Openfoam is not succesful for tetrahedral meshes
Hello everyone,
For a long time, i am experiencing OF with cases which are unstructured tetrahedral meshes. Those cases are really meshed very well including boundary layers and refined local regions. Cases are for external flow analysis, mostly transonic regime. Even though i tried lots of settings, i cannot run cases correctly. Whatever i tried is not good enough for tetra meshes. It seems OF works well with only hexa meshs, for best snappyHexMesh should be adviced. Prof. Jasak advices reconCentral for tetrahedral meshes but it did not help me at all. Likewise pointLinear shows some improvements, but it is not enough too. Is there anyone who can claim that i can run external flow dynamic cases which are made of tetrahedral meshes ?? I am really curious about what you got achieved? Sorry for tough attitude, but the results make me really pissed off. Have good days! Edit: I can share a constant and 0.orig file, if you let me know how to share 80 mb zip file. |
Hey, ... donīt be pissed of :) ... other software toolboxes for which you pay a lot of money are even more crazier - maybe not in that particular regard but in other topics.
Can you show us the fvSolution, fvSchemes and controlDict file? |
3 Attachment(s)
Hi Tobi,
I second the above opinion about tetrahedral meshes but have no problems in accepting your assertion about other software toolboxes :) Coming to the topic, I have also observed that hex meshes (from snappy or other software) perform far better in terms of convergence behavior with turbulent flows. I haven't gone to the extent of modifying reconCentral scheme for OpenFOAM standard version but tried a few other things with the numerical schemes. The best performance so far was obtained with the combination: Would you please give me some suggestions? Thanks very much, -Kumar |
Hey, ...
the schemes do look okay. However, the gradient scheme could be modified by using the cell or edge limiter. Gradients should be calculated corrected in order to get correct results. Furthermore, nCorrectors could help stabilizing the solution within one SIMPLE iteration (not sure right now which solver you are using but for simpleFoam we donīt have that option). And I second you. Hex-Meshes are great for numerical simulation but are not applicable always. By the way, Fluent uses the polygon meshes mostly and the coupled solver. However, the solution will blow up while using other algorithms such as SIMPLE or SIMPLEC. |
Thanks for quick responses.
Sorry but i dont agree about your opinion about Fluent. I mostly use Fluent as pressure-based segregated solver for steady-state external problems. Even though I only use tetra meshs, and most of them are not the best meshes, it can really handle very well. If you can detail your experience about fluent, i will be very grateful. I attached my bcs and schemes. I prepared this settings for 0.84 Mach, 3.03 aoa Onera m6 case. I tried rhoSimpleFoam and rhoPimpleFoam. What i sent is for rhoSimpleFoam case. Thanks for your collaboration. Extra Note: What i sent can handle at some point very well, but after some iteration it just blows up. I refined mesh , problem should be numeric. If you want, i can send the residual plot. |
I forgot to add mesh check result. Here it is. As you can see it fails but it is due to inflation layers.
|
Common practise is to set the laplacian and snGrad to the same scheme (check out kishpishars files). I am not a big fan of the linearUpwind as it also introduces some unphysical behavior.
So my first approach would be:
A comparison of numerical schemes in OpenFOAM, mesh density, cell types and OpenFOAM versions is given here: https://holzmann-cfd.com/community/n...sport-analysis All cases I had in Fluent in HVAC analysis crashes almost after a few iterations using SIMPLE or SIMPLEC algorithm. Even a almost converged solution by using the coupled scheme crashes immediately. However, I will not work with fluent too much anymore, hence, I donīt care :) |
Thank you, i noted everything you said.
Your Convective Schemes Analysis is very helpful, also thanks for that. I am just curious about that have you ever made successful analysis which are fully made up tetrahedral meshes ? |
Honestly, since I am using FOAM, I never used tetrahedral meshes. However, there is a talk on YouTube from Hrv. Jasak. He is talking about tetrahedron meshes and numerics. So in principal I would say, we can work with tet meshes.
|
Quote:
Even in the old days with STARCD and/or STARCCM+ always stayed far away from tet meshes. If you have a tet mesh, can try using its poly dual - should be better. However, the polyDualMesh in OpenFOAM will look a bit dodgy at concave geometry features. To be really useful it would also need some cell splitting there (easy to conceptualize in 2D, not so easy to implement in 3D). |
Quote:
Obvious, I forgot the polyDualMesh application. Nevertheless, I never worked with tet-meshes and hence, no experience. Is it still tricky to work with tets and FOAM? |
Quote:
|
Hi Tobi,
Quote:
In my experience, it is not that tetrahedral meshes are useless with OF, rather it is often the case that convergence is quite bumpy and the residuals don't fall to the same levels as with Hex meshes. It may still be possible to obtain reasonable looking solutions. Here are a few suggestions from my limited experience: Mesh: As far as possible, generate tet meshes with nearly equilateral triangles with smooth size variation. This would make the average non-orthogonality higher compared to Hex meshes, but the maximum non-ortho will be around 60. The solutions might still oscillate but the solver crashes etc. can be avoided. Turbulent model: kEpsilon seems to work better with this type of meshes than the other variants realizable, RNG etc. fvSchemes:
|
Quote:
If you can enlighten us, i'll be very grateful. |
Quote:
All that is written above comes from my experience on fully tet meshes. |
Quote:
|
Quote:
|
I summarized my observations only in the context of steady state incompressible flows using simpleFoam solver.
Quote:
Quote:
Quote:
In a practical sense, aren't such finite volume CFD calculations a trade-off between stability and accuracy? You try to use the combination of schemes that give you the best possible accuracy for the problem at hand while maintaining stable runs.. |
Quote:
Thanks for your kind responses, have good day. |
Hey,
well there are a lot of things to do so I don't think that I am able to create a test case :). Quote:
|
All times are GMT -4. The time now is 15:40. |