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?

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.

Cheers

Hi

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

good luck

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.

Goodluck,

vivek