
[Sponsors] 
April 29, 2013, 14:16 
Implicit source term

#1 
Member
Ronald McDonald
Join Date: Jul 2012
Posts: 38
Rep Power: 5 
Dear openFoamers,
I'd like to add an implicit source term to my pde. It would look like this: HTML Code:
solve ( Foam::fvm::laplacian(sigmaeff, phi) == iagCell*((Foam::exp(alphaaa*F*(phiaophiEaEqgCell)/(Rg*T)))(Foam::exp(alphaca*F*(phiaophiEaEqgCell)/(Rg*T)))) ); I looked at OpenFoam documentation, specifically from this site: http://www.foamcfd.org/Nabla/guides/...sGuidese9.html And it talks about using Su, Sp, and SuSp. I would like to use those things but I'm not sure how to. In the documentation it talks about a rho and phi, where rho can either be a dimensioned scalar or a volscalarField, and phi is the volscalarfield. Now in my pde I do not know what rho would be. Also, I found another link talking about this: http://openfoamwiki.net/index.php/Ho...sport_equation Any help you, the community, could provide would be great! Sincerely, Benjamin 

April 29, 2013, 15:52 

#2 
Senior Member
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 14 
Hi Benjamin,
If you do a incompressible simulation, rho is simply 1.0. Now, regarding your source term. The fact that it is inside the exponential function makes it impossible to included implicitly. This is only possible for linear systems. The closest you will probably get is something like Code:
fvm::Sp(exp(...)/phi,phi) Cheers, L 

April 30, 2013, 13:01 

#3 
Member
Ronald McDonald
Join Date: Jul 2012
Posts: 38
Rep Power: 5 
Dear openFoamers,
Thank you for your response, Lieven. I suppose I cannot implement an implicit source term in that manner, specifically using the Foam::fvm::Sp function of openFoam. Then I am stumped on how to implement the pde in openFoam. My equation with more clarity is attached to this file using Latex. where phi_e is the volscalarField and all others are either constant or independent of phi. When I put this equation into openFoam directly I get some funky results, incorrect as compared to similar simulations. Thus, I think it has to do with the phi on the right side of the equation and the equation as an implicit pde. Any help would be really great as I feel that this is my last and final hurdle to get my simulation running smoothly. Sincerely, Benjamin 

May 1, 2013, 06:23 

#4 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 275
Rep Power: 10 
Dear Benjamin,
Yes, I am not surprised that you are having trouble with that source ... Did you try to underrelax? fvMatrix phiEqn ( fvm::laplacian(sigmaeff, phi) == iagCell*((Foam::exp(alphaaa*F*(phiaophiEaEqgCell)/(Rg*T)))(Foam::exp(alphaca*F*(phiaophiEaEqgCell)/(Rg*T)))) ); phiEqn.relax(0.5); phiEqn.solve(); Make sure to b build/solve multiple times! I order to make it (more) implicit, you need to linearise your source term. There are many ways, but I suggest to use Picard's method. http://www.cfdonline.com/Wiki/Sourc..._linearization Once you get through the maths, the code will look volScalarField Sp = // derived equations volScalarField Sc = // derived equations fvMatrix phiEqn ( fvm::laplacian(sigmaeff, phi) == fvm::Sp(Sp, phi) + Sc ); phiEqn.relax(0.5); phiEqn.solve(); Best Regards, Henrik Last edited by henrik; May 1, 2013 at 10:14. 

May 8, 2013, 12:16 

#5 
Member
Ronald McDonald
Join Date: Jul 2012
Posts: 38
Rep Power: 5 
Dear openFoamers,
Thank you, Henrik, for your help. I am still trying to linearize but I have another idea. I would like to do the following: Etta = phiao  phi  EaEqgCell; If Etta > .5 then Etta = .5; Else Etta = phiao  phi EaEqgCell; fvMatrix phiEqn ( fvm::laplacian(sigmaeff, phi) == iagCell*((Foam::exp(alphaaa*F*(Etta)/(Rg*T)))(Foam::exp(alphaca*F*(Etta)/(Rg*T)))) ); phiEqn.relax(0.5); phiEqn.solve(); It's the if statement I am having trouble with. How would I do that in my solver? How to create an if statement? Sincerely, Benjamin 

May 8, 2013, 16:20 

#6 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 275
Rep Power: 10 
Benjamin,
Did you try to underrelax? Did it make a difference? Having a switch is nasty  especially if you try to linearise. Anyway, the way to do it is to use the pos and neg functions. Alternatively, you can loop through the field cell by cell and use raw C++. Henrik 

May 10, 2013, 14:28 
Pleasantly perplexed

#7  
Member
Ronald McDonald
Join Date: Jul 2012
Posts: 38
Rep Power: 5 
Dear OpenFoamers,
Hi Henrik. I did try to underrelax and it didn't make a difference, I got an error right away. I did put an ifstatement in and it ran without an error. However, it leads to another problem I have. Currently, my solver looks like this: HTML Code:
Info<< "\nCalculating concentration distribution\n" << endl; while (simple.loop()) { Info<< "Time = " << runTime.timeName() << nl << endl; //**Add laplacians to all four species: O2, N2, H2O, H2 while (simple.correctNonOrthogonal()) { #include "diffusion.H" #include "partialpressure.H" #include "equilibriumpotential.H" #include "currentdensity.H" #include "mapToCell.H" #include "Etta.H" #include "chargedensity.H" #include "electricpotential.H" } //#include "mapFromCell.H" #include "write.H" Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; } Info<< "End\n" << endl; return 0; Now I think there is something going on with the "solve" command that allows openFoam to be able to get the old value and put it back into the equation. It seems like outside and BEFORE the solve equation it is not reading the old values back. But AFTER the solve equation it seems to work well. Now to my question: how do I read back the output of the solve equation, place it before my electricpotential.H file (so that I can edit it) and then place it back into my pde? In essence, I would like to see phi changing when I check on it BEFORE my solve equation of the pde. What do you, the community of openFoamers, think about this obfuscating situation? Sincerely, Benjamin Quote:


May 11, 2013, 12:36 

#8 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 275
Rep Power: 10 
Benjamin,
underrelaxation MUST change the residuals  If they do not change, you are not underrelaxing! I am entirely sure that I understand what you are trying to do, but I will provide enough rope to you in order to hang yourself The solve statement writes the result into field it is operating on. If you put loops into your code, the explicit terms see the new (time) values. The idea here is to iterate until the (nonlinear) system of equations converges. Of course, ddt() needs the old time values to function correctly and that's why they are stored automagically. You can retrieve them by calling .oldTime() on the field. Henrik 

May 29, 2013, 16:47 

#9  
Member
Ronald McDonald
Join Date: Jul 2012
Posts: 38
Rep Power: 5 
Thanks, Henrik, for your help. I changed the fvsolutions folder to:
phi { solver smoothSolver; smoother GaussSeidel; preconditioner DIC; tolerance 1e06; relTol 0; } And it runs without error. I'm not sure why. And it also takes about 6x longer to run, which sucks. I am onto a new problem, also with source terms. Currently, I have as the source terms: HTML Code:
sah2ogCell = jbvagCell/(F*4)*H2OMM; sah2gCell = jbvagCell*H2MM/(4*F); HTML Code:
{ forAll (sah2o, cellI) { sah2o[cellI] = sah2ogCell[anodeCellMap[cellI]]; } } { forAll (sah2, cellI) { sah2[cellI] = sah2gCell[anodeCellMap[cellI]]; } } HTML Code:
fvScalarMatrix H2OEqn ( fvm::ddt(H2O) == fvm::laplacian(DH2Oeff, H2O) + sah2o ); H2OEqn.solve(); fvScalarMatrix H2Eqn ( fvm::ddt(H2) == fvm::laplacian(DH2eff, H2)  sah2 ); H2Eqn.solve(); Sincerely, Benjamin Quote:


May 30, 2013, 04:54 

#10 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 275
Rep Power: 10 
Dear Benjamin,
How many iterations does the linear solver take? Probably a lot. If so, switch to GAMG  that should be much more efficient as laplacians are a prime target for these solvers. Do you employ outer iterations, ie. do you solve phi multiple times per time step? If so, Picard's method should speed up convergence. It's hard to tell what is going wrong in your new problem. First thing to do is to write out the source fields and check that they are correct. A likely problem is that of boundedness, ie. negative source terms will drive your species negative. I your current implementation there is nothing to prevent this. You should make the source implicit fvm::Sp and possibly clip after the solution. Have a look into reactingFoam how this can be done. Henrik 

September 8, 2013, 06:47 
Implicit source term

#11  
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AU
Posts: 126
Rep Power: 6 
Hi Henrik,
I have a stupid question to ask. What do you mean by "build/solve it multiple times!!"? Is it be done in the solve() function considering the tolerance in the fvSolution automatically?? or I have to add another loop inside the time loop like: while(runTime.loop()) { do ( volScalarField Sp = // derived equations volScalarField Sc = // derived equations fvMatrix phiEqn ( fvm::laplacian(sigmaeff, phi) == fvm::Sp(Sp, phi) + Sc ); phiEqn.relax(0.5); phiEqn.solve(); )while(...condition) } Quote:


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
transient source term  strakakl  OpenFOAM  38  November 19, 2013 02:18 
Problem of SOURCE term gradient in UDS  wind  Fluent UDF and Scheme Programming  5  June 21, 2013 05:39 
funkySetFields compilation error  tayo  OpenFOAM  39  December 3, 2012 06:18 
Adding implicit source term to momentum equation  fs82  OpenFOAM  6  September 23, 2009 03:29 
Compiling gmshFoam with OpenFOAM1.5  BlGene  Open Source Meshers: Gmsh, Netgen, CGNS, ...  10  August 6, 2009 04:26 