CFD Online Discussion Forums - Error in thermophysical properties (chtMultiRegionFoam)

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)

- - Error in thermophysical properties (chtMultiRegionFoam) (https://www.cfd-online.com/Forums/openfoam-pre-processing/124938-error-thermophysical-properties-chtmultiregionfoam.html)

Hi Wyldckat,

I am having the same issues as fkika. I have a smaller model with convection and heat transfer working correctly with the same thermophysical properties.

I was using 2.4 but I just upgraded to 3.0 using the standard instructions on the Openfoam website. Both versions received the same error.

FOAM FATAL ERROR:
Kappa defined to employ fluidThermo method, but thermo package not available

From function temperatureCoupledBase::kappa(const scalarField&) const
in file turbulentFluidThermoModels/derivedFvPatchFields/temperatureCoupledBase/temperatureCoupledBase.C at line 138.

I tried understanding the source code, however it is fairly difficult to understand what each variable is.

Thanks!

Hi Atkinson!

You provided more information than the previous fellow, however, you only provided the answer to one out of four questions Bruno did...

Quote:

Originally Posted by wyldckat (Post 571142)

Quick questions @fkika: Please provide more details, such as:

Which OpenFOAM version are you using?
Which installation instructions did you follow for installing OpenFOAM?

Can you reproduce this error with one of OpenFOAM's tutorials?

How is the content of the files "thermophysicalProperties" in your case? If you don't know where they are, run:

Code:

find . -name thermophysicalProperties

Quote:

Originally Posted by satkinson (Post 573736)

Well, first of all, I never saw this message before. I don't know if it is a new, or modified, message included from version 2.4 on (the last version I worked with is 2.3.x), or if I am too good! :D

Having said that, according to what the error message says, I would point out the following possible information you likely missed:

You defined kappa to be computed as fluidThermo in a solid region. Check regionProperties file.
You defined, as Bruno suggested, something wrong in thermophysicalProperties file.

Maybe if you check this information you can figure out what is going wrong.

Hope it helps.

Best regards,

Alex

Hi Alex,

Thanks for your quick reply. I have attached a txt file onto the forum with my thermophysicalpropperties but it doesn't seem to show up on windows systems. Here is the code;

Code:

thermoType 

{ 

    type            heRhoThermo; 

    mixture         pureMixture; 

    transport       const; 

    thermo          hConst; 

    equationOfState perfectGas; 

    specie          specie; 

    energy          sensibleEnthalpy; 

}



mixture

{

    specie

    {

        nMoles          1;

        molWeight       4;

    }

    thermodynamics

    {

        Cp              5195; 

        Hf              0;

    }

    transport

    {

        mu              2.71191e-4;

        Pr              0.66;

    }

}

i have already got this set of properties to work on another model where I just used convection. This is the next stage where I add convection and conduction together.

I am using helium as a compressible flow, in the new version of openfoam it insisted I used a mut file instead of a nut file (which seemed a bit odd).

I have not tried to get this error on any tutorials, how would I go about doing that?

I installed the new Openfoam version 3.0 using the instructions on the website. The instructions are found here; http://www.openfoam.org/download/ubuntu.php
I did not receive any errors on my system.

Thanks!

Greetings to all!

Curiously enough, I helped update the code documentation for this boundary condition a few days before 3.0.0 was released: http://www.openfoam.org/mantisbt/view.php?id=1875

And Alex has the right idea:

Quote:

Originally Posted by zfaraday (Post 573928)

You defined kappa to be computed as fluidThermo in a solid region. Check regionProperties file.

But I believe the problem is in one of the T files for one or more of the solid regions, because the error message is related to the boundary condition "temperatureCoupledBase" and it has defined "fluidThermo" instead of "solidThermo".

Quote:

Originally Posted by satkinson (Post 573938)

I am using helium as a compressible flow, in the new version of openfoam it insisted I used a mut file instead of a nut file (which seemed a bit odd).

General implementation uses "mut" for compressible flow, even if the fluid is incompressible.

Quote:

Originally Posted by satkinson (Post 573938)

I have not tried to get this error on any tutorials, how would I go about doing that?

:confused: Remember following the 3 tutorial chapters from the OpenFOAM User Guide? There it explains how to play around with the tutorial cases ;)
Another example is this: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D - which is essentially a tutorial that forces the person reading it to play with the case and test what each bit does...

@satkinson: And if you still have problems with figuring out the problem, please follow the instructions given here: http://www.cfd-online.com/Forums/ope...-get-help.html

Best regards,
Bruno

Hi All,

I checked the Temperature files as mentioned and one of them was incorrectly labled as fluidthermo. Thanks so much!

Dear Bruno one question about turbulentHeatFluxTemperature BCs. Since you once helped in updating the documentation (http://www.openfoam.org/mantisbt/view.php?id=1875) maybe you have some idea.
In OpenFOAM 2.4 it was possible to use an incompressible solver like buoyantBoussinesqSimpleFoam and set in the T file a patch with type turbulentHeatFluxTemperature
In OF 3.0 on the contrary I get the error

Quote:

Reading field T

--> FOAM FATAL IO ERROR:
Unknown patchField type turbulentHeatFluxTemperature for patch type wall

Valid patchField types are :

104
(
advective
alphatJayatillekeWallFunction
atmBoundaryLayerInletEpsilon
atmBoundaryLayerInletK
calculated
codedFixedValue
codedMixed
compressible::alphatJayatillekeWallFunction
compressible::alphatWallFunction
compressible::thermalBaffle1D<hConstSolidThermoPhy sics>
compressible::thermalBaffle1D<hPowerSolidThermoPhy sics>
compressible::turbulentHeatFluxTemperature
...

I can't use turbulentHeatFluxTemperature anymore only compressible::turbulentHeatFluxTemperature is there.
I have noticed that in OF24 turbulentHeatFluxTemperature can be found in incompressible:
https://github.com/OpenFOAM/OpenFOAM...hScalarField.H

while in OF301 can be found only in compressible:
src/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.H
Do you know the reason?

I used the following workaround to solve the issue:

1) switch solver: use buoyantSimpleFoam instead of buoyantBoussinesqSimpleFoam
2) copy from the tutorial /heatTransfer/buoyantSimpleFoam/hotRadiationRoom/constant the thermophysicalProperties file; and set the equationOfState to Boussinesq;

Code:

thermoType

{

    type            heRhoThermo;

    mixture         pureMixture;

    transport       const;

    thermo          hConst;

    equationOfState Boussinesq; //hConst;

    specie          specie;

    energy          sensibleEnthalpy;

}



pRef            100000;



mixture

{

    specie

    {

        nMoles          1;

        molWeight       28.9;

    }

    thermodynamics

    {

        Cp              1000;

        Hf              0;

    }

    transport

    {

        mu              1.8e-05;

        Pr              0.7;

    }

    

    equationOfState 

    {

        rho0             1.225;  

        T0               273;     

        beta             2;  

    }

}

3) in the 0/T file put compressible:: before turbulentHeatFluxTemperature; and add the kappa lines

Code:

floor 

{     type compressible::turbulentHeatFluxTemperature; 

      gradient uniform 0; 

      heatSource power; 

      q uniform 64; 

      kappa fluidThermo; 

      kappaName none; 

}

in this way it runs without errors:

Code:

SIMPLE: convergence criteria

    field p_rgh     tolerance 0.01

    field U     tolerance 0.001

    field h     tolerance 0.001

    field G     tolerance 0.001

    field "(k|epsilon|omega)"     tolerance 0.001



Reading thermophysical properties



Selecting thermodynamics package 

{

    type            heRhoThermo;

    mixture         pureMixture;

    transport       const;

    thermo          hConst;

    equationOfState Boussinesq;

    specie          specie;

    energy          sensibleEnthalpy;

}



Reading field U



Reading/calculating face flux field phi



Creating turbulence model



Selecting turbulence model type RAS

Selecting RAS turbulence model kEpsilon

kEpsilonCoeffs

{

    Cmu             0.09;

    C1              1.44;

    C2              1.92;

    C3              -0.33;

    sigmak          1;

    sigmaEps        1.3;

}





Reading g



Reading hRef

Calculating field g.h



Reading field p_rgh



No MRF models present



No finite volume options present



Selecting radiationModel P1

Selecting absorptionEmissionModel constantAbsorptionEmission

Selecting scatterModel none

Selecting sootModel none

Selecting transmissivityModel none



Starting time loop



Time = 1



DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.00446568, No Iterations 1

DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.00440658, No Iterations 1

DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.0020939, No Iterations 1

DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.000306369, No Iterations 1

DICPCG:  Solving for G, Initial residual = 1, Final residual = 0.0877135, No Iterations 16

DICPCG:  Solving for p_rgh, Initial residual = 0.802888, Final residual = 0.00664506, No Iterations 25

time step continuity errors : sum local = 0.028538, global = 1.78087e-17, cumulative = 1.78087e-17

rho max/min : -64.9248 -554.925

DILUPBiCG:  Solving for epsilon, Initial residual = 0.0201837, Final residual = 0.0002457, No Iterations 1

bounding epsilon, min: -0.0462023 max: 0.253471 average: 0.0444903

DILUPBiCG:  Solving for k, Initial residual = 1, Final residual = 0.0120747, No Iterations 1

ExecutionTime = 1.05 s  ClockTime = 1 s



Time = 2

sources
http://www.openfoam.org/mantisbt/view.php?id=1856
https://develop.openfoam.com/Develop...plus/issues/96

Quote:

Originally Posted by mukut (Post 457172)

Hello foamers!

I have modified multiRegionHeater Tutorial of chtMultiRegionFoam to following geometry, as I want to simulate plasma actuator induced flow:
http://i40.tinypic.com/2j61uag.jpg

In tutorials, following regions were created by toposetDict:

topAir
bottomAir
heater
leftSolid
rightSolid

Then I have modified the geometry of this tutorial like as above image in which I have defined following regions by topoSetDict

topAir (same as tutorial but differ in dimension)
bottomAir (same as tutorial but differ in dimension)
heater (as a dielectric material which is kapton film)
leftSolid (as a top electrode which is copper)
rightSolid (as a bottom electrode which is copper)
innerelec (as a inner electrode which is also copper)

I have set themophysical properties for each region according to their material properties except topAir and bottomAir as they are same air regions in my case like tutorials.

I have run following commands in the terminal:

Code:

blockMesh

topoSet

splitMeshRegions -cellZones -overwrite 

decomposePar -allRegions

mpirun -np 4 chtMultiRegionFoam -parallel

But I found following error after executing
mpirun -np 4 chtMultiRegionFoam -parallel

Code:

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$  mpirun -np 4 chtMultiRegionFoam -parallel

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.2.1                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/



Build  : 2.2.1-57f3c3617a2d

Exec   : chtMultiRegionFoam -parallel

Date   : Oct 12 2013

Time   : 09:50:20

Host   : "mukut-Endeavor-MR3300"

PID    : 4482

Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater

nProcs : 4

Slaves : 

3

(

"mukut-Endeavor-MR3300.4483"

"mukut-Endeavor-MR3300.4484"

"mukut-Endeavor-MR3300.4485"

)



Pstream initialized with:

    floatTransfer      : 0

    nProcsSimpleSum    : 0

    commsType          : nonBlocking

    polling iterations : 0

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 bottomAir for time = 0



Create fluid mesh for region topAir for time = 0



Create solid mesh for region heater for time = 0



Create solid mesh for region leftSolid for time = 0



Create solid mesh for region rightSolid for time = 0



Create solid mesh for region innerelec for time = 0



*** Reading fluid mesh thermophysical properties for region bottomAir



    Adding to thermoFluid



Selecting thermodynamics package 

{

    type            heRhoThermo;

    mixture         pureMixture;

    transport       const;

    thermo          hConst;

    equationOfState perfectGas;

    specie          specie;

    energy          sensibleEnthalpy;

}



    Adding to rhoFluid

[2] #0  

    Adding to UFluid



    Adding to phiFluid



Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

[2] #1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

[2] #2   in "/lib/x86_64-linux-gnu/libc.so.6"

[2]  #3  Foam::heRhoThermo<Foam::rhoThermo,  Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie>  >, Foam::sensibleEnthalpy> > > >::calculate() in  "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"

[2]  #4   Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo,   Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie>  >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh  const&, Foam::word const&) in  "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"

[2]  #5  Foam::autoPtr<Foam::rhoThermo>  Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&,  Foam::word const&) in  "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"

[2]  #6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word  const&) in  "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"

[2] #7  

[2]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"

[2] #8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"

[2] #9  

[2]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"

[mukut-Endeavor-MR3300:04484] *** Process received signal ***

[mukut-Endeavor-MR3300:04484] Signal: Floating point exception (8)

[mukut-Endeavor-MR3300:04484] Signal code:  (-6)

[mukut-Endeavor-MR3300:04484] Failing at address: 0x3e800001184

[mukut-Endeavor-MR3300:04484] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f05aec694a0]

[mukut-Endeavor-MR3300:04484] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f05aec69425]

[mukut-Endeavor-MR3300:04484] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f05aec694a0]

[mukut-Endeavor-MR3300:04484]  [ 3]  /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11heRhoThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEE9calculateEv+0x6cd)  [0x7f05b3ccbdad]

[mukut-Endeavor-MR3300:04484] [ 4]  /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x5c)  [0x7f05b3ceba6c]

[mukut-Endeavor-MR3300:04484] [ 5]  /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x11b)  [0x7f05b3cabccb]

[mukut-Endeavor-MR3300:04484] [ 6]  /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9)  [0x7f05b3caa1d9]

[mukut-Endeavor-MR3300:04484] [ 7] chtMultiRegionFoam() [0x423ff8]

[mukut-Endeavor-MR3300:04484] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f05aec5476d]

[mukut-Endeavor-MR3300:04484] [ 9] chtMultiRegionFoam() [0x42c5ed]

[mukut-Endeavor-MR3300:04484] *** End of error message ***

--------------------------------------------------------------------------

mpirun noticed that process rank 2 with PID 4484 on node mukut-Endeavor-MR3300 exited on signal 8 (Floating point exception).

How can I get rid of it?

Thanks in advance.

Best regards,
Mukut

Quote:

Originally Posted by fabian_roesler (Post 472487)

Hi mukut

How did you solve the problem with the foam::error::printStack? I am facing the same problem like you did in OpenFOAM 2.2.2. I perform simulations with compressibleInterFoam on a case with round about 2e6 cells. In serial the simulation runs perfect but would take weeks to finish. In parallel run I get the following error massage (I cleaned the full error output to show only errors from one calculation node):

Code:

/*---------------------------------------------------------------------------*\ 

 | =========                 |                                                 | 

 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           | 

 |  \\    /   O peration     | Version:  2.2.2                                 | 

 |   \\  /    A nd           | Web:      www.OpenFOAM.org                      | 

 |    \\/     M anipulation  |                                                 | 

 \*---------------------------------------------------------------------------*/ 

 Build  : 2.2.2-9739c53ec43f 

 Exec   : compressibleInterFoam -parallel 

 Date   : Jan 30 2014 

 Time   : 08:40:54 

 Host   : "nod00" 

 PID    : 31247 

 Case   : /home/me/OpenFOAM/me-2.2.2/run/test 

 nProcs : 16 

 Slaves :  

 15 

 ( 

 "nod01.31248" 

 "nod02.31249" 

 "nod03.31250" 

 "nod04.31251" 

 "nod05.29274" 

 "nod06.29275" 

 "nod07.29276" 

 "nod08.29277" 

 "nod09.29278" 

 "nod10.11981" 

 "nod11.11982" 

 "nod12.11983" 

 "nod13.11984" 

 "nod14.11985" 

 "nod15.11986" 

 ) 

  

 Pstream initialized with: 

     floatTransfer      : 0 

     nProcsSimpleSum    : 0 

     commsType          : nonBlocking 

     polling iterations : 0 

 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 mesh for time = 0 

  

  

 Reading g 

  

 PIMPLE: Operating solver in PISO mode 

  

 Reading field p_rgh 

  

 Reading field U 

  

 Reading/calculating face flux field phi 

  

 Constructing twoPhaseMixtureThermo 

  

 Selecting thermodynamics package  

 { 

     type            heRhoThermo; 

     mixture         pureMixture; 

     transport       const; 

     thermo          hConst; 

     equationOfState perfectFluid; 

     specie          specie; 

     energy          sensibleInternalEnergy; 

 } 

  

 [3] #0  Foam::error::printStack(Foam::Ostream&) 

 [3] #1  Foam::sigFpe::sigHandler(int) in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so" 

 [3] #2  in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so" 

 [3] #3  Foam::heThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::he(Foam::Field<double> const&, Foam::Field<double> const&, int) const[5]  at sigaction.c:0 

 [3] #4  Foam::heThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::init() in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so" 

 [3] #5  Foam::heThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::heThermo(Foam::fvMesh const&, Foam::word const&) in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so" 

 [3] #6  Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so" 

 [3] #7  Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so" 

 [3] #8  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so" 

 [3] #9  Foam::twoPhaseMixtureThermo::twoPhaseMixtureThermo(Foam::fvMesh const&) in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so" 

 [3] #10   in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libtwoPhaseMixtureThermo.so" 

 [3] #11  __libc_start_main in "/home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libtwoPhaseMixtureThermo.so" 

 [3] #12   in "/lib64/libc.so.6" 

  

 [nod03:31250] *** Process received signal *** 

 [nod03:31250] Signal: Floating point exception (8) 

 [nod03:31250] Signal code:  (-6) 

 [nod03:31250] Failing at address: 0x2271800007a12 

 [nod03:31250] [ 0] /lib64/libc.so.6() [0x3f64832920] 

 [nod03:31250] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x3f648328a5] 

 [nod03:31250] [ 2] /lib64/libc.so.6() [0x3f64832920] 

 [nod03:31250] [ 3] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so(_ZNK4Foam8heThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_12perfectFluidINS_6specieEEEEENS_22sensibleInternalEnergyEEEEEEEE2heERKNS_5FieldIdEESJ_i+0x9e) [0x7f35e50fcbae] 

 [nod03:31250] [ 4] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam8heThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_12perfectFluidINS_6specieEEEEENS_22sensibleInternalEnergyEEEEEEEE4initEv+0x206) [0x7f35e5123c96] 

 [nod03:31250] [ 5] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam8heThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_12perfectFluidINS_6specieEEEEENS_22sensibleInternalEnergyEEEEEEEEC2ERKNS_6fvMeshERKNS_4wordE+0x25a) [0x7f35e51306ba] 

 [nod03:31250] [ 6] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_12perfectFluidINS_6specieEEEEENS_22sensibleInternalEnergyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x3c) [0x7f35e51307cc] 

 [nod03:31250] [ 7] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x115) [0x7f35e50f2495] 

 [nod03:31250] [ 8] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9) [0x7f35e50f0969] 

 [nod03:31250] [ 9] /home/me/OpenFOAM/OpenFOAM-2.2.2/platforms/linux64Gcc45DPOpt/lib/libtwoPhaseMixtureThermo.so(_ZN4Foam21twoPhaseMixtureThermoC2ERKNS_6fvMeshE+0x280) [0x7f35e53c64b0] 

 [nod03:31250] [10] compressibleInterFoam() [0x42d908] 

 [nod03:31250] [11] /lib64/libc.so.6(__libc_start_main+0xfd) [0x3f6481ecdd] 

 [nod03:31250] [12] compressibleInterFoam() [0x425679] 

 [nod03:31250] *** End of error message *** 

  

 mpirun noticed that process rank 1 with PID 31248 on node nod03 exited on signal 8 (Floating point exception). 

 --------------------------------------------------------------------------

The error occurs when OpenFOAM tries to initialize the thermophysical model of the air phase. I only changed the geometry from the tutorial case. Moreover, the error shows a problem of the thermophysical model, not the case itself. Thanks for your help.

Cheers

Fabian

This error is caused by rhoThermo model for fluid region, so please check your initial value settings in 0/p, T, k, epsilon, p_rgh file.
If the initial value is equal 0 in fluid region or solid-fluid interface, floating point exception will be caused.

ERROR: Cannot find a fluidThermo or solidThermo instance

Dear Foamers,
I am very new to openfoam and CFD, kindly I need your help.

I have been simulating conjugate heat transfer between solid(wall) to fluid.
So i used externalWallHeatFluxHeatTransfer boundary condition on the wall surfaces and used kappaMethod as solidThermo on my temperature(T) file.
After i started to run my solver, I encounter this error ,

--> FOAM FATAL ERROR:
Cannot find a fluidThermo or solidThermo instance

From function Foam::tmp<Foam::Field<double> > Foam::temperatureCoupledBase::kappa(const fvPatchScalarField&) const
in file derivedFvPatchFields/temperatureCoupledBase/temperatureCoupledBase.C at line 124.

FOAM exiting.

How to solve this error?

Thanks
Rishi