CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

janafThermo error T=0

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 24, 2010, 07:48
Default janafThermo error T=0
  #1
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8
mabinty is on a distinguished road
Dear all!

I implemented a combustion model into chtMultiRegionFoam using the janafThermo<equationOfState> (hsPsiMixtureThermo<veryInhomogeneousMixture<suthe rlandTransport<specieThermo<janafThermo<perfectGas >>>>>). Any time when I apply the solidWallMixedTemperatureCoupled BC to couple the solid and fluid regions I get the following error:

Code:
--> FOAM FATAL ERROR: 
attempt to use janafThermo<equationOfState> out of temperature range 200 -> 6000;  T = 0

    From function janafThermo<equationOfState>::checkT(const scalar T) const
    in file /home/aa/OpenFOAM/OpenFOAM-1.6.x/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 64.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  Foam::hsPsiMixtureThermo<Foam::veryInhomogeneousMixture<Foam::sutherlandTransport<Foam::specieThermo<Foam::janafThermo<Foam::perfectGas> > > > >::hs(Foam::Field<double> const&, int) const in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libreactionSensibleEnthalpyThermophysicalModels.so"
#3  Foam::mixedEnthalpyFvPatchScalarField::updateCoeffs() in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#4  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::dimensionSet const&) in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcombustionModels.so"
#5  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::Sp<double>(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcombustionModels.so"
#6  Foam::radiation::radiationModel::Shs(Foam::basicThermo&) const in "/home/aa/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libradiation.so"
#7  main in "/home/aa/OpenFOAM/aa-1.6.x/applications/bin/linux64GccDPOpt/chtMultiRegionFireFoam"
#8  __libc_start_main in "/lib/libc.so.6"
#9  _start at /build/buildd/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116
Following behavior is observed:
(1) The error disappears when any other BC than solidWallMixedTemperatureCoupled is applied at the solid-fluid interface.
(2) I checked the values of the solid-fluid interface and internal temperatures and all of them are greater than zero.
(3) The error happens at the first time the code enters the sensible enthalpy (hs) equation.
(4) The problem appears no matter the combustion model is en- or disabled.

Does anybody have made similar experience or have any idea what the problem could be? I greatly appreciat your comments!

Best regards,
Aram
mabinty is offline   Reply With Quote

Old   May 24, 2010, 07:57
Default
  #2
Member
 
MSR CHANDRA MURTHY
Join Date: Mar 2009
Posts: 32
Rep Power: 8
chandramurthy is on a distinguished road
it looks like the error relates to lower bound of JANAF table. try with manually changing the lower bound from 200 K to much lower value of about 50 K. initialize the T field above this value. probably this may fix it.
chandramurthy is offline   Reply With Quote

Old   May 25, 2010, 08:04
Default
  #3
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8
mabinty is on a distinguished road
hi chandra,

thanks for your comment! I tried to set the the lower temperature to e.g. 50K but the problem persists. From somewhere the checkT-function gets a T-value equal to zero, but only when the mentioned BC is used; I couldn t figure out yet where or how T=0K occurs but I ll keep on digging.

regards,
aram
mabinty is offline   Reply With Quote

Old   May 25, 2010, 10:37
Default
  #4
Member
 
Cedric Van Holsbeke
Join Date: Dec 2009
Location: Belgium
Posts: 81
Rep Power: 7
CedricVH is on a distinguished road
Have you already tried the new Janaf model?
CedricVH is offline   Reply With Quote

Old   May 25, 2010, 14:16
Default
  #5
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8
mabinty is on a distinguished road
hi!

i played arround with the initial temperatures of the fluid and solid regions and observed the following:

the "solidWallMixedTemperatureCoupled" BC is of type "mixedFvPatchScalarField", switching between "fixedValue" (if heat flux is outgoing) and "fixedGradient" (when flux is incoming) for the T. I figured out that the above mentioned error message from JANAF happens at the moment one of the fluid patches on the solid-fluid intreface is set to "fixedGradient" (no error if all patches ar set to "fixedValue"!). hence, I thought the problem depends on the sign of the heat flux or the T-gradient at the interface (as it governs the switching of the mixed BC) and used a "fixedGradient" BC with different signs of "gradient" for T on the fluid side. no error message was outputed, neither for a positive nor a negative T-gradient. therefore the problem is with the mixed BC in combination with JANAF. I ll keep on digging and report.

@cedric: thanks a lot for the hint! I ll have a look at the new JANAF model.

regards,
aram
mabinty is offline   Reply With Quote

Old   May 26, 2010, 10:36
Default
  #6
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8
mabinty is on a distinguished road
hi all!

finally i found the problem. when using the solidWallMixedTemperatureCoupled BC a mixedEnthalpyFvPatchScalarField is used to calculate the BC for hs when entering the hs-equation. there a refValue() for hs is determined as follows (see mixedEnthalpyFvPatchScalarField.C):

refValue() = thermo.hs(Tw.refValue(), patchi);

Tw is the temeperature field evaluated by the solidWallMixedTemperatureCoupled BC, where the Tw.refValue() is calculated as (see solidWallMixedTemperatureCoupledFvPatchScalarField .C):

Code:
// if outgoing flux use fixed value, else fixed gradient.
        if (normalGradient()[i] < 0.0)
        {
            this->refValue()[i] = operator[](i);
            this->refGrad()[i] = 0.0;   // not used
            this->valueFraction()[i] = 1.0;
            nFixed++;
        }
        else    
        {
            this->refValue()[i] = 0.0;      // not used;
            this->refGrad()[i] = normalGradient()[i];
            this->valueFraction()[i] = 0.0;
        }
in case the BC uses fixedValue, no problem; for fixedGradient the refValue() is set to 0.0 (not relevant as valueFraction() = 0.0), what is used to evaluate thermo.hs(Tw.refValue(), patchi), hence the error T=0 is sent. as the refValue() for the case of valueFraction() = 0.0 isn t used I set refValue()[i] = 200.0 and the problem doesn t appear anymore

best regards,
aram

ps: should this be reported as a bug????
mabinty is offline   Reply With Quote

Old   May 27, 2010, 02:30
Default
  #7
Member
 
MSR CHANDRA MURTHY
Join Date: Mar 2009
Posts: 32
Rep Power: 8
chandramurthy is on a distinguished road
very nice troubleshooting!!!
chandramurthy 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
janafThermo: How to read formula? or at least: How to use hPolynomialThermo? bgoeppner OpenFOAM 0 February 22, 2010 16:17
Inconsistent declaration of hConstThermo vs janafThermo dominik_christ OpenFOAM Bugs 6 October 31, 2008 05:15
XiFoam janafthermo error AT tavasoly OpenFOAM Running, Solving & CFD 1 July 1, 2008 11:15


All times are GMT -4. The time now is 17:10.