CFD Online Logo CFD Online URL
Home > Forums > CFX

Slow convergence

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Display Modes
Old   July 7, 2004, 03:41
Default Slow convergence
Posts: n/a
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
  Reply With Quote

Old   July 7, 2004, 16:59
Default Re: Slow convergence
Posts: n/a
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

Regards, Robin
  Reply With Quote


Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Convergence Centurion2011 FLUENT 24 May 9, 2015 08:02
slow convergence in chtMultiRegionSimpleFoam sven82 OpenFOAM Running, Solving & CFD 4 October 2, 2014 10:15
Force can not converge colopolo CFX 13 October 4, 2011 22:03
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
Slow convergence for Boundary Layer flow Biga Main CFD Forum 2 November 18, 2004 17:51

All times are GMT -4. The time now is 12:43.