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

Error in thermophysical properties (chtMultiRegionFoam)

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

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 17, 2015, 13:56
Default
  #21
New Member
 
S Atkinson
Join Date: Mar 2015
Posts: 14
Rep Power: 4
satkinson is on a distinguished road
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!
Attached Files
File Type: txt thermophysicalProperties.txt (1.6 KB, 54 views)
satkinson is offline   Reply With Quote

Old   November 18, 2015, 15:34
Default
  #22
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 336
Rep Power: 15
zfaraday will become famous soon enough
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 View Post
Quick questions @fkika: Please provide more details, such as:
  1. Which OpenFOAM version are you using?
  2. Which installation instructions did you follow for installing OpenFOAM?
  3. Can you reproduce this error with one of OpenFOAM's tutorials?
  4. 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 View Post
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!

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!

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
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   November 18, 2015, 17:58
Default
  #23
New Member
 
S Atkinson
Join Date: Mar 2015
Posts: 14
Rep Power: 4
satkinson is on a distinguished road
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!
vs1 likes this.
satkinson is offline   Reply With Quote

Old   November 22, 2015, 17:28
Default
  #24
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,021
Blog Entries: 39
Rep Power: 109
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
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 View Post
  • 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 View Post
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 View Post
I have not tried to get this error on any tutorials, how would I go about doing that?
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
__________________
wyldckat is offline   Reply With Quote

Old   November 23, 2015, 09:17
Default
  #25
New Member
 
S Atkinson
Join Date: Mar 2015
Posts: 14
Rep Power: 4
satkinson is on a distinguished road
Hi All,

I checked the Temperature files as mentioned and one of them was incorrectly labled as fluidthermo. Thanks so much!
satkinson is offline   Reply With Quote

Old   April 12, 2016, 03:12
Default
  #26
Member
 
Al
Join Date: Jul 2013
Location: Japan
Posts: 45
Blog Entries: 3
Rep Power: 7
donQi is on a distinguished road
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?
FLZ likes this.
donQi is offline   Reply With Quote

Old   April 13, 2016, 03:12
Default
  #27
Member
 
Al
Join Date: Jul 2013
Location: Japan
Posts: 45
Blog Entries: 3
Rep Power: 7
donQi is on a distinguished road
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
nikitin-pro likes this.
donQi is offline   Reply With Quote

Old   October 5, 2017, 06:48
Default
  #28
vs1
New Member
 
vaibhav
Join Date: Sep 2016
Posts: 11
Rep Power: 3
vs1 is on a distinguished road
Quote:
Originally Posted by mukut View Post
Hello foamers!

I have modified multiRegionHeater Tutorial of chtMultiRegionFoam to following geometry, as I want to simulate plasma actuator induced flow:


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 View Post
Hi mukut

How did you solve the problem with the foam::error:rintStack? 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.
vs1 is offline   Reply With Quote

Reply

Tags
chtmultiregionfoam, error, plasma actuator modeling, pre-processing

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
table properties for thermophysical properties romant OpenFOAM Running, Solving & CFD 1 August 12, 2014 08:41
thermophysical properties immortality OpenFOAM Running, Solving & CFD 0 December 2, 2012 07:49
polynomial thermophysical properties in a solid region (chtMultiRegionSimpleFoam) Koga OpenFOAM Programming & Development 0 November 15, 2012 05:14
how to incorporate temperature dependent thermophysical properties in fluent. CANDY Fluent UDF and Scheme Programming 4 October 22, 2012 04:19
thermophysical properties of ham Alex Ivancic Main CFD Forum 1 November 5, 1998 12:09


All times are GMT -4. The time now is 16:28.