[cfdonline2mohsen]

Dear Foamers
Hi!

I want to add a constant volumetric source term to the scalar transport equation which acts only in a particular volumetric region of the domain.

I modified the scalar transport equation as follows:

solve
	(
	  fvm::ddt(T)
	  + fvm::div(phi, T)
	  - fvm::laplacian(DT, T)
	  ==
	  sourceValue
	);

Then I defined the sourceValue in the createFields.H file as follows:

dimensionedScalar sourceValue(twoPhaseProperties.lookup("sourceValue"));

It will read the sourceValue from the transportProperties file of my case. In the transportProperties file,I gave the sourceValue as follows:

sourceValue      sourceValue [0 0 -1 0 0 0 0] 0.42;

By using this approach, the sourceValue=0.42 is used for the entire domain but I want to use the sourceValue=0.42 for only a specific volumetric region inside my domain.

I have two questions:

1) How can I define this volumetric region inside my domain? is there any utility?

2) How can I change the transportProperties file to consider sourceValue=0.42 only for this specific volumetric region and sourceValue=0 for the rest of the domain?


Any help in this regard would be much appreciated.
Thank you so much in advance.

[zfaraday]

Maybe your approach would be to create your source region by using topoSet utility first. Then, once you have created your zone where you want to locate your source, you can use the fvOption framework in order to create the source (I assume it's a heat source). It's an easy approach and you don't need to modify your solver!

Regards,

Alex

[Cyp]

or declare your sourceTerm as a volScalarField and assign it different values (0 and 0.42) with setField

[fabian_roesler]

The tip with the cellZone is correct. You can add whatever source you like throughout a fvOption:

energySource 
{ 
    type            scalarSemiImplicitSource; 
    active          true; 
    selectionMode   cellZone; 
    cellZone        porosity; 
 
    scalarSemiImplicitSourceCoeffs 
    { 
        volumeMode      absolute; 
        injectionRateSuSp 
        { 
            h           (10 0); 
        } 
    } 
}

The value for an absolute heat source is given in unit [W] while the specific heat is volume specific and is given in [W/m³]. Some other possible sources are:

• Mass source in kg/s (absolute) or kg/m³s (specific)
• Momentum source in kg m/s² (absolute) or kg/m²s² (specific)
• Heat source in J/s (absolute) or J/m³s (specific)

Cheers

Fabian

[cfdonline2mohsen]

Thanks Cyprien
I thought that setFields can only be used for initial conditions (initialization) like the dam break example in the user guide?
Am I wrong?
Because my source exists there all the time not only at t=0.
I quote the user guide:

setFields     Set values on a selected set of cells/patchfaces through a dictionary

Can I use setFields to set my sourceValue on a particular volumetric region of the domain for all the timesteps? and How?

It's so kind of you.

[fabian_roesler]

No you can't. As a source term is not just setting a simple value but solving for it implicit during the solution process, setFields will not help you much. It's only a tool to set initial conditions.
Create a cellZone and use fvOptions or change your solver code to implement a source to your equation.

Cheers

Fabian

[Cyp]

Once you have assign different values to your "sourceTerm" with setFields your source term will have the same value for all the time steps.

[ARTem]

Also you can use more general approach, if e.g. you have a function describing the source distribution S = f(x,y,z). You should edit createFields.H by adding

volScalarField S
(   
    IOobject
    (   
        "S",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
    ),
    mesh,
    // yourSourceDimension is dimensionSet(0,0,0,0,0) with appropriate dimensions
    dimensionedScalar("S",yourSourceDimension,scalar(0))
);

forAll(mesh.C(), celli)
{
   vector Ci = mesh.C()[celli];
   // For a general case
   // S[celli] = yourFunction(Ci.x(), Ci.y(), Ci.z());

   // For your case
   if(Ci.x() > x1 && Ci.x() < x2) S[celli] = S1;
   else S[celli] = S2; 
}

S.write() // Writing just ones for checking S distribution in paraview

with yourFunction beeing "scalar yourFunction(scalar x, scalar y, scalar z) const;" and x1, x2 being scalar type.

[cfdonline2mohsen]

Originally Posted by Cyp

Once you have assign different values to your "sourceTerm" with setFields your source term will have the same value for all the time steps.

Thanks Cyprien
But I think you are wrong!
When you assign different values to your field with setFields, It will not have the same value for all the time steps!
setFields is only designed for setting the initial conditions on your fields as stated by fabian_roesler in this post and also by Bernhard in #4 and also in #5.
If you take a look at Figure 2.21 on page U-60 of the user guide and compare it with Figure 2.22, you will see that it will change.

Thanks you so much again.

[cfdonline2mohsen]

Thank you all.

I think I can not use setFields as stated by Cyp for this purpose.
Then I have two options:

1) fvOptions and topoSet utilities as stated by zfaraday and fabian_roesler
which is only available after OpenFOAM v2.2.0.

2) Modifying my solver to implement my source into the equation as stated by ARTem and fabian_roesler.

Since I use OF 2.1.1., I prefer to use the second approach as suggested by ARTem.

Any further advice and suggestions will be highly appreciated.

[Cyp]

Originally Posted by cfdonline2mohsen

Thanks Cyprien
But I think you are wrong!
When you assign different values to your field with setFields, It will not have the same value for all the time steps!
setFields is only designed for setting the initial conditions on your fields as stated by fabian_roesler in this post and also by Bernhard in #4 and also in #5.
If you take a look at Figure 2.21 on page U-60 of the user guide and compare it with Figure 2.22, you will see that it will change.

Thanks you so much again.

Of course it will have the same value at all the time steps!! In the tutorial you mentioned, setFields is used to initialise your field alpha1, that will be modified later with the solver interFoam.

In your case, you want to assign different value to your volScalarField called "sourceTerm". You CAN do that with setFields (and it is actually the fastest way and is kind of similar to the method suggested by ARTem). Since there is no equation that will modify "sourceTerm", it will keep the same value for all the time step.

Best,

[cfdonline2mohsen]

Originally Posted by Cyp

Of course it will have the same value at all the time steps!! In the tutorial you mentioned, setFields is used to initialise your field alpha1, that will be modified later with the solver interFoam.

In your case, you want to assign different value to your volScalarField called "sourceTerm". You CAN do that with setFields (and it is actually the fastest way and is kind of similar to the method suggested by ARTem). Since there is no equation that will modify "sourceTerm", it will keep the same value for all the time step.

Best,

Thank you Cyprien for your supplementary comments.Then I will try setFields first to see the results.
It's so nice of you.

[michall]

Hi,

The topic is quite old and probably obvious for more advanced users yet I don't see final answer. Recently I had to add a source term in the enthalpy equation in the OF 2.1.1 (so no fvOption yet).

I merge discussed solution of cfdonline2mohsen and ARTem. I added my source in createFields.H (like in ARTem post #8) and used setFields to set a constant value of my source in certain region only. It worked, but the problem was that in the next time step the value of the source was 0 again. The problem was the following line:

 
dimensionedScalar("S",yourSourceDimension,scalar(0))

which was setting the value of the source back to 0. Without this line it works ok. and the dimensions are specified in my source file in startTime directory. In summary:
1) Add "source" to your equation
2) Modify createFields.H:

volScalarField hSource
(   
    IOobject
    (   
        "hSource",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

(AUTO_WRITE is not needed but I wanted to check if it works.)
3) Compile
4) Use setFields
So this is working solution in my case.

[rob3rt 0ng]

Hi,

Is there a way to specify the actual initial value of a variable (i.e. concentration) and its diffusivity in the fvOptions?

Thanks and regards,
Robert

[fabian_roesler]

I didn't get your question entirely. Initial values are defined in the fields them selves.
In fvOptions you can define extra sources acting inside the conservation equations.

Cheers

Fabian

[sisetrun]

Hey everybody,

thank you for the discretion how to add the source to solver.

I am trying to modify the scalarTransport solver. The goal is to add the tracer directly in front of an obstacle and not at the inlet patch. I want to set the value of the tracer to 1 to obtain same info as from common scalarTransportFoam.

I managed to add a tracer source (T_source) to scalarTransportFoam and to set its value to 1 in my domain. When I run the modified scalarTransportFoam, my T_source stays constant at 1 and the tracer is spread through the volume. BUT: the values for T are very small (around 5e-3).

Do you have an idea to fix this? Is there maybe something wring with the dimensions?

Thank you for your time

Best regards