
[Sponsors] 
November 28, 2011, 06:26 
InterFoam: add a source term in alpha eq.

#1 
Member
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 10 
Goodmorning,
I'm try to simulate the growth of a cristal using,as a basis, interfoam. As i'm at the beginning, i consider as a first case, a simple 2D circle that grows at a constant velocity "Uoo". Alpha=1 in the circle and 0 outside. So what i want to "see" it's just a simple circle that grows in time in my square domain. If the basic alpha transport equation is something like that: d(alpha)/dt+U*grad(alpha)=0 in my case I add a "second" velocity that is the envelope growth: d(alpha)/dt+U*grad(alpha)+Ug*grad(alpha)=0 So if I initialise my U=0 (I 've not motion of my circle) and I impose a constant Ug, how it's possible to integrate correctly this term "Ug*grad(alpha)" in the equation? I tried to replace directly U=Ug BUT the calculation of the phi fluxes is quite complicated and realted to Ueqn so I cannot do that easily. I know perhaps is a dummy question but it's 10 days I'm trying to figure out how to solve it and I don't see a clever solution to that. Thank you in advance. Last edited by Alucard; November 28, 2011 at 06:42. 

November 28, 2011, 08:37 

#2 
Member
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 9 
Hi,
if i were you i would take a look at the alphaEqn.H of interPhaseChangeFoam and just tailor it to suite your needs. Although i don't understand your reasons behind it, because the alpha transport equation reads somehow different from what you have posted here. 

November 28, 2011, 09:24 

#3  
Member
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 10 
Quote:
thank you I'm looking at it right now I guess I've to work on the "Su" term (I don't know exactly how yet! Why I'm using the interfoam approach? Cause I have two phases in my study (liquid and solid) and So I need a "marker" for the phase. So as I need a method that allows me to transport phases without numerical diffusion I thought to interFoam where all the "tricks" in order to have a sharp interface during time are already developped. So i tried rigid translations and roatation of a circle with success and now I was trying to add the term related to surface growth. In the complete problem it will be function of Temperature and other thermodynamical parameters but for the moment I impose it. Why so do you think my approach is not the good one? Thanks 

November 28, 2011, 09:39 

#4 
Member
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 10 
So a good way to do that could be to write the "Su" term like that?
volScalarField Su ( IOobject ( "Su", runTime.timeName(), mesh ), // Divergence term is handled explicitly to be // consistent with the explicit transport solution fvc::grad(alpha1) & Ug ); where Ug is the "growth velocity" vector field (I already initalised in my code)? Thank you again. 

November 28, 2011, 09:41 

#5 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 265
Rep Power: 11 
Hello,
I think interFoam is not the best method in cristal grow, because usually the interface transition is very sharp, and with VOF method, you will get a "sharp but not enough" interface, + difficulties to set thermal source / density. The best method may be Level set, but i don"t know how to deal with in OpenFoam (though i've seen a VOF/ level set coupling related to openFoam somewhere in a workshop pdf.) Anyway, i would try to setup an hybrid buoyant+InterFoam, i.e thermal with variable properties and VOF, so if you go that way, we can share some part of the solver. regards, olivier 

November 28, 2011, 10:20 

#6 
Member
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 9 
Hi Alucard,
yes your Su looks fine, give it a try. From the point of view of OF it looks good , if it makes sense from a point of view of the physics you'll see. Greets 

November 28, 2011, 13:02 

#7  
Member
valerio
Join Date: Jun 2009
Location: Nancy
Posts: 30
Rep Power: 10 
Quote:
it worked in OF (compilation+running) but not under a phisical point of view...I don't know why, i also tried to solve explicitly the equation: " alpha1=alpha1runTime.deltaT()*(Ug_mod*mag(fvc::grad(alpha1))); " with Ug_mod, module of the velocity vector but I'm having strong oscillations close to the circleinterface and alpha that becomes higher than 1. Do you think something is wrong? (before I tried to put Su as supposed and i got the same kinda of results) 

November 29, 2011, 05:10 

#8 
Member
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 9 
Hmm,
don't worry it never works at the first try Did you also implement source and sink terms to the pEqn and UEqn? Because it might be that you create some 1st phase but do not transport it away. Bon courage! Sabin 

November 29, 2011, 09:50 

#9 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,261
Rep Power: 23 
olivierG, the solidliquid interface is sharp for pure materials, and diffuse for melting of alloys.
Nonetheless I agree interFoam is not the best choice for this problem. Instead, if not too late, I recommend having a look at phasechange solvers which other users have posted: http://www.cfdonline.com/Forums/ope...gproblem.html 

January 13, 2012, 11:16 
melting solver

#10 
Senior Member
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 210
Rep Power: 11 
Hi all
nice that my melting solver http://www.cfdonline.com/Forums/ope...gproblem.html made it into another thread of this forum. I although tried using interFoam for melting and solidification problems. But as you have a solid phase, alpha cannot be transported as done in VOF. My solver uses the enthalpyporositymethod proposed by Voller. The solver will be improved in the next months. Regards Fabian 

April 22, 2017, 00:27 
Urgent: Addition of source term to alpha equation in interFoam

#11 
New Member
Akshay
Join Date: Nov 2016
Location: Chennai,India
Posts: 7
Rep Power: 2 
Hi all,
I want to add a source term to the alpha equation in the interFoam solver. I am using OpenFOAMv1612+ version. I tried to do it in the following way I added following to alphaEqn.H Code:
//Creating Source Terms for alpha equation volScalarField::DimensionedField Su ( IOobject ( "Su", runTime.timeName(), mesh ), mesh, dimensionedScalar("Su", dimensionSet(0,0,1,0,0,0,0), scalar(0.0)) ); volScalarField::DimensionedField Sp ( IOobject ( "Sp", runTime.timeName(), mesh ), mesh, dimensionedScalar("Sp", dimensionSet(0,0, 1,0,0,0,0), 0.0) ); Code:
fvScalarMatrix alpha1Eqn ( ( LTS ? fv::localEulerDdtScheme<scalar>(mesh).fvmDdt(alpha1) : fv::EulerDdtScheme<scalar>(mesh).fvmDdt(alpha1) ) + fv::gaussConvectionScheme<scalar> ( mesh, phiCN, upwind<scalar>(mesh, phiCN) ).fvmDiv(phiCN, alpha1) == Sp ); Code:
if( (sourceZ0.05<=centroidZ) & (centroidZ < sourceZ)) { if(alpha1[cellI] < 0.5) { Sp[cellI] = 1; } else { Sp[cellI] = 0; } } if( (sourceZ<centroidZ) & (centroidZ<=sourceZ+0.05)) { if(alpha1[cellI] < 0.5) { Sp[cellI] = 1; } else { Sp[cellI] = 0; } } else { Sp[cellI] = 0; } Can anyone please help with this? Whether the way I declared the source term is right or wrong? And the way I added it to the equation? It is really urgent so please help me if possible. Thanking you, Akshay 

August 3, 2017, 02:23 

#12  
Member
Mahdi
Join Date: Jul 2012
Posts: 50
Rep Power: 7 
Quote:
I am not sure if you have already found the answer, but for others: You would need to take a look at the source code of MULES as well as the how it is impelemented in interPhaseChangeFoam. Therefore, it seems you should just add: MULES::correct(geometricOneField(), alpha1, talphaPhiUn(), talphaPhiCorr.ref(), Sp, Su, 1, 0); and MULES::explicitSolve(geometricOneField(), alpha1, phiCN, alphaPhi, Sp, Su, 1, 0); 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
GPU Linear Solvers for OpenFOAM  gocarts  OpenFOAM Announcements from Other Sources  36  March 29, 2017 08:05 
Solve poisson equation just add a source term  nandiganavishal  OpenFOAM Running, Solving & CFD  17  January 21, 2017 05:24 
DxFoam reader update  hjasak  OpenFOAM PostProcessing  69  April 24, 2008 01:24 
How can I add a source term  danielle  OpenFOAM Running, Solving & CFD  1  February 29, 2008 12:52 
UDFs for Scalar Eqn  Fluid/Solid HT  Greg Perkins  FLUENT  0  October 11, 2000 03:43 