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

Volume fractions initialization when using degassing boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 1, 2014, 00:23
Default Volume fractions initialization when using degassing boundary condition
  #1
Member
 
Join Date: Feb 2011
Posts: 85
Rep Power: 6
Antanas is on a distinguished road
I need some help with understanding how CFX handles problems with incompressible two-phase flows in bubble columns where degassing condition is used. For example, we use degassing condition if we don't want to include the freeboard region in simulation. This condition doesn't allow liquid to leave the domain. Now at initial time we have volume filled with incompressible liquid only. Because there no free space then how can we put incompressible gas there? I think that we must initialize gas volume fraction with value not equal zero. If so then what value should we use? I can't find info in CFX help.

I found presentation where it is said "Normally the continuous phase is not removed at a degassing boundary, but for an initial guess that has zero volume fraction for the dispersed phase, some must be removed to make room for the entering dispersed phase". What does "some must be removed" mean exactly? Should I just set gas volume fraction, for example = 0.01 in the domain or maybe I should make it dependent on height?
Antanas is offline   Reply With Quote

Old   April 1, 2014, 14:32
Default
  #2
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by Antanas View Post
Should I just set gas volume fraction, for example = 0.01 in the domain or maybe I should make it dependent on height?
No, you should have an outlet for the continuous phase.

Is the outlet with the degassing condition the only outlet in your domain? There is no other way for the liquid to leave (an opening, for example)? If that's the case, CFX should diverge, because you're breaking the volume conservation equation.

The presentation you mentioned is talking about the fact that, if your initial condition states that there is no gas in your domain and at t=0 you start pumping in gas, the liquid should leave the domain, that is, "(...) some [continuous phase] must be removed to make room for the entering dispersed phase (...)".
brunoc is offline   Reply With Quote

Old   April 1, 2014, 22:00
Default
  #3
Member
 
Join Date: Feb 2011
Posts: 85
Rep Power: 6
Antanas is on a distinguished road
Quote:
Originally Posted by brunoc View Post
No, you should have an outlet for the continuous phase.

Is the outlet with the degassing condition the only outlet in your domain? There is no other way for the liquid to leave (an opening, for example)? If that's the case, CFX should diverge, because you're breaking the volume conservation equation.

The presentation you mentioned is talking about the fact that, if your initial condition states that there is no gas in your domain and at t=0 you start pumping in gas, the liquid should leave the domain, that is, "(...) some [continuous phase] must be removed to make room for the entering dispersed phase (...)".
Have you seen "Gas-Liquid Flow in an Airlift Reactor" tutorial in CFX help?
There is only one outlet. This outlet is with degassing condition option. And volume fractions are initialized with values 1 for water and 0 for air, so no continuous phase removed to make room for the entering dispersed phase. Solver doesn't diverge.
Antanas is offline   Reply With Quote

Old   April 2, 2014, 10:39
Default
  #4
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by Antanas View Post
Have you seen "Gas-Liquid Flow in an Airlift Reactor" tutorial in CFX help?
There is only one outlet. This outlet is with degassing condition option. And volume fractions are initialized with values 1 for water and 0 for air, so no continuous phase removed to make room for the entering dispersed phase. Solver doesn't diverge.
Just saw it. Maybe CFX is doing some weird magic in the background. :P

I think that the reason the tutorial doesn't crash is related to how the inlet is set. It has 25% air @ 0.3 m/s and 75% water @ 0.0 m/s. Effectively, there is no water coming in.

I think the idea is to represent a grid, where the flow area is smaller then the total grid area, such that a higher velocity is achieved by the gas. But I'd have to take a better look at the equations to find out how this works out numerically, that is, setting a multiphase inlet where one fluid enter with a volfrac of 0.25 and the other with 0.0.

On this same tutorial, if you set the air.vf to 1 and try to run it, CFX crashes.
brunoc is offline   Reply With Quote

Old   April 3, 2014, 00:33
Default
  #5
Member
 
Join Date: Feb 2011
Posts: 85
Rep Power: 6
Antanas is on a distinguished road
Quote:
Originally Posted by brunoc View Post
Just saw it. Maybe CFX is doing some weird magic in the background. :P

I think that the reason the tutorial doesn't crash is related to how the inlet is set. It has 25% air @ 0.3 m/s and 75% water @ 0.0 m/s. Effectively, there is no water coming in.

I think the idea is to represent a grid, where the flow area is smaller then the total grid area, such that a higher velocity is achieved by the gas. But I'd have to take a better look at the equations to find out how this works out numerically, that is, setting a multiphase inlet where one fluid enter with a volfrac of 0.25 and the other with 0.0.

On this same tutorial, if you set the air.vf to 1 and try to run it, CFX crashes.
We definitely must do something to avoid solution divergence. I set air volume fraction at inlet to 1 and changed air inlet velocity to 1.2 [m/s]. Solution diverged. Then I set initial air volume fraction in whole domain to 0.01 - solution diveged again. Then I set initial air volume fraction in riser to 0.01 and 0 in downcomer (this is suggested in the tutorial to improve convergence). Solution converged.

I found this suggestions in Fluent help:
Quote:
No inputs are necessary for the degassing boundary condition. However, the initial condition for volume fraction must be set appropriately. It is recommended that the gas phase volume fraction be initialized with a non-zero value smaller than the steady-state gas holdup value.
But I tried to use this when modeled simple bubble column in transient. Convergence criteria (RMS<1e-5, cons. target = 0.01) were not achieved within 20 coef. loops. And linear solver constantly showed fails (F).
Antanas 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
UDF for degassing boundary condition peaker007 Fluent UDF and Scheme Programming 4 December 20, 2012 08:33
Volume of Flow Rate (VFR) boundary condition therockyy FLOW-3D 0 May 23, 2011 14:19
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 10:33.