[praveen@cfd-online.com]

I am trying to generate cartesian mesh for butterfly valve using cfMesh. My observation is for lower angles of valve opening (10,20,30), there are warnings of non-orthogonal faces > 70deg and it causes the simulation to diverge. Refining the mesh helps in avoiding this warning and also helps in convergence. But the mesh count goes very high.

Why they are appearing for lower angles of valve opening? How to avoid non-orthogonal faces>70deg in meshing? Is there any command that I can include in the meshDict file, to put control over mesh quality during mesh generation.

Here is the link to download the mesh setup directory: https://drive.google.com/file/d/0B_ZwZhNE5SPLMWNWWmNESjk0STQ/view?usp=sharing

[peyman.davvalo.khongar]

Moi!

There is one important thing about your case. If you look at your boundary in polymesh directory, the faces have type empty. Do you run your simulations with this type or you modify it before running your solver?

Some suggestions when you work with cfMesh:

1- Try to use fms format rather than stl. run this command:

surfaceFeatureEdges -angle 60 ButterflyValve_FusionModel_30deg_DenseSTL.stl geo.fms

and then in the meshDict use the fms format. Before running cartesianMesh, open your fms file and modify the types and the names if you want. You can see what i mean in this thread:

Symmetry patch issue in cfMesh from stl file


2- when I take a look at your mesh, the non-orthogonal faces appears near to the narrow region between your disc and pipe. (Look at the attached photo). One thing you can do is to just keep this configuration of your meshDict and add 4 objectRefinements around those narrow regions. Like a sphere:

objectRefinements
 {
 sphere
 {
    additionalRefinementLevels 1; // or cellSize SizeOfCell;
    type sphere;
    centre (0.5 0 0);
    radius 0.03;
   }
}

Of course you have to take a look at your geometry and define centre and radius by your own. Above is just an example.

Hope it helps.

Moikka,

Peyman