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

- - **Convergence Problem in Axisymmetric Periodic Flow**
(*https://www.cfd-online.com/Forums/fluent/129597-convergence-problem-axisymmetric-periodic-flow.html*)

Convergence Problem in Axisymmetric Periodic FlowHi everyone,
I am modelling a periodic flow for a 3D pipe, using an axisymmetric model. The flow is to be in the Z direction, with half-width (or radius) of 3 m. The Reynolds number is 34,132 and the working fluid is air. This gives my inlet velocity of 0.081 m/s. I set the turbulence intensity as 4.3% and turbulent length scale of 0.42. I have a problem, however, in obtaining convergence. My current convergence criterion is 1e-06 for all the variables. With the initialization values below: http://i59.tinypic.com/34hxg82.jpg My convergence plot is: http://i61.tinypic.com/2qxnrxi.png I have tried to run a full 3D pipe periodic flow as well. For my initial mesh, I managed to obtain convergence, however, as I refine it further (by increasing the bias factor from 10 to 20), now it won't converge. Not sure what's going on! So any comments/feedbacks will be greatly appreciated! Thanks so much in advance for your help! |

2D axisymmetric domains in fluent must have the x-axis as symmetry axis.
Additionally, for translational periodic flows with a very short streamwise extent, it is not unusual to take 10e5 or even more iterations to converge. 10e-6 for the residual values may still be too loose as a convergence criterion in this case. Make sure to double-check convergence with some other quantity like wall shear stress. |

Quote:
I've just tried it in xy plane and it converges now!! Thank you! I am not sure, however, how to 'double-check convergence' with other quantity like wall shear stress.. I'm still new to CFD so I would really appreciate it if you would share some guidelines/resources on this? :-) Many thanks!! |

The basic idea is that you should never judge convergence based on the value of some residuals alone.
They are a good indicator, but sooner or later you will run into trouble if you rely on them too much. The absolute minimum for a simulation like yours is to set up a monitor point to monitor the average wall shear stress at the pipe wall. These two links have lots of valuable information on this topic: http://www.cfd-online.com/Forums/flu...nvergence.html http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F |

All times are GMT -4. The time now is 01:18. |