[foamaof]

Dear foamers,

i am quite new in openfoam and have a problem with merging of two regions as you can see in pic 1. My real model is a bit more complex like this example, so i want to use a tetrahedral mesh. After i exported this model from salome to foam, i tried methods like stitchMesh to put the 2 from openfoam identified regions together, but it didn't work. A closer look to the connecting faces (pic 2) shows, that the faces of the thethadrons from the regions doesn't fit completely to each other (Maybe the reason for failure?). Does anybody have any idea, how to fix that problem? Or are there other ways to solve that? Thanks

Anton

[Antimony]

Hi,

Have you tried stitchMesh with the -partial flag?

Best,
Antimony

[foamaof]

Hi Antimony,

thanks for reply. I solved the problem in a strange way as follows (the interfaces are int1 of region 1 and int2 of region 2):

1. ideasUnvToFoam testmesh.unv
2. stitchMesh -overwrite -toleranceDict tolerance int1 int2. But first i have to hide or copy the T,u,p files from the 0-folder to an other folder (if i don't, i'll get the message:

--> FOAM FATAL IO ERROR:
Cannot find patchField entry for int1

file: C:/Users/Simulationen/testmesh/0/T.boundaryField from line 26 to line 36.)

3. open the boundary file in polyMesh and manually remove the int1 and int2 patches.
4. copy T,u and p back to 0-folder.
5. start the show with porousSimpleFoam

I don't unterstand the point 2. where i first have to hide the p,T,u files, before i can start stitchMesh. Or is there a more elegant way to stich 2 regions together?

Anton

[Antimony]

Hi,

Typically in your time folder, for each of your field files, you need to have all the patches that are named in constant/polyMesh/boundary to be present in the field files. If you don't then OF will throw an error. Even if the patch is meant to be intermediate and not in the final version, OF expects it to be in the field files.

From your naming, I would think int1 and int2 are the interfaces that will most likely 'disappear' when you stitch the two meshes. And since they would not be in the final version of the mesh on which you run the simulation, int1 and int2 would not have been mentioned in T, U, p etc. If you have a time directory, then int1 and int2 should be mentioned in them to ensure that stitchMesh runs. Renaming your time directory to time directory.something is a simple way to circumvent this issue (and which is what you have already figured out )

Hope this clarifies.

Cheers,
Antimony

[foamaof]

Hi,

aah okay, thank you for that advice As expected, I got another problem with stitchMesh. I can only mention one Masterpatch and one Slavepatch. Thats okay for two Regions with one interface (2 patches). But what can i do, if i have to stitch more than two patches (interfaces) together for example a cube inside another bigger cube. Is it possible to do that with stichMesh?

regards,
Anton

[Antimony]

Hi,

Yes. In a rather roundabout way though.

Refer to my two posts (#24 and #25) here:

http://www.cfd-online.com/Forums/ope...sh-used-2.html

Cheers,
Antimony