[sherlok_holmes]

Hi All,

I am trying to simulate the flow through a butterfly valve on openFoam. I have created two different meshes (fine and coarse) with 8.6 million and 3.11 million mesh count. Both the meshes looks fine and does not show any errors in checkMesh operation. Though no error has been detected the solution diverges in 10 iterations for the coarse mesh while it converges in 400 iterations for fine mesh.

The only difference I find in both the meshes is that the non-orthogonal angle for coarse mesh is higher as compared to that of fine mesh (please refer the attached image for comparison).

Now my question is:

Can we change the default checkMesh criteria in openfoam for non-orthogonal faces from 70 degree to 60 degree or any other angle?
Alternatively How can I write a vtk file for non-orthogonal faces with an angle more than 60 degree?

Thanks for help.

[cutter]

Hi,

mesh quality criteria are usually specified in system/meshQualityDict. The path to such dictionary files can be passed to checkMesh by using the -meshQuality option.

Please have a look at the following links to obtain more insight:

https://github.com/OpenFOAM/OpenFOAM...sh/checkMesh.C

https://github.com/OpenFOAM/OpenFOAM...ualityDict.cfg (default settings)

Cutter

[sherlok_holmes]

Dear Mr Cutter,

Thank you for the reply.

I have tried to run the meshQualityDict with the required mesh quality parameter and it worked.

But now when i write the vtk file for the defined mesh criteria through foamtoVTK -faceSet meshQualityFaces it writes all the faces in the meshQualityFaces.

Is there any way to write a separate vtk file for every user defined checkMesh criteria?

Like i wanted to write vtk files for user defined maxNonOrtho and user defined maxBoundarySkewness separately.

Thanking in anticipation.

[sherlok_holmes]

Please reply as per your earliest convenience.


Best Regards

[Antimony]

Hi,

Doesn't the output of checkMesh go to individual "sets"? nonOrthoFaces would be one, skewFaces would be another etc. etc. In which case you can create each set separately with the foamToVTK command, no?

Cheers,
Antimony

[obscureed]

This is an old thread, but it shows up on a Google search, so here is what I have found:

You can get checkMesh to automatically convert sets to vtk format for viewing using

checkMesh -meshQuality -writesets vtk

(see https://www.openfoam.com/releases/op...0+/meshing.php)

The -meshQuality option in that command causes a separate check based on ./system/meshQualityDict. Faces that fail *any* of those user-defined criteria are all exported into *one* set: ./postProcessing/constant/meshQualityFaces/meshQualityFaces.vtk. The standard sets (skewFaces and so on) are based on the standard criteria.

So, it appears that there is no way to get a separate VTK for each *user-defined* criterion. If you want to look only at, for example, skewness > 7, then you need to hack your ./system/meshQualityDict such that all faces pass all the other criteria. (Save a copy of a sensible meshQualityDict, for use in meshing!) For example, you might find it necessary to set

minTetQuality -9.999e30;

minTetQuality is a strange one: on real meshes that I have tried, there are sometimes a few faces have negative values (reported as "faces with face-decomposition tet quality < 0.0"). This seems alarming, judging from the comments in an official meshQualityDict. (See the earlier links from cutter, or test your navigation skills and patience by trying to find an up-to-date equivalent.) Yet these faces do not show up in a standard meshCheck report. (This is perhaps because the up-to-date meshQualityDict.cfg has large negative minTetQuality, disabling the check. What is the difference between meshQualityDict and meshQualityDict.cfg in https://github.com/OpenFOAM/OpenFOAM...esh/generation?) The meshes typically solve happily enough.