[LucaFen]

Hi guys,
i'm simulating air-flow in a pipe with janaf thermophysical properties.
After few iterations i get the following warning:

smoothSolver:  Solving for Ux, Initial residual = 0.0439616, Final residual = 8.21134e-05, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.0322465, Final residual = 6.6714e-05, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 0.0565688, Final residual = 9.47675e-05, No Iterations 2
DILUPBiCG:  Solving for e, Initial residual = 0.956923, Final residual = 0.0387152, No Iterations 1
--> FOAM Warning : 
    From function janafThermo<EquationOfState>::limit(const scalar T) const
    in file /home/openfoam/OpenFOAM/OpenFOAM-2.3.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
    attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 177.597
--> FOAM Warning : 
    From function janafThermo<EquationOfState>::limit(const scalar T) const
    in file /home/openfoam/OpenFOAM/OpenFOAM-2.3.1/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
    attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 6000;  T = 177.349
GAMG:  Solving for p, Initial residual = 0.0334125, Final residual = 0.00116066, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.00224451, Final residual = 9.06173e-05, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.000569202, Final residual = 2.02722e-05, No Iterations 4
time step continuity errors : sum local = 5.47722e-06, global = 1.75769e-07, cumulative = 1.3574e-07
rho max/min : 5.33983 5.33553
smoothSolver:  Solving for epsilon, Initial residual = 0.333987, Final residual = 2.81183e-06, No Iterations 2
smoothSolver:  Solving for k, Initial residual = 0.340597, Final residual = 3.04902e-06, No Iterations 2
ExecutionTime = 37.59 s  ClockTime = 38 s

Open Foam doesn't return a fatal error, but the following iterations get worse and returns a huge number of warning.

I checked on other threads but i haven't found any useful hint.

Boundary conditions and thermophysical properties files are attached.
boundaryconditions.zip

thermophysicalProperties (copy).zip

[LucaFen]

I solved!
The problem was that the initial condition was too far from the solution and the JANAF model suffers of instability.
I used a time-variable boundary condition to progressively grow up the velocity till the value requested.

[fabri]

Hi LucaFen,
I have the same problem.
Could you explain me in detail how did you solve this warning?

Thank you very much in advance
Best regards
Fabri

Here my warning:

--> FOAM Warning :
From function Foam::scalar Foam::janafThermo<EquationOfState>::limit(Foam::sc alar) const [with EquationOfState = Foam:erfectGas<Foam::specie>; Foam::scalar = double]
in file /modeling/OpenFOAM/OpenFOAM-4.0/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 105
attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 4000; T = 159.418
min/max(T) = 200, 2240.28

[LucaFen]

Hi Fabri,
I changed the BC for the velocity inlet from fixedValue to uniformFixedValue as follows:

Inlet
{
type uniformFixedValue;
uniformValue table
2
(
(0 (0 0 0) )
(4500 (300 0 0) )
);


This means that the at each iteration the inlet velocity is increased according to a linear law definined by the initial and final time ( 0 and 4500) and by the velocity values( (0 0 0) and (300 0 0)).

in this way I noticed that the solver (rhoSimpleFoam) works better and is more stable.