[Antanas]

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?

[brunoc]

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 (...)".

[Antanas]

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.

[brunoc]

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.

[Antanas]

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:

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).

[azna]

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

[ghorrocks]

It sounds like your problem is more fundamental than just the details of the degassing boundary.

[azna]

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.

[ghorrocks]

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.