# grid adaptation for better convergence.

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

 March 30, 2004, 17:08 grid adaptation for better convergence. #1 co2 Guest   Posts: n/a 03/30/2004 I have a volume made of conical frustum placed on top of a cylinder. I am trying to solve for natural convection currents in this volume using Boussinesq approximation for density variation. From Ra number calculations, I know that the conditions are turbulent in this volume (Ra>10^10) I have a good hex mesh with max skew ness of 0.51 with all turbulent boundary layers resolved well. Still I am having trouble in getting convergence. The last residual values reported are: Continuity = 6.0564e-03 X-velocity = 2.5158e-04 Y-velocity = 1.9871e-04 Z-velocity = 2.4165e-03 energy = 6.9842e-07 k = 3.3916e-04 epsilon = 4.3959e-04 Thus I guess it is not too bad of a convergence, but I want to use grid adaptation in fluent to improve my results. Can someone suggest as to what type of adaptation I should be focusing on?

 March 30, 2004, 19:01 Re: grid adaptation for better convergence. #2 Otilia Guest   Posts: n/a Check wall y+. It should be between 30 and 300 if you are using standard wall treatment. You may need to use EWT (y+<5) to better capture natural convection. I assume you have a closed domain, so you can not use mass balance to double-check convergence. The high residuals are very likely to be caused by the transient behaviour of the solution. Natural convection is usually an unsteady phenomena that needs to be simulated with a transient simulation. You will see what I mean if you solve the problem with the unsteady solver and animate a contour plot of temperature/velocities (create a video). Solution will change with time.

 March 30, 2004, 21:39 Re: grid adaptation for better convergence. #3 co2 Guest   Posts: n/a well, i do not have closed domain. I have a vent (pressure outlet BC) at the top. thanks a lot for all the explanation. But my question was what type of grid adaptation I should use ? should I keep refining my mesh till y+ gets in the correct range of 30 to 300? I donot want my grid size to go too high to keep solution time down. thanks, CO2

 March 31, 2004, 02:54 Re: grid adaptation for better convergence. #4 Alamgir Guest   Posts: n/a To adapt the grid you use velocity or pressure bc. Alamgir

 March 31, 2004, 06:22 Re: grid adaptation for better convergence. #5 zxaar Guest   Posts: n/a last year i did one natural convection problem, in the start i had some convergence problems, but after refinign the mesh that went away, and second we found it conversing with coupled solver (better than segregated), so you can try coupled solver, might help.

 March 31, 2004, 11:12 Re: grid adaptation for better convergence. #6 co2 Guest   Posts: n/a coupled solver: isnt it true that coupled solver is used only for highly compressible flows? I tried coupled solver in my case, the solution was obtained but vel vectors were looking weird - it was as if gravity was acting in X direction, although i had specified it in Z drn. I solved the steady case yesterday with all hex elements in my geometry - I had to use low underrelax params - around all of them 0.5 - IS THAT OK? k-EPSILON model was on, since Re numbers in headspace of the tank geometry are around 15000 (due to low viscosity of air) - after gettting solution to the the problem i found out that Y+ max value was 12.81 and Y+ min was 0 ----- Thus I guess now I need to coursen the grid - Can some one suggest me how and where I should coarsen it ? Any other suggestions will be great !

 March 31, 2004, 18:47 Re: grid adaptation for better convergence. #7 Otilia Guest   Posts: n/a You can either coarsen the mesh (and use standard wall treatment) or refine the mesh (and use enhanced wall treatment). Second option is the most sensible!!! I do not think you have to mess around with underrelaxation too much. I am pretty sure that the unsteady phenomena do not let you converge the solution in steady-state. Have you tried a transient simulation. It is very likely that a transient simulation will solve your problem!! If there are transient phenomena you will never fully converge your steady-state simulation.

 March 31, 2004, 21:52 Re: grid adaptation for better convergence. #8 co2 Guest   Posts: n/a thank you very much to everyone for your good answers! your input is certainly helping me to make improvements to my model. I am about to finalize my grid - I am getting good convergence and realistic values from my steady state model. In the transient case, I will incorporate changing ambient temperature, changing conv. heat transfer coeff at tank walls using profile files, I will simulate the effect of revolving sun and changing sun radiation heat flux through a udf .. I am thinking of allowing large number of iterations per time step so that my solution coverges sufficiently at each time step .. WHAT WILL BE YOUR RECOMMENDATION ON THE NUMBER OF ITERATIONS THAT I SHOULD BE ALLOWING PER TIME STEP? thanks, CO2

 April 1, 2004, 19:06 Re: grid adaptation for better convergence. #9 Otilia Guest   Posts: n/a You can not use a huge time step and wait for hundreds of iteration to converge it. What you have to do is to choose a time-step size so that you converge the solution in no more than 40 steps.

 April 2, 2004, 15:08 Re: grid adaptation for better convergence. #10 co2 Guest   Posts: n/a well, I am taking a time step of 30 minutes since my radiation data, ambient temp data, wind velocity data is for every hour. Even if I break down times steps further, I guess BC's are going to remain constant - THEN WHAT IS THE POINT IN FURTHER REDUCING TIME STEP SIZE - I WAS THINKING I CAN EVEN HAVE A TIME STEP OF 1 HOUR - WHAT DO YOU THINK? Well, I am giving a max of 200 iterations per time step. I am seeing that fluent does not require the whole 200 iterations, but I guess setting 200 iterations keeps me on the safter side - CORRECT ? WHY DO YOU SAY THAT ONLY 40 ITERATIONS SHOULD BE ALLOWED ? WHAT IS SO WRONG IF THE RESIDUALS GO LOWER AND LOWER EVERY TIME STEP ?

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post David FLUENT 5 March 25, 2022 04:33 bohis FLUENT 0 January 16, 2009 04:00 Craig FLUENT 1 July 16, 2008 00:24 Christopher Haugh Main CFD Forum 2 March 9, 2007 13:42 vipul jindal Main CFD Forum 2 August 31, 2004 06:22

All times are GMT -4. The time now is 11:27.

 Contact Us - CFD Online - Privacy Statement - Top