CFD Online Discussion Forums - Is it possible to avoid reconstructParMesh?

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Is it possible to avoid reconstructParMesh? (https://www.cfd-online.com/Forums/openfoam-solving/198383-possible-avoid-reconstructparmesh.html)

Is it possible to avoid reconstructParMesh?

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!

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.

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

For future readers...

After sHM in parallel you need to run

Code:

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

Code:

#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)

Code:

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

Code:

reconstructParMesh -constant

reconstructPar -latestTime

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

Quote:

Originally Posted by RobertHB (Post 680604)

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

Also works with normal ParaView.