[sturgeon]

Hi all

I am experiencing an error that I can't locate the source of. I copied the CircuitBoardCooling case for buoyantSimpleFoam and modified the geometry and boundary conditions and am getting this error:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1612+                                |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : v1612+
Exec   : buoyantSimpleFoam
Date   : Aug 25 2017
Time   : 09:17:20
Host   : "default"
PID    : 1132
Case   : /home/ofuser/workingDir/thermalMountain3
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p_rgh  tolerance 0.001
    field U      tolerance 0.0001
    field h      tolerance 0.0001
    field "(k|epsilon|omega)"    tolerance 0.005

Reading thermophysical properties

Selecting thermodynamics package
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

--> FOAM Warning :
    From function groovyBCFvPatchField<Type>::groovyBCFvPatchField(const fvPatch& p,const DimensionedField<Type, volMesh>& iF,const dictionary& dict)
    in file groovyBCFvPatchField.C at line 131
    No value defined for T on inlet therefore using the internal field next to the patch
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
}


Reading g

Reading hRef
Calculating field g.h

Reading field p_rgh

No MRF models present

Radiation model not active: radiationProperties not found
Selecting radiationModel none
No finite volume options present



--> FOAM FATAL ERROR:

    request for dictionary transportProperties from objectRegistry region0 failed
    available objects of type dictionary are

8
(
MRFProperties
radiationProperties
turbulenceProperties
fvSchemes
fvOptions
fvSolution
thermophysicalProperties
data
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::IOdictionary]
    in file /home/buzz2/pawan/OpenFOAM/OpenFOAM-v1612+/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 219.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so"
#2  Foam::IOdictionary const& Foam::objectRegistry::lookupObject<Foam::IOdictionary>(Foam::word const&, bool) const in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#3  Foam::incompressible::alphatJayatillekeWallFunctionFvPatchScalarField::updateCoeffs() in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib/libincompressibleTurbulenceModels.so"
#4  Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/bin/buoyantSimpleFoam"
#5  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::evaluate() in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/bin/buoyantSimpleFoam"
#6  Foam::EddyDiffusivity<Foam::ThermalDiffusivity<Foam::CompressibleTurbulenceModel<Foam::fluidThermo> > >::correctNut() in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTurbulenceModels.so"
#7  Foam::RASModels::kEpsilon<Foam::EddyDiffusivity<Foam::ThermalDiffusivity<Foam::CompressibleTurbulenceModel<Foam::fluidThermo> > > >::correctNut() in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTurbulenceModels.so"
#8  ? in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/bin/buoyantSimpleFoam"
#9  __libc_start_main in "/lib64/libc.so.6"
#10  ? in "/opt/OpenFOAM/OpenFOAM-v1612+/platforms/linux64GccDPInt32Opt/bin/buoyantSimpleFoam"
Aborted

I searched and couldn't find an exact match for this issue but it seems like something is missing from the transport section in thermophysicalProperties. But I copied that file directly from the circuitBoardCooling case, which executes fine for me

If I deliberately mess up the transport section by deleting Pr and Mu, the error instead complains that these values aren't defined. So I am even more confused, since that suggests that everything that should be defined is defined.

If anyone could help me locate my issue, it would be much appreciated

Cheers
sturgeon

[sturgeon]

I apologise for bumping this but I am still unable to resolve this issue and was hoping someone could offer some advice.

Cheers
sturgeon

EDIT:

Further trying to diagnose my issue... if I rename the entry in thermophysicalProperties from "mixture" to a nonsense word I get the error:

--> FOAM FATAL IO ERROR:
keyword mixture is undefined in dictionary "/home/ofuser/workingDir/thermalMountain3/constant/thermophysicalProperties"

file: /home/ofuser/workingDir/thermalMountain3/constant/thermophysicalProperties from line 20 to line 44.

    From function const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&) const
    in file db/dictionary/dictionary.C at line 699.

FOAM exiting

So clearly it is looking for something specifically called "mixture". So I thought perhaps I need to define the domain as being made up of this fluid, but I've searched every file in the CircuitBoardCooling case for a reference for "mixture" and I can't find anything

EDIT 2:

So I managed to get past the previous error, I believe it's because my alphat boundaries were incorrectly set. Now, however, I am getting this error:

--> FOAM FATAL ERROR:

    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]

    From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
    in file /home/buzz2/pawan/OpenFOAM/OpenFOAM-v1612+/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.

FOAM aborting

I am really not sure what to make of this. I have searched online and the common advice seems to be to check the dimensions are set correctly, but I have checked every file in 0/ and they match the dimensions of the circuit board case I based this on, including pressure which is using the correct units for compressible flow...

Any guidance would be appreciated, I have been searching the internet and comparing case files but can't seem to find any reason for this, particularly since this is 99% a modified version of the circuitboard case which executes perfectly.

EDIT 3:

Okay, I believe this was due to phi needing to haves dimensions changed between incompressible and compressible cases. Hopefully this helps anyone who finds this thread with a similar problem.

[AbdulazizAlkandari]

I am getting your same first error but for buoyantPimpleFoam, how exactly did you manage to fix it?

[artymk4]

Originally Posted by AbdulazizAlkandari

I am getting your same first error but for buoyantPimpleFoam, how exactly did you manage to fix it?

Which error?
I had error "keyword mixture is undefined in dictionary ..." and the only problem was that I was missing ";" at the end of line
thermoType hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>;

[Alexee]

Originally Posted by AbdulazizAlkandari

I am getting your same first error but for buoyantPimpleFoam, how exactly did you manage to fix it?

The "object registry" error can arise from improper boundary condition for alphat. I also had it, but it disappeared when I changed them to match the tutorial (calculated on inlet and outlet, alphatWallFunction on the walls).