CFD Online Logo CFD Online URL
Home > Forums > NUMECA

Difficulty calculating high p*k compressor

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

LinkBack Thread Tools Display Modes
Old   May 1, 2003, 08:02
Default Difficulty calculating high p*k compressor
jiang chen
Posts: n/a
Hello my friend: When Numeca used to calculate one stage axial flow compressor performance(full 3D calculation), I found it is difficulty to calculate when the back pressure is high (the back pressure is not over stall pressure). Other words, it is difficulty to calculate the high pressure ratio axial flow compressor or Fan. Who has experience, I call for reply. Thank you.
  Reply With Quote

Old   May 1, 2003, 14:35
Default Re: Difficulty calculating high p*k compressor
Allan D. Grosvenor
Posts: n/a
Hello Jiang,

It would be interesting to know whether you are employing a mass flow or pressure boundary condition at the outflow boundary. If you are using a mass flow B.C. and there is any flow separation adjacent to the domain exit, make sure you employ 'backflow control' to ensure that energy is not falsely injected back into the domain due to the local inflow. This option will maintain any real reversed flow, while locally applying a physically correct boundary condition. Additionally, in the case of a mass flow B.C., it would be worth checking how appropriate the chosen initial pressure is.

If you are using the Baldwin-Lomax turbulence model, please note that this one is known to underpredict turbulent mixing in adverse pressure gradient flow, and therefore tends to overpredict separation. During the numerical transient, significant levels of false flow separation may be developing, thereby detracting from convergence stability. You would observe an oscillation in average continuity equation residual if this were the case. If you saved intermediate solution files, you would observe an oscillation of velocity profiles at the outflow boundary. I would strongly recommend use of the more robust and accurate Spalart-Allmaras turbulence model. We have achieved significant improvements in both accuracy and convergence stability for off-design performance prediction of a wide rage of machines with this model.

You might also try modifying your multigrid strategy. Prior to automatic prolongation to the finest grid, try increasing the number of FMG (coarse grid initialization) cycles to say 300 or more. Calculation on the coarse grids is quite cheap, and can significantly increase your convergence rate. It might also be worthwhile increasing the number of coarse grid MG sweeps. In case you've modified the number of MG levels from the default value, please note that we generally recommend three.

FINE/Turbo is routinely used for simulating multiple design points from surge to choke for radial and axial machinery. Please feel free to contact your local support office to receive associated validation reports and papers. Additionally, you might be interested in relevant papers that study endwall blockage, tip clearance effects and casing treatment techniques.

Best regards, Allan
  Reply With Quote


Thread Tools
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 On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Difficulty in generating 3-D mesh Rucy FLUENT 3 November 10, 2005 10:53
Convergence Difficulty Sankalp CFX 0 September 27, 2004 17:32
convergence difficulty Devin CFX 1 March 2, 2004 19:42
I faced difficulty in a fortran error J. Kim Main CFD Forum 6 March 19, 2002 18:36
Convergency Difficulty!! Min-Hua Wang CFX 8 November 14, 2001 14:31

All times are GMT -4. The time now is 01:51.