# Vof method in interFoam

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 16, 2011, 07:54 Vof method in interFoam #1 Senior Member   Andrea Ferrari Join Date: Dec 2010 Posts: 275 Rep Power: 7 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: 12 You can have a look here for example, some useful information and references are given: VOF method

 February 16, 2011, 08:56 #3 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 919 Rep Power: 17 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: 275 Rep Power: 7 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: 275 Rep Power: 7 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

February 17, 2011, 03:30
#6
Senior Member

Kathrin Kissling
Join Date: Mar 2009
Location: Besigheim, Germany
Posts: 134
Rep Power: 8
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
Attached Images
 formel.png (7.7 KB, 163 views)

 February 17, 2011, 04:42 #7 Senior Member   Andrea Ferrari Join Date: Dec 2010 Posts: 275 Rep Power: 7 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``` 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

 February 17, 2011, 04:50 #8 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 8 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: 275 Rep Power: 7 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

 February 17, 2011, 05:20 #10 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 919 Rep Power: 17 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: 275 Rep Power: 7 Very simple! Thanks again andrea

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Greg Perkins Main CFD Forum 2 September 10, 2012 04:05 yeeking86 CFX 7 August 23, 2010 18:24 GCM Main CFD Forum 0 July 28, 2009 15:44 asaha OpenFOAM Running, Solving & CFD 1 June 26, 2009 04:27 Louis FLUENT 0 March 14, 2006 10:28

All times are GMT -4. The time now is 05:00.