Reconstruction issue

[starflame-Qot]

hello，I tested two tutorial cases, freeProFlame2D and damBreak2D, and both worked fine in reconstructParMesh.

However, once I use reconstructPar, I will get the following error, as shown in the figure.

It doesn't go wrong from the beginning, it happens sometime in the middle.(actually, freeProFlame2D case was reported error at the first moment)

When I use reconstructPar -latestTime, I can synthesize the data for the last time.

Thanks for your potential help.

[JanGaertner]

I had the same issue, never could figure out why it happens as it appears kinda random.

However, I think this is an OpenFOAM issue. I also experienced reconstruct problems with a static mesh for large scale computations on a super computer.

If you have an idea how to solve this, it would be greatly appreciated.

[FoamScience]

I see.

The problem seems to be originating from a bug in reconstructPar. It is somehow trying to read mesh data of the previous time steps instead of the current one!!!

There is a simple workaround. Reconstruction seems to work if you specify the time as a CLI argument:

reconstructParMesh
for t in $(foamListTimes); do reconstructPar -time $t; done

Or, even better, always reconstruct using distributePar:

runParallel redistributePar -reconstruct

I personally like the second way better. Thanks for reporting this behavior.

I'll keep this issue open; and track progress on fully resolving this bug. If I find time, I'll investigate this further during the weekend.

• add a wiki note about using redistributePar
• switch all tutorials to use redistributePar for decomposition/reconstruction
• fix reconstructPar bug: trying to read some processor meshes from the wrong time folders

[MahadevP2001]

After reconstructParMesh, when I run reconstructPar -time I sometimes get the warning :

--> FOAM Warning :
From virtual Foam::polyMesh::readUpdateState Foam::polyMesh::readUpdate()
in file meshes/polyMesh/polyMeshIO.C at line 235
Number of patches has changed. This may have unexpected consequences. Proceed with care.
--> FOAM Warning :
From int main(int, char**)
in file reconstructPar.C at line 369
readUpdate for the reconstructed mesh:2
readUpdate for the processor meshes :3
These should be equal or your addressing might be incorrect. Please check your time directories for any mesh directories.
Reconstructing FV fields

Reconstructing volScalarFields

However , the reconstruction proceeds without exiting with a fatal error as described here. And I am able to visualize results on Paraview. Is the warning a cause for concern?

[FoamScience]

After reconstructParMesh, when I run reconstructPar -time I sometimes get the warning :

--> FOAM Warning : From virtual Foam::polyMesh::readUpdateState Foam::polyMesh::readUpdate() in file meshes/polyMesh/polyMeshIO.C at line 235 Number of patches has changed. This may have unexpected consequences. Proceed with care. --> FOAM Warning : From int main(int, char**) in file reconstructPar.C at line 369 readUpdate for the reconstructed mesh:2 readUpdate for the processor meshes :3 These should be equal or your addressing might be incorrect. Please check your time directories for any mesh directories. Reconstructing FV fields

Reconstructing volScalarFields

However , the reconstruction proceeds without exiting with a fatal error as described here. And I am able to visualize results on Paraview. Is the warning a cause for concern?

Not really, I never got to the bottom of it, but I think that's just a warning the some boundary conditions may not support changing patches. Should be safe for all BCs that come with OpenFOAM; custom BCs shouldn't cache lists related to face/Cell IDs; If they do, they must provide functionality that maps cached lists (eg. autoMap methods)