Convergence problem in CFX

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

 July 24, 2006, 08:57 Convergence problem in CFX #1 Nicola Guest   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? Thanks P.S. I imposed a mass flow and normal velocity direction and in this case I had a good convergence!!!

 July 24, 2006, 09:55 Re: Convergence problem in CFX #2 Mike Guest   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

 July 25, 2006, 02:31 Re: Convergence problem in CFX #3 Nicola Guest   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!

 July 25, 2006, 07:48 Re: Convergence problem in CFX #4 Mike Guest   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

 July 26, 2006, 11:44 Re: Convergence problem in CFX #5 anna Guest   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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post fiqs CFX 2 April 21, 2010 15:47 Bedotto NUMECA 1 March 18, 2010 00:40 Luk CFX 5 March 14, 2008 05:59 limseokmin FLUENT 3 November 14, 2004 13:43 Pandu Sattvika CFX 1 December 1, 2001 05:07

All times are GMT -4. The time now is 14:48.