hello,

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

dave

Hi

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.

Regards

jens

thanks jens for your advice. i'll try this out tonight.

dave

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.

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,

dave