[Aurelien Thinat]

Hello everyone,

I'm looking for a way to model a degassing boundary condition for twoPhaseEulerFoam solver.

The case :
Air bubbles are injected at the bottom of a water tank, free surface at the top.

As far as I know I have three options :

1) Compute the interface of the free surface.

2) Slip wall at the BC and add a negative source term in the alpha equation and pressure equation at the last cell before the BC. Something like : S = - alpha/time_step.
How should I modify the momentum equation ? I guess I have to include a source term in the momentum equation too.

3) Find a boundary condition setup as there is on Fluent or CFX. But I could'nt find any litterature on this subject.

I have already tested a setup and I'm not really happy with the result:
p : fixedValue
alpha : inletOutlet
Ua : zeroGradient
Ub : surfaceNormalFixedValue : 0

Do you have any tips on how to manage this kind of problem ?

[enoch]

I'm also looking for this BC available for twoPhaseEulerFoam.
That'd be very appreciated if you give me some idea on how to implement this BC or share a source code with me.^^
Thanks in advance for your big help.

[Aurelien Thinat]

Hi Enoch,

There are 2 ways of dealing with that as far as I know :

- slip wall for the continuous phase and free stream for the dispersed one. I had few problems with this in OpenFoam-2.1.1. Since OF-2.2 release, it seems ok.

- source term applied at the first cells near your degassing BC. At each time step you extract the mass of the dispersed phase (something like : alpha 1 * rho1 / DT). You'll have to modify the pressure equation and add source terms in the momentum equations. I'm not fond of this but well...it does the trick.

[jp279]

Originally Posted by Aurelien Thinat

Hi Enoch,

There are 2 ways of dealing with that as far as I know :

- slip wall for the continuous phase and free stream for the dispersed one. I had few problems with this in OpenFoam-2.1.1. Since OF-2.2 release, it seems ok.

- source term applied at the first cells near your degassing BC. At each time step you extract the mass of the dispersed phase (something like : alpha 1 * rho1 / DT). You'll have to modify the pressure equation and add source terms in the momentum equations. I'm not fond of this but well...it does the trick.

Hi Aurelien,

About the first option - Slip wall for the continuous phase is understood, but why free stream for the dispersed phase? I mean one can use pressureInletOutletVelocity or inletOutlet too.

About the second option - Do you have any reference for this option? I haven't found much about making changes in the source code to implement degassing BC (except for the CFX Tutorial on UDFs, which does something similar to what you mentioned above).

[cdegroot]

I wasn't able to find anything online for a degassing boundary condition in OpenFOAM, so I wrote a degassing source using fvOptions. Here's a link in case anyone finds it useful: https://bitbucket.org/cdegroot/degassingsourcefvoptions