[aerothermal]

Hi maddalena,

Now my problem is converged but I am looking to improve the results, mainly the separation point location for the cylinder flow. You were right. Part of the problem was the boundary conditions and part the mesh.

I already converged and validated CFD++ results agains the experimental data for Cp and Nu of a rough cylinder. However, I am struggling to find an accurate configuration for OpenFoam.

Could you post your final fvSchemes and fvSolution?
I may help me

My final results for rhoSimpleFoam will be posted on-line as a wiki when I finished it.

Regards,

Guilherme

[maddalena]

Hi,

Originally Posted by aerothermal

Could you post your final fvSchemes and fvSolution?

well, everything is posted here. If you want the original files, give me some time since this analysis is two years old and I need to find them on my backup harddisk...

mad

[aerothermal]

Hi maddalena,

Could you tell me if your last successful configuration was the one described ?http://www.cfd-online.com/Forums/ope...tml#post212960

What solver and preconditioner did you choose in fvSolution for each variable?

I tried to put Gauss upwind in div((muEff*dev2(grad(U).T()))) but OF1.7 gave a EOF error on that line. If I chosse Gauss linear, it runs OK. What did you use there?

Thanks,

aerothermal

[s.m]

Originally Posted by maddalena

Dear Maruthamuthu, Dear Daniel,

thanks for your support and advices. Here there are some answers (and some more questions as well...):

1) I have some problems to apply Fluent boundary condition for turbolence exactly. In fact, if I use converged Fluent value for k and epsilon both in boundaries and in internalField, my simulation does not converge, in the meaning that cl and cd values oscillate giving meaningless results (negative cl, for example). The main reason for that is that epsilon value is not sufficiently uniform within the domain and has to be bounded by simpleFoam. Using the trick of an epsilon two order of magnitude lower within the domain let the simulation converge.

2) At the moment, I am using realizableKE model for turbolence, both in OF and in Fluent, with the same (the defalut) realizableKECoeffs. There is not any stagnation correction modelled in it.

3) I am running a Hi-Re model, and my yPlusRAS -latestTime check says that: […] Patch 3 named surf y+: min: 0.322683 max: 13.9875 average: 2.08982. In any case, I remeshed my domain to obtain a grid with a max y+ around 25, the simulation is running... stay tuned for updates!

4) I know that low-Re models should be applied when the turbolent Reynolds number is low enough and viscous effects are important. However, I am wondering if there is a sort of correlation between the turbolent Reynolds number and the flow Reynolds number, i.e.: in which Re range should I use a Hi-Re model or a Low-Re model? In any case, I have some doubts that a low-Re model is the right one for my case, since the what I'd like to simulate is not only stall and post stall, but also the behaviour with low AoA, with no flow separation.

5) Of course, I can see a small boundary layer around my wing...

6) And... I changed my div(phi,U) to div(phi,U) Gauss linear. Thanks.

After a closer comparison of p, U, k and epsilon countour plot obtained with OF and Fluent converged simulations, I can add that:

1) p max and min values are not the same in OF and Fluent, however the data range (pmax – pmin) are almost the same.

2) U range are the same.

3) Epsilon and k values are way too low in the OF converged solution, and I think this is the main reason of my low aerodynamic coefficients. Maybe the above trick helps to let the solution converge, but towards wrong values...

However, I am not puzzled by numerical values... well... not only from them. I think that the most strange result is an attached flow for such a high AoA as 24°. I agree that the turbolence model could be not the right one for this kind of problem, but... I expect that the flow separates in any case! Is this strictly connected with my low k and epsilon values? Or maybe should I change my solver e.g. turn to turbFoam?

Cheers,

Maddalena.

Hi Maddalena,
would yo please explain more about the trick that make your simulation converged?
this sentence "Using the trick of an epsilon two order of magnitude lower within the domain let the simulation converge. "
thank you very much.

[s.m]

Originally Posted by maddalena

Hello FOAMers,
in order to obtain better convergence and results closer to Fluent for my external aerodynamic simulation, I changed one more time my fvSchemes, following some suggestions I had from HRV. Now it looks like this:

• gradSchemes: faceMDLimited Gauss linear 0.5;
• divSchemes: Gauss GammaV 1 on div(phi,U); Gauss upwind everywhere else.
• laplacianSchemes: Gauss linear limited 0.33 on laplacian(DepsilonEff,epsilon), Gauss linear limited 0.5 everywhere else.
• interpolationSchemes: linear;
• snGradSchemes: limited 0.5;

Moreover, I increased tolerance and relTol for every variable:
{
...
tolerance 1e-09;
relTol 0.01;
}
This helped me to obtain better numerical convergence. However, a certain difference between OF and Fluent still remain (alpha = 8°):

• Fluent:
  • CL: 0.6317
  • CD: 0.0870
  • pmax:137
  • pmin:-199
• OF:
  • CL: 0.6596
  • CD: 0.0522
  • pmax: 115
  • pmin: -179

I could not find a numerical set-up or domain discretisation that allows me to obtain a smaller gap between the two solvers, so I can say that this is the best I could have with the standard OF distribution for a case similar to mine.
Since Fluent results are closer to experimental values, I can conclude that OF 1.5 underestimates aerodynamic coefficients as a consequence of a numerically different pressure field around the wing.
Please, feel free to add anything in addition to this.
Regards,
Maddalena

Hi Maddalena
Thank you very much, for sharing good information for us. whould you please tell me what was your solver for p and U for this set up, that you get good results?
thank you again.
Regards.

[s.m]

Originally Posted by alberto

Hi,

the mesh is OK.



That should be possible.
The -extend 1.6 release has the reconCentral scheme, which should improve this. Some time ago I took the freedom of compiling it for 1.7.x (see attachment). You can use it as interpolation scheme (add the library to controlDict) with the cellLimited option for gradients.



It depends on the meshing tools you have. ICEM can do that, Harpoon does that, CD-Adapco has a tool to do that too. OpenFOAM has snappyHexMesh, which is a bit painful to use, if your geometry has a lot of borders that have to be well defined.

Best,

Dear alberto,
as i read in this frum, you admit the vessilen's mesh with "Max skewness = 1.98187"
my question is: in gambit or fluent skeness 0.9 is really high but in openFoam skewness 2, or even more is OK, what is the difference between their definition?
what is the upper limite for skewness?

Thank you very much