[Hisham]

Dear Foamers,

I try to make an internal faceZone/faceSet in a Gmsh geometry. I defined a physical surface of the internal surfaces in question. I run

gmsh -3 file.geo; gmshToFoam file.msh

. By viewing the output in paraFoam, the faceZone/faceSet exists but has a different name than the physical surface. It has the name of a cellZone that is not even adjacent to the surfaces.

Question time:
1. Did anyone face the same problem or has anyone produced internal faceZones without this problem?
2. Is there a workaround?

Best regards,
Hisham

[Hisham]

It seems that there is a bug in gmshToFoam. Changing:

01058         forAll(zoneFaces, zoneI)
01059         {
01060             if (zoneFaces[zoneI].size())
01061             {
01062                 label physReg = zoneToPhys[zoneI];
01063 
01064                 Map<word>::const_iterator iter = physicalNames.find(physReg);
01065 
01066                 word zoneName = "faceZone_" + name(zoneI);
01067                 if (iter != physicalNames.end())
01068                 {
01069                     zoneName = iter();
01070                 }
01071 
01072                 Info<< "Writing zone " << zoneI << " to faceZone "
01073                     << zoneName << " and faceSet"
01074                     << endl;

to:

01058         forAll(zoneFaces, zoneI)
01059         {
01060             if (zoneFaces[zoneI].size())
01061             {
01062                 label physReg = patchToPhys[zoneI];
01063 
01064                 Map<word>::const_iterator iter = physicalNames.find(physReg);
01065 
01066                 word zoneName = "faceZone_" + name(zoneI);
01067                 if (iter != physicalNames.end())
01068                 {
01069                     zoneName = iter();
01070                 }
01071 
01072                 Info<< "Writing zone " << zoneI << " to faceZone "
01073                     << zoneName << " and faceSet"
01074                     << endl;

solves the problem for me!

Regards,
Hisham