Hey all, I'm currently workin
I'm currently working on a comparison between cfx and openfoam. Therefore I need the meshes in both formats. Therefore I build a mesh in icemCFD and converted it to cfx4 as it was said to be the best way. The conversion of the mesh worked, but just gave little errors about patches:
Default patch type set to wall
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 573
Found 94 undefined faces in mesh; adding to default patch.
Number of non-orthogonality errors: 0. Number of severely non-orthogonal faces: 18.
--> FOAM Warning :
From function primitiveMesh::checkFaceSkewness(const bool report, labelHashSet* setPtr) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 838
Large face skewness detected. Max skewness = 493.014 percent.
This may impair the quality of the result.
12 highly skew faces detected.
Failed 1 mesh geometry checks.
Failed some mesh checks.
The Problem now is that I've got the mesh in the openFOAM format, but the patches aren't defined in 'boundaries', although I though I did this in icemCFD and therefore should appear also in oprnFOAM!? Do I really have to search manually for the faces for all boundaries and fill them in?
Hi Florian From my experien
From my experience, the best way to export a mesh from ICEM-CFD to OpenFoam is to use a the star-CD 3.2.0 format.
1) Set solver
2) Set boundary conditions
3) write output
-Remember to set the "write shells in element file" to none.
-Be sure that for "Boundaries to write", only "Those with a BC type" is checked.
Than through the starToFoam utility you will have your mesh. It works fine with 2D and 3D bodies. I have had problems with axi-symmetric bodies. If you get this to work, please let me know.
Futhermore, Im very interested in seeing any results of your comparison between the codes.
hello all, I have tried con
I have tried converting icemcfd meshes to openfoam by first exporting to Fluent_V6 then using fluentmeshtofoam utility.
However I could not convert hexa_dominant meshes to openfoam.
Also, cfxToFoam utility requires a mesh in .geo format.I was unable to export the meshes from icemcfd to this format.
I need some help in these regards.
I have found that most meshes
I have found that most meshes created in ICEM have to be imported to their native solvers and re-saved before they convert to Foam. No idea why.
cfxToFoam is a very old converter and only supports up to cfx4 block structured meshes, which arent exported by ICEM.
I'm afraid to compare CFX and foam will probably require at least a two step process:
1) Either make the two meshes seperately and to the same specs in blockMesh and ICEM
- make the mesh in ICEM,
- export it to Fluent or STAR format.
- Open the mesh in STAR/Fluent and export the geometry again.
- Convert to Foam.
|All times are GMT -4. The time now is 16:00.|