- **FLUENT**
(*http://www.cfd-online.com/Forums/fluent/*)

- - **Problem with residuals, especially continuity**
(*http://www.cfd-online.com/Forums/fluent/81056-problem-residuals-especially-continuity.html*)

Problem with residuals, especially continuityHello everyone,
I'm solving a case with the steady SST k-omega scheme in Fluent 12.1 with a coupled solver with second order discretizations. The relaxation factors and Courant number values I use are lower than their default values. I also solve for the energy equation. The results I get are ok for my case; however I would like to get better convergence to be sure that the results are accurate. The continuity residuals reach a steady level of 10^-2, but I'd definitely like that to go down more. Because continuity residuals should easily reach a level of 10^-4 at least. Other residuals are better but none of them g lower than 10^-4. I tried to diagnose the problem and noticed one thing that was weird: The velocity, turbulent kinetic energy and specific dissipation rate profiles I inserted at the inlet are all correctly seen at the end of the run. But the turbulence intensity that corresponds to these is not; I get incredibly high turbulence intensity values. My mesh is very well defined, worked on it for quite a while so I don't think it's related to that. Any suggestions on how to decrease residual levels and improve convergence? Also a general question: Is it better to use a single scheme (coupled, simplec etc.) or start out with a simplec scheme for a couple hundred iterations than continue with coupled? Does that have an effect on residual levels? |

Same issues here...Hello Ozgur_,
This thread is quite old now, but since there were no replies I was wondering whether you solved your convergence issues because I am facing something very similar at the moment (but not solving density)... In your case I am quite surprised that having correct velocity and TKE profiles you then have wrong turbulence intensity! Could you throw more light into what happened at last? About switching the solver scheme I don't think that this should have a great impact, but in general a segregated solver takes more iterations to reach the same solution. The transport equations of your turbulence model could present better convergence with a segregated solver though, since they would be solved after and based on the results of momentum, continuity and energy equations. Changing the scheme is changing the algorithms that solve the PDE's; in principle you would change the rate of convergence of your problem but not its accuracy and final residuals. On the other hand coupled schemes are less sensitive to initial conditions and mesh quality, but they could perform bad in rotating machinery and complex geometry internal flows. For more information you might want to check the link below: http://www.ansys.com/staticassets/AN...Continuity.pdf Did you try to monitor that the mass flow out of your domain is balanced with the mass flow in? The residual monitor for a pressure-based solver is the sum of the imbalances in all the cells and for a density-based solver it is something like the rate of change of the variables with "time" (time=iteration for pseudo-transient steady simulation). Despite the continuity residual being large, say O(e-2), if your physical quantities monitored do show mass conservation you could deem your simulation converged (after all continuity would be satisfied in your whole domain). Lastly, my main concern would be that if the physics of the "real" flow cannot be coped by your models, the residuals would tend to be high. For example bad residuals could be due to forcing a steady solution in an inherently unsteady flow.Regards, MDB |

Hi,
have you tried to use the pseudo-transient formulation? In same cases it improves the convergence for steady state simulation. Andrea |

All times are GMT -4. The time now is 03:25. |