[gianniTre]

Hi everybody,

I run simulations about a bubbling fluidized bed with a central jet trough the solver twoPhaseEulerFoam, with OpenFOAM 2.3.0 .
With the same model proposed in the respective tutorial there are not problem.
When I try to use the fictionalStressModel proposed by Scaeffer, instead of Sinclair and Jackson model, the error below appeares:

MULES: Solving for alpha.particles
MULES: Solving for alpha.particles
smoothSolver:  Solving for alpha.particles, Initial residual = 0.000210983, Final residual = 9.29629e-10, No Iterations 33
alpha.particles volume fraction = 0.299921  Min(alpha1) = 1.6525e-28  Max(alpha1) = 0.63922
smoothSolver:  Solving for e.particles, Initial residual = 0.181574, Final residual = 5.93711e-07, No Iterations 16
smoothSolver:  Solving for e.air, Initial residual = 0.795681, Final residual = 1.13052e-07, No Iterations 4


--> FOAM FATAL ERROR: 
Maximum number of iterations exceeded

    From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const
    in file /home/sergio/rpmbuild/BUILD/OpenFOAM-2.3.0/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/share/apps/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

I try to change relaxation factor, to reduce relative tolerance and increase numbers of outer correctors.
The results is that the source of the error changes: initially it was energy equation, reducing relaxation factor alpha equation became the error, and so on.
Mesh is perfect orthogonal.
Anybody knows why changing the frictional stress model, I get this error?

Thank you.

[RjwV]

Hello gianniTre,

I am a little bit confused about your settings. I know the Schaeffer frictional stress model. However I do not know the Sinclair and Jackson frictional stress model, I assume you mean Johnson and Jackson?

Note the warning, maximum number of iterations exceeded. Looks like your pressure solution is not converging... can you try decreasing your time-step, or maybe even increasing your number of corrector loops for the pressure if the decrease in time-step alone does not help?

Kind regards,
Ramon

[gianniTre]

Hello Ramon,

thank you for your reply, and sorry for the delay in getting back to you.

About Sinclair and Jackson frictional stress model you are right, I mean Johnson and Jackson, I mixed up with the name!

I think that I have resolved my problem:

About correction on pressure loops or decreasing of time step, I tried but the errors did not disappeared.
I obtained convergence only if I use a value of 0.6 for the threshold value of alpha (\alpha_{s,fr,min}) instead of the value usually used in literature (0.63). If there were errors also for this value, for example if I tried different value of inlet velocity or change mesh parameters, I obtained convergence decreasing time step and increasing number of corrector loops for the pressure, but this set up gives a high computational time.

I found strange that I can obtain convergence only for that value of \alpha_{s,fr,min} (in fact if I tried different value errors remains) so I tried to change the solver in the fvSolution for the equation. Originally a smoother solver was used, I use a PCG solver, and I obtained a fast convergence. When some problems arise , I resolved giving a lower value for tolerance of alpha equations or reducing the max Courant number is enough to convergence. The fact that change the solver was enough and I never thinking about it, demonstrates that I am a beginner!

In any case thanks for the reply.

Kind regards,
Giovanni