Hi CFX 5.7 users. I need some advice regarding slow convergence.

I am using the 2-fluid model, for 3D modelling of a bubble plume with air bubbles in water. I am getting rather slow convergence for a steady-state solution. The residual plots flatten out after approximately 200 iterations. This continues until at least 1000 iterations (I think modelling further is pointless)! There's only small spikes on the residual plot. Only the RMS-residuals for U-MOM(Air) and V-MOM(Air) falls below 1E-04. The rest of the residuals are above this convergence criterium. Especially the RMS residuals for the volume fractions are high (approx. 1E-2). I have used timesteps of both 0.1 and 1 sec.

The results of the simulation look as expected, with a well developed bubble plume. I just think that I should be able to get better convergence, in order to say that I have a well converged solution...

Does anyone have any solutions/has anyone experienced the same problem for 2 phase modelling?

Regards Jesper

Hi Jesper,

Slow convergence may be due to a number of things. A common mistake is to use too small a timescale. To determine an appropriate timescale create a streamline, starting from your inlet, in CFX-Post. You can then calculate the Length averaged Time on this streamline using the CFX-Post calculator. This value should be roughly half the advection timescale.

If the value you get is much larger or smaller than the timesteps you have used, try setting the Physical Timescale in the solver to this value.

Another reason for slow or poor convergence may be numerical instability. If this is the case, reducing your timestep by a factor of 10 should help. Generally, you should run for a while with a very large timestep before doing this to ensure you have passed through the start up transients.

Lastly, it is always possible that you model does not have a steady state solution. You can write out a series of backup files and view the changing flowfield to determine whether this is the case.

It also helps to isolate the non-converging regions. To do so, set the expert parameter "output eq flows=t" and write a backup or res file. You can then post-process the residual fields to see where the problem areas are. If the residuals are below your criteria in, say 90% of your model, and the non-converging regions are away from the region of interest, it may be safe to just stop the run and take the results as they are.

For more advice on selecting a timestep, go to http://www-waterloo.ansys.com/cfxcom...onvergence.htm.

Regards, Robin