|
[Sponsors] |
Volume fractions initialization when using degassing boundary condition |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 1, 2014, 00:23 |
Volume fractions initialization when using degassing boundary condition
|
#1 |
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 |
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: 277
Rep Power: 21 |
Quote:
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: 496
Rep Power: 18 |
Quote:
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: 277
Rep Power: 21 |
Quote:
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: 496
Rep Power: 18 |
Quote:
I found this suggestions in Fluent help: Quote:
|
|||
November 23, 2015, 12:54 |
degassing boundary condition
|
#6 |
Member
azna
Join Date: Nov 2012
Posts: 30
Rep Power: 13 |
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, 16:11 |
|
#7 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
It sounds like your problem is more fundamental than just the details of the degassing boundary.
|
|
November 23, 2015, 17:52 |
|
#8 | |
Member
azna
Join Date: Nov 2012
Posts: 30
Rep Power: 13 |
Quote:
The redults of degassing are not correct around 10 cm to the watersurface. Below this, the results are good. |
||
November 23, 2015, 21:36 |
|
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
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. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Wind turbine simulation | Saturn | CFX | 58 | July 3, 2020 01:13 |
UDF for degassing boundary condition | peaker007 | Fluent UDF and Scheme Programming | 5 | November 23, 2015 12:55 |
Volume of Flow Rate (VFR) boundary condition | therockyy | FLOW-3D | 0 | May 23, 2011 14:19 |
[blockMesh] Axisymmetrical mesh | Rasmus Gjesing (Gjesing) | OpenFOAM Meshing & Mesh Conversion | 10 | April 2, 2007 14:00 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 15:55 |