CFD Online Logo CFD Online URL
Home > Forums > FLUENT

back pressure at exit for supersonic flow

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

Like Tree2Likes
  • 2 Post By Razvan

LinkBack Thread Tools Display Modes
Old   April 6, 2007, 12:25
Default back pressure at exit for supersonic flow
Posts: n/a
I use Fluent 6.2 version. I am simulate the Laval nozzile. In the convergent part, it is subsonic. In the divergent flow, the flow is supersonic, when the pressure at exit is very low. Now I increase the back pressure at exit, this pressure would propagate upstream to genreate a shock wave which would be between the throat and the exit, according to the text book. However, the simulate result showed that this back pressure could not be exerted on the flow. The result of the contour showed that the the flow always supersonic flow, the shock wave is not generated. Firstly, I use the converged superonic flow in the divergent as initial condition, the pressure at exit is 7725 pa. Then, I given the "pressure-outlet" as 505325 Pa, then computing. When I plot, I find that the pressure at exit is still 7725 Pa.

Could any body comment this? How to make the back pressure on role to the flow at the exit?

Thanks in advance!

  Reply With Quote

Old   April 6, 2007, 19:05
Default Re: back pressure at exit for supersonic flow
Posts: n/a
You might be able to calculate the mass flow at the exit relative to your desired pressure, and then use this as a "target mass flow" input into your boundary condition at the exit plane.
  Reply With Quote

Old   April 8, 2007, 09:13
Default Re: back pressure at exit for supersonic flow
Posts: n/a
Thanks for your response.

However, there is no "target mass flow" at the boundary condition at the exit plane.

  Reply With Quote

Old   April 10, 2007, 03:29
Default Re: back pressure at exit for supersonic flow
Posts: n/a
If you are simulating just the nozzle itself, with no exterior, then the answer to your problem is simple: the exit of the flow domain is fully supersonic, so whatever condition you try to impose on the exit boundary will be totally ignored by the solver. This is completely physical: in a supersonic region, any perturbation cannot propagate upstream, because the velocity which the perturbation traveles with (sound speed) is always smaller then the flow velocity (supersonic speed = higher then sound speed).

To be able to overcome this problem, you have two options:

- first, if you do not want to modify the grid, then you will have to restart the calculation using a small upstream pressure (let's say, 1.5 x exit pressure), and slowly increase it; at a certain pressure ratio, depending on the nozzle geometry, the throat will become choked, and after a slight increase of the pressure ratio, a shock system will be generated in the divergent part of the nozzle; if increasing the P.R. even more, then the shock system will travel from throat toward exit, and at the design P.R. will reach the exit and vanish.

- secondly, if you are willing to modify the grid, then go back to Gambit, and add a generous amount of exterior domain (at least 25 nozzle diam. in lenght, and 10 nozzle diam. in height); then recalculate the flow with your present conditions; now, if you modify the exit pressure, at 25 nozzle diam. away, the exit being subsonic, the perturbation will propagate upstream and you will be able to obtain the shock system inside the nozzle.

Personally, I prefer the first way, because it requires a smaller grid and it is much more realistic.

All the best,

vinayender and waiter120 like this.
  Reply With Quote

Old   April 12, 2007, 02:25
Default Thank you very much for your help. *NM*
Posts: n/a
  Reply With Quote

Old   April 13, 2007, 02:02
Default You're welcome! *NM*
Posts: n/a
  Reply With Quote

Old   April 24, 2014, 15:13
New Member
Join Date: Mar 2014
Posts: 6
Rep Power: 5
Zoli is on a distinguished road
Thank you !
Zoli is offline   Reply With Quote


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
Pressure outlet in two-phase flow in horizontal 2D channel AlmostSurelyRob Main CFD Forum 0 November 17, 2010 08:32
pressure distribution in water flow, differences in icoFoam and COMSOL deniggo OpenFOAM Running, Solving & CFD 14 September 30, 2010 03:48
Mass flow BCs and Pressure differential BC CFDLife CFX 5 January 26, 2009 08:14
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19

All times are GMT -4. The time now is 15:23.