[Jabo]

Hi,

I need the wallHeatTransfer condition in my spray simulation as the experiment had a chamber with heated walls.

Immediately upon implementing wallHeatTransfer in 0/T and running sprayFoam the simulation crashes, immediately after "Selecting thermodynamics package"

So I tried the aachenBomb tutorial case and that crashes in the same way.

Here's the log:

--> FOAM FATAL ERROR: 

    request for turbulenceModel turbulenceModel from objectRegistry region0 failed
    available objects of type turbulenceModel are
0()

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/james/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::compressible::turbulenceModel const& Foam::objectRegistry::lookupObject<Foam::compressible::turbulenceModel>(Foam::word const&) const at ??:?
#3  Foam::wallHeatTransferFvPatchScalarField::updateCoeffs() at ??:?
#4  Foam::mixedFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) at ??:?
#5  Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#6  Foam::fvPatchField<double>::adddictionaryConstructorToTable<Foam::wallHeatTransferFvPatchScalarField>::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#7  Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#8  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::readField(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#9  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields(Foam::dictionary const&) at ??:?
#10  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields() at ??:?
#11  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) at ??:?
#12  Foam::basicThermo::basicThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#13  Foam::fluidThermo::fluidThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#14  Foam::psiThermo::psiThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#15  Foam::psiReactionThermo::psiReactionThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#16  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#17  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&) at ??:?
#18  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReactionThermo>(Foam::fvMesh const&, Foam::word const&) at ??:?
#19  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) at ??:?
#20  Foam::psiChemistryModel::psiChemistryModel(Foam::fvMesh const&) at ??:?
#21  Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::chemistryModel(Foam::fvMesh const&) at ??:?
#22  Foam::ode<Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::ode(Foam::fvMesh const&) at ??:?
#23  Foam::psiChemistryModel::addfvMeshConstructorToTable<Foam::ode<Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&) at ??:?
#24  Foam::autoPtr<Foam::psiChemistryModel> Foam::basicChemistryModel::New<Foam::psiChemistryModel>(Foam::fvMesh const&) at ??:?
#25  Foam::psiChemistryModel::New(Foam::fvMesh const&) at ??:?
#26  Foam::combustionModels::psiChemistryCombustion::psiChemistryCombustion(Foam::word const&, Foam::fvMesh const&) at ??:?
#27  Foam::combustionModels::laminar<Foam::combustionModels::psiChemistryCombustion>::laminar(Foam::word const&, Foam::fvMesh const&) at ??:?
#28  Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion>::PaSR(Foam::word const&, Foam::fvMesh const&) at ??:?
#29  Foam::combustionModels::psiCombustionModel::adddictionaryConstructorToTable<Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion> >::New(Foam::word const&, Foam::fvMesh const&) at ??:?
#30  Foam::combustionModels::psiCombustionModel::New(Foam::fvMesh const&) at ??:?
#31  
 at ??:?
#32  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#33  
 at ??:?
Aborted (core dumped)

What's the issue here? and how do I fix it?

[Jabo]

It doesn't just crash the sprayFoam tutorial. It crashes every lagrangian tutorial.

[Jabo]

and engineFoam.

[alexeym]

Hi,

not quite sure the BC is intended to use as boundary condition for temperature.

In sparyFoam for example thermophysical model is created at line 5 of createFields.H, as a result temperature field is created, temperature boundary conditions are updated. But turbulence model is created only on line 60 of the same file.

So wallHeatFlux BC is trying to fetch turbulence model from IOobject DB:

    const compressible::turbulenceModel& turbModel =
        db().lookupObject<compressible::turbulenceModel>
        (
            "turbulenceModel"
        );

when turbulence model is not created yet.

Also if you take a look at wallHeatTransferFvPatchScalarField.H:

Description
    This boundary condition provides an enthalpy condition for wall heat
    transfer

I'm not quite sure the BC was intended for use at all, I wasn't able to find usage of Tinf in the code.

[Jabo]

Agreed. I've just stumbled across externalWallHeatFluxTemperature which I think is what I need.