CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)
-   -   Problem about drag model in twoPhaseEulerFoam (https://www.cfd-online.com/Forums/openfoam/75946-problem-about-drag-model-twophaseeulerfoam.html)

beauty May 10, 2010 10:57

Problem about drag model in twoPhaseEulerFoam
 
2 Attachment(s)
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

l_r_mcglashan May 11, 2010 12:28

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?

beauty May 12, 2010 04:36

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

l_r_mcglashan May 12, 2010 06:01

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.

beauty May 12, 2010 09:08

Quote:

Originally Posted by l_r_mcglashan (Post 258452)
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

mksingh May 13, 2010 17:49

Regarding twoPhaseEulerFoam
 
Quote:

Originally Posted by beauty (Post 258472)
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

alberto May 13, 2010 21:13

Quote:

Originally Posted by beauty (Post 258182)
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 May 13, 2010 21:14

Quote:

Originally Posted by mksingh (Post 258695)
================================================== =======
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,

beauty May 14, 2010 06:15

To M K
 
Quote:

Originally Posted by mksingh (Post 258695)
================================================== =======
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 May 14, 2010 06:37

To Alberto
 
1 Attachment(s)
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

alberto May 14, 2010 11:36

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 May 14, 2010 11:37

Quote:

Originally Posted by beauty (Post 258753)
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,

beauty May 15, 2010 00:11

happen to have the same view
 
Quote:

Originally Posted by alberto (Post 258805)
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:p. Please let me know what's the result.

beauty

alberto May 15, 2010 00:20

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,


All times are GMT -4. The time now is 15:29.