CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Convergence problem in CFX (

Nicola July 24, 2006 08:57

Convergence problem in CFX
Hello everybody,

I simulated a diffuser of a steam turbine. I have problems with Mass and Momentum RMS. These values oscillate between e-3 and e-4. I' d want at least e-5. Boundary conditions are:

1) INLET: Profile Data (Total Pressure, Total Temperature, Velocity directions);

2) OUTLET: Opening with static pressure and static temperature imposed;

3) WALL: Adiabatic and no slip wall.

I already decreased time scale and used upwind scheme instead high resolution! What can I do?


P.S. I imposed a mass flow and normal velocity direction and in this case I had a good convergence!!!

Mike July 24, 2006 09:55

Re: Convergence problem in CFX
I assume there's no GGI's if it's just the diffuser? Go back to High Resolution, Upwind won't help. Create a monitor plot for mass flow at the outlet - I assume it will be oscillating with a constant period. If so, you can try increasing the timestep so that you are not resolving the oscillations. Also, are you using Average Static Pressure at the Outlet? If not, use this instead of a uniform Static Pressure. Is it necessary to use an Opening at the Outlet? If you have recirculation at the outlet then you may need to move your outlet further downstream. If all else fails run it transient. Mike

Nicola July 25, 2006 02:31

Re: Convergence problem in CFX
Hi Mike,

It's only the diffuser! Boundary profile on inlet was calculated in a previous simulation on outlet of last low pressure stage that is immediately upstream diffuser. I can't move outlet downstream and if I imposed an outlet condition, simulation stops!

Oscillations are periodic so I think you are right about increasing timescale. Auto time scale is about 4.5*10^-3. How much do I increase time scale? Is 4.5*10^-2 a good value?

Thank you!

Mike July 25, 2006 07:48

Re: Convergence problem in CFX
Try increasing the timestep to about the advection time of the diffuser, using the previous solution as the starting point. The Solver may fail at this timestep, you'll just have to see. The mass flow oscillations may or may not be physical. Looking at the locations of the maximum residuals may provide a clue - e.g. if they are near the outlet then the imposed boundary condition may not be appropriate. You can also run in transient for one oscillation period and see where the solution is changing. Mike

anna July 26, 2006 11:44

Re: Convergence problem in CFX
Hi Nicola,

my suggestion is:

outlet: opening with relative pressure 0 Pa outlet: static pressure: define an expression for the temperature at the outlet areaAve(T)@outlet

Change to physical timescale and decrease it to 0.1s.

change the calculation to double precision.

Good luck

All times are GMT -4. The time now is 20:15.