|
[Sponsors] |
[Commercial meshers] Icem cfd multidomain mesh conversion |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 9, 2012, 04:27 |
Icem cfd multidomain mesh conversion
|
#1 |
Senior Member
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17 |
Hi all,
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? Best, Attila Code:
--> 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" |
|
March 9, 2012, 05:44 |
|
#2 |
Super Moderator
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,095
Rep Power: 34 |
Hi,
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). Philip |
|
May 2, 2013, 12:03 |
|
#3 |
New Member
Join Date: Sep 2011
Posts: 15
Rep Power: 15 |
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 ))) |
|
Tags |
fluentmeshtofoam, icem cfd, mesh conversion |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Import Mesh from ICEM CFD to CFX | Andre Almeida | CFX | 16 | April 19, 2016 04:42 |
Moving mesh | Niklas Wikstrom (Wikstrom) | OpenFOAM Running, Solving & CFD | 122 | June 15, 2014 07:20 |
Export mesh from ICEM CFD for Fluent | summerdream | ANSYS | 2 | September 10, 2013 13:12 |
[ICEM] Problem with volume mesh in ICEM CFD | kolapoasafa | ANSYS Meshing & Geometry | 2 | September 16, 2011 04:54 |
Boddy fitted Hexcore Mesh in ICEM Cfd | Mitch | CFX | 0 | December 29, 2008 07:07 |