[giorgianig]

I am generating a mesh in SALOME (unv format) and exporting to OpenFoam using ideasUnvToFoam. I use the Netgen algorithm with viscous layers.

When I generate the mesh, some pyramids are created: those pyramids are not exported in unv, so I split them in tetrahedrons. However, when I convert the mesh using ideasUnvToFoam, some defaultFaces are created:

--> FOAM Warning :
    From Foam::polyMesh::polyMesh(const Foam::IOobject&, Foam::pointField&&, const cellShapeList&, const faceListList&, const wordList&, const wordList&, const Foam::word&, const Foam::word&, const wordList&, bool)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 645
    Found 4311 undefined faces in mesh; adding to default patch defaultFaces
End

I visualized these faces in Paraview, they are internal and close to my walls. I think they are generated due to the splitting of the pyramids.

I tried to put the flag "empty" to these faces in the boundary file, but the simulation with pisoFoam crashes after some iterations due to k and epsilon blowing up close to these faces.



My questions are:



1- is there a way to avoid internal faces when splitting pyramids?
2- if NO, how should I deal with them?


Thanks in advance,
Giorgio

[Alczem]

Hey


Maybe you can try to delete and recreate the groups from your geometry after splitting the pyramids into tetrahedrons? The defaultFaces newly created are probably due to the new faces not belonging to any group.


By the way, how do you split your pyramids in Salome? I have been struggling with this issue for some time.


Let me know if you manage to solve this!

[giorgianig]

To split pyramids: select the mesh, Modification->Split Volumes, deselect Apply to all, Filter by Geometry Type: pyramids.

I am not sure about your procedure... they are internal faces, so why the groups of faces that I create should affect them?

[Alczem]

Ah my bad, I read your post a bit too fast. Maybe you can sew the internal faces together into one face only, I suspect Salome creates duplicate faces when it splits the pyramids. Another thing you could try: use some OpenFOAM utilites such as mergeOrSplitBaffles or stitchMesh maybe? Iam not sure but maybe that could work.


Thanks for the tip about splitting, and sorry for not helping more

[giorgianig]

Yes, I'll try that indeed. Anyway, I found out that you can use the python script salomeToOpenFOAM.py to export the mesh with also pyramids, and seems to work fine.

[GerhardHolzinger]

Originally Posted by giorgianig

... those pyramids are not exported in unv ...

Have you tried a different approach to exporting the mesh?




It is well known, that Salome's export to UNV has no love for pyramids, however, there are other means of exporting a mesh from Salome to OpenFOAM



PS: Should have read the thread fully to the end, I realized just after posting that your last post is about the very thing I was suggesting.


https://github.com/nicolasedh/salomeToOpenFOAM

[Alczem]

Originally Posted by giorgianig

Yes, I'll try that indeed. Anyway, I found out that you can use the python script salomeToOpenFOAM.py to export the mesh with also pyramids, and seems to work fine.

It worked for you right off the bat? I am using Salome 9.10 and it is not working, lot of errors other than the usual wrong syntax (like the print parenthesis missing etc).

[giorgianig]

Yes it worked. I am on Salome 9.9.0 and I am using salomeToOpenFOAM.py right from the Salome interface.

[GerhardHolzinger]

The original code from https://github.com/nicolasedh/salomeToOpenFOAM has not received updates for a while.


So, I would recommend to check out one of the many forks of the original code.
Among others:


https://github.com/meritzio/salomeToOpenFOAM


https://github.com/EastEriq/salomeToOpenFOAM


https://github.com/oseen/salomeToOpenFOAM



I don't remember which of these is on my machine.

[Alczem]

Originally Posted by GerhardHolzinger

The original code from https://github.com/nicolasedh/salomeToOpenFOAM has not received updates for a while.


So, I would recommend to check out one of the many forks of the original code.
Among others:


https://github.com/meritzio/salomeToOpenFOAM


https://github.com/EastEriq/salomeToOpenFOAM


https://github.com/oseen/salomeToOpenFOAM



I don't remember which of these is on my machine.

The EastEriq fork works with Salome 9.10, thanks for the links