|March 9, 2012, 04:27||
Icem cfd multidomain mesh conversion
Join Date: Mar 2009
Posts: 355Rep Power: 8
I have a mesh constisting of 3 domains. Each of them are connected by one interface in icemcfd. I want to use the MRFSimpleFoam, so I export the mesh in Fluent V6format, and run the fluentMeshToFoam. However, the conversion fails. Here is the error message. Any suggestion?
--> FOAM FATAL ERROR: Cannot find match for first face. cell model: tet first model face: 3(1 2 3) Mesh faces: 4 ( 0() 0() 0() 0() ) From function create3DCellShape(const label cellIndex, const labelList& faceLabels, const labelListList& faces, const labelList& owner, const labelList& neighbour, const label fluentCellModelID) in file create3DCellShape.C at line 185. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/fluentMeshToFoam" #3 in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/fluentMeshToFoam" #4 __libc_start_main in "/lib64/libc.so.6" #5 in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
CFD= Cleverly Formatted Data
|March 9, 2012, 05:44||
Join Date: Mar 2009
Posts: 579Rep Power: 19
Maybe if you try flutent3DMeshToFoam instead of fluentMeshToFoam?
Also, exporting each domain separately to separate cases and then merging the meshes and stitching them is an option (using mergeMeshes and stitchMesh).
|May 2, 2013, 11:03||
Join Date: Sep 2011
Posts: 14Rep Power: 6
Hello, for everyone. I want share my solution of converting ICEM CFD hex mesh to OpenFOAM mesh.
This was found thanks to this amazing forum and all of its users.
So my recipe is like that.
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
That’s ALL )))
|fluentmeshtofoam, icem cfd, mesh conversion|
|Thread||Thread Starter||Forum||Replies||Last Post|
|Moving mesh||Niklas Wikstrom (Wikstrom)||OpenFOAM Running, Solving & CFD||122||June 15, 2014 06:20|
|Import Mesh from ICEM CFD to CFX||Andre Almeida||CFX||10||April 20, 2014 15:33|
|How to import mesh from icem cfd to star cd||jopawipr||STAR-CD||4||November 9, 2012 16:18|
|[ICEM] Problem with volume mesh in ICEM CFD||kolapoasafa||ANSYS Meshing & Geometry||2||September 16, 2011 03:54|
|Boddy fitted Hexcore Mesh in ICEM Cfd||Mitch||CFX||0||December 29, 2008 07:07|