CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Problem with frictional stress model in twoPhaseEulerFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 11, 2015, 07:48
Smile Problem with frictional stress model in twoPhaseEulerFoam
  #1
New Member
 
Giovanni Tretola
Join Date: May 2015
Posts: 2
Rep Power: 0
gianniTre is on a distinguished road
Sponsored Links
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:

Code:
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.
gianniTre is offline   Reply With Quote
Sponsored Links

Old   August 17, 2015, 05:36
Default
  #2
New Member
 
Ramon
Join Date: Feb 2014
Location: Eindhoven
Posts: 25
Rep Power: 5
RjwV is on a distinguished road
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
RjwV is offline   Reply With Quote

Old   October 20, 2015, 06:37
Default
  #3
New Member
 
Giovanni Tretola
Join Date: May 2015
Posts: 2
Rep Power: 0
gianniTre is on a distinguished road
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
gianniTre is offline   Reply With Quote

Reply

Tags
frictional stress model, opehfoam, two fluid model, twophaseeulerfoam

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
Use of k-epsilon and k-omega Models Jade M Main CFD Forum 27 August 11, 2017 15:41
Simulation of Axisymmetric Free Jet using LRR Reynolds Stress Model skyinventorbt OpenFOAM 0 August 14, 2013 06:18
Stability problem due to turbulent dispersion force in a subcooled boiling model Edy OpenFOAM 7 August 10, 2011 12:00
multiphase mixing Problem with MRF model in MixSim Srinivas FLUENT 0 October 17, 2005 06:35
Writing a BCDEFI problem for RSM model S. Bottenheim Siemens 2 January 28, 2005 09:55

Sponsored Links


All times are GMT -4. The time now is 20:19.