CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Implicit solver for gamma volumefraction equation (http://www.cfd-online.com/Forums/openfoam-solving/58552-implicit-solver-gamma-volumefraction-equation.html)

sek June 20, 2007 11:19

Cuurently, the volume-fraction
 
Cuurently, the volume-fraction equation in interFoam, for instance, uses an explicit solver. I was curious whether using an implicit solver would allow me to use larger time-step size. So, I tried to call MULES::implicitSolve01 instead of MULE::explicitSolve1 in gammaEqn.H. It seems to work. One thing I'm not sure about is one of the argument Dpsi of dimensionedScalar type. Looking at the MULE implementation, Dpsi of appears to be a diffusivity introduced as a stabulity measure for gamma equation. I set it to a small value, which seems to work.

Can someone comment on whether I'm doing things right, please?

ngj September 9, 2008 07:42

Hi all I would like to rest
 
Hi all

I would like to restart this discussion. Is there anyone who has successfully implemented an implicit solver for the gamma equation?
I tried the above approach but was not able to get it to work.

Further, what is the argument behind the hard-coded "MULES::explicitSolve01" in the interFoam-solvers.

I am currently using 1.4.1.

Thank you for any help or suggestions.

/ Niels

pbohorquez September 9, 2008 12:12

MULES::implicitSolve works wit
 
MULES::implicitSolve works with success in the solver interPhaseChangeFoam (OF-1.5).

Following src/finiteVolume/fvMatrices/solvers/MULES/MULES.H it reads

MULES:explicitSolve01(psi, phi, phiPsi) ask you for:
- psi: actual value of the variable to be solved
- phi: normal convective flux
- psiPhi: actual explicit flux of the variable to solve. It is also used to return the limited flux of the bounded solution.

Obviously, psi = gamma for interFoam. Then, phi = US, where U is the velocity vector and S is the normal to the cell surface times the cell-surface area. Its value comes from the PISO-loop. Finally, psiPhi = gamma [U+(1-gamma)U<sub>r,gamma</sub>]S = gamma U<sub>gamma</sub>S, where U<sub>r,gamma</sub> is the relative velocity of the water with respect to the air at the thick free-surface, and U<sub>gamma</sub> is the velocity of the gamma-phase.

Patricio

ngj September 10, 2008 05:53

Hi Patricio Thanks for the
 
Hi Patricio

Thanks for the quick answer. I will download 1.5. and look into it.

Best regards,

Niels

ngj September 12, 2008 09:06

Hi all I have tried to find
 
Hi all

I have tried to find some documentation on the MULES-procedure, but on Web of Science I can only find references to the "animal"-kind of MULES.

Further in Henrik Ruches he describes what looks like the used procedure, but refer to a N_a_b_l_a Ltd technical note.

Thus is is possible that

H.G.Weller, Derivation, modelling and solution of the conditionally averaged two-phase flow equations. Technical Report TR/HGW/02, N_a_b_l_a Ltd, 2002

could be made available? If anyone knows another source of documentation I would be happy to know about it.

Best regards and a good weekend to all,

Niels

eugene September 12, 2008 10:50

MULES was invented by Henry la
 
MULES was invented by Henry last year (or was it 2006?) and nothing has ever been published, so you aren't likely to find any documentation about it.

ngj September 13, 2008 05:20

Hi @Eugene Okay, I am s
 
Hi

@Eugene

Okay, I am sorry to hear that, but there is of course nothing to do about it.

@Other

I have tried to shift to a MULES::implicitSolver in interFoam, but I keep running it problems with my fvSolution file. From the source "MULESImplicit" should be a subDict in the gamma-solution file, thus I have added this to the file:

gamma PBiCG
{
MULESImplicit
{
maxIter 1000;
nLimiterIter 10;
maxUnboundedness 1;
CoCoeff 0.2;
}
preconditioner DILU;
tolerance 1e-06;
relTol 0;
};

thus even though I have added it as a subDict, I keep getting this error message:

keyword MULESImplicit is undefined in dictionary "/home/ngj/OpenFOAM/ngj-1.5/run/tutorials/interFoam/damBreak/system/fvSolution:: gamma"

file: /home/ngj/OpenFOAM/ngj-1.5/run/tutorials/interFoam/damBreak/system/fvSolution::g amma from line 47 to line 54.

From function dictionary::subDict(const word& keyword)
in file db/dictionary/dictionary.C at line 288.

FOAM exiting

Thus if any knows how to set the gamma-part of fvSolution, then please help.

Best regards,

Niels

P.S. For any, do not take the values in the subDict seriously, as I have not looked into the meaning behind those yet.

kjmaki September 13, 2008 07:16

Hi Niels! I am sorry that I
 
Hi Niels!

I am sorry that I can't help you with the MULESImplicit, but I find it strange that the MULESExplicit controls are read from the PISO dict, and the Implicit are from the gamma dict. Do you know why they would do that?

Also, there is some mention on the gamma transport equation that FOAM uses in the thesis by Rusche (2002), sec 4.2.1. You will see that it references private communication with Weller for the details though.

Have a great weekend!

Kevin

pbohorquez September 13, 2008 08:31

Hi Niels I suppose that you
 
Hi Niels

I suppose that you have replaced the files gamma* of interFoam with those from interPhaseChangeFoam, commented the lines related to Sp & Su in gammaEqn.H and call MULES::implicitSolve(oneField(), gamma, phi, phiGamma, zeroField(), zeroField(), 1, 0); (or similar)

Then you must try this option instead of the one you proposed:
gamma
MULESImplicit
{
maxIter 1000;
nLimiterIter 10;
maxUnboundedness 1;
CoCoeff 0.2;
solver PBiCG
{
preconditioner DILU;
tolerance 1e-06;
relTol 0;
};
};

and add to fvSchemes the following line:
div(rhoPhi,U) Gauss limitedLinearV 1; It works.




Patricio

pbohorquez September 13, 2008 08:36

Hi Niels I suppose that you
 
Hi Niels

I suppose that you have replaced the files gamma* of interFoam with those from interPhaseChangeFoam, commented the lines related to Sp & Su in gammaEqn.H and call MULES::implicitSolve(oneField(), gamma, phi, phiGamma, zeroField(), zeroField(), 1, 0); (or similar)

Then you must try this option instead of the one you proposed:
gamma
MULESImplicit
{
maxIter 1000;
nLimiterIter 10;
maxUnboundedness 1;
CoCoeff 0.2;
solver PBiCG
{
preconditioner DILU;
tolerance 1e-06;
relTol 0;
};
};

and add to fvSchemes the following line: div(rhoPhi,U) Gauss limitedLinearV 1; It works. I have sent a message to your email with the files

Patricio

ngj September 13, 2008 11:59

Hi Patricio Yes, I have cha
 
Hi Patricio

Yes, I have changed the gamma* files, and I will get to work a.s.a.p.

Again, thanks for your kind help.

/ Niels

caw September 14, 2008 14:57

Dear Niels, i have been fol
 
Dear Niels,

i have been following up this thread and tried the impicit version of interFoam myself.
Out of curiosity: What do you try to achive by using an implicit formulation for the gamma equation?
And do you succeed?

Thing that spring to my mind:
- stability -> higher time steps
- steady state solutions

Could you comment on that please?

Best regards
Christian

ngj September 16, 2008 08:30

Hi Christian Sorry for the
 
Hi Christian

Sorry for the wait, I am in the middle of a not-coorporating reinstall, so I will make it short.

The actual goal was to consider if the implicit solver did give raise to a different exchange of energy between water and air. I, and I know others have the same problem, get large velocities in the air phase, significantly larger than the wave propagation speed.

Due to reinstallation, I have not reached a conclusion, thus this is the closests I can get.

Generally I have not experienced instability problems with waves, except if they break and I use a laminar solver, then the energy cannot be dissipated at a significantly large enough rate.

Best regards,

Niels

santhanuj April 6, 2009 10:42

can anyone tell me how the relative velocity is calculated???

isabel June 29, 2009 13:27

I need to solve the gamma equation in interFoam. But I want to add a source as that:

d(gamma)/dt + div(U*gamma) + div(phigamma) = source

How can I do this? Perhaps with this line: ?

MULES:: implicitSolve(gamma,phi,phiGamma,source)

ngj June 30, 2009 05:39

Hi Isabel

Please look into the source in the folder:

~/OpenFOAM/src/finiteVolume/fvMatrix/solvers/MULES

and you will be able to find out about the syntax.

Best regards,

Niels

isabel June 30, 2009 07:54

Thank you very much, ngj
The key is in MULESTemplates.C in these lines:


fvScalarMatrix psiConvectionDiffusion
(
fvm::ddt(rho, psi)
+ fv::gaussConvectionScheme<scalar>(mesh, phi, UDs).fvmDiv(phi, psi)
- fvm::Sp(Sp, psi)
- Su
);


I think that the equation that it is solving is:

d(rho*psi)/dt + div(phi*psi) - Sp*psi - Su = 0

Am I right?

sandy July 7, 2009 04:29

Quote:

Originally Posted by isabel (Post 220950)
Thank you very much, ngj
The key is in MULESTemplates.C in these lines:


fvScalarMatrix psiConvectionDiffusion
(
fvm::ddt(rho, psi)
+ fv::gaussConvectionScheme<scalar>(mesh, phi, UDs).fvmDiv(phi, psi)
- fvm::Sp(Sp, psi)
- Su
);


I think that the equation that it is solving is:

d(rho*psi)/dt + div(phi*psi) - Sp*psi - Su = 0

Am I right?

==================================

Hi, it seems that you lost the compressible term: div(gamma*(1-gamma)*phi). I guess the gamma equation should be as follows:

d(rho*gamma)/dt + div(phi*gamma) + div(gamma*(1-gamma)*phi) - Sp*gamma - Su = 0

In MULESTemplates.C,
phiPsi = phiGamma = phi*gamma + gamma*(1-gamma)*phi

is it right? If that, in gammaEqu.H, why Su = divU*gamma + vDotcAlphal ? It look like that the term divU*gamma was repeatedly solved ?? :confused:

I knew, to the gamma transport equation,
Source term = vDotvAlphal * gamma + (1 - gamma) * vDotcAlphal = (vDotvAlphal - vDotcAlphal) * gamma + vDotcAlphal.
So, Sp = (vDotvAlphal - vDotcAlphal) * gamma , and it will be solved implicitly.
Su = vDotcAlphal, and it is an explicit term in this equation.

but again, why Su also includes the term divU*gamma in gammaEqu.H ? If the MULES::implicitSolver was chose, this term should be deleted, right? :confused:

isabel July 7, 2009 13:28

Thank you very much, sandy.


I have been studying the interPhaseChange solver carefully.
As you say, in gammaEqn.H we define the variable phigamma:


phigamma = phi*gamma + gamma*(1-gamma)*phir
Sp = vDotvAlphal – vDotcAlphal
Su = div(U)*gamma + vDotcAlphal


And then, when we execute MULES::explicitSolve(oneField(),gamma,phi,phiGamma ,Sp,Su,1,0);
we associate:

rho → oneField ()
psi → gamma
phi → phi
phiPsi → phigamma
Sp → Sp
Su → Su
psiMax → 1
psiMin → 0


and then, the key is in this lines of MULESTemplates.C:


fvScalarMatrix psiConvectionDiffusion
(
fvm::ddt(rho, psi)
+ fv::gaussConvectionScheme<scalar>(mesh, phi, UDs).fvmDiv(phi, psi)
- fvm::Sp(Sp, psi)
- Su
);

......


solve
(
psiConvectionDiffusion + fvc::div(lambda*phiCorr),
MULEScontrols.lookup("solver")
);


That I think that the equation is


d(1*psi)/dt + div(phigamma) + Sp*gamma - Su = 0



I don't know what means this line:
fv::gaussConvectionScheme<scalar>(mesh, phi, UDs).fvmDiv(phi, psi)

but I think you are right, div(U) is repeated. I will ask for my advisors and I will confirmate.

Do you know what these lines means?


slicedSurfaceScalarField lambda
(
IOobject
(
"lambda",
mesh.time().timeName(),
mesh,
IOobject::NO_READ,
IOobject::NO_WRITE,
false
),
mesh,
dimless,
allLambda,
false // Use slices for the couples
);

sandy July 7, 2009 19:20

but I think you are right, div(U) is repeated. I will ask for my advisors and I will confirmate.

Do you know what these lines means?


slicedSurfaceScalarField lambda
(
IOobject
(
"lambda",
mesh.time().timeName(),
mesh,
IOobject::NO_READ,
IOobject::NO_WRITE,
false
),
mesh,
dimless,
allLambda,
false // Use slices for the couples
);[/QUOTE]
=============================

Hi isabel, you have a great advisor, right? You are lucky. I think, in above code, lambda = allLambda, if you want know more informations about it, you can change the code as follows:

-------------------------------------
slicedSurfaceScalarField lambda
(
IOobject
(
"lambda",
mesh.time().timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE,
false
),
mesh,
dimless,
allLambda,
false // Use slices for the couples
);
-----------------------------------

Then, you can get an detailed output file in every iterative step about the "lambda" field.

By the way, this kind of method can also help us to easily debug the codes in OF.

But, now I still don't know what means this line:
fv::gaussConvectionScheme<scalar>(mesh, phi, UDs).fvmDiv(phi, psi), and how to deal with the divU*gamma of Su ..... if you know them, please let me know too. Thanks.


All times are GMT -4. The time now is 22:58.