RunFunctions: a Quick Cheatsheet

All OpenFOAM tutorials have Allrun and Allclean scripts which call some mysterious RunFunctions from even more mysterious sources. The most mysterious thing of all this is how poorly those are documented.

Since those are not a big deal, I decided to jot down some remarks so a newcomer can tell what they are for.

The Manual Way

To be honest, one could easily get along without those functions. Just call OpenFOAM applications by their name:


# background mesh for Snappy
blockMesh > log.blockMesh

# decompose and mesh
decomposePar -force > log.decomposePar
mpirun -np 4 snappyHexMesh -overwrite > log.snappyHexMesh
mpirun -np 4 checkMesh > log.checkMesh
mpirun -np 4 renumberMesh -overwrite > log.renumberMesh

# see an explanation below
rm -r 0
cp -r 0.orig 0

# run the solver
mpirun -np 4 simpleFoam

As you can see, it works just fine, but it does get a little verbose and repetitive. And if you decide to change the number of processors, you have to edit system/decomposeParDict and every parallel-running application call in all your scripts.

RunFunctions to the Rescue

These functions are defined in $WM_PROJECT_DIR/bin/tools/RunFunctions so if you want to use them, you have to tell Bash where they are (mind the dot at the beginning):

. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions

Now the above script will look like this:

. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions

# background mesh for Snappy
runApplication blockMesh

# decompose and mesh
runApplication decomposePar -force
runParallel snappyHexMesh -overwrite
runParallel checkMesh
runParallel renumberMesh -overwrite

# restore 0/ directory

# run the solver
runParallel `getApplication`


  • runApplication will, as the name suggests, run the specified application.
  • It will redirect the app’s output to a log file.
  • Also, if the log exists, it will not run!
  • If you don’t care about existing logs, you can overwrite it with -o option:
    runApplication -o decomposePar -force
  • If you run the app multiple times and want the same log, append to an existing one with -a option:
    runApplication -a decomposePar -force
  • If you want separate logs for multiple runs, you can name the log with -s option. For instance, when merging multiple parts of meshes, your script might look like this:
    runAppliration -s inlet mergeMeshes ../mesh-inlet
    runApplication -s outlet mergeMeshes ../mesh-outlet

    These commands will create two logs, log.mergeMeshes.inlet and log.mergeMeshes.outlet.


The same as runApplication but it will first interrogate system/decomposeParDict to get number of processors. It will then run your app in parallel with MPI. The same logging options apply as to runApplication.


This will read system/controlDict.application and return that command. You will usually need this just to avoid hard-coding solvers. According to DRY principle, it is already specified in controlDict and that should be enough.

Instead, feed getApplication’s output to runApplication / runParallel:

runApplication `getApplication`

That saves you quite some steps:

  • Matching decomposeParDict.numberOfSubdomains
  • Matching controlDict.application
  • Invoking MPI
  • Keeping log files and whatsit.


If you run potentialFoam, setFields and similar apps, they will overwrite boundary conditions that you meticulously prepared in your 0/ directory.

To prevent that from happening, it is wise to keep your boundary conditions in a directory where solvers can’t touch them and copy them to 0/ just before runs. It’s easy to do that by hand but restore0Dir will also take care of some other stuff (#include directives, parallel runs, …).

Anyway, a line saved is a line less to maintain.

Bonus Hint: CleanFunctions

There are more goodies that come in hand with RunFunctions! Type this into shell:

cat $WM_PROJECT_DIR/bin/tools/CleanFunctions

and take a scroll through the output to find commands such as:

  • cleanDynamicCode
  • cleanSnappyFiles
  • cleanPostProcessing
  • cleanCase
  • cleanCase0

Have fun!


  1. Absolutely helpful!! really thank you for pointing out such extraordinary tricks 😀

  2. Thank you so much for this excellent blog. I am struggling in learning OpenFOAM because it is so poorly documented. This is crazy for such widespread open-source software.

Leave a Reply