Hi.

I'm trying to redo a CFD simulation done in FLUENT using CFX in stead. It has to do with a hydro cyclone with water/air with an air core in the middle. The Fluent approach was using a Mixture Model in the multiphase options instead of the more difficult Euler-Euler approach. How do I set the corresponding settings in CFX. Does it have a "mixture Model" and what it's "name"?

Thanks

Hi,

I am not familiar with the mixture model in Fluent so I don't know exactly what physics it models, but in CFX if the free surface stays sharp and there is minimal bubbly or frothy areas you will find the homogeneous multiphase model with the coupled multiphase solver. An example of setting this up is the free surface flow over a bump tutorial example.

If you have droplet or bubble regions which are of significance you will need to consider an inhomogeneous model.

Glenn Horrocks

OK, thanks. I will try that. There is no bubble regions, just one "big" air core in the centre. Do I treat both phases as continous fluids?

I don't think you want to do this as a homogeneous mixture. Although you'll have a free surface, the gas phase needs to be able to move relative to the liquid phase (and vice versa) in order to separate into a gas and liquid region. A homogeneous model assumes the two fluids share the same velocity field, which will not allow this.

That said, you could potentially run this using the Algebraic Slip Model, which requires the gas and liquid phases to be defined as two components of a multi-component fluid. ASM adds a "slip velocity" to allow relative motion between the components. The general assumption is that the slip velocity is low, so you may have problems if it isn't.

My 2c, use inhomogeneous (Eularian-Eularian) multiphase.

-CycLone

Hi,

Cyclone's comments just goes to show that the choice of multiphase model is rarely obvious! It needs to be carefully considered based on the important physics of the model.

However I still think based on what has been described the homogeneous multiphase model should work well. It does not allow relative slip between the gas and liquid phases but if all points in the domain are either entirely liquid or entirely gas (as it is in a sharp free surface model) then relative slip is not required.

Maybe run both a homogeneous and inhomogeneous model and see if it results in any difference. The homogeneous model will certainly run a lot faster.

Glenn Horrocks

Thank you both of you. I think I have what I need.

Hi Glen,

I think the slip will be important in this case. The whole point of a cyclone is to separate low density air from high density air or water. A core will develop, but only after the air has separated from the water coming in (or vice versa). If you have a mixed air/water inlet condition and use homogeneous multiphase your core will not develop.

-CycLone

Hi,

Yes, I totally agree with your comment. Providing there is a period when the air and water are mixed then an inhomogeneous model is required. If not then homogeneous is OK. It will depend on the details of the set up.

Glenn Horrocks

So if the particles I want to separate are in the water part, and the air core just forms due to the outlets being open to atmosphere, which settings are the optimal? - FLuentSwitch

What are you trying to separate from the water? You haven't mentioned particles until now. Is air mixed with the water at the inlet?

It's really quite simple. If the air and water are mixed at some point and need to separate, you need to have either full multiphase (so each has its own velocity field and can move in different directions) or you need to set up a multi-component mixture and turn on the Algebraic Slip Model.

Homogeneous multiphase is only appropriate if the drag is so high that the two phases move together, or if the two phases are immiscible and form a free surface.

-CycLone

Hi Cyclone. I'm sorry if I have let anything vital out of the conservation, but my first problem was with regards to the water and air in a hydrocyclone. I had not set my mind on the particles yet at that moment.

But the whole story is that water and particles (7% VF) enter at the inlet to the cyclone. The under- and overflow openings are open to atmosphere and quickly an air core will form. Just like in the bath tub. Particles should then separate out in the bottom together with only 20% of the water (experimental says a 20/80 split between under and overflow. My Idea was, and still is, to determine the multiphase flow field of water and the air core, and finally adding the particles at the end, only as a one-coupling with the flow. that worked promising for the old Fluent calculations so it should hopefully work fine for me also. I have succeeded in creating the air core in the middle, using the BSL Reynold Stress turbulence model, but all the particles unfortunately exist at the bottom, even though the particles are as small as 1 micron. Thanks

just for reference... Fluent mixture model = cfx asm model.

Hi FluentSwitch,

1) So finally what model did you use for water/air so that air core could develop? Algebric slip model or full Euler-Euler model?

2) Do you specify 'opening' type boundary conditions at both the outlets of your cyclone?

3) I have been facing the same problem that all the particles were being collected at the bottom...that is not possible at all, otherwise there will not be any need to hire design engineers....I was taking fully developed water flow field and tracking particles in steady state for 1 or 2 iterations? what was your procedure..may be we can find out the right way and help each other...

Thanks, KK

I actually tried both models, but very little it helped. I still get all the particles to separate out of the bottom. It irritates me a lot, since Fluent had no problem in establish a well separation efficiency curve. The way fluent did this was using, as I said before, a mixture model. Then run in transient for several seconds and then applying the particles which one only 1-way coupled. I have done similar, but without success...

[vga67]

Hi everybody,

I want to simulate a water-air bubble model in CFX. Is mixture model in CFX a good choice for modeling such case?
thank you
Hamid