Clifford A. Brown

Glenn Research Center, Cleveland, Ohio

Ray Hixon

University of Toledo, Toledo, Ohio

Effect of Turbulence Modeling on an Excited Jet

NASA/TM—2010-216768

September 2010

AIAA–2009–3191
NASA STI Program . . . in Profi le

Since its founding, NASA has been dedicated to the 

advancement of aeronautics and space science. The 

NASA Scientifi c and Technical Information (STI) 

program plays a key part in helping NASA maintain 

this important role.

The NASA STI Program operates under the auspices 

of the Agency Chief Information Offi cer. It collects, 

organizes, provides for archiving, and disseminates 

NASA’s STI. The NASA STI program provides access 

to the NASA Aeronautics and Space Database and 

its public interface, the NASA Technical Reports 

Server, thus providing one of the largest collections 

of aeronautical and space science STI in the world. 

Results are published in both non-NASA channels 

and by NASA in the NASA STI Report Series, which 

includes the following report types:

• TECHNICAL PUBLICATION. Reports of 

completed research or a major signifi cant phase 

of research that present the results of NASA 

programs and include extensive data or theoretical 

analysis. Includes compilations of signifi cant 

scientifi c and technical data and information 

deemed to be of continuing reference value. 

NASA counterpart of peer-reviewed formal 

professional papers but has less stringent 

limitations on manuscript length and extent of 

graphic presentations.

• TECHNICAL MEMORANDUM. Scientifi c 

and technical fi ndings that are preliminary or 

of specialized interest, e.g., quick release 

reports, working papers, and bibliographies that 

contain minimal annotation. Does not contain 

extensive analysis.

• CONTRACTOR REPORT. Scientifi c and 

technical fi ndings by NASA-sponsored 

contractors and grantees.

• CONFERENCE PUBLICATION. Collected 

papers from scientifi c and technical 

conferences, symposia, seminars, or other 

meetings sponsored or cosponsored by NASA.

• SPECIAL PUBLICATION. Scientifi c, 

technical, or historical information from 

NASA programs, projects, and missions, often 

concerned with subjects having substantial 

public interest.

• TECHNICAL TRANSLATION. Englishlanguage translations of foreign scientifi c and 

technical material pertinent to NASA’s mission.

Specialized services also include creating custom 

thesauri, building customized databases, organizing 

and publishing research results.

For more information about the NASA STI 

program, see the following:

• Access the NASA STI program home page at 

http://www.sti.nasa.gov

• E-mail your question via the Internet to help@

sti.nasa.gov

• Fax your question to the NASA STI Help Desk 

at 443–757–5803

• Telephone the NASA STI Help Desk at

 443–757–5802

• Write to:

 NASA Center for AeroSpace Information (CASI)

 7115 Standard Drive

 Hanover, MD 21076–1320
Clifford A. Brown

Glenn Research Center, Cleveland, Ohio

Ray Hixon

University of Toledo, Toledo, Ohio

Effect of Turbulence Modeling on an Excited Jet

NASA/TM—2010-216768

September 2010

AIAA–2009–3191

Prepared for the 

15th Aeroacoustics Conference (30th AIAA Aeroacoustics Conference)

cosponsored by AIAA and CEAS

Miami, Florida, May 11–13, 2009

National Aeronautics and

Space Administration

Glenn Research Center

Cleveland, Ohio 44135
Available from

NASA Center for Aerospace Information

7115 Standard Drive

Hanover, MD 21076–1320

National Technical Information Service

5301 Shawnee Road

Alexandria, VA 22312

Available electronically at http://gltrs.grc.nasa.gov

This work was sponsored by the Fundamental Aeronautics Program 

at the NASA Glenn Research Center.

Level of Review: This material has been technically reviewed by technical management. 
NASA/TM—2010-216768 1 

Effect of Turbulence Modeling on an Excited Jet 

Clifford A. Brown 

National Aeronautics and Space Administration 

Glenn Research Center 

Cleveland, Ohio 44135 

Ray Hixon 

University of Toledo 

Toledo, Ohio 43606 

Abstract 

The flow dynamics in a high-speed jet are dominated by unsteady turbulent flow structures in the 

plume. Jet excitation seeks to control these flow structures through the natural instabilities present in the 

initial shear layer of the jet. Understanding and optimizing the excitation input, for jet noise reduction or 

plume mixing enhancement, requires many trials that may be done experimentally or computationally at a 

significant cost savings. Numerical simulations, which model various parts of the unsteady dynamics to 

reduce the computational expense of the simulation, must adequately capture the unsteady flow dynamics 

in the excited jet for the results are to be used. Four CFD methods are considered for use in an excited jet 

problem, including two turbulence models with an Unsteady Reynolds Averaged Navier-Stokes 

(URANS) solver, one Large Eddy Simulation (LES) solver, and one URANS/LES hybrid method. Each 

method is used to simulate a simplified excited jet and the results are evaluated based on the flow data, 

computation time, and numerical stability. The knowledge gained about the effect of turbulence modeling 

and CFD methods from these basic simulations will guide and assist future three-dimensional (3–D) 

simulations that will be used to understand and optimize a realistic excited jet for a particular application. 

Introduction 

The flow dynamics in a high-speed jet are dominated by the unsteady turbulent flow structures that 

characterize the energy cascade in the jet plume. These flow structures, which range in size from largescale eddies on the order of the jet diameter that transport energy to the extremely small-scale eddies that 

dissipate energy through viscous forces, originate in the naturally unstable free-shear boundary layer 

formed between the high-speed jet flow and the surrounding fluid. As the fluids mix in the jet plume, 

Kelvin-Helmholtz instability waves are formed. These instability waves grow and decay as the jet 

develops, governing the formation and destruction of the unsteady turbulent flow structures. Jet excitation 

must exploit these natural instabilities to exert control on the turbulent structures or the energy of the jet 

will overwhelm the input perturbation. If perturbations are input at the nozzle exit impact the jet where 

the flow structures are smaller and less energetic, then large changes to the to the jet flow downstream can 

be created with a relatively small energy input. Moreover, the downstream characteristics of the jet plume 

can be predetermined by selecting an appropriate instability wave (mode and frequency) to amplify with 

the input perturbation. 

Jet excitation has many potential uses. It may be used to reduce the thermal signature of the jet or to 

mitigate the noise generated. Proper excitation, however, requires intelligently selecting the best 

excitation input from the infinite number of possibilities to optimize the effect. Modern experimental 

techniques, such as particle image velocimetry and phased array microphones, can provide detailed flow 

and acoustic information that could be used to optimize the excitation but these experiments are too costly 

for the large number of cases required for a true optimization, especially at the larger and more realistic 

facilities. Numerical simulations can provide a cost effective alternative to experiments for optimizing the 

excitation input, leaving only the best cases to be confirmed using experiments. 
NASA/TM—2010-216768 2 

Direct Numerical Simulations (DNS) solve the compressible Navier-Stokes equations to calculate the 

complete history of a flow without modeling assumptions. In a DNS calculation, all time- and lengthscales are resolved throughout the flow, necessitating very small time steps and very fine grid spacing. 

This limits the use of DNS for a realistic high Reynolds number jet flow because resolving the wide range 

of time- and length-scales between the nozzle boundary layer and the turbulent eddies in the plume 

quickly becomes computationally overwhelming. Thus, part or all of the unsteady turbulent flow cannot 

be directly simulated and the unresolved flow must be modeled. As more of the flow is modeled rather 

than resolved, the computational effort is reduced but at a cost; the solution becomes more dependent of 

the modeling assumptions. It is necessary, therefore, to understand the methods and assumptions used in 

the simulations in order to balance quality of the result with the computational expense required. 

A jet excitation test case has been developed to study the advantages and disadvantages of four 

common turbulent flow simulation models. The simulation results for these test cases are not intended to 

exactly recreate experimental results but rather to provide a basis, at minimal computational expense, 

from which to choose the best method for future simulations and to intelligently begin these future 

simulations with some knowledge of the grid and time resolution required to achieve more accurate 

results. Although the NASA Fundamental Aeronautics Program, under the Supersonics project, is 

supporting this research with the goal of developing the next generation of technology to reduce the 

environmental impact of noise around airports with minimal impact of engine performance, the 

knowledge gained from these simulations can be applied to any application of jet excitation. 

The Problem—Jet Excitation 

Jet excitation amplifies instabilities naturally present in a jet to alter the downstream development of 

the jet. Actuators are used, typically at or near the nozzle exit to excite these instabilities. Historically, 

many different actuators have been used to in excitation experiments, including loudspeakers, air 

injection, and synthetic jets. More recently, the Localized Arc Filament Plasma Actuators (LAFPA) have 

shown considerable promise as high amplitude, high frequency flow actuators (Refs. 1 and 2). Developed 

at Ohio State University, the LAFPA use a high temperature spark to generate a shock wave that impacts 

the jet flow at the nozzle exit. These actuators are a good test of the CFD methods for a couple of reasons. 

First, the on or off nature of the LAFPA spark challenge the numerical stability of the CFD method. 

Second, the sharp gradients generated offer a real test of the codes ability to propagate waves through the 

flow. Implementing the LAFPA actuators into a CFD code, however, is another issue. 

The LAFPA uses high voltage electronics to rapidly heat the air at multiple locations near the nozzle 

exit to create the plasma. Electricity is fed to two electrodes periodically causing a spark to jump across 

the tips and ionize the air forming plasma. The electrodes are recessed in a small cavity to prevent the 

flow from blowing the spark off before it can heat the air. At this point, there are three primary forces 

working in the plasma. The electrohydrodynamic (EHD) and magnetohydrodynamic (MHD) forces, 

which are created by the interactions of charged particles within the plasma, and Joule heating effects, 

which are created by the rapid heating of air in and around the actuator (Ref. 3). Research shows that the 

impact of the EHD and MHD forces is limited in high-speed flows and that Joule heating is the primary 

forcing mechanism in the LAFPA (Ref. 3). Schlieren measurements have supported this conclusion by 

showing that the shock waves generated by the rapid heating behave similar to small surfaces periodically 

inserted in the flow (Refs. 4 and 5). Although there are several ways this type of actuator could be 

modeled in a CFD solver, perhaps the simplest is to stop the solver and reset the flow values in the 

actuator cavity to simulate the high temperature and pressure created by the actuator. This makes the 

actuator operate on a time scale that is not resolved by the CFD solver as it turns on and off 

instantaneously. Temperature was used as the control variable and, based on emission spectroscopy 

measurements (Ref. 3) and prior simulations (Ref. 6), was set at Ta = 1000 C. Further simplifying the 

model, the temperature and pressure in the actuator are related by the ideal gas law (density is constant 

because the actuator operates instantaneously so mass can not enter or leave the actuator). While this is a 

significant assumption as the air in the actuator cavity is not an ideal gas under these conditions, the point 
NASA/TM—2010-216768 3 

of these simulations is not to exactly reproduce experimental results but to learn about simulating excited 

jets. The ideal gas relation is a convenient starting point that can be adjusted in future simulations to more 

closely replicate an experimental setup. 

The nozzle simulated is a simplified version of the nozzle used at OSU (Fig. 1). This geometry was 

selected because most of the data available with the LAFPA actuators was acquired using this nozzle at 

OSU. This jet, which has an exit diameter (Dj) of 1-in., is also relatively small so excitation frequencies 

around the peak jet instabilities (Stourhal number based on jet diameter, StDj0.3) are higher than on a 

larger jet reducing the number of time steps needed to simulate one cycle. The geometry was simplified 

by making the external surface of the nozzle a straight line, removing the corners and cavities that would 

require many grid points to resolve but do not significantly contribute to the solution given the thickness 

of the nozzle lip. In fact, preliminary simulations indicated that this external surface could be treated as an 

inviscid wall, removing still more grid points that would be required to resolve a viscous boundary layer, 

without affecting the flow solution. 

The jet conditions for all the baseline (no actuator) and excited jet simulations were run with an 

acoustic Mach number (Ma = Vjet/cambient) Ma = 0.9, cold jet exit flow. These conditions were used to 

ensure a high-speed, high-energy jet without the added complications of a supersonic jet (i.e., shock 

cells). Only the axisymmetric azimuthal mode (m = 0) can be excited in a 2–D or axisymmetric 

simulation, so it was the targeted mode in all the simulations. The excitation frequency used in each case 

was near the preferred jet frequency of StDj0.3, which is approximately 4 kHz for this nozzle and flow 

conditions and where the jet should be the most responsive to the actuator perturbations. 
NASA/TM—2010-216768 4 

Solvers and Turbulence Models 

Computational fluid dynamics (CFD) is commonly used to simulate all different kinds of fluid flow. 

The jet problem combines near wall flow, requiring some resolution of a boundary layer with small time 

and length scales, and free shear flow, where the large-scale flow structures and turbulent energy 

dissipation requires both large and small time and length scales. The most complete CFD method, Direct 

Numerical Simulation (DNS), solves the complete compressible Navier-Stokes equations in threedimensions (3–D) without any modeling assumptions. This requires that all turbulent time and length 

scales be resolved throughout the flow, necessitating small time steps and very fine grid spacing and 

effectively limiting the use of DNS to low Reynolds number flows in limited spatial domains. To simulate 

more realistic problems, assumptions about the flow physics must be made and models applied to cover 

the regions excluded by these assumptions. Typically, solvers separate the flow into large and small 

scales, based either on time or space, and assume that the large scales dominate the flow. The large scales 

are then computed while the small scales are modeled or filtered significantly reducing the required 

computation time at the expense of some detailed flow information. 

The Reynolds Averaged Navier-Stokes (RANS) method separates the flow variables in time into 

time-averaged (mean flow) and fluctuating (turbulence) parts. The mean flow is then solved directly and 

the effect of the flow unsteadiness is accounted for by using a turbulence model. Therefore, in a RANS 

type solver, the turbulence model has the critical role of accounting for all the turbulent unsteady flow 

energy. In a jet, this means that the turbulence model is responsible for dissipating energy from the largest 

turbulent eddies down to the fine scale turbulence as the jet mixes with the ambient flow. 

A time accurate variant of the RANS method, the Unsteady Reynolds Averaged Navier-Stokes 

(URANS) method, allows slowly varying unsteadiness, which varies on a much longer scale than the 

turbulence, to be calculated directly while still modeling the effect of the turbulence. In an excited jet, the 

turbulence model will also affect the flow unsteadiness created by the actuator and, thereby, the growth 

and decay of the instabilities input even though the excitation itself will typically be at a time-scale much 

longer than the turbulence (if it is not, then a URANS solver has very little chance of working since all 

the flow characteristics would be entirely modeled). 

Turbulence models, by design, have a dissipative effect on the mean flow. The best turbulence model 

for a particular case will greatly depend on the problem being solved and what kind of flow the model 

was calibrated for. For jet excitation, the turbulence model should be minimally dissipative so as allow 

the perturbations to grow in the shear layer near the nozzle exit and up to the saturation amplitude for the 

particular excitation mode, recognizing that at some point the dissipative nature of the turbulence model 

will retard the perturbation amplitude. This may be acceptable depending on the purpose of the 

simulation. For example, if a simulation is run to determine the impact of an actuator technology on the 

jet shear layer immediately after the nozzle exit, then the downstream dissipation of the turbulence model 

would not be a concern. URANS solvers offer the best combination of accuracy, stability, and speed of 

any method currently available for most problems. As such, the URANS solver is a good place to start an 

investigation into simulation methods for excited jets. If this method produces acceptable accuracy in the 

regions of interest within the jet, then the advantage in computation speed that URANS enjoys over other 

methods can be used to more efficiently optimize the excitation input. 

While URANS CFD solvers are currently the mature simulation methods of choice for most 

problems, Large Eddy Simulations (LES) are the rapidly developing next generation of flow solvers. LES 

solvers reduce the solution by separating the flow variables based on space, rather than time, to create a 

time accurate solution where both the mean and the large-scale fluctuating parts of the flow are captured. 

The LES methods model or dissipate only the portion of the flow that cannot be resolved based on the 

mesh spacing (sub-grid scales) and solve directly all of the larger flow scales. This allows the user more 

direct control over which turbulent flow features are resolved but also generally results in many more grid 

points and smaller time steps, leading to a significant increase in computational expense, compared to a 

URANS simulation. The issue of computational expense is particularly acute in problems where there is 

flow along a surface and some resolution of the viscous boundary layer is necessary. Also, because the 
NASA/TM—2010-216768 5 

dissipation is applied to a much smaller portion of the flow, LES simulations tend to be less 

computationally stable than their URANS counterparts. 

The excited jet is necessarily a time dependent problem, a factor that plays to the strength of LES 

simulations. Additionally, the reduced dissipation from the turbulence model should allow the 

perturbations to grow and decay in a more realistic manner throughout the jet. However, the need to 

resolve the viscous boundary layer near the actuator and near the nozzle walls as well as the initial thin 

shear layer in the developing jet makes LES simulations of excited jets computationally intensive and 

limits the number of excitation parameters that can be studied. And while the reduced dissipation makes 

LES more likely to accurately capture the development of the perturbations farther downstream, it also 

makes the simulation more susceptible to numerical instability caused by sudden changes imparted by 

certain types of actuators. 

A sample from the turbulence models that are commonly used in jet simulations were selected and 

tested on the excited jet problem. The WIND–US URANS solver represents the currently state of the art 

in URANS CFD codes. The WIND–US code was developed and is currently maintained by the NPARC 

Alliance between the NASA Glenn Research Center and the USAF Arnold Engineering Development 

Center (Refs. 7 to 9). The WIND–US code is a multi-purpose 3–D solver for both the Euler and NavierStokes equations in both steady and unsteady problems, with support for chemically reacting flows. The 

code also features support for several one-equation, two-equation, and hybrid RANS/LES turbulence 

models. Two standard two-equation turbulence models, the Chien k- and SST models, and one hybrid 

RANS/LES turbulence model, the Spalart-DES model, were selected for this study to represent three 

different approaches to the problem of turbulence modeling and were used with WIND–US so simulate 

the excited jet. 

The NASA Glenn Research Center BASS code was selected as a representative LES code. The BASS 

code (Refs. 10 and 11) is currently being developed as a general purpose CAA/LES flow solver for 

compressible flow simulations. The code solves the non-linear Euler and Navier-Stokes equations on 

generalized curvilinear coordinate grids using the chain rule form of the governing equations. In order to 

accurately predict the unsteady flow dynamics, high-order spatial differencing methods are combined 

with optimized explicit time marching schemes. A shock-capturing artificial dissipation scheme with 10th 

order background dissipation is used to remove unresolved waves form the flow solution (Ref. 12). The 

BASS development effort has been focused to this point on the prediction of tone and broadband noise 

from jet engine stators using the inviscid Euler equations (Refs. 13 and 14). 

Simulations of an excited jet were run using each turbulence model. Each simulation used either an 

axisymmetric or 2–D grid to minimize the computation time required for each one. Grid and solver 

parameters were recorded so that this information can be used in future simulations and the solutions were 

studied for possible advantages or limitations inherent to each method. 

Chien k- Model 

The Chien k- was selected as a standard two-equation model (Refs. 15 and 16). This model was 

added to WIND–US as a robust and stable k- model suitable for a variety of flows. The model features 

stability enhancements in the form of limiters that cap the turbulence quantities, relaxation to increase 

stability at start-up, and a correction for adverse pressure gradient flows. The WIND–US implementation 

also offers the option of the Sarkar and Wilcox compressibility corrections. All options were held to 

default values for these simulations and neither the Sarkar nor Wilcox compressibility corrections were 

used. Although these coefficients may be adjusted to improve the results, the default values should give a 

reasonable idea of the model behavior while avoiding the large number of simulations that would be 

required to fully investigate each parameter. 

The Chien model was tested with the standard WIND–US second-order Roe upwind scheme modified 

for stretched grids and employing a TVD flux limiter. The MacCormack DQ limiter (Ref. 17), which is 

available in WIND–US and commonly used to speed convergence in steady flows, was disabled after 

early trials showed that it limited the growth of the actuator perturbations. First-order implicit time 
NASA/TM—2010-216768 6 

marching was used, with the default parameters, and a constant time step of 100 ns was found to be the 

upper limit for stability throughout the cycle. The computational time per time step ranged from 0.45 to 

0.60 sec using 14-processors on a local computer cluster and the grid had approximately 275,000 points. 

The grid was refined to show the grid independence of the solution. 

Although the Chien k- model as implemented in WIND–US features stability enhancements, it was 

unstable at the start of each actuator cycle. It is noted in the WIND–US manual that a different turbulence 

model may be required to initialize the turbulence before the Chien k- model is used (Ref. 9). Each 

actuator cycle, therefore, was started using the SST turbulence model for the equivalent of one time step. 

Once the turbulence was initialized, the k- model was stable and able to complete the cycle. This process 

added a considerable amount of work for the user and is a drawback to using this model in cyclical 

problems such as jet excitation. 

Menter SST Model 

A relative of the k- turbulence model, the Menter SST (Ref. 18) blends the k- model of Wilcox in 

the near wall and boundary layer regions with a standard k- model in the free stream and free shear 

regions by reformulating the k- model into the k- form. This adds stability in the near wall region 

compared to a standard k- model and, in fact, it is recommended in the WIND–US manual that the SST 

model be used to initialize the turbulence before the Chien k- model is used (Ref. 9). It has also been 

documented that the SST model is the most complete choice for simulating jet flows with WIND–US 

(Refs. 19 and 20). All coefficients and parameters for the SST model were kept to their default values. 

The SST model, like the Chien k- model, was used with the standard WIND–US second-order Roe 

upwind scheme modified for stretched grids with the TVD flux limiter but without the MacCormack DQ 

limiter. First-order implicit time marching was used and grid refinement showed the grid independence of 

the solution. Also like the Chien k- model, a maximum time step of 100 ns was used for stability 

throughout the cycle. Time steps were also completed slightly faster, at between 0.35 and 0.40 sec on 

average, than recorded for the k- model using the same 14-processors system. 

Spalart–DES Model 

The Spalart–DES model was developed to overcome some the computational limitations of LES in 

near wall and boundary layer flows while retaining the accuracy of a LES simulation in the free stream 

(Refs. 21 and 22). The one-equation Spalart-Allmaras turbulence model is used exclusively in the near 

wall region. In the free stream region, the Spalart-Allmaras model implicitly reduces to a sub-grid-scale 

model to deal with the flow not directly calculated on the grid. This allows the transition to LES to occur 

implicitly, controlled by one parameter, rather than forcing the user to explicitly declare zones. 

The model uses the same second-order Roe scheme in space as the other WIND–US simulations (the 

Spalart–DES model was developed with a fourth-order central difference scheme but this Roe scheme 

was used because it is the default in WIND–US). A first-order implicit scheme is used for time marching. 

Again, all parameters were left unchanged from the default values and the time step was held at 100 ns for 

stability. A second-order time marching scheme available in WIND–US was tested with the Spalart–DES 

model but found to be unstable when the actuators where enabled. This reduction in stability is due to the 

lower dissipation inherent in the second-order scheme. Topologically, the grid used for the DES 

simulations was identical to the grid used for the other WIND–US simulations. Also like the other 

WIND–US simulations, the DES simulations were run using the axisymmetric assumption. The number 

of grid points, however, was increased in both the x and y-directions away from the nozzle, to total 

approximately 1.9 million points, because the DES simulations need to resolve smaller turbulent length 

scales that are modeled in both the SST and k- simulations. As expected, the increased grid density 

resulted in an increase in computation time, to between 2.10 and 2.25 sec per time step using 24-

processors on the computer cluster (10 processors more than the previous simulations). 
NASA/TM—2010-216768 7 

LES 

The BASS CAA/LES solver was used to simulate the excited jet test case as a fully time accurate 

alternative to the URANS simulations. The BASS code solved the filtered Navier-Stokes equations, in 

2–D, using an Implicit LES (ILES) strategy (Ref. 23), in which the 10th order artificial dissipation model 

in the code is used to filter the sub-grid turbulence scale. The HALE–RK67 explicit time marching 

scheme (Ref. 24) was used with the Tam and Webb optimized fourth-order DRP spatial differencing 

scheme (Ref. 25) for these simulations. At the outer edges for the computational domain, the Thompson 

boundary conditions (Refs. 26 and 27) were combined with sponge layers (Ref. 28) to prevent reflections 

from reentering the domain. 

An entirely new grid was required for the BASS simulations. The BASS code has been developed 

with several automatic parallelization features that require the grid to have full face block to block 

matching, resulting in a grid with 506 blocks. BASS also requires more grid points in the viscous 

boundary layer along the nozzle wall, and particularly at near the actuator walls, than any of the WIND–

US simulations for numerical stability. The grid also included both sides of the jet, rather than only one 

side with a symmetry boundary condition along the nozzle centerline as run in the WIND–US 

simulations, to improve the simulation along the centerline. The grid was stretched away from the nozzle 

in the axial and radial directions, especially past x/Dj = 10 where the flow was not studied resulting in a 

grid that contained only approximately 215,000 points. And while this is the smallest grid by number of 

points tested, BASS still required around 4 sec per time step using 17 processors on the computer cluster, 

the longest of any simulation. In order to decrease the total time required to compute one actuator cycle 

while maintaining stability, the time step was changed during the cycle. The maximum stable time step 

was 0.75 ns (7.5×10–10 sec) from the start of a cycle until the actuator flow passed the nozzle exit. The 

time step could then be raised to 3.75 ns (3.75×10–9 sec) for the remainder of the cycle. 

Note that BASS is still in development and work is ongoing to streamline the code and make it more 

efficient, particularly in the area of parallelization and the associated message passing. An AdamsBashforth multi-time-stepping scheme is also being added to reduce the computation required per time 

step (Ref. 29). 

Simulation Results 

Simulations of a baseline (unexcited, no actuator) jet were conducted using URANS and LES CFD 

codes to establish the jet flow before the actuators were added. These baseline results, shown in Figure 2, 

were computed by allowing the simulation to reach a converged solution while the DES and LES mean 

flows were computed by time averaging a series of instantaneous flow fields. These plots show the SST 

simulation results in a longer jet potential core than the k- simulation, which is consistent with past 

results (Ref. 30). The DES and LES results show an even shorter high-speed region compared to the k-

results although the flow in the DES simulation continues along the jet axis at a relatively high speed. 

This may be caused by the hybrid URANS/LES nature of the DES model (not having quite the right 

balance between a pure RANS turbulence model and a LES sub-grid model) and the axisymmetric 

assumption, which prevents the flow structures from breaking up in the azimuthal direction. The DES 

results also show a jet that spreads slower than the other models while the LES shows a jet spreading 

faster than observed in the other results though this behavior may be grid dependent. It is worth reiterating 

here that caution should be used before drawing any firm conclusions using either the DES axisymmetric 

or the LES 2–D simulations. Large-scale turbulent structures, which both methods calculate directly, are 

inherently 3–D and need to be computed as such. The information gleaned from analyzing the results of 

these 2–D simulations will only serve to guide future 3–D simulations. 

Once the baseline flow is computed, the actuator is introduced into the flow. Figure 3 shows the 

density of the flow in the actuator region 20 μs after the beginning of the actuator cycle. The LAFPA type 

actuator was expected to generate a shock wave that perturbs the flow, which is observed in the density 
NASA/TM—2010-216768 8 
NASA/TM—2010-216768 9 

plot from all the simulations. The wave leaves the actuator cavity with sufficient power to cause the flow 

to separate from the nozzle surface right at the nozzle exit as the jet flow is forced around the pressure 

wave, behavior which is consistent with the expected mechanism behind the LAFPA. The flow separation 

sets up a vortical flow structure that will travel downstream and affect the development of the jet; 

however, the effect that this structure has on the jet will be strongly affected by the turbulence model. 

The instantaneous vorticity throughout the flow at the end of the actuator cycle for each simulation is 

shown in Figure 4. Both the SST and k- models support the initial vortex created by the actuator but do 

not allow it to develop, damping it out around x/Dj = 1. The DES model allows the vortex to propagate 

downstream and grow with minimal loss of energy, which is expected from an approach that is designed 

to capture the large-scale unsteady flow dynamics directly. The axisymmetric assumption applied in the 

DES simulations also disrupts the energy cascade, an inherently 3–D processes where large-scale 

structures break down into smaller structures before energy is dissipated by viscous forces, by preventing 

the flow from moving in the azimuthal direction. The LES also shows the propensity to propagate the 

vortex, with vorticity appearing up to x/Dj = 4, but the structures are not as sharp as those found in the 

DES results and do not persist downstream. This strongly suggests that the LES grid is too coarse in this 

region and, therefore, is dissipating rather than calculating the smaller turbulent scales needed to support 

these vortices. 

The unsteady flow dynamics that may be resolved in a DES or LES simulation is determined by the 

grid spacing and the numerical scheme employed. Every numerical scheme requires some number of 

points to get an accurate spatial derivative and, thus, and accurate time derivative. The DRP scheme in 

BASS requires approximately 6 grid points per wavelength for a simple harmonic disturbance. The 

second-order Roe method used in the DES simulations needs on the order of 40 grid points to resolve the 

same disturbance and propagate the waves at the correct speed (the waves will propagate with fewer 

points but at an incorrect speed). In both case, more grid density is required to resolve any non-linear flow 
NASA/TM—2010-216768 10 

dynamics that may be present. Any turbulence small than the minimum grid spacing is dissipated 

resulting in the smearing and loss of the flow structure. Figure 5 shows the density of the grids used for 

the DES and LES simulations, where the grid density was defined as the maximum of ∆x and ∆y at each 

point. The DES grid has a significant number of additional grid points in the near nozzle region than the 

LES grid. This increases the grid density on the DES grid enough to overcome the additional number of 

points required by 2nd-order Roe scheme. The LES grid stretches quickly in the radial direction outside 

the nozzle and downstream, especially past x/Dj = 10, to reduce the total number of points and reduce the 

computation time. The difference between the LES and DES vorticity results (Fig. 4) and a comparison of 

the grid, however, indicates that the LES grid stretches too quickly. A much finer grid, on the order of the 

DES grid, should significantly improve the LES results and should be used for future LES simulations. 

A vortex forms at the nozzle exit in response to the flow separation created by the actuator. That 

vortex propagates downstream and is either supported or dissipated at different levels by the CFD method 

used in the simulation. These observations, while insightful, are not easily compared qualitatively to the 

available experimental data. And although the there is little point in trying to quantitatively reproduce 

these results, a qualitative comparison may be instructive. Researchers at OSU have recorded pressure 

fluctuations, as a function of time, at several axial stations at the jet lipline (y/Dj = 0.5). After computing a 

Fourier transform, this data shows the axial growth and decay of the actuator perturbation by extracting 

only the pressure fluctuations at the actuator frequency. Similar data, sampled over one actuator cycle, 

can be extracted from the time accurate simulation data recorded using each of the turbulence models 

once a sufficient number of cycles have been run to initialize the flow (the minimum was found to be 

approximately 8 cycles to extract data up to x/Dj≈10). 

The numerical results for each simulation is are compared to the experimental data in Figure 6. Note 

that the experimental data is amplitude shifted so that any comparison of absolute amplitudes invalid. 

However, the perturbation growth rate, peak location, and decay rate are useful and can be compared to 

the experimental data for each scheme. The results shown in Figure 6 indicate that all of the simulation 

methods have some limitations. The pure URANS simulations using the SST and k- turbulence models 

have an initial growth rate similar to the experimental data over the first x/Dj≈1.0 from the nozzle exit. 

The jet response determined using SST model then flattens out and decays far short of the experimental 

peak location at x/Dj≈2.5. The jet response using the Chien k- model, however, continues to grow, 

although more slowly, and peaks around x/Dj≈2 before decaying rapidly. In both cases, the rate at which 

the perturbation decays far exceeds the rate measured in the experiment, a result that is not surprising 

based on the models propensity to dissipate the downstream flow structures. 
NASA/TM—2010-216768 11 

Unlike the pure URANS turbulence models, the jet response simulated using the Spalart-DES hybrid 

URANS/LES model has the slowest initial growth rate. It also places the peak jet response the farthest 

downstream, around x/Dj≈4 or x/Dj≈1.5 downstream of the measured peak location and allows the 

perturbation to continue downstream almost undamped. While it is not surprising that the DES model, 

especially in an axisymmetric simulation, does not dissipate the perturbation like the pure URANS 

simulations, it is somewhat surprising that the initial growth rate is not closer to the experimental, SST, or 

k- results. It is possible that the Spalart-Allmaras RANS turbulence model, operating in the near wall 

region, is over damping the initial perturbation and, in effect, reducing the strength of the actuator 

perturbation. If this is the case, varying the constant that controls the size of RANS region should change 

the jet response. However, as the authors of this model note, the value of this constant has little effect in 

2–D simulations and needs to be set using 3–D simulations (Ref. 21). 

Finally, the LES simulation, using the BASS code, calculates a jet response somewhere between the 

other simulations. The initial growth rate, while faster than the DES simulations, is slower than the SST, 

k-, and experimental data. The response, however, continues to grow and has a peak near the peak 

response location measured in the experiments. A short amplitude decrease is followed by a period of 

generally flat response where the response would be expected to decay based on the experimental data. 

As was the case in the DES simulations, these persistent levels are expected in a 2–D LES simulation 

because the flow structures are not permitted to decay in the azimuthal direction. LES, because it is 

filtered in space rather than time, is heavily dependent on the grid spacing and, based on the vorticity data 

and length scale map, it is likely that the grid stretches too far too close to the nozzle exit to support the 

additional growth rate measured in the experiment. 

The jet response determined at the nozzle lipline is an easily measured metric in an experiment where 

time and equipment limits the number of data points available. One of the strengths of CFD is the ability 

to sample the entire flow field at any desired interval. Figure 7 shows pressure, recorded at the end of an 

actuator cycle from simulations using each of the turbulence models, to support the previous comparisons 
NASA/TM—2010-216768 12 

from only along the jet lipline. Note that in the URANS simulations, the pressure fluctuations are entirely 

due to the actuator because all the natural flow unsteadiness is modeled. The DES and LES results, 

however, contain pressure fluctuations from the turbulence in the jet as well and the actuator. First, the 

damping of all flow structures by the SST and k- turbulence models is observed by x/Dj≈5. The flow 

fields from the DES and LES, by comparison, show vortices traveling to the end of the domain, which is 

expected based on the slow perturbation decay rates observed previously. The data also shows differences 

between the DES and LES simulations. The DES simulation shows well defined vortices interacting at 

various points in the flow field (e.g., the two vortices at x/Dj≈4). In the LES simulation data, however, the 

flow structures are fuzzy and the interaction is not captured in the flow field. This difference shows the 

need for tighter grid spacing in the LES simulation, which, in theory, will capture these flow features 

given enough grid. 

Conclusions 

Jet excitation has many applications ranging from noise reduction to enhanced plume mixing. 

Computational fluid dynamics (CFD) can be used to research and optimize the excitation input, reducing 

the number of experiments required and, thus, the cost to develop the technology. CFD, however, is a 

viable option only if a suitable simulation method can be found. 

A series of simulations studied the advantages and disadvantages of four different turbulence models 

for a jet excitation problem with the goal of guiding future simulations. The results indicated that pure 

URANS turbulence models fall short of the expected results. The URANS/LES hybrid model, in the form 

of the Spalart–DES model, has potential, based on both computation speed and flow results, and should 

be investigated in the future using full 3–D simulations. Furthermore, these simulations should begin with 

a study of the impact that the size of the URANS region has on the initial growth rate of the perturbations, 

which is the biggest unknown in this hybrid method and which may significantly alter the initial 

perturbation growth rate. The LES simulations also showed potential based on the flow data and should 

also be continued using full 3–D simulations with a finer spaced grid (on the order of the DES grid). The 
NASA/TM—2010-216768 13 

biggest drawback to the LES simulations is the computation time required, but this should be greatly 

reduced by improvements in the efficiency of the code as it is developed. Ultimately, future simulations 

of excited jets will benefit from the knowledge and experience gained through these simplified 

simulations. 

References 

1. Samimy, M., Kim, J.-H., Kastner, J., Adamovich, I., and Utkin, Y., “Active control of a Mach 0.9 Jet 

for Noise Mitigation Using Plasma Actuators,” AIAA J., Vol. 45(4), 890–901, 2007. 

2. Samimy, M., Kim, J.-H., Kastner, J., Adamovich, I., and Utkin, Y., “Active control of high-speed 

and high-Reynolds number jets using plasma actuators,” J. Fluid Mech., Vol. 578, 305–330, 2007. 

3. Utkin, Y., Keshav, S., Kim, J.-H., Kastner, J., Adamovich, I., and Samimy, M., “Development and 

Use of Localized Arc Filament Plasma Actuators For High-speed Flow Control,” J. of Physics D: 

Applied Physics, 40, 685–694, 2007. 

4. Leonov, S., Bityurin, V., Savelkin, K., and Yarantsev, D., “Effect of Electrical Discharge on 

Separation Processes and Shock Position in Supersonic Airflow,” AIAA 2002–0355, 40th AIAA 

Aerospace Sciences Meeting and Exhibit, 14–17 January 2002, Reno, NV. 

5. Leonov, S., Bityurin, V., and Yarantsev, D., “The Effect of Plasma Induced Separation,” AIAA 

2003–3853, 34th AIAA Plasmadynamics and Lasers Conference, 23–26 June 2003, Orlando, FL. 

6. Brown, C., “Scalability of the Localized Arc Filament Plasma Actuators,” AIAA 2008–3043, 14th 

AIAA/CEAS Aeroacoustics Conference, 5–7 May 2008, Vancouver, Canada. 

7. Bush, R., Power, G., and Towne, C., “WIND: The Production Flow Solver of the NPARC Alliance,” 

AIAA 1998–0935, 1998. 

8. Nelson, C. C. and Power, G. D., “CHSSI Project CFD–7: The NPARC Alliance Flow Simulation 

System,” AIAA 2001–0594, 2001. 

9. The Wind User’s Guide, User Manual, The NPARC Alliance, 

http://www.grc.nasa.gov/WWW/winddocs/user/index.html 

10. Hixon, R., Nallasamy, M., and Sawyer, S., “Parallelization Strategy for an Explicit Computational 

Aeroacoustics Code,” AIAA 2002–2583, July 2002. 

11. Hixon, R., Nallasamy, M., Sawyer, S., and Dyson, R., “Comparison of Numerical Schemes for a 

Realistic Computation Aeroacoustics Problem,” International Journal of Aeroacoustics, Vol. 3, 

pp. 379–397, 2004. 

12. Hixon, R., Bhate, D., Nallasamy, M., and Sawyer, S., “Shock-Capturing Dissipation Schemes for 

High-Accuracy Computational Aeroacoustics (CAA) Codes,” AIAA 2006–2413, May 2006. 

13. Hixon, R., Nallasamy, M., and Sawyer, S., “Progress towards the prediction of turbomachinery noise 

using Computational Aeroacoustics,” Inter-Noise paper IN06–116, Dec. 2006. 

14. Nallasamy, M., Hixon, R., and Sawyer, S., “Solution of unsteady Euler equations: Gust-cascade 

interaction tones,” Computers and Fluids, Vol. 36, pp. 724–741, 2007. 

15. Chien, K.Y., “Prediction of Channel and Boundary-Layer Flows with a Low-Reynolds-Number 

Turbulence Model,” AIAA J., Vol. 20(1), pp. 33–38, 1982. 

16. Yoder, D.A. and Georgiadis, N.J., “Implementation and Validation of the Chien k- Turbulence 

Model in the WIND Navier-Stokes Code,” AIAA 1999–0745, 37th AIAA Aerospace Sciences 

Meeting and Exhibit, 11–13 January 1999, Reno, NV. 

17. MacCormack, R.W., “Considerations for Fast Navier-Stokes Solvers,” presented at the conference on 

Advances of Flow Simulation Techniques, Davis, CA, May 1997. 

18. Menter, F.R., “Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications,” 

AIAA J., Vol. 32(8), pp. 1598–1605, August 1994. 

19. Georgiadis, N. and Papamoschou, D., “Computational Investigations of High-Speed Dual-Stream 

Jets,” AIAA 2003–3311, 2003. 

20. Georgiadis, N.J., Rumsey, C.L., Yoder, D.A., and Zaman, K.B.M.Q., “Effects of RANS Turbulence 

Modeling on Calculation of Lobed Nozzle Flowfields,” AIAA 2003–1271, 2003. 
NASA/TM—2010-216768 14 

21. Spalart, P.R., Jou, W.H., Strelets, M., and Allmaras, S.R., “Comments on the Feasibility of LES for 

Wings, And on a Hybrid RANS/LES Approach,” First AFOSR International Conference On 

DNS/LES, August 4–8, 1997, Ruston, LA. (In Advances in DNS/LES, Liu, C. and Liu, Z., eds., 

Greyden Press, Columbus OH.) 

22. Shur, M., Spalart, P.R., Strelets, M., and Travin, A., “Detached-Eddy Simulation of an Airfoil at High 

Angle of Attack,” 4th International Symposium on Engineering Turbulence Modeling and 

Measurements, May 24–26 1999, Corisca. 

23. Grinstein, F., Drikakis, D., Fureby, C., and Youngs, D., “Transition and Turbulence Decay in the 

Taylor-Green Vortex,” AIAA 2006–0698, January 2006. 

24. Hixon, R., Allampali, V., Nallasamy, M., and Sawyer, S., “High-Accuracy Large-Step Explicit 

Runge-Kutta (HALE–RK) Schemes for Computational Aeroacoustics,” AIAA 2006–0797, January 

2006. 

25. Tam, C.K.W. and Webb, J.C., “Dispersion-relation-preserving finite-difference schemes for 

computational acoustics,” J. of Computational Physics, Vol. 107, pp. 262–281, 1993. 

26. Thompson, K.W., “Time dependent boundary conditions for hyperbolic systems,” J. of 

Computational Physics, Vol. 68, pp. 1–24, 1987. 

27. Thompson, K.W., “Time dependent boundary conditions for hyperbolic systems II,” J. of 

Computational Physics, Vol. 89, pp. 439–461, 1990. 

28. Goodrich, J., “A Comparison of Three PML Treatments for CAA (and CFD),” AIAA 2008–2922, 

May 2008. 

29. Allampali, V. and Hixon, R., “Implementation of Multi-Time Step Adams-Bashforth Time Marching 

Schemes for CAA,” AIAA 2008–0029, January 2008. 

30. Georgiadis, N.J., Yoder, D.A., and Engblom, W.A., “Evaluation of Modified Two-Equation 

Turbulence Models for Jet Flow Predictions,” AIAA J., Vol. 44(12), pp. 3107–3114, December 2006. 
REPORT DOCUMENTATION PAGE Form Approved 

OMB No. 0704-0188 

The public reporting burden for this collection of information is estimated to average 1 hour per response, including the time for reviewing instructions, searching existing data sources, gathering and maintaining the 

data needed, and completing and reviewing the collection of information. Send comments regarding this burden estimate or any other aspect of this collection of information, including suggestions for reducing this 

burden, to Department of Defense, Washington Headquarters Services, Directorate for Information Operations and Reports (0704-0188), 1215 Jefferson Davis Highway, Suite 1204, Arlington, VA 22202-4302. 

Respondents should be aware that notwithstanding any other provision of law, no person shall be subject to any penalty for failing to comply with a collection of information if it does not display a currently valid OMB 

control number. 

PLEASE DO NOT RETURN YOUR FORM TO THE ABOVE ADDRESS. 

1. REPORT DATE (DD-MM-YYYY)

01-09-2010 

2. REPORT TYPE

Technical Memorandum 

3. DATES COVERED (From - To)

4. TITLE AND SUBTITLE

Effect of Turbulence Modeling on an Excited Jet 

5a. CONTRACT NUMBER

5b. GRANT NUMBER

5c. PROGRAM ELEMENT NUMBER

6. AUTHOR(S)

Brown, Clifford, A.; Hixon, Ray 

5d. PROJECT NUMBER

5e. TASK NUMBER

5f. WORK UNIT NUMBER

WBS 984754.02.07.03.17.03 

7. PERFORMING ORGANIZATION NAME(S) AND ADDRESS(ES)

National Aeronautics and Space Administration 

John H. Glenn Research Center at Lewis Field 

Cleveland, Ohio 44135-3191 

8. PERFORMING ORGANIZATION

 REPORT NUMBER

E-17393 

9. SPONSORING/MONITORING AGENCY NAME(S) AND ADDRESS(ES)

National Aeronautics and Space Administration 

Washington, DC 20546-0001 

10. SPONSORING/MONITOR'S

 ACRONYM(S)

NASA 

11. SPONSORING/MONITORING

 REPORT NUMBER

NASA/TM-2010-216768 

12. DISTRIBUTION/AVAILABILITY STATEMENT

Unclassified-Unlimited 

Subject Category: 71 

Available electronically at http://gltrs.grc.nasa.gov 

This publication is available from the NASA Center for AeroSpace Information, 443-757-5802

13. SUPPLEMENTARY NOTES

14. ABSTRACT

The flow dynamics in a high-speed jet are dominated by unsteady turbulent flow structures in the plume. Jet excitation seeks to control these 

flow structures through the natural instabilities present in the initial shear layer of the jet. Understanding and optimizing the excitation input, 

for jet noise reduction or plume mixing enhancement, requires many trials that may be done experimentally or computationally at a 

significant cost savings. Numerical simulations, which model various parts of the unsteady dynamics to reduce the computational expense of 

the simulation, must adequately capture the unsteady flow dynamics in the excited jet for the results are to be used. Four CFD methods are 

considered for use in an excited jet problem, including two turbulence models with an Unsteady Reynolds Averaged Navier-Stokes 

(URANS) solver, one Large Eddy Simulation (LES) solver, and one URANS/LES hybrid method. Each method is used to simulate a 

simplified excited jet and the results are evaluated based on the flow data, computation time, and numerical stability. The knowledge gained 

about the effect of turbulence modeling and CFD methods from these basic simulations will guide and assist future three-dimensional (3-D) 

simulations that will be used to understand and optimize a realistic excited jet for a particular application. 

15. SUBJECT TERMS

Aerodynamic noise 

16. SECURITY CLASSIFICATION OF: 17. LIMITATION OF

 ABSTRACT

UU 

18. NUMBER

 OF 

 PAGES

20 

19a. NAME OF RESPONSIBLE PERSON

STI Help Desk (email:help@sti.nasa.gov) 

a. REPORT

U 

b. ABSTRACT

U 

c. THIS 

PAGE

U 

19b. TELEPHONE NUMBER (include area code)

443-757-5802 

Standard Form 298 (Rev. 8-98)

Prescribed by ANSI Std. Z39-18