[Chubmaster]

I am trying to create a 2D simulation of a flat plate at various angles against incoming air. I used blockmesh to create a rectangular mesh 1 cell deep (x direction), and then used snappyHexMesh to merge it with the flate plate stl. However this creates more cells in the x direction. I am attempting to use extrudeMesh to make the front face the whole mesh.



When I run extrudeMesh, I get:

Writing mesh to  "/mnt/c/Users/Avedis/Desktop/Fluids_stuff/flateplate02D/constant/region0"

, it does not write to the most recent polymesh.
When I check the constant directory its not there. If I look at the most recent time in paraview, its the same mesh as before. I don't think it did anything.


this is my extrudeMeshDict:

constructFrom       patch;

sourceCase          ".";

sourcePatches       (front);

exposedPatchName    back;

flipNormals         false;

extrudeModel        linearNormal;

nLayers             1;

expansionRatio      1.0;

linearNormalCoeffs
{
    thickness       0.01;
}

mergeFaces          false;

[matejfor]

Hi, not sure if it is still an issue, but perhaps there was some message utility prints out to the terminal? What does it say?

[leobaz]

Hello, this topic may be a bit old, but I'm currently working on OpenFoam and also trying to get a 2D mesh after snappyHexMesh turned my 2D mesh into a 3D mesh. So I used extrudeMesh as Chubmaster did and got the same issue. My mesh is apparently written in constant/region0 but there is no region0 file in my constant folder. Does anyone managed to use extrudeMesh and get a 2D mesh ?

[matejfor]

Hi,

the information that your mesh was written to constant/region0 maybe is not very lucky one, but is here for the cases you build multiregion mesh. Region0 is the default one, so your mesh is written to constant/polyMesh/ directory. In case of a multiregion mesh, it would be constant/<regionName>/polyMesh.

If you have more doubts, try

>> find $FOAM_TUTORIALS -name extrudeMeshDict

for more examples.


Hope it helps

[leobaz]

Hi,


Thank you for your answer. I tried to run some tutorials which uses this and I finally found what was wrong. It is necessary to execute "snappyHexMesh -overwrite" instead of just "snappyHexMesh" before running extrudeMesh. I hope this can help people.

[matejfor]

Yes. Well done. SnappyHexMesh is writing the mesh to the time directory according to the time step settings in <system>/controlDict. So without an argument, it is going to write the mesh into a next time directory. overwrite option will make it to write the polyMesh directory into a constant directory.

You can actually copy the polyMesh directory manually yourself e.g.:

>> cp -r 3/polyMesh constant/polyMesh

if your snappyHexMesh has written the final mesh to time dir. 3.
For more info on snappyHexMesh, please look here:

https://www.openfoam.com/documentati...pyhexmesh.html

happy foaming