# Turbulence model convergence problem

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

 August 14, 2008, 08:32 Turbulence model convergence problem #1 Andrew Guest   Posts: n/a Hi, I am modeling a buoyancy drive flow in a concentric cylinder annulus. For very high temperature difference, i am assuming the flow to be turbulent and used SST and Reynolds stress BSL model. I set all the initial turbulence conditions to automatic. Upon solving, i only get convergence to 10^-5 using RMS criteria at 1500 iterations. Rate of convergence is very low. Can anyone tell me why is that so? Have i set anything wrong? Andrew

 August 14, 2008, 08:33 Re: Turbulence model convergence problem #2 Andrew Guest   Posts: n/a Note: i am running a steady state simulation... could it be the solution is actually not steady?

 August 14, 2008, 09:23 Re: Turbulence model convergence problem #3 John S. Guest   Posts: n/a 1e-5 is decent for residual convergence. I would check your timescale. If your timescale is too small convergence can take a long time to achieve. In general, the Reynolds Stress models should be run with a lower timescale.

 August 14, 2008, 11:51 Re: Turbulence model convergence problem #4 Andrew Guest   Posts: n/a my residuals were all stuck fluctuating at only 10^-3. I am using SST models with turbulence buoyancy on. I don't have any idea what time scale factor or what time scale control to use.

 August 14, 2008, 15:10 Re: Turbulence model convergence problem #5 Ricardo Guest   Posts: n/a One criterion is the Courant Number, even though you get convergence, with high courrant number, is better the value around 1, the MAx value, what results in a RMS courant number samller arounf o(10^-1). RElated to SST model, consider the y+ value, it is below 2 as recomended? And has the fact that your case don't have a steady state solution, and you 'll see oscilations of residue with a aplitude and frequence nearly constant, after some interations. This is a indication, not a certain, that your problem has a periodic behavior.

 August 14, 2008, 18:25 Re: Turbulence model convergence problem #6 Andrew Guest   Posts: n/a Yes, my y+ value is below 2. I can't get convergence while i turned on buoyancy turbulence option in cfx. I turned it off, the the solution was able to get up to 10^4 RMS and the results seems fine. I am also not sure whether to turn on turbulence buoyancy. Also, i am not sure of using the full buoyancy model with varying density or the bousinnesq model assuming constant density. Any ideas?

 August 14, 2008, 19:45 Re: Turbulence model convergence problem #7 Ricardo Guest   Posts: n/a generally, the buoyancy option for turbulence overprecict the eddy viscosity and kill the dynamic behavior. Por exmplae, if you have a bubble colum, the plume with buoyancy can be well-behaved, and when you turn off, the dynamic and instabilities of the flow arise. The model is not so good yet in my opnion. but depends on the case. Related to density, depends on the case again. Variable density is hard to converge, requiring small time steps... generaly, and boussineq model, well, is there the thermal gradient strong? If not, boussinesq is a good approach, if is strong or very steep,no! But As you problme is in steady state, begin with contant density and turbulence on bouyance tirned off. Oce converged, use this solution as initial guess to a density variable simulation and/or boussinesq. It is a good a approach to complicated problmes, a initial simulation more simple and step-by-step, effort the model with more features until you reach the desired solution. I have a multiphase problem that operation takes 1.5 hours! I begun with a transient simulation durig 35seconds and I've used the last time step as initial guess to a steady state with a pseudo elapsed time aroud 2 hours - the time wich I wated! Try similarsome thing . from simple to complex models until you have the good slution. Good luck!

 August 17, 2008, 19:35 Re: Turbulence model convergence problem #8 Glenn Horrocks Guest   Posts: n/a Have you looked at this page? http://www.cfd-online.com/Wiki/Ansys...gence_criteria Glenn Horrocks

 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 FelixL OpenFOAM Programming & Development 114 July 6, 2016 07:10 usama FLUENT 1 August 18, 2011 07:12 qascapri FLUENT 0 January 24, 2011 11:48 akonduri OpenFOAM 2 September 17, 2010 00:49 gianlu OpenFOAM Running, Solving & CFD 1 July 25, 2009 11:27

All times are GMT -4. The time now is 08:59.