CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Arbitrary cyclic patch (http://www.cfd-online.com/Forums/openfoam-solving/59885-arbitrary-cyclic-patch.html)

luca November 2, 2006 05:58

Hi, I need to manage mesh w
 
Hi,

I need to manage mesh with cyclic patch. The problem is that I cannot use couplePatch utility because of are no integral cyclic patches. It's possible in OF to manage "Arbitrary" cyclic patch or do you have suggestions about it?!

Luca

mattijs November 3, 2006 04:51

Arbitrary cyclics do not exist
 
Arbitrary cyclics do not exist. Any matching (to create cut faces) should be done as a preprocessing step. There is no ready made tool in OpenFOAM to do this. You might be able to program something like:
- create an offsetted mesh (transformPoints)
- merge the original and offsetted mesh (mergeMeshes)
- create overlapping region (stitchMesh)
- remove the offsetted region (subsetMesh)
- duplicate the cut faces from stitchMesh to the other side of the geometry (missing tool)
- create cyclics (createPatches)

hjasak November 3, 2006 07:45

Actually, there is work going
 
Actually, there is work going on on this but it is not released into the public domain. There are 2 ways of doing this, one of which works on the originl mesh and another that performs face cutting using my sliding interface tools.

Hrv

luca November 6, 2006 04:14

Thanks a lot for your suggesti
 
Thanks a lot for your suggestions

Luca

cosimobianchini December 20, 2006 12:24

Hi Mattijs, I'm trying to fol
 
Hi Mattijs,
I'm trying to follow your suggestions on how to modify cyclic patches to obtain OneToOne correspondence between the faces on different patches enabling the match as cyclic patches.
Apart of the missing tool (copy the slave patch of the stitchMesh on the master one), I'm stuck on how to remove the mergedMesh from the mesh itself.
I don't understand how to define the <set> argument in the subsetMesh command line.
Thank you very much for your explanation

Cosimo

mattijs December 21, 2006 18:50

The argument to subsetMesh is
 
The argument to subsetMesh is a cellSet. cellSets can be defined using the cellSet or setSet utility.

Have a look at e.g. boxToCell in the sample cellSetDict in the cellSet source directory.


All times are GMT -4. The time now is 20:50.