[Andrea_85]

Hi all,

I am a fairly new user of openfoam 1.7. I am working with interFoam to simulate multiphase flow and i would like some explanation on how VOF method is implemented in openfoam.
Which is the equation that OF solves for alpha?

Is something like that d(alpha)/dt+div(alpha U)==0 ?
or is there an additional term to ensure the compression of the interface?

I had a look at alphaEqn.H but I did not understand that equation is solved

Is there extensive documentation on how the VOF is implemented in OF 1.7?

Thanks
andrea

[Bernhard]

You can have a look here for example, some useful information and references are given:
http://www.cfd-online.com/Forums/ope...of-method.html

[akidess]

Have a look at the thesis by Henrik Rusche, it contains all the basics.

[Andrea_85]

Thanks for the answers,

I have already read the previous posts and a little bit the thesis of Henrik Rusche. All these things are related to earlier versions of OF and I would like to know how OF is implemented now, in 1.7 version (i do not know if is the last one but i guess). It is the same?
I do not think so because I read that the VOF implemented now is different from previous versions.

Is there any documentation (paper, manual stuff like that), maybe written by who has implemented the VOF in openfoam 1.7?

thanks
andrea

[Andrea_85]

I think, if I understand correctly, that the equation that OF solves is:

d(alpha)/dt +div(alpha*U)+div(Ur*alpha*(1-alpha))=0

Is correct?
where i can find the definition of Ur in the code and and how is it calculated?

andrea

[kathrin_kissling]

The definition is inside alphaEqn.H. Notice that we do not work on velocities but on fluxes. Tis operation is performed on the faces.

surfaceScalarField phic = mag(phi/mesh.magSf());
phic = min(interface.cAlpha()*phic, max(phic));
surfaceScalarField phir = phic*interface.nHatf();

The formula is below in the attachment.

Hope this helps.

Best

Kathrin

[Andrea_85]

Thanks Kathrin,

I copy and paste from interfacePropierties.H (not all the file):

/*---------------------------------------------------------------------------*\
00052                            Class interfaceProperties Declaration
00053 \*---------------------------------------------------------------------------*/
00054 
00055 class interfaceProperties
00056 {
00057     // Private data
00058 
00059         //- Keep a reference to the transportProperties dictionary
00060         const dictionary& transportPropertiesDict_;
00061 
00062         //- Compression coefficient
00063         scalar cAlpha_;
00064 
00065         //- Surface tension
00066         dimensionedScalar sigma_;
00067 
00068         //- Stabilisation for normalisation of the interface normal
00069         const dimensionedScalar deltaN_;
00070 
00071         const volScalarField& alpha1_;
00072         const volVectorField& U_;
00073         surfaceScalarField nHatf_;
00074         volScalarField K_;
00075

cAlpha is the compression coefficient but i really do not understand where is defined and which value is used in the calculations. Is a constant? (even if you do not define any cAlpha in constan/transportProperties.)

Thank a lot
andrea

[kathrin_kissling]

Hi andrea,

it is constant and defined in the fvSolution dictionary.
The read in is in interfaceProperties.C

00146 transportPropertiesDict_(dict),
00147 cAlpha_
00148 (
00149 readScalar
00150 (
00151 alpha1.mesh().solutionDict().subDict("PISO").lookup("cAlpha")
00152 )
00153 ),

Best

Kathrin

[Andrea_85]

Thank you very much, very helpful!

I want to ask one last thing. In the alphaEqn.H what is scalar(1)?

for (int aCorr=0; aCorr<nAlphaCorr; aCorr++)
{
surfaceScalarField phiAlpha =
fvc::flux
(
phi,
alpha1,
alphaScheme
)
+ fvc::flux

(
-fvc::flux(-phir, scalar(1) - alpha1, alpharScheme),
alpha1,
alpharScheme
);


Thanks a lot

andrea

[akidess]

Exactly what it says - a scalar with the value 1. OpenFoam is smart enough to do the arithmetic operation for the entire volField even if one of the operands is a scalar value.

[Andrea_85]

Very simple!

Thanks again

andrea