CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

GMSH Meshes

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 25, 2005, 13:10
Default Hi, I'm trying to use gmsh
  #1
rbw
New Member
 
Ramiro Brito Willmersdorf
Join Date: Mar 2009
Location: Recife, Pernambuco, Brasil
Posts: 16
Rep Power: 8
rbw is on a distinguished road
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.
rbw is offline   Reply With Quote

Old   September 25, 2005, 13:16
Default The message means that the con
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 25, 2005, 16:16
Default I so not wanted to read that..
  #3
rbw
New Member
 
Ramiro Brito Willmersdorf
Join Date: Mar 2009
Location: Recife, Pernambuco, Brasil
Posts: 16
Rep Power: 8
rbw is on a distinguished road
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 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

Many thanks,

Ramiro.
rbw is offline   Reply With Quote

Old   September 25, 2005, 16:22
Default Try checkMesh: always popular
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 25, 2005, 16:25
Default BTW, I will be in South Americ
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 26, 2005, 04:20
Default About gmsh: I don't think gmsh
  #6
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
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.
mattijs is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with Gmsh nishant_hull Open Source Meshers: Gmsh, Netgen, CGNS, ... 18 April 22, 2015 08:43
gmsh jojo Main CFD Forum 5 August 31, 2009 23:11
Gmsh and samplesurface touf Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 December 10, 2007 03:27
Gmsh with physicals Rasmus Gjesing (Gjesing) Open Source Meshers: Gmsh, Netgen, CGNS, ... 9 February 2, 2006 15:36
Using stitchmesh on imported gmsh meshes christian67 OpenFOAM Meshing Format & General Technical 0 November 26, 2005 05:22


All times are GMT -4. The time now is 23:22.