMECA products on the machine will require redefining the license service based on the most
recent product.
In NUMECA Administration Tool
1. Go to the NUMECA Administration Tool home page,
2. click on License Management,
3. click on the Advanced button at the bottom of the Activate Product tab,
4. select the License server tab,
5. click on the Stop license server button to stop the specified license server.
6. The words "SUCCEEDED" or "Failed" are shown depending on the success or failure of the
uninstalling process, respectively.
7. Click on the Remove from autostart button to complete the uninstalling process.
Or in LMTools
1. Browse
to
DIRECTORY/<product_name>/flexlm.
in Windows Explorer
the
directory NUMECA_ INSTALLATION_
2. Double click on lmtools.exe.
3. Select Configuration Using Services.
4. Click on the Start/Stop/ReRead tab.
5. Select the NUMECA license service from the list of services.
6. Click on Stop to stop the license service.
7. Click on the tab Configure Services.
8. Select the NUMECA license service through the Service Name pull down menu.
9. Click on Remove Service to remove the service.
Close PVM
FINE™ environment uses PVM. Before uninstalling FINE™, the PVM process must be closed.
This can be done as follows:
1. Start the Task Manager (Modules/Task Manager) from the FINE™ GUI and select the
Hosts definition page in the menu on the left.
2. Click on the button Shutdown. A warning message will appear stating that all hosts will be
removed from the Virtual Machine and that FINE™ GUI will be closed. Click on yes to
continue.
Uninstall the Product
Before uninstalling verify the following:
l that there are no running tasks on the machine,
l that the license service was stopped as described in the previous section ("Uninstall license
service" (p. 27)).
Depending upon the configuration, there are several possibilities:
l If the product is the only product and the only version on the computer: uninstall in mono-
version environment.
l If other products and/ or other versions are installed on the same machine, it is possible to: 
l to remove only some of these products/ versions: partly uninstall
in multi- version
environment",
l to remove all products: fully uninstall in multi-version environment".
Uninstall in mono-version environment
Proceed as follows to remove FINE™/Open v72 in a mono- version environment under
Windows:
1. Optional: 
a. go to NUMECA_INSTALLATION_DIRECTORY/fineopen72/bin64 in a dos shell and
b.
type smpd -remove so as to remove the services for MPICH2.
Please do notice that this step is optional and only applies if MPICH2 services have not yet
been removed. Otherwise, an error message indicating that the service has not been installed
will appear. Please also notice that the services can be installed back if necessary with the
command smpd -install.
c. Go to NUMECA_ INSTALLATION_ DIRECTORY/impi5/
in a dos shell and type
hydra_service -remove so as to remove the services for IntelMPI.
Please do notice that this step is optional and only applies if IntelMPI services have not yet
been removed. Otherwise, an error message indicating that the service has not been installed
will appear. Please also notice that the services can be installed back if necessary with the
command hydra_service.exe -install.
2. Go to NUMECA_INSTALLATION_DIRECTORY/pvm/bin in a dos shell and type nirshd -
remove so as to remove the services for RSH daemons.
Please notice that the services can be installed back if necessary with the command nirshd -
install.
3. Proceed with a reboot of the PC.
4. Open the Windows Control Panel (Start/Settings/Control Panel) and double click on the
icon Programs and Features.
5. Select Fineopen72 from the list and click on Add/Remove.
Partly uninstall in multi-version environment
Proceed as follows to remove FINE™/Open with OpenLabs™ v72 or
for example
FINE™/Open v6.1 (but not both) in a multi-version environment under Windows:
1. Open the Windows Control Panel (Start/Settings/Control Panel) and double click on the
icon Programs and Features.
2. Select Fine72 or Fineopen61 from the list and click on Uninstall.
Fully uninstall in multi-version environment
Proceed as follows to remove FINE™/Open with OpenLabs™ v72 and,
FINE™/Open with OpenLabs™ v61 in a multi-version environment under Windows:
for example,
1. Optional: 
a. go to NUMECA_INSTALLATION_DIRECTORY/fineopen72/bin64 in a dos shell and
b.
type smpd -remove so as to remove the services for MPICH2.
Please do notice that this step is optional and only applies if MPICH2 services have not yet
been removed. Otherwise, an error message indicating that the service has not been installed
will appear. Please also notice that the services can be installed back if necessary with the
command smpd -install.
c. Go to NUMECA_ INSTALLATION_ DIRECTORY/impi5/
in a dos shell and type
hydra_service -remove so as to remove the services for IntelMPI.
Please do notice that this step is optional and only applies if IntelMPI services have not yet
been removed. Otherwise, an error message indicating that the service has not been installed
will appear. Please also notice that the services can be installed back if necessary with the
command hydra_service.exe -install.
2. Go to NUMECA_INSTALLATION_DIRECTORY/pvm/bin in a dos shell and type nirshd -
remove so as to remove the services for RSH daemons.
Please notice that the services can be installed back if necessary with the command nirshd -
install.
3. Proceed with a reboot of the PC.
4. Open the Windows Control Panel (Start/Settings/Control Panel) and double click on the
icon Programs and Features.
5. Select Fineopen61 from the list and click on Uninstall.
6. Select Fineopen72 from the list and click on Uninstall.
2.1.5
Troubleshooting
Introduction
In most cases, a straightforward and careful execution of the instructions detailed in the
installation note enables to start NUMECA software smoothly. In case it is not working as
expected this section provides information on how to handle most common situations.
Product not starting
In case FINE™/Open with OpenLabs™ does not start, check the following items:
l Is NUMECA software installed with administrator privileges? If not, perform the installation
again with administrator privileges.
l Check whether 'Hide file extensions for known types' (activated by default for .dat extensions)
is disabled to enter the name of the license file with its extension license.dat.
l Is the license file valid and active to start the product ?
ll Check if the license server is up. If so, the numeca.exe process should run in the Windows
Task Manager. If not, please do the instructions for license installation.
l Some license check problems may occur if the host computer cannot find the server IP-address
corresponding to the hostname information included in the first line of the license key. To
solve this problem, replace the hostname by the IP-address of the license server. This operation
does not invalidate the license key.
l Check if the license key file is well readable by every user.
l Did the user configure his/ her working environment? If not, perform the configuration
according to the section "User Configuration" (p. 23); then log out and log in.
l Has the machine been rebooted after a change in the environment variables? If not, reboot it.
l Check if the TCP/IP protocol is installed on the machine. The protocol is mandatory to ensure
the correct function of the floating licenses.
l Are the NUMECA software components visible from the machine? If not, install them.
l Clean PMV files:
1. Close all tasks opened, including the FINE™GUI.
2. Open the Windows Task Manager and select the thumbnail Processes.
3. Check that no process pvmd3.exe is running. If so, select the process and click End
Process to stop it.
4. Delete any files called pvm*.username in the directory defined by the environment variable
PVM_TMP (usually C:\tmp).
Graphical problems and system crashes
NUMECA software makes use of the advantages of the available Graphics Card. Some trouble
may however come up with the default driver OPENGL since it may not be supported by the user
host computer and machine display. In order to set the system compatible with a more portable
driver, typically MSW driver is used under Windows instead. Note however that the proposed
drivers are usually less efficient in terms of graphical speed than the default driver.
To change the used driver
1. Log in as administrator.
2. Launch regedit from the Start/Run menu.
3. Go to the HKEY_LOCAL_MACHINE/SOFTWARE/NUMECA International register.
4. Go into the folder of the package for which to modify the driver, e.g.: Fine# where # is the
version number.
5. Modify the DRIVER entry to either OPENGL or MSW.
The selection will take effect at the next session.
Screen flashes
In some circumstances, the graphical area can flash during interactive operations, depending upon
the driver selected. Setting the environment variable NI_ DOUBLEBUFFERING to ON in
HKEY_ LOCAL_ MACHINE/SOFTWARE/NUMECA International/<product_ name> register
may solve the problem. To launch the registry editor, access regedit in the Start/Run text box.
Flow solver not starting in parallel mode
The parallel account must be configured at first use .
To launch parallel computations on Windows, the solver uses the MPICH2 libraries and the smpd
process manager. The smpd service is automatically installed and started during the installation of
FINE™. If the user has already the smpd service installation before installing FINE™, there may
be a conflict between the smpd services and thus the smpd service in FINE™ may not be started.
If the user gets the error message smpd version mismatch during the parallel computation, check
if the FINE™ smpd service is started. If not, stop other smpd services and start the one installed
by FINE™ (the service name is MPICH2 Process Manager, Argonne National Lab and the
linked executable is Installation_path\fine<version>\bin64\smpd.exe).
Cannot connect to other hosts
At the first execution of task manager
Can the machine be "seen" from the remote hosts (and vice-versa)? Use the ping command to
check this item.
Is the machine name included in the computer list within the rhosts.txt file of the user? Please
notice that capital letters must be used; extra-characters like "è, ä, ë, ..." may lead to potential
problems and should better be avoided.
Task manager launched once with success
In case the user can no longer connect to other hosts while this operation has at least be successful
once, the following should be checked:
1. a. Start the Task Manager (Modules/Task Manager) from the FINE™ GUI and select the
Hosts definition page in the menu on the left.
b. Click on the button Shutdown. A warning message will appear stating that all hosts will be
removed from the Virtual Machine and that FINE™ GUI will be closed. Click on yes to
continue.
2. Close all currently open tasks (including the FINE™ GUI) and remove pvmd.* and pvml.*,
located in the directory defined by the environment variable PVM_TMP (by default C:\tmp), if
applicable. Additionally kill the PVM daemon pvmd3.exe, if applicable. The status of PVM
daemon can be observed by accessing the Windows Task Manager.
Remote copy does not work
The remote copy option can be accessed in Task Manager Tasks Definition area.
This option does not work if the user configuration file .cshrc (Linux platform) gives output to a
shell. To test whether it applies, open a DOS shell on the Windows machine and type the
command rsh machine_name echo YES <Enter> (where machine_name refers to the name of
the Linux machine). If the value returned is YES, the configuration is correct and the remote copy
option is expected to work properly. If additional lines are returned, problems are expected. If so,
further troubleshooting is needed as described in the following section.
Further troubleshooting
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
The following information can be helpful:
l the license key file license.dat.
tool
(started
l the hostname and hostid. This information can be obtained by launching the NUMECA
Administration
from Start/Programs/NUMECA software/<product_
name>/Administration Wizard menu) or by executing into the subdirectory NUMECA_
INSTALLATION_ DIRECTORY\<product_ name>\flexlm the lmtools.exe (for Hostname
and HostID for NUMECA as Computer/Hostname and Ethernet Address under the
System Settings tab).
l the product name and version for which installation is causing problems.
l a description of the configuration (in terms of name, Windows version, local or domain user).
l the debug.log file generated when starting the license service.
l the .out files in C:\tmp.
l the pvml.username in C:\tmp (or directory defined by the environment variable PVM_TMP).
2.2
LINUX
The user is strongly advised to consult the "Linux" (p. 8) system requirements prior to start any
installation. Troubles may indeed appear during the installation and configuration phases in case
the listed hardware and software requirements would not be fully satisfied.
Please do notice that the documentation package attached to NUMECA software is not installed
during the installation procedure and can be downloaded from the Products page of the Customer
Area of www.numeca.be.
In case of trouble: .
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
At the end of the "Troubleshooting" (p. 50) the information to provide is listed.
2.2.1
Installation
Install FINE™/Open with OpenLabs™ under Linux
1. Log in the workstation corresponding to the selected OS. It is strongly recommended not to
install the software as "root" or using the command "sudo" because the user may have no
permission to execute the software afterward. It is strongly recommended to check the
permission of the disk and directory the user will select for the software installation.
2. Check and make sure that the necessary disk space is available prior to starting the installation
process.
For the disk space requirements, see also: the "Linux" (p. 8) system requirements.
3. Get the installation package from the Products page of the Customer Area (www.numeca.be).
4. Check that the file can be accessed with full permission and extract it by typing the command
line: tar -xvf <package_name>.tar.
Do NOT extract the tar file in the target directory NUMECA_ INSTALLATION_
DIRECTORY in which the product will be installed.
5. Go to the directory containing the files extracted from the tar archive and type the command
./install_numeca <ENTER>.
The trusted storage based licensing requires a LSB compliant platform. After license agreement, a
check is performed to verify whether the host machine is LSB compliant. It is required if the
license server is installed on the host machine.
6. During the installation, the user will be asked to accept the terms of the License Agreement.
7. Enter the installation directory (referred to as NUMECA_INSTALLATION_DIRECTORY)
in function of one of the following scenarios:
l If NUMECA software was not installed before on the machine, choose a directory of your
preference. Providing a directory name that does not exist will create it automatically.
l If NUMECA software was already installed before, choose the same NUMECA_
INSTALLATION_DIRECTORY to use the multiple versions and/ or products in one
multi-version environment.
It is important to notice that a common NUMECA_INSTALLATION_DIRECTORY
should be shared by all NUMECA installations, otherwise the multi-version installation
will not be set up adequately. This is important e.g. for the good functioning of
PVM when launching several products or versions one after the other.
In order to run distributed memory parallel computations with OpenMPI, NUMECA
products must be installed in the same directory on different machines.
the old
If the product has not been installed in the same 'NUMECA_INSTALLATION_DIRECTORY'
/NUMECA_ INSTALLATION_
'add_ version.sh'
as
DIRECTORY/COMMON/ will allow the user to link previous versions by specifying their full
path name (e.g.: /usr/numeca_software/fineautogrid122).
product. The
script
in
8. Finally, the so-called 'HostName' and 'HostID' information required to generate a license file
will be shown. This information should be sent to NUMECA local sales or support office.
Alternative to find the HostName and HostID from the Administration Tool
From the home page, the 'HostName' and 'HostID' can be found at the License Management
-> License server status tab (available in Advanced mode).
Alternative to find the HostName and HostID from a shell
Type the commands:
NUMECA_INSTALLATION_DIRECTORY/<product_
name>/LINUX/install/flex64/lmutil lmhostid -hostname <Enter>
and
NUMECA_INSTALLATION_DIRECTORY/<product_
name>/LINUX/install/flex64/lmutil lmhostid <Enter>.
9. After the package is installed, the NUMECA Administration Tool is launched automatically.
This is a tool for license management and provides a graphical user interface for the
management of the license server and client machines. The tool offers a guide through the
process of setting up and configuring a license server.
Alternative to access the Administration Tool
After installation, the Administration Tool can also be started through the command admin#,
where # is the software version (e.g. admin72). Click on Finish to leave the tool and to finalize
the installation.
Tasks that can be performed in the NUMECA Administration Tool
l License Management: to configure the machine as license server and/ or client.
l User Configuration: to set the PATH in the .bashrc/.cshrc/.profile files.
l Network Configuration: to clean and reinitialize PVM, to setup SSH connections to other
machines/ users.
l Diagnostics: to assess and fix problems with license management and graphics.
10. When receiving the license file from NUMECA, perform the license management and user
configuration:
l "License management" (p. 38)
l "User Configuration" (p. 44)
Launch the software as described in the user guide of your product while taking into account
the points of attention as listed in the "Software launch" (p. 47) section of the Linux user
configuration.
2.2.2
License management
Introduction
Before using NUMECA software, a valid floating license is required.
What is a floating license?
With a floating license each software component is managed by an independent maximum
number of concurrent accesses (number of processes). Floating licenses are managed by a license
server which checks if process access is free. If so, when launching a software component, license
access is given to the user process or access is denied otherwise. The license can be accessed on
the same computer but also on other computers (clients) with Linux or Windows, connected
through a network to the license server. The license server can be a Linux or a Windows
machine.
Important points of attention for license servers:
l NUMECA updates the security ID of license files with each major release. License files
with old security ID cannot be used with the latest NUMECA software. Please send your
old license file to NUMECA local sales or support office for an upgrade of the license file.
l Redundant license server can be delivered allowing to manage a floating license by several
servers. For more information, contact NUMECA local sales or support office.
l Machines used as license server must have a fixed first IP address. For example, when
using VPN on Windows, VPN will become the first network interface. In this case, the
license server will not work properly.
l By default it is not possible to use a virtual machine as a license server. To install a license
server on a virtual machine, contact your account manager.
l FlexLM requires LSB (Linux Standard Base) compliant OS.
NUMECA software must be installed on the license server. At the end of the installation, the
license information (the HostName and HostID of this computer) must be sent to NUMECA local
sales or support office in order to get a license file.
Before using NUMECA software, the license daemon should be configured on the license server.
To set up the license server it is necessary to prepare the license file and launch the server either
though the NUMECA Administration Tool or in a shell.
Access to the NUMECA Administration Tool
At the end of the installation of NUMECA software the Administration Tool is launched
automatically.
It can also be started anytime on Linux using the command: admin#, where # is the software
version.
It is recommended to run the Administration Tool as root to fully benefit from all possibilities of the
Administration Tool.
Example
adminopen72
Prepare the license file
To install the license service take the following steps:
1. Rename the license file as license.dat.
2. Copy the license.dat file in the directory that all users are able to access.
3. Check that the license file has the read- execute access privileges (execute chmod 755
license.dat).
The "license.dat" file must be readable by each user.
When using a TCP port for the license server, the port number has to be added in the license file on
the server/vendor line:
1. SERVER hostname hostid and VENDOR numeca should be replaced by SERVER
hostname hostid portnumber1 and VENDOR numeca portnumber2;
2.
3.
reread the license file,
start NUMECA software and specify the license server writing portnumber@hostname . All
specified ports should be opened and free.
License set-up in NUMECA Administration Tool
Start floating license service
To start the license service:
1. Select License Management.
2. On the line Activate from license file browse to the license file.
3. Click on Apply.
Automatic start at machine boot
After the manual start of the license service, it is possible to have it automatically start at machine
boot:
1. In License management click on the Advanced button.
2. Go to the License server tab.
3. Press the Set autostart server button.
When starting the license service through the NUMECA Administration Tool, it uses the cron
daemon of the user who installs the software to define the automatic start of the license at machine
boot. Cron is a daemon used to schedule various kind of tasks on Linux. This tool uses crontab
text files that specify commands/ tasks to run at certain time intervals. In the case of NUMECA
Administration Tool, the cron daemon automatically starts the license service using the license file
(s) or existing server specified in the previous license server set-up. In absence of a previous set-
NUMECA_ INSTALLATION_
up,
DIRECTORY/flexlm/any.lic as the license server file location for the autostart.
daemon
dummy
address
uses
the
the
Verify license service status
To verify that the license server is correctly running do the following:
1. From the NUMECA Administration Tool home page, click on License Management .
2. Click on the Advanced button at the bottom of the Activate Product tab.
3. Select the License server status tab.
4. Select the license server on the left-hand side drop down menu.
5. Information regarding the available features, the number of available licenses and the number
of used licenses is shown under the License server info section.
Floating license on Linux client
When a floating license service is installed on a license server, this license service may be used by
other computers with a network connection to the license server. In this section, it is assumed that
the license server is running.
1. Go to the NUMECA Administration Tool home page,
2. click on License Management,
3. select the Activate Product tab,
4. select the Activate from existing server option.
Users willing to launch NUMECA software on a client should perform a user configuration on
this machine before first use as described in the section "User Configuration" (p. 44).
Update of license file
When a license file is expired, contact NUMECA local sales or support office to obtain an
updated license file.
Replace the active license file license.dat with the update license provided by NUMECA
(renamed as license.dat).
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
1. Go to the NUMECA Administration Tool home page, click on License Management .
2. Click on the Advanced button at the bottom of the Activate Product tab.
3. Select the License server tab.
4. Click on the Re-read license button.
5. The words "SUCCEEDED" or "Failed" are shown depending on the update success or
failure, respectively.
If the version of the Flexlm tool is upgraded or the version of the license file security ID is
upgraded, an update of the license file is not sufficient. The user must shutdown the running
license server and start a new license server with the latest Flexlm tool and the latest license file.
Alternative license server set-up from a shell
Start of the license service
To start the license daemon manually, do the following operations:
1. Go
to
directory
the
name>/LINUX/install/flex64/
NUMECA_ INSTALLATION_ DIRECTORY/<product_
2. Execute
./lmgrd
DIRECTORY/COMMON/license.dat -l $HOME/.numeca/debug_numeca.log
command:
the
NUMECA_ INSTALLATION_
-
In these lines, 'NUMECA_INSTALLATION_DIRECTORY' should be replaced by the absolute
directory path where you have installed NUMECA software.
The manual start operations must be repeated each time the server machine is rebooted.
Automatic start at machine boot
The license daemon can be automatically started during the workstation boot process. For
example to do so on LINUX Red Hat Enterprise 5.1:
1. Login as "root"
2. Go to the /etc directory
3. Edit the inittab file
4. Add the following line at the end:
lmgr:35:wait:/NUMECA_INSTALLATION_DIRECTORY/<product_
name>/LINUX/install/flex64/lmgrd -c License_path/license.dat
In this line, 'NUMECA_INSTALLATION_DIRECTORY' should be replaced by the absolute
directory path where you have installed NUMECA software, 'License_path' should be replaced
by the absolute directory path where the license file is located.
The license server can also be started from /etc/rc#.d/. For more information contact your system
administrator or NUMECA local sales or support office.
Verify License Service Status
To verify that the license server is correctly running do the following:
1. Go to the directory:
NUMECA_INSTALLATION_DIRECTORY/<product_name>/LINUX/install/flex64/
2. Execute the command: ./lmutil lmstat -c License_path/license.dat
If the license server is up this will be shown in the shell with the words: "license server UP
(MASTER) v11.13". The vendor daemon numeca needs to be up as well as indicated with the
words: "Vendor daemon status (on license_server_machine_name): numeca: UP v11.13
If the license server or vendor daemon is not up see: "User Configuration" (p. 44).
3. To display the active users of a given feature, use the following command: ./lmutil lmstat -a -c
License_path/license.dat
Floating license on Linux client
When a floating license is installed on a license server, this license may be used by other
computers with a network connection to the license server. In this section, it is assumed that the
license server is running.
On a Linux client, the path of the NUMECA_ LICENSE_ FILE should be defined in the
~/.flexlmrc file:
l in csh or tcsh shell:
setenv NUMECA_LICENSE_FILE /full-path/license.dat or @servername
l in bash or korn shell:
NUMECA_LICENSE_FILE=/full-path/license.dat or @servername
export NUMECA_LICENSE_FILE
Users willing to launch NUMECA software on a client should perform a user configuration on
this machine before first use as described in section "User Configuration" (p. 44).
Update of license file
When a floating license file is expired, contact NUMECA local sales or support office to obtain
an updated license file and follow the instructions below.
1. Rename the license file to license.dat.
2. Replace the active license file with the updated provided license on license server.
It is strongly suggested to make a backup of the old license file, for safety, by renaming it to
"license.old".
3. Go to the directory
NUMECA_INSTALLATION_DIRECTORY/<product_name>/LINUX/install/flex64/
4. Execute the command:
./lmutil lmreread -c LICENSE_FULL_PATH/license.dat
If the version of the Flexlm tool is upgraded or the version of the license file format is upgraded, an
update of the license file is not sufficient. The user must shutdown the running license server and start
a new license server with the latest Flexlm tool and the latest license file.
Optional: ask software to wait for license
request
that NUMECA products wait
in
To
/home/user/.numeca/preferences.dat using the keyword LICENSE_WAIT. This functionality is
available for all products.
license,
define
active
for
an
it
Example
PRODUCT FINE/Open
LICENSE_WAIT
END_PRODUCT
Student version with activation ID
In general a license certificate (text file) is provided to give access to NUMECA software.
Alternatively the NUMECA Administration tool allows to use an activation ID to start the license
server. For example, the free student version is based on an activation ID and the instructions how
to use it are provided together with the activation ID. Use of an activation ID requires the use of
Trusted storage and installation of an anchor service. Hence this terminology can be found in the
NUMECA Administration Tool but can be safely ignored in case of a license certificate in text
file format.
Example of an Activation ID: C2a9-561f-7895-435b-acb5-3520-c166-4bcc
2.2.3
User Configuration
Introduction
At the end of the installation, each user willing to use NUMECA software must initially configure
his/ her working environment by running an initialization script.
Configure the user environment
1. Log in as user.
2. Go to the directory NUMECA_INSTALLATION_DIRECTORY/COMMON, and execute
the command ./configure. This operation will add a couple of lines in the user's .cshrc, .tcshrc
or .profile file (located in user's home directory) and add the NUMECA software in user's
default path.
3. Log out and log in again to apply the information in the .cshrc , .tcshrc or .profile file.
On Linux, NUMECA software saves some data (preferences, user fluid database, templates...) in the
folder $HOME\.numeca\. The variable $HOME is imposed by NUMECA software and cannot be
modified.
During the runtime, NUMECA software writes temporary data in the directory $HOME/.numeca/tmp.
This tmp directory can be redefined by defining the environment variable NI_TMP_DIR.
Optional: configure account to allow remote computations
When configuring the FINE™ environment for remote computations, it is strongly advised to
suspend all currently running tasks and shutdown the PVM daemon before starting the
configuration.:
1. Start the Task Manager (Modules/Task Manager) from the FINE™ GUI and select the
Hosts definition page in the menu on the left.
2. Click on the button Shutdown. A warning message will appear stating that all hosts will be
removed from the Virtual Machine and that FINE™ GUI will be closed. Click on yes to
continue.
RSH
FINE™ enables to launch computations on remote machines by using the Task Manager
capabilities. To be able to perform remote launches using rsh command, NUMECA software
must be installed on the remote machine and explicit permission must be specified in the dedicated
.rhosts file, located in the user's home directory. To this end, the following operation must be
checked and/ or performed:
1. Edit the .rhosts file and check information describing the list of computer and user authorized
to use the Task Manager. Example of .rhosts file:
computer1 user1 computer2 user1 computer3 user1
2. Check the permission of the .rhosts file (600 is required).
3. Check that the rsh command is active on all machines listed in the .rhosts file. This can be
done by typing the command rsh machine_name and checking that no password is requested.
If the system keeps requesting a password, please verify that the previous steps have been
correctly followed or contact your system administrator. Please note that the rsh command is
not available on HP and should better be replaced by the remsh command.
4. Check that the rlogin command allows user to login on all machines listed in the .rhosts file,
without requiring any password information. Providing these few tests are successful, the Task
Manager is ready to use.
Use of NUMECA software with other applications that would require an access to PVM can lead to
conflicts. Contact NUMECA local sales or support office for more information.
SSH
FINE™ enables to launch computations on remote machines by using the Task Manager
capabilities. To be able to perform remote launches using ssh command, NUMECA software
must be installed on the remote machine and the environment variable "NI_RSHCMD" should be
set to "ssh":
l in csh or tcsh shell:
setenv NI_RSHCMD ssh
l in bash or korn shell:
export NI_RSHCMD=ssh
and explicit permission must be specified in the dedicated ~/.ssh/authorized_keys file. To this
end, the following operations must be checked and/ or performed:
l In a shell, the command ssh-keygen -t dsa will generate in the directory ~/.ssh two files, one
private key and one public key.
l Check the permission of the private key (600 is required).
l The public key can be put on the other machine in the ~/.ssh/authorized_keys file.
The permissions on the file must be very strict:
l chmod 750 ~/
l chmod -R 700 ~/.ssh
Use of NUMECA software with other applications that would require an access to PVM can lead to
conflicts. Contact NUMECA local sales or support office for more information.
Software launch
When launching the FINE™ environment, the user should note:
l It is not allowed for one user to simultaneously open (and therefore launch tasks in) more than
one FINE™ environment with different versions.
l In a multi-version environment, it is strongly suggested to shutdown the Task Manager when
switching from version to version, in order to avoid possible conflicts due to the PVM
daemon. This warning only applies if the versions have been installed in distinct NUMECA_
INSTALLATION_DIRECTORY locations.
To launch the components:
<productname><version#> -print <Enter>
Examples
For FINE™/Open with OpenLabs™: fineopen72-print <Enter>
For CFView™: cfviewopen72 -print
For HEXPRESS™: hexpress72-print <Enter>
For HEXPRESS™/Hybrid: hexpresshybrid72-print <Enter>
It is important to outline that no output is displayed by default in the shell where the software is
launched. Instead the output is redirected to log files, located in the directory ~/.numeca/tmp/ and
named as startup_logfile_fine, startup_logfile_hexpress, startup_logfile_cfview.
However, outputs can still be forced for display in the shell. Add the - print command to the
command line. This will give additional information during software launch, especially during the
initial configuration of the software.
2.2.4 Uninstallation
Introduction
This section details the steps required to properly remove an installation of NUMECA software.
Depending upon the configuration, there are several possibilities:
l If the product is the only product and the only version on the computer: uninstall in mono-
version environment.
l If other products and/ or other versions are installed on the same machine, it is possible to: 
l to remove only some of these products/ versions: partly uninstall
in multi- version
environment",
l to remove all products: fully uninstall in multi-version environment".
Furthermore, the license service may be stopped if NUMECA software is not used on any
machine connected to the license server.
Uninstall License Service
Points of attention:
l Instructions related to the NUMECA license service must be removed if the machine has
been configured to start automatically the license service at start up. These instructions can
be accessed in the /etc/inittab file.
l It is not possible to stop the license server without an internet connection.
l The license server cannot be started or stopped without a network connection.
In NUMECA Administration Tool
1. From the NUMECA Administration Tool home page, click on License Management,
2. Click on the Advanced button at the bottom of the Activate Product tab.
3. Select the License server tab.
4. Click on the Stop license server button to stop the specified license server.
5. The words "SUCCEEDED" or "Failed" are shown depending on the success or failure of the
uninstalling process, respectively.
6. Click on the Remove from autostart button to complete the uninstalling process.
In a shell
The license service should be stopped before uninstalling NUMECA software.
To do so, the following operations must be performed:
1. Go
to
directory
the
name>/OSname/install/flex#/
NUMECA_ INSTALLATION_ DIRECTORY/<product_
2. Execute the command: ./lmutil lmdown -c LICENSE_FULL_PATH/license.dat
Close PVM
FINE™ environment uses PVM. Before uninstalling FINE™, the PVM process must be closed.
This can be done as follows:
1. Start the Task Manager (Modules/Task Manager) from the FINE™ GUI and select the
Hosts definition page in the menu on the left.
2. Click on the button Shutdown. A warning message will appear stating that all hosts will be
removed from the Virtual Machine and that FINE™ GUI will be closed. Click on yes to
continue.
Uninstall in mono-version environment
Proceed as follows to remove a product in a mono-version environment under Linux:
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in the subsection
"Uninstall License Service" (p. 48).
3. Remove the lines from "#begin NUMECA configuration" to "#end NUMECA configuration"
from the user's .cshrc, .tcshrc or .profile file.
4. Remove the directory NUMECA_INSTALLATION_DIRECTORY and its content.
Partly uninstall in multi-version environment
Proceed as follows to remove one product version in a multi-version environment under Linux:
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in the subsection
"Uninstall License Service" (p. 48) .
3. Remove the directory NUMECA_INSTALLATION_DIRECTORY/<product_name>/ and
all of its content.
Before removing the directory NUMECA_INSTALLATION_DIRECTORY/<product_name>/, check
and make sure that the license file is not inside the directory.
Fully uninstall in multi-version environment
Proceed as follows to remove all NUMECA products in a multi-version environment under
Linux:
1. Verify that there are no running tasks on the machine.
2. Stop the license service before uninstalling NUMECA software. More details in the subsection
"Uninstall License Service" (p. 48).
3. Remove the lines from "#begin NUMECA configuration" to "#end NUMECA configuration"
from the user's .cshrc, .tcshrc or .profile file.
4. Remove the directory NUMECA_INSTALLATION_DIRECTORY and its content.
2.2.5
Troubleshooting
Introduction
In most cases, a straightforward and careful execution of the instructions detailed in the previous
chapters enables the user to start NUMECA software smoothly. In case of problems, this section
aims at providing guidelines on how to detect and solve possible troubleshooting.
FINE™/Open with OpenLabs™ not starting
In case FINE™/Open with OpenLabs™ fails to start, use the -print argument in the command
line, for example cfviewopen72 -print to start the product.
This argument will output information in the shell (including the location of the license file) which
may be helpful to understand the problem. With this information at hand, check the following
items:
l Is the license file valid and active to start the product ?
l Check if the license server is up. On the license server, two active daemons should be present.
This can be seen using the commands ps -ealf | grep lmgrd and ps -ealf | grep numeca. If not,
follow the instructions for license installation.
l Some license check problems may occur if the host computer cannot find the server IP-address
corresponding to the hostname information included in the first line of the license key. To
solve this problem, replace the hostname by the IP-address of the license server. This operation
does not invalidate the license key.
l Check if the license key file is well readable by every user.
l Did the user configure the working environment? Before using NUMECA software, each user
must configure the working environment using the command ./configure within the
NUMECA_INSTALLATION_DIRECTORY/COMMON/ directory; then log out and log in.
l Is the graphics driver appropriate for the display ? Try to activate the X11 driver.
To change the used driver
To change the driver permanently for every next launch of the software:
1. Open the file ~\.numeca\.drivers
2. Type: host_ name display_ name possible_ drivers chosen_ driver e.g. gauss.numeca.be
gauss OPENGL:X11 X11
The selection will take effect at the next session.
Alternatively, the driver can be manually specified in a shell for that shell session only through
the following commands:
l in csh or tcsh shell:
setenv NI_DRIVER X11
l in bash or korn shell:
NI_DRIVER=X11 export NI_DRIVER
l Check if the TCP/IP protocol is installed on the machine. The protocol is mandatory to ensure
the correct function of the floating licenses.
l Are the NUMECA software components visible from the machine? If not, install them.
l Is the OS adequate? If not, copy the correct tar file and start the installation again.
l Are the Linux permissions sufficient for the user to access NUMECA software installed? Ask
your system administrator.
l Successive installation of FINE™ can possibly lead to trouble if tasks have been improperly
stopped. To purge this issue:
Close all tasks opened (including FINE™ GUI) and kill the PVM daemon related to the user
(if applicable). This operation can be performed through the kill command applied to the
corresponding process number. Process numbers can be outlined using the command ps -ef |
grep pvm. This operation must be performed on each machine the user can possibly access.
Graphical problems and system crashes
NUMECA software makes use of the advantages of Graphics Card available. Some trouble may
however come up with the default driver OPENGL since it may not be supported by the user host
computer and machine display.
In order to set the system compatible with a more portable driver, refer to the following
instructions. Note however that the proposed drivers are usually less efficient in terms of graphical
speed than the default driver.
To change the used driver
To change the driver permanently for every next launch of the software:
1. Open the file ~\.numeca\.drivers
2. Type: host_name display_name possible_drivers chosen_driver e.g. gauss.numeca.be gauss
OPENGL:X11 X11
The selection will take effect at the next session.
Alternatively, the driver can be manually specified in a shell for that shell session only through the
following commands:
l in csh or tcsh shell:
setenv NI_DRIVER X11
l in bash or korn shell:
NI_DRIVER=X11 export NI_DRIVER
GUI flashes
In some circumstances, the graphical area can flash during interactive operations, depending upon
the driver selected. This mostly happens when using the X11 driver. Setting the environment
variable NI_DOUBLEBUFFERING to ON into the user profile (.cshrc, .profile, .tcshrc,...)
may solve the problem under Linux. The variable can be manually specified through the
following commands:
l for csh or tcsh shells: setenv NI_DOUBLEBUFFERING ON
l for
bash
korn
DOUBLEBUFFERING
or
shells:
NI_ DOUBLEBUFFERING=ON
export
NI_
Display drivers not detected
NUMECA products with GUI check the available working drivers and updates automatically in
the .drivers file located in the .numeca directory of the user at first launch on a new machine/
display. This operation is only completed during the first execution, since it may take some time.
As a consequence, the upgrade of drivers on an existing machine/ display cannot be automatically
detected.
Cannot connect to other hosts
At first execution of Task Manager
In case the user cannot connect to other hosts at the first execution of the Task Manager, the
following should be checked:
l Is the machine included in the computer list within the .rhosts file (when running remote
commands with rsh)? This file details the computers authorized to use the Task Manager. The
file is located in the user home directory.
Example of .rhosts file
computer1 user1 computer2 user1 computer3 user1
l Has the .rhosts adequate permission (when running remote commands with rsh)? (600 is
required)
l Is NUMECA software adequately installed on the selected remote hosts? If not, perform the
installation.
l Is the rsh command active on all machines listed in the .rhosts file? This check can be done by
typing the command line rsh machine_name echo \$PVM_ROOT <Enter>. All selected
machines must be accessed without requiring any password information and the $PVM_
ROOT variable should be displayed adequately. Please note that the rsh command is not
available on HP and should better be replaced by the remsh command.
l Is the user .cshrc, .tcshrc or .profile file fully executed when opening a new batch shell (non
interactive mode)? Ask your system administrator to check this issue.
Task Manager launched once with success
In case the user can no longer connect to other hosts while this operation has at least been
successful once, the following should be checked:
1. Start the Task Manager (Modules/Task Manager) from the FINE™ GUI and select the
Hosts definition page in the menu on the left.
2. Click on the button Shutdown. A warning message will appear stating that all hosts will be
removed from the Virtual Machine and that FINE™ GUI will be closed. Click on yes to
continue.
3. Close all tasks opened (including FINE™ GUI) and kill the PVM daemon related to the user
(if applicable). This operation can be performed through the kill command applied to the
corresponding process number. Process numbers can be outlined using the command ps -ef |
grep pvm. This operation must be performed on each machine the user can possibly access.
Further troubleshooting
For more information and troubleshooting:
l consult the forum in NUMECA's Customer Area with a section dedicated to installation.
l or contact NUMECA local sales or support office (for active maintenance plans only).
To help to find a solution within the shortest delays, please provide a detailed description of the
observed behavior and performed analysis.
The following information can be helpful:
l the license key file license.dat.
l the hostname and hostid. This information can be obtained by launching the NUMECA
Administration tool (starting through the command admin) or by executing the commands
lmutil
lmhostid <Enter> in the NUMECA_
INSTALLATION_DIRECTORY/<product_name>/LINUX/install/flex64/ directory.
lmhostid - hostname <Enter> and lmutil
l the product name and version for which installation is causing problems.
l a description of the configuration (in terms of name, platform and OS for each machine on
which NUMECA software is installed).
l the .log file generated during the installation and located in the /tmp directory on the machine
from where the script ./install_numeca has been launched .
l the "startup_logfile_*" files located in ~\.numeca\tmp.
© NUMECA International, all rights reserved
EN201805181138