|
[Sponsors] |
April 30, 2018, 08:18 |
Negative initial temperature
|
#1 |
New Member
Join Date: Apr 2018
Posts: 9
Rep Power: 8 |
Hello,
i'm trying to simulate the heating of a cube with a channel full of hot oil through it with the chtMultiRegionSimpleFoam-solver. But whenever the initialfield temperature of the oil differs from the temperature of my inlet, openfoam aborts after a few time steps with the explanation, that the inital temperature is negative. The error message says something about an error in thermophysicalProperties.H line 54. Does anybody know a solution, please? I attach the T, fvSolution and fvsheme files of the fluid. |
|
April 30, 2018, 10:36 |
|
#2 | |
Member
ff
Join Date: Feb 2010
Posts: 81
Rep Power: 16 |
Do you have radiation in your case?
Quote:
|
||
April 30, 2018, 11:02 |
|
#3 |
New Member
Join Date: Apr 2018
Posts: 9
Rep Power: 8 |
I have the file, but the radiation is turned off.
|
|
April 30, 2018, 12:01 |
|
#4 |
Member
ff
Join Date: Feb 2010
Posts: 81
Rep Power: 16 |
||
April 30, 2018, 13:13 |
|
#5 |
New Member
Join Date: Apr 2018
Posts: 9
Rep Power: 8 |
The geometry is quite simple. A cube with a hole and a cylinder inside the hole. The cube is declared as solid and the cylinder as fluid.
|
|
May 1, 2018, 12:58 |
|
#6 |
New Member
Join Date: Apr 2018
Posts: 9
Rep Power: 8 |
Maybe it is helpful, if i post the complete error message:
Time = 417 Solving for fluid region FLUIDROHR DILUPBiCG: Solving for h, Initial residual = 0.0006912361, Final residual = 2.371398e-11, No Iterations 1 Min/max T:-0.6823983 433 GAMG: Solving for p_rgh, Initial residual = 0.7395947, Final residual = 0.3443955, No Iterations 10 time step continuity errors : sum local = 1.071075e-13, global = 4.308673e-16, cumulative = -1.476626e-14 Min/max rho:2 2 Solving for solid region SOLIDWURFEL DICPCG: Solving for h, Initial residual = 0.009793508, Final residual = 0.0001714627, No Iterations 3 DICPCG: Solving for h, Initial residual = 0.01000549, Final residual = 0.000171063, No Iterations 3 DICPCG: Solving for h, Initial residual = 0.009274253, Final residual = 0.0001471489, No Iterations 3 DICPCG: Solving for h, Initial residual = 0.009199457, Final residual = 0.0001446249, No Iterations 3 Min/max T:316.1508 318.3617 ExecutionTime = 88.38 s ClockTime = 92 s Time = 418 Solving for fluid region FLUIDROHR DILUPBiCG: Solving for h, Initial residual = 0.0006895797, Final residual = 2.367034e-11, No Iterations 1 --> FOAM FATAL ERROR: Negative initial temperature T0: -0.6823983 From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hConstThermo<Foam::rhoConst<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::rho Const<Foam::specie> >, Foam::sensibleEnthalpy>] in file /home/pawan/OpenFOAM/OpenFOAM-v1712/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54. FOAM aborting #0 Foam::error:rintStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam::constTransport<Foam::speci es::thermo<Foam::hConstThermo<Foam::rhoConst<Foam: :specie> >, Foam::sensibleEnthalpy> > > >::calculate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, bool) at ??:? #3 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam::constTransport<Foam::speci es::thermo<Foam::hConstThermo<Foam::rhoConst<Foam: :specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:? #4 ? at ??:? #5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #6 ? at ??:? Abgebrochen (Speicherabzug geschrieben) FLUIDROHR is the oil-cylinder and SOLIDWURFEL is the cube. The respective line says this: scalar Ttol = T0*tol_; |
|
May 2, 2018, 13:27 |
|
#7 |
Member
ff
Join Date: Feb 2010
Posts: 81
Rep Power: 16 |
can you use min/Max functionobject to identify where is the negative temperature?
|
|
May 2, 2018, 14:13 |
|
#8 |
New Member
Join Date: Apr 2018
Posts: 9
Rep Power: 8 |
Sorry, i am not very experienced, how do i do that?
Via trial and error, I also found out, that i can postpone the error by decreasing the relaxationFactors for h. But then i don't have any heat transfer between inlet and oil(not sure if that is always the case, or only with the small relaxation factor) Last edited by Lexe; May 2, 2018 at 17:48. |
|
May 7, 2018, 09:00 |
|
#9 |
New Member
Join Date: Apr 2018
Posts: 9
Rep Power: 8 |
Anybody? Please, i need this for my thesis and i'm running out of time.
|
|
May 7, 2018, 18:40 |
|
#10 |
New Member
Osman Mirza Demircan
Join Date: May 2017
Location: Ankara, Türkiye
Posts: 29
Rep Power: 9 |
I'm not familiar with that solver but maybe you could make use of a fvOptions file with the limitTemperature function in it? Here's an example,
limitTemperature { type limitTemperature; active true; limitTemperatureCoeffs { selectionMode all; Tmin 200; Tmax 400; } }
__________________
Osman Mirza Demircan |
|
September 20, 2018, 07:46 |
|
#11 |
New Member
vaibhav
Join Date: Sep 2016
Posts: 15
Rep Power: 10 |
I get the same error when i set turbulence to laminar but with other turbulence models the error is gone.
|
|
September 23, 2018, 18:25 |
|
#12 |
New Member
Join Date: Aug 2017
Posts: 18
Rep Power: 9 |
I am not familiar with that solver but I think that you should check how it calculates the temperature. Then you will better understand who's the culprit.
Have you tried to reduce the time step or the cell size? |
|
September 24, 2018, 05:22 |
|
#13 | |||
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
Hi all,
just a few comments on your situations Quote:
Quote:
Quote:
__________________
Keep foaming, Tobias Holzmann |
||||
July 6, 2019, 13:52 |
The Same Problem
|
#14 |
New Member
Jalil
Join Date: Nov 2018
Posts: 8
Rep Power: 8 |
Dear Tobias and everyone else!
Thank you for your nice comments. I have the same problem. I am trying to simulate an air pocket traveling upstream in a pipe and eventually escaping from a ventilation hole at the top of the the tower (image attached). I use compressibleInterFoam solver, but the temperature drops below zero and the simulation stops. As you mentioned, I am not sure about the boundary conditions, but I am sure BCs are set wrong. The "limitTemperature" function does not work. I have attached an image of the apparatus and a file that contains all BCs from 0 folder. Can you please have a look and let me know what is wrong with them. Thank you all in advance! Jalil |
|
October 23, 2019, 11:29 |
|
#15 |
New Member
Robson Leo Pachaly
Join Date: Oct 2019
Posts: 3
Rep Power: 7 |
Hello everyone,
I'm trying to simulate something very similar to Jalil and having the same problem. The limitTemperature function approach also did not work for me. Does anybody have any other solution? Thanks! |
|
October 23, 2019, 11:49 |
|
#16 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
Hi,
For me, the limit Temperature function is working fine always. Is it initialized at the start of the application?
__________________
Keep foaming, Tobias Holzmann |
|
January 10, 2020, 05:12 |
|
#17 | |
New Member
Arne
Join Date: Dec 2018
Posts: 19
Rep Power: 8 |
Quote:
Hello everyone I also have a problem with 'limitTemperature', but it is only when I try to run this in parallel. In that case, it seems to ignore the fvOptions (it errors at the same time with the same negative value for the temperature as when fvOptions was not present) even though it is certainly read. Does anyone have experience with limitTemperature in parallel run? Thanks in advance. Best regards Arne |
||
January 12, 2020, 12:01 |
|
#18 |
New Member
Jalil
Join Date: Nov 2018
Posts: 8
Rep Power: 8 |
Based on my experience, the problem "Negative Initial Temperature" usually existed with the mesh. If there are some bad cells in the mesh or the cells are too different from each other in a region i.e the cells are refined in some regions and are very course in some other regions, then the model crashes.
I tried changing the mesh multiple times and it finally worked. |
|
April 9, 2020, 22:16 |
|
#19 |
Member
Sai Guruprasad Jakkala
Join Date: Jan 2017
Posts: 34
Rep Power: 9 |
I was having the same problem and changing the mesh got rid of the problem.
Make sure that there is no sudden change in mesh spacings. |
|
May 22, 2020, 04:01 |
|
#20 | |
New Member
Jad
Join Date: Jun 2013
Posts: 15
Rep Power: 13 |
Quote:
Same here. Running a mesh convergence study on a buoyantSimpleFoam case and it ran just fine (ie boundary conditions are OK) until a bad quality iteration of the mesh made it crash with negative temperature. In many cases just running checkMesh will give you a good idea of how your simulation is likely to behave. |
||
Tags |
chtmultiregionsimpefoam, temperature calculation |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Free surface issues with interDyMFoam for hydroturbine | oumnion | OpenFOAM Running, Solving & CFD | 0 | October 6, 2017 15:05 |
Extrusion with OpenFoam problem No. Iterations 0 | Lord Kelvin | OpenFOAM Running, Solving & CFD | 8 | March 28, 2016 12:08 |
Cannot run the code properly: very large time step continuity error | crst15 | OpenFOAM Running, Solving & CFD | 9 | December 14, 2014 19:17 |
pimpleFoam: turbulence->correct(); is not executed when using residualControl | hfs | OpenFOAM Running, Solving & CFD | 3 | October 29, 2013 09:35 |
SLTS+rhoPisoFoam: what is rDeltaT??? | nileshjrane | OpenFOAM Running, Solving & CFD | 4 | February 25, 2013 05:13 |