[LeandroGSS]

Hello everyone,
I have already searched the internet and this forum for a week trying to find an answer to my question.

How do you best model a flow, in which the fluid (air) comes out of a nozzle, which is attached to a cylinder reading "3 bar"?

I first tried to find a formula that calculates the air speed out of this nozzle by knowing the pressure. Of course, Bernoulli is NOT an option here, because my fluid is very compressible.
So I found in a forum (am I allowed to post external links here?) which says that a test should be made: p/po < 0.528 (po is the absolute pressure in the tank, and p is the atmospheric pressure). It says, if below this critical number, the flow is "chocked" and the air is moving exactly at 1 Mach (343 m/s).

First question, does it proceed?

I tried to simulate it with CFX and did the following:
- I choose Ideal Gas and activated Heat Transfer (as "Total Energy"), in order to have a compressible fluid.
- Turbulence Model = SST
- For my inlet, I choose "Supersonic" and there I had to choose two boundary conditions. I took "total pressure = 3 bar" and "relative pressure = 0 bar".

My expectation was that the program would calculate the air speed coming and if I get Mach 1 there, than the assumption of the other forum was right.

My simulation runs for a few steps and then suddenly I get a warning saying that a wall was put in my outlet (100%) to prevent fluid entering the domain. The simulation breaks. If a switch my outlet for an opening, I will get a massage saying "overflow in the domain" or something like this.

Clearly I am doing something wrong with my boundary conditions.

So, what can you recommend? It seems something very simple, but I am stuck with it. It is just an inlet, whose source is a pressurized cylinder reading "3 bar" that contains air.

Thank you very much for the attention.


Theference https://www.physicsforums.com/thread...nozzle.694656/

[ghorrocks]

The equations you quote are for inviscid flow. So be aware that flow losses from viscosity and other losses will cause the CFX result to deviate from the ideal. If you keep the losses small then the CFX result will be a good approximation of the ideal result. If you have a lossy simulation - well, you can get anything

You probably did not want a supersonic inlet. The flow is probably subsonic at the inlet and accelerates to Mach 1 in the throat.

[LeandroGSS]

Thank you Gleen!
Would you or anyone suggest any better approach for this kind of simulation?
So I will model it as "subsonic". Should I set velocity = Mach 1 or Total Pressure = 3 bar as my boundary condition at the Inlet?

Am I maybe understanding my 3 bar pressurized cylinder wrong? I mean, if my pressure meter says 3 bar and if I assume no height differences and no dynamic pressure inside the cylinder, than my total pressure is 3 bar. And according to energy conservation, the total pressure (dynamic + relative) at the inlet should also be 3 bar.
What I find "weird" is to believe that the gas really exit the nozzle or reaches somewhere Mach 1. It seems really too much.

[ghorrocks]

You define your boundary conditions to match the conditions you are simulating. If you have a large reservior of 3 bar gas then you can assume the velocity in the reservoir is small but the pressure is 3 bar. So using a 3 bar total pressure inlet would make sense, as long as the inlet is placed in a region where the flow velocity is small.

Be careful with your definitions of static pressure, total pressure, gauge pressure and absolute pressure. Absolute pressure = gauge pressure + reference pressure. In terms of absolute pressure your outlet is probably 1 bar and your tank is probably 4 bar.

That means you have a 4:1 pressure ratio across your nozzle, and if your flow is close to ideal then the equation your showed in post #1 indicates it should choke and have Mach=1 at the throat.