CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   k-omega-SST breakdown with high resolution mesh (http://www.cfd-online.com/Forums/openfoam-solving/87700-k-omega-sst-breakdown-high-resolution-mesh.html)

romant April 27, 2011 01:58

k-omega-SST breakdown with high resolution mesh
 
Lately I ran into problems using buoyantBoussinesqSimpleFoam together with the k-omega-SST model by menter when I increase the mesh resolution in order to find mesh independency.

when the cell count gets too large the whole simulation breaks down, it does not converge, and there is neither heat transfer in the annulus nor does the velocity field fully develop. the curious thing about it is, that with higher inlet velocities, this cell count can be higher,

has anyone an idea, why this could be and/or if there are limitation in the usage of kOmegaSST?

romant May 5, 2011 05:20

updated bug report for this
 
maybe somebody has an idea. here is also the updated bug report:

http://www.openfoam.com/mantisbt/view.php?id=179

the solution is in the bug report. but for clarity, if someone wants to run the kOmegaSST in OpenFOAM in low Re mode, the following should be considered:

http://www.openfoam.com/mantisbt/view.php?id=179#c351

quote from henry:

Note that the k-omega SST model we provide is in high-Re form and does not include the wall-damping terms often included in the k-omega model for near-wall and low-Re flow. However, you can still use the k-omega SST model for low-Re and near wall flow for a range of resolutions if you use a continuous wall-function (which in OpenFOAM-1.7.x is named nutSpalartAllmarasWallFunction for historical reasons) and this should be used as the wall BC in nut. The BC of k for the continuous wall-function should be kqRWallFunction.

If these changes do not help it may be worth investigating the viscosity averaging in omegaWallFunctionFvPatchScalarField:

scalar omegaVis = 6.0*nuw[faceI]/(beta1_*sqr(y[faceI]));
scalar omegaLog = sqrt(k[faceCellI])/(Cmu25*kappa_*y[faceI]);
omega[faceCellI] = sqrt(sqr(omegaVis) + sqr(omegaLog));

we have found cases for which this causes a sudden change in the viscosity near the wall if the mesh is sufficiently fine and that just using the logarithmic part give more continuous behavior:

omega[faceCellI] = omegaLog;

timo_IHS January 13, 2012 15:20

Hallo Roman,

do you still have this problem?
I also encountered problems with convergence with finer meshes for the kOmegaSST model.
The problem comes, since the modification of nut with sqrt(2) was introduced about one year ago.

nut_ = a1_*k_/max(a1_*omega_, F2()*sqrt(2.0)*mag(symm(fvc::grad(U_))));

Without this factor sqrt(2) there is no problem with convergence, but the results are poorer compared to CFX.

An unevaluated thesis of me is, that this factor is additionally not used in some areas. And/or there should be a slightly modification in the omega-equation (only in some areas), instead of:
2*gamma*S2
-->
gamma*omega/k*P
(or similar, sorry it is friday evening)

as you can see in:
Development and Application of SST-SAS Turbulence Model in the DESIDER Project, of Egorov and Menter

Are there any comments on that?

vkrastev February 19, 2012 09:14

Hi all,
I have opened a tread about this issue here:

http://www.cfd-online.com/Forums/ope...estigated.html

Regards

V.

cm_jubayer July 3, 2012 16:21

Hi Roman,

Have you resolved the issue with this high resolution mesh with buoyantBoussinesqSimpleFoam solver and k-omega SST model? I am facing a similar problem. For my wind loading on solar panel problem, I have used pisoFoam solver k-omega SST without any problem. However, for my heat transfer problem, I increased the mesh resolution close to the surface of the panel (y+<5) and used buoyantBoussinesqPimpleFoam solver. My simulation is blowing up (large negative bounding values for k and omega). I have tried various schemes in fvschemes but still could not find a solution. What else should I consider for making my simulation converge?

Jubayer

romant July 4, 2012 02:44

Hej Jubayer,

I have found a solution that is more or less connected to the smoothness of the mesh. If the cell growth is too larger close to the wall, you will end up with a non-physical solution and/or blowing up solution.

I made sure that the cell growth is only 1.1 close to the wall and going towards the core one could increase the cell growth. In snappyHexMesh this is solved by actually using the right amount of boundary layers with a slow growth. In blockMesh, one would need to use different block towards the core of the flow and use a block with very smooth grading towards the wall.

cm_jubayer July 4, 2012 11:45

Thanks Roman. I'll definitely try smoothing my mesh.


Jubayer


All times are GMT -4. The time now is 02:21.