BwUniCluster2.0/Software/OpenFoam

Description	Content
module load	cae/openfoam
Availability	bwUniCluster | BwForCluster_Chemistry | bwGRiD-Tübingen
License	GNU General Public Licence
Citing	n/a
Links	Openfoam Homepage | Documentation
Graphical Interface	No

Description

The OpenFOAM® (Open Field Operation and Manipulation) CFD Toolbox is a free, open source CFD software package with an extensive range of features to solve anything from complex fluid flows involving chemical reactions, turbulence and heat transfer, to solid dynamics and electromagnetics.

Versions and Availability

A list of versions currently available on all bwHPC-C5-Clusters can be obtained from the

Cluster Information System CIS

{{#widget:Iframe |url=https://cis-hpc.uni-konstanz.de/prod.cis/bwUniCluster/cae/openfoam |width=99% |height=600 |border=0 }}
In order to check what OpenFOAM versions are installed on the system, run the following command:

$ module avail cae/openfoam

Typically, several OpenFOAM versions might be available.
Any available version can be accessed by loading the appropriate module:

$ module load cae/openfoam/<version>

with <version> specifying the desired version.

To activate the OpenFOAM applications, after the module is loaded, run the following:

$ source $FOAM_INIT

or simply:

$ foamInit

Parallel run with OpenFOAM

To improve the concurrently solving process and decrease the error occurrence probability while running an OpenFOAM job in parallel (on a singlenode), some modifications have been introduced. Specifically, after the case decomposition is done, it is recommended to save the decomposed data directly on the nodes local folder and run from there. When the calculations are over, the data is moved back to the case folder and reconstructed. It will improve the overall performance, considering that you allocated enough wall-time to decompose and rebuild your cases, as it moves theprocessor*folders to and out of the nodes local work-space. For such a procedure it is necessary to use the following commands for decomposition and reconstruction of the geometry domain:

$ decomposeParHPC
$ reconstructParHPC
$ reconstructParMeshHPC

instead of:

$ decomposPar
$ reconstructPar
$ recontructParMesh

For example, if you want to runsnappyHexMeshin parallel, you may use the following commands:

$ decomposeParMeshHPC
$ mpiexec snappyHexMesh -overwrite
$ reconstructParMeshHPC -constant

instead of:

$ decomposePar
$ mpiexec snappyHexMesh -overwrite
$ reconstructParMesh -constant

Building an OpenFOAM batch file for parallel processing

General information

To run any job in a parallel mode with OpenFOAM, it is necessary to decompose the geometry domain into segments, equal to the number of processors (or threads) you intend to use. That means, for example, if you want to run a case on 8 processors, you will have to decompose the mesh in 8 segments, first. Then, you start the solver in parallel mode, letting OpenFOAM to run calculations concurrently on these segments, one processor responding for one segment of the mesh, sharing the data with all other processors in between. There is, of course, a mechanism that connects properly the calculations, so you don't loose your data or generate wrong results. Decomposition and segments building process is handled bydecomposeParutility. In "system/decomposeParDict" you may specify, how many "segments" you want your geometry domain to be divided in, and which decomposition method to use. The automatic one is "scotch". It trims the mesh, collecting as many cells as possible per processor, trying to avoid having empty segments or segments with few cells. If you want your mesh to be divided in other way, specifying the number of segments it should be cut in x, y or z direction, for example, you can use "simple" or "hierarchical" methods. There are some other ways as well, with more documentation on the internet.

Wrapper script generation

Attention: openfoam module loads automatically the necessary openmpi module for parallel run, do NOT load another version of mpi, as it may conflict with the loaded openfoam version.

A job-script to submit a batch job called job_openfoam.sh that runs icoFoam solver with OpenFoam version 2.4.0, on 8 processors, requiring 6000 MByte of total physical memory per processor and total wall clock time of 6 hours looks like:

#!/bin/bash #MSUB -l nodes=1:ppn=8 #MSUB -l walltime=06:00:00 #MSUB -l pmem=6000mb #MSUB -v FOAM_MODULE="cae/openfoam/2.4.0" #MSUB -v MPIRUN_OPTIONS="--bind-to core --map-by core -report-bindings" #MSUB -v EXECUTABLE="icoFoam" #MSUB -N test_icoFoam #MSUB -o icoFoam.log #MSUB -j oe startexe="mpirun ${MPIRUN_OPTIONS} ${EXECUTABLE} -parallel" # openfoam-2.4.0 automatically loads mpi/openmpi/1.8-gnu-4.9 module load ${FOAM_MODULE} foamInit # remove decomposePar if you already decomposed your case beforehand decomposePar && # starting the solver in parallel. Name of the solver is given in the "EXECUTABLE" variable, # in the header echo $startexe exec $startexe && # remove reconstructPar and the '&&' operator from the command above # if you would like to reconstruct the case later reconstructPar

Using I/O and reducing the amount of data and files

In OpenFOAM, you can control which variables or fields are written at specific times. For example, for post-processing purposes, you might need only a subset of variables. In order to control which files will be written, there is a function object called "writeObjects".

An example controlDict file may look like this: At the top of the file (entry "writeControl") you specify that ALL fields (variables) required for restarting are saved every 12 wall-clock hours. Then, additionally, at the bottom of the controlDict in the "functions" block, you can add a function object of type "writeObjects". With this function object, you can control the output of specific fields independent of the entry at the top of the file:

/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1.x | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // startFrom latestTime; startTime 0; stopAt endTime; endTime 1e2; deltaT 1e-5; writeControl clockTime; writeInterval 43200; // write ALL fields necessary to restart your simulation // every 43200 wall-clock seconds = 12 hours of real time purgeWrite 0; writeFormat binary; writePrecision 10; writeCompression off; timeFormat general; timePrecision 10; runTimeModifiable false; functions { writeFields // name of the function object { type writeObjects; libs ( "libutilityFunctionObjects.so" ); objects ( T U rho // list of fields/variables to be written ); // E.g. write every 1e-5 seconds of simulation time only the specified fields writeControl runTime; writeInterval 1e-5; // write every 1e-5 seconds } }

You can also define multiple function objects in order to write different subsets of fields at different times. You can also use wildcards in the list of fields- for example, in order to write out all fields starting with "RR_" you can add

"RR_.*"

to the list of objects. You can get a list of valid field names by writing "banana" in the field list. During the run of the solver all valid field names are printed. The output time can be changed too. Instead of writing at specific times in the simulation, you can also write after a certain number of time steps or depening on the wall clock time:

// write every 100th simulation time step
writeControl timeStep;
writeInterval 100;

// every 3600 seconds of real wall clock time
writeControl runtime;
writeInterval 3600; 

If you use OpenFOAM before version 4.0 or 1606, the type of function object is:

type writeRegisteredObject; // (instead of type writeObjects) 

If you use OpenFOAM before version 3.0, you have to load the library with

functionObjectLibs ("libIOFunctionObjects.so"); // (instead of libs ( "libutilityFunctionObjects.so" )) 

and exchange the entry "writeControl" with "outputControl".

OpenFOAM and ParaView on bwUniCluster

ParaView is not directly linked to OpenFOAM installation on the cluster. Therefore, to visualize OpenFOAM jobs with ParaView, they will have to be manually opened within the specific ParaView module.

1. Load the ParaView module. For example:

$ module load cae/paraview/4.3.1

2. Create a dummy '*.openfoam' file in the OpenFOAM case folder:

$ cd <case_folder_path>
$ touch <case_name>.openfoam

NOTICE: the name of the dummy file should be the same as the name of the OpenFOAM case folder, with '.openfoam' extension.

3. Open ParaView:

$ paraview

NOTICE: ParaView is a visualization software which requires X-server to run.

4. In Paraview go to 'File' -> 'Open', or press Ctrl+O. Choose to show 'All files (*)', and open your <case_name>.openfoam file. In the pop-up window select OpenFOAM, and press 'Ok'.

5. That's it! Enjoy ParaView and OpenFOAM.

---