
[Sponsors] 
December 13, 2012, 08:33 
Convergence criteria

#1 
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 5 
Hi to all!
does anybody know how are the residuals defined in openFoam? Which kinds of residuals is it possible to use? And..is it possible to use as convergence criteria the values of a force coefficient (lift coefficient, drag coefficient)? Thanks in advance Simone 

December 14, 2012, 09:25 

#2 
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 5 
Does anyone have some idea?


December 14, 2012, 10:52 

#3 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 16 
Hi Simone, check appendix A of this paper:
http://www.cimec.org.ar/ojs/index.ph...File/3263/3186 Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar 

December 14, 2012, 17:13 

#4  
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 297
Rep Power: 14 
Quote:
With RANS however, there is no guaranty that if Cl or Cd stabilize at a certain value, the solution is converged as well. But if the solution is converged, you can be sure of the values for Cl and Cd being correct. Or said differently, you can't be sure that you have obtained the correct values for Cl and Cd as long as you don't check the residuals... 

December 17, 2012, 05:15 

#5 
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 5 
Dear Lieven, my situation is the following:
I've been running some simulations with prescribed convergence criteria for the residuals of U and p. I was actually almost sure that, when those criteria were reached, the coefficients would be stabilized as well, but they weren't. So, what I've done was running a simulation without convergence criteria (and for many more iterations than the previous simulations) and check when the force coefficients were stabilized by plotting them. Finally, what I'm doing now is running the simulations again for a prescribed number of iterations, that guarantees both the satisfaction of the residuals and of the coefficients. I only wanted to know if there was some way to automate all the process, and so I'll check the appendix suggested by santiago as soon as possible. Do you think my reasoning is correct? Cheers Simone 

December 17, 2012, 05:59 

#6  
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 297
Rep Power: 14 
Quote:
Quote:
What you could do is figure out the size of the residuals when you are fully converged. Then set the convergence criteria to a value 10x higher than the convergedresiduals (e.g. is the latter is 1e14, set it to 1e12 or 13. This won't make a lot of difference. Just don't think that if residuals drop 4 or 5 orders of magnitude that the solution is converged, this is in general simply not true (although this is what you read in manuals). You can still set a maximum number of iterations but if convergence is reached sooner, the simulation will stop earlier. Kind regards, L 

December 17, 2012, 07:06 

#7 
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 5 
Well Lieven thanks again for your reply.. What maybe I don't have underlined enough is that the stabilization of the coefficient needs a higher number of iterations than those requested from the simple "convergence of the residuals"; in this new situation the residuals are then far smaller then my "first" simulations when I didn't look at the stabilization of the coefficient.
with this clarification does my reasoning looks more correct for you? Thanks again Simone 

December 17, 2012, 07:45 

#8  
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 297
Rep Power: 14 
Quote:
Quote:
Quote:
Greetz, L 

February 5, 2015, 05:08 

#9 
New Member
Gareth
Join Date: Jun 2010
Posts: 29
Rep Power: 8 
Hi all
In a similar line of questioning, i am trying a 2d model of a foil in openFoam, steady state with a simpleFoam solver When i initially set my residuals, the tolerance was very high. And i set my iterations to a overly large value (>15000). What i noticed is that my Cl and Cd values leveled off fairly early, but the tolerance of my U and P meant the solver kept on running. No matter the number of iterations the U and P residuals would not drop. they also flattened out between 1e4 and 1e5 for U while P never dropped under 0.01. My question is then can i not calculate my Cl and Cd residuals and use that as a cut off value? Check out the residual plot and Cl and Cd plot in attachment Thanks Last edited by bullmut; February 5, 2015 at 05:14. Reason: addition of images 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Force can not converge  colopolo  CFX  13  October 4, 2011 22:03 
What value shall I set for the Convergence criteria?  steventay  CFX  7  May 14, 2010 12:44 
starccm+ convergence criteria  star  CDadapco  2  January 14, 2009 05:57 
Convergence Criteria  edwin  FLUENT  1  February 14, 2008 20:24 
Global Convergence Criteria  asaha  OpenFOAM Running, Solving & CFD  0  December 9, 2007 10:53 