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

simple model, difficult outlet

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 24, 2006, 20:03
Default simple model, difficult outlet
  #1
Eric
Guest
 
Posts: n/a
Dear Friends,

My model is a cylinder: 2.8 mm in diameter, 7.35 mm in length. One end of the cylinder is inlet and the other is out. At inlet, velocity = 311.4 m/s; how to set the boundary condition at Out? If I set the pressure at OUT as 1 atm, maybe not good, could you give me some advice?

Thank you in advace.

Eric
  Reply With Quote

Old   December 25, 2006, 11:32
Default Re: simple model, difficult outlet
  #2
Manu
Guest
 
Posts: n/a
Preessure Outlet Relative Pressure : 0
  Reply With Quote

Old   December 28, 2006, 10:31
Default Re: simple model, difficult outlet
  #3
Sameer
Guest
 
Posts: n/a
Hi Eric !

In your problem velocity is very high ( 311.4 m/s ), flow must be highly turbulent and undevloped. I think you should try with mass flow rate at inlet and outlet as a opening.
  Reply With Quote

Old   December 29, 2006, 13:31
Default Re: simple model, difficult outlet
  #4
Robin
Guest
 
Posts: n/a
It depends on what is downstream of your outlet that you have not included in your model. Keep in mind that a boundary condition is an approximation of what the external conditions may be.

Since you are modelling a pipe and have specified the flow at the inlet, a pressure outlet would be appropriate. I wouldn't bother with an opening unless you really expect reversed flow.

There are two options for the pressure: average static pressure or "static pressure".

The Average Static Pressure option will allow the pressure value to vary locally, but maintain the area averaged for pressure at the value you specify, thus allowing the profile to develop naturally. This is appropriate if the flow continues along the pipe beyond your boundary condition.

The "Static Pressure" option will maintain a constant static pressure at the outlet. This would approximate the conditions occurring when the pipe exits into a large plenum. In such a case, the static pressure would be roughly constant across the pipe.

If the fluid is liquid and you are not including cavitattion, it really doesn't matter what pressure you set. The solution will be the same relative to the outlet.

If flow is compressible, you need to consider the conditions more carefully. If you don't know the outlet pressure and flow is entering your domain from a large plenum, you would probably be better off specifying a total pressure at your inlet equal to the static pressure of your plenum (if the velocity is sufficiently low in the plenum, the Ptotal=Pstatic) and a mass flow rate at the outlet.

Again, there are some options as to how the static pressure will vary at the mass flow outlet; Scale Mass Flows, Shift Pressure, and Constant Flux.

The default is mass flow update option "Scale Mass Flows" and does the equivalent of the Average Static Pressure, allowing the local mass flow rate to vary naturally but maintaining the total flow rate specified.

Shift Pressure allows you to enter a relative pressure profile which the solver will match by shifting up or down to get your mass flow rate. If you put a constant value in here, you will get a constant static pressure at the outlet, which as before will approximately represent the conditions at a sudden expansion.

The last option, Constant Flux, is not physically realistic for this case as it will force the mass flux to be constant everywhere.

Finally, if you only know the pressure conditions at the inlet and outlet, you can set it up with a total pressure at the inlet and a static pressure at the outlet, in which case the mass flow rate will be determined.

Regards, Robin
  Reply With Quote

Old   December 29, 2006, 22:16
Default Re: simple model, difficult outlet
  #5
Eric
Guest
 
Posts: n/a
Dear Friends,

Happy new year.

Thank you for your helping and I will try as you said.

Mang thanks

Eric
  Reply With Quote

Old   May 22, 2014, 02:32
Default inlet boundary conditions
  #6
New Member
 
Join Date: May 2014
Posts: 4
Rep Power: 3
Ashwin k is on a distinguished road
hello guys,
i have seen ur above comments regarding wat boundary conditions should be specified at inlet and outlet. from above i concluded that for outlet pressure condition should be given and for inlet velocity condition should be given.
in my problem i m using a cylinder with diameter of 8mm with inlet and outlet port diameters 7mm and 2.8mm respectively distance from inlet to outlet port is 32mm. pump operates at 400bar. so now how do i find velocity at the inlet.

thank u in advance
Ashwin k is offline   Reply With Quote

Old   May 23, 2014, 04:44
Default
  #7
Member
 
SanS
Join Date: Mar 2009
Posts: 42
Rep Power: 8
sans is on a distinguished road
Do you know the flow?
sans is offline   Reply With Quote

Old   May 23, 2014, 08:13
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,832
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Sans is right - the boundary conditions you apply are the flow conditions you know about the flow. It oculd be flow rate or pressure.

You mention 400 bar - remember that this should be just used as the reference pressure, the important thing for the simulation is the pressure rise/drop, so the pressure difference between the inlet and outlet.
ghorrocks is offline   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
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
outlet boundary conditions Xhoven OpenFOAM Running, Solving & CFD 3 June 11, 2011 19:33
Simple 1D Stress FE Model Jonny6001 Main CFD Forum 1 March 25, 2010 06:22
Problems bout CFD model of biomass gasification, Downdraft gasifier wanglong FLUENT 2 November 26, 2009 00:27
Please help with flow around car modelling! Tudor Miron CFX 17 March 19, 2004 20:23


All times are GMT -4. The time now is 08:25.