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

Continuity Residual

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 4, 2005, 12:29
Default Continuity Residual
  #1
Joung Ae
Guest
 
Posts: n/a
What do i have to change if the continuity residuals don't decrease?
  Reply With Quote

Old   October 4, 2005, 22:57
Default Re: Continuity Residual
  #2
KHAN
Guest
 
Posts: n/a
Hi even i have the same problem, the residual is not at all decreasing, i guess this is becose the boundary conditions are not properly set up. if u able to figure it out let me know ok. thanks

  Reply With Quote

Old   October 5, 2005, 10:28
Default Re: Continuity Residual
  #3
Jason
Guest
 
Posts: n/a
There have been many discussions on this. There are many possible ways of "fixing" this, including a better mesh, using the dp solver (fluent 3ddp or fluent 2ddp) or fixing your boundary conditions, but there may be nothing to fix... you model may be converged even if you're not dropping a full 3 orders of magnitude. You have to be careful because the residuals are scaled based on your initial guess, so if your initial guess is close, then your residuals may not drop as much (this usually shows up in the continuity residual for segregated solver, and will show up for everything but turbulence residuals if using the coupled solver). You should be using monitors to judge your convergence, not just the residuals. The residuals are good for telling you how your model is behaving, and you should use them as a guide to judge convergence (increasing residuals is bad, you either want extrememly small residuals, or you want them to level off... leveling off can be a sign of convergence as well and that goes back to the fact that the residuals are scaled), but you should be monitoring whatever it is you're trying to get out of the model. For example, if in the end you're going to be reporting forces, then monitor the forces to make sure they are really converged. You should be doing this no matter what the residuals are doing. I've seen the residuals drop 6 orders of magnitude, but the forces continued to drift. IMHO, Fluent shouldn't be set up to judge convergence based on residuals, it should be set up to judge convergence based on monitor criteria that you define, because each model is unique.

If you search the forum for "continuity residuals" or "convergence" you should come up with some more in-depth conversations on the topic.

Hope this helps, and good luck, Jason
  Reply With Quote

Old   October 5, 2005, 14:51
Default Re: Continuity Residual
  #4
Mick
Guest
 
Posts: n/a
Hello Jason,

Many thanks for the comprehensive explanation. I was wondering if you can suggest a solution to what I think is a problem.

Well, I am monitoring drag and lift during the analysis, it takes about 9000 iterations to converge. Is it normal?

It is a 2D analysis, I have used the segregated solver.

Thanks in advance.

Mick
  Reply With Quote

Old   October 5, 2005, 23:46
Default Re: Continuity Residual
  #5
ztdep
Guest
 
Posts: n/a
i have experienced 20000 iterations to converge.
  Reply With Quote

Old   October 6, 2005, 04:34
Default Re: Continuity Residual
  #6
Mick
Guest
 
Posts: n/a
Cheers mate, thats fine! Well, some literature mentioned about their designs taking only 2000 to converge, thats why I was like why whats wrong with me here!

Thanks once again.

Mick
  Reply With Quote

Old   October 6, 2005, 10:22
Default Re: Continuity Residual
  #7
RoM
Guest
 
Posts: n/a
I think there is nothing wrong with your models. I usually need at least 5000 iterations to get convergeance. And for all those models presented in literature, they all run very stable, dont need much iterations and always produce best results which will fit with experimental values almost 100%, hmmm...

RoM
  Reply With Quote

Old   October 6, 2005, 10:39
Default Re: Continuity Residual
  #8
Jason
Guest
 
Posts: n/a
For a 2D airfoil, 2 to 3 thousand iterations is pretty common. It depends on the model setup: your mesh, BCs, solver choice, turublence model, etc... A coupled solver generally solves in fewer iterations than a segregated solver if you're in the compressible regime (Mach > 0.3 or so) and don't have a large separation region, but takes more memory and longer to complete a single iteration... for a 2D model, your mesh size is generally small enough where you won't notice much of a difference though. It also depends on what level of convergence you're looking for... if you're shooting for 2 significant figures, then that's going to take many less iterations than 4 sig figs. If you don't mind sharing, what are you analyzing (type of airfoil, airspeed, angle of attack, BCs, turbulence model, y+ values)? Maybe someone can make some suggestions that will help you cut down your time to convergence.

Jason
  Reply With Quote

Old   October 7, 2005, 01:43
Default Re: Continuity Residual
  #9
Mick
Guest
 
Posts: n/a
Hello Jason,

Sure no problems, its a twin element aerofoil and I am optimising it for downforce. Its a custom made aerofoil, and the airspeed is 55 km/hr. I am using the S-A turbulence model and the Y+ range from 30 to 65 approx. which is right I guess!

The tubulence intensity at the inlet is 0.2% and the turbulent length scale is about 0.1m.

If you want to know some ting else then please let me know.

Many Thanks,

Mick
  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 16:33
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 06:24
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM 6 April 12, 2011 12:24
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 12:16
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


All times are GMT -4. The time now is 16:31.