[Rojj]

Hi,

I am running a quite large case and the reconstruction of the mesh takes a very long time.

Is it possible to run mpirun simpleFoam without having to reconstruct the mesh and decompose it again?

I am running OF 4.1. My current workflow is

blockMesh
surfaceFeatureExtract
decomposePar
mpirun -np X snappyHexMesh -overwrite -parallel

reconstructParMesh -constant

decomposePar
mpirun -np X renumberMesh -overwrite -parallel
mpirun -np X simpleFoam -overwrite -parallel

I know that I can postProcess without reconstructing the case, but can I go from decomposed mesh to solution directly?

Thanks!

[eric]

Yes, you do not need to recompose the mesh before running the solver. Have a look at the Allrun file in for instance the motorBike tutorial:
$FOAM_TUTORIALS/incompressible/simpleFoam/motorBike/Allrun

There are some commands there that help copying the 0 folder to all the individual processors. In OpenFOAM 5, you can just add -copyZero as argument to the decomposePar command.

[Rojj]

Thanks Eric! Can't even tell you how much it has helped me.

For future readers...

After sHM in parallel you need to run

ls -d processor* | xargs -I {} rm -rf ./{}/0
ls -d processor* | xargs -I {} cp -r 0.orig ./{}/0

This is a nice linux way to replace all the 0 folders in the processorX folder with the original ones.

Remember to add

#includeEtc "caseDicts/setConstraintTypes"

in all the boundary fields. This will cause an error if you are using PyFOAM (I am). In that case just replace the actual content of caseDicts/setConstraintTypes.


I finally run (not sure if patchSummary is needed)

mpirun --mca orte_base_help_aggregate 0 -np X patchSummary -parallel
mpirun --mca orte_base_help_aggregate 0 -np X renumberMesh -overwrite -parallel
mpirun --mca orte_base_help_aggregate 0 -np X simpleFoam -parallel

If you want to reconstruct the case at this point, you also need to reconstruct the constant directory so

reconstructParMesh -constant
reconstructPar -latestTime

[RobertHB]

And you don't necessarily need to reconstruct. Using paraFoam -builtin you can view your decomposed case in paraview.

[akidess]

Originally Posted by RobertHB

And you don't necessarily need to reconstruct. Using paraFoam -builtin you can view your decomposed case in paraview.

Also works with normal ParaView.