CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (http://www.cfd-online.com/Forums/openfoam-meshing-other/)
-   -   From ansys meshing to openfoam (http://www.cfd-online.com/Forums/openfoam-meshing-other/107592-ansys-meshing-openfoam.html)

Danath October 2, 2012 05:38

From ansys meshing to openfoam
 
I have created a 3d geometry with gambit and meshing with ansys meshing and i exported as .msh

when i type fluent3DMeshToFoam singleserpantinefine.msh


/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-0bc225064152
Exec : fluent3DMeshToFoam singleserpantinefine.msh
Date : Oct 02 2012
Time : 12:30:08
Host : "danath-desktop"
PID : 1915
Case : /home/danath/OpenFOAM/danath-2.1.0/run/tutorials/singleserpantine
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Dimension of grid: 3
Number of points: 9835676
Number of faces: 28616972
Number of cells: 9401296
--> FOAM Warning : Found unknown block of type: "3010"
on line 14


--> FOAM FATAL ERROR:
Do not understand characters: �
on line 15

From function fluentMeshToFoam::lexer
in file fluent3DMeshToFoam.L at line 747.

FOAM exiting

where is the problem ?


http://albertopassalacqua.com/?p=885 is it safe ?

wyldckat October 2, 2012 16:22

Greetings Evangelos,

The fix that is presented in http://albertopassalacqua.com/?p=885 is meant to be used as follows:
  1. Edit the file "~/.bashrc" and add to the end of the file a new line with:
    Code:

    export AWP_WRITE_FLUENT_MESH_ASCII=1
  2. Start a new terminal.
  3. Launch Workbench directly from the new terminal.
    • If you are only able to launch the Workbench application from the menu, then you might need to logout and then log back in.
  4. Export the mesh on Workbench again to ".msh".
  5. Now you can go back to the terminal and convert the ".msh" file to OpenFOAM.
Best regards,
Bruno

jrrygg October 21, 2012 11:34

Hi,

I would like to trythis fix to see if I can succesfully import my Ansys mesh. However I am running Ansys Workbench in Windows, how can I specify that I would like the .msh-file in ASCII-format?

Regards,

Jone

wyldckat October 22, 2012 08:38

Greetings Jone and welcome to forum!

Quote:

Originally Posted by jrrygg (Post 387769)
I would like to trythis fix to see if I can succesfully import my Ansys mesh. However I am running Ansys Workbench in Windows, how can I specify that I would like the .msh-file in ASCII-format?

Search for "How To Manage Environment Variables in Windows". Example: http://support.microsoft.com/kb/310519

Best regards,
Bruno

phsieh2005 October 22, 2012 11:26

Hi, Jone,

Depending on which ANSYS version you are using. If you are using V14, then, you do not have to set the ascii = 1 throught windows variable.

In Workbench Meshing, seclect "Tools", then, click "Export" under Meshing. Set ANSYS Fluent format to "Ascii".

After this, you can export the mesh and select Fluent *.msh format.

Pei-Ying

jrrygg October 23, 2012 10:33

Thank you very much both of you! I will check this out as soon as I get my new installation running.

Have a nice day!


All times are GMT -4. The time now is 22:34.