how to create 2d cases with netgen
Hi there - I would like to create a 2d case with the front and rear faces of the domain being of type empty. However, for meshes that I have imported using netgen I get the following error in the initialization step:
--> FOAM FATAL ERROR:
This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.
Because the mesh is only one layer of cells thick I have to assume this is because netgen creates tetrahedral meshes. I have also tried importing quad dominated meshes from netgen without success.
It seems that others may have had similar issues, but any help would be greatly appreciated.
Thank you all very much for all the help.
A Good Evening to you, and sorry for the delay in replying to your post.
Well... OpenFOAM more or less works exclusively with 3-D cases, with 2-D being emulated by using a mesh which is flat (2 dimensional), and contains only one layer of cells in the third dimension.
A Mesh of this kind will not be very easy to generate using Netgen, because you cannot explicitly tell Netgen to limit itself to purely one layer of cells in one dimension. Netgen is essentially an unstructured tetrahedral mesh generation tool.
What you really need, is a way to extrude 2-D meshes in the third dimension.
I looked around in the palette of OpenFOAM mesh utilities, and found two utilities "extrude2DMesh" and "extrudeMesh".
Now... "extrudeMesh" seems to work only with an already existing volume (3-D) mesh, in order to further extrude an existent patch along its normal.
"extrude2DMesh" seems to be more of a 2-D mesh extrusion tool, but I could not get it to work (yet).
I have extruded 2-D meshes into the third dimension some time ago, using the Salomé Platform.... using this program, you can easily mesh a 2-D surface, and extrude this mesh.
Once you extrude it, you can export the mesh in the "UNV" format, and use the mesh conversion tool "unvToFoam" (I think?) to convert it into the OpenFOAM format.
Hope this helps :-)!
Have a great day ahead!
there is a little video howto http://www.caelinux.org/wiki/index.p...ELinux_2007.29
salome makes use of netgen or gmsh as some of the meshing tools among many (plugins for external meshers)
Hi Philippose and Elvis - Thanks for the help. For now I was able to get by using blockMesh, but perhaps as my geometry becomes more complex I will try out one of the software packages you recommend.
The other way to tackle this problem is to use Gambit as a mesh generator. You can generate a face mesh and then use "Geometry->Volume>Sweep Faces" and activate the option "with mesh". This will create the ideal mesh to use for 2D openfoam calculations. You can export mesh and then use "fluent3DMeshToFoam" command and set the appropriate boundary conditions in "constant/polyMesh/bondary".
|All times are GMT -4. The time now is 22:48.|