# Volume fractions initialization when using degassing boundary condition

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 1, 2014, 00:23 Volume fractions initialization when using degassing boundary condition #1 Senior Member   Join Date: Feb 2011 Posts: 274 Rep Power: 7 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?

April 1, 2014, 14:32
#2
Senior Member

Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 250
Rep Power: 12
Quote:
 Originally Posted by Antanas 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 (...)".

April 1, 2014, 22:00
#3
Senior Member

Join Date: Feb 2011
Posts: 274
Rep Power: 7
Quote:
 Originally Posted by brunoc 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.

April 2, 2014, 10:39
#4
Senior Member

Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 250
Rep Power: 12
Quote:
 Originally Posted by Antanas 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.

April 3, 2014, 00:33
#5
Senior Member

Join Date: Feb 2011
Posts: 274
Rep Power: 7
Quote:
 Originally Posted by brunoc 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).

 November 23, 2015, 13:54 degassing boundary condition #6 New Member   azna Join Date: Nov 2012 Posts: 26 Rep Power: 5 Hi, I'm working on a bubble column. I was wondering that how can I modify settings in the degassing boundary condition ? close to the water surface, it under predicts velocity for both air and water. Is there any way that I can fix this problem near the water surface ? the flow pattern with degassing boundary is correct however, velocities near the water surface is very low comparing with experimental values. Thanks a lot

 November 23, 2015, 17:11 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,295 Rep Power: 88 It sounds like your problem is more fundamental than just the details of the degassing boundary.

November 23, 2015, 18:52
#8
New Member

azna
Join Date: Nov 2012
Posts: 26
Rep Power: 5
Quote:
 Originally Posted by ghorrocks It sounds like your problem is more fundamental than just the details of the degassing boundary.
I din't think so, if I consider the boundary condition as pressure outlet where the pressure equals to atmospheric pressure, the error between experimental and Fluent results are less than 10% , however the flow pattern with degassing is better.

The redults of degassing are not correct around 10 cm to the watersurface. Below this, the results are good.

 November 23, 2015, 22:36 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,295 Rep Power: 88 If you are running this in Fluent then try the Fluent forum for answers specifically on Fluent. This is the CFX forum. Application of a pressure outlet can distort the flow near the boundary, especially if there is flow tangential to the boundary. So if this flow is inhibited then the cross flows at the surface will be artificially reduced. So I do not consider comparing these results to a pressure outlet a useful benchmark.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post peaker007 Fluent UDF and Scheme Programming 5 November 23, 2015 13:55 Saturn CFX 34 October 16, 2014 05:27 therockyy FLOW-3D 0 May 23, 2011 14:19 Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00 Mark CFX 6 November 15, 2004 16:55

All times are GMT -4. The time now is 03:37.

 Contact Us - CFD Online - Top