
[Sponsors] 
April 20, 2012, 22:39 

#81 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
Well I have read through H.Rusche thesis and the kepsilon model used in the thesis is Gosman's model. I read your earlier posts as well as the bubbleFoam wiki and I can see that Gosmans model is not used in bubbleFoam. My question is why are the source terms for k and epsilon, S_k and S_eps not included in bubbleFoam?
Also my understanding is that Gosman's model is used in twoPhaseeulerFoam? Kind Regards Matt 

April 21, 2012, 05:51 

#82 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
They seem to implement a simpler form of the model than the one from Gosman (in Rusche's thesis they mention that Gosman's model might cause numerical problems).
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 22, 2012, 07:22 

#83 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
Thank you for the responses Alberto your help is always much appreciated.
I think it may be worth my while to have a look more closely at Gosman's model to hopefully determine what his source terms represent. I am currently looking into running the bubbleFoam/twoPhaseEulerFoam bubble column tutorial with turbulence and I cannot seem to get it working, just trying to broaden my understanding of the kepsilon model. I think I have made the appropriate changes to fvSolutions and fvSchemes (added the variables to be solved and the new laplacian terms for the turbulence equations). However my solution blows up after very few timesteps. I am at the moment trying to get the tutorial running with turbulence before I move on to my specific tank geometry (tank with parabolic profile) Matt 

April 23, 2012, 11:30 

#84 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Do you have parts of the system where alpha = 1? If so, the turbulence model implemented in twoPhaseEulerFoam/bubbleFoam is unstable in that limit, since beta > 0.
You might want to consider, depending on your system, a mixture formulation, or to make some change to the implementation to manage the case beta > 0 more robustly. If you need info on this, let me know. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 24, 2012, 04:58 

#85  
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
Quote:
Hi Alberto, I noticed that you have already mentioned the method for making changes to the solver... Are bubbleFoam and twoPhaseEuler the same in terms of turbulence models? Have these 2 solvers undergone much change since previous versions? There are areas of my domain where alpha is equal to 1, so I will definately need to make some modifications here. Kind Regards Matt 

April 25, 2012, 02:47 

#86  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Quote:
For the limit of beta > 0, you can probably define a minimum value of alpha in some term of the equation (see what they do in compressibleTwoPhaseEulerFoam for the drag), or drop the cells where beta < small from the solution, and fix the value of the variable there (risky approach in terms of robustness). Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 4, 2012, 08:57 

#87 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
Hi Alberto,
I have finally attempted some modifications to the bubbleFoam solver to implement the mixture turbulence model. I have a question relating to the implementation of the first divergence term in the equations.. I am not sure what this term means? Also I have not included the source terms yet as they are not implemented in bubblefoam as standard, but I would eventually like to implement these once I get it working without them. Kind Regards Matt 

May 4, 2012, 22:46 

#88  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Quote:
rho > rhoMix U > UMix mu > muMix (molecular viscosity) and the resulting k and epsilon belong to the mixture. Please note that the same consideration applies to wall functions. The divergence term div(rho_mix*U_mix*k_mix) is the convective term. In bubbleFoam U_mix is simply the face velocity of the mixture phi, and rho_mix is "rho = alpha*rhoa + beta*rhob", which should be available already. Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 4, 2012, 23:33 

#89 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
sorry about that I didn't even mention.. I am using Rusche PhD thesis
the equations I am referring to are equations 3.66 and 3.67 I have circled the div terms which I am unsure about in the attached image. Cheers Matt 

May 4, 2012, 23:47 

#90 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Those terms are what is in the code already:
fvm::div(phib, k) and fvm::div(phib, epsilon). The next divergence term has to be discretized as fvm::Sp(fvc::div(phib), k) Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. Last edited by alberto; May 9, 2012 at 13:35. Reason: Corrected typo (Su > Sp) 

May 5, 2012, 01:43 

#91 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
I have added the extra term as you suggested and recompiled but now I get the following error message:
> FOAM FATAL ERROR: incompatible dimensions for operation [epsilon[0 2 4 0 0 0 0] ]  [epsilon[0 0 1 0 0 0 0] ] From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&) in file /opt/openfoam201/src/finiteVolume/lnInclude/fvMatrix.C at line 1278. 

May 5, 2012, 02:28 

#92 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
First, let me correct one typo: I wrote "Su" instead of "Sp".
If you use fvm::div(phib, epsilon)  fvm::Sp(fvc::div(phib), epsilon) it should work out, since the units are: [phi] = m/s [epsilon] = m^2/s^3 so the first term is m^2/s^4 (accounting for the units introduced by the divergence). The second term gives [div(phib)] = 1/s [epsilon] = m^2/s^3 so again m^2/s^4 as before. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 5, 2012, 03:08 

#93 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
Thanks a lot Alberto,
I have compiled the solver again, so basically equations 3.66 and 3.67 (Rusche) are implemented as my turbulence model without the source terms. The solver now runs on the bubbleColumn tute, after halving the time step, for the full 20 sec however after about 10 sec of the solution the flow takes on the shape in the image and does not change.. Should I be using a different scheme for the kepsilon terms? I'm not sure what is causing this. The settings are the same as the bubbleColumn tute with the following changes: added the kepsilon terms to the fvSchemes dict halved time step to 0.001s turned correctAlpha to yes Kind Regards Matt 

May 5, 2012, 03:10 

#94 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Could you check the values of turbulent viscosity?
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 5, 2012, 03:28 

#95 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
turbulent viscosity was taken from Paraview..


May 5, 2012, 14:08 

#96 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
This seems quite normal.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 9, 2012, 04:06 

#97 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 6 
Hi Alberto,
So I have made some modifications to the createRASTurbulence.H file, namely the alphaEps coefficient (I believe this is the Schmidt number in the dissipation equation). It is set to 0.76923 originally in the solver however Rusche uses 1.3. My problem is that once I change it to 1.3 and recompile the solver blows up.. I have tried running the solver on a case that I had already run without changing alphaEps and it did not solve. I also have not been able to figure out why I am having problems I had posted earlier with the flow! I am guessing that I am missing something in the code. I only changed parts of the section of kEpsilon.H as follows: // Dissipation equation fvScalarMatrix epsEqn ( fvm::ddt(epsilon) + fvm::div(phib, epsilon)  fvm::Sp(fvc::div(phi), epsilon)  fvm::laplacian ( nuEffb/alphaEps, epsilon, "laplacian(DepsilonEff,epsilon)" ) == C1*G*epsilon/k  fvm::Sp(C2*epsilon/k, epsilon) ); #include "wallDissipation.H" epsEqn.relax(); epsEqn.solve(); epsilon.max(dimensionedScalar("zero", epsilon.dimensions(), 1.0e15)); // Turbulent kinetic energy equation fvScalarMatrix kEqn ( fvm::ddt(k) + fvm::div(phib, k)  fvm::Sp(fvc::div(phi), k)  fvm::laplacian ( nuEffb/alphak, k, "laplacian(DkEff,k)" ) == G  fvm::Sp(epsilon/k, k) ); Does this look ok to you? Kind Regards Matt Last edited by matt.mech.eng; May 9, 2012 at 11:18. 

May 9, 2012, 13:37 

#98 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
There was a typo that I corrected in my previous post: fvm::Sp(fvc::div(phi), k) should be fvm::Sp(fvc::div(phib), k). Same for epsilon: you should use phib.
Also, you don't need to recompile the code to change alphaEps. Just specify it in the appropriate dictionary in the constant/RASProperties dictionary. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 23, 2013, 06:31 

#99 
New Member

Hi, just a little question: in the latest implementation of twoPhaseEulerFoam i see the term above discussed:
fvm::Sp(fvc::div(phib),k) and the same for eps equation. My question is: does this term have any importance for incompressible simulations? In the previous versions of the code it isn't implemented in the incompressible version. Thanks, Lapo 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Burgerbs equation non constant Boundary Conditions Initial Conditions  arkangel  OpenFOAM Running, Solving & CFD  1  October 2, 2008 14:48 
Boundary conditions for turbulent boundary layer  Thomas  FLUENT  1  June 17, 2008 05:14 
boundary conditions for boundary layer flow  A. Alzoubi  CFX  0  November 3, 2007 08:11 
TwoPhaseEulerFoam and InletOutlet boundary condition  hemph  OpenFOAM Running, Solving & CFD  10  January 29, 2007 10:47 
Integral boundary conditions turbulent intensitylength boundary conditions  olesen  OpenFOAM Running, Solving & CFD  0  July 27, 2006 07:18 