
[Sponsors] 
November 12, 2010, 09:00 
Convergence Issues

#1 
Senior Member

Join Date: Oct 2010
Posts: 303
Rep Power: 9 
While working with a CFD problem, I’ve followed two different approaches in specifying a Pressure Boundary condition. In the first case I’ve set the Boundary pressure to 0 and the reference pressure to the Boundary absolute pressure (= 1 atm.) and in the second case I’ve done it the other way around.
For the purpose of having a mere observation of the convergence trend in both the cases, I’ve set a very loose residual target of 5.E03 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 wasn’t converging even after 300 iterations so I stopped the run and by the time the run was stopped, the residuals were around 1.8E02. 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 I’ve in relation to this description: 1. In spite of having high residuals, at around 1.8E02 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.E03. 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.
__________________
Best regards, Santhosh. 

November 12, 2010, 09:26 

#2 
Member
Join Date: Feb 2010
Location: Australia
Posts: 65
Rep Power: 8 
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? 

November 12, 2010, 12:28 

#3 
Senior Member

Join Date: Oct 2010
Posts: 303
Rep Power: 9 
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.E3 but later on when I ran it for a residual target of 1.E04 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.E4 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, Santhosh. 

November 13, 2010, 05:34 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,405
Rep Power: 97 
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. 

Thread Tools  
Display Modes  


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 