CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   groovyBC for perfectGas modell (http://www.cfd-online.com/Forums/openfoam-pre-processing/113695-groovybc-perfectgas-modell.html)

aronman February 25, 2013 08:50

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

gschaider February 25, 2013 17:23

Quote:

Originally Posted by aronman (Post 409919)
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?

aronman February 26, 2013 04:54

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:

gschaider February 26, 2013 06:17

Quote:

Originally Posted by aronman (Post 410118)
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)

aronman February 26, 2013 09:27

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


All times are GMT -4. The time now is 09:11.