[evrikon]

Hi forum,

in OpenFoam 1.6.x the boundary condition which represents a constant heat flux through the boundary does not work for incompressible cases like buoyantBoussinesqSimpleFoam. To see the bug please have a look into

/src/turbulenceModels/incompressible/turbulentHeatFluxTemperatureFvPatchScalarField.C
:line 160

You can see:
const scalarField& Cpp =
patch().lookupPatchField<volScalarField, scalar>(CpName_);

This is not correct because an incompressible solver does not have any information about Cp.
-----------------------------------------
Here is my bugfix:

void turbulentHeatFluxTemperatureFvPatchScalarField::up dateCoeffs()
{
if (updated())
{
return;
}

const RASModel& rasModel = db().lookupObject<RASModel>("RASProperties");

const scalarField alphaEffp =
patch().lookupPatchField<volScalarField, scalar>(alphaEffName_);

// const scalarField& Cpp =
// patch().lookupPatchField<volScalarField, scalar>(CpName_);

transportModel& laminarTransport = rasModel.transport();
dimensionedScalar Cp(laminarTransport.lookup("Cp"));

gradient() = q_/(Cp.value()*alphaEffp);

fixedGradientFvPatchScalarField::updateCoeffs();
}
-------------------------------------------------------------------------------------------------
Further I specified Cp by adding one line into readTransportProperties.H for solver buoyantBoussinesqSimpleFoam:

//Bug fix OLK: Cp is needed for fixedHeatFlux boundary condition
// Heat capacity
dimensionedScalar Cp(laminarTransport.lookup("Cp"));
-------------------------------------------------------------------------------------------------
For other incompressible solvers with heat transfer it should be done too.

Now I can use the new boundary condition turbulentHeatFluxTemperature for both compressible and incompressible cases.

Cheers, Oleksiy

[rob3rt]

Hello Evrikon,

I had this error while trying to compile your bugfix.

derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.C:1 59: error: ‘transportModel’ was not declared in this scope
derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.C:1 59: error: ‘laminarTransport’ was not declared in this scope
derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.C:1 59: error: ‘rasModel’ was not declared in this scope
derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.C:1 62: error: ‘Cpp’ was not declared in this scope

What should I declare to make this working?

And

another question is: what is difference between turbulentHeatFluxTemperature (without rho) and wallHeatFlux (http://openfoamwiki.net/index.php/Contrib_wallHeatFlux)?
I think both can be used for incompressible cases, right?

Thanks very much for your time.

Kind Regards,
Robert.

[evrikon]

Dear Robert,

I implemented this bug fix directly in OpenFoam 1.6.x. I changed the boundary condition in turbulentHeatFluxFvPatchField.C as described above and recompiled the whole turbulenceModels staff. It takes only a few minutes. If you try to do that, please do a backup of turbulenceModels directory before!

I assume you simply miss the corresponding libraries. Do you try to define this boundary condition as your own library? Then you do need to look into your Make/files and Make/Options.

[cgoniva]

Dear Oleksiy,

Shouldn't you add rho to the equation:
"gradient() = q_/(Cp.value()*alphaEffp*rho0); "
as this is done here (http://openfoamwiki.net/index.php/Contrib_wallHeatFlux) ???

This rho should be read from dictionary as you did for Cp:
"dimensionedScalar rho0(laminarTransport.lookup("rho0")); "

Cheers,
Chris

[cgoniva]

oh... some mistake, it should be:

"gradient() = q_/(Cp.value()*alphaEffp*rho0.value()); "

Cheers, Chris

[evrikon]

No, I only speak about the incompressible case where no rho is present in OpenFoam. Therefore the gradient is not divided by rho. For compressible cases it should be divided.