Vof method in interFoam
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 
You can have a look here for example, some useful information and references are given:
http://www.cfdonline.com/Forums/ope...ofmethod.html 
Have a look at the thesis by Henrik Rusche, it contains all the basics.

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 
I think, if I understand correctly, that the equation that OF solves is:
d(alpha)/dt +div(alpha*U)+div(Ur*alpha*(1alpha))=0 Is correct? where i can find the definition of Ur in the code and and how is it calculated? andrea 
1 Attachment(s)
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 
Thanks Kathrin,
I copy and paste from interfacePropierties.H (not all the file): Code:
/**\ Thank a lot andrea 
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 
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 
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.

Very simple!
Thanks again andrea 
All times are GMT 4. The time now is 09:51. 