
[Sponsors] 
November 1, 2012, 08:02 
Problem running simpleFoam with kOmegaSST turbulence model

#1 
New Member
MB
Join Date: Sep 2012
Posts: 29
Rep Power: 5 
Hello,
I'm trying to run a channelcase (4m^2) with a smaller crosssection (0.05m^2) in between. My boundaryconditions are: Code:
inlet_velocity (0.3 0 0) inlet_pressure zeroGradient inlet_k uniform 2e04 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 2e04 wall_omega omegaWallFunction uniform 0.2 wall_nut nutkWallFunction uniform 0 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; } Code:
solvers { p { solver GAMG; tolerance 1e06; relTol 0.01; smoother DICGaussSeidel; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 50; mergeLevels 1; } U { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } k { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } omega { solver PBiCG; preconditioner DILU; tolerance 1e05; 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; } } 

November 1, 2012, 09:23 

#2 
Senior Member
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8 
can you post images of the mesh? have you tried to visualize where the k and omega rises to high values?


November 1, 2012, 10:15 

#3 
New Member
MB
Join Date: Sep 2012
Posts: 29
Rep Power: 5 
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.


November 1, 2012, 18:15 

#4 
Senior Member
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8 
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... 

November 2, 2012, 18:31 

#5 
New Member
MB
Join Date: Sep 2012
Posts: 29
Rep Power: 5 
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

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; } 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 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; } Tom 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
multiphaseInterFoam for RAS turbulence model  chiven  OpenFOAM Bugs  7  August 23, 2011 02:52 
Turbulence model for mixing problem???  nileshjrane  Main CFD Forum  7  September 14, 2010 04:57 
Turbulence model for mixing problem  nileshjrane  OpenFOAM Running, Solving & CFD  1  September 7, 2010 17:48 
Implementing and running a new turbulence model  svens  OpenFOAM  3  August 21, 2009 02:59 
Why Turbulence models are not universal.  Senthil  Main CFD Forum  4  July 5, 2000 04:34 