Is this convergence real?
1 Attachment(s)
Hi,
I am performing a steady state simulation. At low Re, i am able to get convergence by using a small physical timescale of 1e4 s. At higher Re, I start the simulation with the same physical timescale. However, I have to progressively reduce the timescale to reduce the residuals. Please refer the attached figure for the behavior of the momentum residuals. I impose a convergence criteria of 1e6 and a conservation target of 0.1%. 1. With the physical timescale of 1e4 s, residuals stabilize and I reduce the timescale to 1e5 s. The residuals reduce but again stabilize at a lower level. 2. Then I gradually reduce the timescale to 1e9 s but it has no effect on the residuals. 3. On reduction of timescale further to 1e10 s and 1e11 s, the residuals reduce sharply (within 23 iterations of reduction of residuals each time) but again stabilize at lower level. 4. Finally, when I reduce the timescale to 1e12 s, residuals reduce sharply in the very next iteration to below the convergence criteria and the simulation stops giving the message that the convergence criteria and conservation targets have been met. These sudden reductions with residuals seem very unreal. Has the simulation actually converged or I am looking a numerical instability which is just fortuitously resulting in a somewhat false reduction of residuals? 
Probably a numerical round off thing. It is unusual that it reduces the residual, it normally increases it. Try using double precision numerics and see if the same thing happens.

Hi Glen,
I am using double precision numerics only. 
Glen,
This is the same problem that I discussed with you in the thread http://www.cfdonline.com/Forums/cfx...snumbers.html Following your recommendation, I had done transient simulation for this case and it evolved into steady state successfully. However, I was using a very fine mesh there. What I need is to get steady state solution using a steady state simulation. The transient simulation takes a lot of time. So I have made the mesh much coarser so as to avoid any local transient flow phenomena that I may be resolving in the very fine mesh. And I have used this coarse mesh in the simulation whose residuals I am displaying above in this thread. 
I see. In that case I suspect you just about got to the ultimate accuracy of your computer and simulation at 500 iterations, and are definitely there at 1000 iterations. The stuff beyond that is just numerical roundoff playing tricks and can be ignored.

But Can I regard it as a QUANTITATIVELY converged steady state solution ?
Because according to the CFX 12.1 manual, for RMS Residual Level : The Residual • Values larger than 1e4 may be sufﬁcient to obtain a qualitative understanding of the ﬂow ﬁeld. • 1e4 is relatively loose convergence, but may be sufﬁcient for many engineering applications. • 1e5 is good convergence, and usually sufﬁcient for most engineering applications. • 1e6 or lower is very tight convergence, and occasionally required for geometrically sensitive problems. 
As ever, the best way to determine this is with a sensitivity analysis. Choose an output parameter of interest to your simulation (pressure loss, heat loss, whatever but preferably something which is a single number) and plot it against different convergence residuals. When the parameter of interest to you has converged to within a tolerance you are happy with then you can define your convergence tolerance.

As Glenn said in his last post, try defining a variable to monitor, and looka t it if it is stable.
I had the same behaviour once, and it is not a good resiudal plot. If I were you, I would selec the Autotime scale, and there you will see if your phusical time scale is good.. Furthemore, you might have a numerical error, try to evaluate some parameter such as Courant and Reynolds. I do not think it is a transient problem, because when you have tranisent problem the behaviour is different, for example, when you change the Physical time scale you do not change your residual plot.... Good luck! 
Thanks Glen and juliom for ur replies..will check it

All times are GMT 4. The time now is 17:26. 