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

Convergence Issue

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 21, 2011, 10:36
Default Convergence Issue
  #1
New Member
 
Join Date: Sep 2010
Posts: 28
Rep Power: 0
zephyrus17 is on a distinguished road
I'm doing a Steady State age of air validation case where air @ 25C enters a simple room through a square inlet and exits from an exit across the room. The air enters at 1.68m/s and the outlet is just a 0 Pa outlet. I'm monitoring the age of air and also monitoring the turbulence kinetic energy (is this the most suitable?) to judge convergence. I'm following the journal and using the standard k-e turbulence model with 14% turbulence intensity.

Here is the journal article for it: http://www.inive.org/members_area/me...%5CUFSC492.pdf

The coarse mesh would converge with no problems, however the fine mesh would not. The advection time is around 17 seconds. I tried setting the local timestep to 5, at first; tried playing with the physical timestep, varying from 200 down to 0.17 seconds. No matter what I did, the converge would drop swifty to 1e-3, then just bounce around there. The lowest I got it down to was around 8e-4.

There was nothing wrong with the mesh itself as it showed no issues in the solver .out file.

Any suggestions on what to do next or what I'm doing wrong?
zephyrus17 is offline   Reply With Quote

Old   August 22, 2011, 09:56
Default
  #2
Member
 
Join Date: Mar 2010
Posts: 42
Rep Power: 6
lindner is on a distinguished road
Hi,
You can check the values of y+ for the new mesh, it should be around 30 and 300 for the k-epsilon turbulent model.
Look at the streamlines and search for recirculation in the room, maybe you need to change to SST model to capture that right (and refine the mesh to have y+ around 1).

regards,
lindner
lindner is offline   Reply With Quote

Old   August 22, 2011, 10:07
Default
  #3
New Member
 
Join Date: Sep 2010
Posts: 28
Rep Power: 0
zephyrus17 is on a distinguished road
The y+ is at 111.7 at it's maximum. And sadly I can't change the turbulence model because I need to follow the journal article to validate it. And I can't change the mesh as well due to the same reasons.

So in other words, given the current situation, I can't change anything else other than the timestep, solver controls, etc to get it to converge down.
zephyrus17 is offline   Reply With Quote

Old   August 22, 2011, 10:19
Default
  #4
Member
 
Join Date: Mar 2010
Posts: 42
Rep Power: 6
lindner is on a distinguished road
Try using the Production Limiter Kato Launder on the Advanced Turbulence Control inside Fluid Models (right under Wall Function).
lindner is offline   Reply With Quote

Old   August 22, 2011, 10:35
Default
  #5
New Member
 
Join Date: Sep 2010
Posts: 28
Rep Power: 0
zephyrus17 is on a distinguished road
Doesn't work. It stopped the 'bouncing' of the converge around the 1e-3 mark and spread it out, which looks good, but it's risen to around 1.6e-3. And the bounces are now merely more spread out.
zephyrus17 is offline   Reply With Quote

Old   August 22, 2011, 12:37
Default
  #6
Member
 
Join Date: Mar 2010
Posts: 42
Rep Power: 6
lindner is on a distinguished road
Did you compare the results even with the non-converged solution? I did this Bartak case last year using OpenFOAM and got good results, but don't remember having issues with convergence. I will check my setup later and try to find something useful.
lindner is offline   Reply With Quote

Old   August 22, 2011, 18:30
Default
  #7
New Member
 
Join Date: Sep 2010
Posts: 28
Rep Power: 0
zephyrus17 is on a distinguished road
I did. The results are pretty much the same. The Age of Air monitoring point can be assumed to be stabilised. However, this is a pretty good case in study of how to get something to stabilise for me
zephyrus17 is offline   Reply With Quote

Old   August 24, 2011, 04:28
Default
  #8
New Member
 
Zhang Yang
Join Date: Jun 2011
Location: Zürich
Posts: 28
Rep Power: 6
swiss_zhang is on a distinguished road
Following Ideal:

1: How many iteration steps have you set? Increase the iteration step and try it.

2: use Adaptive Time Step
swiss_zhang is offline   Reply With Quote

Old   August 24, 2011, 06:24
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,444
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
There is a FAQ which will help here, and it goes into much more detail:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Note that divergence when going to finer meshes is very common. It usually means the reduced dissipation of the finer mesh is causing the flow to become transient. Try the tricks on the FAQ, and if that does not work you will have to run it transient.
ghorrocks is offline   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
Convergence Centurion2011 FLUENT 19 February 3, 2014 12:07
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
Convergence issue in SST for Porous model Raj CFX 0 May 2, 2008 02:43
CFX-Solver, issue with convergence behavior Andy CFX 7 September 5, 2006 03:24
Convergence issue with continuity equation Jake FLUENT 6 June 15, 2005 16:14


All times are GMT -4. The time now is 00:08.