# Calculating Interface Area with InterFoam

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

 August 23, 2007, 15:47 Hello, I am interested in i #1 New Member   Vinay Ramohalli Gopala Join Date: Mar 2009 Location: Netherlands Posts: 13 Rep Power: 10 Sponsored Links Hello, I am interested in implementing Mass and Heat transfer across the interface using VOF (interFoam solver), which requires an accurate description of the interfacial area in each cell. Can someone suggest a way to calculate the interfacial area using the present interFoam VOF implementation? Thanks in advance,

 August 24, 2007, 05:58 Hi Vinay Check out this li #2 Senior Member   Join Date: Mar 2009 Posts: 248 Rep Power: 11 Hi Vinay Check out this link in the forum http://www.cfd-online.com/OpenFOAM_D...ges/1/172.html Regards Jaswinder

 February 26, 2009, 08:34 The links seems to be dead. C #3 Senior Member   Fabian Roesler Join Date: Mar 2009 Location: Germany Posts: 210 Rep Power: 11 The links seems to be dead. Can anybody post the correct link of the discussion? Thanks allot in advance. Regards Fabian

 February 17, 2010, 11:32 interface area #4 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 14 Did you ever find a solution to the problem of calculating the interface area within the cell? __________________ ~roman

 July 31, 2010, 05:34 #5 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,216 Blog Entries: 1 Rep Power: 17 hi friends did you find any way to calculate interface area ?

 July 31, 2010, 08:25 never found one #6 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 14 Hej, I tried finding a solution, but I in the end created a model to simulate and predict the size of the interface area. I assumed that the size of the cell is regular. Then calculated the area that is double diagonal within the a regular cell (in this case a cube then) and varied the size of the interface area with the amount of alpha1 within the cell, max at 0.5 alpha1 and full size of the double diagonal area. Of course this can be made better. Additional information that can be used within such a model can be the velocity, the angle at which the interface is within the cell and the irregularity of the cell. __________________ ~roman

 July 31, 2010, 10:36 #7 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,216 Blog Entries: 1 Rep Power: 17 hi roman could you please describe ur method step by step or mathematically because i didnt get what you said it was ambiguous for me thanks in advance

 July 31, 2010, 10:50 mathematical method #8 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 14 assume a regular cell. in the case of a hexahedral cell this means, a cube with sides of length a. This length is obtainable by using the volume of a cell,V , and taking the third root. You can put a plane diagonally through the cube. The size of this plane is given by Amax =√(3) * V^(2/3) When the cell is now filled with phase 1, you can read the alpha1 value. The maximum area, Amax, is now varied based on the alpha1 value. with A = Amax*2 * alpha1; 0 ≤ α < 0.5 A = Amax*2(1-alpha1); 0.5 ≤ α ≤ 1 The code that I used for this is Code: Foam::tmp Foam::phaseChangeTwoPhaseMixtures::AlbaNovaInterface::interfaceArea() const { // return the interfacial area based on model for interfacial area // returns dimensions Area // model based on regular volume cells, taking the largest cut area // as maximum for area, linear increase and decrease with alpha const volScalarField& cellVolume = alpha1_.db().lookupObject("cellVolu"); volScalarField limitedAlpha1 = min(max(alpha1_, scalar(0)), scalar(1)); const dimensionedScalar areaFactor("areaFactor",dimensionSet(0,2,0,0,0,0,0), 0.0); volScalarField interfaceArea = alpha1_ * areaFactor; volScalarField maxArea = alpha1_ * areaFactor; maxArea = sqrt(3.0)*pow(cellVolume,(2.0/3.0)); return tmp ( (neg(limitedAlpha1-0.5)*maxArea*2.0*limitedAlpha1) + (pos(limitedAlpha1-0.5)*maxArea*(-2.0*( limitedAlpha1 - 1.0))) ); } I know that the code is not the cleanest and strictest code. For example at the part where the field with the interface areas are created, but it was at a time I didn't know too much yet :-) __________________ ~roman Last edited by romant; July 31, 2010 at 16:36. Reason: missing factor in calculation for the area

 August 1, 2010, 02:53 #9 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,216 Blog Entries: 1 Rep Power: 17 thank roman but could please tell me how could u get "cellVolu" in ur code ?

 August 1, 2010, 05:29 create an accessible volume field #10 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 14 Hej, I created a volume field in createFields.H Code: // create access for cell volumes during runtime // needed by AlbaNovaInterface volScalarField cellVolu ( IOobject ( "cellVolu", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), mesh, dimensionedScalar("zero", dimVolume, 0.0) ); cellVolu.internalField() = mesh.V(); this is now available throughout the runtime. It is never written, but is readable. __________________ ~roman

 October 30, 2014, 04:43 Length of the interface #11 Member   Vignesh Join Date: Oct 2012 Location: Darmstadt, Germany Posts: 63 Rep Power: 6 Dear All, I know this thread is old but, I would like to know how to calculate the length of the interface in interfoam ? __________________ Thanks and Regards Vignesh

 October 30, 2014, 04:47 #12 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 14 One way if determining the interface size has been described in the previous posts. A length would not be a real size for a cells, as a cell 3D and you need an area. vigneshTG likes this. __________________ ~roman

October 30, 2014, 11:08
#13
Member

Vignesh
Join Date: Oct 2012
Posts: 63
Rep Power: 6
Quote:
 Originally Posted by romant One way if determining the interface size has been described in the previous posts. A length would not be a real size for a cells, as a cell 3D and you need an area.
Thank you !! Now i get it
__________________
Thanks and Regards

Vignesh

 June 8, 2015, 08:13 #14 Senior Member   Join Date: May 2011 Posts: 231 Rep Power: 9 HI Foamers, I am trying to implement Roman's code but I have following error: PHP Code:                                           ^ In file included from alphaEqnSubCycle.H:35:0,                  from myInterConPhaseChangeFoam.C:83: alphaEqn.H: In function ‘int main(int, char**)’: alphaEqn.H:86:3: error: ‘mDotCondense’ was not declared in this scope    mDotCondense = mDotcAlphal*(1-alpha1); // multiply by (1-alpha1) because given back that way    ^ In file included from alphaEqnSubCycle.H:40:0,                  from myInterConPhaseChangeFoam.C:83: alphaEqn.H:86:3: error: ‘mDotCondense’ was not declared in this scope    mDotCondense = mDotcAlphal*(1-alpha1); // multiply by (1-alpha1) because given back that way    ^ In file included from myInterConPhaseChangeFoam.C:61:0: /usr/local/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/readTimeControls.H:38:8: warning: unused variable ‘maxDeltaT’ [-Wunused-variable]  scalar maxDeltaT =         ^ make: *** [Make/linux64GccDPOpt/myInterConPhaseChangeFoam.o] Error 1  Can you help me?

 June 8, 2015, 10:18 #15 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 368 Rep Power: 14 I think to understand how the code is implemented, you need to take a look at how the other models for cavitationFoam are implemented. Different models could be chosen in version 1.7 for which this model was created. I am not sure what it looks like today (as of version 2.3 or 2.4). The models that I implemented were not hard coded into the solver but where as all the other models selectable. __________________ ~roman

 September 1, 2015, 10:47 Calculating interface area of a jet #16 Member   HM Join Date: Apr 2015 Posts: 30 Rep Power: 4 Hi Foamers, I am running some simulations on a jet impacting a quiescent pool with interFoam. I was wondering if there is any way that we can calculate the interfacial area of a jet at the impact location. Thanks in advance.

September 1, 2015, 15:36
#17
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
Quote:
 Originally Posted by jaswi Check out this link in the forum http://www.cfd-online.com/OpenFOAM_D...ges/1/172.html
Quote:
 Originally Posted by fabian_roesler The links seems to be dead. Can anybody post the correct link of the discussion?
6 years too late, but here's the recovered link that I found via web.archive.org: https://web.archive.org/web/20080130...tml?1108672034

 September 1, 2015, 17:43 #18 Member   HM Join Date: Apr 2015 Posts: 30 Rep Power: 4 Bruno thanks for the reply, but I am only interested in the interface area of the jet at the impinging location. The method described will calculate the interface area all over the pool and the bubbles beneath the surface, which I am not interested. Thanks

September 12, 2015, 15:38
#19
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
Greetings Hojjat,
Quote:
 Originally Posted by hojjat.m but I am only interested in the interface area of the jet at the impinging location.
If the impact location was a wall (water jet moving through the air onto a wall), it would be fairly easy. If the interface area was between two different fluids in a three fluids simulation, it would be doable.
Problem is that you want to calculate the impact area between two fluids of the same ... er, wait, is it a jet of a fluid different from the quiescent fluid in the pool?

In other words: without a clear picture/image of what you're trying to calculate, I don't know if it's even possible at all.
At best, I can imagine it would be possible to calculate the area in a cross section of the domain that is operating at a certain flow speed for a specific phase.

Best regards,
Bruno
__________________

Last edited by wyldckat; September 12, 2015 at 15:39. Reason: added more details to the initial description

 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 asaha OpenFOAM Paraview & paraFoam 9 January 26, 2011 09:05 jaswi OpenFOAM Post-Processing 9 December 10, 2009 12:07 asaha OpenFOAM Running, Solving & CFD 25 October 21, 2009 04:34 cricke OpenFOAM Running, Solving & CFD 0 December 10, 2007 08:17 Asghari FLUENT 0 April 16, 2007 08:12