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

density current-outlet boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 12, 2011, 10:52
Default density current-outlet boundary condition
  #1
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
I want to simulate an open-channel flow that at the begining of my experience has only water and air. The experience begins with the injection of a mixture of water and sediments into this channel. I have a device that allows the water height to remains constant. I would like to know your opinion about:

-As i am not interested in modeling the air part i am modeling the free surface with a free slip boundary condition. Agree?
-At the outlet boundary condition i am using the option average static pressure, with relative pressure=0 and the pressure profile blend=0.05 (average over whole outlet). Agree?
Best Regards
antonio is offline   Reply With Quote

Old   September 12, 2011, 19:59
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
-As i am not interested in modeling the air part i am modeling the free surface with a free slip boundary condition. Agree?
No. A pressure boundary is better, as the pressure at the free surface is atmospheric (assuming surface tension is insignificant).

Quote:
At the outlet boundary condition i am using the option average static pressure, with relative pressure=0 and the pressure profile blend=0.05 (average over whole outlet). Agree?
As long as it represents what you are trying to model it sounds good.
ghorrocks is offline   Reply With Quote

Old   September 13, 2011, 05:22
Default
  #3
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Hi Glenn.
In what relates my top boundary condition i will try to check your suggestion. CFX is computing a recirculation zone in the top of my domain that was not supposed to be there and I want to check if itīs possible to improve my results in this zone.

In what concerns my outlet boundary condition, in my experimental setup, I have initially an hydrostatic pressure distribution in the outlet (just clean water) but then, when I inject the mixture (water+sediments) the pressure distribution ceases to be hydrostatic...Also the sediments and the water that left the domain are captured by a feedback circuit. I have choosen the option average static pressure, with relative pressure=0 and the pressure profile blend=0.05 (average over whole outlet) because it seemed to be the most appropriate for me.
antonio is offline   Reply With Quote

Old   September 13, 2011, 10:11
Default
  #4
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Do you consider this is the best way of modeling the outlet ? I am having some difficulties with my results so I need to check all details. Thanks.
Regards.
antonio is offline   Reply With Quote

Old   September 15, 2011, 07:10
Default
  #5
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Glenn, in what concerns the top boundary condition, you were referring to a condition of "opening" type?Such as in the free surface over a bump tutorial?
antonio is offline   Reply With Quote

Old   September 15, 2011, 19:05
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Yes, an opening.

If you are having troubles with your outlet boundary then move it further downstream.
ghorrocks is offline   Reply With Quote

Old   September 22, 2011, 10:09
Default
  #7
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Glenn, but if I put an opening boundary condition it may happen that the fluid goes out of my domain...and in my experience the water level remains constant.Furthermore it could be even harder to get convergence. Do you agree with my comment?
I have tried to implement a symmetry boundary at the top of the domain but i have received a very strange error.
antonio is offline   Reply With Quote

Old   September 22, 2011, 10:24
Default
  #8
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Also, do you think that a no-slip wall will be an option for my top boundary condition. As i have said I am having negative velocities at the top of my domain that should be approximately = zero(at the moment i am using a free slip wall)
antonio is offline   Reply With Quote

Old   September 22, 2011, 18:23
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
if I put an opening boundary condition it may happen that the fluid goes out of my domain
If you are happy to run this model as a multiphase free surface model then you can let the simulation sort out the interface. But if the free surface is simple you can simplify your model down to a single phase model with a pressure boundary as the free surface. Why a pressure boundary? Because the best description of a free surface (in most cases) is that it is at atmospheric pressure. This does mean a small amount of flow will probably go in or out of the boundary but this is an approximation of the system so you would expect some deviation. It is up to you to determine whether this simplification is acceptable or not.

The alternative (a free slip boundary) means that the pressure will vary along the interface.

If you want to use the single phase approximation you then need to choose whether the correct pressure but small flow across the interface (ie the pressure approach) or the wrong pressure but no flow across the interface (ie the free slip boundary approach) is best.
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
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
External Radiation Boundary Condition (Two sided wall), Grid Interface CFD XUE FLUENT 0 July 8, 2010 06:49
VOF Outlet boundary condition in cfd - ace JM Main CFD Forum 0 December 15, 2006 09:07
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
Outlet velocity boundary condition Jay FLUENT 4 December 15, 2002 09:27


All times are GMT -4. The time now is 10:55.