CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

TwoPhaseEulerFoam and Boundary conditions

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

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 19, 2010, 03:39
Default
  #61
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9
chai is on a distinguished road
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

chai is offline   Reply With Quote

Old   April 19, 2010, 04:00
Default
  #62
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by chai View Post
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.


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 Euler-Euler 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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   April 19, 2010, 23:05
Default
  #63
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9
chai is on a distinguished road
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 air-water two-phase 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
chai is offline   Reply With Quote

Old   April 22, 2010, 01:09
Default help
  #64
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 8
mohsenkh599 is an unknown quantity at this point
hi
I want to simulate two phase flow through a porous media. is there a solver in openfoam which I can use?
the Best
mohsenkh599 is offline   Reply With Quote

Old   April 22, 2010, 01:20
Default
  #65
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by mohsenkh599 View Post
hi
I want to simulate two phase flow through a porous media. is there a solver in openfoam which I can use?
the Best
The only multiphase solver with porous zone effect included out of the box is porousInterFoam, which uses the VOF approach. You can of course modify other solvers to account for it.

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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   April 22, 2010, 01:27
Default
  #66
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 8
mohsenkh599 is an unknown quantity at this point
thank you very much
I got it. thanks
mohsenkh599 is offline   Reply With Quote

Old   June 13, 2010, 01:13
Default
  #67
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9
chai is on a distinguished road
Hi Alberto
Iím also simulating a bubble column case for air-water. 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
chai is offline   Reply With Quote

Old   June 13, 2010, 02:34
Default
  #68
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by chai View Post
Hi Alberto
Iím also simulating a bubble column case for air-water. 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
Hi,

what you notice depends on the fact twoPhaseEulerFoam uses the phase-intensive formulation of the momentum equation. In simple words, the phase momentum equations are re-arranged 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 phase-intensive form solves this problem by writing the equations in non-conservative 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:
  • if alpha[cellI] < smallAlpha (arbitrary value, small enough, might be 10^-6 (single precision) or 10^-8 (double precision) as done in some other code), UaPost[cellI] = 0
  • if 1-alpha[cellI] < smallAlpha, UbPost[cellI] = 0
Clearly this needs to be done only when it is outputTime. Additionally, do not do it directly on Ua and Ub.

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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   June 14, 2010, 13:53
Default
  #69
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9
chai is on a distinguished road
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
chai is offline   Reply With Quote

Old   June 14, 2010, 14:40
Default
  #70
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by chai View Post
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?
What you usually do is to limit the k and epsilon so that they stay positive, and then limit the "turbulent viscosity ratio", meaning the ratio

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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   June 15, 2010, 09:34
Default
  #71
New Member
 
sugy
Join Date: Jun 2010
Posts: 1
Rep Power: 0
nnsgy is on a distinguished road
Hi
Thank you for your answer.
This mixture hypothesis sounds intereting. Are there any documents of it ?

Best regards
Chai
nnsgy is offline   Reply With Quote

Old   July 5, 2010, 23:09
Default
  #72
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 8
beauty is on a distinguished road
Quote:
Originally Posted by alberto View Post
Hi,

twoPhaseEulerFoam implements the turbulence mixture model of Gosman (see H. Rusche thesis).The implementation is done completely in the code, where you can find also the implementation of the wall functions.

To implement a new model:

- Remove the current model equations, or add a switch to decide which turbulence model you want to use. Equations are in twoPhaseEulerFoam/turbulenceModel/kEpsilon.H. In the same directory you find the headers where wall functions are implemented.

- Assuming all turbulence models you want to try rely on the hypothesis of turbulence viscosity, you do not have to deeply change the structure of the solver. Simply change the parts where the turbulent and effective viscosities are computed.
For explicit closures, this is all what you need to do.

- For models involving transport equations, you should code them, following the example of the k-eps equations already in the code.

As a side note, to compile twoPhaseEulerFoam, you need to run ./Allwmake because there are additional classes to be compiled.

Best,
Alberto
Hi, alberto
I have some problem when using twoPhaseEulerFoam to simulate gas-solid two-phase 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?
parameters-----inlet----outlet----walls
alpha----------0.01--------0-gradient ---------0-gradient
epsilon--------0.05------0-gradient -------0-gradient
k--------------0.05-----0-gradient ------0-gradient
p--------------0-gradient---uniform 0-------0-gradient
Theata---------0.0001----0-gradient -----0-gradient
Ua-------------0.5 m/s --------0-gradient--------fixed value 0
Ub-------------0.5m/s---0-gradient---------fixed 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
Attached Files
File Type: zip u-p.zip (30.8 KB, 17 views)
beauty is offline   Reply With Quote

Old   July 6, 2010, 04:47
Default
  #73
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   July 6, 2010, 07:35
Default
  #74
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 8
beauty is on a distinguished road
Hi, alberto
I see that, thank you for your reply!

beauty
beauty is offline   Reply With Quote

Old   August 5, 2010, 02:47
Default
  #75
Senior Member
 
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 9
chiven is on a distinguished road
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 = 1.38479e-08, Final residual = 5.80563e-25, No Iterations 1
Dispersed phase volume fraction = 0.50738  Min(alpha) = 0  Max(alpha) = 1.00008
DILUPBiCG:  Solving for alpha, Initial residual = 1.25486e-20, Final residual = 1.25486e-20, No Iterations 0
Dispersed phase volume fraction = 0.50738  Min(alpha) = 0  Max(alpha) = 1.00008
DILUPBiCG:  Solving for alpha, Initial residual = 1.25486e-20, Final residual = 1.25486e-20, 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 = 2.752e-05, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.000997852, Final residual = 9.78322e-06, No Iterations 2
time step continuity errors : sum local = 9.10235e-07, global = 3.8794e-09, cumulative = 3.8794e-09
DILUPBiCG:  Solving for alpha, Initial residual = 9.17413e-05, Final residual = 3.50207e-11, No Iterations 2
Dispersed phase volume fraction = 0.507375  Min(alpha) = 0  Max(alpha) = 1.00004
DILUPBiCG:  Solving for alpha, Initial residual = 9.60749e-07, Final residual = 4.32947e-13, No Iterations 2
Dispersed phase volume fraction = 0.507375  Min(alpha) = 0  Max(alpha) = 1.00004
DILUPBiCG:  Solving for alpha, Initial residual = 1.72154e-08, Final residual = 2.47802e-11, 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 = 5.66783e-05, 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 = 9.51382e-05, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.00178332, Final residual = 1.19047e-05, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.000453534, Final residual = 1.50636e-06, No Iterations 3
time step continuity errors : sum local = 7.8859e-07, global = 1.97743e-09, cumulative = 5.85683e-09
ExecutionTime = 1.4 s  ClockTime = 3 s
Time = 0.0009
DILUPBiCG:  Solving for alpha, Initial residual = 6.92919e-05, Final residual = 6.40338e-11, No Iterations 2
Dispersed phase volume fraction = 0.507338  Min(alpha) = -8.45905e-24  Max(alpha) = 1.00034
DILUPBiCG:  Solving for alpha, Initial residual = 1.81131e-07, Final residual = 4.97962e-14, No Iterations 2
Dispersed phase volume fraction = 0.507338  Min(alpha) = -8.459e-24  Max(alpha) = 1.00034
DILUPBiCG:  Solving for alpha, Initial residual = 1.00796e-09, Final residual = 2.10872e-12, No Iterations 1
Dispersed phase volume fraction = 0.507338  Min(alpha) = -8.459e-24  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 = 3.54374e-05, No Iterations 6
GAMG:  Solving for p, Initial residual = 0.00286344, Final residual = 1.38734e-05, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.000610208, Final residual = 4.13386e-06, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.000155264, Final residual = 1.46421e-06, No Iterations 6
time step continuity errors : sum local = 7.71506e-07, global = 4.2508e-09, cumulative = 7.15679e-08
DILUPBiCG:  Solving for alpha, Initial residual = 1.86645e-06, Final residual = 5.63336e-13, No Iterations 2
Dispersed phase volume fraction = 0.507338  Min(alpha) = -8.45767e-24  Max(alpha) = 1.00034
DILUPBiCG:  Solving for alpha, Initial residual = 5.41579e-09, Final residual = 1.75491e-11, No Iterations 1
Dispersed phase volume fraction = 0.507338  Min(alpha) = -8.45767e-24  Max(alpha) = 1.00034
DILUPBiCG:  Solving for alpha, Initial residual = 8.63358e-11, Final residual = 8.63358e-11, No Iterations 0
Dispersed phase volume fraction = 0.507338  Min(alpha) = -8.45767e-24  Max(alpha) = 1.00034
GAMG:  Solving for p, Initial residual = 0.0140125, Final residual = 7.98277e-05, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.00472174, Final residual = 1.96878e-05, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.000934931, Final residual = 9.05272e-06, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.000275176, Final residual = 2.15058e-06, No Iterations 3
GAMG:  Solving for p, Initial residual = 6.70355e-05, Final residual = 3.16043e-07, No Iterations 5
time step continuity errors : sum local = 7.71366e-07, global = 4.25032e-09, cumulative = 7.58182e-08
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 = 6.90647e-05, Final residual = 5.27474e-11, No Iterations 2
Dispersed phase volume fraction = 0.507334  Min(alpha) = -8.37912e-24  Max(alpha) = 1.00037
DILUPBiCG:  Solving for alpha, Initial residual = 1.61556e-07, Final residual = 5.13531e-14, No Iterations 2
Dispersed phase volume fraction = 0.507334  Min(alpha) = -8.37906e-24  Max(alpha) = 1.00037
DILUPBiCG:  Solving for alpha, Initial residual = 8.15377e-10, Final residual = 1.26952e-12, No Iterations 1
Dispersed phase volume fraction = 0.507334  Min(alpha) = -8.37906e-24  Max(alpha) = 1.00037
 
[65] #0  Foam::error::printStack(Foam::Ostream&) in "/home/g9/a094039/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[65] #1  Foam::sigFpe::sigFpeHandler(int) in "/home/g9/a094039/OpenFOAM/OpenFOAM-1.6/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/OpenFOAM-1.6/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/OpenFOAM-1.6/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/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[65] #6  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/g9/a094039/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[65] #7  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/g9/a094039/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libfiniteVolume.so"
[65] #8  main in "/home/g9/a094039/OpenFOAM/OpenFOAM-1.6/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/OpenFOAM-1.6/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
 
chiven is offline   Reply With Quote

Old   August 6, 2010, 13:43
Default
  #76
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9
chai is on a distinguished road
Can you give a much more detailed description of you case?
Moreover, do you run the case in parallel?

chai
chai is offline   Reply With Quote

Old   August 7, 2010, 02:57
Default
  #77
Senior Member
 
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 9
chiven is on a distinguished road
Quote:
Originally Posted by chai View Post
Can you give a much more detailed description of you case?
Moreover, do you run the case in parallel?

chai

Hi, Chai, thanks for the input.
In my case, a cold water flow is injected into a hot two-phase 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 OF-friends 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
chiven is offline   Reply With Quote

Old   August 7, 2010, 09:18
Default
  #78
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 9
chai is on a distinguished road
I think this problem is due to the parallel computing. try to run your case only using a single processor.

chai
chai is offline   Reply With Quote

Old   April 20, 2012, 03:54
Default source terms in bubblefoam implementation of turbulence model
  #79
Member
 
Join Date: Feb 2012
Posts: 57
Rep Power: 6
matt.mech.eng is on a distinguished road
Hi Alberto,

What happens to the source terms in the turbulence model used by openfoam? There appears to be no source terms..

Cheers

Matt
matt.mech.eng is offline   Reply With Quote

Old   April 20, 2012, 15:32
Default
  #80
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Hi Matt, the k-epsilon model used in bubbleFoam is a standard k-eps, 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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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. Al-zoubi 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


All times are GMT -4. The time now is 04:16.