# Implicit source term

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 April 29, 2013, 14:16 Implicit source term #1 Member   Ronald McDonald Join Date: Jul 2012 Posts: 38 Rep Power: 7 Sponsored Links 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*(phiao-phi-EaEqgCell)/(Rg*T)))-(Foam::exp(-alphaca*F*(phiao-phi-EaEqgCell)/(Rg*T)))) );``` Where phi is my volscalarfield (Notice phi is on both sides of the equation). Other variables are independent or constant. 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
 Sponsored Links

 April 29, 2013, 15:52 #2 Senior Member   Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 297 Rep Power: 15 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)` but I don't know how much effect this will have... It's certainly not fully explicit. Cheers, L

April 30, 2013, 13:01
#3
Member

Ronald McDonald
Join Date: Jul 2012
Posts: 38
Rep Power: 7
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
Attached Images
 Selection_043.jpg (7.6 KB, 112 views)

 May 1, 2013, 06:23 #4 Senior Member   Henrik Rusche Join Date: Mar 2009 Location: Braunschweig, Niedersachsen, Germany Posts: 277 Rep Power: 11 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*(phiao-phi-EaEqgCell)/(Rg*T)))-(Foam::exp(-alphaca*F*(phiao-phi-EaEqgCell)/(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.cfd-online.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 sylvester, wyldckat, LarsPT and 2 others like this. 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: 7 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: 277 Rep Power: 11 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: 7
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 if-statement 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;```
The electricpotential.H file has that crazy laplaican(sigmaeff,phi) = source pde. Now the really really interesting thing is that when I look at phi directly in paraview or even after that equation, let's say between electricpotential.H and the curly bracket }, I get an everchanging phi and it seems correct. However, when I look at phi BEFORE the electricpotential.H equation, I get a phi that changes after one time step to a linear curve between its two boundary conditions and that's it. It remains steady thereafter.

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:
 Originally Posted by henrik 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 11, 2013, 12:36 #8 Senior Member   Henrik Rusche Join Date: Mar 2009 Location: Braunschweig, Niedersachsen, Germany Posts: 277 Rep Power: 11 Benjamin, underrelaxation MUST change the residuals - If they do not change, you are not under-relaxing! 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 (non-linear) 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: 7
Thanks, Henrik, for your help. I changed the fvsolutions folder to:

phi
{
solver smoothSolver;
smoother GaussSeidel;
preconditioner DIC;
tolerance 1e-06;
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);```
Where sah2ogCell and sah2gCell both are volscalarfields. I then map those to my specified regions with:

HTML Code:
```    {
forAll (sah2o, cellI)
{
sah2o[cellI] = sah2ogCell[anodeCellMap[cellI]];
}

}

{
forAll (sah2, cellI)
{
sah2[cellI] = sah2gCell[anodeCellMap[cellI]];
}

}```
Then I place them in my diffusion equations like so:

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();```
It compiles fine but I get a floating point exception error after the first iteration. After this if I comment out H2 and make sah2o have an internal field of 1e-14 (previously zero) then that runs without error, but the same does not hold for sah2. Any ideas why I'm getting an error when i try to run it? Is there another why to add these source terms?

Sincerely,

Benjamin

Quote:
 Originally Posted by henrik Benjamin, underrelaxation MUST change the residuals - If they do not change, you are not under-relaxing! 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 (non-linear) 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 30, 2013, 04:54 #10 Senior Member   Henrik Rusche Join Date: Mar 2009 Location: Braunschweig, Niedersachsen, Germany Posts: 277 Rep Power: 11 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: AUS
Posts: 132
Rep Power: 7
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:
 Originally Posted by henrik 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*(phiao-phi-EaEqgCell)/(Rg*T)))-(Foam::exp(-alphaca*F*(phiao-phi-EaEqgCell)/(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.cfd-online.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

 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 strakakl OpenFOAM 38 November 19, 2013 02:18 wind Fluent UDF and Scheme Programming 5 June 21, 2013 05:39 tayo OpenFOAM 39 December 3, 2012 06:18 fs82 OpenFOAM 6 September 23, 2009 03:29 BlGene Open Source Meshers: Gmsh, Netgen, CGNS, ... 10 August 6, 2009 04:26

 Sponsored Links

All times are GMT -4. The time now is 03:26.

 Contact Us - CFD Online - Top