CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

k-omega-SST breakdown with high resolution mesh

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 27, 2011, 01:58
Default k-omega-SST breakdown with high resolution mesh
  #1
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 360
Rep Power: 12
romant is on a distinguished road
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?
__________________
~roman
romant is offline   Reply With Quote

Old   May 5, 2011, 05:20
Default updated bug report for this
  #2
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 360
Rep Power: 12
romant is on a distinguished road
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;
__________________
~roman

Last edited by romant; May 5, 2011 at 06:56. Reason: change in bug status
romant is offline   Reply With Quote

Old   January 13, 2012, 15:20
Default
  #3
Member
 
Timo K.
Join Date: Feb 2010
Location: University of Stuttgart
Posts: 66
Rep Power: 7
timo_IHS is on a distinguished road
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?
timo_IHS is offline   Reply With Quote

Old   February 19, 2012, 09:14
Default
  #4
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Hi all,
I have opened a tread about this issue here:

Why Menter's SST model low-Re issue has not been seriously investigated?

Regards

V.
vkrastev is offline   Reply With Quote

Old   July 3, 2012, 16:21
Default
  #5
Member
 
Jubayer
Join Date: Oct 2009
Location: The University of Western Ontario, London, Ontario
Posts: 42
Blog Entries: 1
Rep Power: 7
cm_jubayer is on a distinguished road
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
cm_jubayer is offline   Reply With Quote

Old   July 4, 2012, 02:44
Default
  #6
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 360
Rep Power: 12
romant is on a distinguished road
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.
__________________
~roman
romant is offline   Reply With Quote

Old   July 4, 2012, 11:45
Default
  #7
Member
 
Jubayer
Join Date: Oct 2009
Location: The University of Western Ontario, London, Ontario
Posts: 42
Blog Entries: 1
Rep Power: 7
cm_jubayer is on a distinguished road
Thanks Roman. I'll definitely try smoothing my mesh.


Jubayer
cm_jubayer is offline   Reply With Quote

Reply

Tags
heat transfer, komegasst, turbulence

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
larger blend factor or high resolution ? amine CFX 2 March 4, 2008 21:28
upwind vs high resolution Richard CFX 3 February 20, 2006 07:35


All times are GMT -4. The time now is 09:19.