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

Problem about drag model in twoPhaseEulerFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 10, 2010, 09:57
Default Problem about drag model in twoPhaseEulerFoam
  #1
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
beauty is on a distinguished road
Hi, friends
I encountered some problems about the drag models in the twoPhaseEulerFoam solver.
1First one is about the calculation of particle Remolds number in drag models. For example, in sourcefile of WeYu.C, the code is as follows:

Foam::tmp<Foam::volScalarField> Foam::WenYu::K
(
const volScalarField& Ur
) const
{
volScalarField beta = max(scalar(1) - alpha_, scalar(1.0e-6));
volScalarField bp = pow(beta, -2.65);

volScalarField Re = max(Ur*phasea_.d()/phaseb_.nu(), scalar(1.0e-3));
volScalarField Cds = 24.0*(scalar(1) + 0.15*pow(Re, 0.687))/Re;

forAll(Re, celli)
{
if(Re[celli] > 1000.0)
{
Cds[celli] = 0.44;
}
}

return 0.75*Cds*phaseb_.rho()*Ur*bp/phasea_.d();
}
From the code, the particle Remolds number is calculated by Re=ρb|Ur|da/μb, and the Ur is defined via const volScalarField& Ur. But in theory, Remolds number is defined as Re=ρbUrda/μb. I am a rookie with C++, is the sentence const volScalarField& Ur equals to|Ur|?
2Second is the compile error when change the blue line to:
volScalarField Cds = 24.0*(scalar(1) + 0.15*pow(Re*beta, 0.687))/(Re*beta);
I attach my source file and the log of wmake.
Look forward to your advance.
Thanks!

beauty
Attached Files
File Type: zip myWenYu.zip (6.9 KB, 5 views)
File Type: zip log.zip (1.9 KB, 6 views)
beauty is offline   Reply With Quote

Old   May 11, 2010, 11:28
Default
  #2
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
1) You have to send it the magnitude of the relative velocity. You can see this within the twoPhaseEulerFoam solver in liftDragCoeffs.H.

2) I'm not sure. Did you 'wmake libso' in interfacialModels?
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   May 12, 2010, 03:36
Default
  #3
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
beauty is on a distinguished road
Hi
Thank you for your help. Yes, it is like you said I have to send the magnitude of the relative velocity, which is executed by liftDragCoeffs.H in twoPhaseEulerFoam. Miss the file (liftDragCoeffs.H) is my fault.
I didn’t “wmake libso” in interfacialModels. I just performed “wmake” in terminal. Is this the problem?

beauty
beauty is offline   Reply With Quote

Old   May 12, 2010, 05:01
Default
  #4
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
I assume that what you did was copy one of the dragModels and alter it slightly? You need to recreate the library libEulerianInterfacialModels. You'll see in the folder twoPhaseEulerFoam/interfacialModels there is a folder Make/ add your new model to Make/files, and then run 'wmake libso' from the folder twoPhaseEulerFoam/interfacialModel. You'll then be able to use your new drag model.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   May 12, 2010, 08:08
Default
  #5
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
beauty is on a distinguished road
Quote:
Originally Posted by l_r_mcglashan View Post
I assume that what you did was copy one of the dragModels and alter it slightly? You need to recreate the library libEulerianInterfacialModels. You'll see in the folder twoPhaseEulerFoam/interfacialModels there is a folder Make/ add your new model to Make/files, and then run 'wmake libso' from the folder twoPhaseEulerFoam/interfacialModel. You'll then be able to use your new drag model.
yes, you are right. I just copy one dragModel and alter it. Then I add my new model to Make/files, and run wmake.Today I compiled the dragmodel following your guidance, everything is ok. Thank you very much.
beauty

Last edited by beauty; May 13, 2010 at 10:05.
beauty is offline   Reply With Quote

Old   May 13, 2010, 16:49
Default Regarding twoPhaseEulerFoam
  #6
New Member
 
M K Singh
Join Date: Sep 2009
Posts: 19
Rep Power: 7
mksingh is on a distinguished road
Quote:
Originally Posted by beauty View Post
yes, you are right. I just copy one dragModel and alter it. Then I add my new model to Make/files, and run wmake.Today I compiled the dragmodel following your guidance, everything is ok. Thank you very much.
beauty
================================================== =======
Hi
Regarding twoPhaseEulerFoam in OF1.6, I tried a simple 3-D bubble column, but never successful in getting right results. Some times I get very unstable free surface and after a certain point I see that whole domain is filled with continuous phase. Have you encountered the same problems with TwoPhaseEulerFoam?
With regards.
M K
mksingh is offline   Reply With Quote

Old   May 13, 2010, 20:13
Default
  #7
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by beauty View Post
volScalarField Cds = 24.0*(scalar(1) + 0.15*pow(Re*beta, 0.687))/(Re*beta);
Why do you divide by beta?

I know it is "common practise" to see that around, but Wen & Yu drag does not contain alpha inside the Reynolds number. The correction due to the presence of more than one particles is made introducing the beta^{-2.65}, the rest stays the same as in the single-particle case.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods

Last edited by alberto; May 13, 2010 at 20:17. Reason: Added explanation
alberto is offline   Reply With Quote

Old   May 13, 2010, 20:14
Default
  #8
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by mksingh View Post
================================================== =======
Hi
Regarding twoPhaseEulerFoam in OF1.6, I tried a simple 3-D bubble column, but never successful in getting right results. Some times I get very unstable free surface and after a certain point I see that whole domain is filled with continuous phase. Have you encountered the same problems with TwoPhaseEulerFoam?
With regards.
M K
Usually this happens because your Courant number (time step) is too big.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   May 14, 2010, 05:15
Default To M K
  #9
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
beauty is on a distinguished road
Quote:
Originally Posted by mksingh View Post
================================================== =======
Hi
Regarding twoPhaseEulerFoam in OF1.6, I tried a simple 3-D bubble column, but never successful in getting right results. Some times I get very unstable free surface and after a certain point I see that whole domain is filled with continuous phase. Have you encountered the same problems with TwoPhaseEulerFoam?
With regards.
M K
Hi
I didn't encounter the same problem. I am a rookie to openfoam, so I can't give you good solution, I feel so sorry. Maybe the reason is as Alberto said, your time step is too big. I have seen a paper about simulaiton of the gas-solid fluidized bed, in which the time step is set to 0.00001.
beauty
beauty is offline   Reply With Quote

Old   May 14, 2010, 05:37
Default To Alberto
  #10
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
beauty is on a distinguished road
Hi, Alberto
After seeing your reply, I check my equation again. The WenYu drag Model I have read in paper is different from the expression in openfoam. I can't write formula here, so I attached a file. what is your opinion?
beauty
Attached Files
File Type: doc The expression.doc (19.0 KB, 9 views)
beauty is offline   Reply With Quote

Old   May 14, 2010, 10:36
Default
  #11
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hello,

they're both used. I checked again, and you find both of them reported as "Wen & Yu (1966)" model. I'll try to find the original paper from Wen & Yu (1966) to clarify.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   May 14, 2010, 10:37
Default
  #12
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by beauty View Post
I have seen a paper about simulaiton of the gas-solid fluidized bed, in which the time step is set to 0.00001.
Quite normal time step for dense fluidized beds. Usually 5 10^-4 - 10^-5, and even smaller if you introduce frictional models.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   May 14, 2010, 23:11
Default happen to have the same view
  #13
New Member
 
beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
beauty is on a distinguished road
Quote:
Originally Posted by alberto View Post
Hello,

they're both used. I checked again, and you find both of them reported as "Wen & Yu (1966)" model. I'll try to find the original paper from Wen & Yu (1966) to clarify.
Hi
It's happy to see that. I also have the idea to find the original paper. Please let me know what's the result.

beauty
beauty is offline   Reply With Quote

Old   May 14, 2010, 23:20
Default
  #14
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
I didn't have time to go to the library and dig it out. In the meanwhile, the good review of

Enwald, Peirano and Amstedt, "Eulerian two-phase theory applied to fluidization", Int. J. Multiphase Flow, 1996

report that Wen & Yu used the Schiller and Naumann correlation for Cd, which does not contain alpha multiplying the Reynolds number.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
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
Use of k-epsilon and k-omega Models Jade M Main CFD Forum 12 June 2, 2015 13:16
Polyflow Simulation with ViscoElastic Model memory problem sid2909 ANSYS 0 May 10, 2010 05:27
multiphase mixing Problem with MRF model in MixSim Srinivas FLUENT 0 October 17, 2005 06:35
Converge problem of Mixture Model Jen FLUENT 8 August 17, 2005 18:23
Writing a BCDEFI problem for RSM model S. Bottenheim CD-adapco 2 January 28, 2005 09:55


All times are GMT -4. The time now is 19:22.