
[Sponsors] 
June 21, 2010, 06:32 
Nonlinear turbulence model NonlinearShih

#1 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 10 
Hi all,
I've simulated a fully developed channel flow with the nonlinear shih model. The residuals are quite good (R<10e7). But looking at the pressure it isn't constant over the channelhight and looking at the veloicty in ydirection, they are nonzero. I have simulated this channel flow with a lowReynoldsturbulence model and showed the different results in the following plot. I have seen results that look nearly the same with the LRR model... Maybe it's because of the pressure near the walls. For BC I'm using zeroGradient for walls and the outlet, for inlet a fixed Value. I'm using OpenFOAM 1.6 with directMapped bc's for U,k,epsilon at the inlet. The solver is simpleFoam. If someone has any hind please let me know. Best regards, Thomas 

July 15, 2010, 03:13 

#2 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 10 
Hi all,
I have simulated a fully developed channel flow using the solver boundaryFoam. Here I have no problems and I get good results using for turbulence modelling NonlinearKEShih or the LienCubicKELowRe. But starting a simulation with simpleFoam or pisoFoam I get bad results as described above. Has anybody solved any flow with walls without this problem using simpleFoam or any solver regarding convection? Thanks a lot, Thomas 

July 23, 2010, 10:52 

#3 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 10 
Hi all,
I'm nut sure, but could it be the problem of the simple or the pisoalgorithm? I have seen in buoyantboussinesqSimpleFoam that if an additional term is added in the Uequation (here the buoancyterm), that this term has to be added as flux in phi, too. In the NavierStokesequations I get here the additional buoancyterm: g*rho_delta in the Uequation. And the flux phi is corrected with this term, which is needed for the pequation: surfaceScalarField ghf("ghf", g & mesh.Cf()); surfaceScalarField buoyancyPhi = rUAf *ghf*fvc::snGrad(rhok)*mesh.magSf(); phi = phi  buoyancyPhi; ... Normal turbulence models like the kepsilon are modelling the turbulence isotropic and because of that, the Reynoldsstresses have not to be regarded in the poissonequation of the pressure, the same as the viscous stresses. You get the poissonequation by div(NavierStokesequations). But in nonlinear turbulencemodels and algebraic stress models they are nonzero. So I have to split my turbulence in a isotropic and the nonisotropic part. And I have to calculate a phi_nonisotropic and have to add it to the phi. I'm not sure if that's right. Can anybody help me? Thank you very much, Thomas Regards Thomas 

August 5, 2010, 05:17 

#4 
Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 10 
Hi all,
I have modified the mySimpleFoamsolver to calculate the residuals of continuityequation about div(U) and the orginal one div(phi), too. The residuals of div(phi) are about 10^09, but the residuals of div(U) are about 0.7 If I'm simulating using an isotropic turbulencemodel for example the LaunderSharma I get div(phi) are about 10^09, the residuals of div(U) are about 10^04. So they are much better here. The problem of the simple and the pisoalgorithmus is, that they are calculating the the pressureequation using phi. fvScalarMatrix pEqn ( fvm::laplacian(1.0/AU, p) == fvc::div(phi) ); and correct the fluxes afterwards if (nonOrth == nNonOrthCorr) { phi = pEqn.flux(); } I have seen in the posting http://www.cfdonline.com/Forums/ope...odyforce.html that you can built an additional force to the NS and pressureequation. So could it be possible to solve the divdevReff of the turbulencemodel isotropic and add the additional explicit nonlinearpart like a force? Regards Thomas 

August 30, 2010, 09:48 

#5 
New Member
Olli
Join Date: Mar 2010
Location: Berlin
Posts: 13
Rep Power: 9 
Hi Thomas,
maybe there is something wrong with your BC's. I used the anisotropic model and it works perfectly for my needs. I used the following BC's: U: INLET { type fixedValue; value uniform (.619552 0 0); } WALL { type fixedValue; value uniform (0 0 0); } OUTLET { type zeroGradient; } p: INLET { type zeroGradient; } WALL { type zeroGradient; } OUTLET { type fixedValue; value uniform 0; } epsilon: INLET { type fixedValue; value uniform .0003532; } WALL { type zeroGradient; } OUTLET { type zeroGradient; } k: INLET { type fixedValue; value uniform .000605; } WALL { type zeroGradient; } OUTLET { type zeroGradient; } nut: INLET { type calculated; value uniform 0; } WALL { type nutWallFunction; value uniform 0; } OUTLET { type calculated; value uniform 0; } nuTilda: INLET { type fixedValue; value uniform 0; } WALL { type zeroGradient; } OUTLET { type zeroGradient; } Is your mesh 2d or 3d? Are the dimensions/scaling of the domain right? Are the results mesh independent? What is the Reynoldsnumber? ... This would be some questions I'd usually ask. Best regards, Olli 

November 29, 2016, 12:00 

#6  
Member
António Soares
Join Date: Mar 2015
Location: Lisbon, Portugal
Posts: 35
Rep Power: 4 
Greetings,
I'm trying to use the Nonlinear Shih ke model in porousSimpleFoam. I'm missing something in the divScheme part of the fvSchemes file but I don't know what I have to add (all I know is that it has something to do with the nonlinear term). The error message is as follows: Quote:
Any help would be appreciated. 

November 29, 2016, 13:09 

#7  
Member
António Soares
Join Date: Mar 2015
Location: Lisbon, Portugal
Posts: 35
Rep Power: 4 
OK, so i just added the following line to the fvSchemes.divSchemes:
Quote:
However, I'm still getting the following error message on the first time step: Quote:


November 29, 2016, 15:25 

#8  
Member
António Soares
Join Date: Mar 2015
Location: Lisbon, Portugal
Posts: 35
Rep Power: 4 
OK, so I tried the following and so far it seems to be working (although beats me if it actually is the proper scheme):
Quote:


December 16, 2016, 18:11 

#9 
New Member
Javier Martinez
Join Date: Nov 2012
Posts: 2
Rep Power: 0 
Dear Thomas,
I don't know if you got to solve your problem or if you keep working in OF, but I am finding the same issue in recent versions (ofdev), I guess it was never solved. As you commented for fully developed channel flow vertical velocity is not zero. Pressure distribution should not be zero since dp/dy should account for the contribution of Re stress terms:  dp/dy = d(uv)/dx + d(vv)/dy, and those terms are not zero when non linear models are considered. However, due to continuity vertical velocity should be perfectly zero everywhere. When boundaryFoam is used the devReff term in velocity equation is not entirely considered, but it is projected in the direction of the flow), therefore no problem appears. However when simpleFoam is used the problem you mentioned of nonzero vertical velocity does appear for nonlinear models. I have been playing myself to try to find out the problem: I played first with solving tolerances, mesh distribution (uniform or nonuniform), all kinds of schemes, periodic conditions (empty for 2D or cyclic 3D)... I also tried to separate the nonlinear from the linear part (recalculating all terms in the solver and adding manually the terms to the velocity equation) to make sure the nonlinear part was added correctly. However the problem is still there. SIMPLE algorithm should work since the nonlinear stress contribution is added to the source of the velocity equation, and is therefore considered in the HbyA, which is used by the pressure equation to satisfy continuity. Therefore I don't know what else could be failing. I also tried to add Majumdar correction to the traditional RhieChow method used in simpleFoam, but it didn't change the problem. Please let me know if anybody figured out what could be going wrong. I checked the behavior of nonlinear models in other commercial codes and they don't suffer from this problem. Best regards, Javier 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Superlinear speedup in OpenFOAM 13  msrinath80  OpenFOAM Running, Solving & CFD  18  March 3, 2015 06:36 
SimpleFoam case with SpalartAllmaras turbulence model implemented  nedved  OpenFOAM Running, Solving & CFD  2  November 30, 2014 23:43 
Adding a Turbulence Model  doug  OpenFOAM Running, Solving & CFD  10  October 2, 2012 06:55 
KOmega Turbulence model from wwwopenFOAMWikinet  philippose  OpenFOAM Running, Solving & CFD  30  August 4, 2010 10:26 
v2f turbulence model in CFX?  flga  CFX  14  November 23, 2006 07:12 