 |
 |
 |
|
|
|
[Sponsors] | ||||
Error in thermophysical properties (chtMultiRegionFoam) |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 17, 2015, 13:56
|
|
#21 |
|
New Member
S Atkinson
Join Date: Mar 2015
Posts: 14
Rep Power: 11  |
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! |
|
|
|
|
|
November 18, 2015, 15:34
|
|
#22 | ||
|
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 |
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:
Quote:
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:
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! 
|
|||
|
|
|
|||
|
November 18, 2015, 17:58
|
|
#23 |
|
New Member
S Atkinson
Join Date: Mar 2015
Posts: 14
Rep Power: 11 |
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 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! |
|
|
|
|
|
|
November 22, 2015, 17:28
|
|
#24 | |||
|
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,982
Blog Entries: 45
Rep Power: 128  |
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:
Quote:
Quote:
 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
__________________
|
||||
|
|
|
||||
|
November 23, 2015, 09:17
|
|
#25 |
|
New Member
S Atkinson
Join Date: Mar 2015
Posts: 14
Rep Power: 11 |
Hi All,
I checked the Temperature files as mentioned and one of them was incorrectly labled as fluidthermo. Thanks so much! |
|
|
|
|
|
|
April 12, 2016, 04:12
|
|
#26 | |
|
Member
|
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:
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? |
||
|
|
|
||
|
April 13, 2016, 04:12
|
|
#27 |
|
Member
|
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;
}
}
Code:
floor
{ type compressible::turbulentHeatFluxTemperature;
gradient uniform 0;
heatSource power;
q uniform 64;
kappa fluidThermo;
kappaName none;
}
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
http://www.openfoam.org/mantisbt/view.php?id=1856 https://develop.openfoam.com/Develop...plus/issues/96 |
|
|
|
|
|
|
October 5, 2017, 07:48
|
|
#28 | ||
|
New Member
vaibhav
Join Date: Sep 2016
Posts: 15
Rep Power: 10 |
Quote:
Quote:
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. |
|||
|
|
|
|||
|
November 23, 2021, 07:34
|
ERROR: Cannot find a fluidThermo or solidThermo instance
|
#29 |
|
New Member
Join Date: Mar 2021
Posts: 1
Rep Power: 0 |
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 |
|
|
|
|
|
|
| Tags |
| chtmultiregionfoam, error, plasma actuator modeling, pre-processing |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| table properties for thermophysical properties | romant | OpenFOAM Running, Solving & CFD | 1 | August 12, 2014 09:41 |
| 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 05:19 |
| thermophysical properties of ham | Alex Ivancic | Main CFD Forum | 1 | November 5, 1998 12:09 |
11Likes
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):
Linear Mode
