# Problem about drag model in twoPhaseEulerFoam

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

May 10, 2010, 09:57
Problem about drag model in twoPhaseEulerFoam
#1
New Member

beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
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.
Thanks!

beauty
Attached Files
 myWenYu.zip (6.9 KB, 5 views) log.zip (1.9 KB, 6 views)

 May 11, 2010, 11:28 #2 Senior Member   Laurence R. McGlashan Join Date: Mar 2009 Posts: 370 Rep Power: 14 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

 May 12, 2010, 03:36 #3 New Member   beauty Join Date: Feb 2010 Posts: 27 Blog Entries: 1 Rep Power: 7 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

 May 12, 2010, 05:01 #4 Senior Member   Laurence R. McGlashan Join Date: Mar 2009 Posts: 370 Rep Power: 14 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

May 12, 2010, 08:08
#5
New Member

beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
Quote:
 Originally Posted by l_r_mcglashan 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.

May 13, 2010, 16:49
Regarding twoPhaseEulerFoam
#6
New Member

M K Singh
Join Date: Sep 2009
Posts: 19
Rep Power: 7
Quote:
 Originally Posted by beauty 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

May 13, 2010, 20:13
#7
Senior Member

Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
Quote:
 Originally Posted by beauty 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

May 13, 2010, 20:14
#8
Senior Member

Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
Quote:
 Originally Posted by mksingh ================================================== ======= 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

May 14, 2010, 05:15
To M K
#9
New Member

beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
Quote:
 Originally Posted by mksingh ================================================== ======= 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

May 14, 2010, 05:37
To Alberto
#10
New Member

beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
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
 The expression.doc (19.0 KB, 9 views)

 May 14, 2010, 10:36 #11 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,894 Rep Power: 26 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

May 14, 2010, 10:37
#12
Senior Member

Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
Quote:
 Originally Posted by beauty 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

May 14, 2010, 23:11
happen to have the same view
#13
New Member

beauty
Join Date: Feb 2010
Posts: 27
Blog Entries: 1
Rep Power: 7
Quote:
 Originally Posted by alberto 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

 May 14, 2010, 23:20 #14 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,894 Rep Power: 26 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Jade M Main CFD Forum 12 June 2, 2015 13:16 sid2909 ANSYS 0 May 10, 2010 05:27 Srinivas FLUENT 0 October 17, 2005 06:35 Jen FLUENT 8 August 17, 2005 18:23 S. Bottenheim CD-adapco 2 January 28, 2005 09:55

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

 Contact Us - CFD Online - Top