CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

grid adaptation for better convergence.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 30, 2004, 16:08
Default 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?

  Reply With Quote

Old   March 30, 2004, 18:01
Default 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.
  Reply With Quote

Old   March 30, 2004, 20:39
Default 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
  Reply With Quote

Old   March 31, 2004, 01:54
Default Re: grid adaptation for better convergence.
  #4
Alamgir
Guest
 
Posts: n/a
To adapt the grid you use velocity or pressure bc.

Alamgir
  Reply With Quote

Old   March 31, 2004, 05:22
Default 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.
  Reply With Quote

Old   March 31, 2004, 10:12
Default 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 !

  Reply With Quote

Old   March 31, 2004, 17:47
Default 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.
  Reply With Quote

Old   March 31, 2004, 20:52
Default 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
  Reply With Quote

Old   April 1, 2004, 18:06
Default 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.
  Reply With Quote

Old   April 2, 2004, 14:08
Default 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 ?

  Reply With Quote

Reply

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
grid partition AND dynamic mesh adaptation !!!!!!! bohis FLUENT 0 January 16, 2009 04:00
Multiple Dynamic Grid Adaptation Craig FLUENT 1 July 15, 2008 23:24
Relative Error in Grid Convergence Christopher Haugh Main CFD Forum 2 March 9, 2007 13:42
On grid independent solution for pulsatile flow David FLUENT 4 June 8, 2005 16:20
Dynamic grid adaptation vipul jindal Main CFD Forum 2 August 31, 2004 05:22


All times are GMT -4. The time now is 05:08.