CFD Online Logo CFD Online URL
Home > Forums > CFX

Convergence Issues

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

LinkBack Thread Tools Display Modes
Old   November 12, 2010, 09:00
Default Convergence Issues
Senior Member
Join Date: Oct 2010
Posts: 302
Rep Power: 9
saisanthoshm88 is on a distinguished road
While working with a CFD problem, Iíve followed two different approaches in specifying a Pressure Boundary condition. In the first case Iíve set the Boundary pressure to 0 and the reference pressure to the Boundary absolute pressure (= 1 atm.) and in the second case Iíve done it the other way around.
For the purpose of having a mere observation of the convergence trend in both the cases, Iíve set a very loose residual target of 5.E-03 R.M.S. In the first case, the solution converged very quickly within two minutes and in 5 iterations. In the second case the solution wasnít converging even after 300 iterations so I stopped the run and by the time the run was stopped, the residuals were around 1.8E-02.
The convergence history in the first case was zigzag but in the second case it is almost a straight line. Attached images can throw a better illustration.

The following are the questions Iíve in relation to this description:

1. In spite of having high residuals, at around 1.8E-02 the post processed

results of the second case are found to be more accurate than those

of the first case with low residuals at around 5.E-03. what can be the

reason for this?

2. In specifying a pressure boundary condition what is the recommended

approach to follow, the first (or) the second please clarify upon this.

Attached Images
File Type: jpg Images_convergence.JPG (17.8 KB, 28 views)
Best regards,
saisanthoshm88 is offline   Reply With Quote

Old   November 12, 2010, 09:26
Join Date: Feb 2010
Location: Australia
Posts: 65
Rep Power: 7
RossFS is on a distinguished road
re: pressure being set in two different ways.
As far as I can tell these are identical setups so ought to give identical results?

re: convergence
How are you certain that your solution has converged? Just because you have met the residual target you have set does not mean that the solution has converged. For example, wall shear at a certain point might still be changing rapidly even though your RMS residuals are "converged". You have to check whether certain monitor point values are close to constant to get an idea as to whether your solution has converged or not.

In the second case where you can't get your residuals to do anything other than flat line, have you tried altering the time step of the simulation?
RossFS is offline   Reply With Quote

Old   November 12, 2010, 12:28
Senior Member
Join Date: Oct 2010
Posts: 302
Rep Power: 9
saisanthoshm88 is on a distinguished road
I didn't try such steps because I was working upon a electronics cooling problem which is indeed one of the ANSYS work shops so I already have the correct result for temperatures in the simulation from the presentation. I was only trying to do some simple experiments to understand the trends of convergence and more over I was saying that I ran the case 1 with residual target of 5.E-3 but later on when I ran it for a residual target of 1.E-04 everything went well and I got the results that exactly matched with those given in the presentation. My problem is not that I don't have accurate results. And in the second case with a flat trend of convergence, I also checked the domain imbalances and found them to be convincing . I was only asking that if it is reasonable to stop the run if a flat trend as seen in the second case is encountered.
Then if you say that both the approaches for specifying a pressure boundary condition do the same job then why is it that the convergence histories are that very different. When I ran the case 1 for a residual target of 1.E-4 I didn't see any flat trend it monotonically converged. I know that both the approaches serve the same purpose of setting up the desired absolute pressure at the boundary. I was asking a suggestion for a better approach so that there can be an ease in getting a good trend of convergence and in most of the tutorials I found that the first approach, i.e.., the approach of setting up a 0 pressure at the boundary and the Boundary absolute pressure as the reference pressure was recommended. I asked the question only to confirm upon that.
Best regards,
saisanthoshm88 is offline   Reply With Quote

Old   November 13, 2010, 05:34
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,053
Rep Power: 86
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This is very basic numerical methods. Simply when you set the reference pressure correctly (your first case) then the pressure is resolved more accurately by the numerical precision of the solver. For instance 100001 Pa abs and 100002 Pa abs is resolved as 1Pa rel and 2Pa rel, a factor of 2 different.

In the second case you are loosing precision because the difference between 100001 and 100002Pa is about 0.001% and this is challenge for any numerical system to accurately resolve.

Hence case 1 converges easily and case 2 converges slowly, if it converges at all.

If case 2 is more accurate than case 1 then that is just luck. You obviously have large errors in your analysis (even case 1) and should do a lot of work to improve accuracy.
ghorrocks is offline   Reply With Quote


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
Laminar Pipe Flow convergence issues preichl OpenFOAM Running, Solving & CFD 11 September 22, 2014 21:22
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
Grid size, convergence issues franzdrs Main CFD Forum 3 June 18, 2009 07:57
convergence issues (discontinuity mastered!) Matthew R FLUENT 0 October 12, 2006 03:55
RSTM convergence issues nazario Main CFD Forum 0 June 23, 2006 07:23

All times are GMT -4. The time now is 12:32.