Hi, I'm trying to use gmsh
 

Hi,

I'm trying to use gmsh as a preprocessor for OpenFOAM cases. When I use gmshToFoam, I get the following message:

> --> FOAM Warning :
> From function polyMesh::polyMesh(... construct from shapes...)
> in file meshes/polyMesh/createPolyMesh.C at line 467
> Found 654 undefined faces in mesh; adding to default patch.
> End

Everything else seems to be fine, but I didn't try to run anything yet. I just would like to know if this is something I should start worrying about or not.

The message means that the con
 

The message means that the converted has found 645 faces for which it could not establish a boundary condition based on your gmsh file. This also might meant that you have a potential error in the mesh, for example of some of those face are internal to the mesh but have not been matched correctly. If the geometry is 2-D and you have 654/2 cells, all is probably well.

Have a look at your model and try to identify those faces: if this is just a piece of the boundary you did notbother define, all is well, however, if you think the complete outside surface is covered with boundary patch definitions, you may be in trouble. Also, try to visualise the default patch (might require some fiddling if the type is empty).

Enjoy,

Hrv

I so not wanted to read that..
 

I so not wanted to read that...

That said, I tried again with a small example, where it's more physically possible to check things by hand.

It did generate the same message.

I checked the boundary list (not so nice because you have to translate the id's of the nodes by hand http://www.cfd-online.com/OpenFOAM_D...part/happy.gif and all the boundary patches are correct: they have the correct number of faces and the correct faces are listed; and the internal faces appear before the boundary ones. In spite of what the warning says, the last section of the boundary file says that there are 0 faces on the default patch, and they start at 30, but there are only 29 faces listed in the face file.

So everything looks fine, overall.

I couldn't help but notice that the number of faces that the conversion program complains about is the exact number of surface elements (triangles) that are generated by gmsh (it always does this, even when you ask for a 3D mesh.)

I think this is probably the source of the warning message. I could find no trace of these 2d elements after the conversion, but I wonder if there is any problem with them. The first comment on the source code of the conversion program explicitly says that it needs the surface elements (at least that' s how I read it.)

So I think I'll just carry on regardless and see what happens next http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Many thanks,

Ramiro.

Try checkMesh: always popular
 

Try checkMesh: always popular :-) Pay close attention to messages about the boundary, especially whether your boundary is topologically and geometrically closed. If it is, all is probably well.

BTW, did you manage to take a look at the faces that give you trouble, say in paraFoam?

Good luck,

Hrv

BTW, I will be in South Americ
 

BTW, I will be in South America in a few weeks time, doing some lecturing on CFD at the University Santa Maria in Valparaiso Chile and going for a short visit to Buenos Aires at the end of October. If there are any FOAM users in either place interested in a drink/chat, please E-mail me. More details to follow on my web site...

Hrv

About gmsh: I don't think gmsh
 

About gmsh: I don't think gmsh can have different regions for different faces of a tet so by default all outside faces are put in the 'defaultFaces' patch.

However if the converter finds triangles/quads in the file it will use the region number on these to 'patchify' the corresponding face of the tet.
So in gmsh you can create a surface and use that region to specify the patches on the tet mesh.