I am modelling an air flow in a piping system, using ideal gas, coupled solver, standard k-epsilon turbulence model, sutherland law for viscosity. I am expecting choked flow at an orifice in the system.

The model seems to be converging by looking at pressures and mass balances however i have mach numbers of 5 downstream of the choking point.

Can anyone suggest what may be wrong with this model or any tips in general for modelling chocked flow?

what are your dimensions (area ratio of throat to inlet, or throat to outlet) and what are the pressures used?

16 bar gauge inlet 1bar gauge outlet 5mm throat 22mm inlet and outlet

I assume you have a circular pipe?

So area ratio of throat to outlet and inlet is (5/22)^2 =about 0.05.

If you consider non-dimensional mass flow: m*root(cp*T0)/(A*P0), then at throat, it is 1.281.

Given your area ratio, that works out to be 0.06617 at the inlet and outlet, which corresponds to about M = 0.03 and M=4.75. So your area ratio itself is why the Mach numbers are so high downstream.

To just hit M = 2 downstream, you just need a 17 mm throat in a 22 mm pipe!

I hope this helps.

i thought it was impossible to get a mach number above unity in a pipe apart from with a converging diverging nozzle?

You're right in that for a flow in a pipe, the effect of heating or friction will cause the Mach number to rise at most to unity. Hmmm...let me think about this for a while...

I seem to remember that the M=1 in a conv. nozzle is under "orderly conditions". If the inlet conditions are at high pressure then the pressure are high after the nozzle and an expansion are necessary. Again I seem to remember that this is done by the air accelerating to M>1 forming at chock, and then decelerating. This process induces friction loss, which lowers the pressure level. The flow keeps accelerating and decelerating until the pressure level is the same as the surroundings. I don't know if there is a fixed level to which the velocity accelerates until the chock formes, but why not M=5 in some cases.

I hope this helps and I certainly hope that I remember correct

You will get sonic condition in the throat and the throat-area will fix your mass-flow. After the restriction throat you will get a supersonic expansion. With 16 bar you will be able to reach about Mach 2.5, then you will get shocks that take down your flow to subsonic conditions again. You will not be able to reach supersonic exit conditions with the area ratio you mentioned.

My experience from running this type of simulations in fluent is not very good - the segregated solver can produce very strange results and not very well resolved shocks, the implicit coupled solver is often diffuclt to get convergence with. I'd recommend you to try the explicit coupled solver, but YMMW.

YMMW?

Thanks, I have been using coupled implicit, I will try coupled explicit.

You mentioned that you have seen some strange results running this kind of analysis in fluent. I am particularly interested in modelling mass flow and will later be looking at a transient situation with changing inlet and outlet pressures. Will Fluent struggle to model this?

YMMW = your mileage may wary

The segregated solver in Fluent often has difficult to establish supersonic/transonic flow fields and tends to get "stuck" in non-physical solutions like the one you describe with a supersonic outflow.

If you have a choked orrifice you don't need CFD to predict the mass-flow. The mass-flow can easily be calculated by hand if you know the orrifice area and the upstream conditions.