[FFD]

Hello,
My geometry is a kind of a helix. The flow flows through the helix.
So I made a mesh in Ansys Meshing and I have very high skewness values.

I have about 10.000.000 cells
My min. Skewness is: 1,71641165032099E-05
My max. Skewness is: 0,999397641071006
No matter what I try. My skewness is always round about 0.999.

I selected as preset: CFD, relevance is 100 and everything is set to pretty fine.
Many said that the Inflation might cause problems. I tried it turned on program controlled and off. Both had similar results.

So I looked up at cfd-online already and tried some of the tips.
I provide some pictures with a very high skewness cells.
To the names of the pictures: W_Prism is with turned on Inflation and WO_Prism is with turned off Inflation.
Any suggestions on how to fix these cells?
Thank you in advise.
FFD

[Kapi]

mate,
try to give edge sizing at those points and make sure you keep behavior as "hard". Try and give 2-3 element across

[arulmechmb]

Could you try with structure mesh


Sent from my SM-J700F using CFD Online Forum mobile app

[CeesH]

well-defined cylindrical bodies I'd advise to mesh with sweep meshing. This will take some pre-processing, since you need to split the domain in a few easily sweepable bodies (and always, a poor cylindrical core which has to be filled with tets or poorly structured hex anyway, but it typically does end up better than fully unstructured)

Otherwise, merge the faces on both sides of the line in geometry do that you don't force the cells to collapse exactly on that line. In that case, I highly recommend transforming to a polyhedral mesh in FLUENT - it's much faster than using unstructured tets.

[FFD]

What do you mean with sweep Mesh?

The other case you suggest is to merge the high skewed cells? How could I do it in Ansys?

[CeesH]

sweep meshing is a way to create structured hexahedrals in a well-defined domain (which has a constant size in at least 1 direction). You can find it under mesh -> methods in ANSYS mesher, but it only works for certain types of bodies (you can check by right clicking mesh, and tick "show sweepable bodies")

[FFD]

I gonna try it. I tried now to convert my mesh into a polyhedral mesh. The simulation is converging. But I do have a reversed flow in my outlet, which I wouldn't expect there to be, as I do have a laminar flow through a helix. Is it a Mesh issue or is it now an Issue with my model?

[CeesH]

also with laminar flow, there could be vortices at certain points in the domain. If these locations coincide with the inlet or outlet you can get flow reversal. It could be physical or numerical, that's up to you to evaluate. HOw is the mesh quality with polyhedra? if that works fine, you might as well stick to it - personal experience with poylmesh so far is very good (although I have not used it extensively). Previously, I frequently went to great efforts to make large parts of the mesh sweepable and hence filled with structured hex, only using unstructured tet for really curved complex sections. For some more recent projects, I just filled the complete thing with polyhedrals - saving a lot of meshing time.

[FFD]

But the convergence isn't a sign that my mesh is fine?

[CeesH]

It certainly is a start, but a converging solution is not necessarily an accurate solution.

A quick comparison of some work I did recently on a mixing tank: I made 3 meshes:
Full tetrahedral -- 2000k cells - max skewness 0.8 - time/1000 iter (12 cores) 1200 seconds
Mixed hex-tet -- 600k cells - max skewness 0.92 - time/1000 iter (12 cores) 450 seconds
Fuill polyhedral -- 500k cells - max skewness 0.46 - time/1000 iter (12 cores) 600 seconds

I did not compare the quality of the solutions yet for this case, but from what I've seen so far, quality of poly is better than both hex and tet at equal cell count. In any case, however, a mesh dependency study is still needed.

[EdgarG]

Have you try use spheres of influence in the high skewness zones?