This document has been superseded 

by a later version. For the latest 

version go to the web site: 

http://fire.nist.gov/fds
NIST Special Publication 1019

Fire Dynamics Simulator (Version 4)

User’s Guide

Kevin McGrattan

Glenn Forney
NIST Special Publication 1019

Fire Dynamics Simulator (Version 4)

User’s Guide

Kevin McGrattan

Glenn Forney

Fire Research Division

Building and Fire Research Laboratory

in cooperation with

VTT Building and Transport, Finland

July 2004

UNITED STATES OF AMERICA

DEPARTMENT OF COMMERCE

U.S. Department of Commerce

Donald L. Evans, Secretary

Technology Administration

Phillip J. Bond, Under Secretary for Technology

National Institute of Standards and Technology

Arden L. Bement, Jr., Director
Certain commercial entities, equipment, or materials may be identified in this

document in order to describe an experimental procedure or concept adequately. Such

identification is not intended to imply recommendation or endorsement by the

National Institute of Standards and Technology, nor is it intended to imply that the

entities, materials, or equipment are necessarily the best available for the purpose.

National Institute of Standards and Technology Special Publication 1019

Natl. Inst. Stand. Technol. Spec. Publ. 1019, 90 pages (July 2004)

CODEN: NSPUE2

U.S. GOVERNMENT PRINTING OFFICE

WASHINGTON: 2004

For sale by the Superintendent of Documents, U.S. Government Printing Office

Internet: bookstore.gpo.gov – Phone: (202) 512-1800 – Fax: (202) 512-2250

Mail: Stop SSOP, Washington, DC 20402-0001

Preface

This guide describes how to use the Fire Dynamics Simulator (FDS). It does not provide the background

theory. A companion document, called the FDS Technical Reference Guide [1], contains details about the

governing equations, numerical methods and validation work. Although the User’s Guide contains all the

information necessary to perform fire simulations, the reader should also become familiar with some of

the background theory in the Technical Reference Guide. The software and the User’s Guide provide only

limited guidance as to the proper prescription of input parameters.

The FDS User’s Guide contains limited information on how to operate Smokeview, the companion

visualization program for FDS. Its full capability is described in the “User’s Guide for Smokeview Version

4” [2]. This guide also contains information on how Smokeview can be used to design FDS calculations,

providing a short tutorial on the use of both models.

i
ii
Disclaimer

The US Department of Commerce makes no warranty, expressed or implied, to users of the Fire Dynamics

Simulator (FDS), and accepts no responsibility for its use. Users of FDS assume sole responsibility under

Federal law for determining the appropriateness of its use in any particular application; for any conclusions

drawn from the results of its use; and for any actions taken or not taken as a result of analyses performed

using these tools.

Users are warned that FDS is intended for use only by those competent in the fields of fluid dynamics,

thermodynamics, combustion, and heat transfer, and is intended only to supplement the informed judgment

of the qualified user. The software package is a computer model that may or may not have predictive

capability when applied to a specific set of factual circumstances. Lack of accurate predictions by the model

could lead to erroneous conclusions with regard to fire safety. All results should be evaluated by an informed

user.

Throughout this document, the mention of computer hardware or commercial software does not constitute endorsement by NIST, nor does it indicate that the products are necessarily those best suited for the

intended purpose.

iii
iv
Acknowledgments

The Fire Dynamics Simulator, in various forms, has been under development for almost 25 years. However,

the publicly released software has only existed since 2000. While many individuals have contributed to

the development of the model and its validation, a smaller group is actually responsible for writing the

computer program. The FDS Technical Reference Guide contains an extensive list of model contributors.

Here, however, we recognize those individuals who have done the actual programming.

Originally, the basic hydrodynamic solver was designed by Ronald Rehm and Howard Baum with programming help from Darcy Barnett, Dan Lozier and Hai Tang of the Computing and Applied Mathematics

Laboratory (CAML) at NIST, and Dan Corley of the Building and Fire Research Laboratory (BFRL). Jim

Sims of CAML developed the original visualization software. The direct pressure solver was written by

Roland Sweet of the National Center for Atmospheric Research (NCAR), Boulder, Colorado. Kevin McGrattan expanded the basic program to include fire-specific routines, and he remains the custodian of the

FDS source code. Glenn Forney developed the companion visualization program Smokeview and remains

its custodian. Kuldeep Prasad added the multiple-mesh data structures, paving the way for parallel processing. William (Ruddy) Mell has added special routines to extend the model into areas such as microgravity

combustion and wildland fire spread. Charles Bouldin devised the basic framework of the parallel version

of the code.

Jason Floyd, a former NIST Post-Doc, wrote the mixture fraction and droplet evaporation routines. Simo

Hostikka, a NIST guest researcher from VTT Building and Transport, Finland, wrote the radiation solver

and the char pyrolysis routine. Although no longer at NIST, both continue to make significant contributions

to the source code.

v
vi
Contents

Preface i

Disclaimer iii

Acknowledgments v

1 Introduction 1

1.1 Features of FDS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1

1.2 What’s New in FDS 4? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2

2 Getting Started 3

2.1 How to get FDS and Smokeview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

2.2 Computer Hardware Requirements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

2.3 Computer Operating System (OS) and Software Requirements . . . . . . . . . . . . . . . . 4

3 Running FDS 5

3.1 Creating the FDS Input Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5

3.2 Starting an FDS Calculation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5

3.2.1 Starting an FDS Calculation (Single Processor Version) . . . . . . . . . . . . . . . . 6

3.2.2 Starting an FDS Calculation (Multiple Processor Version) . . . . . . . . . . . . . . 6

3.3 Monitoring Progress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

3.4 Error Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

3.5 Reporting Bugs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9

4 Setting up the Input File for FDS 11

4.1 Preliminaries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

4.1.1 Naming the Job: The HEAD Namelist Group . . . . . . . . . . . . . . . . . . . . . 13

4.1.2 Setting Time Limits: The TIME Namelist Group . . . . . . . . . . . . . . . . . . . 13

4.2 The Numerical Grid . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14

4.2.1 Defining the Computational Domain: The PDIM Namelist Group . . . . . . . . . . 14

4.2.2 Setting the Grid Size: The GRID Namelist Group . . . . . . . . . . . . . . . . . . . 14

4.2.3 Multiple Meshes and Parallel Processing . . . . . . . . . . . . . . . . . . . . . . . 15

4.3 Setting Global Parameters: The MISC Namelist Group . . . . . . . . . . . . . . . . . . . . 17

4.4 Prescribing the Geometry and the Fire . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19

4.4.1 Prescribing Boundary Conditions: The SURF Namelist Group . . . . . . . . . . . . 19

4.4.2 Combustion Parameters: The REAC Namelist Group . . . . . . . . . . . . . . . . . 24

4.4.3 Important Issues Related to Combustion . . . . . . . . . . . . . . . . . . . . . . . . 25

4.4.4 Creating Obstructions: The OBST Namelist Group . . . . . . . . . . . . . . . . . . 27

vii
4.4.5 Creating Voids: The HOLE Namelist Group . . . . . . . . . . . . . . . . . . . . . . 28

4.4.6 Designating Vents and Surfaces: The VENT Namelist Group . . . . . . . . . . . . . 29

4.4.7 Coloring Obstructions, Vents and Surfaces . . . . . . . . . . . . . . . . . . . . . . 30

4.5 Lagrangian Particles: The PART Namelist Group . . . . . . . . . . . . . . . . . . . . . . . 32

4.6 Sprinklers and Detectors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34

4.6.1 Specifying Sprinklers: The SPRK Namelist Group . . . . . . . . . . . . . . . . . . 34

4.6.2 Specifying Heat Detectors: The HEAT Namelist Group . . . . . . . . . . . . . . . . 36

4.7 Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38

4.7.1 Point Measurements: The THCP Namelist Group . . . . . . . . . . . . . . . . . . . 38

4.7.2 Animated Planar Slices: The SLCF Namelist Group . . . . . . . . . . . . . . . . . 39

4.7.3 Animated Boundary Quantities: The BNDF Namelist Group . . . . . . . . . . . . . 39

4.7.4 Animated Isosurfaces: The ISOF Namelist Group . . . . . . . . . . . . . . . . . . 42

4.7.5 Static Data Dumps: The PL3D Namelist Group . . . . . . . . . . . . . . . . . . . . 43

4.7.6 Extracting Numbers from the Output Data Files . . . . . . . . . . . . . . . . . . . . 43

5 Special Features 47

5.1 Stopping and Restarting Calculations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47

5.2 Stretching the Grid: The TRNX, TRNY and/or TRNZ Namelist Groups . . . . . . . . . . . . 48

5.3 Initial Conditions: The INIT Namelist Group . . . . . . . . . . . . . . . . . . . . . . . . . 49

5.4 Creating or Removing Obstructions; Opening or Closing Vents . . . . . . . . . . . . . . . . 50

5.5 Extra Species . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51

5.6 Finite-Rate or Premixed Combustion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 52

5.7 Pyrolysis Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53

5.7.1 Thermoplastics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53

5.7.2 Charring Fuels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54

5.7.3 Liquid Fuels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55

5.8 Burning Liquid Fuel Droplets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55

5.9 Suppression by Water (Mixture Fraction Model Only) . . . . . . . . . . . . . . . . . . . . . 56

5.10 Visibility . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56

5.11 Layer Height and the Average Upper and Lower Layer Temperatures . . . . . . . . . . . . . 57

5.12 Leakage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58

5.13 Fires and Flows in the Outdoors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58

5.14 2D and Axially-Symmetric Calculations . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59

5.15 Restoring the Baroclinic Vorticity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59

5.16 Fine-Tuning the Radiation Transport Model . . . . . . . . . . . . . . . . . . . . . . . . . . 63

5.17 Defying Gravity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63

5.18 Isothermal and Salt Water Simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63

5.19 Non-rectangular Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64

5.20 Texture Mapping . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64

6 Conclusion 67

References 69

Appendices 69

viii
A Compiling the Source Code for FDS 71

A.1 Serial Compilation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71

A.2 Parallel Compilation using Windows and MPICH . . . . . . . . . . . . . . . . . . . . . . . 73

B Alphabetical List of Input Parameters 75

C Output File Formats 85

C.1 Diagnostic Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85

C.2 Plot3D Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86

C.3 Thermocouple Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87

C.4 Sprinkler Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87

C.5 Heat Release Rate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87

C.6 Gas Mass Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88

C.7 Mixture Fraction State Relations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88

C.8 Slice Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88

C.9 Boundary Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89

C.10 Particle Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89

ix
x
Chapter 1

Introduction

Fire Dynamics Simulator (FDS) is a computational fluid dynamics (CFD) model of fire-driven fluid flow.

The software described in this document solves numerically a form of the Navier-Stokes equations appropriate for low-speed, thermally-driven flow with an emphasis on smoke and heat transport from fires. The

formulation of the equations and the numerical algorithm are contained in a companion document, called

Fire Dynamics Simulator (Version 4.0) – Technical Reference Guide [1].

Smokeview is a visualization program that is used to display the results of an FDS simulation. Some

examples of Smokeview are shown in this document. A detailed description can be found in a companion

document, called User’s Guide for Smokeview Version 4 [2].

1.1 Features of FDS

Version 1 of FDS was publicly released in February 2000. Version 2 was publicly released in December

2001. To date, about half of the applications of the model have been for design of smoke handling systems

and sprinkler/detector activation studies. The other half consist of residential and industrial fire reconstructions. Throughout its development, FDS has been aimed at solving practical fire problems in fire protection

engineering, while at the same time providing a tool to study fundamental fire dynamics and combustion.

Hydrodynamic Model FDS solves numerically a form of the Navier-Stokes equations appropriate for lowspeed, thermally-driven flow with an emphasis on smoke and heat transport from fires. The core

algorithm is an explicit predictor-corrector scheme, second order accurate in space and time. Turbulence is treated by means of the Smagorinsky form of Large Eddy Simulation (LES). It is possible to

perform a Direct Numerical Simulation (DNS) if the underlying numerical grid is fine enough. LES

is the default mode of operation.

Combustion Model For most applications, FDS uses a mixture fraction combustion model. The mixture

fraction is a conserved scalar quantity that is defined as the fraction of gas at a given point in the flow

field that originated as fuel. The model assumes that combustion is mixing-controlled, and that the

reaction of fuel and oxygen is infinitely fast. The mass fractions of all of the major reactants and

products can be derived from the mixture fraction by means of “state relations,” empirical expressions

arrived at by a combination of simplified analysis and measurement.

Radiation Transport Radiative heat transfer is included in the model via the solution of the radiation transport equation for a non-scattering gray gas, and in some limited cases using a wide band model. The

equation is solved using a technique similar to finite volume methods for convective transport, thus

the name given to it is the Finite Volume Method (FVM). Using approximately 100 discrete angles,

1
the finite volume solver requires about 15 % of the total CPU time of a calculation, a modest cost

given the complexity of radiation heat transfer. Water droplets can absorb thermal radiation. This is

important in cases involving mist sprinklers, but also plays a role in all sprinkler cases. The absorption

coefficients are based on Mie theory.

Geometry FDS approximates the governing equations on a rectilinear grid. The user prescribes rectangular

obstructions that are forced to conform with the underlying grid.

Multiple Meshes This is a term used to describe the use of more than one rectangular mesh in a calculation.

It is possible to prescribe more than one rectangular mesh to handle cases where the computational

domain is not easily embedded within a single mesh.

Boundary Conditions All solid surfaces are assigned thermal boundary conditions, plus information about

the burning behavior of the material. Usually, material properties are stored in a database and invoked

by name. Heat and mass transfer to and from solid surfaces is usually handled with empirical correlations, although it is possible to compute directly the heat and mass transfer when performing a Direct

Numerical Simulation (DNS).

1.2 What’s New in FDS 4?

FDS 4 has the same overall features as FDS 3, but there have been several refinements, re-organizations and

bug fixes. Among the more important are:

Parallel Processing It is possible to run an FDS calculation on more than one computer using the Message

Passing Interface (MPI). Details can be found in Section 3.2.2.

Multiple Meshes Improvements have been made to the multiple mesh capability allowing more flexibility

in designing simulations. See Section 4.2.3 for details.

Holes One can now specify a cutout in much the same way as an obstruction. This is useful for carving

doors and windows out of solid walls without having to break up the walls into pieces. See Section 4.4.5 for details.

Char Model A char model has been implemented in which a thin pyrolysis front is tracked inside a solid

fuel. The front separates virgin fuel from char. Thermal properties for fuel and char must be provided

by the user. See Section 5.7.2 for details.

Temperature-dependent Material Properties It is now possible to prescribe material properties of solids

as a function of temperature. Note that this refinement has altered some of the pyrolysis conventions

used in previous versions of FDS. Read Section 4.4.1 to see how old input files may be affected by

the changes.

Lagrangian Particles The format of the input file has changed in regard to the treatment of Lagrangian

particles, including sprinkler droplets and tracer particles. The underlying physical models are the

same, but the book keeping within the code is different to accommodate on-going research at NIST.

FDS 3 input files still run in FDS 4, but some of the effects have changed. See Section 4.5 for details

about changes to particle parameters.

Layer Height A simple calculation of the layer (or interface) height has been added to FDS to enable users

to compare FDS and zone model calculations or to present FDS results in a simplified manner. See

Section 5.11 for details.

2
Chapter 2

Getting Started

Fire Dynamics Simulator (FDS) is a Fortran 90 computer program that solves the governing equations for

thermally-induced fluid flow and fire. A detailed description of the equations and how they are solved

numerically is described in Ref. [1]. The output of FDS is visualized using a computer program called

Smokeview. The User’s Guide for Smokeview is Ref. [2].

2.1 How to get FDS and Smokeview

All of the files associated with FDS and Smokeview are linked to the URL

http://fire.nist.gov/fds

Information about new versions, bug fixes, etc., is found at the web site. Since FDS is not always backward

compatible, the new executable name contains the version number fds#.exe. Users may want to retain

copies of older FDS executables for the purpose of comparing new and old output. The graphics program

Smokeview is backward compatible, and users are urged to replace the old Smokeview files with the new.

The FDS distribution consists of a self-extracting set-up program for Windows-based PCs. Unix, Linux

and Mac users are directed to an anonymous FTP (File Transfer Protocol) site for source code, some compiled executables, Makefiles, etc. After downloading the set-up program to a PC, double-clicking on the

icon walks the user through a series of steps as the program pieces get installed. The most important part

of the installation is the creation of a directory (usually called c:\nist\fds) in which are installed the FDS

and Smokeview executables, the Smokeview preference file smokeview.ini and a few directories containing sample cases, reference manuals, and supplemental data files. The set-up program also defines PATH

variables and associates the .smv file extension to the Smokeview program so that one may either type

Smokeview at any command line prompt or double click on any .smv file.

Users who have already downloaded earlier versions of FDS retain the same file structure as before,

only now new files are distributed into various directories. To avoid naming conflicts, files associated with a

particular version usually have that number somehow worked into the name.

2.2 Computer Hardware Requirements

FDS requires a relatively fast CPU and a substantial amount of random-access memory (RAM). For a

Windows-based PC, the processor should be at least as fast as a 1 GHz Pentium III, with at least 512 MB

RAM. Of course, more is better, and serious users ought to consider purchasing a computer with the fastest

available CPU and largest amount of RAM. Plus, a large hard drive is needed to store the output of calculations. It is not unusual for a single calculation to generate on the order of 1 GB of output files. Most

3
computers now come with hard drives of at least 20 GB. For Unix-based workstations, the processor and

memory should be at least as fast and as large as the PC specifications.

Most computers purchased within the past few years are adequate for running Smokeview with the

caveat that additional memory (RAM) should be purchased to bring the memory size up to at least 512 MB.

This is so the computer can display results without “swapping” to disk. For Smokeview it is more important

to obtain a fast graphics card than a fast CPU. If the computer is to run both FDS and Smokeview, then it is

important to obtain a fast CPU as well.

2.3 Computer Operating System (OS) and Software Requirements

The goal of making FDS and Smokeview publicly available has been to enable practicing fire protection

engineers to perform fairly sophisticated fire simulations at a reasonable cost. Thus, FDS and Smokeview

have been designed for computers running Microsoft Windows, Mac OS X, and various implementations of

Unix/Linux. Since most engineers use MS Windows, compiled versions of FDS and Smokeview are available for this OS. FDS/Smokeview run under any version of Windows except the initial release of Windows

95 that lacks the necessary libraries needed by Smokeview1.

Unix, Linux and Mac users can still run FDS and Smokeview by downloading the appropriate precompiled executables and installing them wherever they see fit. If the pre-compiled FDS executable does not

work (usually because of library incompatibilities), the FDS source code can be downloaded and compiled

using a Fortran 90 and C compiler (See Appendix A for details). If Smokeview does not work on the Linux

or Unix workstation, one should use a Windows PC to view FDS output.

For those wishing to run FDS in parallel, MPI (Message Passing Interface) must be installed on each of

the computers within the cluster. Information about installing MPI on a Windows PC is given in Appendix A.

For other platforms, there are a variety of implementations of MPI that may be suitable. Consult the system

administrator or hardware/software vendor.

1Some users of Windows ME have noticed trouble manipulating the Smokeview window. If given a choice, one ought to run

under Windows 2000 or beyond.

4
Chapter 3

Running FDS

Running FDS is relatively simple. All of the parameters that describe a given fire scenario are typed into

a text file that is referred to as the “data” or “input” file. In this document, the data file is designated as

job name.data, where “job name” stands for any character string that helps to identify the simulation. All

of the output files associated with the calculation have this common prefix.

In addition to the input file, there are often several external files containing input parameters for the

simulation. One such file is referred to as the “database” file, for it contains parameters describing common

materials and fuels. Usually, the database file is kept in a separate directory from that being used for the

calculation. Files containing information about specific sprinklers are also stored along with the database

file. The database and sprinkler files can be modified and/or moved to wherever appropriate.

It is suggested that a new user start with an existing data file, run it as is, and then make the appropriate

changes to the input file for the desired scenario. By running a sample case, the user becomes familiar

with the procedure, learn how to use Smokeview, and ensure that his/her computer is up to the task before

embarking on learning how to create new input files.

3.1 Creating the FDS Input Data File

The input data file provides the program with parameters to describe the scenario under consideration. The

parameters are organized into groups of related variables. For example, the group SURF contains parameters

to describe the properties of solid surfaces. Each line of the input file contains parameters belonging to

the same group. These lines are written as Fortran namelist formatted records. Each record starts with

the character & followed immediately by the name of the namelist group (HEAD, GRID, VENT, etc.),

followed by a list of the input parameters corresponding to that group, and finally terminated with a slash.

Details about the input parameters can be found in Chapter 4.

3.2 Starting an FDS Calculation

There are two ways to run FDS – one way is to run on a single processor (CPU), the other way is to run

on multiple CPUs. The single CPU executable (fds#.exe) works in a similar way to previous versions and

is described presently. The parallel executable (fds# mpi.exe) does not work in the traditional way; the

differences are explained below. Note that the input file for both single and parallel processing is the same.

5
3.2.1 Starting an FDS Calculation (Single Processor Version)

Sample input files are provided with the program for new users who are encouraged to first run a sample

calculation before attempting to write an input file. Assuming that an input file called job name.data exists

in some directory, run the program either in a DOS or Unix command prompt as follows:

Windows: Open up a Command Prompt window, and change directories (“cd”) to where the input file for

the case is, then run the code by typing

fds4 < job_name.data

The character string job name is usually designated within the input file as the CHID. It is recommended

that the name of the input file and the CHID be the same so that all of the files associated with a given

calculation have a consistent name. The input file is read by FDS as standard input (indicated by the “<”

sign), and diagnostic output is written out onto the screen. Unlike early versions of FDS, detailed diagnostic

information is automatically written to a file CHID.out. Do not redirect the screen output to a file.

Unix/Linux: Change directories to where the data file for the case is, then run the code by typing

fds4 < job_name.data

The input parameters are read in as standard input, and error statements and other diagnostics are written

out to the screen. To run the job in the background:

fds4 < job_name.data > job_name.err &

Note that in the latter case, the screen output is stored in the file job name.err and the detailed diagnostics are saved automatically in a file CHID.out, where CHID is a character string, usually the same as

job name, designated in the input file. It is preferable to run jobs in the background so as to free the

console for other uses.

3.2.2 Starting an FDS Calculation (Multiple Processor Version)

Running FDS across a network using multiple processors and multiple banks of memory (RAM) is more

difficult than running the single processor version. More is required of the user to make the connections

between the machines as seamless as possible. This involves creating accounts for a given user on each

machine, sharing directories, increasing the speed of the network, making each machine aware of the others,

etc. Some of these details are handled by the parallel-processing software, others are not. Undoubtedly the

process will be simplified in years to come, but for the moment, parallel-processing is still relatively new and

requires more expertise in terms of understanding both the operating system and the network connections of

a given set of computers.

FDS uses MPI (Message-Passing Interface) [3] to allow multiple computers to run a single FDS job.

Actually, the job must be broken up into multiple meshes, and a processor is assigned to work on each

mesh. Each processor runs an FDS job (called a thread) for its given mesh, and the MPI handles the transfer

of information between meshes. There are different implementations of MPI, much like there are different

Fortran and C compilers. Each implementation is essentially a library of subroutines called from FDS that

transfer data from one thread to another across a fast network. The format of the subroutine calls has been

widely accepted in the community, allowing different vendors and organizations the freedom to develop

better software while working within an open framework.

The way FDS is executed in parallel depends on which implementation of MPI has been installed. To

avoid any conflicts, it was decided to do away with the simple command prompt style of running the single

6
processor version of FDS. Instead, the parallel version of FDS looks for the name of the input file by opening

a one-line text file called fds.data and reading the name of the input file on the first line. The file fds.data

should contain only the name of the real input file job name.data on the first line and nothing else. Note

that all these file names are case-sensitive.

At NIST, the parallel version of FDS is presently run on Windows PCs connected by the Local Area

Network (LAN, 100 Mbps), or on a cluster of Linux PCs linked together with a dedicated, fast (1000 Mbps)

network. The Windows computers use MPICH, a free implementation of MPI from Argonne National

Laboratory, USA. With MPICH, a parallel FDS calculation can be invoked either from the command line or

by using a Graphical User Interface (GUI). After the MPICH libraries are installed on each computer and

the necessary directories are shared, FDS is run using the command issued from one of the computers

mpirun config.txt

where config.txt is a text file containing the name and location of the FDS executable, the working

directory, and the names of the various computers that are to run the job. For example, the config.txt file

might look like this

exe \\machine1\nist\fds\fds4_mpi.exe

dir \\machine1\nist\fds\samples\

hosts

machine1 2

machine2 1

machine3 2

Note that all the computers must be able to access the executable and the working directory on machine1.

This is achieved under Windows by “sharing.” Under Unix/Linux, the process involves cross-mounting the

file systems of the various machines. The numbers following the “host” machines represent the number of

threads to run on that particular machine. In this example, 5 threads are run for an FDS calculation that has

5 meshes.

On the Linux cluster in the Building and Fire Research Lab at NIST, LAM/MPI, a free implemenation

from Indiana University, is installed. With LAM/MPI, the computers to be used are linked prior to the actual

execution of FDS with a separate command called a “lamboot.” FDS is then run using the command

mpirun -np 5 fds4_mpi

where the 5 indicates that 5 processors are to be used. In this case, the executable fds4 mpi is located in the

working directory. To make the process run in the background

mpirun -np 5 fds4_mpi > job_name.err &

The file job name.err contains what is normally printed out to the screen.

In Appendix A, there is a detailed description of how one compiles and runs FDS in parallel under

Windows using MPICH. For more information about LAM/MPI, visit the web site

http://www.lam-mpi.org/

Note that there are several other implementations of MPI, some free, some not. Support for the software

varies, thus FDS has been designed to run under any of the more popular versions without too much user

intervention. However, keep in mind that parallel processing is a relatively new area of computer science,

and there are bound to be painful growth spurts in the years ahead.

7
3.3 Monitoring Progress

Diagnostics for a given calculation are written into a file called CHID.out. The CPU usage and simulation

time are written here, so one can see how far along the program has progressed. At any time during a

calculation, Smokeview can be run and the progress can be checked visually. To stop a calculation before

its scheduled time, either kill the process, or preferably create a file in the same directory as the output files

called CHID.stop. The existence of this file stops the program gracefully, causing it to dump out the latest

flow variables for viewing in Smokeview.

Since calculations can be hours or days long, there is a restart feature in FDS. Details of how to use this

feature are given in Section 5.1. Briefly, specify at the beginning of calculation how often a “restart” file

should be saved. Should something happen to disrupt the calculation, like a power outage, the calculation

can be restarted from the time the last restart file was saved.

3.4 Error Statements

An FDS calculation may end before the user-prescribed time limit. Following is a list of common error

statements and how to diagnose the problems:

Input File Error: The most common errors in FDS are due to mis-typed input statements. These errors

result in the immediate halting of the program and a statement like, “ERROR: Problem with the

HEAD line.” For these errors, check the line in the input file named in the error statement. Make sure

the parameter names are spelled correctly. Make sure that a / is put at the end of the record. Make

sure that the right type of information is being provided for each parameter, like whether one real

number is expected, or several integers, or whatever. Make sure there are no non-ASCII characters

being used, as can sometimes happen when text is cut and pasted from other applications or wordprocessing software. Make sure zeros are zeros and O’s are O’s. Make sure 1’s are not !’s. Make sure

apostrophes are used to designate character strings. Make sure the text file on a Unix/Linux machine

was not created on a DOS machine, and vice versa. Make sure that all the parameters listed are still

being used – new versions of FDS often drop or change parameters to force users to re-examine old

input files.

Numerical Instability: It is possible that during an FDS calculation the flow velocity at some location in

the domain can increase due to numerical error causing the time step size to decrease to a point where

logic in the code decides that the results are unphysical and stops the calculation with an error message

in the file CHID.out. In these cases, FDS ends by dumping out one final Plot3D file giving the user

some means by which to see where the error is occurring within the computational domain. Usually,

a numerical instability can be identified by fictitiously large velocity vectors emanating from a small

region within the domain. Common causes of such instabilities are grid cells that have an aspect ratio

larger than 2 to 1, high speed flow through a small opening, a sudden change in the heat release rate,

or any number of sudden changes to the flow field. There are various ways to solve the problem,

depending on the situation. Try to diagnose and fix the problem before reporting it. It is difficult for

anyone but the originator of the input file to diagnose the problem.

Inadequate Computer Resources: The calculation might be using more RAM than the machine has, or

the output files could have used up all the available disk space. In these situations, the computer may

or may not produce an intelligible error message. Sometimes the computer is just unresponsive. It

is the user’s responsibility to ensure that the computer has adequate resources to do the calculation.

Remember, there is no limit to how big or how long FDS calculations can be – it depends on the

resources of the computer. For any new simulation, try running the case with a modest-sized grid, and

8
gradually make refinements until the computer can no longer handle it. Then back off somewhat on

the size of the calculation so that the computer can comfortably run the case. Trying to run with 90

Run-Time Error: An error occurs either within the computer operating system or the FDS program. An

error message is printed out by the operating system of the computer onto the screen or into the

diagnostic output file. This message is most often unintelligible to most people, including the programmers, although occasionally one might get a small clue if there is mention of a specific problem,

like “stack overflow,” “divide by zero,” or “file write error, unit=...” These errors may be caused by

a bug in FDS, for example if a number is divided by zero, or an array is used before it is allocated,

or any number of other problems. Before reporting the error, try to systematically simplify the input

file until the error goes away. This process usually brings to light some feature of the calculation

responsible for the problem and helps in the debugging.

Poisson Initialization: Sometimes at the very start of a calculation, an error appears stating that there is a

problem with the “Poisson initialization.” The equation for pressure in FDS is known as the Poisson

equation. The Poisson solver consists of large system of linear equations that must be initialized at the

start of the calculation. Most often, an error in the initialization step is due to a grid dimension being

less than 4 (except in the case of a two-dimensional calculation). It is also possible that something

is fundamentally wrong with the coordinates of the computational domain. Diagnose the problem by

checking the GRID and Physical DIMension (PDIM) lines in the input file.

3.5 Reporting Bugs

Because FDS development is on-going, problems will inevitably occur with various routines and features.

The developers need to know if a certain feature is not working, and bug reporting is encouraged. However,

the problem must be clearly identified. The best way to do this is to simplify the input file as much as

possible so that the bug can be diagnosed. Also, limit the bug reports to those features that clearly do not

work. Physical problems such as fires that do not ignite, flames that do not spread, etc., may be related to the

grid resolution or scenario formulation and need to be investigated first by the user before being reported.

If an error message originates from the operating system as opposed to FDS, first investigate some of

the obvious possibilities, such as memory size, disk space, etc. If that does not solve the problem, report the

bug with as much information about the error message and circumstances related to the problem. The input

file should be simplified as much as possible so that the bug occurs early in the calculation. The input file

should have no references to external databases. In this way, the developers can quickly run the problem

input file and hopefully diagnose the problem.

9
10
Chapter 4

Setting up the Input File for FDS

The first step in performing a calculation is to generate a text input file that provides the program with

all of the necessary information to describe the scenario under consideration. The most important inputs

determine the physical size of the overall rectangular domain, the grid dimensions, and the additional geometrical features. Next, the fire and other boundary conditions must be specified. Finally, there are a number

of parameters that customize the output files to capture the most important flow quantities. Input data is prescribed by writing a small file that uses the namelist formatted records. Each line of the file begins with

the character & followed immediately by the name of the namelist group (HEAD, GRID, VENT, etc.),

followed by a space or comma delimited list of the input parameters corresponding to that group. Each list

is terminated with a slash. Note that the parameters listed are only those that need to be changed from the

default. The structure of an input file is shown below.

&HEAD CHID=’sample’,TITLE=’A Sample Input File’ /

&GRID IBAR=24,JBAR=24,KBAR=48 /

&PDIM XBAR0=-.30,XBAR=0.30,YBAR0=-.30,YBAR=0.30,ZBAR=1.2 /

&TIME TWFIN=10. /

&MISC RADIATION=.FALSE. /

&SURF ID=’burner’,HRRPUA=1000. /

&OBST XB=-.20,0.20,-.20,0.20,0.00,0.05,SURF_IDS=’burner’,’INERT’,’INERT’ /

&VENT CB=’XBAR’ ,SURF_ID=’OPEN’ /

&VENT CB=’ZBAR’ ,SURF_ID=’OPEN’ /

&SLCF PBY=0.,QUANTITY=’TEMPERATURE’ /

&BNDF QUANTITY=’HEAT_FLUX’ /

The parameters in the input file can be integers (IBAR=24), real numbers (XBAR=0.30), groups of

real numbers (XB=-.20,0.20,...), character strings (CHID=’sample’), groups of character strings

(SURF IDS = ’burner’ ’INERT’ ’INERT’), or logicals (RADIATION=.FALSE.). A logical parameter is either .TRUE. or .FALSE. – the periods are a Fortran convention. Character strings that are

listed in this User’s Manual ought to be copied exactly as written – the code is case sensitive and underscores

do matter. Also note that character strings can be enclosed either by apostrophes or quotation marks. Be

careful not to create the input file by pasting text from something other than a simple text editor, in which

case the punctuation marks may not transfer properly into the text file.

Input parameters can be separated by either a comma, space, or line break. Comments and notes can be

written into the file so long as nothing comes between the ampersand & and the slash / except appropriate

parameters corresponding to that particular namelist group. Note that FDS is case-sensitive. Copy exactly

the parameter names from this manual and do not assume that the program understands if the case is changed.

Rarely does anyone actually write an input file from scratch. Usually, one takes a sample input file that

has been distributed with the FDS release and modifies it appropriately. It is strongly encouraged that when

11
looking at a new scenario, first select a pre-written input file that resembles the case, make the necessary

changes, then run the case at fairly low resolution to determine if the geometry is set up correctly. It is best

to start off with a relatively simple file that captures the main features of the problem without getting tied

down with too much detail that might mask a fundamental flaw in the calculation. Initial calculations ought

to be gridded coarsely so that the run times are less than an hour and corrections can easily be made without

wasting too much time.

12
4.1 Preliminaries

The first few lines in the input file handle some custodial details like naming the job and establishing the time

of the simulation. The name of the job is important because often a project involves numerous simulations

in which case the names of the individual simulations can help organize the effort.

4.1.1 Naming the Job: The HEAD Namelist Group

The first thing to do when setting up an input file is to give the job a name. The namelist group HEAD

contains two parameters. CHID is character string of 30 characters or less used to tag output files with

a given character string. If, for example, CHID=’sample’, it is convenient to name the input data file

sample.data so that the input file can be associated with the output files. No periods or spaces are allowed

in CHID because the output files are tagged with suffixes that are meaningful to certain computer operating

systems. TITLE is a character string of 60 characters or less that describes the problem.

&HEAD CHID=’sample’,TITLE=’A Sample Input File’ /

4.1.2 Setting Time Limits: The TIME Namelist Group

TIME is the name of a group of parameters defining the time duration of the simulation and the initial time

step used to advance the solution of the discretized equations. Usually, only the duration of the simulation

is required on this line, via the parameter TWFIN (Time When FINished). The default is 1 s. If TWFIN is

set to zero, only the set-up work is performed, allowing one to quickly check the geometry in Smokeview.

The initial time step size can also be prescribed with DT. This parameter is normally set automatically

by dividing the size of a grid cell by the characteristic velocity of the flow. During the calculation, the time

step is adjusted so that the CFL condition is satisfied. The default value of DT is 5(δxδyδz)

1

3 /

√

gH s, where

δx, δy, and δz are the dimensions of the smallest grid cell, H is the height of the computational domain, and

g is the acceleration of gravity.

One additional parameter in the TIME group is SYNCHRONIZE, a logical flag (.TRUE. or .FALSE.)

indicating that in a parallel computation the time step for each mesh should be the same, thus ensuring that

each mesh is processed each iteration. More details can be found in Section 4.2.3.

13
4.2 The Numerical Grid

All FDS calculations must be performed within a domain that is made up of rectangular meshes, each with

its own rectilinear grid. All obstructions, vents, etc. are forced to conform with the numerical grid(s). To

establish a grid, first specify the overall physical dimensions of the rectangular grid via the PDIM namelist

group. Second, specify the number of grid cells spanning each coordinate direction via the GRID namelist

group. Finally, if desired, the grid cells can be stretched or shrunk in two of three coordinate directions via

the TRNX, TRNY, and/or TRNZ groups (See Section 5.2). For cases in which more than one grid is used in

the calculation, see Section 4.2.3 below for guidelines.

4.2.1 Defining the Computational Domain: The PDIM Namelist Group

PDIM is the name of the group of parameters defining the size of the physical domain. The coordinate

system spanned by these dimensions conforms to the right hand rule (See Fig. 4.1). The physical domain is

a single right parallelepiped, i.e. a box. The origin of the domain is the point (XBAR0,YBAR0,ZBAR0),

and the opposite corner of the domain is at the point (XBAR,YBAR,ZBAR). By default, XBAR0, YBAR0,

ZBAR0 are zero, in which case the physical dimensions of the domain are given as XBAR, YBAR and ZBAR

in units of meters. Unless otherwise directed, the domain is subdivided uniformly to form a grid of IBAR by

JBAR by KBAR cells specified by the GRID namelist group. If it is desired that the grid cells not be uniform

in size, then the namelist groups TRNX, TRNY and/or TRNZ may be used to alter the uniform gridding (See

Section 5.2).

Any obstructions or vents that extend beyond the boundary of the physical domain are cut off at the

boundary. There is no penalty for defining objects outside of the domain, but these objects do not appear in

Smokeview.

4.2.2 Setting the Grid Size: The GRID Namelist Group

The namelist group GRID contains the dimensions of the computational grid. The grid consists of IBAR

cells in the x direction, JBAR cells in the y direction, and KBAR cells in the z direction. Usually, the z

direction is assumed to be the vertical direction. The longer horizontal dimension should be taken as the

x-direction. Note that it is best if the grid cells are close to cubes, that is, the length, width and height of the

cells ought to be roughly the same. Also, because an important part of the calculation uses a Poisson solver

based on Fast Fourier Transforms (FFTs), the dimensions of the grid should each be of the form 2l 3

m 5n

,

where l, m and n are integers. For example, 64 = 2

6

, 72 = 2

332

and 108 = 2

233

are good grid dimensions.

However, 37, 99 and 109 are not.

&GRID IBAR=64,JBAR=32,KBAR=32 /

Following is a list of numbers between 1 and 1024 that can be factored down to 2’s, 3’s and 5’s:

2 3 4 5 6 8 9 10 12 15

16 18 20 24 25 27 30 32 36 40

45 48 50 54 60 64 72 75 80 81

90 96 100 108 120 125 128 135 144 150

160 162 180 192 200 216 225 240 243 250

256 270 288 300 320 324 360 375 384 400

405 432 450 480 486 500 512 540 576 600

625 640 648 675 720 729 750 768 800 810

864 900 960 972 1000 1024

14
Figure 4.1: An example of a multiple-mesh geometry.

Note that IBAR, JBAR and KBAR should be at least 4, except for two-dimensional calculations, in which

case JBAR=1.

4.2.3 Multiple Meshes and Parallel Processing

The term “multiple meshes” means that the computational domain consists of more than one rectangular

mesh, usually connected although this is not required. In each mesh, the governing equations are solved

with a time step based on the flow speed within that particular mesh. Because each mesh can have different

time steps, this technique can save CPU time by requiring relatively coarse meshes to be updated only when

necessary. Coarse meshes are best used in regions where temporal and spatial gradients of key quantities

are small or unimportant. Also, to run FDS in parallel, one needs to break up the computational domain into

multiple meshes so that each processor receives one mesh to work on. Whether the calculation is to be run

on a single processor, or on multiple processors, the rules of prescribing multiple meshes are similar, with

some issues to keep in mind. Here is a list of guidelines and warnings about the use of multiple meshes.

• If more than one mesh is used, there should be a GRID and PDIM line for each. The order in which

these lines are entered in the input file matters. In general, the meshes should be entered from finest

to coarsest. FDS assumes that a mesh listed first has precedence over a mesh listed second if the two

meshes overlap. Meshes can overlap, abut, or not touch at all. In the last case, essentially two separate

15
calculations are performed with no communication at all between them. Obstructions and vents are

entered in terms of the overall coordinate system and need not apply to any one particular mesh. Each

mesh checks the coordinates of all the geometric entities and decides whether or not they are to be

included.

• Avoid putting mesh boundaries where critical action is expected, especially fire. Sometimes fire

spread from mesh to mesh cannot be avoided, but if at all possible try to keep mesh interfaces relatively

free of complicating phenomena since the exchange of information across mesh boundaries is not as

accurate as cell to cell exchanges within one mesh.

• Information from other meshes is received only at the exterior boundary of a given mesh. This means

that a mesh that is completely embedded within another receives information at its exterior boundary,

but the larger mesh receives no information from the mesh embedded within. Essentially, the larger,

usually coarser, mesh is doing its own simulation of the scenario and is not affected by the smaller,

usually finer, mesh embedded within it. Details within the fine grid, especially related to fire growth

and spread, may not be picked up by the coarse grid. In such cases, it is preferable to isolate the

detailed fire behavior within one mesh, and position coarser meshes at the exterior boundary of the

fine mesh. Then the fine and coarse meshes mutually exchange information.

• Experiment with different mesh configurations using relatively coarse grid cells to ensure that information is being transferred properly from mesh to mesh. There are two issues of concern. First, does

it appear that the flow is being badly affected by the mesh boundary? If so, try to move the mesh

boundaries away from areas of activity. Second, is there too much of a jump in cell size from one

mesh to another? If so, consider whether the loss of information moving from a fine to a coarse mesh

is tolerable.

• Be careful when using the shortcut convention of declaring an entire face of the domain to be an OPEN

vent. Every grid takes on this attribute. See Section 4.4.6 for more details.

• If more than one mesh is used in a calculation, there can be no background pressure rise. Essentially,

the different compartments are assumed to leak.

• In a parallel calculation, one can force the time steps in all meshes to be the same by setting

SYNCHRONIZE=.TRUE.

on the TIME line. With this setting, all meshes are active each iteration. For a single-processor, multiple mesh calculation, this strategy reduces and may even eliminate any benefit seen by using multiple

meshes. However, in a parallel calculation, if a particular mesh is inactive during an iteration because

it is not ready to be updated, then the processor assigned to that mesh is also inactive. Forcing the mesh

to be updated with a smaller than ideal time step does not cost anything since that processor would

have been idle anyway. The benefit is that there is a tighter connection between meshes. It is also possible to synchronize the time step in a select set of meshes. To do this, add SYNCHRONIZE=.TRUE.

to the appropriate GRID lines. Do not then add SYNCHRONIZE=.TRUE. to the TIME line as it

over-rides the GRID line settings.

• If an planar obstruction is close to where two meshes abut, make sure that each mesh “sees” the

obstruction. If the obstruction is even a millimeter outside of one of the meshes, that mesh may not

account for it, in which case information is not transferred properly between meshes.

16
• When running a case with multiple meshes in parallel, the efficiency of the calculation can be checked

as follows: (1) Set SYNCHRONIZE=.TRUE. on the TIME line, (2) Let the program run several

hundred time steps, (3) Calculate the difference in wall clock time between two 100 iteration print

outs in the file CHID.out (see Section C.1). Divide the time difference by 100. This is the average

elapsed wall clock time per time step, (4) Look at the CPU/step for each mesh. The largest value

should be less than, but close to, the average elapsed wall clock time. The efficiency of the parallel

calculation is the maximum CPU/step divided by the average wall clock time per step. If this

number is between 90 % and 100 %, the parallel code is working well.

4.3 Setting Global Parameters: The MISC Namelist Group

MISC is the namelist group of miscellaneous input parameters. Only one MISC line should be entered in

the data file. The MISC parameters vary in scope and degree of importance. The most important parameter in this category is the one that determines whether a Large Eddy Simulation (LES) calculation is to be

performed, or whether a Direct Numerical Simulation (DNS) is to be performed. By default, an LES calculation is performed. If a DNS calculation is desired, enter DNS=.TRUE. on the MISC line. An example of

a MISC line is

&MISC SURF_DEFAULT=’CONCRETE’,REACTION=’METHANE’,

DATABASE=’c:\nist\fds\database4\database4.data’ /

This establishes that all bounding surfaces are to be made of CONCRETE unless otherwise indicated, that the

combustion stoichiometry is for METHANE, and that the definition of CONCRETE, METHANE, and various

other keywords throughout the input file are found in the file defined by DATABASE. Other inputs found on

the MISC line include:

DATABASE A character string indicating the name of a file that contains information about surface materials

and reaction parameters for various fuels. The DATABASE file does not need to be designated if none

of its entries are to be used.

DATABASE DIRECTORY A character string indicating the full path name of the directory where the database

and sprinkler files are stored. If DATABASE DIRECTORY is specified, there is no need to specify a

DATABASE file, it is assumed to be database4.data.

SURF DEFAULT Character string indicating which of the listed SURF IDs is to be considered the default.

The default is ’INERT’. SURF is a namelist group describing the properties of vents and surfaces,

and is discussed in Section 4.4.1.

REACTION Character string indicating which of the listed groups of reaction (REAC) parameters are to be

used. The default is ’PROPANE’, meaning that unless REACTION is specified, it is assumed that the

fuel is propane. See Section 4.4.2 for a description of reaction parameters.

TMPA Ambient temperature in degrees Celsius. (Default 20 ◦C)

U0, V0 and W0 Initial values of velocity components in m/s. These can be used to prescribe an initial

wind through the domain. (Default 0 m/s)

TMPO Temperature outside the computational domain, in degrees Celsius. (Default 20 ◦C)

NFRAMES Default number of output dumps per calculation. Thermocouple data, slice data, particle data,

and boundary data is saved every TWFIN/NFRAMES unless otherwise specified with DTSAM on the

THCP, SLCF, and BNDF namelist lines. (Default 1000)

17
DTPAR Time increment in seconds between Lagrangian particle insertions at solid surfaces. If more particles are desired, lower the input value of this parameter. (Default 0.05 s)

DTSPAR Time increment in seconds between droplet insertions at sprinklers. (Default 0.05 s)

DTSAM PART Time increment between tracer particle (and sprinkler droplet) data dumps in seconds. These

dumps add to a file called CHID.part which can be used to produce an animation of the flow field.

(Default TWFIN/NFRAMES)

NPPS Number of particles per set. The maximum number of particles that can be output into the file

CHID.part every DTSAM seconds. (Default 100000)

MAXIMUM DROPLETS Maximum number of Lagrangian particles per mesh. (Default 500000)

18
4.4 Prescribing the Geometry and the Fire

Most of the work in setting up a calculation lies in specifying the geometry of the space to be modeled

and applying boundary conditions to these objects. The geometry is described in terms of rectangular

obstructions that can heat up, burn, conduct heat, etc.; and vents from which air or fuel can be either injected

into, or drawn from, the flow domain. A boundary condition needs to be assigned to each obstruction

and vent describing its thermal properties. A fire is just one type of boundary condition. The following

namelist groups describe how to prescribe the boundary conditions and the obstructions and vents to which

the boundary conditions are assigned.

4.4.1 Prescribing Boundary Conditions: The SURF Namelist Group

SURF is the namelist group that defines boundary conditions for all solid surfaces or openings within or

bounding the flow domain. The physical coordinates of obstructions or vents are listed in the OBST and

VENT namelist groups below. Boundary conditions for the obstructions and vents are prescribed by referencing the appropriate SURF line(s) whose parameters are described presently.

The default boundary condition for all solid surfaces is that of a cold, inert wall. If only this boundary

condition is needed, there is no need to add any SURF lines to the input file. If additional boundary conditions are desired, they are to be listed one boundary condition at a time. Each SURF line consists of an

identification string ID=’...’ to allow references to it by an obstruction or vent. Thus, on each OBST and

VENT line, the character string SURF ID=’...’ indicates the ID of the SURF line containing the desired

boundary condition parameters. If a particular SURF line is to be applied as the default boundary condition,

CONCRETE for example, set SURF DEFAULT=’CONCRETE’ on the MISC line.

Fire (Mixture Fraction Model) A fire is basically modeled as the ejection of pyrolyzed fuel from a solid

surface or vent that burns when mixed with oxygen. This is the default mixture fraction model of combustion. Specify either a heat release rate per unit area or a heat of vaporization at the fuel surface. The

stoichiometry of the reaction is set by the parameter REACTION on the MISC line. All of the species associated with the combustion process are accounted for by way of the mixture fraction variable and should

not be explicitly prescribed. The exception to this rule is where a non-reacting gas is introduced into the

domain that merely serves as a diluent, like CO2 from an extinguisher or H2O from evaporated sprinkler

droplets (see Section 5.5 for details). If a finite rate combustion model is desired instead of the default

mixture fraction model, see Section 5.6.

Following is a list of parameters that are prescribed on a SURF line to designate a fire using the mixture

fraction approach.

HRRPUA Heat Release Rate Per Unit Area (kW/m2). This parameter is used to control the burning rate of

the fuel, as in the case of a prescribed fire using a gas burner. If all one desires is a fire of a given size,

then HRRPUA is the only thing that need be set, for example

&SURF ID=’FIRE’,HRRPUA=500. /

applies 500 kW/m2to any surface with the attribute SURF ID=’FIRE’. See the discussion of Time

Dependent Boundary Conditions below to learn how to ramp the heat release rate up and down.

HEAT OF VAPORIZATION (kJ/kg). This is an alternative to HRRPUA. This is the amount of energy required to vaporize a solid or liquid fuel once it has reached its ignition temperature TMPIGN. If it is

desired that the burning rate of the fuel be dependent on heat feedback from the fire, use this parameter

rather than HRRPUA. Do not specify HRRPUA and HEAT OF VAPORIZATION on the same SURF

19
line. They are mutually exclusive inputs. Also, if HEAT OF VAPORIZATION is specified for a given

material, something else must serve as an ignition source to ignite the material.

BURN AWAY If a burning object is to disappear from the calculation once it is exhausted of fuel, set

BURN AWAY=.TRUE.. Use this parameter cautiously. If an object has the potential of burning away,

a significant amount of extra memory has to be set aside to store additional surface information as

the rectangular block is eaten away. Note that in previous versions of FDS (3 and lower), the parameter DENSITY or SURFACE DENSITY controlled both burn out and the removal of burnt objects.

This is no longer true. If BURN AWAY is prescribed as a SURF parameter, then a solid object with

this SURF ID disappears from a calculation as the mass of each of its grid cells is consumed. The

mass of each grid cell is the volume of the grid cell multiplied by the DENSITY of the obstruction.

BURN AWAY can be applied to thermally-thin or thick materials, as long as a DENSITY is also prescribed and the obstruction is at least one grid cell wide. Note also that if BURN AWAY is prescribed,

the SURF should be applied to the entire object, not just a face of the object because it is unclear how

to handle edges of solid obstructions that have different SURF IDs on different faces. Also note that

the amount of combustible fuel equals the DENSITY times the volume of the grid cell. If the volume

of the obstruction changes because it has to conform to the uniform grid, FDS does not adjust the

burning rate to account for this as it does with various quantities associated with areas, like HRRPUA.

Thermal Boundary Conditions: There are four types of thermal boundary conditions: fixed temperature solid surface, fixed heat flux solid surface, thermally-thick solid or thermally-thin sheet. For a given

boundary condition (i.e. for the same SURF line), choose only one of these. For a solid surface of fixed

temperature, set TMPWAL to be the surface temperature in units of ◦C. For a solid surface of fixed convective

heat flux, set HEAT FLUX to be the convective heat flux in units of kW/m2

. If HEAT FLUX is positive, the

wall heats up the surrounding gases. If HEAT FLUX is negative, the wall cools the surrounding gases.

A solid surface that heats up due to radiative and convective heat transfer from the surrounding gas can

be either thermally-thick or thermally-thin. For a thermally-thick solid, prescribe the thermal conductivity

KS (W/m·K), DENSITY (kg/m3), specific heat C P (kJ/kg/K), and the thickness DELTA (m) of the material1.

Both KS and C P can be functions of temperature. DENSITY cannot be a function of temperature. See the

discussion of RAMPs below for more details. The prescription of the thermal conductivity directs the code to

perform a one-dimensional heat transfer calculation across the thickness of the material 2. The thickness is

not the same as the thickness of the entire wall, but rather the lining material that forms the outermost layer

of the wall. See discussion below for more details.

For thermally-thin wall linings, prescribe C DELTA RHO, the product of the specific heat (kJ/kg/K),

density (kg/m3), and thickness (m) of the liner. A thermally-thin liner is assumed to be the same temperature

throughout its width. These three parameters may be prescribed individually using C P (kJ/kg/K), DELTA

(m) and DENSITY (kg/m3), in which case, C P can be made temperature-dependent. Note that the absence

of thermal conductivity directs the code to assume the material is thermally-thin instead of thick. If the

thermal conductivity is prescribed, a thermally-thick calculation is performed.

Fixed temperature or fixed heat flux boundary conditions are easy to apply, but only of limited usefulness in real fire scenarios. In most cases, walls, ceilings and floors are made up of several layers of lining

materials, the most important of which is the outermost layer. FDS only considers the thermal properties for

1

In older versions of FDS, the thermal diffusivity ALPHA (m2/s) was used to represent k/ρ/cp. This parameter can still be used,

but individual prescription of k, ρ and cp is preferred.

2The default number of nodes used in the one-dimensional heat conduction calculation into a thermally-thick solid is 20. To

change this parameter, WALL POINTS can be added to the SURF line. Note that the nodes are not uniformly spaced, but rather are

clustered so that the first cell in the solid is approximately 0.1 mm. This value may be changed by adding the parameter DX SOLID

to the SURF line. See the FDS Technical Reference Guide [1] for details about the heat transfer calculation.

20
this outermost layer. It is assumed that this layer backs up to an air gap at ambient temperature (like a sheet

of gypsum board attached to wood studs), or it backs up to an insulated material in which case no heat is lost

to the backing material, or it backs up to the room on the other side of the wall. By default, it is assumed

that the wall liner backs up to an air gap. If the wall liner is assumed to back up against an insulating material, like a sheet of steel attached to a fiber insulating board, the expression BACKING=’INSULATED’

on the SURF line prevents any heat loss from the back side of the material. An example of where this

might be used is in home furnishing. Recent work by Fleischmann and Chen [4] on the ignition properties of upholstery suggests that treating a fabric covered slab of polyurethane foam as thermally-thin

produces a slightly better correlation than thermally-thick. If their thermally-thin data is used, the attribute

BACKING=’INSULATED’ should be invoked. Finally, if it is desired that the heat transfer through the

wall into the space behind the wall, the attribute BACKING=’EXPOSED’ should be listed. This feature

only works if the wall is one grid cell thick, and if there is a non-zero volume of computational domain on

the other side of the wall. Obviously, if the wall is an external boundary of the domain, the heat is lost to the

void.

The emissivity of a solid surface may be set with EMISSIVITY, which is 1 by default. If the wall

lining material is flammable, set its ignition temperature with TMPIGN, the temperature (◦C) at which the

material begins burning. This is only set if the wall liner is thermally-thick or thermally-thin. Heat fluxes to

solid surfaces are both convective and radiative. If TMPIGN is set, a heat release rate per unit area HRRPUA

or HEAT OF VAPORIZATION should also be given. (Default: TMPIGN is 5000 ◦C, i.e. no burning occurs

unless this parameter is explicitly prescribed.)

The following are a few examples of SURF lines. These and several others are found in the DATABASE

file.

&SURF ID = ’CONCRETE’

FYI = ’Thermally-thick material’

KS = 1.0

C_P = 0.88

DENSITY = 2000.

DELTA = 0.2 /

&SURF ID = ’UPHOLSTERY’

FYI = ’Assumed thermally-thin material’

C_DELTA_RHO = 1.29

BACKING = ’INSULATED’

TMPIGN = 280.

DENSITY = 20.0

HEAT_OF_VAPORIZATION=2500. /

&SURF ID = ’SHEET METAL’

FYI = ’Thermally-thin material’

C_DELTA_RHO = 4.7 /

Velocity Boundary Condition Velocity boundary conditions affect both the normal and tangential components of the velocity vector at boundaries. The normal component of velocity is controlled by the parameter

VEL. If VEL is negative, the flow is entering the computational domain. If VEL is positive, the flow is exiting the domain. Sometimes it is desired that a given volume flux through a vent be prescribed rather than a

velocity. If this is the case then VOLUME FLUX can be prescribed instead of VEL. The units are m3

/s. If the

flow is entering the computational domain, VOLUME FLUX should be a negative number. Note that either

VEL or VOLUME FLUX should be prescribed, not both. The choice depends on whether an exact velocity

is desired at a given vent, or whether the given volume flux is desired. The dimensions of the vent that are

prescribed usually change because the prescribed vent dimensions are sometimes altered so that the vent

21
edges line up with grid cells. Also note that a SURF group with a VOLUME FLUX prescribed should only be

called by a VENT, not an OBST. Finally, note that if HRRPUA or HEAT OF VAPORIZATION is prescribed,

no velocity should be prescribed. The combustible gases are ejected at a velocity computed by the code.

As an example, a simple blowing vent would be described by the line

&SURF ID=’BLOWER’,VEL=-1.2,TMPWAL=50. /

The vent with SURF ID=’BLOWER’ would blow 50 ◦C air at 1.2 m/s into the flow domain. Making VEL

positive would suck air out, in which case TMPWAL would not be necessary.

The tangential velocity boundary condition controls how the gas “sticks” to a solid surface. In theory,

the tangential component of velocity is zero at the surface, but increases rapidly through a narrow region

called the boundary layer. For most practical problems, the grid is not fine enough to resolve the boundary

layer, which is typically a few millimeters thick. For this reason, in an LES calculation, the velocity at

the wall is set to be a fraction of its value in the grid cell adjacent to the wall. Only in a DNS calculation

is the velocity at the wall set to zero. To alter these defaults, set a parameter called VBC. This parameter

ranges from -1 to 1. If a no-slip wall is desired, VBC=-1. If a free-slip wall is desired, VBC=1. Numbers in

between -1 and 1 can represent partial slip conditions, which may be appropriate for simulations involving

large grid cells. (Default VBC is 0.5 for LES, -1.0 for DNS)

In the case of a blowing vent (or even a solid surface), it is possible to prescribe both the normal and

tangential components of the flow (or just the tangential). The normal component is specified with VEL as

described above. The tangential is prescribed via a pair of real numbers VEL T representing the desired

tangential velocity components. For example, the line

&SURF ID=’LOUVER’,VEL=-1.2,VEL_T=0.5,-0.3 /

is a boundary condition for a louver vent that pushes air into the space with a normal velocity of 1.2 m/s, and

with a tangential velocity of 0.5 m/s in either the x or y direction and -0.3 m/s in either the y or z direction,

depending on what the normal direction is.

Time Dependent Boundary Conditions At the start of any calculation, the temperature is ambient everywhere, the flow velocity is zero everywhere, nothing is burning, and the mass fractions of all species are

uniform. When the calculation starts temperatures, velocities, burning rates, etc., are ramped-up from their

starting values because nothing can happen instantaneously. By default, everything is ramped-up to their

prescribed values in roughly 1 s. However, control the rate at which things turn on, or turn off, by specifying time histories for the boundary conditions that are listed on a given SURF line. The above boundary

conditions can be made time-dependent using either prescribed functions or user-defined functions. The

parameters TAU Q and TAU V indicate that thermal or hydrodynamic quantities are to ramp up to their prescribed values in TAU seconds and remain there. TAU Q is the characteristic ramp-up time of the heat release

rate per unit area HRRPUA or wall temperature TMPWAL. TAU V is the ramp-up time of the normal velocity

at a surface VEL or the volume flux VOLUME FLUX. If TAU Q is positive, then the heat release rate ramps

up like tanh(t/τ). If negative, then the HRR ramps up like (t/τ)

2

. If the fire ramps up following a t

2

curve, it

remains constant after TAU Q seconds. These rules apply to TAU V as well. The default value for all TAUs

is 1 s. If something other than a tanh or t

2

ramp up is desired, then a user-defined burning history must be

input. To do this, set RAMP Q or RAMP V equal to a character string designating the ramp function to use

for that particular surface type, then somewhere in the input file generate lines of the form:

&RAMP ID=’rampname1’,T= 0.0,F=0.0 /

&RAMP ID=’rampname1’,T= 5.0,F=0.5 /

&RAMP ID=’rampname1’,T=10.0,F=0.7 /

.

22
.

.

&RAMP ID=’rampname2’,T= 0.0,F=0.0 /

&RAMP ID=’rampname2’,T=10.0,F=0.3 /

&RAMP ID=’rampname2’,T=20.0,F=0.8 /

.

.

.

Here, T is the time, and F indicates the fraction of the heat release rate, wall temperature, velocity, mass

fraction, etc., to apply. Linear interpolation is used to fill in intermediate time points. Be sure that the

prescribed function starts at T=0., the ignition time. Note that the TAUs and the RAMPs are mutually

exclusive. For a given surface quantity, both cannot be prescribed.

As an example, the simple blowing vent from above can be controlled via the lines

&SURF ID=’BLOWER’,VEL=-1.2,TMPWAL=50.,

RAMP_V=’BLOWER RAMP’,

RAMP_Q=’HEATER RAMP’ /

&RAMP ID=’BLOWER RAMP’,T= 0.0,F=0.0 /

&RAMP ID=’BLOWER RAMP’,T=10.0,F=1.0 /

&RAMP ID=’BLOWER RAMP’,T=80.0,F=1.0 /

&RAMP ID=’BLOWER RAMP’,T=90.0,F=0.0 /

&RAMP ID=’HEATER RAMP’,T= 0.0,F=0.0 /

&RAMP ID=’HEATER RAMP’,T=20.0,F=1.0 /

&RAMP ID=’HEATER RAMP’,T=30.0,F=1.0 /

&RAMP ID=’HEATER RAMP’,T=40.0,F=0.0 /

Now the temperature and velocity of the incoming air stream would follow the same ramp functions. Note

that the temperature and velocity can be independently controlled by assigning different RAMPs to RAMP Q

and RAMP V, respectively.

Temperature-Dependent Boundary Conditions Certain thermal parameters like the specific heat of the

solid (C P) or the thermal conductivity of the solid (KS) can be made temperature-dependent using the

RAMP convention. As an example, take the material properties for marinite, a wall material suitable for high

temperature applications.

&SURF ID=’MARINITE’

RGB = 0.70,0.70,0.70

BACKING = ’EXPOSED’

EMISSIVITY=0.8

DENSITY = 737.

RAMP_C_P=’rampcp’

RAMP_KS=’rampks’

DELTA=0.0254 /

&RAMP ID=’rampks’,T= 24.,F=0.13 /

&RAMP ID=’rampks’,T=149.,F=0.12 /

&RAMP ID=’rampks’,T=538.,F=0.12 /

&RAMP ID=’rampcp’,T= 93.,F=1.172 /

&RAMP ID=’rampcp’,T=205.,F=1.255 /

23
&RAMP ID=’rampcp’,T=316.,F=1.339 /

&RAMP ID=’rampcp’,T=425.,F=1.423 /

Notice that with temperature-dependent quantities, the RAMP parameter T now means Temperature, and F

is the actual value of either C P or KS. Neither C P nor KS is given on the SURF line, but rather the RAMP

names. One should prescribe either a constant value for C P or KS or a RAMP name, but not both.

4.4.2 Combustion Parameters: The REAC Namelist Group

There are two ways of designating a fire: the first is to prescribe a Heat Release Rate Per Unit Area HRRPUA

on a SURF line. The other is to prescribe a HEAT OF VAPORIZATION, in which case the burning rate

of the fuel depends on the net heat feedback to the surface. In both cases, the mixture fraction combustion model is used. The REAC line is used for various parameters associated with the gas phase reaction

of fuel and oxygen. Note that if only the fire’s heat release rate is specified with HRRPUA, then these

parameters usually do not require adjusting. However, if the burning behavior of a fuel is governed by

its HEAT OF VAPORIZATION, care must be taken in selecting the appropriate reaction parameters. See

Section 4.4.3 for additional details.

It is assumed that a single hydrocarbon fuel is being burned, with constant yields of CO and soot

CxHyOz +νO2 O2 → νCO2 CO2 +νH2O H2O+νCO CO+νSoot Soot (4.1)

Specify the ideal stoichiometric coefficients for the fuel, O2, CO2 and H2O, and yields for CO and soot.

The yield of CO, for example, is defined as the fraction of the fuel mass that is converted into CO, and is

denoted yCO. Do not directly specify the stoichiometric coefficients for CO or soot because these numbers

are usually reported in terms of mass yields. It is assumed that the CO and soot are created at the flame

and transported with the combustion products. No growth, oxidation or after burning is assumed. Research

continues to refine the handling of these products of incomplete combustion. For the moment, the ideal

stoichiometric coefficients for O2, CO2 and H2O are adjusted to account for the production of CO and soot

at the start of a calculation. The actual stoichioimetric coefficients used in the calculations are

νO2 =



x−

Mf

2MCO

yCO −

Mf

MC

ys



+

y

4

−

z

2

νCO2 = x−

Mf

MCO

yCO −

Mf

MC

ys

νH2O =

y

2

νCO =

Mf

MCO

yCO

νsoot =

Mf

MC

ys

The following parameters may be prescribed on the REAC line. Note that only one REAC line may be

used. Most often, one selects a reaction from the DATABASE via the REACTION parameter on the MISC

line.

ID A character string naming the reaction. It is optional if the REAC line is included within the data input

file, mandatory if the REAC line is included in the DATABASE file.

NU O2, NU H2O, NU FUEL, NU CO2 Ideal stoichiometric coefficients for the reaction of a hydrocarbon fuel. NU FUEL is 1 by default. All numbers are positive. Default values are those of propane.

24
MW FUEL Molecular weight of the fuel (g/mol). Default is for propane, 44 g/mol. If the fuel has nitrogen in

it, add the parameter FUEL N2 to indicate how many molecules of N2 there are. For example urethane

is C3H7NO2. For it, FUEL N2=0.5 because there is half of a N2 molecule.

SOOT YIELD The fraction of fuel mass converted into smoke particulate, ys. Note that this parameter does

not apply to the processes of soot growth and oxidation, but rather to the net production of the smoke

particulate from the fire. (Default 0.01)

CO YIELD The fraction of fuel mass converted into carbon monoxide, yCO. Normally, this parameter need

not be set, because by default yCO is linked to the SOOT YIELD, ys, via the correlation developed by

Koyl  ̈ u and Faeth  ̈

yCO =

12x

Mf νf

0.0014+0.37 ys

where x is the number of carbon atoms in a fuel molecule, Mfis the molecular weight of the fuel, and

νfis the stoichiometric coefficient of the fuel, assumed to be 1 here [5]. Note that this correlation

refers to well-ventilated fires. Yields of CO and soot in underventilated fires is still a subject of active

research.

EPUMO2 Energy Per Unit Mass Oxygen, ∆HO2(kJ/kg). The amount of energy released per unit mass of

oxygen consumed. (Default 13,100 kJ/kg). Note that the heat of combustion

∆H ≈

νO2 MO2

νf Mf

∆HO2

is modified slightly due to the presence of soot and CO.

RADIATIVE FRACTION The fraction of energy released from the flame as thermal radiation. This parameter requires some interpretation. See Section 4.4.3 for details. (Default 0.35)

A few sample REAC lines are given here. More can be found in the DATABASE file.

&REAC ID=’METHANE’

MW_FUEL=16

NU_O2=2.

NU_CO2=1.

NU_H2O=2.

RADIATIVE_FRACTION=0.15

SOOT_YIELD=0.01 /

&REAC ID=’WOOD’

SOOT_YIELD = 0.01

NU_O2 = 3.7

NU_CO2 = 3.4

NU_H2O = 3.1

MW_FUEL = 87.

EPUMO2 = 8850. /

4.4.3 Important Issues Related to Combustion

This section explains the various approximations that affect both the gas phase parameters (REAC line) and

the solid (or liquid) phase parameters (SURF line). These approximations are needed either to compensate

for less than desirable grid resolution or limitations of the mixture fraction combustion model.

25
Heat Release Rate: For coarsely gridded calculations, it is not possible to resolve the fire adequately, and as

a result the heat release rate and flame height can be underestimated [6]. There are several ways to remedy

the problem, one of which is to choose a different value of the mixture fraction when defining the flame

sheet. The program has built into it a routine that redefines the stoichiometric value of the mixture fraction

Zf,e f f

Zf

= min 1 , C

D

∗

δx



(4.2)

where Zfis the ideal stoichiometric value of the mixture fraction, C is an empirical constant (not an input

parameter), and D

∗

is the characteristic fire diameter

D

∗ =



Q ̇

ρ∞ cp T∞

√g

2

5

(4.3)

“Good” or “bad” resolution depends on both the size of the fire and the size of the grid cells. For relatively

small values of D

∗

and/or large grid cells, the stoichiometric value of the mixture fraction is intentionally

reduced, resulting in a better estimate of flame height and structure. In cases where D

∗

is relatively large and

the cells relatively small, no adjustment need be made to the stoichiometric value of the mixture fraction. As

always, a sufficiently resolved grid eliminates the need for these types of corrections, but in many instances

it is difficult to both finely grid the region near the fire while at the same time saving enough cells for the

rest of the space.

By default, the re-adjustment of the stoichiometric value of the mixture fraction is applied automatically.

To turn it off, specify AUTOMATIC Z=.FALSE. on the MISC line, in which case the ideal stoichiometric

value of the mixture fraction is used to mark the flame zone. Also, minor adjustments can be made to

the flame height by setting Z CONSTANT to a value different than 1 on the REAC line. This parameter is

essentially a normalized version of 1/C from Eq. (4.2). Reducing Z CONSTANT shortens the flame length;

increasing it lengthens the flame.

Radiative Fraction: The fraction of energy released from the fire as thermal radiation is a function of

both the flame temperature and chemical composition, neither of which are well known in a large scale

fire calculation. In calculations in which the grid cells are on the order of a centimeter and larger, the

temperature near the flame surface cannot be relied upon when computing the source term in the radiation

transport equation, especially because of the T

4 dependence. To compensate, if one prescribes a non-zero

value of RADIATIVE FRACTION, a grid cell cut by the flame radiates that fraction of the chemical energy

being released into it. Some of that energy may be reabsorbed elsewhere, yielding a net radiative loss that

is less than RADIATIVE FRACTION, depending mainly on the size of the fire and the soot loading. If it is

desired to use the radiation transport equation as is, then RADIATIVE FRACTION ought to be set to zero,

and the source term in the radiative transport equation is then based solely on the gas temperature and the

chemical composition.

Heat of Combustion: The user does not usually prescribe the heat of combustion explicitly. Normally, the

stoichiometric parameters listed on the REAC line are used to compute the heat of combustion. However, if

a HEAT OF VAPORIZATION has been specified on a SURF line and the heat of combustion of the material

differs from that specified by the governing REACTION, then add a HEAT OF COMBUSTION (kJ/kg) to the

SURF line. In a mixture fraction based combustion model, it is assumed that there is only one fuel. However,

in a realistic fire scenario, there may be many fuels originating from the various burning objects in the

building. Specify the stoichiometry of the predominant reaction via the REAC namelist group. Often these

parameters are stored in the DATABASE file, in which case simply prescribe a REACTION on the MISC line.

26
If the stoichiometry of the burning material differs from the global reaction, the HEAT OF COMBUSTION

is used to ensure that an equivalent amount of fuel is injected into the flow domain from the burning object.

Predicting the Burning Rate: Either prescribe the burning rate of the fuel via the parameter HRRPUA on the

SURF line, or let the burning rate be predicted based on the fuel’s thermal properties and its HEAT OF VAPORIZATION.

This latter action introduces a fair amount of uncertainty into the calculation because the burning rate is a

function of the energy fed back from the fire via convection and radiation, and the energy conducted through

the solid or liquid fuel. The various phenomena are still subjects of active research, so be aware of the potential errors introduced into the calculation. One of the greatest sources of error is the radiative heat flux from

the fire to the fuel surface. The error is due to a combination of insufficient grid resolution in the boundary

layer, and uncertainty in the absorption coefficient and flame temperature. As a result, the heat flux to the

fuel surface is often over-predicted. Until improvement can be made in the radiation calculation, prevent

excess pyrolysis of fuel by prescribing a BURNING RATE MAX (kg/m2/s) on the SURF line that limits the

burning rate of the fuel to its measured maximum.

Gas Phase Fire Suppression: Modeling suppression of a fire due to the introduction of a suppression agent

like CO2 or water mist, or due to the exhaustion of oxygen within a compartment is challenging because the

relevant physical mechanisms occur at length scales smaller than a single grid cell. Flames are extinguished

due to lowered temperatures and dilution of the oxygen supply. With the mixture fraction model, only the

dilution effect is accounted for because it is assumed that fuel and oxygen burn regardless of the temperature.

However, a simple suppression algorithm has been implemented in FDS that attempts to guage whether or

not a flame is viable near the stoichiometric mixture fraction surface. The Technical Reference Guide [1]

contains more details about how the mechanism works. The only parameters the user can control are the

Limiting Oxygen Index X O2 LL, and the CRITICAL FLAME TEMPERATURE. Both are set on the REAC

line. The default values are 0.15 and 1427 ◦C, respectively. To turn off the suppression algorithm, set

SUPPRESSION=.FALSE. on the MISC line.

4.4.4 Creating Obstructions: The OBST Namelist Group

OBST is the namelist group listing information about obstructions. Each OBST line contains the coordinates

of a rectangular solid within the flow domain. This solid is defined by two points (x1,y1,z1) and (x2,y2,z2)

that are entered on the OBST line in terms of the sextuplet XB=X1,X2,Y1,Y2,Z1,Z2. In addition to

the coordinates, the boundary conditions for the obstruction can be specified with the parameter SURF ID,

which designates which SURF group to apply at the surface of the obstruction. If the obstruction has different boundary conditions for its top, sides and bottom, do not prescribe only one boundary condition with

SURF ID. Instead, use SURF IDS, an array of three character strings specifying the boundary condition IDs

for the top, sides and bottom of the obstruction, respectively. If the default boundary condition is desired,

then SURF ID(S) need not be set. However, if at least one of the surface conditions for an obstruction is

the inert default, it can be referred to as ’INERT’. For example:

&SURF ID=’FIRE’,HRRPUA=1000.0 /

&OBST XB=2.3,4.5,1.3,4.8,0.0,9.2,SURF_IDS=’FIRE’,’INERT’,’INERT’ /

puts a fire on top of the obstruction. This is a simple way of prescribing a burner.

Some additional features of obstructions are as follows:

• In addition to SURF ID and SURF IDS, one can also use the sextuplet SURF ID6 as follows:

&OBST XB=2.3,4.5,1.3,4.8,0.0,9.2,

SURF_ID6=’FIRE’,’INERT’,’HOT’,’COLD’,’BLOW’,’INERT’ /

27
where the six surface descriptors refer to the planes x = 2.3, x = 4.5, y = 1.3, y = 4.8, z = 0.0, and

z = 9.2, respectively. Note that SURF ID6 should not be used on the same OBST line as SURF ID

or SURF IDS.

• Obstructions can have zero thickness. Often, thin sheets, like a window, form a barrier, but if the

numerical grid is coarse relative to the thickness of the barrier, the obstruction might be unnecessarily

bulky if it is assumed to be one layer of grid cells thick. To remedy this, the logic of FDS has been

changed so that all faces of an obstruction are shifted to the closest grid cell. If the obstruction is

very thin, the two faces may be approximated on the same cell face. FDS and Smokeview render this

obstruction as a thin sheet, but it is allowed to have thermally thin or thick boundary conditions. This

feature is still fragile, especially in terms of burning and blowing gas. A thin sheet obstruction can

only have one velocity vector on its face, thus a gas cannot be injected reliably from a thin obstruction

because whatever is pushed from one side is necessarily pulled from the other. For full functionality,

the obstruction should be specified to be at least one grid cell thick. Thin sheet obstructions work fine

as flow barriers, but other features are fragile and should be used with caution. Also note that unlike

earlier versions of FDS, now obstructions that are too small relative to the underlying numerical grid

are rejected. Be careful when testing cases on coarse grids.

• Obstructions may be created or removed during a simulation. See Section 5.4 for details.

• Obstructions can be protected from the HOLE punching feature. Sometimes it is convenient to create

a door or window using a HOLE. For example, suppose a HOLE is punched in a wall to represent

a door or window. An obstruction can be defined to fill this hole (presumably to be removed or

colored differently or whatever) so long as the phrase PERMIT HOLE=.FALSE. is included on the

OBST line. In general, any OBSTruction can be made impenetrable to a HOLE using this phrase. By

default, PERMIT HOLE=.TRUE., meaning that an OBSTruction is assumed to be penetrable unless

otherwise directed.

4.4.5 Creating Voids: The HOLE Namelist Group

It is often convenient to carve a hole out of an existing obstruction or set of obstructions. To do this, add

lines of the form

&HOLE XB=2.0,4.5,1.9,4.8,0.0,9.2 /

Any solid grid cells within the volume 2.0 < x < 4.5, 1.9 < y < 4.8, 0.0 < z < 9.2 are removed. Obstructions

intersecting the volume are broken up into smaller blocks. If the hole represents a door or window, a good

rule of thumb is to punch more than enough to create the hole. For example, if the OBST line denotes a wall

0.1 m thick:

&OBST XB=1.0,1.1,0.0,5.0,0.0,3.0 /

and one wants to create a door, add this:

&HOLE XB=0.99,1.11,2.0,3.0,0.0,2.0 /

The extra centimeter added to the x coordinates of the hole make it clear that the hole is to punch through

the entire obstruction. Students of American politics appreciate that it is not wise to leave hanging chads.

When a HOLE is created, the affected obstruction(s) are either rejected, or created or removed at predetermined times. For example, adding the parameter T CREATE to the HOLE line creates the hole after the

given number of seconds. Likewise, T REMOVE re-fills the hole after the given number of seconds. Notice

28
that T CREATE on a HOLE line has the opposite effect as T CREATE on an OBST line. The same applies

for T REMOVE.

If the hole is to be created or removed in response to a HEAT detector, use the parameters HEAT CREATE

or HEAT REMOVE. Each is a character string naming the appropriate HEAT detector. For example:

&HOLE XB=2.0,4.5,1.9,4.8,0.0,9.2,HEAT_CREATE=’heat2’ /

&HEAT XYZ=3.2,4.4,6.8,ACTIVATION_TEMPERATURE=74.,RTI=100.,LABEL=’heat2’ /

creates a hole when heat2 activates. Note that the old convention of using a negative value for T CREATE

or T REMOVE does not work here. Also, if the HOLE line contains HEAT CREATE=’ALL’, then any HEAT

detector creates the hole.

If it is desired that the obstruction(s) to be cut out should have a different color than the original obstruction, set the real triplet RGB on the HOLE line. If an obstruction is not to be punctured by a HOLE, add

PERMIT HOLE=.FALSE. to the OBST line.

It is a good idea to inspect the geometry by running either a setup job (TWFIN=0 on the TIME line) or

a short-time job to test the operation of T CREATE and/or T REMOVE.

Note that a HOLE cannot be used on a VENT or a mesh boundary.

4.4.6 Designating Vents and Surfaces: The VENT Namelist Group

Whereas the OBST group is used to prescribe obstructions within the computational domain, the VENT

group is used to prescribe planes adjacent to obstructions or external walls. The vents are chosen in a similar

manner to the obstructions, with the sextuplet XB denoting a plane abutting a solid surface. Two of the six

coordinates must be the same, denoting a plane as opposed to a solid. An easy way to specify an entire

external wall is to replace XB with CB, a character string whose value is one of the following: ’XBAR’,

’XBAR0’, ’YBAR’, ’YBAR0’, ’ZBAR’ or ’ZBAR0’ denoting the planes x = XBAR, x = XBAR0, y =

YBAR, y = YBAR0, z = ZBAR or z = ZBAR0, respectively. Like an obstruction, the boundary condition

index of a vent is specified with SURF ID, indicating which of the listed SURF lines to apply. If the default

boundary condition is desired, then SURF ID need not be set.

Be careful when using the CB shortcut when doing a multiple mesh simulation, that is, when more

than one rectangular mesh is used. The plane designated by the keyword CB is applied to all of the grids,

possibly leading to confusion about whether a plane is a solid wall or an open boundary. Check the geometry

in Smokeview to assure that the VENTs are properly prescribed. Use color as much as possible to doublecheck the set-up. More detail on color in Section 4.4.7.

The term “VENT” is somewhat misleading. Taken literally, a VENT can be used to model components

of the ventilation system in a building, like a diffuser or a return. In these cases, the VENT coordinates form

a plane on a solid surface forming the boundary of the duct. No holes need to be created through the solid; it

is assumed that air is pushed out of or sucked into duct work within the wall. Less literally, a VENT is used

simply as a means of applying a particular boundary condition to a rectangular patch on a solid surface.

A fire, for example, is usually created by first generating a solid obstruction via an OBST line, and then

specifying a VENT somewhere on one of the faces of the solid with a SURF ID pointing to a SURF line with

the characteristics of the thermal and combustion properties of the fuel.

There are two reserved SURF ID’s that may be applied to a VENT. The first is SURF ID=’OPEN’. This

is used only if the VENT is applied to the exterior boundary of the computational domain, where it denotes

a passive opening to the outside. It is assumed here that the exterior boundary of the computational domain

is a solid wall, and the OPEN vent is essentially an open door or window. The second reserved SURF ID is

for a symmetry plane, in which case the VENT has the attribute SURF ID=’MIRROR’. Usually, a MIRROR

spans an entire face of the computational domain, essentially doubling the size of the domain with the

MIRROR acting as a plane of symmetry. The flow on the opposite side of the MIRROR is exactly reversed.

29
From a numerical point of view, a MIRROR is a no-flux, free-slip boundary. As with OPEN, a MIRROR can

only be prescribed at an exterior boundary of the computational domain. Often, OPEN or MIRROR VENTs

are prescribed along an entire side of the computational domain, in which case the “CB” notation is handy.

Vents to the outside of the computational domain (OPEN vents) may be opened or closed during a

simulation. See Section 5.4 for details.

There is one exception to the rule that VENTs ought to be prescribed flush against a solid obstruction or

external boundary. A VENT that is prescribed in the interior of the domain without any solid surface flush

up against it can act as a fan. For example, the lines

&PDIM XBAR=1.0,YBAR=1.0,ZBAR=1.0 /

.

.

&SURF ID=’BLOW’,VEL=2.1,TAU_V=5.0 /

&VENT XB=0.50,0.50,0.25,0.75,0.25,0.75,SURF_ID=’BLOW’ /

create a plane within the unit cube domain that blows air at 2.1 m/s in the positive x direction, ramping up

in about 5 s. In general, the value of VEL associated with a VENT that is not aligned with a solid surface

blows gases in the coordinate direction normal to the VENT – positive if VEL is positive, negative if VEL

is negative. Note that only velocity boundary conditions are appropriate on a SURF line associated with a

free-standing VENT because there is no solid obstruction on which to impose thermal or material boundary

conditions.

One final note for VENT: if an error message appears requesting that the orientation of a vent be specified, first check to make sure that the vent is a plane. If the vent is a plane, then the orientation can be

forced by specifying the parameter IOR. If the normal direction of the VENT is in the positive x direction,

set IOR=1. If the normal direction is in the negative x direction, set IOR=-1. For the y and z direction, use

the number 2 and 3, respectively. Setting IOR may sometimes solve the problem, but it is more likely that

if there is an error message about orientation, then the VENT is buried within a solid obstruction, in which

case the program cannot determine the direction in which the VENT is facing.

4.4.7 Coloring Obstructions, Vents and Surfaces

Surface and obstruction colors are prescribed in a number of ways. If one desires that all surfaces associated

with a given SURF line be colored the same way, prescribe a triplet of real numbers called RGB on the SURF

line. The three numbers may be between 0 and 1, indicating the amount of Red, Green and Blue that make

up the color. Table 4.1 lists the RGB indices for a variety of colors. It is highly recommended that colors be

assigned to surfaces via the SURF line because as the geometries of FDS simulations become more complex,

it is very useful to use color as a spot check to determine if the desired surface properties have been assigned

throughout the room or building under study. For example,

&SURF ID=’UPHOLSTERY’,...,RGB=0.0,1.0,0.0 /

causes the furnishings to be colored green in Smokeview. Fractions of “R”, “G” and “B” can be used to

create more life-like colors. It is best to avoid using the primary colors because these same colors are used

by Smokeview to draw color contours.

Obstructions and vents may be colored individually (over-riding the SURF line’s RGB) by specifying COLOR = ’RED’, ’BLUE’, ’BLACK’, ’YELLOW’, ’GREEN’, ’MAGENTA’, ’WHITE’,

’CYAN’ or ’INVISIBLE’ on the respective OBST or VENT line. Using ’INVISIBLE’ causes the

vent or obstruction to not be drawn. Colors may also be specified using the triplet RGB on an OBST or

VENT line to gain a wider color pallette. The use of RGB is preferable, especially to create colors that do not

clash with the pastel colors used to show temperatures, concentrations, etc.

30
Table 4.1: RGB values for various colors.

Color Red Green Blue

Red 1.0 0.0 0.0

Green 0.0 1.0 0.0

Blue 0.0 0.0 1.0

White 1.0 1.0 1.0

Black 0.0 0.0 0.0

Gray 0.5 0.5 0.5

Magenta 1.0 0.0 1.0

Yellow 1.0 1.0 0.0

Cyan 0.0 1.0 1.0

Tan 0.8 0.6 0.4

Orange 1.0 0.5 0.0

31
4.5 Lagrangian Particles: The PART Namelist Group

Lagrangian particles are used in FDS as water or liquid fuel droplets, flow tracers, and various other things.

Sometimes the particles have mass, sometimes they do not. Some evaporate, absorb radiation, etc. PART is

the namelist group that is used to prescribe parameters associated with Lagrangian particles.

Properties of different types of Lagrangian particles are designated via one or more PART lines. Much

like SURF lines contain the properties of a solid surface or vent, PART lines contain information about

particles and droplets. Once a particular type of particle or droplet has been described using a PART line,

then the name of that particle or droplet is invoked elsewhere in the input file. For example, an input file

may have several PART lines that include the properties of different types of Lagrangian particles:

&PART ID=’smoke’,... /

&PART ID=’water’,... /

These Lagrangian particles can be introduced at a solid surface via the SURF line that defines the properties

of the material, for example

&SURF ...,PART_ID=’smoke’ /

or the PART type can be invoked from a SPRK line to change the properties of the droplets ejected by a

sprinkler, for example

&SPRK PART_ID=’water’,... /

The frequency at which Lagrangian particles are added to the simulation is controlled by the parameters

DTPAR and DTSPAR which are prescribed on the MISC line. Regardless of type, particles at solid surfaces

are inserted every DTPAR seconds and droplets from sprinklers every DTSPAR seconds. It is not possible to

have different particle types inserted more often than others.

The simplest use of Lagrangian particles is for visualization, in which case the particles are considered

massless tracers. In this case, the particles are defined via the line

&PART ID=’tracers’,MASSLESS=.TRUE.,... /

Other options for massless particles are

SAMPLING FACTOR Sampling factor for the particle output file CHID.part. This parameter can be used

to reduce the size of the particle output file used to animate the simulation. (Default 1)

QUANTITY A character string indicating which scalar quantity should be used to color the particles when

viewed as an animation. The choices are ’TEMPERATURE’ (

◦C), ’DIAMETER’ (μm), or ’VELOCITY’

(m/s). If the particles are to be one color, specify QUANTITY=’RED’, ’BLUE’, ’BLACK’,

’YELLOW’, ’GREEN’, ’MAGENTA’, ’WHITE’ or ’CYAN’. Note that if the particles are

MASSLESS, it is not appropriate to color them according to their ’DIAMETER’ or ’TEMPERATURE’.

Unlike early versions of FDS, particles are no longer colored by gas phase quantities, but rather by

properties of the particle itself. For example, ’TEMPERATURE’ refers to the temperature of the

particle itself (assuming it has mass) rather than the local gas temperature.

AGE Number of seconds the particle or droplet exists. Useful parameter to use when trying to reduce the

number of droplets or particles in a simulation.

For Lagrangian particles that are not MASSLESS, the following additional parameters can be included

on the PART line. Note that many of these parameters are used only for certain types of particles or droplets

and need to be specified only if they are relevant.

32
DENSITY The density of the liquid or solid droplet/particle. (Default 1000 kg/m3

)

VAPORIZATION TEMPERATURE Boiling temperature of liquid droplet. (Default 100 ◦C)

MELTING TEMPERATURE Melting (solidification) temperature of liquid droplet. (Default 0 ◦C)

SPECIFIC HEAT Specific heat of liquid or solid droplet/particle. (Default 4.184 kJ/kg/K)

HEAT OF VAPORIZATION Latent heat of vaporization of liquid droplet. (Default 2259 kJ/kg)

DIAMETER Median volumetric diameter of droplets/particles, with the distribution assumed to be a combination of Rosin-Rammler and log-normal (Default 100 μm). The width of the distribution is controlled

by the parameter GAMMA D, default 2.4. See discussion of sprinkler data files in Section 4.6.1 for details. (Default 100 μm)

STATIC Logical parameter indicating whether particles move or just serve as obstructions or clutter. This

parameter should only be used when NUMBER INITIAL DROPLETS is greater than 0. (Default

.FALSE.)

FUEL Logical parameter indicating whether the liquid droplets evaporate into fuel gas and burn. (Default

.FALSE.). If FUEL=.TRUE., then also add HEAT OF COMBUSTION (kJ/kg) of the fuel.

WATER Logical parameter indicating whether the liquid droplets evaporate into WATER VAPOR, which is

a separate species that is automatically added to the calculation. (Default .FALSE.)

NUMBER INITIAL DROPLETS Seed the domain with particles/droplets at the start of the simulation. (Default 0). If non-zero, also specify MASS PER VOLUME (kg/m3

) which specifies the particle/droplet

mass per unit volume (Default 1 kg/m3). Do not confuse this parameter with DENSITY. For example,

water has a DENSITY of 1000 kg/m3, whereas a liter of water broken up into droplets and spread over

a cubic meter has a MASS PER VOLUME of 1 kg/m3.

DROPLETS PER SECOND Number of sprinkler droplets inserted every second per active sprinkler. Note

that this parameter only affects sprinkler droplets. Changing this parameter does not change the flow

rate, but rather the number of droplets used to represent the flow. (Default 1000)

33
4.6 Sprinklers and Detectors

Research to better characterize a sprinkler’s spray distribution and droplet size has led to a need for a file

format to record everything about a particular sprinkler in one file. Much of this is transparent to the user

who simply specifies the physical coordinates of the sprinkler in the data file job name.data. The data

for the particular sprinkler is kept in a file called sprinkler name.spk. Heat detector parameters are given

within the input file itself. All one needs to do is specify the physical coordinates and an RTI within the data

file job name.data.

4.6.1 Specifying Sprinklers: The SPRK Namelist Group

Information about a given sprinkler is contained in a separate file, called, for example, sprinkler name.spk3

.

A sample file is shown in Fig. 4.2. All the sprinkler characteristics are stored in this file. The user only has

to provide lines of the form

&SPRK XYZ=3.0,5.6,2.3,MAKE=’sprinkler_make’,LABEL=’doorway’ /

in the input data file job name.data. The physical coordinates of the sprinkler are given by a triplet of real

numbers XYZ. The make of the sprinkler is given by a character string MAKE, for which there exists a file

called sprinkler make.spk containing thermal properties and other information about the sprinkler. The

character string LABEL is merely a descriptor to identify the sprinkler in various output files.

There is an option to manually activate the sprinkler by setting T ACTIVATE in seconds on the SPRK

line itself. The sprinkler can be shut off by setting T DEACTIVATE. Also, the (normally) downwarddirected sprinkler spray can be redirected in some other direction. The triplet ORIENTATION can be added

to a given SPRK line to change the direction of the spray. The default value of ORIENTATION is (0,0,-1),

but if one were to prescribe

&SPRK XYZ=3.0,5.6,2.3,MAKE=’sprinkler_make’,ORIENTATION=1,0,0 /

the sprinkler would point in the positive x direction. If the designated sprinkler has a spray which is not

axially-symmetric, another parameter called ROTATION can be used to rotate the spray through a given

number of degrees. The default value is 0, but experiment with a single sprinkler flow calculation to ensure

that the sprinkler is being re-oriented as desired.

In addition to the sprinkler parameters listed on the SPRK line, one may also want to adjust some

parameters that control the number and frequency of droplet insertions. These parameters are typically

entered under the namelist group PART. See Section 4.5 for details.

If the sprinkler system is of the dry-pipe variety, prescribe a time delay for the system by adding a

DELAY (s) to the PIPE namelist line. The PIPE namelist group contains information about the sprinkler

system as a whole. For the moment, it contains only two parameters, DELAY and PRESSURE. Note that

only one PIPE line is read by FDS. If DELAY is set to be non-zero, then that amount of time has to elapse

before water is allowed to flow from any activated sprinkler.

Be aware that sprinklers produce many droplets that need to be tracked in the calculation. To limit the

burden, sprinkler droplets are given an AGE of 60 s, and also sprinkler droplets disappear when they hit the

lower boundary of the computational domain, regardless of whether it is solid or not. To allow droplets to

live longer than AGE, add PART ID=’whatever’ to the SPRK line, where ’whatever’ is the ID of a

PART line which can be used to modify the properties of the water droplets. For example,

&SPRK XYZ=3.0,5.6,2.3,MAKE=’sprinkler_make’,PART_ID=’my water droplets’ /

&PART ID=’my water droplets’,WATER=.TRUE.,AGE=300.,QUANTITY=’DIAMETER’ /

3The MISC character string DATABASE DIRECTORY can be used to point to a directory where sprinkler files are stored.

34
allows control over some of the properties of the water droplets from a sprinkler. The phrase WATER=.TRUE.

is important to direct the program to evaporate the droplets into WATER VAPOR without requiring one to explicitly add WATER VAPOR to the calculation. The phrase QUANTITY=’DIAMETER’ directs Smokeview

to color the water droplets according to their diameter.

To stop FDS from removing sprinkler droplets from the lower boundary of the computational domain,

add the phrase POROUS FLOOR=.FALSE. to the MISC line. Be aware, however, that droplets that land

on the floor continue to move horizontally in randomly selected directions; bouncing off obstructions, and

consuming CPU time.

Sprinkler properties listed in the file sprinkler name.spk are

RTI Response Time Index of the sprinkler in units of √m·s. (Default 165.)

C-FACTOR C-Factor of sprinkler in units of √m/s. (Default 0.)

K-FACTOR K-Factor of sprinkler in units of L/min/bar 1

2 . (Default 166) The flow rate is given by  ̇mw = K

√p

where  ̇mw is the flow rate in L/min, K the K-factor in L/min/(bar) 1

2 and p the gauge pressure in bar4

ACTIVATION TEMPERATURE Link activation temperature (◦C). (Default 74 ◦C)

OPERATING PRESSURE Sprinkler operating pressure in units of bar. This is the pressure at which the

sprinkler was tested. If one desires to flow the sprinkler at a different pressure than that at which it

was tested, a single line

&PIPE PRESSURE=1.5 /

should be added to the input data file, and then all sprinklers operate at this new pressure, 1.5 bar

for example. The reason for the two pressures is that a slight adjustment is made to the droplet size

distribution to account for the fact that the sprinkler operates at a different pressure than that at which

it was tested. In the absence of any user-specified PRESSURE, the OPERATING PRESSURE listed

in the .spk file is used.

OFFSET DISTANCE Radius of a sphere (m) surrounding the sprinkler where the water droplets are initially

placed in the simulation. It is assumed that at and beyond the OFFSET DISTANCE the droplets have

completely broken up and are transported independently of each other. (Default 0.10 m)

VELOCITY Description of the initial droplet velocity distribution. There are two options of inputs here,

designated by either a 1 or a 2 on the line immediately following the keyword VELOCITY. For case

1, the parameters: Minimum Spray Angle, Maximum Spray Angle, and Speed should be given values. The angles outline a conical spray pattern relative to the south pole of the sphere centered at

the sprinkler with radius OFFSET DISTANCE. For example, a Minimum Spray Angle of 20◦and

a Maximum Spray Angle of 80◦ directs the water droplets to leave the sprinkler through a conical

region 20◦ north of the south pole and 10◦south of the equator. The droplets are uniformly distributed

within this belt. If more detailed information about the sprinkler spray is known, then the keyword

VELOCITY is followed by a 2, indicating that the normal component of velocity of the droplets is

given as a function of na azimuthal (latitudinal) points starting at the bottom of the sphere, and nl

longitudinal points starting at one of the frame arms. The integers na and nl should be listed on the

line following the “2”, as in the example (Fig. 4.2). The case 2 VELOCITY data is applicable on a

sphere centered about the sprinkler whose radius is the OFFSET DISTANCE. This is typically the

distance from the sprinkler itself where all the spray characteristic measurements have been made.

41 bar is equivalent to 14.5 psi, 1 gpm is equivalent to 3.785 L/min, 1 gpm/psi

1

2 is equivalent to 14.41 L/min/bar

1

2 .

35
FLUX Relative water mass flux (kg/m2

/s), entered in the same way as the case 2 for VELOCITY. If case 1

for VELOCITY is used, there is no need to even specify a FLUX.

SIZE DISTRIBUTION Information about the droplet size distribution. The median volumetric droplet

diameter can either be a global value, or it can be prescribed as a function of the solid angle. If the

median diameter is independent of position, the key word SIZE DISTRIBUTION is to be followed

by the number 1 on the next line to indicate that the information given is a global average. The next

line after that has the median volumetric diameter (800 μm in the sample case), plus the parameter γ

from the Rosin-Rammler/log-normal distribution

F(d) =







√

1

2π

Z d

0

1

σd

0 e

−

[ln(d

0/dm)]2

2σ2 dd0

(d ≤ dm)

1−e

−0.693(

d

dm

)

γ

(dm < d)

(4.4)

Note that the parameter σ is given the value σ = 2/(

√

2π(ln 2) γ) = 1.15/γ which ensures that the

two functions are smoothly joined at d = dm. The larger the value of γ, the narrower the droplet size

is distributed about the median value. Its default value is 2.4.

If one has information about the median droplet size as a function of the sprinkler solid angle, that

information can be entered as in the following example:

SIZE_DISTRIBUTION

2

4 1 2.4

700

600

500

400

Here, the number 2 is the code number directing FDS to read the next few lines in a certain way. The

4 indicates that there are 4 values of the median diameter from the south pole to the north pole of the

sphere surrounding the sprinkler. For each latitudinal zone, there is only one value, meaning that this

value is independent of longitude. The value of 700 μm is for the south pole to 45◦ S, 600 μm is for

45◦ S to the equator, 500 μm is for the equator to 45◦ N, and 400 μm is for 45◦ N to the north pole.

The number 2.4 following the number of latitudinal and longitudinal points is the value of γ. Note

that γ is not a function of position. Only the median diameter can be a function of position.

For more information about sprinklers, see the Technical Reference Guide [1].

4.6.2 Specifying Heat Detectors: The HEAT Namelist Group

HEAT is the namelist group used to specify heat detectors. A heat detector is designated in the data input

file with a line(s) of the form

&HEAT XYZ=3.0,5.6,2.3,RTI=132.,ACTIVATION_TEMPERATURE=74.,LABEL=’door’ /

Like a sprinkler, the physical coordinates of the heat detector are given by a triplet of real numbers XYZ.

Unlike a sprinkler, there is no external file with thermal properties for a heat detector. RTI is the Response

Time Index in units of √

m·s. ACTIVATION TEMPERATURE is the link activation temperature in degrees

C (Default 74 ◦C). LABEL is just a descriptor.

Note that a heat detector can be used to trigger an event to happen, like the opening of a VENT to the

outside or the removal of an OBSTstruction. See Section 5.4 for details.

36
MANUFACTURER

Acme

MODEL

Splash2000

OPERATING_PRESSURE

0.50

K-FACTOR

80.

RTI

110.

C-FACTOR

0.

ACTIVATION_TEMPERATURE

74.

OFFSET_DISTANCE

0.10

SIZE_DISTRIBUTION

1

800 2.4

VELOCITY

2

60,24

6.3,6.4,6.5, ... (24 longitudinal zones, like time zones in this case)

.

.

.

(60 azimuthal zones, south pole to north pole, 3 degrees per zone)

FLUX

2

60,24

11.9,13.0,13.5, ...

.

.

.

Figure 4.2: A sample sprinkler file. Note that the keywords should be written exactly as they are

written here, and they should start in the very left column of each line. Note that this sample file

includes a fairly detailed description of the spray pattern, requiring extensive measurements. In most

cases, the VELOCITY and FLUX can be described with just a few parameters.

37
4.7 Output Files

Before a calculation is started, carefully consider what information should be saved. All output quantities

must be specified at the start of the calculation. In most cases, there is no way to retrieve information after

the calculation ends if it was not specified from the start. There are several different ways of visualizing the

results of a calculation. Most familiar to experimentalists is to save a given quantity at a single point in space

so that this quantity can be plotted as a function of time, like a thermocouple temperature measurement. The

namelist group THCP is used to specify “thermocouple” or point measurements.

An animated isosurface (ISOF) is a three dimensional contour of a scalar quantity. For example, a

300 ◦C temperature isosurface shows where the gas temperature is 300 ◦C. By default, the stoichiometric

value of the mixture fraction is visualized via an isosurface. Choose several other quantities to visualize via

an isosurface.

In order to visualize the flow patterns better, one can save planar slices of data, either in the gas or solid

phases, by using the SLCF (SLiCe File) or BNDF (BouNDary File) namelist group. Both of these output

formats permit one to animate these quantities in time.

For static pictures of the flow field, use the PL3D (PLot3D file) namelist group. Plot3D format is used

by many CFD programs as a simple way to store specified quantities over the entire grid at one instant in

time.

Finally, tracer particles can be injected into the flow field from vents or obstacles, and then viewed in

Smokeview. Use the PART namelist group to control the injection rate, sampling rate and other parameters

associated with particles. Note: unlike in FDS version 1, particles are no longer used to introduce heat into

the flow, thus particles no longer are ejected automatically from burning surfaces.

The time increment between data dumps can be controlled. For THCP, SLCF, ISOF and PART files,

data is written out to files every TWFIN/NFRAMES seconds. For BNDF files, data is written out every

TWFIN/NFRAMES/2 seconds. The parameter NFRAMES may be specified on the MISC line. For the PL3D

format, data is written out every TWFIN/5 seconds. To change the sampling rate of any output file type, the

parameter DTSAM should be set on any one line of that particular group. For example, if one desires that

THCP data be written out every second, then the string DTSAM=1. should be written on one of the THCP

lines. This one entry dictates that all THCP data be written out every second. All of the other data files are

updated according to the default increment, or according to another prescription of DTSAM.

4.7.1 Point Measurements: The THCP Namelist Group

THCP is the name of a group of parameters that can be used to record values of various quantities at a

point as a function of time, much like a thermocouple or other point measurement. Each THCP line consists of the coordinates of the point at which the measurement is to be recorded, XYZ, and a quantity to

record, QUANTITY. The quantities are either gas phase (see Table 4.2) or solid phase (see Table 4.3).

Many of the gas phase quantities are self-explanatory. However, some require explanation. For example,

THERMOCOUPLE is the temperature of the thermocouple itself, usually close to the gas temperature, but not

always. It is determined by solving the following equation for TTC iteratively [7]

εTC(σT

4

TC −U/4) +h(TTC −Tg) = 0 (4.5)

where εTC is the emissivity of the thermocouple, U is the integrated radiative intensity, Tg is the true gas

temperature, and h is the heat transfer coefficient to a small sphere, h = kaNu/Pr/dTC. See the discussion on

heat transfer to a water droplet in the Technical Reference Guide for details of the convective heat transfer

to a small sphere.

When prescribing a solid phase quantity, be sure to position the probe at a solid surface. It is not always

obvious where the solid surface is since the grid does not always align with the input obstruction locations.

38
To help locate the appropriate surface, the parameter IOR must be included when designating a solid phase

quantity. If the orientation of the solid surface is in the positive x direction IOR=1, negative x direction

IOR=-1, positive y IOR=2, negative IOR=-2, positive z IOR=3, and negative z IOR=-3. There are

still instances where FDS cannot determine which solid surface is being designated, in which case an error

message appears in the diagnostic output file. Re-position the probe and try again. For example, the line

&THCP XYZ=0.7,0.9,2.1,QUANTITY=’WALL_TEMPERATURE’,IOR=-2,LABEL=’whatever’ /

designates the surface temperature of a wall facing the negative y direction.

In addition to point measurements, the THCP group can be used to report integrated quantities (See

Table 4.4). For example, one often wants to know the mass flow out of a door or window. To report this,

add the line

&THCP XB=0.3,0.5,2.1,2.5,3.0,3.0,QUANTITY=’MASS FLOW’,LABEL=’whatever’ /

Note that in this case, a plane is specified rather than a point. The sextuplet XB is used for this purpose.

Notice when a flow is desired, two of the six coordinates need to be the same. Another QUANTITY, HRR,

can be used to compute the total heat release rate within a subset of the domain. In this case, the sextuplet XB

ought to define a volume rather than a plane. Specification of the plane or volume over which the integration

is to take place can only be done using XB – avoid planes or volumes that cross multiple mesh boundaries.

FDS has to decide which mesh to use in the integration, and it chooses the finest mesh overlapping the

centroid of the designated plane or volume.

The thermocouples can be labeled with the character string LABEL for easier identification in the output

file. The output file is a comma-delimited ASCII file called CHID tc.csv which can be imported into most

spread sheet software packages.

4.7.2 Animated Planar Slices: The SLCF Namelist Group

The SLCF (“slice file”) namelist group allows one to record various gas phase quantities (Table 4.2) at more

than a single point. A “slice” refers to a subset of the whole domain. It can be a line, plane, or volume,

depending on the values of XB. The sextuplet XB indicates the boundaries of the region for which values of

QUANTITY are to be recorded every DTSAM s. XB is prescribed as in the OBST or VENT groups, with the

possibility that 0, 2, or 4 out of the 6 values be the same to indicate a volume, plane or line, respectively.

A handy trick is to specify, for example, PBY=5.3 instead of XB if it is desired that the entire plane

y = 5.3 slicing through the domain be saved. PBX and PBZ control planes perpendicular to the x and z axes,

respectively.

Slice file information is recorded in files labeled CHID n.sf, where n is the index of the slice file. A

Fortran 90 routine fds2ascii produces a test file from a line, plane or volume of data. See Section 4.7.6 for

more details.

Figure 4.3 shows several snapshots of a vertical animated slice from Smokeview where the slice is

colored according to gas temperature. Slice files are displayed by selecting the desired file from the

Load/Unload menu in Smokeview.

Animated vectors are displayed using data contained in two or more slice files. The direction and length

of the vectors are determined from the U, V and/or W velocity slice files. The vector colors are determined

from the file (such as temperature) selected from the Load/Unload menu. Figure 4.4 shows a sequence

of vector slices corresponding to the shaded temperature contours found in Figure 4.3.

4.7.3 Animated Boundary Quantities: The BNDF Namelist Group

The BNDF (“boundary file”) namelist group allows one to record surface quantities at all solid obstructions.

The possible output quantities are listed in Table 4.3. As with the SLCF group, each quantity is prescribed

39
Quantity Description Symbol Units

DENSITY density ρ kg/m3

TEMPERATURE gas temperature T

◦C

THERMOCOUPLE thermocouple temperature TTC

◦C

U-VELOCITY velocity component u m/s

V-VELOCITY velocity component v m/s

W-VELOCITY velocity component w m/s

VELOCITY flow speed √

u

2 +v2 +w2 m/s

PRESSURE perturbation pressure p ̃ Pa

H total pressure divided by density H = |u|

2/2+ p ̃/ρ (m/s)2

HRRPUV HRR Per Unit Volume q ̇

000 kW/m3

MIXTURE FRACTION mixture fraction Z kg/kg

DYNAMIC VISCOSITY dynamic viscosity μ kg/m/s

KINEMATIC VISCOSITY kinematic viscosity ν = μ/ρ m2/s

DIVERGENCE divergence ∇·u s

−1

WMPUV Water Mass PUV m

000

w kg/m3

WATER VAPOR water vapor mass frac. Yw kg/kg

oxygen O2 volume fraction XO2(Z) mol/mol

oxygen mass fraction O2 mass fraction YO2(Z) kg/kg

fuel fuel volume fraction XF(Z) mol/mol

nitrogen N2 volume fraction XN2(Z) mol/mol

water vapor H2O volume fraction XH2O(Z) mol/mol

carbon dioxide CO2 volume fraction XCO2(Z) mol/mol

carbon monoxide CO volume fraction XCO(Z) ppm

soot volume fraction soot volume fraction ρYs/ρs ppm

soot density smoke particulate concentration ρYs mg/m3

extinction coefficient light extinction coef. K = Km ρYs 1/m

visibility visibility distance S = C/K m

DROPLET FLUX X water mass flux in x direction m ̇

00

w

(SLCF only) kg/m2/s

DROPLET FLUX Y water mass flux in y direction m ̇

00

w

(SLCF only) kg/m2/s

DROPLET FLUX Z water mass flux in z direction m ̇

00

w

(SLCF only) kg/m2/s

Table 4.2: Gas Phase Output Quantities for THCP, SLCF or PL3D. Note that lower case quantities are appropriate only for calculations involving the mixture fraction. If individual species are

listed via SPEC namelist lines, the Quantity for mass and volume fractions are [SPECIES ID] and

[SPECIES ID] VF. The quantities water vapor and WATER VAPOR denote the volume fraction

of water vapor generated by combustion and the mass fraction of water vapor from evaporated sprinkler droplets, respectively. See Section 5.10 for a discussion of extinction coefficient and

visibility.

40
30 s 60 s 240 s

Figure 4.3: Slice file snapshots of shaded temperature contours in a vertical plane centered at the fire origin

at t=(30, 60, 240) s after ignition. The data file for these contours was generated by adding the line

&SLCF PBY=1.5,QUANTITY=’TEMPERATURE’ /

to an FDS input file.

30 s 60 s 240 s

Figure 4.4: Vector slice file snapshots of shaded vector plots in a vertical plane centered at the fire origin at

t=(30, 60, 240) s after ignition. The data files for these vector plots were generated by adding the line

&SLCF PBY=1.5,QUANTITY=’TEMPERATURE’,VECTOR=.TRUE. /

to an FDS input file.

41
Quantity Description Symbol Units

RADIATIVE FLUX net radiative flux q ̇

00

r kW/m2

CONVECTIVE FLUX convective flux into solid q ̇

00

c = h(Tg −Tw) kW/m2

HEAT FLUX net heat flux into solid q ̇

00

r +q ̇

00

c kW/m2

GAUGE HEAT FLUX equivalent flux to cold wall q ̇

00

r /ε+q ̇

00

c +h(Tw −T∞) +σ(T

4

w −T

4

∞) kW/m2

INCIDENT HEAT FLUX incident heat flux q ̇

00

r /ε+q ̇

00

c +σT

4

w kW/m2

WALL TEMPERATURE wall temperature Tw C

INSIDE WALL TEMPERATURE inner wall temperature Ts(x) C

BURNING RATE mass loss rate per unit area m ̇

00

f

kg/m2/s

PRESSURE COEFFICIENT pressure coefficient Cp = (p− p0)/(

1

2

ρ∞U

2

) N/A

WMPUA Water Mass Per Unit Area m ̇

00

w kg/m2

WCPUA Water Cooling Per Unit Area q ̇

00

w kW/m2

Table 4.3: Solid Phase Output Quantities for THCP and BNDF. Notes: (1) the difference between

HEAT FLUX and GAUGE HEAT FLUX. The former is the rate at which energy is absorbed by the solid

surface; the latter is the amount of energy that would be absorbed if the surface were cold. It is

more appropriate to use GAUGE HEAT FLUX when comparing predictions with experimental measurements. If the heat flux gauge used in an experiment has a temperature other than ambient, set

GAUGE TEMPERATURE on the MISC line. (2) If PRESSURE COEFFICIENT is prescribed, one also

needs to prescribe U via the parameter CHARACTERISTIC VELOCITY on the MISC line. (3) To get

an inner wall temperature, INSIDE WALL TEMPERATURE, the parameter DEPTH (in meters) must be

provided on the same THCP line. Note that INSIDE WALL TEMPERATURE is allowed only as a THCP,

not a BNDF, QUANTITY.

with a separate BNDF line, and the output files are of the form CHID n.bf. No physical coordinates need be

specified, however, just QUANTITY and DTSAM (if desired).

Note that BNDF files can become very large, so caution should be used in prescribing the time interval.

One way to reduce the size of the output file is to “turn off” the drawing of boundary information on desired

obstructions. On any given OBST line, if the string BNDF BLOCK=.FALSE. is included, the obstruction

is not colored. To turn off all boundary drawing, set BNDF DEFAULT=.FALSE. on the MISC line. Then

individual obstructions can be turned back on with BNDF BLOCK=.TRUE. on the appropriate OBST line.

Figure 4.5 shows several snapshots of a boundary file animation where the surfaces are colored according to their temperature. Boundary files are displayed by selecting the desired file from the Smokeview

Load/Unload menu.

4.7.4 Animated Isosurfaces: The ISOF Namelist Group

The ISOF (“ISOsurface File”) namelist group allows one to save one or more values of a single gas phase

quantity and render them as an animated sequence. The allowable quantities are DENSITY, TEMPERATURE,

HRRPUV and MIXTURE FRACTION. By default, the stoichiometric value of the mixture fraction is saved.

For example, three different values of the temperature can be saved via the line

&ISOF QUANTITY=’TEMPERATURE’,VALUE(1)=50.,VALUE(2)=200.,VALUE(3)=500. /

where the values are in degrees C. Note that the isosurface output files CHID n.iso can become very large,

so experiment with different sampling rates.

Figure 4.6 shows snapshots from an isosurface file animation at several time steps for a fire (mixture

fraction level ≈ 0.05) and a smoke layer interface (mixture fraction level ≈ 0.001). These values are just for

42
Quantity Description Symbol Units

VOLUME FLOW volume flow rate Ru· dS m3/s

MASS FLOW mass flow rate Rρu· dS kg/s

HEAT FLOW convective heat flow rate Rcpρ(T −T∞)u· dS kW

HRR heat release rate Rq ̇

000 dV kW

Table 4.4: Integrated Output Quantities for THCP only. These quantities differ from point measurements. See Section 4.7.1 for details.

example. Smoke layers can be visualized with various values of the mixture fraction variable. Isosurface

files are displayed by selecting the desired file from the Smokeview Load/Unload menu.

4.7.5 Static Data Dumps: The PL3D Namelist Group

PL3D is the namelist group that defines how often and what quantities are to be output into files of Plot3D

format. At most one PL3D line should be listed in the input file. Five quantities from Table 4.2 are written

out to a file at one instant in time every DTSAM s. The default specification is

&PL3D DTSAM=TWFIN/5,QUANTITIES=’TEMPERATURE’,

’U-VELOCITY’,’V-VELOCITY’,’W-VELOCITY’,’HRRPUV’ /

It’s best to leave the velocity components as is, because Smokeview uses them to draw velocity vectors. The

first and fifth quantities can be changed with the parameter QUANTITIES(1) and QUANTITIES(5).

Data stored in Plot3D [8] files use a format developed by NASA and used by many CFD programs for

representing simulation results. An FDS simulation creates a Plot3D file every DTSAM seconds. Plot3D

data is visualized in three ways: as 2D contours, vector plots and isosurfaces. Figure 4.7a shows an example

of a 2D Plot3D contour. Vector plots may be viewed if one or more of the u, v and w velocity components

are stored in the Plot3D file. The vector length and direction show the direction and relative speed of the

fluid flow. The vector colors show a scalar fluid quantity such as temperature. Figure 4.7b shows vectors

in a doorway. Note the hot flow (red color) leaving the fire room in the upper part of the door and the cool

flow (blue color) entering fire room in the lower part of the door. Figure 4.8 gives an example of isosurfaces

for two different temperature levels. Plot3D data are stored in files with extension .q . There is an optional

file that can be output with coordinate information if another visualization package is being used to render

the files. If one writes WRITE XYZ=.TRUE. on the PL3D line, a file with suffix .xyz is written out.

Smokeview does not require this file because the coordinate information can be obtained elsewhere.

4.7.6 Extracting Numbers from the Output Data Files

Often it is desired to present results of calculations in some form other than those offered by Smokeview.

In this case, there is a short Fortran 90 program called fds2ascii.f, with a PC compiled version called

fds2ascii.exe. To run the program, just type

fds2ascii

at the command prompt. The user is asked a series of questions about which type of output file to process, what time interval to time average the data, and so forth. A single file is produced with the name

CHID fds2ascii.csv.

43
30 s 60 s 240

Figure 4.5: Boundary file snapshots of shaded wall temperatures at t=(30, 60, 240) s after ignition. The data

file for these snapshots was generated by adding the line

&BNDF QUANTITY=’WALL TEMPERATURE’ /

to an FDS input file.

30 s 60 s 240 s

Figure 4.6: Isosurface file snapshots of mixture fraction levels at t=(30, 60, 240) s after ignition. The data

file for these snapshots was generated by adding the line

&ISOF QUANTITY=’MIXTURE FRACTION’,VALUE(1)=0.05,VALUE(2)=0.001 /

to an FDS input file.

44
a) shaded 2D temperature contour plots in a

vertical plane through the fire and a horizontal plane below the ceiling

b) shaded temperature vector plot in a vertical plane through the doorway. The “a”

key may be depressed to alter the vector

sizes. The “s” key may be depressed to

alter the number of vectors displayed.

Figure 4.7: Plot3D contour and vector plot examples.

a) isosurface at 140 ◦C b) isosurface at 320 ◦C

Figure 4.8: Plot3D isocontour example.

45
46
Chapter 5

Special Features

The following sections describe some special features of the FDS model that are not usually invoked for

engineering applications. Some of these features represent current research efforts and are to be considered

fragile.

5.1 Stopping and Restarting Calculations

Normally, a simulation consists of a sequence of events starting from ambient conditions. However, there

are occasions where the user might want to stop a calculation, make a few limited adjustments, and then

restart the calculation from that point in time. To do this, first bring the calculation to a halt gracefully

by creating a file called CHID.stop in the directory where the output files are located. Remember that

FDS is case-sensitive. The file name must be exactly the same as the CHID and ‘stop’ should be lower

case. FDS checks for the existence of this file at each time step, and if it finds it, gracefully shuts down

the calculation after first creating a final Plot3D file and a file (or files in the case of a multiple mesh job)

called CHID.restart (or CHID nn.restart). To restart a job, the file(s) CHID.restart should exist in the

current working directory, and the phrase RESTART=.TRUE. needs to be added to the MISC line of the

data file controlling the continued job. For example, suppose that the job whose CHID is “plume” is halted

by the user who creates a dummy file called plume.stop in the directory where all the output files are being

created. To restart this job from where it left off, add RESTART=.TRUE. to the MISC line of the input file

plume.data, or whatever the user has chosen to name the input file. The existence of a restart file with the

same CHID as the original job tells the code to save the new data in the same files as the old.

When running the restarted job, the diagnostic output of the restarted job is appended to the file CHID.out

that was created by the original job. All of the other output files from the original run are appended as well.

There may be times when one wants to save restart files periodically during a run as insurance against

power outages or system crashes. If this is the case, at the start of the original run set DTCORE=50. on

the MISC line to save restart files every 50 s, for example. The default for DTCORE is infinity, meaning no

restart files are created unless the user gracefully stops a job by creating a dummy file called CHID.stop.

Note that between job stops and restarts, major changes cannot be made in the calculation like adding or

removing vents and obstructions. The changes are limited to those parameters that do not instantly alter the

existing flow field. Since the restart capability has been used infrequently at NIST, it should be considered

a fragile construct. Examine the output to ensure that no sudden or unexpected events occur during the stop

and restart.

47
Figure 5.1: Piecewise Linear Transformation. Figure 5.2: Polynomial Transformation.

5.2 Stretching the Grid: The TRNX, TRNY and/or TRNZ Namelist Groups

By default the grid cells that fill the computational domain are uniform in size. However, it is possible to

specify that the cells be non-uniform in one or two of the three coordinate directions. For a given coordinate

direction, x, y or z, a function can be prescribed that maps the uniformly-spaced computational grid to a

non-uniformly spaced physical grid. Take the x direction as an example. A function x = f(ξ) maps the

uniformly-spaced Computational Coordinate (CC) (XBAR0 ≤ ξ ≤ XBAR) to the Physical Coordinate (PC)

(XBAR0 ≤ x ≤ XBAR). The function has three mandatory constraints: it must be monotonic, it must map

XBAR0 to XBAR0, and it must map XBAR to XBAR. The default transformation function is f(ξ) = ξ (uniform

grid). If uniform gridding is desired in the x direction, then nothing need be specified, and no &TRNX lines

should be written. The same is true for the y and z directions.

Two types of transformation functions are allowed. The first, and simplest, is a piecewise linear function.

Figure 5.1 gives an example of a piecewise linear transformation, in this case applied to the y coordinate

direction. The graph indicates how the uniformly-spaced computational grid (horizontal axis) is mapped

to the non-uniformly-spaced physical grid (vertical axis). In this case, the function is made up of straight

line segments connecting user-prescribed points (CC,PC). Note that the points should be given in increasing

order. The parameters used in this example are

&TRNY CC=0.30,PC=0.50,MESH_NUMBER=2 /

&TRNY CC=1.20,PC=1.00,MESH_NUMBER=2 /

The parameter CC refers to the Computational Coordinate, located on the horizontal axis; PC is the Physical

Coordinate, located on the vertical axis. In this example, the uniformly-spaced grid cells between 0 and 0.3

on the horizontal axis are mapped to larger, but still uniformly-spaced, cells on the vertical axis between

0 and 0.5. Then the segment between 0.3 and 1.2 on the horizontal axis is mapped to a segment between

0.5 and 1.0 on the vertical axis. Finally, the segment between 1.2 and 1.5 on the horizontal axis is mapped

to the segment between 1.0 and 1.5 on the vertical axis. The slopes of the line segments indicate whether

the grid is being stretched (slopes greater than 1) or shrunk (slopes less than 1). The tricky part about

this process is that the user usually has a desired shrinking/stretching strategy for the physical coordinate

48
(vertical axis), and must work backwards to determine what the corresponding points are in computational

space (horizontal axis). Note that the above transformation is applied to the second mesh in a multiple mesh

job.

The second type of transformation is a polynomial function whose constraints are of the form

d

IDERIV f(CC)

dξ

IDERIV

= PC

Figure 5.2 gives an example of a polynomial transformation. The parameters used in this example are

&TRNX IDERIV=0,CC=0.75,PC=0.75,MESH_NUMBER=3 /

&TRNX IDERIV=1,CC=0.75,PC=0.50,MESH_NUMBER=3 /

which correspond to the constraints f(0.75) = 0.75 and d f

dξ

(0.75) = 0.5, or, in words, the function maps 0.75

into 0.75 and the slope of the function at ξ = 0.75 is 0.5 . Note that these constraints are optional. The two

mandatory constraints f(XBAR0) = XBAR0 and f(XBAR) = XBAR need not, and should not, be prescribed.

The reason for this is that the mandatory constraints are already built into the linear system of equations that

is solved to yield the coefficients of the nth order polynomial. In the above example, two optional constraints

plus the two mandatory constraints yield a unique cubic polynomial f(ξ) = c0 +c1 ξ+c2 ξ

2 +c3 ξ3

. More

optional constraints lead to higher order polynomial functions. The monotonicity of the function is checked

by the program and an error message is produced if it is not monotonic. Note that the transformation above

is applied to the third mesh in a multiple mesh job.

The vertical and horizontal lines on Figs. 5.1 and 5.2 indicate how the uniformly spaced computational

grid on the horizontal axis is transformed into a non-uniformly spaced physical grid on the vertical axis.

The slope of the transformation function indicates the degree to which the computational cells is stretched

(slope greater than 1) or shrunk (slope less than 1). Note that shrinking cells in one region necessarily leads

to stretching cells elsewhere. When one or two coordinate directions are transformed, the aspect ratio of

the grid cells in the 3D mesh vary. To be on the safe side, transformations that alter the aspect ratio of

cells beyond 2 or 3 should be avoided. Keep in mind that the large eddy simulation technique is based

on the assumption that the numerical grid should be fine enough to allow the formation of eddies that are

responsible for the mixing. In general, eddy formation is limited by the largest dimension of a grid cell,

thus shrinking the grid in one or two directions may not necessarily lead to a better simulation if the third

dimension is large. Also note that transformations, in general, reduce the efficiency of the computation, with

two coordinate transformations impairing efficiency more than a transformation in one coordinate direction.

5.3 Initial Conditions: The INIT Namelist Group

Usually, an FDS calculation is initialized with constant ambient conditions; that is, the temperature, density

and species mass fractions are fixed. However, there are some problems for which it is convenient to change

the ambient conditions within some rectangular region of the domain. If so, add lines of the form

&INIT XB=0.5,0.8,2.1,3.4,2.5,3.6,QUANTITY=’TEMPERATURE’,VALUE=30. /

Here, within the region whose bounds are given by the sextuplet XB, the initial temperature shall be 30 ◦C

instead of the ambient. This construct can also be used for QUANTITY=’DENSITY’ or SPECIES ID

where SPECIES ID is a character string that is the name of a listed species.

This construct may be useful in examining the influence of stack effect in a building, where the temperature is different inside and out.

A solid obstruction can be given an initial temperature via the parameter TMPWAL0 on the SURF line.

49
5.4 Creating or Removing Obstructions; Opening or Closing Vents

In many fire scenarios, the opening or closing of a door or window can lead to dramatic changes in the course

of the fire. Sometimes these actions are taken intentionally, sometimes as a result of the fire. Within the

framework of an FDS calculation, these actions are represented by the creation or removal of solid obstacles,

or the opening or closing of exterior vents.

Remove or create a solid obstruction by entering a time via the parameter T REMOVE or T CREATE on

the OBST line that defines the obstruction that is to be created or removed. For example, the line

&OBST XB=...,SURF_ID=’whatever’,T_CREATE=39. /

instructs the code to create the given obstruction 39 s after the start of the simulation. Likewise, the line

&OBST XB=...,SURF_ID=’whatever’,T_REMOVE=39. /

instructs the code to remove the obstruction after 39 s. To create an obstruction and then remove it, combine

the instructions as follows

&OBST XB=...,SURF_ID=’whatever’,T_CREATE=30.,T_REMOVE=39. /

To remove an obstruction, then re-create one in its place, use 2 lines

&OBST XB=...,SURF_ID=’whatever’,T_REMOVE=30. /

&OBST XB=...,SURF_ID=’whatever’,T_CREATE=39. /

since the code simply sees this as two different obstructions. Experiment with these combinations using a

simple case before trying a case to make sure that the code indeed is doing what is intended.

One additional feature is to time the removal or creation of an obstruction with a thermally-responsive

device; in FDS the device being a HEAT detector. Assigning the character strings HEAT REMOVE or

HEAT CREATE the name of a HEAT detector will direct FDS to remove or create the obstruction upon

activation of the detector. For example, the lines

&OBST XB=...,SURF_ID=’whatever’,HEAT_REMOVE=’det2’ /

.

.

&HEAT XYZ=...,RTI=...,ACTIVATION_TEMPERATURE=87. ,LABEL=’det1’ /

&HEAT XYZ=...,RTI=...,ACTIVATION_TEMPERATURE=110.,LABEL=’det2’ /

causes the given obstruction to be removed when the specified HEAT detector activates. If either HEAT REMOVE

or HEAT CREATE is set to ’ALL’, then the desired action is triggered by the activation of any HEAT detector.

The removal and creation of an obstruction can be used to model the opening of a door that connects

one part of the domain to another. If one wants to open or close a window or door to the outside of the

computational domain (i.e. the atmosphere), a similar set of parameters can be used on the VENT line. For

example, the line

&VENT XB=...,SURF_ID=’OPEN’,T_CLOSE=39. /

instructs the code to close a vent to the exterior of the domain at 39 s. The line

&VENT XB=...,SURF_ID=’OPEN’,HEAT_OPEN=’det1’ /

.

.

&HEAT XYZ=...,RTI=...,ACTIVATION_TEMPERATURE=87. ,LABEL=’det1’ /

&HEAT XYZ=...,RTI=...,ACTIVATION_TEMPERATURE=110.,LABEL=’det2’ /

50
instructs the code to open an initially closed vent to the outside when the first HEAT detector activates.

One additional feature associated with a VENT is to specify a time or a thermal device that controls

when the VENT’s SURF ID is to be applied. For example, suppose it is desired that when the HEAT detector

labelled ’det2’, a fan should be turned on. Set

&SURF ID=’FAN’,VOLUME_FLUX=5. /

&VENT XB=...,SURF_ID=’FAN’,HEAT_ACTIVATE=’det2’ /

If it is desired that the fan be turned off, use the parameter HEAT DEACTIVATE in the very same way. Note

that T ACTIVATE and T DEACTIVATE are equivalent to T OPEN and T CLOSE. Also note that none of

these control parameters should be applied to a MIRROR.

5.5 Extra Species

Normally when one specifies a fire via either HRRPUA or HEAT OF VAPORIZATION, the mixture fraction

combustion model is applied. A single scalar variable, Z, represents the state of the combustion process from

pure fuel (Z = 1) to pure air (Z = 0). The major reactants and products of combustion – fuel, O2, CO2, H2O,

N2, CO and soot – are all pre-tabulated functions of the mixture fraction, Z. In other words, the value of Z

in any given grid cell determines the mass fraction of all the gases listed. The user-defined stoichiometry

listed under the REAC namelist group is used to generate the table associating the mass fractions with Z.

One need not, and should not, explicitly list the reactants and products of combustion.

Suppose however that gases are introduced into the domain that are neither reactants nor products of

combustion. This gas can be tracked separately from the mixture fraction via a second scalar transport

equation1. In fact, there does not need to be any fire at all – the FDS code can be used to transport a mixture

of non-reacting ideal gases.

The namelist group SPEC is used to specify each additional species. Each SPEC line should include at the very least the name of the species via a character string called (ID). Next, if the ambient

(initial) mass fraction of the gas is something other than 0, then the parameter MASS FRACTION 0 is

used to specify it. Several gases that can be included in a calculation are listed in Table 5.1. The physical properties of these gases are known and do not need to be specified. However, if a desired gas is

not included in Table 5.1, its molecular weight MW must be specified in units of g/mol. In addition, if a

DNS calculation is being performed, either the Lennard-Jones potential parameters σ (SIGMALJ) and ε/k

(EPSILONKLJ) should be specified; or the VISCOSITY (kg/m/s), THERMAL CONDUCTIVITY (W/m/K),

and DIFFUSION COEFFICIENT (m2/s) between the given species and the background species should be

specified.

&SPEC ID=’ARGON’,MASS_FRACTION_0=0.1,MW=40. /

There are three types of boundary conditions for the listed species. Reference to a given species is via its

place in the input file. For example, the second listed species is N=2. If a simple no-flux condition is desired

at a solid wall, do not set anything. If the mass fraction of the Nth species is to be some value at a forced

flow boundary, set MASS FRACTION(N) equal to the desired mass fraction on the appropriate SURF line.

If the mass flux of the Nth species is desired, set MASS FLUX(N) instead of MASS FRACTION(N). If

MASS FLUX(N) is set, no VEL should be set. It is automatically calculated based on the mass flux. The

mass flux is in units of kg/m2/s.

1 Often an extra gas introduced into a calculation is the same as a product of combustion, like water vapor from a sprinkler or

carbon dioxide from an extinguisher. These gases are tracked separately, thus water vapor generated by the combustion is tracked via

the mixture fraction variable and water vapor generated by evaporating sprinkler droplets is tracked via its own transport equation.

In the case of sprinklers, do not specify WATER VAPOR as an extra species – it is done automatically.

51
Use TAU MF(N) or RAMP MF(N) to control the ramp-ups for either the mass fraction or mass flux of

species N. The mass fraction of species N at the surface is given by

YN(t) = YN(0) + f(t) (YN −YN(0))

where YN(0) is the ambient mass fraction of species N (MASS FRACTION 0 in the Nth SPEC namelist

line is used to prescribe YN(0)), YN is the desired mass fraction to which the function f(t) is ramping

(MASS FRACTION(N) specified in the SURF line is used to prescribe YN). The function f(t) is either a

tanh, t

2

, or user-defined function. For a user-defined function, indicate the name of the ramp function with

RAMP MF(N), a character string (see Time Dependent Boundary Conditions in Section 4.4.1).

As an example, the lines

&SPEC ID=’ARGON’,MASS_FRACTION_0=0.1,MW=40. /

&SPEC ID=’HELIUM’ /

.

.

&SURF ID=’INLET’,MASS_FRACTION(2)=0.2,VEL=-0.3,TAU_MF(2)=0.5,TAU_V=0.5 /

specify that ARGON and HELIUM are to be included in the calculation in addition to the (unlisted) default

BACKGROUND SPECIES=’AIR’. At the INLET, a mixture of helium (0.2 by mass), argon (0.1 by mass

because nothing different is specified), and air (0.7 by mass making up the rest) flows out at a velocity of

0.3 m/s into the flow domain. The mass fraction of helium and the velocity are both ramped up according to

the function tanh(t/0.5).

5.6 Finite-Rate or Premixed Combustion

By default, FDS assumes that the fire is essentially an infinitely-fast reaction between fuel and oxygen, and

this reaction is not dependent on the surrounding gas temperature. It also assumes that the reaction zone is

an infinitely thin sheet with fuel on one side and oxygen on the other. If a finite-rate or a pre-mixed reaction

is desired, the following steps must be taken:

1. It is strongly recommended that finite-rate reactions be invoked only when FDS is running in DNS

mode. Set DNS=.TRUE. on the MISC line. Note: one may attempt to use the finite-rate reaction

scheme in an LES calculation, but because the temperature in a large scale calculation is smeared out

over a grid cell, some of the reaction parameters may need to be modified to account for the lower

temperatures.

2. The BACKGROUND SPECIES on the MISC line is normally set to be ’NITROGEN’.

3. The namelist group SPEC is used to specify each additional species. Do not enter a SPEC line for

the background species. Each SPEC line should include the name of the species (ID) and its ambient

(initial) mass fraction, MASS FRACTION 0. Several gases that can be included in a calculation are

listed in Table 5.1. The physical properties of these gases are known and need not be specified.

However, if a desired gas is not included in Table 5.1, its molecular weight MW must be specified in

units of g/mol. In addition, if a DNS calculation is being performed, either the Lennard-Jones potential

parameters σ (SIGMALJ) and ε/k (EPSILONKLJ) should be specified; or the VISCOSITY (kg/m/s),

THERMAL CONDUCTIVITY (W/m/K), and DIFFUSION COEFFICIENT (m2

/s) between the given

species and the background species should be specified. If the listed species is to be consumed or

generated by the finite-rate reaction, its stoichiometric coefficient, NU, needs to be specified. Note

that the background species cannot participate in the reaction except as a diluent.

52
Table 5.1: Optional Gas Species [9]

Species Mol. Wgt. σ k/ε

(g/mol) (A)  ̊ (K)

AIR 29 3.711 78.6

CARBON DIOXIDE 44 3.941 195.2

CARBON MONOXIDE 28 3.690 91.7

HELIUM 4 2.551 10.22

METHANE 16 3.758 148.6

NITROGEN 28 3.798 71.4

OXYGEN 32 3.467 106.7

PROPANE 44 5.118 237.1

WATER VAPOR 18 2.641 809.1

4. Read Section 5.5 for a description of the boundary conditions for the gas species.

5. The REAC namelist group is used to designate the fuel and the reaction rate parameters.

FUEL Character string indicating which of the listed optional gas species is the fuel.

BOF Pre-exponential factor in one-step chemical reaction in units of cm3/mole/s.

E Activation energy for one-step chemical reaction in units of kJ/kmol.

XNO Exponent for oxygen concentration in one-step chemical reaction. (Default 1.)

XNF Exponent for fuel concentration in one-step chemical reaction. (Default 1.)

DELTAH The effective heat of combustion for one-step chemical reaction in units of kJ/kg. (Default

40,000 kJ/kg)

5.7 Pyrolysis Models

Fuel for a fire can be either a gas, solid or liquid. Gaseous fuels are easist to model because there is no phase

change. In fact, specifying HRRPUA on the SURF line is equivalent to defining a gas burner with a specified

flow rate. If this is all that is desired, skip this section. Otherwise, predicting the burning rate of solids and

liquids requires more information to define the physical properties of the fuel.

5.7.1 Thermoplastics

By default, a solid burning object is assumed to be a homogenous material that burns at the surface. The

alternative is to specify PHASE=’CHAR’ or PHASE=’LIQUID’ to direct the code to model the material as

a char former or liquid, respectively (see below). For a thermoplastic material, specify the thermal properties

of the material. The material can be regarded as thermally-thick or thin. In the former case, specify the

thickness DELTA (m), DENSITY (kg/m3), thermal conductivity KS or RAMP KS (W/m/K), specific heat

C P or RAMP C P (kJ/kg/K). For a thermally-thin material, specify the product of the specific heat, thickness

and density, C DELTA RHO (kJ/m2/K); or specify separately the thickness DELTA (m), DENSITY (kg/m3),

and specific heat C P or RAMP C P (kJ/kg/K). The default thickness is 0.1 m and the default density is

450 kg/m3. Do not specify the thermal conductivity if the material is to be regarded as thermally-thin.

53
The burning rate of a thermoplastic is given by the expression

m ̇

00 = A ρs e−E/RT (5.1)

The density of the material ρsis either directly prescribed via the parameter DENSITY, or is inferred from

the other parameters. It is preferable to prescribe DENSITY explicitly. A is prescribed under the name A,

with units of m/s. E, the activation energy, is prescribed via E in units of kJ/kmol. Remember that 1 kcal

is 4.184 kJ, and be careful with factors of 1000. A and E are not readily accessible for most real fuels.

However, if they are known, prescribe both. Avoid prescribing just one because they act as a pair. If A and E

are not known, which is usually the case, prescribe MASS FLUX CRITICAL (kg/m2

/s) and TMPIGN (

◦C).

This directs the code to choose A and E so that the fuel burns at the rate MASS FLUX CRITICAL when

its surface reaches the temperature TMPIGN. Note that the temperature is read in using degrees Celsius, but

is then converted to degrees Kelvin within the program. The default value of MASS FLUX CRITICAL is

0.02 kg/m2/s. The default TMPIGN is 5000 ◦C (in other words, no burning occurs).

Remember to include the HEAT OF VAPORIZATION (kJ/kg) if the solid is to be regarded as a thermoplastic.

5.7.2 Charring Fuels

By default, a burning object is assumed to be a homogenous solid that burns at the surface. However, many

materials burn internally, leaving char in the wake of a pyrolysis front that progresses into the material. To

specify this type of burning behavior, set PHASE=’CHAR’ on the SURF line, then specify material properties for both the virgin material and the char. For the virgin material, the properties are those of a thermallythick solid: DELTA (m), DENSITY (kg/m3

), KS or RAMP KS (W/m/K), C P or RAMP C P (kJ/kg/K).

For the char, the parameters are similar: CHAR DENSITY, KS CHAR or RAMP KS CHAR, C P CHAR or

RAMP C P CHAR.

The burning behavior is described using similar parameters as a thermoplastic material:

m ̇

00 = A (ρs −ρc) e−E/RT (5.2)

The density of the virgin material ρs and the density of the char ρc are both directly prescribed via the

parameters DENSITY and CHAR DENSITY. A is prescribed under the name A, with units of m/s. E, the

activation energy, is prescribed via E in units of kJ/kmol. These parameters are not readily accessible for

most real fuels. An alternative is to prescribe MASS FLUX CRITICAL (kg/m2/s) and TMPIGN (

◦C). This

directs the code to choose A and E so that the fuel burns at the rate MASS FLUX CRITICAL when its

surface reaches the temperature TMPIGN. Note that the temperature is read in using degrees Celsius, but

is then converted to degrees Kelvin within the program. The default value of MASS FLUX CRITICAL is

0.02 kg/m2/s. The default TMPIGN is 5000 ◦C (in other words, no burning occurs).

Remember to include the HEAT OF VAPORIZATION (kJ/kg) if the solid is to be regarded as a charring fuel. Note that the HEAT OF VAPORIZATION refers to the gasification of the virgin material at the

pyrolysis front. It is not an “effective” value that is often used to model the effect of the char shielding the

virgin material from the heat flux at the surface.

One additional parameter describing a charring material is MOISTURE FRACTION, giving the mass

fraction of water in the virgin material. An entry for a charring material is given here, only as an example:

&SURF ID=’SPRUCE’

PHASE = ’CHAR’

MOISTURE_FRACTION = 0.05

DELTA=0.01

54
TMPIGN=360.0

HEAT_OF_VAPORIZATION=500.

DENSITY = 450.

RAMP_KS = ’KS’,

RAMP_C_P = ’CPV’,

RAMP_C_P_CHAR = ’CPC’,

RAMP_KS_CHAR = ’KSC’,

CHAR_DENSITY = 120.

WALL_POINTS = 30

BACKING = ’INSULATED’/

&RAMP ID = ’KS’, T = 20., F = 0.13 /

&RAMP ID = ’KS’, T = 500., F = 0.29 /

&RAMP ID = ’KSC’, T = 20., F = 0.077 /

&RAMP ID = ’KSC’, T = 900., F = 0.16 /

&RAMP ID = ’CPV’, T = 20., F = 1.2 /

&RAMP ID = ’CPV’, T = 500., F = 3.0 /

&RAMP ID = ’CPC’, T = 20., F = 0.68 /

&RAMP ID = ’CPC’, T = 400., F = 1.5 /

&RAMP ID = ’CPC’, T = 900., F = 1.8 /

5.7.3 Liquid Fuels

For a liquid fuel, specify PHASE=’LIQUID’ on the SURF line. The thermal parameters are the same as

those of a thermally-thick solid. The evaporation rate of the fuel is governed by the Clausius-Clapeyron

equation (see FDS Technical Reference Guide for details). The only drawback of this approach is that the

fuel gases burn regardless of any ignition source. Thus, if PHASE=’LIQUID’ is specified, the fuel begins

burning at once. An example of a liquid fuel is

&SURF ID=’METHANOL’

HEAT_OF_VAPORIZATION=1101.

PHASE=’LIQUID’

DELTA=0.01

KS=0.20

DENSITY=900.

C_P=2.5

TMPIGN=65. /

Note that TMPIGN is assumed to be the boiling temperature of the liquid. The thermal conductivity, density and specific heat are used to compute the loss of heat into the liquid via conduction using the same

one-dimensional heat transfer equation that is used for solids. Obviously, the convection of the liquid is

important, but is not considered in the model.

5.8 Burning Liquid Fuel Droplets

The evaporization of water droplets from sprinklers has been generalized so that a liquid fuel spray nozzle

can be modeled. Fuel evaporation is triggered by the inclusion of the phrase FUEL=.TRUE. on the appropriate PART line. The spray nozzle characteristics are specified in the same way as those for a sprinkler.

Fuel properties are specified as follows:

55
&PART ID=’heptane’,FUEL=.TRUE.,

VAPORIZATION_TEMPERATURE=98.0,

HEAT_OF_VAPORIZATION=316.0,

SPECIFIC_HEAT=2.25,

DENSITY=688.0,... /

The vaporization (boiling) temperature of the liquid fuel is in degrees Celsius, the heat of vaporization is in

units of kJ/kg, the specific heat is in units of kJ/kg/K, and the density is in units of kg/m3. FUEL=.TRUE.

automatically invokes a mixture fraction calculation in which fuel from the evaporating fuel droplets is

burned when it has diluted to the appropriate stoichiometric value. Note that this construct is fragile and

subject to grid dependence. If the grid cells are too coarse, the evaporating fuel is diluted to such a degree

that it never burns. Proper resolution depends on the type of fuel and the amount of fuel being ejected from

the nozzle.

5.9 Suppression by Water (Mixture Fraction Model Only)

Modeling suppression of a fire by a water spray is challenging because the relevant physical mechanisms

occur at length scales smaller than a single grid cell. In the gas phase, flames are extinguished due to

lowered temperatures and dilution of the oxygen supply. See Section 4.4.3 for more information about gas

phase suppression.

For the solid phase, water reduces the fuel pyrolysis rate by cooling the fuel surface and also changing

the chemical reactions that liberate fuel gases from the solid. If the fuel has been assigned a

HEAT OF VAPORIZATION, there is no need to set any additional suppression parameters. It is assumed

that water impinging on the fuel surface takes energy away from the pyrolysis process and thereby reduces

the burning rate of the fuel. If the surface has been assigned a HRRPUA (Heat Release Rate Per Unit Area),

a parameter needs to be specified that governs the suppression of the fire by water. An empirical way to

account for fire suppression by water is to characterize the reduction of the pyrolysis rate in terms of an

exponential function. The local mass loss rate of the fuel is expressed in the form

m ̇

00

f

(t) = m ̇

00

f,0

(t) e

−

R

k(t) dt (5.3)

Here  ̇m

00

f,0

(t) is the user-prescribed burning rate per unit area when no water is applied and k is a function of

the local water mass per unit area, m

00

w

, expressed in units of kg/m2.

k(t) = E COEFFICIENT m

00

w

(t) s

−1

(5.4)

The parameter E COEFFICIENT must be obtained experimentally, and it is expressed in units of m2/kg/s.

Usually, this type of suppression algorithm is invoked when the fuel is complicated, like a cartoned commodity.

Another parameter used in water suppression calculations is the fuel POROSITY which is the fraction

of water that does not cascade down the side of the fuel package, either because of absorption or because it

is trapped within the interior of the fuel. Both POROSITY and E COEFFICIENT are 0 by default and both

are prescribed on the SURF line.

5.10 Visibility

If one is performing a fire calculation using the mixture fraction approach, the smoke is tracked along with

all other major products of combustion. The most useful quantity for assessing visibility in a space is the

56
light extinction coefficient, K [10]. The intensity of monochromatic light passing a distance L through smoke

is attenuated according to

I/I0 = e

−KL (5.5)

The light extinction coefficient, K, is a product of the density of smoke particulate, ρYs, and a mass specific

extinction coefficient that is fuel dependent

K = Km ρYs (5.6)

Estimates of visibility through smoke can be made by using the equation

S = C/K (5.7)

where C is a nondimensional constant characteristic of the type of object being viewed through the smoke,

i.e. C = 8 for a light-emitting sign and C = 3 for a light-reflecting sign [10]. Since K varies from point

to point in the domain, the visibility S does as well. Keep in mind that FDS can only track smoke whose

production rate and composition are specified. Predicting either is beyond the capability of the present

version of the model.

Three parameter control smoke production and visibility; each parameter is input on the REAC line. The

first parameter is SOOT YIELD, which is the fraction of fuel mass that is converted to soot. The second

parameter is called the MASS EXTINCTION COEFFICIENT, and it is the Km in Eq. (5.6). The default

value is 7600 m2/kg, a value suggested for flaming combustion of wood and plastics. The third parameter is

called the VISIBILITY FACTOR, the constant C in Eq. (5.7). It is 3 by default.

The slice, Plot3D or thermocouple output quantity extinction coefficient is K. The visibility

S is output via the keyword visibility. Note that each is tied to the mixture fraction formulation of

combustion.

5.11 Layer Height and the Average Upper and Lower Layer Temperatures

Fire protection engineers often need to estimate the location of the interface between the hot, smoke-laden

upper layer and the cooler lower layer in a burning compartment. Relatively simple fire models, often referred to as two-zone models, compute this quantity directly, along with the average temperature of the upper

and lower layers. In a computational fluid dynamics (CFD) model like FDS, there are not two distinct zones,

but rather a continuous profile of temperature. Nevertheless, there are methods that have been developed to

estimate layer height and average temperatures from a continuous vertical profile of temperature. One such

method is as follows: Consider a continuous function T(z) defining temperature T as a function of height

above the floor z, where z = 0 is the floor and z = H is the ceiling. Define Tu as the upper layer temperature,

Tl as the lower layer temperature, and zint as the interface height. Conservation of energy dictates that

(H −zint) Tu +zint Tl =

Z H

0

T(z) dz = I1 (5.8)

and conservation of mass (assuming a perfect gas) dictates that

(H −zint)

1

Tu

+zint

1

Tl

=

Z H

0

1

T(z)

dz = I2 (5.9)

Solving for zint:

zint =

Tl(I1 I2 −H

2

)

I1 +I2 T

2

l −2Tl H

(5.10)

57
Letting Tl be the temperature in the lowest grid cell and using Simpson’s Rule to perform the numerical

integration of I1 and I2, Tu can be defined as the average upper layer temperature via

(H −zint) Tu =

Z H

zint

T(z) dz (5.11)

Further discustion of this procedure can be found in Ref. [11].

The quantities LAYER HEIGHT, UPPER TEMPERATURE and LOWER TEMPERATURE can be displayed in Smokeview as slice (SLCF) files or in a spread sheet file via “thermocouple” (THCP) entries in

the input file. For example, the entry

&THCP XYZ=2.0,3.0,0.5,QUANTITY=’LAYER HEIGHT’,LABEL=’whatever’ /

produces a time history of the smoke layer height at x = 2 and y = 3. The coordinate z = 0.5 is not used

and can be anything so long as it is within the range of z defined on the PDIM line. Otherwise, the THCP

line is ignored. Normally, the vertical integrations are carried out from the lowest grid cell to the highest

(1 ≤ k ≤ KBAR). To change this, add the parameters K LOW and K HIGH to the THCP or SLCF line. Note

that for any one mesh, there can only be one set of limits.

If multiple meshes are being used, the THCP is assigned to the mesh corresponding to the XYZ coordinates. If two or more meshes overlap at this point, control goes to the mesh with the lowest index, that is, the

mesh listed first in the input file. In the case of a slice file, add the parameter MESH NUMBER to the SLCF

line to indicate directly which mesh to use in the integration if there is any possible chance of confusion.

This also reduces the computation time a bit since the unwanted meshes do not generate undesired slice

files.

5.12 Leakage

For a limited class of scenarios, it is possible to prescribe leakage in an FDS calculation. Three criteria

must be met. First, the boundary of the computational domain must coincide with the exterior walls of

the compartment. Second, there must be no OPEN (passive) vents to the exterior. Third, only one mesh

must be used. If these three criteria are satisfied, then prescribe LEAK AREA on the MISC line, and assign

to at least one of the wall materials (regardless of whether or not it is on the exterior boundary) the attribute LEAKING=.TRUE. on its SURF line. The program assigns the leakage uniformly to the LEAKING

surfaces. The LEAK AREA (m2) is based on the formula

AL = V ̇

p

ρ∞/2(p0 − p∞) (5.12)

where V ̇ is the airflow rate (m3/s) at a given background pressure p0 (Pa). ρ∞ is the ambient density (kg/m3).

Note that the discharge coefficient normally seen in this type of formula is assumed to be 1.

5.13 Fires and Flows in the Outdoors

Simulating a fire in the outdoors is not much different than a fire indoors, but there are several useful parameters that can easily be invoked. First, it is easy to prescribe the wind with a realistic increase in velocity

with altitude. By default the velocity (wind) profile at any vent is a top hat, but the parameter PROFILE

on the SURF line can yield other profiles. For example, PROFILE=’PARABOLIC’ produces a parabolic

profile with VEL being the maximum velocity, and ’ATMOSPHERIC’ produces a typical atmospheric wind

profile of the form u = u0(z/z0)

p

. If an atmospheric profile is prescribed, also prescribe Z0 for z0 and PLE

for p. VEL specifies the reference velocity u0.

58
Another useful parameter for outdoor simulations is the temperature lapse rate of the atmosphere. Typically, in the first few hundred meters of the atmosphere, the temperature decreases several degrees Celsius

per kilometer. These few degrees are important when considering the rise of smoke since the temperature

of the smoke decreases rapidly as it rises. DT0DZ is the lapse rate of the atmosphere in units of ◦C/m. This

need only be set for outdoor calculations where the height of the domain is tens or hundreds of meters. The

default value of DT0DZ is -g/cp ≈-0.0097 ◦C/m.

Figure 5.3 gives an example of an outdoor fire scenario, with the corresponding input data file given

in Figure 5.4. The tanks are built from rectangular obstructions forming a cylindrical shape. The fire is

specified on the top of one tank and a wind is prescribed at one of the computational boundaries.

5.14 2D and Axially-Symmetric Calculations

The governing equations solved in FDS are written in terms of a three dimensional Cartesian coordinate

system. However, a two dimensional Cartesian or two dimensional cylindrical (axisymmetric) calculation

can be performed by setting JBAR=1 on the &GRID line, and for axisymmetry replacing the parameter

XBAR with RBAR on the &PDIM line. No boundary conditions should be set at the planes y = YBAR0 or

y = YBAR, nor at x = RBAR0 in an axisymmetric calculation in which RBAR0=0. For better visualizations,

the difference of YBAR and YBAR0 should be small so that the Smokeview rendering appears to be in 2D.

An example of an axially-symmetric helium plume is shown in Fig. 5.5 with the corresponding input data

file in Fig. 5.6.

5.15 Restoring the Baroclinic Vorticity

There is an approximation made when solving for the pressure where it is assumed that

∇·

1

ρ

∇p ̃ =

1

ρ0

∇

2

p ̃ (5.13)

The consequence of this approximation is that the vorticity generated due to the non-alignment of the density

and pressure gradients, or the baroclinic torque, is neglected. For most large scale applications, the assumption is justified by the fact that the vorticity generated by buoyancy is the dominant source of vorticity. By

neglecting the baroclinic torque the solution of the elliptic partial differential equation obtained by taking

the divergence of the momentum equation is greatly simplified. However, an option exists in the code to

restore the baroclinic torque by decomposing the relevant term in the pressure equation

∇·

∇p ̃

ρ

= ∇·

∇p ̃

ρ ̄

+∇·



1

ρ

−

1

ρ ̄



∇p ̃ (5.14)

and evaluating the second term on the right hand side with values of pressure from the previous time step.

The expression ρ ̄ is an average density, equal to 2ρminρmax/(ρmin +ρmax). To make this correction, simply

include the statement

BAROCLINIC=.TRUE.

on the MISC line. In a DNS calculation (DNS=.TRUE.), the correction is made by default. However, for

an LES calculation (default), the correction must be explicitly invoked. The cost of the correction is not

prohibitive – try calculations with and without the correction to determine if its inclusion is warranted.

59
Figure 5.3: Instantaneous snapshot of a large oil fire simulation. The domain is 384 m by 384 m by 288

m. Each tank is 84 m in diameter and 27 m tall. The grid is uniform with 6 m grid cells.

60
&HEAD CHID=’tankfarm2’,TITLE=’Japanese Oil Storage Tank Farm’ /

&GRID IBAR=64,JBAR=64,KBAR=48 /

&PDIM XBAR0=64.,XBAR=448.,YBAR0=192.,YBAR=576.,ZBAR=288. /

&TIME TWFIN=60. /

&MISC DT0DZ=0. /

&SURF ID=’WIND’,VEL=-5.,PROFILE=’ATMOSPHERIC’,Z0=27.,PLE=0.15 /

&SURF ID=’FIRE’,HRRPUA=1500.,PART_ID=’tracers’ /

&PART ID=’tracers’,MASSLESS=.TRUE. /

&OBST XB= 0.,138., 0.,768., 0., 9. /

&OBST XB=138.,144., 0.,768., 0., 6. /

&OBST XB=144.,150., 0.,768., 0., 3. /

.

.

.

&OBST XB=174.,180.,372.,396., 0., 27.,SURF_IDS=’FIRE’,’INERT’,’INERT’ /

&OBST XB=180.,186.,360.,408., 0., 27.,SURF_IDS=’FIRE’,’INERT’,’INERT’ /

.

.

&VENT CB=’XBAR0’,SURF_ID=’WIND’ /

&VENT CB=’YBAR’ ,SURF_ID=’OPEN’ /

&VENT CB=’YBAR0’,SURF_ID=’OPEN’ /

&VENT CB=’XBAR’ ,SURF_ID=’OPEN’ /

&VENT CB=’ZBAR’ ,SURF_ID=’OPEN’ /

&SLCF PBY=384.,QUANTITY=’TEMPERATURE’,VECTOR=.TRUE. /

&SLCF PBY=384.,QUANTITY=’HRRPUV’ /

&SLCF PBY=384.,QUANTITY=’MIXTURE_FRACTION’ /

&BNDF QUANTITY=’HEAT_FLUX’ /

&PL3D DTSAM=60. /

Figure 5.4: Input data file for tankfarm scenario.

61
Figure 5.5: Instantaneous snapshot of an axially-symmetric helium plume.

&HEAD CHID=’helium’,TITLE=’Axisymmetric Helium Plume’ /

&GRID IBAR=72,JBAR=1,KBAR=144 /

&PDIM RBAR=0.08,YBAR=0.001,ZBAR=0.16 /

&TIME TWFIN=10.0 /

&MISC DNS=.TRUE.,ISOTHERMAL=.TRUE. /

&SPEC ID=’HELIUM’ /

&SURF ID=’HELIUM’,VEL=-0.673,MASS_FRACTION(1)=1.0,TAU_MF(1)=0.3 /

&VENT CB=’XBAR’ ,SURF_ID=’OPEN’ /

&VENT CB=’ZBAR’ ,SURF_ID=’OPEN’ /

&OBST XB= 0.0,0.036, 0.00, 0.01,0.00,0.02,SURF_IDS=’HELIUM’,’INERT’,’INERT’ /

&PL3D DTSAM=2.0,QUANTITIES(1)=’DENSITY’,QUANTITIES(5)=’HELIUM’ /

&SLCF PBY=0.000,QUANTITY=’DENSITY’,VECTOR=.TRUE. /

&SLCF PBY=0.000,QUANTITY=’HELIUM’ /

Figure 5.6: Input data file for helium plume calculation.

62
5.16 Fine-Tuning the Radiation Transport Model

There are several ways to improve the performance of the Finite Volume Method in solving the radiation

transport equation (RTE), most of which increase the computation time. The solver has two modes of operation – a gray gas model (default) and a wide band model [1]. Modifications to these models can be made via

a namelist group called RADI. If running in gray gas mode (default), increase the number of angles from the

default 100 with the integer parameter NUMBER RADIATION ANGLES. The frequency of calls to the radiation solver can be reduced from every 3 time steps with integer TIME STEP INCREMENT. The increment

over which the angles are updated can be reduced from 5 with the integer ANGLE INCREMENT. Briefly,

if TIME STEP INCREMENT and ANGLE INCREMENT are both set to 1, the radiation field is completely

updated in a single time step, but the cost of the calculation increases significantly.

A few parameters affecting the absorption of radiation by water droplets are as follows: RADTMP is the

assumed radiative source temperature. It is used in the computation of the mean scattering and absorption

cross sections of water droplets. The default is 900 ◦C. NMIEANG is the number of discretization points

of the polar angle in the integration of the single droplet phase function. Increasing NMIEANG improves

the accuracy of the radiative properties of water droplets. The cost of the better accuracy is seen in the

initialization phase, not during the actual simulation. The default value for NMIEANG is 15.

If the optional six band model is desired, set WIDE BAND MODEL=.TRUE.. It is recommended that

this option only be used when the fuel is relatively non-sooting because it adds significantly to the cost of the

calculation. To add three additional fuel bands, set CH4 BANDS=.TRUE.. See FDS Technical Reference

Guide for more details.

Note that the radiation solver has been designed to work with the mixture fraction combustion model.

If the mixture fraction model is not being used, the radiation solver can still be used if CARBON DIOXIDE

is prescribed as a product of combustion, or if a constant absorption coefficient KAPPA0 is specified on

the RADI line. Note also that it is possible to turn off the radiation transport solver (saving roughly 20 %

in CPU time) by adding the statement RADIATION=.FALSE. to the MISC line. For isothermal calculations, the radiation is turned off automatically. If burning is taking place and radiation is turned off, then

RADIATIVE FRACTION from the REAC line is subtracted from the total heat release rate. This radiated

energy completely disappears from the calculation.

5.17 Defying Gravity

Most users of FDS assume that the acceleration of gravity points toward the negative end of the z axis, or

more simply, downward. However, to change the direction of gravity to model a sloping roof or tunnel, for

example, specify the gravity vector on the MISC line with a triplet of numbers of the form GVEC=0.0,0.0,-9.81

(units are m/s2). This is the default, but it can be changed to be any direction.

Note: if sprinklers are specified, the gravity vector must not be changed. Much of the logic governing

the trajectories of water droplets over solid objects assumes that gravity points in the negative z direction.

5.18 Isothermal and Salt Water Simulations

Although FDS was designed specifically for fire simulations, it can be used for other fluid flow simulations

that do not include fire or heat addition of any kind. First, set ISOTHERMAL=.TRUE. on the MISC line.

This logical parameter indicates that the calculation does not involve any change in temperature and no

radiation heat transfer, thus reducing the number of equations that must be solved, simplifying those that

are, and reducing the computation time.

63
A valuable model validation exercise is to simulate the mixing of fresh and salt water. These types of

experiments have traditionally been performed to mimic the movement of smoke in a building. Although

FDS is rarely used for this purpose now, the capability still exists in the code to handle fresh/salt water

interactions. To invoke this feature, include the statements

&MISC ISOTHERMAL=.TRUE.,BACKGROUND_SPECIES=’FRESH WATER’,DENSITY=1000.,

VISCOSITY=1.0E-3,SC=1. /

&SPEC ID=’SALT WATER’,DENSITY=1052.,VISCOSITY=1.0E-3 /

in the input file, along with appropriate boundary conditions for the salt water. Note that the names ’FRESH

WATER’ and ’SALT WATER’ have no particular meaning as far as the code is concerned. What matters

is the designation of DENSITY and VISCOSITY for both, plus a global Schmidt number SC. Without the

designation DNS=.TRUE., the calculation is performed as a Large Eddy Simulation (LES), in which case

the VISCOSITY serves as a lower bound for the Smagorinsky viscosity, and the Schmidt number is used to

relate the viscosity to the material diffusivity.

5.19 Non-rectangular Geometry

The efficiency of FDS is due to the simplicity of its numerical grid. However, there are situations in which

certain geometric features do not conform to the rectangular grid. In these cases, construct the curved

geometry using rectangular obstructions, a process sometimes called “stair stepping”. A concern is that the

stair stepping changes the flow pattern near the wall. To lessen the impact of stair stepping on the flow field

near the wall, prescribe the parameter

SAWTOOTH=.FALSE.

on each OBST line that makes up the stair stepped obstruction. The effect of this parameter is to prevent

vorticity from being generated at sharp corners, in effect smoothing out the jagged steps that make up the

obstruction. This is not a complete solution of the problem, but it does provide a simple way of ensuring that

the flow field around a non-rectangular obstruction is not inhibited by extra drag created at sharp corners.

5.20 Texture Mapping

There are various ways of prescribing the color of various objects within the computational domain, but

there is also a way of pasting images onto the obstructions for the purpose of making the Smokeview images

more realistic. This technique is known as “texture mapping.” For example, to apply a wood paneling image

to a wall, add to the SURF line defining the physical properties of the paneling the text

&SURF ID=’wood paneling’,...,TEXTURE_MAP=’paneling.jpg’,TEXTURE_WIDTH=1.,

TEXTURE_HEIGHT=2. /

Assuming that a JPEG file called paneling.jpg exists in the working directory, Smokeview should read it and

display the image wherever the paneling is used (SGI Users: use rgb files instead of jpg). Note that the image

does not appear when Smokeview is first invoked. It is an option controlled by the Show/Hide menu. The

parameters TEXTURE WIDTH and TEXTURE HEIGHT are the physical dimensions of the image. In this

case, the JPEG image is of a 1 m wide by 2 m high piece of paneling. Smokeview replicates the image as

often as necessary to make it appear that the paneling is applied where desired. Consider carefully how the

image repeats itself when applied in a scene. If the image has no obvious pattern, there is no problem with

the image being repeated. If the image has an obvious direction, the real triplet TEXTURE ORIGIN should

be added to the VENT or OBST line to which a texture map should be applied. For example,

64
&OBST XB=1.0,2.0,3.0,4.0,5.0,7.0,SURF_ID=’wood paneling’,

TEXTURE_ORIGIN=1.0,3.0,5.0 /

applies paneling to an obstruction whose dimensions are 1 m by 1 m by 2 m, such that the image of the

paneling is positioned at the point (1.0,3.0,5.0). The default value of TEXTURE ORIGIN is (0,0,0), and the

global default can be changed by added a TEXTURE ORIGIN statement to the MISC line.

65
66
Chapter 6

Conclusion

The equations and numerical algorithm described in this document form the core of an evolving fire model.

As research into specific fire-related phenomena continues, the relevant parts of the model can be improved.

Because the model was originally designed to analyze industrial scale fires, it can be used reliably when

the fire size is specified and the building is relatively large in relation to the fire. In these cases, the model

predicts flow velocities and temperatures to within 20 % of the experimental measurements. In cases where

the fire is large relative to the enclosure, the uncertainty of the model is greater due both to the lack of input

data for material properties and combustion chemistry and to greater numerical error in combustion and

radiation transport.

Any user of the numerical model must be aware of the assumptions and approximations being employed.

There are two issues to consider before embarking on calculations. First, for both real and simulated fires,

the growth of the fire is very sensitive to the thermal properties of the surrounding materials. Second,

even if all the material properties are known, the physical phenomena of interest may not be simulated due

to limitations in the model algorithms or numerical grid. Except for those few materials that have been

studied to date at NIST, the user must supply the thermal properties of the materials, and then validate the

performance of the model with experiments to ensure that the model has the necessary physics included.

Only then can the model be expected to predict the outcome of fire scenarios that are similar to those that

have actually been tested.

67
68
Bibliography

[1] K.B. McGrattan (editor). Fire Dynamics Simulator (Version 4), Technical Reference Guide. NIST

Special Publication 1018, National Institute of Standards and Technology, Gaithersburg, Maryland,

July 2004.

[2] G.P. Forney and K.B. McGrattan. User’s Guide for Smokeview Version 4. NIST Special Publication

1017, National Institute of Standards and Technology, Gaithersburg, Maryland, July 2004.

[3] W. Gropp, E. Lusk, and A. Skjellum. Using MPI – Portable Parallel Programming with the MessagePassing Interface. MIT Press, Cambridge, Massachusetts, 2 edition, 1999.

[4] C.M. Fleischmann and F.F. Chen. Radiant Ignition of Upholstered Furniture. In Proceedings of the

International Conference on Engineered Fire Protection Design, 2001. Society of Fire Protection

Engineers, Bethesda, Maryland.

[5] U.O. Koylu and G.M. Faeth. Carbon Monoxide and Soot Emissions from Liquid-Fueled Buoyant

Turbulent Diffusion Flames. Combustion and Flame, 87:61–76, 1991.

[6] T. Ma. Numerical Simulation of an Axi-symmetric Fire Plume: Accuracy and Limitations. Master’s

thesis, University of Maryland, 2001.

[7] S. Welsh and P. Rubini. Three-dimensional Simulation of a Fire-Resistance Furnace. In Fire Safety

Science – Proceedings of the Fifth International Symposium. International Association for Fire Safety

Science, 1997.

[8] Pamela P. Walatka and Pieter G. Buning. PLOT3D User’s Manual, version 3.5. NASA Technical

Memorandum 101067, NASA, 1989.

[9] R.C. Reid, J.M. Prausnitz, and B.E. Poling. Properties of Gases and Liquids. McGraw-Hill, Inc., New

York, 4th edition, 1987.

[10] G.W. Mulholland. SFPE Handbook of Fire Protection Engineering, chapter Smoke Production and

Properties. National Fire Protection Association, Quincy, Massachusetts, 3rd edition, 2002.

[11] Y.P. He, A. Fernando, and M.C. Luo. Determination of interface height from measured parameter

profile in enclosure fire experiment. Fire Safety Journal, 31:19–38, 1998.

69
70
Appendix A

Compiling the Source Code for FDS

This section describes how one should compile the FDS source code to run on a variety of different computer

platforms. If a compiled version of FDS exists for the machine on which the calculation is to be run and no

changes have been made to the original source code, there is no need to re-compile the code. For example,

the file fds4.exe is the compiled single processor program for a Windows-based PC; thus PC users do not

need a Fortran compiler and do not need to compile the source code. For machines for which an executable

has not been compiled, the user must compile the code. Fortran 90/95 and C compilers are needed for

compilation.

A.1 Serial Compilation

Table A.1 lists the files that make up the source code. The files with suffix “.f” contain fixed form Fortran

90 instructions conforming to the ANSI and ISO standards, with the exception of those instructions that

pass information between the C and Fortran routines. The source files should be compiled in the order in

which they are listed in Table A.1 because some routines are dependent on others. For Unix/Linux users,

Makefiles for various platforms have been provided that assist in the compilation. Compiler options differ

from platform to platform. Note the following:

• The source code consists mainly of fixed-format Fortran 90 statements organized into 13 files, plus an

extra file containing some additional C routines needed for output to Smokeview. All of the C code

is contained within the file called isob.c. All the other files have the suffix .f, indicating fixed-format

Fortran.

• Be aware that different compilers handle the names of C subroutines differently. Some compilers

append an underscore to the names of the C routines called by the Fortran code. If the compiler

produces an error involving the names of routines that are not recognized, check for compiler options

that prevent the compiler from adding the underscore to the subroutine names.

• The only non-standard Fortran used is a call to a routine called FLUSH. This routine forces the contents of a given output file buffer to be emptied, making it easier to check on the progress of a given

calculation. Most Fortran compilers accept this routine, but if a compiler complains, comment out the

line in mods.f containing the string CALL FLUSH(IUNIT).

• The only compiler option necessary, in addition to any needed to address the above issues, is for full

optimization (usually -O). Some compilers have a standard optimization level, plus various degrees

of “aggressive” optimization. Be cautious in using the highest levels of optimization.

71
• Table A.2 lists some command and options for various different compilers and/or operating systems.

Consult the compiler manual, help/man pages for more details and options. Report any problems if

these options do not work.

• For the single processor version of FDS, use main.f

• The parallel version of FDS uses main mpi.f instead of main.f, plus additional MPI libraries need to

be installed. See next section for more details about parallel compilation.

Table A.1: Source Code Files

File Name Description

mods.f Global arrays and constants

misc.f Miscellaneous routines

pois.f Poisson (pressure) solver

radi.f Radiation solver

sprk.f Lagrangian particle transport and sprinkler activation

read.f Read input parameters

init.f Initialize variables and Poisson solver

divg.f Compute the flow divergence

pres.f Spatial discretization of pressure (Poisson) equation

mass.f Mass equation(s) and thermal boundary conditions

velo.f Momentum equations

dump.f Dumps output data into files

isob.c C Routine for computing isosurface triangles

main.f, main mpi.f Main programs, serial and parallel versions

Table A.2: Commands and options for various Fortran and C compilers

Compiler Fortran Command and Options C Command and Options

Lahey/Fujitsu lf95 -O –staticlink gcc -O

SGI/IRIX f90 -O3 -OPT:Olimit=0 cc -O2 -n32 -mips4

IBM/AIX xlf95 -O5 -qfixed=72 xlc -O

Intel Fortran ifc -O3 -xiW -ip -Vaxlib gcc -O -Dpp noappend

HPUX f90 -O3 cc -O -DHPUX NOAPPEND

Sun f90/f95 -O2 cc -O

DEC f90 -O5 -fast cc -O -Dpp noappend

Digital Visual Fortran See Section A.2 See Section A.2

72
A.2 Parallel Compilation using Windows and MPICH

Following is a set of very specific instructions for compiling and running the parallel version of FDS under

Microsoft Windows using a version of MPI known as MPICH, a product of Argonne National Laboratory

in the USA, and the Digital Visual Fortran (DVF) compiler. For those who do not have a Fortran compiler

of any kind, a pre-compiled executable file fds4 mpi.exe is available from the FDS/Smokeview web site.

In either case, all must follow the directions of installing MPICH and running the code. Those without a

compiler can skip steps 3 and 4 below.

1. Download the Windows version of MPICH from http://www-unix.mcs.anl.gov/mpi/mpich/download.html

2. Install MPICH for each machine. The SDK needs to be installed only on the machine used to compile

FDS.

3. (Only for those with DVF.) Create a new project for a Fortran Console application.

4. (Only for those with DVF.) Apply the following settings:

• Project ⇒Settings ⇒C/C++, Pre-processor Definitions, Add the phrase pp noappend

• Project ⇒Settings ⇒Link, Output, Stack Allocations 50000000

• Project ⇒Settings ⇒Link, General, add dfor.lib to the beginning of the list of objects

• (older versions of compiler) Project ⇒Settings ⇒Fortran; Libraries; Check ”Use Debug C Libraries”

• Project ⇒Settings ⇒Link Input, add C:\Program Files\MPICH\SDK\LIB to ’Additional Library Path’

• Project ⇒Settings ⇒Fortran Preprocessor, add C:\Program Files\MPICH\SDK\INCLUDE to

’INCLUDE AND USE PATHS’

• Project ⇒Settings ⇒Link Input, add ws2 32.lib and mpich.lib to list of objects/libraries.

• Under Project ⇒Settings ⇒Fortran External Procedures, set Argument Passing Conventions to

”C. By Reference”, and String Length Argument Passing to ”After All Args”. (equivalent to

/iface:cref /iface:nomixed str len arg)

• Import source files, inluding main mpi.f, but not main.f (this is for serial version)

• Build

5. Make sure that each machine can find the TCP/IP address of other machines by name. This can be ensured by adding the IP address-name combinations to the C:\Windows\system32\drivers\etc\hosts

file.

6. Parallel jobs are launched either using the graphical MPIRun interface, or by executing mpirun from

the command line. For easier use, add directory C:\Program Files\MPICH\mpd\bin to PATH. To do

this, under My Computer ⇒Properties ⇒Advanced ⇒Environment Variables, add the above directory

name to the Path list.

For command line use, the easiest way to define things for mpirun is to use a configuration file. Two

examples of the config.txt for a job containing three meshes are shown below.

A. fds4 mpi.exe is located in the same place on each computer, and both computers machine1 and

machine2 can see the current directory. Here we are using 2 processors on machine1 (or two threads

if machine1 only has one processor), and 1 processor on machine2.

73
exe C:\nist\fds\fds4_mpi.exe

hosts

machine1 2

machine2 1

B. fds4 mpi.exe can be found on the servermachine, and the working directory \fds\test is on a

shared drive of machine1.

exe \\servermachine\nist\fds\fds4_mpi.exe

dir \\machine1\fds\Test

hosts

machine1 2

machine2 1

To start the simulation, type ’mpirun config.txt’ on the command line. Remember that the input file

name should be written into a file called fds.data See MPICH documentation for additional information.

Note: Make sure the working directory is fully ”shared” since all computers have to write files into it.

This is often the biggest impediment to parallel processing – one must make the connection between

machines as transparent as possible. Have the same username and password on all machines. Check

that all machines can ”see” each other. And be patient. Even experienced computer users are going to

have problems at first ensuring that everything has been set up properly.

74
Appendix B

Alphabetical List of Input Parameters

This section lists the input parameters for FDS as a function of Namelist group, in alphabetical order. It

should only be used as a quick reference. Do not use this list before reading the detailed description of the

parameters. The reason is that many of the listed parameters are mutually exclusive – specifying more than

one can cause the program to either fail or run in an unpredictable manner. Also, some of the parameters

trigger the code to work in a certain mode when specified. For example, specifying the thermal conductivity of a solid surface triggers the code to assume the material to be thermally-thick, mandating that other

properties be specified as well. Simply prescribing as many properties as possible from a handbook is bad

practice. Only prescribe those parameters that are necessary to describe the desired scenario.

BNDF (Boundary File Parameters)

DTSAM Real Time increment s TWFIN/NFRAMES

QUANTITY Character Quantity to visualize

GRID (Grid Parameters)

IBAR Integer No. cells in x direction 10

JBAR Integer No. cells in y direction 10

KBAR Integer No. cells in z direction 10

HEAD (Header Material)

CHID Character Job Identification String ’output’

TITLE Character Title for job

75
HEAT (Heat Detectors)

ACTIVATION TEMPERATURE Real Link temperature ◦C 74

LABEL Character Descriptor

RTI Real Response Time Index √m s 100

XYZ Real Triplet Coordinates m

HOLE (Obstruction Cutout Parameters)

HEAT CREATE Character Name of HEAT detector to create

HEAT REMOVE Character Name of HEAT detector to remove

RGB Real Triplet Color indices for obstruction(s) to be cut

T CREATE Real Time to Create Hole s 0

T REMOVE Real Time to Remove Hole s 1000000

XB Real Sextuplet Physical coordinates m

INIT (Initial Conditions)

QUANTITY Character Parameter to initialize

VALUE Real Initial value

XB Real Sextuplet Coordinates m

ISOF (Isosurface Parameters)

DTSAM Real Time increment s TWFIN/NFRAMES

QUANTITY Character Quantity to visualize

VALUE Real Contour value

76
MISC (Miscellaneous Parameters)

BACKGROUND SPECIES Character Background species

BAROCLINIC Logical Baroclinic torque correction .FALSE.

CSMAG Real Smagorinsky constant 0.20

DATABASE Character Name of Database file

DATABASE DIRECTORY Character Name of Database directory

DENSITY Real Density of background liquid kg/m3

DNS Logical Direct Numerical Simulation .FALSE.

DT0DZ Real Atmospheric temperature lapse rate ◦C/m -0.0097

DTCORE Real Time between core dumps s

DTPAR Real Time between particle inserts s 0.05

DTSPAR Real Time between sprinkler droplets s 0.05

GVEC Real triplet Gravity vector m/s2 0,0,-9.81

ISOTHERMAL Logical Isothermal calculation .FALSE.

INCOMPRESSIBLE Logical Incompressible calculation .FALSE.

NFRAMES Integer Number of Frames of output data 1000

PR Real Prandtl number (LES only) 0.5

PINF Real Ambient pressure Pa 101325

POROUS FLOOR Logical Droplets disappear at floor .TRUE.

RADIATION Logical Radiation calculation flag .TRUE.

REACTION Character Combustion reaction identifier

RESTART Logical Restart previous calculation .FALSE.

SC Real Schmidt number (LES only) 0.5

SMOKE3D Logical Flag for 3D Smoke Visualization .TRUE.

SUPPRESSION Logical Suppression calculation flag .TRUE.

SURF DEFAULT Character Default SURFace type ’INERT’

TEXTURE ORIGIN Char. Triplet Origin of Texture Map m

TMPA Real Ambient Temperature ◦C 20.

TMPO Real Outside Temperature ◦C 20.

U0,V0,W0 Reals Prevailing velocity field m/s 0.

77
OBST (Obstruction Parameters)

BNDF BLOCK Logical Draw Boundary Info .TRUE.

HEAT CREATE Character Name of Controlling Heat Detector

HEAT REMOVE Character Name of Controlling Heat Detector

COLOR Character Color

OUTLINE Logical Draw as Outline .FALSE.

PERMIT HOLE Logical Allow a Hole .TRUE.

RGB Real Triplet Color indices

SAWTOOTH Logical Smooth Obstruction .FALSE.

SURF ID Character Associated Surface

SURF IDS Character Triplet Associated Surfaces (top-side-bottom)

SURF ID6 Character Sextuplet Associated Surfaces (like XB

T CREATE Real Time to Create Obstruction s

T REMOVE Real Time to Remove Obstruction s

TEXTURE ORIGIN Real Triplet Coordinates of Texture Map

THICKEN Logical No Thin Obstructions .FALSE.

XB Real Sextuplet Physical coordinates m

PART (Lagrangian Particles/Droplets)

AGE Real Droplet lifetime s 100000

DENSITY Real Droplet density kg/m3 1000

DIAMETER Real Median Volumetric Diameter μm 100

DROPLETS PER SECOND Integer Drops per second per head 1000

FUEL Logical Liquid Fuel .FALSE.

GAMMA D Real Parameter for size distribution 2.4

HEAT OF COMBUSTION Real Heat of Combustion kJ/kg

HEAT OF VAPORIZATION Real Latent Heat of Vap kJ/kg 2259

ID Character Identifier

INITIAL TEMPERATURE Real Initial Temperature ◦C TMPA

MASSLESS Logical Massless tracers .FALSE.

MASS PER VOLUME Real Droplet mass per unit volume kg/m3 1

MELTING TEMPERATURE Real Melting Temperature ◦C 0

NUMBER INITIAL DROPLETS Integer Number of droplets at start 0

QUANTITY Character Quantity for coloring

SAMPLING FACTOR Integer Filter for output file 1

SPECIFIC HEAT Real Droplet specific heat kJ/kg/K 4.184

STATIC Logical Stationary Particles .FALSE.

VAPORIZATION TEMPERATURE Real Liquid Droplet Boiling Temp ◦C 100

WATER Logical Water Droplet .FALSE.

78
PDIM (Physical Dimensions)

XBAR0, XBAR Real Limits of x coordinate m

YBAR0, YBAR Real Limits of y coordinate m

ZBAR0, ZBAR Real Limits of z coordinate m

RBAR0, RBAR Real Limits of r (cylindrical coordinates) m

PIPE (Sprinkler Pipe Parameters)

DELAY Real Time delay after first activation s 0

PRESSURE Real Pressure in sprinkler pipe bar

PL3D (Plot3D Parameters)

DTSAM Real Time increment s TWFIN/5

QUANTITIES Character Quintuplet Name of Quantities to save

WRITE XYZ Logical Write Coordinate File .FALSE.

RADI (Radiation Parameters)

ANGLE INCREMENT Integer Number of angles skipped per update 5

CH4 BANDS Logical Include extra fuel bands .FALSE.

KAPPA0 Real Constant absorption coefficient 1/m 0

NMIEANG Integer Number of polar angles 15

NUMBER RADIATION ANGLES Integer Number of solid angles 100

PATH Real Path length for radiation calc. m

RADTMP Real Assumed radiative source temp. ◦C 900

TIME STEP INCREMENT Integer Number time steps skipped 3

WIDE BAND MODEL Logical Non-gray gas assumption .FALSE.

RAMP (Ramping Parameters)

F Real Function value

ID Character Identifier

T Real Time (or Temperature) s (or ◦C)

79
REAC (Reaction Parameters)

BOF Real Pre-exponential Factor cm3/mol/s

DELTAH Real Heat of Combustion kJ/kg

E Real Activation Energy kJ/kmol

EPUMO2 Real Energy per Unit Mass O2 kJ/kg

FUEL Character Name of Fuel

FUEL N2 Real Number of N2 molecules in fuel 0

ID Character Identifier

MASS EXTINCTION COEFFICIENT Real Visibility Parameter m2/kg 7600

MAXIMUM VISIBILITY Real Visibility Parameter m 30

MW FUEL Real Molecular Weight of Fuel g/mol 44

NU CO2 Real Stoich. Coefficient for CO2 3

NU FUEL Real Stoich. Coefficient for Fuel 1

NU H2O Real Stoich. Coefficient for Water 4

NU O2 Real Stoich. Coefficient for Oxygen 5

RADIATIVE FRACTION Real Radiative Loss Fraction 0.35

CO YIELD Real Fraction of CO from fuel

SOOT YIELD Real Fraction of soot from fuel 0.01

VISIBILITY FACTOR Real Visibility Parameter 3

XNO, XNF Real Arrhenius Exponent

Y F INLET Real Mass Fraction of Fuel in Burner kg/kg 1.0

Y O2 INFTY Real Ambient Oxygen Mass Fraction kg/kg 0.23

SLCF (Slice File Parameters)

CB Character Plane to save slice file

DTSAM Real Time increment s TWFIN/5

K HIGH Integer Upper K value for LAYER HEIGHT KBAR

K LOW Integer Lower K value for LAYER HEIGHT 1

MESH NUMBER Integer Save only slices in this mesh

PBX Real x-plane to save slice file

PBY Real y-plane to save slice file

PBZ Real z-plane to save slice file

QUANTITY Character Name of Quantity to save

VECTOR Logical Include flow vectors .FALSE.

WRITE XYZ Logical Write Coordinate File .FALSE.

XB Real Sextuplet Coordinates of region to save m

80
SPEC (Species Parameters)

DENSITY Real Density of Liquid Species kg/m3

DIFFUSION COEFFICIENT Real Diffusivity D m2/s

EPSILONKLJ Real Leonard-Jones Parameter 0

ID Character Name of species

MASS FRACTION 0 Real Initial mass fraction 0

MW Real Molecular Weight g/mol 29

NU Real Stoich. coefficient

SIGMALJ Real Leonard-Jones Parameter 0

THERMAL CONDUCTIVITY Real Conductivity k W/m/K

VISCOSITY Real Dynamic Viscosity mu kg/m/s

SPRK (Sprinkler Parameters)

LABEL Character Identifying Label for output

MAKE Character Name of sprinkler (.spk) file

ORIENTATION Real Triplet Direction vector 0,0,-1

PART ID Character Name of associated PART line

ROTATION Real Triplet Rotation Angle deg 0

T ACTIVATE Real User-prescribed Activation s

T DEACTIVATE Real User-prescribed De-Activation s

XYZ Real Triplet Physical coordinates m

81
SURF (Surface Properties)

ADIABATIC Logical Adiabatic thermal BC .FALSE.

A Real Pre-exponential factor m/s 6.5E5

BACKING Character Back face boundary condition ’VOID’

BURN AWAY Logical Remove burnt objects .FALSE.

BURNING RATE MAX Real Maximum Burning Rate kg/m2/s 0.1

C DELTA RHO Real Specific heat x thickness x density m

C P Real Specific heat kJ/kg/K

C P CHAR Real Specific heat of char kJ/kg/K 0.7

DELTA Real Wall thickness m 0.1

DENSITY Real Solid mass per unit volume kg/m3 450.

E Real Activation energy kJ/kmol

E COEFFICIENT Real Extinguishing coefficient 1/s 0.

EMISSIVITY Real Emissivity 1.

FUEL FRACTION Real Mass concentration of fuel kg/kg 1.

HEAT FLUX Real Heat flux at surface kW/m2 0.

HEAT OF COMBUSTION Real Heat of combustion kJ/kg

HEAT OF VAPORIZATION Real Heat of vaporization kJ/kg

HRRPUA Real Heat Release Rate Per Unit Area kW/m2 0.

HRRPUA MAX Real Maximum HRRPUA kW/m2

ID Character Surface IDentifier

KS Real Thermal conductivity W/m/K

KS CHAR Real Thermal conductivity of char W/m/K 0.1

LEAKING Logical Leakage calculation .FALSE.

MASS FLUX(I) Real Array Mass flux of species I

MASS FLUX CRITICAL Real Mass flux at TMPIGN 0.02

MASS FRACTION(I) Real Array Mass fraction of species I

MOISTURE FRACTION Real Water content by mass kg/kg 0.

NPPC Integer Number of particles per cell 1

PART ID Character Lagrangian Particle ID

PHASE Character Phase of boundary ’SOLID’

POROSITY Real Porosity fraction 0.

PLE Real Atmospheric profile exponent 0.3

PROFILE Character Name of velocity profile

RAMP C P Character Ramp ID for specific heat

RAMP C P CHAR Character Ramp ID for char specific heat

RAMP KS Character Ramp ID for conductivity

RAMP KS CHAR Character Ramp ID for char conductivity

RAMP MF(I) Character Ramp ID for species I

RAMP Q Character Ramp ID for HRR

RAMP V Character Ramp ID for velocity

82
SURF (Surface Properties, continued)

RGB Real Triplet Color indices for surface 1.0,0.8,0.4

SURFACE DENSITY Real Density × Thickness kg/m2

TAU MF(I) Real Array Ramp-up time for species I s 1.

TAU Q Real Ramp-up time for HRR s 1.

TAU V Real Ramp-up time for velocity s 1.

TEXTURE HEIGHT Real Height of texture image m 1.

TEXTURE MAP Character Name of texture map file

TEXTURE WIDTH Real Width of texture image m 1.

TMPIGN Real Ignition temperature ◦C 5000.

TMPWAL Real Surface temperature ◦C 20.

TMPWAL0 Real Initial solid temperature ◦C 20.

VBC Real Velocity Slip Index 0.5

VEL Real Normal velocity m/s 0.

VEL T Real Pair Tangential velocity components m/s 0.

VOLUME FLUX Real Normal velocity x vent area m3/s 0.

WALL POINTS Integer Internal wall points 20

Z0 Real Atmospheric profile origin m 10.

THCP (Thermocouples and Point Measurements)

DEPTH Real Depth into surface for internal wall temp. m 0

DIAMETER Real Diameter of Thermocouple Bead m 0.001

DTSAM Real Time increment s TWFIN/NFRAMES

EMISSIVITY Real Emissivity of Thermocouple Bead 0.85

IOR Integer Orientation Parameter

K HIGH Integer Upper K value for LAYER HEIGHT KBAR

K LOW Integer Lower K value for LAYER HEIGHT 1

LABEL Character Identifier for output

QUANTITY Character Name of Quantity to save

XB Real Sextuplet Coordinates of non-point measurement m

XYZ Real Triplet Coordinates of point measurement m

TIME (Time Parameters)

DT Real Initial time step s

TWFIN Real Time When FINished s 1.

TRNX, TRNY, TRNZ (Transformation Parameters)

CC Real Computational coordinate m

IDERIV Integer Order of polynomial transformation

MESH NUMBER Integer Number of mesh to transform

PC Real Physical coordinate or derivative

83
VENT (Vent Parameters)

CB Character Coordinate Plane

HEAT ACTIVATE Character Name of Controlling Heat Detector

HEAT CLOSE Character Name of Controlling Heat Detector

HEAT DEACTIVATE Character Name of Controlling Heat Detector

HEAT OPEN Character Name of Controlling Heat Detector

OUTLINE Logical Draw vent as outline .FALSE.

PBX, PBY, PBZ Real Coordinate Plane

RGB Real Triplet Color indices

SURF ID Character Associated Surface

T ACTIVATE Real Same as T OPEN s

T CLOSE Real Time to Close or De-activate Vent s

T DEACTIVATE Real Same as T CLOSE s

T OPEN Real Time to Open or Activate Vent s

TEXTURE ORIGIN Real Triplet Coordinates of Texture Map

COLOR Character Color

XB Real Sextuplet Physical coordinates m

84
Appendix C

Output File Formats

The output from the code consists of the file CHID.out, plus various data files that are described below.

Most of these output files are written out by the routine dump.f, and can easily be modified to accommodate

various plotting packages.

C.1 Diagnostic Output

The file CHID.out consists of a list of the input parameters, and an accounting of various important quantities, including CPU usage. Typically, diagnostic information is printed out every 100 time steps

.

.

Iteration 8300 May 16, 2003 08:37:53

----------------------------------------------

Mesh 1, Cycle 3427

CPU/step: 2.272 s, Total CPU: 2.15 hr

Time step: 0.03373 s, Total time: 128.86 s

Max CFL number: 0.86E+00 at ( 21, 9, 80)

Max divergence: 0.24E+01 at ( 25, 30, 22)

Min divergence: -.39E+01 at ( 26, 18, 31)

Number of Sprinkler Droplets: 615

Total Heat Release Rate: 7560.777 kW

Radiation Loss to Boundaries: 6776.244 kW

Mesh 2, Cycle 2914

CPU/step: 1.887 s, Total CPU: 1.53 hr

Time step: 0.03045 s, Total time: 128.87 s

Max CFL number: 0.96E+00 at ( 21, 29, 42)

Max divergence: 0.20E+01 at ( 22, 20, 22)

Min divergence: -.60E+01 at ( 7, 26, 48)

Number of Sprinkler Droplets: 301

.

.

85
The Iteration number indicates how many time steps the code has run, whereas the Cycle number for a

given mesh indicates how many time steps have been taken on that mesh. The date and time (wall clock

time) are on the line starting with the word Iteration. The quantity CPU/step is the amount of CPU

time required to complete a time step for that mesh; Total CPU is the amount of CPU time elapsed

since the start of the run; Time step is the time step size for the given mesh; Total time is the time

of the simulation; Max/Min divergence is the max/min value of the function ∇ · u and is used as a

diagnostic when the flow is incompressible (i.e. no heating); and Max CFL number is the maximum

value of the CFL number. The Radiation Loss to Boundaries is the amount of energy that is

being radiated to the boundaries. As compartments heat up, the energy lost to the boundaries can grow

to be an appreciable fraction of the Total Heat Release Rate. Often, a quantity called the Fire

Resolution Index appears. This is an indicator of how well resolved the calculation is – it is the

fraction of the ideal stoichiometric value of the mixture fraction that is being used in the calculation. Finally,

Number of Tracer Particles indicates how many passive particles are being tracked at that time.

Following the completion of a successful run, a summary of the CPU usage per subroutine is listed.

This is useful in determining where most of the computational effort is being placed.

C.2 Plot3D Data

Presently, field data is output every DTSAM seconds in a format used by the graphics package Plot3D. The

Plot3D data sets are single precision (32 bit reals), whole and unformatted. Note that there is blanking, that

is, blocked out data points are not plotted. If the statement WRITE XYZ=.TRUE. is included on the PL3D

line, then the grid data is written out to a file called CHID.xyz

WRITE(LU13) IBAR+1,JBAR+1,KBAR+1

WRITE(LU13) (((X(I),I=0,IBAR),J=0,JBAR),K=0,KBAR),

. (((Y(J),I=0,IBAR),J=0,JBAR),K=0,KBAR),

. (((Z(K),I=0,IBAR),J=0,JBAR),K=0,KBAR),

. (((IBLK(I,J,K),I=0,IBAR),J=0,JBAR),K=0,KBAR)

where X, Y and Z are the coordinates of the cell corners, and IBLK is an indicator of whether or not the cell

is blocked. If the point (X,Y,Z) is completely embedded within a solid region, then IBLK is 0. Otherwise,

IBLK is 1. Normally, the grid file is not dumped.

The flow variables are written to a file called CHID **** **.q, where the stars indicate a time at which

the data is output. The file is written with the lines

WRITE(LU14) IBAR+1,JBAR+1,KBAR+1

WRITE(LU14) ZERO,ZERO,ZERO,ZERO

WRITE(LU14) ((((QQ(I,J,K,N),I=0,IBAR),J=0,JBAR),K=0,KBAR),N=1,5)

The five channels N=1,5 are by default the temperature (◦C), the u, v and w components of the velocity

(m/s), and the heat release rate per unit volume (kW/m3). Alternate variables can be specified with the input

parameter QUANTITIES under the PL3D namelist group. Note that the data is interpolated at cell corners,

thus the dimensions of the Plot3D data sets are one larger than the dimensions of the computational grid.

Smokeview can display the Plot3D data. In addition, the Plot3D data sets can be read into some other

graphics programs that accept the data format. This particular format is very convenient, and recognized by

a number of graphics packages, including AVS, IRIS Explorer and Tecplot 1.

1With the exception of Smokeview, the graphics packages referred to in this document are not included with the source code,

but are commercially available.

86
C.3 Thermocouple Data

Temperature (or other scalar quantity) data at discrete points specified in the input file under the namelist

group THCP is output in comma delimited format in a file called CHID tc.csv. The format of the file is as

follows

NTC

TIME , LABEL(1) , LABEL(2) , ... , LABEL(NTC)

TIME , QUANTITY(1) , QUANTITY(2) , ... , QUANTITY(NTC)

s , UNITS(1) , UNITS(2) , ... , UNITS(NTC)

T(1) , TC(1,1) , TC(2,1) , ... , TC(NTC,1)

T(2) , TC(1,2) , TC(2,2) , ... , TC(NTC,2)

.

.

.

where NTC is the number of thermocouples, LABEL(I) is the user-defined label of the Ith thermocouple,

QUANTITY(I) is the physical quantity represented, UNITS(I) the units, T(J) the time of the Jth dump,

and TC(I,J) the value at the Ith thermocouple at the Jth time. The files can be imported into Microsoft

Excel or almost any other spread sheet program.

C.4 Sprinkler Data

If sprinklers are prescribed in the calculation, then a file called CHID spk.csv is generated. The file lists

the temperature of each sprinkler link. The format of the file is

NSPR

TIME , TEMP , TEMP , ... , TEMP

s , C , C , ... , C

T(1) , TL(1,1) , TL(2,1) , ... , TL(NSPR,1)

T(2) , TL(1,2) , TL(2,2) , ... , TL(NSPR,2)

.

.

.

where NSPR is the number of sprinklers, T(J) is the time of the Jth dump, TL(I,J) is the link temperature

of the Ith sprinkler at the Jth time. The data is ordered the same way as the sprinklers are listed in the input

file.

C.5 Heat Release Rate

Quantities associated with the overall energy budget are reported in the comma delimited file CHID hrr.csv.

The file consists of six columns. The first column contains the time in seconds. The second through fifth

columns contain integrated energy gains and losses, all in units of kW. The second column contains the

total heat release rate, the third contains the radiative heat loss to all the boundaries (solid and open), the

fourth contains the convective and radiative heat loss to the boundaries (i.e. the energy flowing out of the

domain), and the fifth contains the energy conducted into the solid surfaces. The sixth column contains the

total burning rate of fuel, in units of kg/s.

87
The radiative loss to the boundaries can be interpreted as either a volume or boundary integral

Q ̇

r =

Z

∇·qr dV =

Z

qr· dS =

Z

q ̇

00

r dA (C.1)

It represents the energy radiating away from the fire and hot gases into the solid boundaries or out of the

computational domain. The convective loss is the boundary integral

Q ̇

conv =

Z

cp ρ (T −T∞) u· dS (C.2)

where the integral is positive if the flow is out of the domain. The conductive loss to the solid surface is

given by

Q ̇

cond =

Z

q ̇

00

r +q ̇

00

c dA (C.3)

where the integral is positive if heat is being lost into a wall colder than the gas. See the Technical Reference

Guide for more details.

C.6 Gas Mass Data

The total mass of the various gas species at any instant in time is reported in the comma delimited file

CHID mass.csv. The file consists of several columns, the first column containing the time in seconds, the

second contains the total mass of all the gas species in the computational domain in units of kg, the next

lines contain the total mass of the individual species.

C.7 Mixture Fraction State Relations

The functional dependence of the mass fraction of the reactants and products of combustion on the mixture

fraction is reported in the comma delimited file CHID state.csv. The file consists of nominally 10 columns,

the first column containing the mixture fraction, the rest the mass fractions of the various gases.

C.8 Slice Files

The slice files defined under the namelist group SLCF are named CHID n.sf (n=01,02...), and are written

out unformatted, unless otherwise directed. These files are written out from dump.f with the following

lines:

WRITE(LUSF) QUANTITY

WRITE(LUSF) SHORT_NAME

WRITE(LUSF) UNITS

WRITE(LUSF) I1,I2,J1,J2,K1,K2

WRITE(LUSF) TIME

WRITE(LUSF) (((QQ(I,J,K),I=11,I2),J=J1,J2),K=K1,K2)

.

.

.

WRITE(LUSF) TIME

WRITE(LUSF) (((QQ(I,J,K),I=11,I2),J=J1,J2),K=K1,K2)

88
QUANTITY, SHORT NAME and UNITS are character strings of length 30. The sextuplet (I1,I2,J1,J2,K1,K2)

denotes the bounding grid cell nodes. The sextuplet indices correspond to grid cell nodes, or corners, thus

the entire grid would be represented by the sextuplet (0,IBAR,0,JBAR,0,KBAR).

There is a short Fortran 90 program provided, called fds2ascii.f, that can convert slice files into text files

that can be read into a variety of graphics packages. The program combines multiple slice files corresponding to the same “slice” of the computational domain, time-averages the data, and writes the values into one

file, consisting of a line of numbers for each node. Each line contains the physical coordinates of the node,

and the time-averaged quantities corresponding to that node. In particular, the graphics package Tecplot

reads this file and produces contour, streamline and/or vector plots. See Section 4.7.6 for more details about

the program fds2ascii.

C.9 Boundary Files

The boundary files defined under the namelist group BNDF are named CHID n.bf (n=01,02...), and are

written out unformatted. These files are written out from dump.f with the following lines:

WRITE(LUBF) QUANTITY

WRITE(LUBF) SHORT_NAME

WRITE(LUBF) UNITS

WRITE(LUBF) NPATCH

WRITE(LUBF) I1,I2,J1,J2,K1,K2,IOR

WRITE(LUBF) I1,I2,J1,J2,K1,K2,IOR

.

.

.

WRITE(LUBF) TIME

WRITE(LUBF) (((QQ(I,J,K),I=11,I2),J=J1,J2),K=K1,K2)

WRITE(LUBF) (((QQ(I,J,K),I=11,I2),J=J1,J2),K=K1,K2)

.

.

.

WRITE(LUBF) TIME

WRITE(LUBF) (((QQ(I,J,K),I=11,I2),J=J1,J2),K=K1,K2)

WRITE(LUBF) (((QQ(I,J,K),I=11,I2),J=J1,J2),K=K1,K2)

.

.

.

QUANTITY, SHORT NAME and UNITS are character strings of length 30. NPATCH is the number of planes

(or “patches”) that make up the solid boundaries plus the external walls. The sextuplet (I1,I2,J1,J2,K1,K2)

defines the cell nodes of each patch. IOR is an integer indicating the orientation of the patch (±1,±2,±3).

The user does not prescribe these. Note that the data is planar, thus one pair of cell nodes is the same.

Presently, Smokeview is the only program available to view the boundary files.

C.10 Particle Data

The tracer particles and sprinkler droplets are animated using a file called CHID.part. It contains the

particle positions. There is a one line header followed by particle locations output every DTSAM seconds.

89
The structure of the data file is given in the file dump.f by a subroutine called PDMP3D.

WRITE(LU10) ARX,ARY,DTSAM,IPART,NPPS

WRITE(LU10) IBAR,JBAR,KBAR

WRITE(LU10) (X(I),I=0,IBAR),(Y(J),J=0,JBAR),(Z(K),K=0,KBAR)

WRITE(LU10) NB

DO N=1,NB

WRITE(LU10) IB1(N),IB2(N),JB1(N),JB2(N),KB1(N),KB2(N),1

END DO

WRITE(LU10) NV

DO N=1,NV

WRITE(LU10) IV1(N),IV2(N),JV1(N),JV2(N),KV1(N),KV2(N),2

END DO

WRITE(LU10) NSPR

DO N=1,NSPR

WRITE(LU10) XSP0(N),YSP0(N),ZSP0(N)

END DO

where ARX=ZBAR/XBAR and ARY=ZBAR/YBAR are the aspect ratios of the overall domain, IPART is

the index of the scalar quantity associated with the particles, NPPS is the maximum number of particles per

frame, IB1, IB2, etc. are the indices of blocked grid cells, IV1, IV2, etc. indicate vent cell nodes, and

XSP0, YSP0, ZSP0 are the coordinates of the sprinklers. The arrays X(I), Y(J), Z(K) contain

the coordinates of the grid. Every DTSAM seconds the coordinates of the tracer particles and sprinkler

droplets are output

WRITE(LU10) TIME,NP,NN,(ISPR(N),N=1,NSPR)

WRITE(LU10) (XP(I),I=1,NP),

. (YP(I),I=1,NP),

. (ZP(I),I=1,NP),

. (BP(I),I=1,NP)

IF (NASPR.GT.0) THEN

WRITE(LU10) NSP

WRITE(LU10) (XSP(I),I=1,NSP),(YSP(I),I=1,NSP),(ZSP(I),I=1,NSP)

ENDIF

where NP is the number of tracer particles, NN is a dummy integer kept for compatibility reasons, ISPR

denotes whether the sprinkler has activated, NSPR is the number of sprinklers, XP, YP, ZP are the coordinates of the element, BP is a the quantity referenced by IPART, NASPR is the number of active sprinklers,

NSP is the number of sprinkler droplets, and XSP, YSP, ZSP are the droplet coordinates.

90