Iterations Querry
Hello
I ran simulation for 600 iterations and I got converged solution but the results were not accurate/expected. Then i reduced the relaxation factors and did iterations for 2000 until the results converged. In the later case I got accurate/expected results. Can anybody tell the reason why i got the accurate results in higher iteration's case even though the convergence criteria was achieved for both cases. I wil be grateful for you kind response. Mohsin South Korea 
I would say that your calculation wasn't really converged after 600 iterations. Underrelaxation should not influence the final solution.

Thank you Chris
You are right. But how can one know that his solution is not converged until 600 iterations. and now i am getting converged solution after 2000 iterations How can i beleive this is the right converged solution. Is there any procedure for determining the correct number of iterations for a problem? I'll be glad for your response. mohsin 
Monitor a quantity such force, mass flow or pressure average on a face.
Convergence occures if you get a flat monitoring (no more fluctuation while iterating). 
Max Thank you for your reply.
You mean to say that I should create a "surface monitor" for my outlet? for example I should create a surface monitor which will report Pressurestatic pressure at the outlet. With report type as "integral" and If i see a straight line It would mean that the result is converged and no need for further iteration. Is this what you were referring to? 
yes.
I wouldn't target any convergence criterion about residuals. Just let iterate, but break the caculations as you target monitoring doesn't fluctuate anymore. I would also monitor the massflow on your inlet if you are working with drop pressure or the area weighted average of inlet pressure at inlet if you are working with velocity (massflow) 
Max Thank you.
In "Define surface monitor" panel with report type as "integral" under the "surfaces" when i select one surface (example;outlet surface) it gives me flat line but if i select all the surfaces (except default interior) it gives me tiltled line and its not converged until even 3500 iterations. What does it mean? For convergence whether i have to get flat lines for all the surfaces or just when only one surface (for example; Outlet surface) gives flat line it means the solution is converged. Please clarify. 
Actually i have 6 outlet surfaces. on 3 outlet surfaces for "pressure" and "report type" as integral I am getting flat line but for the other 3 outlets I am not getting the flat line.
Any suggestions for determining convergence in this case? Thank you 
choose Area weighted average instead of Intergral, and choose inlet.
What kind of BC did you set at inlet? If you choose outlet, I assume you gave a constant pressure at your outlet, so it is already converged since you enforce the outlet having this value (eg: won't be computed) 
The inlet boundary condition is "velocity inlet" the outlet boundary condition is " Pressure outlet". and I gave the constant outlet pressure "0" at a constant operating pressure of 7Mpa.

Yes Max I got your point. As i gave the pressure outlet condition at the outlet so it will give me straight line coz i have enforced it to be a constant value. So for outlet I need to check for the flat line of "velocity" not "pressure". And for inlet I shouldnot check for velocity (as my inlet is velocity inlet) rather i should check for the flat line of pressure.
whether i have to check for all the surfaces for convergence?and in the meanwhile if the K and Epsilon drops below 10^3 residual level (like 10^2). Would it be ok?(aCTUALLY I am not getting the flat line for pressure at the inlet of my geometry in any case even after 3500 iterations). Thanks 
no, check only the pressure at your inlet

Mr Max thank you for your time.
Can you please explain why I should only check for pressure at the inlet and leave the rest. And whether my target for convergence would only be to make the inlet Pressure as a flat line? The other criteria for convergence is: "You can examine the overall mass, momentum, energy and scalar balances in the Flux Reports panel. The net imbalance should be less than 0.2% of the net flux through the domain when the solution has converged" In my case it is always less than 0.2 percent. 
Actually the convergence criteria of residuals and mass flux is acheived but when i look for surface monitors for inlet pressure, I cant get the flat line. what might be the problem? any suggestions?

Quote:
In your case you gave the massflow, and fluent should compute the pressure distribution on your domain. Since you fixed the outlet, then the inlet pressure should be adjusted (convergence). you can also check the pressure distribution on another surface, but it makes only sense, if the surface should have a constant pressure 
Quote:
It make only sense if the surface should have a constant pressure? Thank you Max 
yes.
For instance, if you compute pressure distribution in a straight pipe, you can take the average pressure on the inlet cap or the outlet cap. but if you take the average pressure on the covering surface (where you have a linear pressure's gradient), then it makes no sense... 
Thank you Max for your help.
I wanted to ask one thing about Surface monitors. I did simulation and surface monitors gave flat lines for inlets. Report of "pressure" and Reprt type was "area weighted Average". But when i saved it and again ran after closing it (coz i wanted to do more iterations) then the line of surface monitor was not straight. Can you tell me the reason? 
If you didn't save the convergence history of the monitor, then the plot resets when you restart fluent. If the monitor was already converged, it might look like it is fluctuating wildly when you continue iterating, but it's really just oscillating with a very small amplitude. You'll never get a value that is exactly constant due to roundoff errors, and the only reason it looked like a flat line previously is because the scale on the plot was larger.

oh ok. Thank you very much Chris. So kind of you.

All times are GMT 4. The time now is 04:05. 