groovyBC for perfectGas modell
 

Hello everybody!


Excuse me if the question is inappropriate or put up in the wrong forum but I am a beginner OpenFOAM user. I encountered the following problem:


I wanted to test groovyBC in the heatTransfer/buoyantSimpleFoam/buoyantCavity tutorial that I put it in 0/T:

hot
{
type groovyBC;
valueExpression "307.75";
// variables "whT3a_fin{patch'Holeaii/fin}=sum(K*snGrad(T)*area()) TT3a{patch'Holeaii/fin}=max(T);whT3a_flowfield{patch'Holeaii/flowfield}=sum(2*snGrad(T)*area());N=5000;W=1800;" ;
value uniform 307.75;
}


The solver stops at reading in the thermophysicalProperties. I've checked it previously that the perfectGas causes it

thermoType hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;

My question is how to eliminate this problem? Some kind of 'libs' in the controlDict?
[These didn't solve it:

libs ( "libOpenFOAM.so" "libsimpleSwakFunctionObjects.so" "libswakFunctionObjects.so" "libcompressibleRASModels.so" "libgroovyBC.so" "libthermophysicalFunctions.so" "libbasicThermophysicalModels.so" "libincompressibleTransportModels.so" "libthermophysicalFunctions.so" );

]

Thanks in advance,

aronman

With "the solver stops" you mean what? Is there an error message?

The same case works if you replace the type in the boundary condition with fixedValue?

re
 

Yes, the solver stops and gives the following error message:

#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::calculate() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::hPsiThermo(Foam::fvMesh const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#5 Foam::basicPsiThermo::addfvMeshConstructorToTable< Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > > >::New(Foam::fvMesh const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#6 Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#7
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/buoyantSimpleFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/buoyantSimpleFoam"
Floating point exception (core dumped)

The original BC was fixed value in this tutorial (heatTransfer/buoyantSimpleFoam/buoyantCavity) and it ran. Then I replaced the BC only at the 'hot' boundary for testing groovyBC. I suspect (checked it) that the perfectGas thermophysical modell doesn't like groovy, but I don't know why. :cool:

I guess this is a problem with the current release that is already fixed in the dev-version. Problem is that during the initialization the BC evaluates to 0 and T=0 is not good in the perfect gas equation.

To verify that this is the problem: set "type fixedValue; value uniform 0;". Should give the same stack-trace.

As a workaround add "refValue $value;" (of course after you reset value from 0 to the proper value)

Thank you very much for your answer. It solved the problem.