Hello, all:

I am using CFX-4 to simulate a turbulent flow in a complex geometry. This is a single phase problem. I have imposed pressure scouces term on some of the block . Now the probelm is convergency get the trouble. Especially mass balance. Can anybody suggest me the strategy of getting convergency in a similar case.

Thanks.

If the model is physically consistent, try to increase the number of iteration of pressure (mass) equation at
:> SOLVER DATA
:> PROGRAM CONTROL

ITERATIONS OF VELOCITY AND PRESSURE EQUATIONS 1

or try to increase PRESSURE at

>> SOLVER DATA
:> SWEEPES INFORMATION
:> MAXIMUM NUMBER PRESSURE 30

There are others strategies suggested in manual.

I hope this help.

Ribeiro

As Ribeiro said and if you are absolutely certain that your source term manipulation is correct, you can increase the number of sweeps carried out for each iteration. You could also reduce the reduction factors slightly, esp. for mass. If mass/pressure are causing troubles in a complex block structue think about using a multigrid solver, and think about reblocking you grid in the Build4 Analysis Form or via Meshimport 9to sweep over a larger domain). These are easy remedies to test. However, if the turbulent terms are causing mass diverging, consider also the use deffered correction of the cross-derivative diffusion terms. you can identify the troublesome terms in the output files. If needed print more info to this file.

The section in the manual about convergence problems is actually very good, try to read it, you will get some good ideas from there.

The two suggestions already mentioned, with deffered correction and using AMG on pressure (only) has helped me many times.

Also try to reduce the under relaxation factors, for complex geometries they can cause problems or try false time steps.

Jan

Hello, thanks.

I believe that the source term manipulation is correct since I compared CFD data with LDA data and found that both matched each other very well in the mean velocity and turbulence kinetic energy. However, the residual file showed a poor convergency in terms of mass scouce. I have read the outpout file and found out the ratio of second iter and the last iter is 1.0 no improvement in mass at all. But the overall mass balance in the whole system is perfect. What that means?

Thanks.

Could you explain how you have impossed the pressure source terms-command file or user fortran Jan

First I define a user2d patch.

>>CREATE PATCH PATCH NAME 'SOURCE' BLOCK NUMBER 'B5' LOW I END

>>MODEL DATA
:>SOURCES

PATCH NAME 'SOURCE'

PRESSURE 10.0 0.0

PER UNIT MASS

END

Actually, the velocity file and turbulence field obtained are very reasonal. The residual of mass term is so poor.

Can you suggested something Many thanks MHW

I have never used the source command with pressure so I am only guessing. If possible for you, without violating what you want, use Body Forces instead, It used to be a better approach when a certain pressure drop should be impossed.

You only include the source term as a SU term, I think that can lead to an unstable solution (check in Patanker)

Jan

I have tried to use transient simulation to reduce the residuals for all variable. It works for all but one variables. It seems that the mass residual never reduces. I have checked the output file and confirm this, however, the overall mass flow rate is perfeccly balanced. It that critical to obtain a convergent mass residual, since the solution matches the LDA measurement almost perfectly both interms of mean and TKE data.

Thanks for suggestion.

MHW