CFD Online Discussion Forums - Building a solver with fixedTemperatureConstraint using fvOptions

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)

- - Building a solver with fixedTemperatureConstraint using fvOptions (https://www.cfd-online.com/Forums/openfoam-programming-development/121464-building-solver-fixedtemperatureconstraint-using-fvoptions.html)

Building a solver with fixedTemperatureConstraint using fvOptions

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

Code:

 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):

Code:

      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.

Code:

  --> 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 -

Hello,

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

regards,
olivier

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

Quote:

Originally Posted by olivierG (Post 442806)

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 -

Quote:

Originally Posted by andre.weiner (Post 442927)

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 -

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.

Quote:

Originally Posted by Fluido (Post 443220)

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

Code:

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

Quote:

Originally Posted by andre.weiner (Post 443236)

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

Code:

void Foam::fv::fixedTemperatureConstraint::setValue

(

    fvMatrix<scalar>& eqn,

    const label

)

{

    const basicThermo& thermo =

        mesh_.lookupObject<basicThermo>("thermophysicalProperties");



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

    {...

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:

Code:

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 -

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

Quote:

Originally Posted by Fluido (Post 443317)

Code:

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