Hello,

I am simulating a piece of the ocean where there is a thin layer of oil (5mm) at the surface. Water current is 1m/s. Same as the oil. I have a wall which is 1 meter high and which is supposed to stop the oil. I am interested in what's happening around the wall when the oil hits the wall. Basically, when does the oil flow under the wall ?

So I have three materials : - Oil - Water - Air

In the fluid pairs, I have chosen the "Open Surface" model for interface transfer for the Water-Air and Oil-Air pairs. But I am little unsure about the Oil-Water pair. Should I use the "Open Surface" or the "Mixture Model" ? If so What Interface Length scale should I use ?

Regards,

Hervé

Hi,

I assume the air, oil and water are all immiscible. This sounds like a free surface simulation where you actually have three phases, not just the normal 2.

Just set the 3 pairs up with the same models as for free surface flows, but setting different surface tension, wall wetting angles or whatever are the relevant properties.

Glenn Horrocks

Hi Glenn,

thanks for your answer

About the surface tension coefficient, I had set 0.073 [N m^-1] for the couple Air-Water and 0.022 [N m^-1] for the couple Air-Oil. Is this correct ? And how can I get the surface tension coefficient for my couple Oil-Water ?

Regards,

Hervé

Hi,

As a first estimate I would use 0.073-0.022=0.051 N/m until you know better. This is based on the surface energy of air not being significant compared to water or oil.

Glenn Horrocks

Thanks again for your answers Regards, Hervé

[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

[JuPa]

Originally Posted by 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

The difference between the free surface model, mixture model, and the particle model is how they treat the interfacial area density. Determining the correct interfacial area density is crucial since in mutliphse flows, the conservation equations are a function of the area density.

The free surface model only considers the interfacial area density to be the gradient of the volume fraction normal to the interface. It's designed for free surface applications. So using it to model air bubbles in water isn't a good choice.

The particle model is more reasonable. Its formulation for area density considers the a constant multiplied by the volume fraction divided by some sauter mean particle or bubble diameter which you specify. It's designed for bubbly flows.

The mixture model is a red herring in that it's not really a model which is given to you, it's more of a model which you give to the solver. i.e. its formulation for the area density is a symmetric one: the product of the two volume fractions divided by some length scale which you specify. This length scale varies from application to application, and in reality will not be a constant but a function of the flow regime. You need to determine what this is.

For bubble cases with the top free surface modelling as a degassing BC use the particle model. For bubbles rising, and breaking the free surface, and coalescence and breakup use the mixture model. For pure free surface problems use the free surface model.

[ghorrocks]

Nice answer Mr CFD. I will just add that free surface models are used when you want to directly resolve the gas/liquid interface in your simulation. This means for most applications you are only going to be able to model 1 or 2 bubbles. If 1 or 2 bubbles is good then use the free surface model.

For many industrial bubbly flows you have thousands or millions of bubbles. This means the free surface model is not suitable and means you should consider the particle and mixture models as explained in the previous post.

[vga67]

Hi

Thanks both of you Mr CFD and Glenn

in fact my case is a single air bubble in water. when I apply sinusoidal pressure at the water boundary the bubble starts to expand and then when the pressure inside the bubble decreases and the bubble has reached its maximum radius it will collapse catastrophically. I have done this in CFX with mixture model and the results are fairly good but my supervisor says that the mixture model is not an appropriate model for simulating this case. Do you agree with him???

Hamid

[JuPa]

Originally Posted by vga67

Hi

Thanks both of you Mr CFD and Glenn

in fact my case is a single air bubble in water. when I apply sinusoidal pressure at the water boundary the bubble starts to expand and then when the pressure inside the bubble decreases and the bubble has reached its maximum radius it will collapse catastrophically. I have done this in CFX with mixture model and the results are fairly good but my supervisor says that the mixture model is not an appropriate model for simulating this case. Do you agree with him???

Hamid

Are your boundaries closed?

If you have a single bubble then the particle model may be sufficient. However you haven't described your problem well, and you haven't included any pictures so it's hard to give advice.

Try it with the particle model and compare to your results with the mixture model. Do you have experimental data?

I take it the bubble is water vapour since it collapses back into the water? If this is the case is the problem non isothermal? I.e. are you modelling the energy equation with some condensing thermal phase change?






Please take the time to explain what you're doing.

[vga67]

hi
Dear Mr CFD
thanks for your patience. my case is exactly " Sonoluminescence ". unfortunately I have no time to test the particle model. I have already gotten the results of my work with mixture model with a time step of """1e-12""" and it takes a long time to test the case with the particle model. the results are fairly in agreement with the experimental data. but my supervisor doesn't accept simulating with mixture model. I ask you about the mixture model because I needed a reason to say to my supervisor that what I have done is right. As I see I have chosen the model wrongly. thank you ...

Hamid