hi All,

I am modeling an incompressible, turbulent flow in a closed vessel. As the flow velocities are small, I am using RNG K-Eps model. For covergence I am monitoring the residuals and a surface integral on the outlet. My question is: I am using the default values in fluent(0.001) for the residuals. And the residuals are not reaching 0.001, but they are decreasing constantly till 0.01 and then there is no significant change. is the solution converged??? or not???

Thanks in advance

If fluent not mentioned that the solution is converged so it not converage and it appeared so if not reach the limit 0.001.

Thanks for the response.

I am monitoring a surface integral which is stable after 200 iterations without any change. Isn't this shows the solution is converged???

Hi Madhukar,

A couple of different things can cause your residuals to level off before truly converging.

1) You may need to change the values of your under-relaxation factors, accessible through Fluent's menus. There is a section in the Fluent manual which describes this well.

2) You may not have a steady state solution. If you are using a steady-state turbulent solver, you may reach a state of pseudo-steadiness, or you may not; it might be better to use a transient solver. You can then analyze an instantaneous or time-averaged solution.

Hope this helps, Amit

Amit what about my case I am already use transient but the residual for vof to the secondary phase not appear for me until the final time step and Fluent not plot for me any results for it ? Can you tell me the reason for this?

K. Baker

This is one of the best questions that anybody has posed in a while. As you've seen, it is sometimes not simple to declare convergence. Something that may help get the residuals down more, is to switch to double precision, and tweaking relaxation parameters may also help. Also, you need to consider the differencing scheme that you are using, and how accurate your initial flow field was. Something that sometimes helps is to get 0.0001 convergence on first order upwind differencing first, and then switch to higher order to see what it does. With external flows, where the initial flow field is normally a very good solution everywhere except near the body, it may also be difficult to get the requisite 0.001 convergence. For other flows 0.001 may not even be good enough. Take a very good look at how your surface integral changes with more iterations, sometimes if you really zoom in (in terms of y-axis scale), you can readily identify a damped oscillation, which is a good indication that you are "straddling" a converged answer. As last resort (or maybe that should be first?), work on your grid quality. If you have a number of skew or very high aspect ratio cells, perhaps away from your surface of interest, it may not affect your surface integral, but could affect the residuals.

Hey Charles,

Thanks for the detailed response. as u said, the surface integral that i am using to monitor the convergence is steady...i mean damped oscillation. I think this shows my solution is converged...right??

once again thanks

Let's call it a necessary but not sufficient condition Generally though, it is a really good indication. A measure I have used to judge convergence has been to get the amplitude of the oscillation of the surface integral down to about 0.25% of its average value.