CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

FluentMeshToFoam segmentation fault

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 16, 2007, 13:05
Default Dear Forum, I am trying to
  #1
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Dear Forum,

I am trying to convert a tetrahedral mesh saved from Fluent as *.msh to OpenFOAM. This is the error I get:

[gtg627eOpenFOAM@ruzzene03 simpleFoam]$ fluentMeshToFoam . plateHole prova3.msh
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : fluentMeshToFoam . plateHole prova3.msh
Date : Oct 16 2007
Time : 12:54:34
Host : ruzzene03
PID : 19685
Root : /home/gtg627eOpenFOAM/OpenFOAM/gtg627eOpenFOAM-1.4.1/run/tutorials/simpleFoam
Case : plateHole
Nprocs : 1
Create time

number of faces: 766892
Number of points: 6716
Reading uniform faces
Reading points


FINISHED LEXING


#0 Foam::error::printStack(Foam:stream&) in "/home/gtg627eOpenFOAM/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/gtg627eOpenFOAM/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/tls/libpthread.so.0"
#3 main in "/home/gtg627eOpenFOAM/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/fl uentMeshToFoam"
#4 __libc_start_main in "/lib/tls/libc.so.6"
#5 __gxx_personality_v0 in "/home/gtg627eOpenFOAM/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/fl uentMeshToFoam"
Segmentation fault

----------------------------------------------------------------

Doe anybody know what may cause this?

Thank you,

Alessandro
gtg627e is offline   Reply With Quote

Old   October 16, 2007, 14:04
Default Did you try fluent3DMeshToFoam
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Did you try fluent3DMeshToFoam?
mattijs is offline   Reply With Quote

Old   October 16, 2007, 15:01
Default Can you run this under gdb or
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Can you run this under gdb or in a debug version? I am pretty certain you will have a zero area face or zero volume cell because flexing has finished with no errors. Ten to one your mesh is broken in some way. If you tell me more, I can fix this.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   October 16, 2007, 15:10
Default Dear Hrv and Mattijs, I ha
  #4
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Dear Hrv and Mattijs,

I have been working on this problem, and I think there is something wrong on my side. I am creating a mesh in ANSYS, importing in Fluent and saving it as *.msh. I think something goes wrong between ANSYS and Fluent. I will get back with the problem as soon as I figure it out.

Thank you for your prompt responses,

Alessandro
gtg627e is offline   Reply With Quote

Old   October 17, 2007, 19:15
Default Dear Hrv and Mattijs, The p
  #5
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Dear Hrv and Mattijs,

The problem with Fluent is that my installation does not include tgrid or gambit. So, I can import my .iges file from ANSYS no problem; however Fluent only lets me save the boundary mesh, and not the entire domain. So, when I was trying to import my mesh in OpenFOAM, I was getting a segmentation fault error because I only had boundary faces.

I am trying to simulate the flow around a sphere, and given the short time I have, I swtiched to gmsh to generate my mesh. I am able to import it into openFOAM and run my case.

You should really consider ANSYSToFoam as an import utility. ANSYS so far has proven to be a far superior mesher than anything else I have used.

As soon as I get my simulation dialed in, I will post the gmsh file and the steps I am taking to run the simulation.

Thank you for you help,

Alessandro Spadoni
gtg627e is offline   Reply With Quote

Old   October 29, 2007, 09:56
Default Hello Forum, I finally solv
  #6
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Hello Forum,

I finally solved my problem. One can easily import ANSYS mesh files as follows:

1. create your mesh in ANSYS.

2. To assign boundary conditions, select nodes at boundaries (this is best done by selecting an area at the boundary and then selecting the associated nodes with nsla,s,1) group them by assigning a group name with cm,outlet,node.....cm,inlet,node...etc.

3. Now assign the domain element characteristics with: allsel,all, cm,fluidElem,elem

4. in prep7 archive your model, writing out a file.cdb, or alternatively issue cdwrite,yourfilename,cdb.

5. Transfer file.cdb into Fluent working directory.

6. Start fluent and do file --> import --> ANSYS --> file.cdb

7. Now you have your nice ANSYS mesh in fluent, including boundary condition definitions.

8. Now save your mesh in Fluent as: file --> write --> case (remember to uncheck "write binary files"). Your new file will have a .cas exstension.

9. tranfer your .cas file into OpenFOAM working directory.

10. Import mesh into OpenFoam as:
fluentMeshToFoam root case yourfile.cas

Done.

I hope this helps,

Alessandro
gtg627e is offline   Reply With Quote

Old   June 27, 2011, 10:34
Default
  #7
New Member
 
Join Date: Jun 2011
Posts: 1
Rep Power: 0
rauhpeha is on a distinguished road
Hello Foamers,

gtg627e had a problem with importing an Ansys-mesh to openFoam, and he solved this problem. Now I tried to import an Ansys-mesh, too. But it does not work. openFoam does not read the .cas-file, although I used the command fluentMeshToFoam as described by gtg627e. The openFoam-output is:
Found end of section in unknown
Embedded blocks in comment or unknown
Found end of section in unknown
Found end of section in unknown
Found unknown block in zone
Found end of section in unknown
Found unknown block in zone
Found end of section in unknown
Found unknown block in zone
Found end of section in unknown

[ The smilies are originally ":" ")" resp. ":" "(" ]
Could anybody tell me what that means? Does anybody know about the mistake which I could have done?
thanks and regards
rauhpeha 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
Segmentation fault in map msg30 OpenFOAM Meshing Format & General Technical 6 March 27, 2008 11:49
Segmentation fault. Nari CD-adapco 3 November 8, 2007 06:04
segmentation fault Suman CD-adapco 2 June 26, 2007 03:14
Segmentation fault billy OpenFOAM Installation 20 April 23, 2007 22:57
Segmentation fault Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Running, Solving & CFD 3 January 10, 2005 06:02


All times are GMT -4. The time now is 11:08.