[vasava]

I have been trying to setup a heat transfer case with multiple domains using chtmultiregionfoam solver. First I ran the tutorials 'multiRegionHeater' and 'multiRegionHeaterRadiation' and using the idea I tried to run my own case. The case is simple the outermost fluid is hot which heats up a pipe and the pipe heats up the cold fluid passing through it.

Here is what I did.
1. Import 3 meshes from fluent.
2. Create respective folders for all the domains in 0/, constant/ and system/ folders.
3. Run chtmultiregionfoam.

My case runs fine until sometime then crashes with error about solving temperature. Here are some questions I have. Although any other suggestion is welcome.

1. Do I need to write 'topoSetDict', 'makeCellSets.setSet' and 'changeDictionaryDict' files for mesh imported from fluent?

2. Since my meshes are imported from fluent I do not have the files 'boundaryRegionAddressing', 'cellRegionAddressing', 'faceRegionAddressing' and 'pointRegionAddressing' in the polymesh folder. Do I have to have these files?

I am very confused and have tried so many boundary conditions but nothing seems to help. Any help of guidance is welcome.

I can not share the meshes but here are my setup files.

[vasava]

I followed procedure suggested by waiter120 in this thread.

1. Prepare mesh in ICEM CFD with all name selections
2. Export it to FLUENT_V6 (for my present experience, you don’t need specify BC in Output -> Boundary Condition (If I am wrong, please correct me))
3. Read mesh in FLUENT
4. Modify names of BC
4a. If you case is multi region (like chtMultiregionFoam). In FLUENT change type of coupled wall. From Wall to Interior (+ add interior- prefix to its name)
5. Change write-type to ascii “file/ binary-files? no”
6. Write .cas file
7. In OpenFOAM work directory
7a. fluentMeshToFoam –wrireZones fluent.cas
7b. splitMeshRegions -cellZones -overwrite

The trick worked fine for me and I could produce the mesh and the partitions with 'boundaryRegionAddressing', 'cellRegionAddressing', 'faceRegionAddressing' and 'pointRegionAddressing' in the polymesh folders.

I am now trying to solve the heat transfer issues.

Please feel free to comment and send advise if you have any.

[vasava]

The trick to convert the interface to interior goes like this. First delete the interface this will create two interfaces with extension 'src' and 'trg'. Then fuse the interfaces with extension 'src' and 'trg' which will create a new interior.