[hsieh]

Hi, Billy,

I believe that Salome v3.2.1 supports writing groups in unv format. It will be great if you can get Salome to support OpenFOAM format directly. But, I do not think it will happen soon.

There is a lot of discussions about Open Source codes common format (OpenFOAM, elmer, Code_Aster,..etc.). It looks like this group is in favor of unv format. In this case, even if EDS/SDRC stopped supporinting I-DEAS, the unv format will continue and live in the Open Source world. So, it will not be a waste for this effort. On www.caelinux.com, you can find some disscusions about this.

pei

[billy]

I tried to develop it further but I get a segmentation fault error. I don't know why this happens. I used some information of mshToFoam. Here is a tar of the utility:

unvToFoam.tgz

Billy

[billy]

Hi,

This is the latest version of unvToFoam. If anyone wants to try it and give me feedback.

unvToFoam.tgz

It only reads tetrahedra and does not read any boundary data. autoPatch can be used to retrieve the patches.

[santos]

Hello Billy

I tried your application with a simple cube meshed with tetrahedra, and it works fine. Nice work!

Ill keep you updated with further testing.

Regards
José Santos

[billy]

There is another problem: the file can only have two datasets 2411 and 2412. If it has more, it will fail. So you have to edit the file manually and erase other datasets if they exist.

[olesen]

In case anyone is interested, I tossed together two scripts for converting between unv and pro-STAR format, which helps with the import/export from Foam: unv_star_conversion.tar.gz

I've also written a small foamMeshToUnv utility, but does anyone know how the boundary regions are specified in the UNV format?

/mark

[billy]

I discovered that Elmer also imports UNV format. I just looked very breifly at the source code. I am not sure they can read regions.

http://www.csc.fi/elmer/

Maybe you can check here:

http://www.sdrl.uc.edu/uff/uff.html

[micpage18]

Hi Billy,

I tried to use your program unvtofoam with OpenFoam 1.2 but I'm not able to make it run. Can you please make a little tutorial where you explain the procedure to use it. Something like the step from the installation of unvtofoam until the conversion of the mesh.

Thank you,

MP

[billy]

OK.

I would do the following:

1. Copy the latest tar to directory: $HOME/OpenFOAM/OpenFOAM-1.2/applications/utilities/mesh/conversion

2. Go to this directory and untar using: tar -xzvf unvToFoam.tgz (This should create a new folder named unvToFoam. In this same directory you have gmshToFoam, mshToFoam, etc.)

3. Still in this directory type: wmake unvToFoam this will compile it and create an executable.

4. If your OpenFOAM installation is correct you should be able to type unvToFoam for example in your home directory and it should run.

5. Create a tetrahedral mesh in Salome and export to unv format (ex: piston.unv). Ensure file has only two datasets 2411 and 2412. You can open the file in a text editor and check it. Datasets start with -1 and then the code of the dataset. ex:
-1
2411
...
-1

6. Then create a new case (ex: piston) in a solver (ex: stressedFoam) using FoamX .

7. Copy the file to the directory of that case.

8. Type: unvToFoam $FOAM_RUN/tutorials/stressedFoam piston $FOAM_RUN/tutorials/stressedFoam/piston/piston.unv

9. You can use autoPatch for example to create new patches.

10. Then use FoamX to assign BC and define the simulation.