CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   request for turbulenceModel from objectRegistry failed (http://www.cfd-online.com/Forums/openfoam-solving/106680-request-turbulencemodel-objectregistry-failed.html)

fogl September 5, 2012 08:18

request for turbulenceModel from objectRegistry failed
 
I would like to stest the simple cht problem of nitrogen flow in cylindrical tube.

When i run the simulation, i get the following error (below). Any idea what could be wrong?

Regards,
Klemen

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.1-221db2718bbb
Exec : chtMultiRegionSimpleFoam
Date : Sep 04 2012
Time : 20:12:23
Host : "kd"
PID : 3723
Case : /home/klemen/OpenFOAM/klemen-2.1.1/run/tutorials/incompressible/icoFoam/dewarCHT2
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create fluid mesh for region nitrogen for time = 0
Create solid mesh for region tube for time = 0
*** Reading fluid mesh thermophysical properties for region nitrogen
Adding to thermoFluid
Selecting thermodynamics package hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
Adding to rhoFluid
Adding to kappaFluid
Adding to UFluid
Adding to phiFluid
Adding to gFluid
Adding to turbulence
Selecting turbulence model type laminar
Adding to ghFluid
Adding to ghfFluid
Selecting radiationModel none
*** Reading solid mesh thermophysical properties for region tube
Adding to thermos
Constructed constSolidThermo with
rho : rho [1 -3 0 0 0 0 0] 7980
Cp : Cp [0 2 -2 -1 0 0 0] 500
K : K [1 1 -3 -1 0 0 0] 15
Hf : Hf [0 2 -2 0 0 0 0] 0
emissivity : emissivity [0 0 0 0 0 0 0] 0
kappa : kappa [0 -1 0 0 0 0 0] 0
sigmaS : sigmaS [0 -1 0 0 0 0 0] 0
Time = 0.01

Solving for fluid region nitrogen
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0022809712, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0047684596, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.030397671, No Iterations 1

--> FOAM FATAL ERROR:
request for turbulenceModel turbulenceModel from objectRegistry tube failed
available objects of type turbulenceModel are
0
(
)

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 131.
FOAM aborting
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2 Foam::Ostream& Foam::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/chtMultiRegionSimpleFoam"
#3 Foam::compressible::turbulenceModel const& Foam::objectRegistry::lookupObject<Foam::compressi ble::turbulenceModel>(Foam::word const&) const in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libcompressibleTurbulenceModel.so"
#4 Foam::temperatureCoupledBase::K(Foam::Field<double > const&) const in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libcompressibleTurbulenceModel.so"
#5 Foam::compressible::turbulentTemperatureCoupledBaf fleMixedFvPatchScalarField::updateCoeffs() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libcompressibleTurbulenceModel.so"
#6 Foam::mixedFvPatchField<double>::evaluate(Foam::UP stream::commsTypes) in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#7 Foam::mixedEnthalpyFvPatchScalarField::updateCoeff s() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libbasicThermophysicalModels.so"
#8 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricFi eld<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/chtMultiRegionSimpleFoam"
#9 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::Sp<double>(Foam::DimensionedField<doubl e, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/chtMultiRegionSimpleFoam"
#10 Foam::radiation::radiationModel::Sh(Foam::basicThe rmo&) const in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libradiationModels.so"
#11
in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/chtMultiRegionSimpleFoam"
#12 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#13
in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/chtMultiRegionSimpleFoam"
Aborted


XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX
nitrogen T IC and BC:


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.x |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class volScalarField;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 100;
boundaryField
{
gasInlet
{
type fixedValue;
value uniform 100;
}
gasOutlet
{
type zeroGradient;
value uniform 0;
}
gasSideX
{
type cyclic;
}
gasSideY
{
type cyclic;
}
nitrogen_to_tube
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 300;
neighbourFieldName T;
K basicThermo;
KName none;

}
}

// ************************************************** *********************** //


XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX
tubeT IC and BC:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.x |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class volScalarField;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 300;
boundaryField
{
tubeInlet
{
type fixedValue;
value uniform 100;
}
tubeOutlet
{
type fixedValue;
value uniform 300;
}
tubeBack
{
type zeroGradient;
value uniform 0;
}
tubeSideX
{
type cyclic;
}
tubeSideY
{
type cyclic;
}
tube_to_nitrogen
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 300;
neighbourFieldName T;
K basicThermo;
KName none;

}

}

// ************************************************** *********************** //

M3hdi September 5, 2012 12:28

Dear Fogl,

I have exactly the same error in a CHT case (OF-210). Did you solve this problem ?

Thanks in advance

Mahdi

wyldckat September 5, 2012 16:56

Greetings to all!

It would be easier to help you, if you could prepare one of the tutorial cases using the settings you want, so we could test this ourselves and help you guys figure out the solution.

For more: http://www.cfd-online.com/Forums/ope...-get-help.html

Best regards,
Bruno

fogl September 6, 2012 03:28

I agree with you Bruno... you can download my case at http://www.smallfiles.org/download/2...T2.tar.gz.html

I modeled a simple tube with nitrogen gas flow inside the tube. I set a fixed temperature BC (to generate the temperatre field) and defined the nitrogen flow velovity at one end.

Regards,
Klemen

M3hdi September 7, 2012 04:43

Has anybody figured out the bug please ?

Mehdi

wyldckat September 9, 2012 13:55

Greetings to all!

I've tested Klemen's case and the same error occurred with me.

But then I tried using the nitrogen thermodynamic parameters in the tutorial "heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater" and it ran with no problems!

I suspected the cyclic boundaries were messing everything up, but after setting them all to wall and fixed values, it still crashed.

I don't more time to do more tests, so I suggest that you guys do the steps over once again, but this time test each individual change, one at a time. For example, follow these steps for gradual changes:
  1. Change the tutorial I mentioned to use nitrogen instead of air. Test it.
  2. Change the tutorial's mesh, in a way that you have a simpler geometry. For example, a simple hot plate and a fluid zone on the top or bottom side. Test it.
  3. Apply cyclics to the previous mesh. Test it.
  4. Finally, wrap the mesh to turn it into a quarter tube as you had.
Good luck!
Bruno

fogl September 10, 2012 08:43

Thank you for your time, Bruno. I will try to test this case like you suggested, and change the configuration step by step.

Is this the only way to fond the cause of error? Is there an option in OpenFoam to somehow run the case in "debug mode"?

Regards,
Klemen

wyldckat September 10, 2012 18:28

Hi Klemen,

It depends on the type of debug mode you're looking for. OpenFOAM has two types:
  1. You can see some additional messages by using the values changeable in OpenFOAM's main "etc/controlDict" file, by changing values from 0 to 1.
  2. You can do a full or partial build in debug mode, as explained here: http://openfoamwiki.net/index.php/Ma...at_is_wrong.3F
Best regards,
Bruno

M3hdi September 11, 2012 05:45

Good morning Foamers,

It runs for my CHT case :) the problem was in the definition of the boundary condition in a solid region :

heater
{
type externalWallHeatFluxTemperature;
K basicThermo;
KName none;
heatSource power;
value uniform 293.15;
q uniform 10.;
}

... changed to

heater
{
type externalWallHeatFluxTemperature;
K solidThermo;
KName none;
heatSource power;
value uniform 293.15;
q uniform 10.;
}

Now the CHT is running !

I hope this helps.

Mehdi

turbulencious October 3, 2012 14:32

hello people,

I am more or less on the same page with you (of 2.1 , chtMultiRegionFoam) and I would like to understand how the convection heat transfer coefficient is calculated. I use as thermophysical properties thermoType hRhoThermo<pureMixture<icoPoly8ThermoPhysics>>; where I input k, cp and μ so I assume that the Prandtl number is calculated through them, and then the Nusselt number and then h (or alpha). What I am unable to find, is where and how exactly are these calculations? namely, in which file?

thank you very much for your consideration


All times are GMT -4. The time now is 09:01.