# Problem running simpleFoam with kOmegaSST turbulence model

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

 November 1, 2012, 08:02 Problem running simpleFoam with kOmegaSST turbulence model #1 New Member   MB Join Date: Sep 2012 Posts: 29 Rep Power: 6 Hello, I'm trying to run a channel-case (4m^2) with a smaller cross-section (0.05m^2) in between. My boundary-conditions are: Code: ```inlet_velocity (0.3 0 0) inlet_pressure zeroGradient inlet_k uniform 2e-04 inlet_omega uniform 0.2 inlet_nut uniform 0 outlet_velocity zeroGradient outlet_pressure uniform 0 outlet_k zeroGradient outlet_omega zeroGradient outlet_nut uniform 0 wall_velocity (0 0 0) wall_pressure zeroGradient wall_k kqRWallFunction uniform 2e-04 wall_omega omegaWallFunction uniform 0.2 wall_nut nutkWallFunction uniform 0``` fvSchemes: Code: ```ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss linear; div(phi,k) Gauss linear; div(phi,omega) Gauss linear; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; }``` and finally fvSolution: Code: ```solvers { p { solver GAMG; tolerance 1e-06; relTol 0.01; smoother DICGaussSeidel; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 50; mergeLevels 1; } U { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0.1; } k { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0.1; } omega { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.3; } equations { U 0.7; k 0.7; epsilon 0.7; omega 0.7; nuTilda 0.7; R 0.7; } }``` The problem is that the calculation diverges with bounding k and omega. Any suggestions?

 November 1, 2012, 09:23 #2 Senior Member     Vieri Abolaffio Join Date: Jul 2010 Location: Always on the move. Posts: 308 Rep Power: 9 can you post images of the mesh? have you tried to visualize where the k and omega rises to high values? __________________ http://www.leadingedge.it/ Naval architecture and CFD consultancy

November 1, 2012, 10:15
#3
New Member

MB
Join Date: Sep 2012
Posts: 29
Rep Power: 6
Quote:
 Originally Posted by sail can you post images of the mesh? have you tried to visualize where the k and omega rises to high values?
there is no defined location where the k and omega values reach the high values. it depends on the timestep... attached you can find two screenshots of a slice through the fluid domain.
Attached Images
 slice1.jpg (75.6 KB, 40 views) slice2.jpg (97.5 KB, 43 views)

 November 1, 2012, 18:15 #4 Senior Member     Vieri Abolaffio Join Date: Jul 2010 Location: Always on the move. Posts: 308 Rep Power: 9 mmm the mesh looks good from here, are the layers correctly added even in the corners? maybe increasing the number of nonOrtogonalCorrectors in the simple loop? if the issue arises in the early timesteps you might want to try to increase the value of the initial omega internal field to artificially stabilize the solution. this is what comes to mind right now... __________________ http://www.leadingedge.it/ Naval architecture and CFD consultancy

 November 2, 2012, 18:31 #5 New Member   MB Join Date: Sep 2012 Posts: 29 Rep Power: 6 tried to solve it without turbulence, but also no convergence. I have no idea what the problem is...

 November 3, 2012, 07:45 #6 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Delft, Netherlands Posts: 326 Rep Power: 12 Hi, Just looking at your fvSchemes, try changing: Code: ```divSchemes { default none; div(phi,U) Gauss linear; div(phi,k) Gauss linear; div(phi,omega) Gauss linear; div((nuEff*dev(T(grad(U))))) Gauss linear; }``` to: Code: ```divSchemes { default none; div(phi,U) Gauss GammaV 0.5; div(phi,k) Gauss Gamma 0.5; div(phi,omega) Gauss Gamma 0.5; div((nuEff*dev(T(grad(U))))) Gauss linear; }``` You are now introducing some filtering, because I doubt that you have the required resolution (Cell Reynolds number <2) for pure central differencing (linear scheme). Or maybe look at limitedLinear instead of Gamma. You may even want to use upwind for the turbulence variables if that is needed for convergence, to my experience the end result is not affected significantly. Especially if you have a lot of nonOrthogonality this may help: Code: ```laplacianSchemes { default Gauss linear limited 0.333; }``` Regards, Tom blake likes this.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post chiven OpenFOAM Bugs 7 August 23, 2011 02:52 nileshjrane Main CFD Forum 7 September 14, 2010 04:57 nileshjrane OpenFOAM Running, Solving & CFD 1 September 7, 2010 17:48 svens OpenFOAM 3 August 21, 2009 02:59 Senthil Main CFD Forum 4 July 5, 2000 04:34

All times are GMT -4. The time now is 21:44.