
[Sponsors] 
April 19, 2010, 03:39 

#61 
New Member
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9 
Hi, Alberto
I have a little question about the k and epsilon equations in bubbleFoam. According to your replies and the thesis of H. Rusche, the turbulent model is developed by Gosman. And I think the equations of k and epsilon should be written as Eq 3.14 and 3.15 in the thesis of H. Rusche. There is no term related to the beta in these equations. But in bubbleFoam the k and epsilon equations have many terms related to beta, such as the source term. These differences really confuse me. Would you please explain and help me with this problem? Awaiting for your replies! Best Regards Chai 

April 19, 2010, 04:00 

#62  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
Nope bubbleFoam doesn't use Gosman's model, since its equations are troublesome when one phase disappears. The model in bubbleFoam uses an equation based on the "continuous phase" (beta) to find k and epsilon for the mixture, and explicitly finds the turbulent viscosity for the dispersed phase. Anyway, this is another area in need of work in OpenFOAM, together with the whole EulerEuler solver stack. I'd suggest a literature search and the implementation of a turbulence model suitable to your application. What are you going to simulate? 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 19, 2010, 23:05 

#63 
New Member
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9 
Hi, Alberto
Thanks for your reply. Do you have any reference related to this turbulence model? I think this model is much different, and I can find no reference related to this model. I want to simulate airwater twophase flow in a three by two rectangle lattice rod bundle. The gas and liquid volume fluxed is between 0.1 and 2 m/s Do you have any ideas about which turbulent model is suitable for my simulation? Best regards Chai 

April 22, 2010, 01:09 
help

#64 
Member
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 8 
hi
I want to simulate two phase flow through a porous media. is there a solver in openfoam which I can use? the Best 

April 22, 2010, 01:20 

#65  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
P.S. Please do not ask your questions in existing threads that are not exactly related to your problem. Open a new thread instead. Thanks. 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 22, 2010, 01:27 

#66 
Member
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 8 
thank you very much
I got it. thanks 

June 13, 2010, 01:13 

#67 
New Member
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9 
Hi Alberto
I’m also simulating a bubble column case for airwater. In my simulation, the bubble velocity in the grids where no gas exists is not equal to zero. Does this phenomenon have physical meaning? Regards Chai 

June 13, 2010, 02:34 

#68  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
what you notice depends on the fact twoPhaseEulerFoam uses the phaseintensive formulation of the momentum equation. In simple words, the phase momentum equations are rearranged to remove the singularity of the equation when the phase fraction alpha tends to zero (In such a case, the momentum equation in conservative form becomes 0 = 0). The phaseintensive form solves this problem by writing the equations in nonconservative form, and dividing by alpha. This formulation of the momentum equation can be solved in the whole domain, since it is well defined for all the physical values of alpha. In addition it has a nice property: when alpha tends to zero, U tends to the particle terminal velocity. To answer your question, considering what I wrote (Oliveira and Issa wrote a paper on the topic as reference), what you notice is perfectly fine and expected. If you want to have a zero velocity where the phase is zero, simply create two fields "UaPost" and "UbPost", set them equal to Ua and Ub, and then check, looping over cells:
I hope this helps. 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. 

June 14, 2010, 13:53 

#69 
New Member
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9 
Hi, Alberto
Thank you for your detailed Explanation. It really helps me to understand this problem. In my simulation the values of k and epsilon near the interface becomes very large. According to your previous post, should I limit the k and epsilon as well as turbulent viscosity to an upper value? Best regards, Chai 

June 14, 2010, 14:40 

#70  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
turbulent viscosity / laminar viscosity of the phase. You might also want to consider the implementation of a better model. If you can rely on the mixture hypothesis, the implementation is very easy. 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. 

June 15, 2010, 09:34 

#71 
New Member
sugy
Join Date: Jun 2010
Posts: 1
Rep Power: 0 
Hi
Thank you for your answer. This mixture hypothesis sounds intereting. Are there any documents of it ? Best regards Chai 

July 5, 2010, 23:09 

#72  
New Member

Quote:
I have some problem when using twoPhaseEulerFoam to simulate gassolid twophase flow in a curved pipe. I want to compare the result with fluent, so I try to use the same BC. But I find that the wall function(epsilonWallFunction .etc) can not be set in 0 file, which is work well in simpleFoam. These are the BC in openFoam. Is there any problem? The velocity and pressure is attached, there are something different. Can you give me some suggestion? parametersinletoutletwalls alpha0.010gradient 0gradient epsilon0.050gradient 0gradient k0.050gradient 0gradient p0gradientuniform 00gradient Theata0.00010gradient 0gradient Ua0.5 m/s 0gradientfixed value 0 Ub0.5m/s0gradientfixed value 0 In addition, you say the turbulence mixture model of Gosman and the wall functions have already been implemented in twoPhaseEulerFoam, but I can not find the folder trubulenceModel in twoPhaseEulerFoam, I use openFoam 1.6. What should I do if I want to implement a new model as you mentioned previously. Thanks very much! beauty 

July 6, 2010, 04:47 

#73 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
The turbulence model is the same used in bubbleFoam, and the files are taken from there (check the Make settings).
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. 

August 5, 2010, 02:47 

#75 
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 10 
HI, greeting. I change the bubbleColumn twoPhaseEulerFoam tutorial case to calculate my case. But some errors shown as follows are met. Any comments? Thank you. Chiven
HTML Code:
Create time Create mesh for time = 0 Reading g Reading transportProperties Calculating face flux field phia Calculating face flux field phib Reading field alpha Reading field p Reading field k Reading field epsilon Calculating field nutb Calculating field nuEffa Calculating field nuEffb Calculating field DDtUa and DDtUb Calculating field g.h Selecting dragModel for phase a: SchillerNaumann Selecting dragModel for phase b: SchillerNaumann dragPhase is blended Selecting viscosityModel Syamlal Selecting conductivityModel HrenyaSinclair Selecting radialModel Gidaspow Selecting granularPressureModel Lun Selecting frictionalStressModel JohnsonJackson Courant Number mean: 0 max: 0.0831755 Starting time loop Courant Number mean: 0 max: 0.0831755 Max Ur Courant Number = 0.0831755 Reading/calculating field UaMean Reading/calculating field UbMean Reading/calculating field alphaMean Reading/calculating field pMean fieldAverage: starting averaging at time 0 Time = 0.0001 DILUPBiCG: Solving for alpha, Initial residual = 1.38479e08, Final residual = 5.80563e25, No Iterations 1 Dispersed phase volume fraction = 0.50738 Min(alpha) = 0 Max(alpha) = 1.00008 DILUPBiCG: Solving for alpha, Initial residual = 1.25486e20, Final residual = 1.25486e20, No Iterations 0 Dispersed phase volume fraction = 0.50738 Min(alpha) = 0 Max(alpha) = 1.00008 DILUPBiCG: Solving for alpha, Initial residual = 1.25486e20, Final residual = 1.25486e20, No Iterations 0 Dispersed phase volume fraction = 0.50738 Min(alpha) = 0 Max(alpha) = 1.00008 GAMG: Solving for p, Initial residual = 1, Final residual = 0.00547221, No Iterations 11 GAMG: Solving for p, Initial residual = 0.185157, Final residual = 0.00133576, No Iterations 2 GAMG: Solving for p, Initial residual = 0.0240601, Final residual = 0.000209944, No Iterations 2 GAMG: Solving for p, Initial residual = 0.00390666, Final residual = 2.752e05, No Iterations 3 GAMG: Solving for p, Initial residual = 0.000997852, Final residual = 9.78322e06, No Iterations 2 time step continuity errors : sum local = 9.10235e07, global = 3.8794e09, cumulative = 3.8794e09 DILUPBiCG: Solving for alpha, Initial residual = 9.17413e05, Final residual = 3.50207e11, No Iterations 2 Dispersed phase volume fraction = 0.507375 Min(alpha) = 0 Max(alpha) = 1.00004 DILUPBiCG: Solving for alpha, Initial residual = 9.60749e07, Final residual = 4.32947e13, No Iterations 2 Dispersed phase volume fraction = 0.507375 Min(alpha) = 0 Max(alpha) = 1.00004 DILUPBiCG: Solving for alpha, Initial residual = 1.72154e08, Final residual = 2.47802e11, No Iterations 1 Dispersed phase volume fraction = 0.507375 Min(alpha) = 0 Max(alpha) = 1.00004 GAMG: Solving for p, Initial residual = 0.00999639, Final residual = 5.66783e05, No Iterations 6 GAMG: Solving for p, Initial residual = 0.0647271, Final residual = 0.000466741, No Iterations 2 GAMG: Solving for p, Initial residual = 0.01067, Final residual = 9.51382e05, No Iterations 2 GAMG: Solving for p, Initial residual = 0.00178332, Final residual = 1.19047e05, No Iterations 3 GAMG: Solving for p, Initial residual = 0.000453534, Final residual = 1.50636e06, No Iterations 3 time step continuity errors : sum local = 7.8859e07, global = 1.97743e09, cumulative = 5.85683e09 ExecutionTime = 1.4 s ClockTime = 3 s Time = 0.0009 DILUPBiCG: Solving for alpha, Initial residual = 6.92919e05, Final residual = 6.40338e11, No Iterations 2 Dispersed phase volume fraction = 0.507338 Min(alpha) = 8.45905e24 Max(alpha) = 1.00034 DILUPBiCG: Solving for alpha, Initial residual = 1.81131e07, Final residual = 4.97962e14, No Iterations 2 Dispersed phase volume fraction = 0.507338 Min(alpha) = 8.459e24 Max(alpha) = 1.00034 DILUPBiCG: Solving for alpha, Initial residual = 1.00796e09, Final residual = 2.10872e12, No Iterations 1 Dispersed phase volume fraction = 0.507338 Min(alpha) = 8.459e24 Max(alpha) = 1.00034 GAMG: Solving for p, Initial residual = 0.0166162, Final residual = 0.00015542, No Iterations 3 GAMG: Solving for p, Initial residual = 0.00529248, Final residual = 3.54374e05, No Iterations 6 GAMG: Solving for p, Initial residual = 0.00286344, Final residual = 1.38734e05, No Iterations 3 GAMG: Solving for p, Initial residual = 0.000610208, Final residual = 4.13386e06, No Iterations 3 GAMG: Solving for p, Initial residual = 0.000155264, Final residual = 1.46421e06, No Iterations 6 time step continuity errors : sum local = 7.71506e07, global = 4.2508e09, cumulative = 7.15679e08 DILUPBiCG: Solving for alpha, Initial residual = 1.86645e06, Final residual = 5.63336e13, No Iterations 2 Dispersed phase volume fraction = 0.507338 Min(alpha) = 8.45767e24 Max(alpha) = 1.00034 DILUPBiCG: Solving for alpha, Initial residual = 5.41579e09, Final residual = 1.75491e11, No Iterations 1 Dispersed phase volume fraction = 0.507338 Min(alpha) = 8.45767e24 Max(alpha) = 1.00034 DILUPBiCG: Solving for alpha, Initial residual = 8.63358e11, Final residual = 8.63358e11, No Iterations 0 Dispersed phase volume fraction = 0.507338 Min(alpha) = 8.45767e24 Max(alpha) = 1.00034 GAMG: Solving for p, Initial residual = 0.0140125, Final residual = 7.98277e05, No Iterations 4 GAMG: Solving for p, Initial residual = 0.00472174, Final residual = 1.96878e05, No Iterations 3 GAMG: Solving for p, Initial residual = 0.000934931, Final residual = 9.05272e06, No Iterations 4 GAMG: Solving for p, Initial residual = 0.000275176, Final residual = 2.15058e06, No Iterations 3 GAMG: Solving for p, Initial residual = 6.70355e05, Final residual = 3.16043e07, No Iterations 5 time step continuity errors : sum local = 7.71366e07, global = 4.25032e09, cumulative = 7.58182e08 ExecutionTime = 9.44 s ClockTime = 12 s Courant Number mean: 0.00255506 max: 0.0831755 Max Ur Courant Number = 0.235694 Calculating averages Time = 0.001 DILUPBiCG: Solving for alpha, Initial residual = 6.90647e05, Final residual = 5.27474e11, No Iterations 2 Dispersed phase volume fraction = 0.507334 Min(alpha) = 8.37912e24 Max(alpha) = 1.00037 DILUPBiCG: Solving for alpha, Initial residual = 1.61556e07, Final residual = 5.13531e14, No Iterations 2 Dispersed phase volume fraction = 0.507334 Min(alpha) = 8.37906e24 Max(alpha) = 1.00037 DILUPBiCG: Solving for alpha, Initial residual = 8.15377e10, Final residual = 1.26952e12, No Iterations 1 Dispersed phase volume fraction = 0.507334 Min(alpha) = 8.37906e24 Max(alpha) = 1.00037 [65] #0 Foam::error::printStack(Foam::Ostream&) in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libOpenFOAM.so" [65] #1 Foam::sigFpe::sigFpeHandler(int) in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libOpenFOAM.so" [65] #2 __restore_rt at sigaction.c:0 [65] #3 Foam::GAMGSolver::scalingFactor(Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libOpenFOAM.so" [65] #4 Foam::GAMGSolver::scalingFactor(Foam::Field<double>&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libOpenFOAM.so" [65] #5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libOpenFOAM.so" [65] #6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libOpenFOAM.so" [65] #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/lib/linux64GccDPOpt/libfiniteVolume.so" [65] #8 main in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/applications/bin/linux64GccDPOpt/twoPhaseEulerFoam" [65] #9 __libc_start_main in "/lib64/libc.so.6" [65] #10 Foam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/g9/a094039/OpenFOAM/OpenFOAM1.6/applications/bin/linux64GccDPOpt/twoPhaseEulerFoam" PLE0152: plexec: Parallel process 65 abnormally terminated. PLE0155: plexec: PPID: 0 Exit status: 15 PLE0155: plexec: PPID: 1 Exit status: 15 PLE0155: plexec: PPID: 2 Exit status: 15 PLE0155: plexec: PPID: 3 Exit status: 15 PLE0155: plexec: PPID: 4 Exit status: 15 PLE0155: plexec: PPID: 5 Exit status: 15 PLE0155: plexec: PPID: 6 Exit status: 15 PLE0155: plexec: PPID: 7 Exit status: 15 PLE0155: plexec: PPID: 8 Exit status: 15 PLE0155: plexec: PPID: 9 Exit status: 15 PLE0155: plexec: PPID: 10 Exit status: 15 

August 6, 2010, 13:43 

#76 
New Member
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9 
Can you give a much more detailed description of you case?
Moreover, do you run the case in parallel? chai 

August 7, 2010, 02:57 

#77  
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 10 
Quote:
Hi, Chai, thanks for the input. In my case, a cold water flow is injected into a hot twophase flow in a pipe. This time, I temporarily don't consider the temperature, and set the parameters referencing to the bubbleColumn tutorial case. Yes, I am running the case in parallel. I am also able to run it in a single processor with fewer meshes. In fact, many OFfriends have ever met the same problems as me. I got some tips from the forum such as adding a relaxation factor, turning off the turbulence model, etc. But failed. I am still thinking how to deal with it. Best regards, Chiven 

August 7, 2010, 09:18 

#78 
New Member
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9 
I think this problem is due to the parallel computing. try to run your case only using a single processor.
chai 

April 20, 2012, 03:54 
source terms in bubblefoam implementation of turbulence model

#79 
Member
Join Date: Feb 2012
Posts: 57
Rep Power: 7 
Hi Alberto,
What happens to the source terms in the turbulence model used by openfoam? There appears to be no source terms.. Cheers Matt 

April 20, 2012, 15:32 

#80 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hi Matt, the kepsilon model used in bubbleFoam is a standard keps, modified for the continuous phase. What source term are you referring to?
__________________
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. 

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 