|
[Sponsors] |
[Commercial meshers] FluentMeshToFoam segmentation fault |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 16, 2007, 13:05 |
FluentMeshToFoam segmentation fault
|
#1 |
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 |
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 |
|
October 16, 2007, 14:04 |
Did you try fluent3DMeshToFoam
|
#2 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
Did you try fluent3DMeshToFoam?
|
|
October 16, 2007, 15:01 |
Can you run this under gdb or
|
#3 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
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 |
|
October 16, 2007, 15:10 |
Dear Hrv and Mattijs,
I ha
|
#4 |
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 |
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 |
|
October 17, 2007, 19:15 |
Dear Hrv and Mattijs,
The p
|
#5 |
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 |
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 |
|
October 29, 2007, 08:56 |
Hello Forum,
I finally solv
|
#6 |
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 |
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 |
|
June 27, 2011, 10:34 |
|
#7 |
New Member
Join Date: Jun 2011
Posts: 1
Rep Power: 0 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Segmentation fault when running dieselFoam or dieselEngineFoam in parallel | francesco | OpenFOAM Bugs | 4 | May 2, 2017 21:59 |
Segmentation fault in SU2 V5.0 | ygd | SU2 | 2 | March 1, 2017 04:38 |
Segmentation fault when running in parallel | Pj. | OpenFOAM Running, Solving & CFD | 3 | April 8, 2015 08:12 |
Segmentation Fault w/ compiled OF 2.2.0 - motorBike example | sudo | OpenFOAM Running, Solving & CFD | 3 | April 2, 2013 17:27 |
segmentation fault when installing OF-2.1.1 on a cluster | Rebecca513 | OpenFOAM Installation | 9 | July 31, 2012 15:06 |