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

Iterations Querry

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 14, 2010, 05:07
Default Iterations Querry
  #1
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Hello

I ran simulation for 600 iterations and I got converged solution but the results were not accurate/expected. Then i reduced the relaxation factors and did iterations for 2000 until the results converged. In the later case I got accurate/expected results. Can anybody tell the reason why i got the accurate results in higher iteration's case even though the convergence criteria was achieved for both cases.

I wil be grateful for you kind response.

Mohsin
South Korea
Mohsin is offline   Reply With Quote

Old   July 14, 2010, 13:44
Default
  #2
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 8
Chris D is on a distinguished road
I would say that your calculation wasn't really converged after 600 iterations. Under-relaxation should not influence the final solution.
Chris D is offline   Reply With Quote

Old   July 15, 2010, 00:59
Default
  #3
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Thank you Chris

You are right. But how can one know that his solution is not converged until 600 iterations. and now i am getting converged solution after 2000 iterations How can i beleive this is the right converged solution. Is there any procedure for determining the correct number of iterations for a problem?

I'll be glad for your response.

mohsin
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 01:03
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
Monitor a quantity such force, mass flow or pressure average on a face.
Convergence occures if you get a flat monitoring (no more fluctuation while iterating).
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 15, 2010, 02:02
Default
  #5
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Max Thank you for your reply.

You mean to say that I should create a "surface monitor" for my outlet? for example I should create a surface monitor which will report Pressure-static pressure at the outlet. With report type as "integral" and If i see a straight line It would mean that the result is converged and no need for further iteration.

Is this what you were referring to?
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 02:56
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
yes.
I wouldn't target any convergence criterion about residuals. Just let iterate, but break the caculations as you target monitoring doesn't fluctuate anymore.
I would also monitor the massflow on your inlet if you are working with drop pressure or the area weighted average of inlet pressure at inlet if you are working with velocity (massflow)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 15, 2010, 03:01
Default
  #7
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Max Thank you.

In "Define surface monitor" panel with report type as "integral" under the "surfaces" when i select one surface (example;outlet surface) it gives me flat line but if i select all the surfaces (except default interior) it gives me tiltled line and its not converged until even 3500 iterations.

What does it mean? For convergence whether i have to get flat lines for all the surfaces or just when only one surface (for example; Outlet surface) gives flat line it means the solution is converged.

Please clarify.
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 03:13
Default
  #8
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Actually i have 6 outlet surfaces. on 3 outlet surfaces for "pressure" and "report type" as integral I am getting flat line but for the other 3 outlets I am not getting the flat line.

Any suggestions for determining convergence in this case? Thank you
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 04:07
Default
  #9
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
choose Area weighted average instead of Intergral, and choose inlet.
What kind of BC did you set at inlet?
If you choose outlet, I assume you gave a constant pressure at your outlet, so it is already converged since you enforce the outlet having this value (eg: won't be computed)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 15, 2010, 04:14
Default
  #10
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
The inlet boundary condition is "velocity inlet" the outlet boundary condition is " Pressure outlet". and I gave the constant outlet pressure "0" at a constant operating pressure of 7Mpa.
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 04:22
Default
  #11
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Yes Max I got your point. As i gave the pressure outlet condition at the outlet so it will give me straight line coz i have enforced it to be a constant value. So for outlet I need to check for the flat line of "velocity" not "pressure". And for inlet I shouldnot check for velocity (as my inlet is velocity inlet) rather i should check for the flat line of pressure.

whether i have to check for all the surfaces for convergence?and in the meanwhile if the K and Epsilon drops below 10^-3 residual level (like 10^-2). Would it be ok?(aCTUALLY I am not getting the flat line for pressure at the inlet of my geometry in any case even after 3500 iterations).

Thanks
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 05:36
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
no, check only the pressure at your inlet
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 15, 2010, 05:46
Default
  #13
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Mr Max thank you for your time.

Can you please explain why I should only check for pressure at the inlet and leave the rest. And whether my target for convergence would only be to make the inlet Pressure as a flat line?

The other criteria for convergence is:

"You can examine the overall mass, momentum, energy and scalar balances in the Flux Reports panel. The net imbalance should be less than 0.2% of the net flux through the domain when the solution has converged" In my case it is always less than 0.2 percent.
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 06:09
Default
  #14
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Actually the convergence criteria of residuals and mass flux is acheived but when i look for surface monitors for inlet pressure, I cant get the flat line. what might be the problem? any suggestions?
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 06:57
Default
  #15
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
Quote:
Originally Posted by Mohsin View Post
Can you please explain why I should only check for pressure at the inlet and leave the rest. And whether my target for convergence would only be to make the inlet Pressure as a flat line?
If your interest is force on a body, you could also monitor the force vs iteration.
In your case you gave the massflow, and fluent should compute the pressure distribution on your domain. Since you fixed the outlet, then the inlet pressure should be adjusted (convergence).
you can also check the pressure distribution on another surface, but it makes only sense, if the surface should have a constant pressure
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 15, 2010, 08:19
Default
  #16
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
you can also check the pressure distribution on another surface, but it makes only sense, if the surface should have a constant pressure
Max I didn't understand your quoted sentence?

It make only sense if the surface should have a constant pressure? Thank you Max
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 08:26
Default
  #17
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
yes.
For instance, if you compute pressure distribution in a straight pipe, you can take the average pressure on the inlet cap or the outlet cap.
but if you take the average pressure on the covering surface (where you have a linear pressure's gradient), then it makes no sense...
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 15, 2010, 12:05
Default
  #18
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Thank you Max for your help.

I wanted to ask one thing about Surface monitors.

I did simulation and surface monitors gave flat lines for inlets. Report of "pressure" and Reprt type was "area weighted Average". But when i saved it and again ran after closing it (coz i wanted to do more iterations) then the line of surface monitor was not straight. Can you tell me the reason?
Mohsin is offline   Reply With Quote

Old   July 15, 2010, 12:35
Default
  #19
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 8
Chris D is on a distinguished road
If you didn't save the convergence history of the monitor, then the plot resets when you restart fluent. If the monitor was already converged, it might look like it is fluctuating wildly when you continue iterating, but it's really just oscillating with a very small amplitude. You'll never get a value that is exactly constant due to round-off errors, and the only reason it looked like a flat line previously is because the scale on the plot was larger.
Chris D is offline   Reply With Quote

Old   July 15, 2010, 12:39
Default
  #20
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
oh ok. Thank you very much Chris. So kind of you.
Mohsin 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
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
Floating point exception error Alan OpenFOAM Running, Solving & CFD 10 April 6, 2012 14:02
Computational time sunnysun OpenFOAM Running, Solving & CFD 5 March 16, 2009 04:32
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 11:16
Unknown error sivakumar OpenFOAM Pre-Processing 9 September 9, 2008 12:53


All times are GMT -4. The time now is 12:46.