CFD Online Discussion Forums - Request for dictionary failed with buoyantSimpleFoam

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

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Request for dictionary failed with buoyantSimpleFoam (https://www.cfd-online.com/Forums/openfoam-solving/191956-request-dictionary-failed-buoyantsimplefoam.html)

Request for dictionary failed with buoyantSimpleFoam

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:

Code:

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  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 :confused:

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

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:

Code:

--> 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 :confused:

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:

Code:

--> 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.

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

Quote:

Originally Posted by AbdulazizAlkandari (Post 731624)

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>>>>>;

Quote:

Originally Posted by AbdulazizAlkandari (Post 731624)

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).