Ansys Flotran: Velocity or Pressure BC?
I am working on a CFD model that consists of a manifold. The pressure head from the compressor is 90 psig at the inlet. I specified P=0 at the outlet.
With outlet pressure at atmospheric (Poutlet=0), the flow will be choked,thus the inlet velocity is the speed of sound. In the ANSYS documentation for compressible flow, only pressure is specified at inlet. I am confused on what boundary condition to apply for the inlet? Should it be velocity only? Or pressure only? Or both? Should the density be varied as well? Or keep it fixed at an air density relative to 90 psig? PLEASE HELP!!! 
Re: Ansys Flotran: Velocity or Pressure BC?
I am having the same problem! I wish I could help!

Re: Ansys Flotran: Velocity or Pressure BC?
Are you really sure the flow is choked at the inlet and not somewhere within the manifold where there is an area change???
You should use variable density, ideal gas air for this. Your boundary condition options are: If you are only partially sure that the inlet flow is choked then you could just set the total pressure at the inlet to 90 psi, normal direction, total temperature is whatever you want. The flow solver will figure out the inlet velocity values for you. If the flow is really sonic or supersonic at the inlet condition, and you know everything then just set inlet v,p and T and use a supersonic inlet condition. Given that you know the inlet stagnation value of pressure/temperature then you can easily figure out v,p and T assuming an isentropic expansion from stagnation to static conditions. Other "stable" options would be a v,T or mass flow, T subsonic inlet. The flow solver will calculate the inlet pressure profile for you. For the latter option you need to know the choked mass flow rate. A less stable option would be a p,T subsonic inlet with zero gradient condition for velocity. Make sure the grid is nice and orthogonal to the inlet if you use this BC. Dan. 
All times are GMT 4. The time now is 06:10. 