CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

groovyBC for perfectGas modell

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 25, 2013, 08:50
Default groovyBC for perfectGas modell
  #1
New Member
 
Join Date: Feb 2013
Posts: 3
Rep Power: 4
aronman is on a distinguished road
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
aronman is offline   Reply With Quote

Old   February 25, 2013, 17:23
Default
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by aronman View Post
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?
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 26, 2013, 04:54
Default re
  #3
New Member
 
Join Date: Feb 2013
Posts: 3
Rep Power: 4
aronman is on a distinguished road
Yes, the solver stops and gives the following error message:

#0 Foam::error:rintStack(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:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::calculate() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam:ureMixture<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:ureMixture<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.
aronman is offline   Reply With Quote

Old   February 26, 2013, 06:17
Default
  #4
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by aronman View Post
Yes, the solver stops and gives the following error message:

#0 Foam::error:rintStack(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:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::hConstThermo<Foam:: perfectGas> > > > >::calculate() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam:ureMixture<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:ureMixture<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.
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)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 26, 2013, 09:27
Default
  #5
New Member
 
Join Date: Feb 2013
Posts: 3
Rep Power: 4
aronman is on a distinguished road
Thank you very much for your answer. It solved the problem.
aronman is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
groovyBC issue - k and epsilon sagnikmazumdar OpenFOAM Running, Solving & CFD 24 March 1, 2015 08:16
groovyBC and funkySetFields married and got a kid named swak4Foam gschaider OpenFOAM 164 January 13, 2015 03:52
Boundary Conditions with GroovyBC, Normal Gradient treima OpenFOAM Programming & Development 2 January 26, 2013 03:37
groovyBC and Eqn.setReference() benk OpenFOAM 3 June 2, 2011 08:49
Wall heat transfer using groovyBC (XiFoam solver) usergk OpenFOAM 7 February 4, 2011 14:36


All times are GMT -4. The time now is 18:11.