CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

Convergence problem in CFX

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

LinkBack Thread Tools Search this Thread Display Modes
Old   July 24, 2006, 08:57
Default Convergence problem in CFX
Posts: n/a
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!!!

  Reply With Quote

Old   July 24, 2006, 09:55
Default Re: Convergence problem in CFX
Posts: n/a
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
  Reply With Quote

Old   July 25, 2006, 02:31
Default Re: Convergence problem in CFX
Posts: n/a
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!
  Reply With Quote

Old   July 25, 2006, 07:48
Default Re: Convergence problem in CFX
Posts: n/a
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
  Reply With Quote

Old   July 26, 2006, 11:44
Default Re: Convergence problem in CFX
Posts: n/a
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
  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
Heat Transfer simulation: No convergence problem fiqs CFX 2 April 21, 2010 15:47
History Convergence: Graphical problem Bedotto NUMECA 1 March 17, 2010 23:40
Urgent Problem with Hypermesh and CFX Luk CFX 5 March 14, 2008 04:59
convergence problem limseokmin FLUENT 3 November 14, 2004 12:43
CFX 4.4 installation problem Pandu Sattvika CFX 1 December 1, 2001 04:07

All times are GMT -4. The time now is 22:07.