[taalf]

Hi everyone,

I would like to share the solution of a problem that have stuck me for numerous days...

I actually wanted to add a passive scalar to the pimpleFoam solver and to continuously inject this scalar into a cellSet, but the scalar value was stuck inside the cellSet after few iterations without logical reason.

I used OpenFOAM 3.0.1.

Case:

I first added a very simple passive scalar transport equation (without diffusivity) into pimpleFoam.

I inspired myself from this well known tutorial:
http://openfoamwiki.net/index.php/How_to_add_temperature_to_icoFoam

Then I created a custom pimpleFoam solver in which I just copy-pasted the transport equation of the basic/scalarTransportFoam solver.

Something like this (a is the scalar field):

             solve
             (
                 fvm::ddt(a)
               + fvm::div(phi, a)
//               - fvm::laplacian(Da, a)
              ==
                 fvOptions(a)
             );

inside the:

        while (pimple.loop())

I then added a source term in the fvOption file to "inject" the scalar in a given cellSet (obtained thanks to topoSet):

scalarSemiImplicitSource
{
    type            scalarSemiImplicitSource;
    active          true;
    
    scalarSemiImplicitSourceCoeffs
    {
        selectionMode   cellSet;
        cellSet         the_cell_set;
        
        volumeMode      specific; //absolute //specific
        injectionRateSuSp
        {
            a              (1 0);
        }
    }
}

On a small test case like the pitzDaily, everything was correct.

Problem:

But then, on a more complex case, the scalar increased as expected into the cellSet... before being stuck after few iterations. Something like this:

# Probe 0 (-22.08 0 1.79212)
#       Probe             0
#        Time
       0.0001        0.0001  # Growing...
       0.0002   0.000199415  # Growing...
       0.0003   0.000298911  # Growing...
       0.0004   0.00039848   # Growing...
       0.0005   0.000498117  # Growing...
       0.0006   0.000498117  # Stuck!
       0.0007   0.000498117
       0.0008   0.000498117

The most surprising thing was that the number of iterations before being stuck was depending on... things like the fineness of the mesh (outside the cellSet) and the dimensions of the cellSet. So it was very strange...

Solution:

Now, here it the reason.

After switching to OpenFOAM 2.4 and 4.0 (same results), after trying the same with pisoFoam (without any improvement), after trying numerous modifications in my solver and checking one hundred times the fvSolution and fvScheme files, I finally had a look at... the log file of my computation.

The Initial residual for my scalar transport equation was under its tolerance, leading to a number of iterations equaling zero. This is why the scalar was stuck.

DILUPBiCG:  Solving for a, Initial residual = 7.45438e-06, Final residual = 7.45438e-06, No Iterations 0

To solve this, I simply moved the line "tolerance" from the "a" to the "aFinal" dictionary in the fvSolution file and ... it works like a charm

    a
    {
        solver          PBiCG;
        preconditioner  DILU;
        relTol          0.1;
    }
    
    aFinal
    {
        $a;
        tolerance       1e-5;
        relTol          0;
    }

Conclusion:

When one doesn't know where to find the error, look first around your feet before looking at the horizon...

... Hope this will help people crossing the same issue.

Best regards,

[blais.bruno]

Thanks for sharing!
I had a similar problem before. I think that when debugging or looking at a very specific thing, setting all residual to drastically low value is a good habit just to make sure the issue isnt there. Then you can increase them progressively for the large simulations !