# Check the convergence of the transient run--> HOW ??!!

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

 February 13, 2012, 02:10 Check the convergence of the transient run--> HOW ??!! #1 Senior Member   mohammad Join Date: Dec 2010 Location: Seoul, South korea Posts: 214 Rep Power: 8 Dear all, I am solving a 3D transient airfoil( with a synthetic jet) with DES turbulence model. I want to know answers for the following questions: 1- How can i know the convergence level due to "coefficient loop"? In an other word, how can i know if the number of "inner loops" per iteraion is enough or not? 2-The "synthetic jet" problem is a secondary flow added to the main flow. This injected flow is " a Sinusoidal" flow. Thus, the value of lift on the blade is varying from timestep to timestep. Thus I want to know how can I understand the convergence for my case. what paramaeters should I use to realize whether my results are converged or not?? Regards, `

 February 13, 2012, 05:35 #2 Senior Member   Join Date: Jul 2011 Location: Berlin, Germany Posts: 165 Rep Power: 7 Hi Mohammad. for your first question here the attempt of an answer. First we certainly agree, that the convergence criteria must be set by yourself and that it is much more a matter of experience or just guessing, as the convergence criteria vary for all problems. I asked the same question to a guy from the cfx support and the answer was: "Usually your case should converge within 10 Iterations. If it does not reach the convergence criterion then there is something wrong. either bad mesh quality, wrong time step etc. If you don't manage to get convergence in 10 iterations then you could try and increase the number of iteration loops (to 20 or more) and see how many are needed to reach convergence. If it never reaches convergence then you definitely should check your case setup." As I understood the guy, the problem can be only a few "bad" grid cells that could prevent reching convergence although the relevant region of the case is solved correctly. Hope this is some kind of helpful to you. Unfortunately there is no "overall" convergence criterion in simulations. It is to check from case to case... Concerning your second question: I can not give you an advice which value to check. You should try to figure out which value would have to become constant during your calculation and then monitor it to see if further computation is needed or the stationary solution reached... One Value I began to monitor after having a CFX course about how to garantuee the quality of the simulations is valid for cases where I have clear In and Outlet. Then you could monitor the pressure difference between in and outlet: areaAve(Pressure)@Inlet-areaAve(Pressure)@Outlet When it becomes constant and parallely your case is converging to the desired RMS or MAX values then you probably will have reached a satisfying solution state. This worked quite fine for (some of) my cases...gas dispersion around buidlings.... Hope this is of some help for you.

February 13, 2012, 06:04
#3
Senior Member

Join Date: Dec 2010
Location: Seoul, South korea
Posts: 214
Rep Power: 8
Quote:
 Originally Posted by monkey1 1)) I asked the same question to a guy from the cfx support and the answer was: "Usually your case should converge within 10 Iterations. 2)) You should try to figure out which value would have to become constant during your calculation and then monitor it to see if further computation is needed or the stationary solution reached... 3)) If you don't manage to get convergence in 10 iterations then you could try and increase the number of iteration loops (to 20 or more) and see how many are needed to reach convergence. .

Hi monkey1, thanks for you thorough answer.

In the above quote:
1-By Saying " 10" , you mean 10 inner iterations, don't you?
2- For my case as I have told , the results would have to be kind of "sinusoidal" responses. So, it i am thinking be cause all the values will be changed from time to time, which values can I compare.???
3- AND THIS QUESTION PLEASE......think that i run my model with coefficient loops=15 ( inner loops) . My question is HOW CAN I MONITOR THE RESULTS of inner loops, to see whether the results are converged within any single timestep( outer iteration) or not. Actually as I can monitor the results of different time steps, I also want to monitor the results of inner loops in any iteration. If they are not converged I can increase the inner loops from 15 to a higher number.

Thanks a lot.

February 13, 2012, 06:16
#4
Senior Member

Lance
Join Date: Mar 2009
Posts: 598
Rep Power: 12
Quote:
 Originally Posted by mohammad My question is HOW CAN I MONITOR THE RESULTS of inner loops, to see whether the results are converged within any single timestep( outer iteration) or not.
Output control/Monitor/ and check "Monitor Coefficient Loop Convergence".
Then you will see how your monitor points converge within each time step.

 February 13, 2012, 06:17 #5 Senior Member   mohammad Join Date: Dec 2010 Location: Seoul, South korea Posts: 214 Rep Power: 8 Thank you Lance

 Tags transient convergence

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post andrea.pasquali OpenFOAM 1 March 16, 2011 06:24 PETE CD-adapco 0 February 17, 2006 12:26 Kevin CD-adapco 5 August 3, 2005 07:35 RK CFX 2 April 6, 2005 09:54 Mark Main CFD Forum 4 April 21, 2004 10:12

All times are GMT -4. The time now is 16:55.