CFD Online Logo CFD Online URL
Home > Forums > FLUENT

Bubbly flow boundary conditions

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

Like Tree1Likes
  • 1 Post By Vivek

LinkBack Thread Tools Display Modes
Old   January 17, 2002, 06:49
Default Bubbly flow boundary conditions
Posts: n/a
Hello All,

I am trying to set up a bubble column in Fluent6 and I'm not sure how to set up the BC for the gas phase at the liquid surface.

I would like the air to be able to leave the surface as it would physically, but I dont want the liquid to be able to leave.

Could anybody help me, please?
  Reply With Quote

Old   January 18, 2002, 05:48
Default Re: Bubbly flow boundary conditions
Sugen Chetty
Posts: n/a
I am doing a similar case involving flotation, but I'm using a earlier version of Fluent. I am going to use the interface as an inlet boundary of type pressure(equal to atmospheric in my case or slightly higher to force the fluid down). In my case I am using a single phase and modelling the scum with trapped air as particles with adjusted density.

  Reply With Quote

Old   January 18, 2002, 17:45
Default Re: Bubbly flow boundary conditions
Posts: n/a

you can use pressure outlet and setting back flow gas volume as 0.0

good luck
  Reply With Quote

Old   February 11, 2002, 13:00
Default Re: Bubbly flow boundary conditions
Posts: n/a
Hey Danny,

It is very simple but not straight forward. In many cases you would seen people model the top gas-liquid surface as outlet using two-fluid model. But, I hope that you would agree with me that two-fluid model is not expected to predict the gas-liquid surface. Ypu can model the top gas-liquid interface as follows:

1. Set top surface as inlet. Set all componet of liquid velocity to zero. Set vertical gas velocity to terminal rise velocity of bubbles (say 0.2 m/s). Note that the gas volume fraction is still a free variable. One you set this velocity, the gas volume fraction at outlet boundary can be estimated as:

flowrate gas hold-up = ----------------------------------

(c/s area x terminal rise velocity)

If bubble size is small (say 1-10mm, where rise velicyt is not much sensitive to bubble diam), one can set the terminal rise velocity to 0.2 cm/s. In other case you can compute it and then set us accordingly.

2. Other approach is to define sink for gas bubbles. for top surface set liquid velocity to zero and set phase velocity of top surface equal to the surface just below it. You can achieve it using appropriate UDFs/UDSs.

Let me know if anything is not clear to you.


beauty likes this.
  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
Low Speed Flow Boundary Conditions Paul Bateman FLUENT 2 January 10, 2013 14:01
Boundary conditions low Mach number flow lost.identity Main CFD Forum 0 November 28, 2010 05:44
Free surface flow settubg boundary conditions and plotting velocity profiles prashanthreddyh FLUENT 1 December 2, 2009 12:06
Internal flow simulation boundary conditions Kishore FLUENT 1 July 10, 2007 11:42
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 01:35.