# Problem with frictional stress model in twoPhaseEulerFoam

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

 May 11, 2015, 07:48 Problem with frictional stress model in twoPhaseEulerFoam #1 New Member   Giovanni Tretola Join Date: May 2015 Posts: 2 Rep Power: 0 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::T(scalar f, scalar T0, scalar (thermo::*F)(const scalar) const, scalar (thermo::*dFdT)(const scalar) const, scalar (thermo::*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.

 August 17, 2015, 05:36 #2 New Member   Ramon Join Date: Feb 2014 Location: Eindhoven Posts: 25 Rep Power: 5 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

 October 20, 2015, 06:37 #3 New Member   Giovanni Tretola Join Date: May 2015 Posts: 2 Rep Power: 0 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Jade M Main CFD Forum 27 August 11, 2017 15:41 skyinventorbt OpenFOAM 0 August 14, 2013 06:18 Edy OpenFOAM 7 August 10, 2011 12:00 Srinivas FLUENT 0 October 17, 2005 06:35 S. Bottenheim Siemens 2 January 28, 2005 09:55