[TerryNiu]

Hi friends. I'll say thanks first. Because as a new elarner of CFX maybe I could ask some stupid questions that I don't realize.

I have a problem here for multiphase flow simulation. The model is a simple cyclone separator, the fluid are natural gas,water and oil, one inlet and two outlets(one is on the top and the other one is at the bottom). I set the buoyancy model and homogeneous turbulence model. Others are all default. The volume fraction proportion of three phase is about 0.05:0.4:0.55

Then I meet the common overflow error warnning, CFX suggests me to set an opening boundary for these two outlet. But the opening boundary of multiphase has a Fluid Values Panel which must set the Volume Fraction of each phase. However, the phase distribution is just the result which I want to simulate.So why opening boundary for multiphase simulation must set Volume Fraction of each phase?

I know there must be some error of my domain setting and boundary settings, can anyone point me out where is it?

[Gert-Jan]

It is all about backflow.

The pressure at your outlets can be such that the solver want material to enter your domain through the outlet. Say you have an outlet pressure of 0 Pa (relative) and the solver calculates -100 Pa close to the outlet, then naturally, material will flow form your outlet to this low pressure point.

Now, if you have an Outlet as boundary condition, then CFX will build partly an artificial wall at the location where material tends to flow into your domain. As a result, material will only leave through the part of the outlet that is still open..
If you have an opening, CFX will let material enter your domain. But then it certainly needs to know what is behind your outlet. For this reason, it wants you to provide this info in terms of volume fractions.

So, the options are:
- use an outlet then you don't have bother. Make sure the outlet is far away from the separation process so the artificial wall does not inflluence your separation.
- use an opening and set reasonable values (0 gas at the bottom outlet, 0 water at the top, oil somewhere in between). In general you can safely provide these numbers as long as (again) your opening is far away from your separation process. And you have to make sure that you evaluate the performance of your cyclone upfront of the opening, at a location where the influence of the outlet values can be ignored.
- Extend your geometry to a location where you know the values. To a knock-out drum for example.

[TerryNiu]

Originally Posted by Gert-Jan

It is all about backflow.

The pressure at your outlets can be such that the solver want material to enter your domain through the outlet. Say you have an outlet pressure of 0 Pa (relative) and the solver calculates -100 Pa close to the outlet, then naturally, material will flow form your outlet to this low pressure point.

Now, if you have an Outlet as boundary condition, then CFX will build partly an artificial wall at the location where material tends to flow into your domain. As a result, material will only leave through the part of the outlet that is still open..
If you have an opening, CFX will let material enter your domain. But then it certainly needs to know what is behind your outlet. For this reason, it wants you to provide this info in terms of volume fractions.

So, the options are:
- use an outlet then you don't have bother. Make sure the outlet is far away from the separation process so the artificial wall does not inflluence your separation.
- use an opening and set reasonable values (0 gas at the bottom outlet, 0 water at the top, oil somewhere in between). In general you can safely provide these numbers as long as (again) your opening is far away from your separation process. And you have to make sure that you evaluate the performance of your cyclone upfront of the opening, at a location where the influence of the outlet values can be ignored.
- Extend your geometry to a location where you know the values. To a knock-out drum for example.

Thanks a lot, I'll try these good suggestions later!