CFD Online Logo CFD Online URL
Home > Forums > OpenFOAM Meshing & Mesh Conversion

Icem cfd multidomain mesh conversion

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Display Modes
Old   March 9, 2012, 04:27
Default Icem cfd multidomain mesh conversion
Senior Member
Attesz's Avatar
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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?


Cannot find match for first face. cell model: tet first model face: 3(1 2 3) Mesh faces: 

    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/"
#1  Foam::error::abort() in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/"
 in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
 in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
#4  __libc_start_main in "/lib64/"
 in "/software/oss/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
CFD= Cleverly Formatted Data
Attesz is offline   Reply With Quote

Old   March 9, 2012, 05:44
Senior Member
bigphil's Avatar
Philip Cardiff
Join Date: Mar 2009
Location: Dublin,Ireland
Posts: 572
Rep Power: 19
bigphil will become famous soon enoughbigphil will become famous soon enough

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).

bigphil is offline   Reply With Quote

Old   May 2, 2013, 11:03
New Member
Join Date: Sep 2011
Posts: 14
Rep Power: 6
waiter120 is on a distinguished road
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 )))
waiter120 is offline   Reply With Quote


fluentmeshtofoam, icem cfd, mesh conversion

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
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

All times are GMT -4. The time now is 01:05.