[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