CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Choked Flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 7, 2003, 12:20
Default Choked Flow
  #1
phil
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   March 10, 2003, 07:54
Default Re: Choked Flow
  #2
Chris
Guest
 
Posts: n/a
what are your dimensions (area ratio of throat to inlet, or throat to outlet) and what are the pressures used?
  Reply With Quote

Old   March 10, 2003, 07:57
Default Re: Choked Flow
  #3
Phil
Guest
 
Posts: n/a
16 bar gauge inlet 1bar gauge outlet 5mm throat 22mm inlet and outlet
  Reply With Quote

Old   March 10, 2003, 12:28
Default Re: Choked Flow
  #4
Chris
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 10, 2003, 12:36
Default Re: Choked Flow
  #5
Phil
Guest
 
Posts: n/a
i thought it was impossible to get a mach number above unity in a pipe apart from with a converging diverging nozzle?
  Reply With Quote

Old   March 10, 2003, 19:34
Default Re: Choked Flow
  #6
Chris
Guest
 
Posts: n/a
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...
  Reply With Quote

Old   March 11, 2003, 03:24
Default Re: Choked Flow
  #7
Christian
Guest
 
Posts: n/a
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
  Reply With Quote

Old   March 11, 2003, 06:00
Default Re: Choked Flow
  #8
Jonas Larsson
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 11, 2003, 06:09
Default Re: Choked Flow
  #9
phil
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   March 11, 2003, 07:13
Default Re: Choked Flow
  #10
Jonas Larsson
Guest
 
Posts: n/a
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.
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Flow meter Design CD adapco Group Marketing CD-adapco 3 June 21, 2011 08:33
What is the difference between liquid reactive flow and gas reactive flow? James Main CFD Forum 6 May 15, 2009 12:14
reversed flow at velocity inlet / mass flow inlet ib FLUENT 1 March 26, 2007 13:11
potential flow vs. Euler flow curious ... Main CFD Forum 23 July 21, 2006 07:40
Plug Flow Franck Main CFD Forum 3 September 4, 2003 05:57


All times are GMT -4. The time now is 11:51.