
[Sponsors] 
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: 9 
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: 10 
Hi Vinay
Check out this link in the forum http://www.cfdonline.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: 10 
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: Stockholm, Sweden
Posts: 366
Rep Power: 13 
Did you ever find a solution to the problem of calculating the interface area within the cell?
__________________
~roman 

July 31, 2010, 08:25 
never found one

#6 
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 13 
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, 10:50 
mathematical method

#8 
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 13 
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(1alpha1); 0.5 ≤ α ≤ 1 The code that I used for this is Code:
Foam::tmp<Foam::volScalarField> 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<volScalarField>("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<volScalarField> ( (neg(limitedAlpha10.5)*maxArea*2.0*limitedAlpha1) + (pos(limitedAlpha10.5)*maxArea*(2.0*( limitedAlpha1  1.0))) ); }
__________________
~roman Last edited by romant; July 31, 2010 at 16:36. Reason: missing factor in calculation for the area 

August 1, 2010, 05:29 
create an accessible volume field

#10 
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 13 
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();
__________________
~roman 

October 30, 2014, 04:43 
Length of the interface

#11 
Member
Vignesh
Join Date: Oct 2012
Location: Darmstadt, Germany
Posts: 59
Rep Power: 5 
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: Stockholm, Sweden
Posts: 366
Rep Power: 13 
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.
__________________
~roman 

October 30, 2014, 11:08 

#13 
Member
Vignesh
Join Date: Oct 2012
Location: Darmstadt, Germany
Posts: 59
Rep Power: 5 
Thank you !! Now i get it
__________________
Thanks and Regards Vignesh 

June 8, 2015, 08:13 

#14 
Senior Member
rkhr
Join Date: May 2011
Posts: 231
Rep Power: 8 
HI Foamers,
I am trying to implement Roman's code but I have following error: PHP Code:


June 8, 2015, 10:18 

#15 
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 366
Rep Power: 13 
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: 3 
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: 9,658
Blog Entries: 39
Rep Power: 99 
Quote:
Quote:


September 1, 2015, 17:43 

#18 
Member
HM
Join Date: Apr 2015
Posts: 30
Rep Power: 3 
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: 9,658
Blog Entries: 39
Rep Power: 99 
Greetings Hojjat,
Quote:
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  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to plot time vs distance traveled by the interface interFoam  asaha  OpenFOAM Paraview & paraFoam  9  January 26, 2011 09:05 
InterFoam freeSurface area calculation with sampleSurface  jaswi  OpenFOAM PostProcessing  9  December 10, 2009 12:07 
How to calculate liquid volume as the interface moves for interFoam Solver  asaha  OpenFOAM Running, Solving & CFD  25  October 21, 2009 04:34 
Problems calculating field gh with interFoam  cricke  OpenFOAM Running, Solving & CFD  0  December 10, 2007 08:17 
How to access interface area in vof model???  Asghari  FLUENT  0  April 16, 2007 08:12 