Hi, I have imported a mesh wit
Hi, I have imported a mesh with fluentMeshToFoam. When I check the imported mesh I get:
--> 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 = 333.553 percent.
This may impair the quality of the result.
98 highly skew faces detected.
Writing 98 skew faces to set skewFaces
If I take a look at those faces, in paraview, they look quite good to me:
My question is: if these faces are bad, can I skip them from the computation some how, because I cannot regenerate the mesh, and they are so few?
It is not the faces themsevles
It is not the faces themsevles, but the connection between the cells (or the cell and the boundary) that is "skew".
You should still be able to run despite the warning. Just keep in mind that interpolations and gradient calculations on these faces will be in error. Exactly how wrong will depend on local flow conditions, but in general I wouldn't worry too much about skewness, no one else seems to.
On the other hand, if the skewness on interior faces goes past 1000% then you might have more serious problems.
Beyond accuracy, skewness can
Beyond accuracy, skewness can seriously effect convergence as well. Bad skewness remove most of the implicitness of the operator computations in those cells (i.e., less goes into the matrix and more goes into the RHS). Depending on the type of solver you are using, this more explicit nature of the operator calculations can lead to slow/erratic convergence or complete instability of the solution.
Of course, if the skewed cells are away from areas of significant flow gradients, this is not going to be much of a problem.
Thank you Eugene, Though, whe
Thank you Eugene,
Though, when I check the mesh with (Gambit, Tgrid, Fluent), the skewness is below 0.87. How it becomes more than 3 (333%) in OpenFOAM? Probably, the definition of skewness is different in Tgrid than in OpenFOAM.
Bottom line, if you say that below 1000% it will work, I will no longer worry about it.
But do you know how to run computations only on a certain range of cells and not all of them?
Michael: Stability is only an
Michael: Stability is only an issue if you actually do skewness correction. While ommitting skewness correction reduces the formal accuracy, it tends to cause convergence problems as you say. In my experience it is generally a better idea to just leave out skewness correction, since a large skewness error will also lead to a higher likelyhood of instablity if the correction is applied. (By default most OpenFOAM fvSchemes dictionaries do not apply skewLinear interpolation.)
Dragos: You could delete the cells connected to these faces using setSet/cellSet and subsetMesh. There is no functionality to just disable cells, you have to remove them from the mesh. I don't think it is necessary with this mesh though.
Can anybody please tell me why definition of skewness is different from gambit and fluent ? If not why then please tell me relation between gambit skewness and OpenFOAM skewness. for gambit, I know formulas by which it finds cell skewness. I am looking for same kind of formulas for OpenFOAM. Thank you very much.
could you explain in more detail how to use setSet/cellSet and subsetMesh with that scope?
Thanks a lot in advance
|All times are GMT -4. The time now is 09:29.|