CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

Gambit meshing error

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

LinkBack Thread Tools Search this Thread Display Modes
Old   October 11, 2003, 19:21
Default Gambit meshing error
Posts: n/a

I am trying to meshing a simple cubic geometry with a solid block in the middle. The solid part is a short cylinder with round edges, see here for a show,

I have no problem in creating both volumes (I created the solid volume and a big cubic volume first, then substracted the solid volume from the big one, with both volumes retained, and finally deleted the redundant the big cubic volume). The problem cames when I tried to mesh the volumes after edge meshing.

Meshing the solid volume went fine. Only meshing the surrounding fluid volume got problem. I understand that some edges and faces are physically only one but are used twice in the database for building up the two volumes, and am sure that I meshed all edges correct.

The problem seems that a face to make up the fluid volume is broken during meshing it. See and for a idea of my description, and,,,, furher show the details about the problematic face.

I really don't know how the face broke. It was fine when I made up volumes.

Any idea that I can fix it?

  Reply With Quote

Old   October 11, 2003, 19:24
Default Re: Gambit meshing error
Posts: n/a
Forgot to mention that I am using GAMBIT v2.04, not the newest v2.1. Thanks.
  Reply With Quote

Old   October 14, 2003, 04:32
Default Re: Gambit meshing error
Posts: n/a
Hi Jx! what is the error message you get from GAMBIT?
  Reply With Quote

Old   October 16, 2003, 16:56
Default Re: Gambit meshing error
Posts: n/a
Calogero, thanks for your input.

The error message in Gambit reads:

ERROR: TG_Mesh_Domain failed with error code 1. ERROR: Tetrahedral meshing has failed for volume FluidArea. This is usually caused by problems in the face meshes. Check the skewnesses of your face meshes and make sure the face mesh sizes are not too large in areas of samll gaps

Thanks for further suggestions!
  Reply With Quote

Old   October 17, 2003, 05:01
Default Re: Gambit meshing error
Posts: n/a
Looks that the spheric face is almost tangent to the block face. This is a problem even if you write codes to generate mesh for this kind of geometry.

You should do some modification and make the angle between 2 faces at least a few degrees.

Good luck.
  Reply With Quote

Old   October 18, 2003, 02:49
Default Re: Gambit meshing error
Posts: n/a
Haai, I have one idea, if you want you can proceed by this way. After substracting the two volumes by retaining them, first you connect the faces which are common, I mean connect the face at the interface of the solid and fluid regions. After doing this you give edge mesh. I think it will not give problem. Send me reply if it is working. Venu gopal IIT Madras Chennai
  Reply With Quote

Old   October 21, 2003, 08:05
Default Re: Gambit meshing error
Posts: n/a
Thank you, Venugopal,

I now can mesh the volumes after linking the interfacial faces as you suggested.

However, a new problem comes up, which is not quite related to this meshing difficulty: I could not couple the interfacial faces in FLUENT as they are physical two sets of faces.

In my previous experience, I created volumes by stitching surrounding faces in GAMBIT. Then after import the mesh to FLUENT, I got shadowed boundaries. I could couple the original boundaries and their shadowed ones as thermal conditions.

While in this case, I created the volumes by substracting two relevant volumes (with retain option). This physically leaves two sets of faces at interfacial surfaces. From FLUENT GUI, I see I have to set seperate thermal boundary conditions for them, which is not appropriate for my case.

What should I do? Thanks for further suggestions.
  Reply With Quote

Old   October 22, 2003, 08:28
Default Re: Gambit meshing error
Posts: n/a
Hi jx! I'm not sure i've understoud what you've said. bt anyway, It happens to me when i DIDN'T link the doubled faces (resultting from substracting volumes) that when i specify the boundaries for the meshed faces in GAMBIT. this latter doesn't tak ein account the doubles faces!!! and it gives me bad import in FLUENT. so, if this is your case, i advise you to link all the faces, or delete the doubled faces (with the unused (unmeshed) volumes. then you specify the boundary type for each face and/or volume. wish it could help
  Reply With Quote

Old   October 22, 2003, 11:52
Default Re: Gambit meshing error
Posts: n/a
Hi, Caloggero,

Thanks for your time.

Yes, I *did* link the faces at the interfacial area before I meshed the volumes. I could see if I did not link them, I would have different face meshing within those faces; and the face meshing turned to be identical on both faces comprised of the solid volume and ones comprised of the fluid volume, only if I linked two sets of faces.

I'd address again that this way I had physically two sets of faces at the common area: one set is part of solid volume surface and the other is part of fluid volume surface. They are different boundaries after being imported into FLUENT, and I can *not* couple them as thermal conditions

The attempt to directly delete one set of the faces will fail because it complains there exist "upper" geometrical components. Aactually a solid or fluid volume is built up on top of them.

What I did to work around this problem is to remove one of the volumes in GAMBIT, say, the fluid volume. This removed all entities that made up the fluid volume, including vertices, edges, outer faces and one set of interfical faces. I then regenerated some vertices, edges, outer faces. Finally I stitched the outer faces and the remained interfacial faces to form the fluid volume again. The geometry now only contains one common set of faces shared by both volumes. FLUENT created shadowed faces accordingly while importing the mesh.

Obviously you see the work around is inconvenient, especially if the surfaces of the volume other than the common faces are also geometrically complicated.

Therefore the prefered solution would be joining the two sets of faces into one and keeping the volumes, either in GAMBIT before mesh export, or in FLUENT after mesh import. But I don't know how to do this. I'll apprecate if someone has a better idea.

Thanks again.

  Reply With Quote

Old   April 3, 2009, 20:17
New Member
Join Date: Mar 2009
Posts: 14
Rep Power: 15
cfdproject is on a distinguished road
I am trying to mesh the continuum between fins..However every time I do it I get error saying perturb nodes and try again.Can Anybody help me
cfdproject is offline   Reply With Quote

Old   May 21, 2009, 09:27
Default Volume Mesh in Gambit
New Member
Join Date: May 2009
Posts: 11
Rep Power: 15
esicia is on a distinguished road
I also have similar problems when meshing a volume in Gambit. I modified the gemoetry and reduce the maximum skewness to 0.54 but the Gambit still doesn't accept the Volume mesh, I realy get confused by this problem.

TG_Mesh_Domain failed error code 1

at tha last I have to divide the volume in two part( inside the chamber, outside the chamber) but i encounter to new problem when I export the mesh file and check the grid in Fluent. I want to model the flow coducting through the outside of the chamber and I can not connect this two part continuously.

is there any suggestion? thanks for your Help.

Have a good time
esicia is offline   Reply With Quote

Old   May 26, 2009, 11:35
Default Same problem
kdrbrk's Avatar
Join Date: May 2009
Posts: 90
Rep Power: 15
kdrbrk is on a distinguished road
A have the same problem, please help !
I am sure that mesh size is not the reason because I am meshing a 20 metre boat with 25mm mesh size. The boat is almost completely yellow because of mesh.
Only thing that I suspect is, there is a very very small face that gambit recognizes, lets say 0.1mm wide and 100mm long, rectangular face.

Can it be the problem?
Edit: I found the problem:

There is a very little surface, which was previously generated in catia in order to close a little opening. after editing in catia and removing that surface, problem resolved.

Last edited by kdrbrk; May 27, 2009 at 12:15. Reason: Resolved problem
kdrbrk is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM Community Contributions 300 October 29, 2014 19:00
UDF: DEFINE_CG_MOTION for vertical jump motion of an electrode! alban Fluent UDF and Scheme Programming 2 June 8, 2010 19:54
POSDAT problem piotka STAR-CD 4 June 12, 2009 09:43
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 21:50
user subroutine error CFDUSER CFX 2 December 9, 2006 07:31

All times are GMT -4. The time now is 23:51.