CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] ansys icem tetra mesh to fluent_v6 conversion problems (

milleniumrider May 2, 2010 04:33

ansys icem tetra mesh to fluent_v6 conversion problems
2 Attachment(s)
Hi all,

I have a tetra mesh with prism layers generated in Ansys ICEM, I've attached a picture below.

Now when I use fluent_v6 solver to export the mesh so I can use it for my simulation in OpenFOAM. It converts the mesh, but skips the parts, INLET, OUTLET and ROTSYMM2. Also it creates shadow faces instead of the ROTSYMM2 part. Basically ROTSYMM1 and ROTSYMM2 are the sides of the grid that are periodic.

To explain a bit more, the grid is periodic and axisymmetric and it is a wedge of 5 degrees part of a cylindrical set up. I have set the rotational periodicity in the global mesh set up part.

Any help on how to get all the parts required for my boundary definition would be very welcome!

PSYMN May 3, 2010 17:09

Do you have elements in those parts...
It looks like it is saying you have no elements in those parts (not referenced by grid)... if you just display the inlet and outlet parts (in the model tree) and try to show shell elements, what do you see?


milleniumrider May 3, 2010 18:51


First thank you for your reply.

When I switch off everything except the relevant parts and switch on shell elements, I see the shells on the parts as in the shell mesh. And it has triangles and quads, most of the elements on these two parts are quads with about 2 elements being triangles I think.

How do I proceed? Any suggestions?

Thank you again for your time.


PSYMN May 4, 2010 01:14

Sorry, I can't tell from here. I have never had this problem.

Has it ever worked for you?

Did you do anything different with those parts? Did you setup BOCO's for them? Usually, I select fluentV6 as my solver and then setup my inlet and outlet, I leave everything else alone so it defaults to wall.

If you didn't do that... Try it... If you did do that, then maybe that doesn't work with OpenFoam (I have not tried OpenFoam), in which case, don't do that. Leave everything as default (walls) and try it that way.

milleniumrider May 4, 2010 03:45

1 Attachment(s)
Hello again,

I have tried something similar before and it worked. I'm attaching a picture below, the difference is that this time I have these "gap regions" in between. Other than that nothing has changed.

About the BOCOs, I'm trying to run an axi-symmetric case in OpenFOAM. For this I need to define a symmetryPlane (AXIS) and the front and back planes (ROTSYMM1 and ROTSYMM2) as periodic. This is what I'm doing in Ansys ICEM with the "output-BC" tab.

So I think I could try others with default wall but I need to define the periodic walls otherwise upon importing to OpenFOAM the periodic alignments wont be exported as well.

Any ideas of how else I could do this?

Cheers again for your time and patience.


PSYMN May 20, 2010 15:55

5 Attachment(s)
Ok, just to close out this thread... (from a while back)

The problem was that the extra lugs were not properly connected and so the mesh generated was not properly connected.

Attachment 3441

In the end, we fixed the geometry, quad meshed one side and extruded it (rotation 5 degrees about the axis) to get the final mesh.

Attachment 3442
Attachment 3443

The inlet and outlet were setup as the curve parts so that the extruded line elements would become the shells for the bocos...

An even better mesh could easily be obtained by blocking this model. In this case, I started with a 2D Blocking and extruded it to get the final 3D blocking.
Attachment 3444
Attachment 3445

All times are GMT -4. The time now is 08:22.