BwUniCluster2.0/Software/OpenFoam

From bwHPC Wiki
Jump to navigation Jump to search
Description Content
module load cae/openfoam
Availability bwUniCluster_2.0 | BwForCluster_JUSTUS_2 | bwGRiD-Tübingen
License GNU General Public Licence
Citing n/a
Links Homepage | Documentation
Graphical Interface No



Description

OpenFOAM (Open-source Field Operation And Manipulation) 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

For a better performance on running OpenFOAM jobs in parallel on bwUniCluster, it is recommended to have the decomposed data in local folders on each node.

Therefore you may use *HPC scripts, wich will copy your data to the node specific folders after running the decomposePar, and copy it back to the local case folder before running reconstructPar.

Don't forget to allocate enough wall-time for decomposition and reconstruction of your cases. As the data will be processed directly on the nodes, and may be lost if the job is cancelled before the data is copied back into the case folder.

Following commands will do that for you: 

$ decomposeParHPC
$ reconstructParHPC
$ reconstructParMeshHPC

instead of: 

$ decomposePar
$ reconstructPar
$ recontructParMesh

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

$ decomposeParMeshHPC
$ mpirun --bind-to core --map-by core -report-bindings snappyHexMesh -overwrite -parallel
$ reconstructParMeshHPC -constant

instead of: 

$ decomposePar
$ mpirun --bind-to core --map-by core -report-bindings snappyHexMesh -overwrite -parallel
$ reconstructParMesh -constant


For running jobs on multiple nodes, OpenFOAM needs passwordless communication between the nodes, to copy data into the local folders.

A small trick using ssh-keygen once will let your nodes to communicate freely over rsh.

Do it once (if you didn't do it already in the past): 

$ ssh-keygen
$ cat $HOME/.ssh/id_rsa.pub >> $HOME/.ssh/authorized_keys

Building an OpenFOAM batch file for parallel processing

General information

Before running OpenFOAM jobs in parallel, 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, 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.

The number of subdomains, in which the geometry will be decomposed, is specified in "system/decomposeParDict", as well as the decomposition method to use.

The automatic decomposition method is "scotch". It trims the mesh, collecting as many cells as possible per processor, trying to avoid having empty segments or segments with not enough 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.

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

# 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 
decomposeParHPC &&

# starting the solver in parallel. Name of the solver is given in the "EXECUTABLE" variable, 
# in the header 
mpirun ${MPIRUN_OPTIONS} ${EXECUTABLE} -parallel &&

reconstructParHPC


Attention: The script above will run a parallel OpenFOAM Job with pre-installed OpenMPI. If you are using an OpenFOAM version wich comes with pre-installed Intel MPI (like, for examplecae/openfoam/v1712-impi) you will have to modify the batch script to use all the advantages of Intel MPI for parallel calculations. For details see:

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.

Retrieved from "https://wiki.bwhpc.de/wiki/index.php?title=BwUniCluster2.0/Software/OpenFoam&oldid=7761"