ANSYS FLUENT
ANSYS FLUENT is a finite volume program (CFD program) for the calculation of flow problems.

Services:
- CAE

License type:	Campus license
Licensed for:	Akademische Forschung und Lehre Geräte des KIT Mitarbeiter des KIT Studierende des KIT (auch auf privaten Geräten) siehe Lizenzbedingungen
Registrierung beim Hersteller:	Erforderlich für Zusatzfunktionen (z.B. Support)

Services provided by SCC:	Bedienungsberatung und Unterstützung beim Zugang zur Infrastruktur Bereitstellung Bereitstellung von Dokumentation Beschaffung, Lizenz- und Vertragsmanagement Betrieb und Pflege der Lizenzserver Fachliche Beratung zur Nutzung Installationsunterstützung Schnittstelle zum Hersteller-Support Unterstützung bei Nutzung auf HPC-Systemen
Provisioning:	FTP-Server HPC-Systems SCC-Pools

FLUENT Quick Start Guide

Introduction
FLUENT System
FLUENTFiles
FLUENTcall
FLUENTcall on the Linux clusters of the SCC
Creating a FLUENT command file
User Defined Functions (UDF) in FLUENT

Introduction

FLUENT is a finite volume program for the calculation of flow problems. The problems that can be treated can be paraphrased as follows:

isothermal: the energy equation is not solved
non-isothermal: the energy equation is solved
compressible and non-compressible fluids
laminar and turbulent flows
steady and unsteady flows
Newtonian and non-Newtonian fluids
multiphase flows (fluid-fluid, fluid-solid)
coupled heat conduction and convection
moving grids
free surfaces
chemical reactions, combustion processes

For a more intensive description, please refer to the FLUENT documentation.

FLUENT System

FLUENT can be used as a standalone application, but also as an integral module within ANSYS Workbench. In this quick guide we focus on the first aspect. The following graphic outlines the workflow of a FLUENT project:

HyperMesh is a modeler and mesher that can create or import the most important solver formats. In addition, GAMBIT and TGrid can be used to create FLUENT meshes until further notice. Information about this can be found here. There are other "Third Party" systems, but we limit ourselves here to the conditions at the SCC.

FLUENT Files

FLUENT works with the following files:


id.msh	is a file that contains the mesh information. It is generated within the Workbench or by ICEM_CFD, HyperMesh, GAMBIT and other preprocessors.
id.cas	is the extended mesh file containing further model information entered during a FLUENT session
id.dat	contains the calculation results, which must also be read in for post-processing
id.ps ....	various formats in which the graphics can be output, including PostScript, EPS, RGB, GIF, TIFF, PPM, TARGA, PICT, HPGL, Window Dump
.cxlayout	is a file in the HOME directory where the layout of the graphical user interface is stored. In later sessions of FLUENT, FLUENT/Post, TGRID this file is taken as a template. This file is created by Save Layout in the File menu.
bel. Name	During a FLUENT session a journal file and a transcript file can be created or a journal file can be read.

FLUENT call

The list of options when calling FLUENT is very long, most of them are not interesting or valid for us. So here are only those that are of importance to and:


fluent	[version]
	[-driverx11\|openglnull]
	[-i journalfile]
	[-g][-gu][-gr]

with the meaning


version 2d 3d 2ddp 3ddp	specifies the FLUENT version to be executed: two-dimensional problem three-dimensional problem two-dimensional problem, double-exact three-dimensional problem, double-exact
g	neither the graphical user interface is opened, nor graphical functions are executed
gu	the graphical user interface is not opened, pure command mode
gr	no graphics are generated
driver	sets the graphics driver; by default the OpenGL driver is set, but if it is not installed, the X11 driver is used
i	a journal file is read and executed

If neither the -g nor the -gu option is set, the FLUENT Launcher opens, where important default settings can be made:

If you click "Start With Selected Options", the actual FLUENT graphical user interface appears.

FLUENT call on the Linux clusters of the SCC

On the Linux cluster bwUniCluster a module concept is used. To use ANSYS, you must first load the appropriate module. You get all available software modules by calling

module avail

typing. To load the module of the current version of ANSYS, enter the following on the bwUniCluster:

module load cae/ansys

You can also load the module with the desired version number, e.g.

module load cae/ansys/2023R2

On the Linux clusters of the SCC, the execution of FLUENT should be under the control of a job management system that provides the computing resources for the FLUENT job. To simplify the use of FLUENT on these clusters, the startup script 'fluentjob' was provided. The call to the solver for the bwUniCluster is thus:

fluentjob -v version -j name -t cpu-time -m memory [-p procs][-n nodes][-q queue]

The meaning of the parameters is the following:

version	is the dimension/accuracy: 2d, 3d, 2ddp, 3ddp
name	command file, contains FLUENT commands for initialization and calling the solver
cpu-time	is the requested CPU time in minutes
memory	is the requested main memory in MByte
procs	number of processors
nodes	Number of nodes
queue	queue class / partition

An example to start a Fluent parallel job on two nodes and 40 processors with 90.000 MB memory for 120 minutes:

fluentjob -v 3d -j test -t 120 -n 2 -p 40 -m 90000

The call of FLUENT can also be done by script. Here below a script "run_fluent.sh", how to start a FLUENT computation in parallel on two nodes with 40 processors each on thebwUniCluster:

1. with IntelMPI:

#!/bin/sh
#SBATCH --nodes=2
#SBATCH --ntasks-per-node=40
#SBATCH --time=2:00:00
#SBATCH --mem=90gb
#SBATCH --partition=multiple
module load cae/ansys/2023R2
source fluentinit
scontrol show hostname ${SLURM_JOB_NODELIST} > fluent.hosts
time fluent 3d -mpi=intel -pib -g -t80 -cnf=fluent.hosts -i test.inp

2. with OpenMPI:

#!/bin/sh
#SBATCH --nodes=2
#SBATCH --ntasks-per-node=40
#SBATCH --time=2:00:00
#SBATCH --mem=90gb
#SBATCH --partition=multiple
module load cae/ansys/2023R2
source fluentinit
scontrol show hostname ${SLURM_JOB_NODELIST} > fluent.hosts
time fluent 3d -mpi=openmpi -g -t80 -cnf=fluent.hosts -i test.inp

To submit the script to the job management system, execute the following

sbatch run_fluent.sh

For more information about the batch system of the respective clusters, see these links:

bwUniCluster

Creating a FLUENT command file

The FLUENT window allows FLUENT input via mouse-driven menus, but one can also, although more tedious, input via keyboard in command mode. Input via commands must be made available in a file in the case of a batch run. The journal file can contribute to this, but it must also be a log file resulting from a session in command mode, otherwise information about the user interface is included.

The simplest procedure, which then leads to a standard command file, is the following:

One prepares the model completely, except for the initialization via the menus Solver -> Initialize... --> Initialize and Solver --> Iterate... --> I terate.
The reading of the .cas file, the initialization, the start of the solver and the writing out of the results are then initiated by the command file, which is read in the fluentjob.
Post-processing is then again done interactively.

Example:

The FLUENT model is called cavity.cas. The following commands are in the cavity.inp file


file/rc cavity.cas	the file cavity.cas is read in
solve/init	it is jumped to the Initialize submenu ofSolve
s-d	set defaults
x 1	initial velocity in x-direction is set to 1
q	Return
if	the program jumps to the Initialize ... submenu of Solve
q	return to
solve/iterate 10	jumps to the iterate submenu of Solve and performs 10 iterations
q	return to
file/wcd cavity.cas	in the file menu case and data files are stored
y
exit

A corresponding call would then be e.g.

fluentjob -v 2d -j cavity.inp -n 1 -p 10 -t 10 -m 40000

Information about the FLUENT commands can be found in the FLUENT Users Guide.

User Defined Functions (UDF) in FLUENT

In FLUENT it is possible to access the solver during the solution phase. This is done via C programs to be created by the user, which directly influence the solution process via standard interfaces, the DEFINE macros, using special data types. UDFs are available for

Boundary conditions: Profiles for velocities, temperature, turbulence, species.
sources: Masses, momentum, energy, turbulence, species
Material properties: viscosity, conductivity, density, etc.
Initial conditions
global functions
scalar functions
model specific functions: reaction rates, turbulent viscosity, discrete phase models.

A detailed description and examples can be found in the UDF manual.

UDFs can be integrated into a model in 2 ways, as interpreted UDF or compiled UDF.

Interpreted UDF	Compiled UDF
The UDF is read and executed line by line by an interpreter at runtime.	The UDF is compiled before the FLUENT job and bound with the FLUENT libraries.
Advantage: Platform independent, as no compiler is required.	Advantage: Fast, efficient, no functional limitations
Disadvantage: Slow and relatively large main memory requirements	Disadvantage: Dependent on operating system and third party compiler

Under the graphic surface the UDFs are merged over the menu sequence Define --> User-Defined --> Functions --> Compiled or Interpreted. They are "linked" into the model, depending upon type over the Define menu and then Boundary Conditions ... ,Cell Zone Conditions... , Materials ... etc. There is also a special menu Define --> User-Defined --> Function Hooks... which is used to hook functions and initial conditions. Again, a detailed description can be found in the UDF manual.

Afterwards the FLUENT model can be further prepared and the .cas file can be saved. When this .cas file is opened in subsequent FLUENT sessions, the UDFs are ready for use without further action. If a journal file was logged during preparation, it can again be used as the basis for a batch input file to start the FLUENT job on the Linux clusters of the SCC under fluentjob.

The procedure described above can also be done in command line format (see example below), so that an input file for fluentjob can be generated to run the whole thing in batch on the SCC clusters.

In the case of compiled UDFs, the translation and loading can also be done outside FLUENT. This has the advantage, especially in the development and testing of the UDF, that everything takes place at the operating system level, so it is faster. If the UDF is error-free and integrated in FLUENT, no UDF-specific input is required in the batch input file. Thus, this variant is the most flexible.

Example

The following example demonstrates what has been said above. It is described in detail in the UDF manual under the examples in chapter 8.2.4. It is a bent tube, one half of which along the axis consists of a porous material, in which a gas consisting of a species a and flowing in from the left is converted into a gas of species b according to a reaction rate. This reaction rate must be formulated as a UDF and is to be included in the model as a compiled UDF. The model is 2-dimensional.

The model is already available in the file rate.cas. The UDF rate.c looks like this

/******************************************************************/
/* */
/* Custom Reaction Rate */
/* RALF 5.0 */
/* */
/* Authors: Heather Andrews and Eric Bish */
/* Date: February 1998 */
/* */
/******************************************************************/

#include "udf.h"

#define K1 2.0e-2
#define K2 5.

DEFINE_VR_RATE(user_rate, cell, thread, r, mole_weight, species_mf, rate, rr_t)
{
float s1 = species_mf[0];
float mw1 = mole_weight[0];

if (FLUID_THREAD_P(thread) && THREAD_VAR(thread).fluid.porous)
*rate = K1*s1/pow((1.+K2*s1),2.0)/mw1;
else
*rate = 0.;
}

Interactive via graphical user interface

After calling FLUENT and reading rate.cas start Define --> User-Defined --> Compiled . ..

Via the Add... button you select rate.c and by default libudf is entered as name for the shared library to be created. With Build you start the Compile/Load process and with Load the just created shared library libudf is loaded into the model. The further procedure can be found in the UDF Manual Chap. 6.2.33 Hooking DEFINE_VR_RATE UDFs. Via Models --> Species --> Edit the following setting should have been done before and saved in rate.cas:

and via Define --> User-Defined --> Function Hooks ... you select the UDF user_rate, as the name was defined in rate.c.

Note that the shared library containing user_rate is also displayed. It remains to initialize and start the solver in the solver menu. One result, the proportion of species a, can be seen in the following contour plot:

Via command line

file/rc rate.cas
define/user-defined/compiled-functions/compile
libudf
yes
rate.c

define/user-defined/compiled-functions/load libudf
define/user-defined/function-hooks
volume-reaction-rate

q
solve/init
s-d
x 0.1
q
if
q
solve/iterate 50
q
file/wcd rate.cas
y
exit

Read in rate.cas
Compile rate.c and generate the
shared library libudf

Loading libudf
Function Hooks

Initialization of the solver

50 iterations

Saving of case and dat file

The empty lines correspond to the pressing of the return key. If the job is to be further calculated, e.g. further iterations, or with other initial conditions, the following is sufficient as input file

file/rc rate.cas
solve/init
s-d
x 0.1
q
if
q
solve/iterate 50
q
file/wcd rate.cas
y
exit

Compile/Load on Linux level

The following description refers to the SCC cluster. On the working directory, which is the directory where the case file rate.cas is located, the following directory structure is built and Makefiles are copied:

mkdir libudf
cd libudf
cp /software/all/ansys_inc13/v130/fluent/fluent13.0.0/src/makefile.udf2 Makefile
mkdir src
cd src
cp /software/all/ansys_inc13/v130/fluent/fluent13.0.0/src/makefile.udf makefile
cd ..
mkdir lnamd64
cd lnamd64

In the subdirectory lnamd64 (the name corresponds to the Linux architecture) subdirectories are now created, depending on dimensionality and precision, i.e. one of

2d 2dp 3d 3dp

and if parallelized computation is to be performed, also

2d_host and 2d_node

or

3d_host and 3d_node

Afterwards the UDF rate.c is copied to src and in makefile the two variables

SOURCE=rate.c
FLUENT_INC=/software/all/ansys_inc13/v130/fluent

are set. Then go to the subdirectory libudf and start

make "FLUENT_ARCH=lnamd64".

The UDF is compiled and the library libudf is created. Afterwards the directory structure looks like this:

The shared library libudf only has to be loaded and the function hooks have to be set up (see above).

ANSYS FLUENT

ANSYS FLUENT

License restrictions

Academic Usage

FLUENT Quick Start Guide

Table of Contents