BwUniCluster2.0/Software/OpenFoam

Description	Content
module load	cae/openfoam
Availability	bwUniCluster_2.0 | BwForCluster_JUSTUS_2 | bwGRiD-Tübingen | BwForCluster_MLS&WISO_Production
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.

Availability

OpenFOAM is available on selected bwHPC-Clusters. A complete list of versions currently installed on the bwHPC-Clusters can be obtained from the Cluster Information System (CIS).

Adding OpenFOAM to Your Environment

In order to check which versions of OpenFOAM are installed on the compute cluster, run the following command:

$ module avail cae/openfoam

In general, several OpenFOAM versions should be returned. The default version can be accessed by loading the appropriate module:

$ module load cae/openfoam

Other OpenFOAM versions (if available) can be loaded according to:

$ module load cae/openfoam/<version>

with <version> specifying the desired version.

To activate the OpenFOAM applications, type

$ 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 8, on 80 processors, on a multiple partition with a total wall clock time of 6 hours looks like:

#!/bin/bash # Allocate nodes #SBATCH --nodes=2 # Number of tasks per node #SBATCH --ntasks-per-node=40 # Queue class https://wiki.bwhpc.de/e/BwUniCluster_2.0_Batch_Queues #SBATCH --partition=multiple # Maximum job run time #SBATCH --time=4:00:00 # Give the job a reasonable name #SBATCH --job-name=openfoam # File name for standard output (%j will be replaced by job id) #SBATCH --output=logs-%j.out # File name for error output #SBATCH --error=logs-%j.err # User defined variables FOAM_VERSION="8" EXECUTABLE="icoFoam" MPIRUN_OPTIONS="--bind-to core --map-by core --report-bindings" module load ${FOAM_VERSION} 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 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:

• Batch Jobs Features

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/5.9

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: To run Paraview using VNC system is required on the bwUniCluster. On the cluster run:

$ start_vnc_desktop --hw-rendering 

Start your VNC client on your desktop PC. NOTICE Information for remote visualization on KIT HPC system is available on: https://wiki.scc.kit.edu/hpc/index.php/Remote_Visualization

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.

---