CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

request for turbulenceModel from objectRegistry failed

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

Like Tree2Likes
  • 2 Post By M3hdi

Reply
 
LinkBack Thread Tools Display Modes
Old   September 5, 2012, 08:18
Default request for turbulenceModel from objectRegistry failed
  #1
New Member
 
klemen
Join Date: Aug 2012
Location: Slovenia
Posts: 21
Rep Power: 4
fogl is on a distinguished road
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:rintStack(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:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/chtMultiRegionSimpleFoam"
#3 Foam::compressible::turbulenceModel const& Foam:bjectRegistry::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:imensionedField<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;

}

}

// ************************************************** *********************** //
fogl is offline   Reply With Quote

Old   September 5, 2012, 12:28
Default
  #2
New Member
 
Join Date: Aug 2011
Location: Paris
Posts: 20
Rep Power: 5
M3hdi is on a distinguished road
Dear Fogl,

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

Thanks in advance

Mahdi
M3hdi is offline   Reply With Quote

Old   September 5, 2012, 16:56
Default
  #3
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,520
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
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: How to give enough info to get help

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   September 6, 2012, 03:28
Default
  #4
New Member
 
klemen
Join Date: Aug 2012
Location: Slovenia
Posts: 21
Rep Power: 4
fogl is on a distinguished road
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
fogl is offline   Reply With Quote

Old   September 7, 2012, 04:43
Default
  #5
New Member
 
Join Date: Aug 2011
Location: Paris
Posts: 20
Rep Power: 5
M3hdi is on a distinguished road
Has anybody figured out the bug please ?

Mehdi
M3hdi is offline   Reply With Quote

Old   September 9, 2012, 13:55
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,520
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
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
wyldckat is offline   Reply With Quote

Old   September 10, 2012, 08:43
Default
  #7
New Member
 
klemen
Join Date: Aug 2012
Location: Slovenia
Posts: 21
Rep Power: 4
fogl is on a distinguished road
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
fogl is offline   Reply With Quote

Old   September 10, 2012, 18:28
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,520
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
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
wyldckat is offline   Reply With Quote

Old   September 11, 2012, 05:45
Default
  #9
New Member
 
Join Date: Aug 2011
Location: Paris
Posts: 20
Rep Power: 5
M3hdi is on a distinguished road
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
wyldckat and Ahmed Khattab like this.
M3hdi is offline   Reply With Quote

Old   October 3, 2012, 14:32
Default
  #10
New Member
 
Join Date: Jul 2012
Posts: 21
Rep Power: 4
turbulencious is on a distinguished road
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
turbulencious 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
Saving ParaFoam views and case sail OpenFOAM Paraview & paraFoam 9 November 25, 2011 16:46
DeardorffDiffStress turbulence model Zuixy OpenFOAM Running, Solving & CFD 0 November 14, 2011 09:44
ParaView/Parafoam error when making animation Disco_Caine OpenFOAM Paraview & paraFoam 6 September 28, 2010 10:54
user subroutine error CFDUSER CFX 2 December 9, 2006 07:31
user defined function cfduser CFX 0 April 29, 2006 11:58


All times are GMT -4. The time now is 00:01.