Non-orthogonal correction in SimpleFOAM
 

I am using a non-orthogonal mesh in the calculation. I tried to put the nonorthogonal as 1 to add some correction. But when I read the code of simpleFoam. I can not understand what difference it can make. It seems the correction just solve the matrix one more time, with little change in the matrix. The change of the matrix is only from

pEqn.setReference(pRefCell, pRefValue)

So I cannot understand what is going on with the non-orthogonal correction. Can any one explain it? Thanks a lot.

Best,

Non-orthogonal correction is not recommended for steady-state solvers as it is not needed to have a converged solution every time-step. Just put it to 0 and set limiters in your fvSchemes file in order to handle a non-orthogonal mesh.

Hi Cedric,

Thanks for your reply. Do you mean I only need to apply the correction in the laplacian terms. For example

laplacian (phi, *) Gauss linear corrected

Thanks a lot.

Best,

If your max orthogonality is < 60, you can indeed use "Gauss linear corrected" for your laplacian scheme, if higher you can use "Gauss linear limited 0.333". Your snGradScheme has to be edited accordingly (either corrected or limited 0.333). You can also limit the other schemes.

For example:

Thanks a lot, Cedric.

In your example, you used
gradSchemes
{
default cellLimited Gauss linear 1;
}

This is my first time to know there is a cellLimited scheme. I am curious about the difference between cellLimited and other limited schemes? If possible, could you also explain what is the function of the numbers following the limited scheme.

Thanks again.

Best,

Limited versions of any of these 3 base gradient schemes (Gauss, leastSquares and fourth) can be selected by preceding the discretisation scheme by cellLimited (or faceLimited),

e.g. a cell limited Gauss scheme,

grad(p) cellLimited Gauss linear 1;

for more details you can refer http://www.openfoam.org/docs/user/fvSchemes.php (4.4.3 Gradient schemes)

This very nice document illustrates a lot about the choice of schemes, under-relaxation, pre conditioners for OpenFOAM.
Special treatment for non-orthogonal meshes.
very well said "Who owns the mesh, owns the solution!!"
http://www.dicat.unige.it/guerrero/o...sandtricks.pdf

Hi all,
I can't find the document that FlowAlways has post.
Has anybody still got this document ?
thank you,
Adrien

Hi all,
I've found one which was maybe the same posted before.
Here is the one I've found :
http://www.dicat.unige.it/guerrero/o...sandtricks.pdf
If anyone has oneother, I would appreciate to have it also.
Have a nice day,
Adrien

Hi Adrien, it seems the pdf u shared is again gone.. could u plz share it again?

You'll find the pdf here: http://www.wolfdynamics.com/tutorial...ut=edit&id=163 ("Tips and tricks")