# acceptable converging?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
January 16, 2016, 07:23
acceptable converging?
#1
Member

cglr
Join Date: Apr 2015
Posts: 31
Rep Power: 11
Hello,

My teacher said that to accomplish a good analysis, I should have a converging of 10^-6 for x,y,z velocities and energy. Is this true? I have a high quality structured mesh but could not reach that converging. The residuals are as shown. The results are sensible. Might these residuals be valid ?
Attached Images
 resu1.PNG (45.5 KB, 21 views)

 January 16, 2016, 07:38 #2 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 Your teacher is wrong. Residuals are indicative, but not conclusive. They provide a relative level of change. How far your residuals will pratically reduce depends on the geometry, on the parameter of interest, on the goodness of the initial guess, etcetera. I've seen cases where all residuals were 10^-3 and the problem was converged, and situations where all were 10^-6 but still the situation was significantly changing over the iterations. So, residuals indicate whether your solution is getting better or worse, but in themselves should not be used to judge convergence on. Better is to judge some physical parameters. For example, does the average velocity in the domain reach a constant value over the iterations. Does the average temperature (if you consider energy)? Does the torque of an impeller reach a steady value, etc., etc. Depending on the problem, you may tune your choice of indicators. For example, are you interested in a surface nusselt number, then check if this reaches a steady value over the iterations. What is good enough depends on your own preference, and on the situation. Typically, I'm satisfied when the parameter of interest stays within a 0.01% range over 1000 iterations, but it may depend on the situation. Havind said that, I have seen no situations where such parameters were sufficiently constant while the residuals were still around 10^-2. So although I can't say with certainty, I'd be surprised if your simulation was sufficiently converged here. wales likes this.

 January 16, 2016, 08:07 #3 Member   cglr Join Date: Apr 2015 Posts: 31 Rep Power: 11 Thank you for clarifying. But I cant understand why these residuals are going up and down steadily as seen. They never get a decisivness. So I cant get rid of my doubts. Could you kindly explain how to check a physical parameter over iterations in order for me to look at it the way you suggested. Im sorry Im limited in fluent. Thanks a lot.

 January 16, 2016, 09:00 #4 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 go to 'volume integrals', select the parameter you want to follow (i.e. velocity magnitude, x-vel, etc..) and click 'plot'. The value then will be tracked over the iterations, just like residuals. Also, you can export it to a text file (select write and add a path), so you can check whether or not any oscillations in the value are significant (although quite frequently this is obvious from the direct plot)

 January 16, 2016, 09:44 #5 Member   cglr Join Date: Apr 2015 Posts: 31 Rep Power: 11 Thanks a lot again, it looks as a reasonable approach and hope the parameters of interest stay constant after some iterations.

January 17, 2016, 04:17
#6
Member

cglr
Join Date: Apr 2015
Posts: 31
Rep Power: 11
Hi,

Unfortunately I cant reach a stability. What might be a possible factor? May the residual attached stay constant after more iterations ?
Attached Images
 plot.jpg (121.2 KB, 20 views)

 January 18, 2016, 09:35 #7 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 607 Rep Power: 0 Mesh quality can always be a problem; what did you mean with good quality mesh? Also, it may help to change your under-relaxation factors under solution controls. If you are making too big steps (too high factors) you may keep oscillating around a better solution without being able to reach it. Especially continuity tends to be quite sensitive, try reducing the under-relaxation for continuity to 0.1 or 0.2. You could choose to use lower order discretization schemes too, but these of course provide additional stability at the cost of extra diffusion.

 January 19, 2016, 02:34 #8 Member   cglr Join Date: Apr 2015 Posts: 31 Rep Power: 11 Ceesh, Thank you for your interest. Could you look over the thread in the following link if you are able to make time any time. It lays the problem out clearly I guess. http://www.cfd-online.com/Forums/flu...residuals.html

 January 19, 2016, 02:39 #9 Member   cglr Join Date: Apr 2015 Posts: 31 Rep Power: 11 min orthogonal guality is about 0.9 and aspect ratio is about 70

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post m zahid FLUENT 1 July 28, 2015 09:05 C.C Fluent UDF and Scheme Programming 0 October 9, 2013 11:11 lampe1234 STAR-CCM+ 0 September 15, 2013 15:43 Boon Ping , Oh Main CFD Forum 8 February 5, 2007 03:54 Boon Ping , Oh Siemens 2 February 2, 2007 10:17

All times are GMT -4. The time now is 02:03.

 Contact Us - CFD Online - Privacy Statement - Top