# LES using FLUENT

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 19, 2004, 09:46 LES using FLUENT #1 sarah_ron Guest   Posts: n/a LES using FLUENT Posted By: sa Date: Fri, 2 Apr 2004, 3:56 p.m. I am a little confused while running LES simulations using FLUENT. I am simulating Incompressible Impinging Jets. Just looking into velocity and pressure profiles and vortex generation. 1) First I run the simulation for a certain number of iterations to get statistically steady flow. 2) Then I use command solve/initialize/init-flow-statistics to zero initial statistics. 3) Then I enable Data Sampling for Time Statistics in the iterate panel. My questions are as follows? A)Is that the correct way to run LES in Fluent? Else please let me know if I am doing something wrong. Because in an example problem by Fluent, I saw they did not perform step 2 and went straight to step 3. B)Also what is my criterion for selecting time step when I am running the implicit scheme? For explicit schemes, we generally resort to CFD criteria. C)Which solver gives better results segregated or coupled ? D) Though PISO is recommended for transient flows, it takes a lot of time. Is it ok to use SIMPLE? E) For momentum discretization, I am using Central Diff. Is 2nd Order Upwind better? F) Is there some tutorial using LES in FLUENT, other than the Acoustics one? Thanks for your help. Sincerely sa

 October 20, 2004, 04:07 Re: LES using FLUENT #2 dieter Guest   Posts: n/a A) If you don't select data sampling from the beginning, statistics are set to zero, so you don't have to reset them when enabling data sampling. That's what fluent does in the manuals. I think the method is good as you use it. B)Choose your timestep small enough... fluent indicates that you should have convergence in 20 iterations per time step, if its not, choose the timestep smaller. C)You have more options when using segregated solver. Coupled solver limits the use of e.g. udf's etc... i think. I don't think it's better or worse D)PISO is more accurate E)2nd order upwind is more accurate, but less stable. in the beginning of the iterations, use first order, if you have some convergence, switch to 2nd order... that's the general rule. F) sorry i don't know..

 October 20, 2004, 13:02 Re: LES using FLUENT #3 Ray Guest   Posts: n/a Question E): Better use central difference for LES rather than 2nd upwind. Ray

 October 21, 2004, 19:59 Re: LES using FLUENT #4 Chetan Kadakia Guest   Posts: n/a Sarah, Why do you choose LES? It is more time consuming. Why do you feel it is required? For the time step, you might want to concern yourself with what kind of eddies you want to resolve. Smaller eddies require smaller time steps, and then you may have some calculation to do. If your time step is too large, and you aren't getting convergence, it may be telling you that the change with time is too aggressive for the time step chosen. That's why Fluent recommends convergence within 20 time steps or so. PISO is recommended for unsteady and Central Differencing is recommended for LES. I don't think you need a specific tutorial on LES. But you do need a smaller grid size than that of a RANS solution, and of course has to be unsteady. It is also preferable to run LES for 3D problems as there is vortex stretching, and the 2D LES solutions wont capture that calculation. I've worked on LES quite a bit, so do email me if you have questions or like to talk more about your problem. Chetan

 October 21, 2004, 22:01 Re: LES using FLUENT #5 dumb Guest   Posts: n/a apart from smaller time step you will need very very fine mesh(specially near wall), go for LES only if you have hardware to run it, i am trying it for flow around cylinder and eventhough my mesh is very fine i still doubt about results (can't comment on my results as run is still in progress, i shall not know much about them before monday)

 October 22, 2004, 17:34 Re: LES using FLUENT #6 sarah_ron Guest   Posts: n/a Thank you very much for your kind reply. I have the following questions about les in fluent, hope you help me. (1) time step: I think there could be two methods for judging the time step. One is to estimate the smallest eddy turnover time, whose size is proportional to smallest grid size. I.e, time step~delta/U, where delta is the smallest grid size and U is maximal velocity. Another method is just that recommended by Fluent manual, i.e converging with 10~20. Am I right? If not, give me some lights; (2) In fluent les tutorial (Acoustics), it chose relaxation factors 1 for all the variables. Why? Just to speed the convergence? (3) To monitor the calculation to achieve "dynamically steady state ", a point monitor is set up in tutorial. Where (what position) should I put the monitor point? Are there any guidelines? (4) To judge the "dynamically steady state ", the pressure value (or other variables) will be oscillation fairly regularly around a horizontal line. But in the tutorial, I found it varies between –2500 and –1250. How could I know whether this range is large or not? Or it doesn't matter ? (5) For convergence, the tutorial put an asymmetric numerical disturbance. Where should I put it? Is there any guideline? (6) After the flow reach the steady state, it needs some time to obtain the stable statistics. How long should it take? Fluent gave some hints, but I am really confusing. For example, if I am dealing with flow in a tube, what should be the characteristic velocity? Thanks sarah

 October 22, 2004, 17:35 Re: LES using FLUENT #7 sarah_ron Guest   Posts: n/a

 October 22, 2004, 17:36 Thank you all #8 sarah_ron Guest   Posts: n/a I very appreciate all your help. Hope I could learn more from you!

 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 anee FLUENT 0 September 27, 2011 01:10 ivanbuz FLUENT 11 March 10, 2010 16:13 khosro1355 Main CFD Forum 1 July 10, 2009 10:49 Sham FLUENT 0 August 1, 2007 21:31 sat FLUENT 0 August 2, 2004 18:32

All times are GMT -4. The time now is 03:54.

 Contact Us - CFD Online - Top