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

Bad convergence

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   August 24, 2013, 12:24
Post Bad convergence
  #1
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
Hi friends.
I use ANSYS CFX.I have a serious problem in converging. Mesh quality is good:
Orthogonality Angle:36.9 ok
Expansion Factor: 13 ok
Aspect Ratio: 8 OK
My model has very large size.(Tunnel with diameter 8 m and length 100 m )
I use teta mesh.Also I use k-e model with free surface flow(standard).
By the way, y plus in my simulation is 100,000! I can reduce this to 8000 with inflation and I can not reduce this any way. Is there any relation between slow convergence and y plus?
After two step, error 1 appears whereas any F in monitor. (All of them are ok!)
I reduced timescale factor to .1 but convergence become very slow!
Is there any solution for this problem?
Best regards
ali
ali92 is offline   Reply With Quote

Old   August 25, 2013, 19:28
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You cannot say mesh quality is good simply by quoting the OK/ok/! factors. This is case dependant and some simulations are MUCH more sensitive to mesh quality than others. The output file is just a guide.

If the tunnel is 8x100 metres, how big is the object inside it you are modelling? Are you using double precision numerics?

This sounds like an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   August 26, 2013, 07:36
Lightbulb
  #3
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
Thanks for your response ghorrocks.
I asked my problems before and you answer my questions kindly.
Problem in Result in bottom outlet

I used double precision but my result did not changed.

I run this model in transient state last night and saw surprisingly it is converged well. (After 100 time step RMS is 1e-5)
My important parameters particularly vent air velocity is logical and constant.
I your opinion my mistake had been steady state?

Total time:10s
Time step:.001s
So number of time step is 10000!
I have to wait 25 day for finishing this time. In time step 200 I stopped solver and checked my simulation but there is still no water in the tunnel. After which time step I can stop this simulation and Compare with physical model?

Thanks in advance.
ali
ali92 is offline   Reply With Quote

Old   August 26, 2013, 07:43
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It is quite possible your flow is transient so steady state was never going to converge. This is quite common, especially with bluff bodies or jet flows (you have both).

If you do not care about the time evolution of the flow and only care about the pseudo-steady state result then do not worry too much about tight convergence in the time steps, just run lots of time steps to get to what might be a psuedo-steady state, then tighten the convergence to get you answer.

If you care about the time evolution then you need to do a convergence critereon sensitivity study to correctly set your convergence critereon.

And I recommend you use adaptive time stepping, homing in on 3-5 coeff loops per iteration, with max and min time step sizes wide enough that you never reach them.
ghorrocks is offline   Reply With Quote

Old   August 26, 2013, 12:06
Post
  #5
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
Thanks alot. But one question:
MAX residuals are 100 times larger RMS residuals! What do you think? Is it a problem?
Attached Images
File Type: jpg MAX.jpg (70.6 KB, 13 views)
File Type: jpg RMS.jpg (69.6 KB, 11 views)
File Type: jpg air velocity.jpg (63.2 KB, 10 views)
File Type: jpg imbalance.jpg (62.3 KB, 8 views)
ali92 is offline   Reply With Quote

Old   August 26, 2013, 18:20
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Probably not a problem.

You are not using adaptive time stepping - you should.
ghorrocks is offline   Reply With Quote

Old   August 27, 2013, 06:49
Post
  #7
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
I am using adaptive time stepping, this way convergence is improved, but I think there is a oscillation behavior. Is it right? Is this behavior a problem?
Inlet data are as follow:
Total time: 5 s
initial time step: .005 s
max time step: .01
min time step: .00001
max coeff loops per iteration: 3
In follow you can see convergence monitor.

With regards
ali
ali92 is offline   Reply With Quote

Old   August 27, 2013, 06:53
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Make sure you never reach the min and max time steps. Also make the max coeff loops per iteration 10.
ali92 likes this.
ghorrocks is offline   Reply With Quote

Old   August 27, 2013, 06:54
Post
  #9
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
Sorry.I forgot put picture:
Attached Images
File Type: jpg air velocity1.jpg (60.9 KB, 7 views)
File Type: jpg RMS1.jpg (69.1 KB, 6 views)
ali92 is offline   Reply With Quote

Old   August 27, 2013, 06:58
Default
  #10
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
How can I check this?

I think I make a mistake. I set 5 for max number of coeff loops in solver control, but set 3 for target max coeff loops in analyse type.
Which of these should be 10?
ali92 is offline   Reply With Quote

Old   August 27, 2013, 07:10
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you are using adaptive time stepping and it is not converging to your criteria then you probably set the limits too tight or put a maximum number of iterations on. As I said in my previous post I suspect you did all of these things.

And if the result is it does not reach steady state (as it appears this does not) then your simulation is not steady but transient so no wonder it did not converge. Run it for long enough that the periodic pattern is consistent, then look at the cycle. You can probably do a time average to get a representative single number, but you should check first.
ghorrocks is offline   Reply With Quote

Old   August 27, 2013, 07:41
Post
  #12
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
I think my solution in #5 which is indicated was correct. RMS 1e-5 is sufficient for me. In that solution air velocity was about 37 that was sensible(Of course this decrease gradually with time)whereas in this solution air velocity is about 10!
What do you think? Do you agree with me?
ali92 is offline   Reply With Quote

Old   August 27, 2013, 07:54
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
At this stage I would not trust any result you have posted so far. You have not shown either result is reliable.
ghorrocks is offline   Reply With Quote

Old   August 27, 2013, 15:18
Post
  #14
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
Dear Glenn
Thanks for your advice.

Unfortunately My time for this project is over. Transient sate take long time and I have to try various time step. But how can I make sure never reach the min and max time steps is my problem. In addition, I do not know what initial time step should be use.

In your opinion is there any way that I use steady state instead transient? Otherwise how can I reach appropriate response with at least possible time?

By the way, What do you mean by the following statement?
"If you are using adaptive time stepping and it is not converging to your criteria then you probably set the limits too tight or put a maximum number of iterations on."

Regards
ali
ali92 is offline   Reply With Quote

Old   August 27, 2013, 18:29
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Set the min to 1e-20 and the max to 1e20 and it will never reach them.

Work out the initial time step by doing an initial run and see what time step it settles on. Then do another simulation using that timestep as the initial time step.

If the flow is transient then there is no way of running it steady state.

Adaptive time stepping should adjust the time step to a value which converges to your tolerance. So in difficult to converge sections you get small time steps.
ghorrocks is offline   Reply With Quote

Old   August 28, 2013, 00:14
Post
  #16
Member
 
ali
Join Date: Jun 2013
Posts: 44
Rep Power: 4
ali92 is on a distinguished road
Thanks a lot for your good advice.
ali92 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 24 May 9, 2015 08:02
Bad convergence 2-way Syetem Coupling sirig Main CFD Forum 0 March 15, 2013 03:38
Force can not converge colopolo CFX 13 October 4, 2011 22:03
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
too bad convergence Davoche Main CFD Forum 2 November 20, 2005 06:08


All times are GMT -4. The time now is 07:13.