[Fluido]

Dear Foamers,

I have been using OpenFOAM for several months for a student project. Everything has been working quite well. But at the moment I am a bit stuck at a problem. Maybe someone can help…

For version 2.2.0 OpenFOAM seems to have introduced a very nice new feature of fvOptions called ‘fixedTemperatureConstraint’, to ‘to fix the temperature to a given value’ (see http://www.openfoam.org/version2.2.0/fvOptions.php). I would like to use this feature to set the temperature of air flowing through a heater to a fixed temperature instead of having to model the heater as a heat source.

My input for the fvOptions file would look like this

 fixedTemperaure1
  {
      type                      fixedTemperatureConstraint;
      active                    true;
      selectionMode         cellZone;
      cellZone                 heater;
   
      fixedTemperatureConstraintCoeffs
      {
          mode              uniform;
          temperature     350;
      }
  }

I would like to include the fixedTemperatureConstraint to a self-built solver for a decoupled, steady state, incompressible temperature equation. The solver is working already. It is just missing the handling of sources. So, here is what I did:

• add fvOptions(T) to the temperature equation
• add fvOptions.constrain(TEqn) to TEqn.H
• #include "fvIOoptionList.H" to solver .C file
• #include "createFvOptions.H" to solver .C file

The code of the TEqn file looks like this now (not showing the definition of the coefficient alphaEff):

      fvScalarMatrix TEqn
      (
          fvm::div(phi, T)
        - fvm::laplacian(alphaEff, T)
        ==
        fvOptions(T)
      );
   
      TEqn.relax();
   
      fvOptions.constrain(TEqn);
   
      TEqn.solve();

Compiling of the solver works fine. But when trying to run a case, I get the following error massage.

  --> FOAM FATAL ERROR: 
   
      request for basicThermo thermophysicalProperties from objectRegistry region0 failed
      available objects of type basicThermo are
   
  0
  (
  )

From my understanding of this error message, OpenFOAM is missing a thermophysical model. So I am wondering:


Is there a thermophysical model necessary for the implementation of the fixedTemperatureConstraint?

If not, do you have any hints where the error messages might come from?

Thank you very much for your help!
- Fluido -

[olivierG]

Hello,

My guess is you forget the "-I$(LIB_SRC)/fvOptions/lnInclude" in your Make/options file.

regards,
olivier

[andre.weiner]

Hey!

You have a simple transport equation for a scalar T, so you have to use the explicitSetValue fvOption. The fixedTemperatureConstraint is for energy equations.
Check also the post of olivier about the wmake options.

regards,
Andre

[Fluido]

Originally Posted by olivierG

Hello,

My guess is you forget the "-I$(LIB_SRC)/fvOptions/lnInclude" in your Make/options file.

regards,
olivier

Hello Olivier,

thank you for your idea!
I checked the options file once again. The fvOptions entry is there. So, that's not the problem...

Regards
- Fluido -

[Fluido]

Originally Posted by andre.weiner

Hey!

You have a simple transport equation for a scalar T, so you have to use the explicitSetValue fvOption. The fixedTemperatureConstraint is for energy equations.
Check also the post of olivier about the wmake options.

regards,
Andre

Hello Andre,

thank you for the info!

If the fixedTemperatureConstraint is made for energy equations, the call for a thermophysical model makes sense somehow. Can I find this information somewhere inside OpenFOAM (without having to dig deep into the code) or somewhere else?

I will try the explicitSetValue option now...

Regards
- Fluido -

[Fluido]

There was a little error in my original post. The error message does not appear when compiling, but when running a case with the compiled solver. So, compiling of the solver works, without any errors.

[andre.weiner]

Originally Posted by Fluido

Hello Andre,

thank you for the info!

If the fixedTemperatureConstraint is made for energy equations, the call for a thermophysical model makes sense somehow. Can I find this information somewhere inside OpenFOAM (without having to dig deep into the code) or somewhere else?

I will try the explicitSetValue option now...

Regards
- Fluido -

You don't have to dig that deep :-)

void Foam::fv::fixedTemperatureConstraint::setValue
(
    fvMatrix<scalar>& eqn,
    const label
)
{
    const basicThermo& thermo =
        mesh_.lookupObject<basicThermo>("thermophysicalProperties");

    if (eqn.psi().name() == thermo.he().name())
    {...

This is a part of the member function that sets the value. As you see it looks for some thermophysicalProperties and then it checks your equation for a part called psi and so on. So this fixedTemperatureConstraint is a little more complicated than what you need.

Regards, Andre

[Fluido]

Originally Posted by andre.weiner

You don't have to dig that deep :-)

void Foam::fv::fixedTemperatureConstraint::setValue
(
    fvMatrix<scalar>& eqn,
    const label
)
{
    const basicThermo& thermo =
        mesh_.lookupObject<basicThermo>("thermophysicalProperties");

    if (eqn.psi().name() == thermo.he().name())
    {...

This is a part of the member function that sets the value. As you see it looks for some thermophysicalProperties and then it checks your equation for a part called psi and so on. So this fixedTemperatureConstraint is a little more complicated than what you need.

Regards, Andre

Ok. I had not looked at the .C file yet (or not close enough). But it is quite obvious from code you posted that OpenFOAM would look for a thermophysical model. Thanks!

Meanwhile I tried the explicitSetValue option. I just changed the input in the fvOptions file to:

source1
{
    type            scalarExplicitSetValue;
    active          true;
    selectionMode   cellZone;
    cellZone         fluid-porous;

    scalarExplicitSetValueCoeffs
    {
        volumeMode      absolute;
        injectionRate
        {
            T              323;
        }
    }
}

And...it works perfectly! :-)

So, thank you again!

- Fluido -

[samiam1000]

Dear All,

I am trying to do something like what you did, but instead of temperatures, I wanna add in a certain cellSet a constant bodyForce.

Do you have an idea about I can do this?

Thanks a lot,
Samuele

[svramana]

Originally Posted by Fluido

Ok. I had not looked at the .C file yet (or not close enough). But it is quite obvious from code you posted that OpenFOAM would look for a thermophysical model. Thanks!

Meanwhile I tried the explicitSetValue option. I just changed the input in the fvOptions file to:

source1
{
    type            scalarExplicitSetValue;
    active          true;
    selectionMode   cellZone;
    cellZone         fluid-porous;

    scalarExplicitSetValueCoeffs
    {
        volumeMode      absolute;
        injectionRate
        {
            T              323;
        }
    }
}

And...it works perfectly! :-)

So, thank you again!

- Fluido -

Hi,i know i am digging into old thread but i am not able to set "scalarExplicitSetValue" in my fvOptions.

any help is appreciated.

Regards,
s.v.Ramana