Hi everyone,

I'm only a new user of CFX. I want to simulate compressible multiphase flow (saturated vapor and saturated liquid). I know their inlet pressure(400kPa) and inlet velocities, however i don't know anything about the outlet condition (in reality, the outlet flows through another device, not exposed to atmosphere). I tried simulating using Pref=1atm, Pout(average static)=0atm, and inlet velocities for the fluids. The results for the velocities are ok, but the values of pressure are almost all negative and as expected the results for densities are lower. However, the shape of the profile especially for static pressure is as expected. Is this results reliable? Meaning can I just add a constant to the results such that the pressure at inlet will be 400kPa? Can I use this adjusted pressure data to correct the values for density?

I've read that it is not an issue for incompressible flow because the important thing is the pressure difference but I'm really trapped on how to set the outlet condition for compressible flow.

Any help is much appreciated! Thanks a lot!

Michelle

Hi Michelle,

If the fluid density varies with pressure and the flow is compressible, the pressure level must be set appropriately for your simulation to have any meaning.

You need to ask "What is driving the flow into and out of the device?". If the flow rate is controlled downstream, then a mass flow rate may be appropriate at the outlet. If the inflow is coming from a plenum, set the inlet total pressure to the plenum static pressure. If you can't set the mass flow rate at the outlet, then do so at the inlet and set an appropriate pressure level at the outlet. If you don't know the flow rate, then you need to know what the delivery and back pressure are.

Regards, Robin

Hi Robin,

Thanks a lot for your very helpful advice. I have data for inlet mass flow rate and I think I'll use the experimental data for exit pressure. I raised my first question because I want to know how to optimize the device using CFD model without performing an experiment first. In experiment, inlet conditions are specified and then outlet parameters are measured. Is it correct to say that for CFX it's "backward"? That in CFX we set an outlet condition (e.g. pressure) and an inlet condition (e.g. mass flow rate), then the results will show other parameters (e.g. inlet pressure,velocity) that can be used to access performance. Is this right or am I just dreaming?

I have an additional question, if I use mass flow rate as inlet condition, can I specify different velocities for the fluids? The inlet is dispersed liquid droplet in vapor wherein the vapor is faster than the liquid. Thank you so much Robin!

Michelle

Hi Michelle,

You should control the CFD analysis just as you would your experiment or as the device would operate; if you set up the analysis with total (i.e. stagnation) conditions at the inlet and a static pressure (i.e. back pressure) at the outlet, the mass flow rate will come from the solution; if you specify inlet total conditions and specify the outlet mass flow rate, CFX will return the back pressure to acheive that flow rate; if you set the mass flow rate at the inlet and specify the outlet pressure, CFX will determine the inlet conditions to acheive that flow rate agains that back pressure; if you have multiple outlets with different mass flow rates, CFX will determine the back pressure at each outlet, and so on...

There are a vast number of boundary condition types available, the key is determining which boundary condition best represents the physics. Familiarity with the system you wish to simulate is very important because you need to be able to make good engineering approximations at these boundaries.

One thing to keep in mind, however, is that for incompressible flow, you must specify a pressure boundary somewhere, otherwise it is nearly impossible to determine the pressure level of the system. Mass flow will always be conserved, so resist the temptation to specify the flow rate in and out. If you don't know the delivery or back pressure, make a reasonable assumption.

Best regards, Robin

Hi Robin!

Wow I'm impressed with your explanation!It makes CFD more and more interesting!Thanks a lot!

By the way, maybe it's a typo error or I'm wrong, maybe you mean "compressible" for this part of your response.. -One thing to keep in mind, however, is that for "incompressible" flow, you must specify a pressure boundary somewhere...

Thanks again,

Michelle

Oops! Yes, that was supposed to be "compressible".

-Robin

Actually, sometimes you don't need to set a pressure BC for compressible flow; for example, filling a tank (inlet, no outlet) with a specified mass flow rate. Or a cylinder with a moving piston but no inlets/outlets. These are transient cases in which the pressure level is set by initial conditions/time history.

[yash.aesi]

Hello,

I am trying to simulate the flow in the air transfer pipe. At the inlet i have static pressure, temperature, mass flow rate. so from this i checked that the flow is compressible. At the inlet i have applied the mass flow inlet boundary condition but at the outlet i don't have any data so what boundary condition should i applied at the outlet ?

Thanks & Regards,
Sonu.

[ghorrocks]

You need to know something about the outlet, probably the pressure.

[yash.aesi]

Hello Glenn,

thanks for replying but rite now i don,t have the pressure at the outlet , that is what i want to calculate (pressure drop).... anything else i can do to find it ??

Thanks & Regards,
Sonu.

[ghorrocks]

The pressure has to be defined somewhere.

So then define the pressure at the inlet and mass flow rate at the outlet.

[yash.aesi]

Hello Glenn,
i already tried this by using the pressure inlet and mass flow outlet BC. but then the problem is that after simulation velocity fields are coming wrong.
for more clarity :
at inlet i have mass flow = 0.1867 kg/s, area = 0.001256 m2, pressure(static)= 159 kPa, temperature(static) = 163 Degree Celsius. these are the given conditions.

so if i use the compressible flow relations then my velocity at the inlet should have to come around 126 m/s but after running with above BC its coming around 47 m/s.

so any idea about it ???

Thanks & Regards,
Sonu

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F