[RobertHB]

Dear all,
i've managed to add a scalarTransport solver to my pisoFOAM simulation using the #includeFunc scalarTransport command.
This works fine as long as i have an inlet and can define an inlet condition for my scalar value s.

Now, for further simulations using cyclic boundaries, i want to implement a scalar source within my domain using the fvOptions dict and the scalarSemiImplicitSource entry. Following the approach taken in multiple thread here in the forum i added the following part to my fvOptions dict.

Tracer
{
    type            scalarSemiImplicitSource;
    active          true; //using yes doesn't change anything

    scalarSemiImplicitSourceCoeffs
    {
        selectionMode   points;
        volumeMode        absolute;
        points            
        (
            (32 29.1 0.5)
            (32 29.1 1)
            (32 29.1 1.5)
        );
        
        injectionRateSuSp
        {
            s   (1.0 0);
        }
    }
}

And the next line to my controlDict

libs  
(
      "libutilityFunctionObjects.so" 
);

The entry is debugged to the point where the solver starts running, but it does not use the above defined scalar source. The following error is printed:

--> FOAM Warning :
From function virtual void Foam::fv:: option::checkApplied() const
in file cfdTools/general/fvOptions/fvOption.C at line 118
Source Tracer defined for field s but never used
--> FOAM Warning :
From function virtual void Foam::fv:: option::checkApplied() const
in file cfdTools/general/fvOptions/fvOption.C at line 118
Source Tracer defined for field s but never used

So, the question is: Where did i make a mistake? Something seems to be wrong here.

PS: OpenFOAM 4.1 on Ubuntu 16.04 LTS

[tomf]

Hi,

Just a quick response, but I think your scalar would be called Tracer, so I think you need to do this:

        injectionRateSuSp
        {
            Tracer   (1.0 0);
        }

Regards,
Tom

[vs11]

Hi Tom,

I have a similar question regarding fvOptions, I want to add source to the entire domain so i have set the selectionMode to "all". So, do i need to set explicitly the cellSet or cellZone or i can just comment it out like i have done here:

src
{
type scalarSemiImplicitSource;
active true;

scalarSemiImplicitSourceCoeffs
{
selectionMode all; // all, cellSet, cellZone, points
//cellSet c1;
volumeMode specific; // absolute;
injectionRateSuSp
{
src (1 0);
}
}
}

Best,
vaibhav

[tomf]

Hi vaibhav,

I would suggest you try it first and if it does not work you can provide the error message so we can do debugging, but it seems unnecessary to give a cellZone or cellSet is you use the entire domain.

Regards,
Tom

[vs11]

Thanks Tom for your quick reply! I will try it out now.

[RobertHB]

Hey Foamers,
i managed to include a scalar source term in my fvOptions using scalarSemiImplicitSource. But the scalar added by the source is unbounded. While any other inlet method (fixedValue, setFields) nicely bounds between 0 and 1, the scalar source exceeds the upper bound.

Any idea why that is?

[RobertHB]

Please ignore the post #6. Obviously by adding a source, you add to the scalar field.

Coming back to the implemented linear equation where ist the constant part and modifying the scalar field . If is the present field/cell value or the weighted average of all neigbour cells (Pantakar, 1980), why is it that the only equation the fits to the sim. results is ?

The simulation shown above does not contain any transport. Neither diffusion nor advection. It simply shows the accumulation of the scalar quantity in one cell.

[Madeinspace]

Hi Robert,

I did something very similar to add mass source term in interFoam. Simulation run fine but I don't see any sourcer term being added in the computation. Could you kindly look where I might have wronged. The fvOptions code is as:


injector1
{
timeStart 0.1;
duration 0.5;
selectionMode points;
points
(
(0.1 0.35 0.0)
);
}

options
{
massSource1
{
type scalarSemiImplicitSource;
active true;

scalarSemiImplicitSourceCoeffs
{
$injector1;

volumeMode absolute; //org
injectionRateSuSp
{

rho.water (1.0 0); // kg/s //didn't work


}
}
}
}

[Madeinspace]

Hi Robert,

I did something very similar to add mass source term in interFoam. Simulation run fine but I don't see any source term being added in the computational domain when viewing in paraFoam. Could you kindly look where I might have wronged. The fvOptions code is as:

injector1
{
    timeStart       0.1;
    duration        0.5;
    selectionMode   points;
    points
    (
        (0.1 0.35 0.0)
    );
}

options
{
    massSource1
    {
        type            scalarSemiImplicitSource;
    active          true; //added from forum
        
        scalarSemiImplicitSourceCoeffs
        {
            $injector1;

            volumeMode          absolute; 
            injectionRateSuSp
            {

                  rho.water      (1.0 0); // kg/s //


            }
        }
    }
}

[RobertHB]

As a quick guess i'd say the options { } is not needed. Then your timing from injector1 should go into massSource1 {... in here ...}, whereas selectionMode and points should go into scalarSemiImplicitSourceCoeffs {... in here ...}.


Here is my working source (without timing):

scalarSource 
{ 
    type scalarSemiImplicitSource; 
    active true; 

    scalarSemiImplicitSourceCoeffs 
    { 
        volumeMode    specific; 
        selectionMode cellSet; 
        cellSet c0; 

        injectionRateSuSp 
        { 
            T (1 0); 
        } 

    }
 }

and here (LINK) is an OpenFOAM 7.0 example on implementing a timer. See if it helps.