I´m a student that trying to optimize a turbo-restrictor that we have to use in our Formula SAE car.I want to know how to specify in CFX5 that I want compressibel flow(can´t find any info in Tutorials and help menu)since the flow in the restrictor will be choked when the airspeed approaching Mach 1,so far I have used "Air ideal gas" but my massflow is to high to be accurate.

Thanks in advance. Thomas SWEDEN

Hi Thomas,

To model choked flow, you also need to use "Total Energy" as your heat transfer model in the fluid domain. Also, there are tutorials which use compressible flow - tutorial 8, "Supersonic flow over a wing" and tutorial 12, "Flow in an Axial Rotor/Stator Arrangement".

Regards, Glenn Horrocks

I´ve tried to use "total energy" as heat transfer and I have looked at the tutorials mentioned but I can´t get it to work-and specifying supersonic didn´t work for me either. Maybe i´m doing something else wrong(I specify domain to:100kPa-Air ideal gas, and set the Boundary conditions to: inlet-100kPa and outlet to 52,8kPa that in teori should get M1 and choked flow-all air goes thru a convergent-divergent pipe with a 20mm minium diam.) looking forward to get some more info. regards Thomas

You say you specify domain to 100kPa. This is OK, but you should understand that this is the reference pressure. All other pressures are relative to this. If you mean for your inlet to be 100kPa absolute, then you should specify the inlet value as 0 kPa. If you mean for your inlet to be 100kPa relative (i.e. 200kPa absolute in your case) then you already have the correct values. Similarly, the outlet pressure is relative to the reference pressure. Hope this helps, Mike

That explain why my massflow was twice as high as expected, so now it should work with correct "Boundary conditions". Thank you for the help, Mike and Glenn regards Thomas