
[Sponsors] 
February 16, 2011, 07:54 
Vof method in interFoam

#1 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 303
Rep Power: 9 
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 

February 16, 2011, 08:55 

#2 
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 14 
You can have a look here for example, some useful information and references are given:
http://www.cfdonline.com/Forums/ope...ofmethod.html 

February 16, 2011, 08:56 

#3 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,164
Rep Power: 20 
Have a look at the thesis by Henrik Rusche, it contains all the basics.


February 16, 2011, 09:09 

#4 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 303
Rep Power: 9 
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 

February 16, 2011, 11:29 

#5 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 303
Rep Power: 9 
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 

February 17, 2011, 03:30 

#6 
Senior Member
Kathrin Kissling
Join Date: Mar 2009
Location: Besigheim, Germany
Posts: 134
Rep Power: 9 
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 

February 17, 2011, 04:42 

#7 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 303
Rep Power: 9 
Thanks Kathrin,
I copy and paste from interfacePropierties.H (not all the file): Code:
/**\ 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 Thank a lot andrea 

February 17, 2011, 04:50 

#8 
Senior Member
Kathrin Kissling
Join Date: Mar 2009
Location: Besigheim, Germany
Posts: 134
Rep Power: 9 
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 

February 17, 2011, 05:14 

#9 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 303
Rep Power: 9 
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 

February 17, 2011, 05:20 

#10 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,164
Rep Power: 20 
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.


February 17, 2011, 05:41 

#11 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 303
Rep Power: 9 
Very simple!
Thanks again andrea 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
VOF Interfacial Area  2D/3D Reconstruction Method  Greg Perkins  Main CFD Forum  2  September 10, 2012 04:05 
How to apply VOF method?  yeeking86  CFX  7  August 23, 2010 18:24 
slop in Hirt's VOF method  GCM  Main CFD Forum  0  July 28, 2009 15:44 
Are the VOF results of interFoam grid independent  asaha  OpenFOAM Running, Solving & CFD  1  June 26, 2009 04:27 
VOF method on intertank transfer  Louis  FLUENT  0  March 14, 2006 10:28 