Hello,

I am having a dilemna :

either I make a calculation with a mesh with some cells having a skewness of 0.98 or I change the mesh at the same place for a non conformal mesh and reduce the skewness.

What solution is best to reach convergence?

Thank you in advance.

Eduardo

I would say non-conformal is better than .98 skewness. You really don't want either in an area of complicated flow though. Can you supply any geometry info and maybe we can find a way to mesh it without either?

Jason

You do not have choice really, with high skewness, on solvers you will not get converged solution. The only solver, that remains stable is fluent, all the other solver simple diverge with high skew. Fluent remains stable by creating lot of error in solution, so the only option is to use non conformal mesh.

Well.

to answer Jason, I have been meshing my geometry for one month trying to change all what was possible to change and best I can have is 0.97. So, what would you consider a maximum skewness for a fluent calculation to converge? As for zxaar, thank you, if I don't manage to reduce the maximum skewness to 0.9, then I'll try the non-conformal mesh.

Eduardo

i persoanlly avoid non-conformal meshing as much as possible. and it is not because that this is bad approach, but because my cases are large and we are forced to use parallel processing. With the parallel processing , fluent gives lot of trouble with nonconformal meshes. Shoots up in the velocity vectors are easily observable where as some cases the non-conformal interfaces starts to behave like a wall. We discussed this issue with our fluent support and it seems there is no cure for it for the moment. however the same problem do not come with fluent6.1 version. (but fluent6.1 has another problem that with interfaces it may not read the mesh even in parallel mode).

My advise would be try to get best mesh without non conformal meshes, but if you fail then use interfaces.

I agree with zxaar.

As for maximum skewness, stay below 0.9 (of course the lower you get the better).

I have a lot of experience meshing imported geometries that create highly skewed elements. If you send me a couple pictures of the problem area I might be able to recommend something.

Good luck, Jason

Hello.

OK, I have managed to reduce the skewness of my mesh. Now, I have a cell with a skewness of 0.94 and it is the only one above 0.9 on a 4 million cells mesh.

Would you now consider non-conformal mesh or this mesh for the calculation?

Thanks in advance.

Eduardo

It really depends on where it is. If it's in an area of complex flow, then it's going to take on a lot of error. If it's in an area of pretty uniform flow, then there really isn't anything there to cause it to build up the error. I've run one model up to .95 skewness in a corner where it was in separated flow. I don't recommend it, but I didn't have enough background in meshing at the time, so I dealt with it. If you have enough Fluent licenses, I would say start running with the mesh you have, and while its running try improving the mesh. Also, you can take a look at the model as its running and looking for areas that are giving your problems and improve the mesh. Then you can interpolate the solution on from the old mesh onto the new mesh so you don't have to iterate from scratch again.

Hope this helps, and good luck, Jason

is it not possible to read this one or two bad skew mesh and ask fluent to adapt it on that region and improve the mesh in that region. So when the fluent adapts it shall divide the mesh such that the skew will be correct. Try venturing into this area.