CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > Siemens

convergence problems

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

LinkBack Thread Tools Search this Thread Display Modes
Old   October 24, 2000, 13:01
Default convergence problems
david aquilina
Posts: n/a

i am using star cd to solve steady state flow through an air duct silencer (or other HVAC applications). my models have been, on the most part fairly simple, there are no complex geometries, and are uniform in the z direction. i am having trouble reaching convergence. my models are on the order of 300 000 cells, with a mesh block size of about 0.5 - 1.0 inch cube in critical areas. i have set the max iteration number to 2000, the convergence and relaxation factors are left at default.

should i be altering the relaxation factors to reach convergence before 2000 iterations, or is +2000 iterations normal for this type of work?

thank you for any tips offered

  Reply With Quote

Old   October 25, 2000, 03:52
Default Re: convergence problems
Jens Bennetsen
Posts: n/a

I don't think that 2000 iteration are enough. Also the default relaxation parameters are to high initially. Geneally I am using 0.3 for the velocity (or lower) and 0.5 for the turbulent eqn.'s.

As a rule of tumb, the number of iterations for convergence ~ 1E-03 are 5 - 10 times Sqrt(no. of cells).

This have been working for many different CFD code. I have not yet tested it for Star.

Hope this helps.


  Reply With Quote

Old   October 25, 2000, 10:06
Default Re: convergence problems
david aquilina
Posts: n/a
thanks jens for your advice. i'll try this out tonight.

  Reply With Quote

Old   October 27, 2000, 00:37
Default Re: convergence problems
Posts: n/a
0.5-1 cube inch per cell, that is coarse mesh. You should not have unstable field values when using k-e turbulence model. You did not mention what kind boundaries used. Try to use pressure boundary instead of OUTLET at the flow outlet. If you did and still not convergent, try reducing relaxation factor of pressure from 0.2 to 0.15, or smaller. Iteration of 2000 is too much. Star should converge in a few houndred unless your mesh was too fine. If this relaxation factor is less than 0.1 and still not converging to a residual below 0.01, then you will have pain/fun of it. Call 911 of ADAPCO, they will fix it.
  Reply With Quote

Old   October 27, 2000, 10:18
Default Re: convergence problems
david aquilina
Posts: n/a
thank you chung,

last night i ran the model with the following relaxation factors:

velocity (momentum) = 0.2

turb ke = 0.5

pressure = 0.1

and viscosity = 1.0 (default)

the model converged to my satisfaction, the oscillations of the residuals were completly damped out.

i had been using an OUTLET boundary. i have yet to use pressure boundries in any of my models - but now i know what im reading about today.

thank you jens and chung for helping me out,

  Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
convergence problems using SBF=1 Fonzie CFX 1 March 23, 2007 09:46
Convergence Problems Carlos FLUENT 0 March 12, 2007 03:44
Problems with Convergence Andres Bernal Ortiz CFX 2 January 16, 2007 08:58
Problems in convergence Simon Siemens 3 February 14, 2005 06:36
Convergence problems Chetan FLUENT 3 April 15, 2004 20:13

All times are GMT -4. The time now is 15:29.