How should I model the effect of a surfactant in CFX?

s-rod · October 7, 2015, 09:05

Hi,

I need to create an emulsion between air and a liquid using a static mixer. However, in the real system we add a surfactant that does not allow the air to get out of the emulsion once it mixes with the liquid.

We checked the rhelogy of the system taking into acount this surfactant and it is exactly the same that we had with no surfactant at all.

If a try to simulate this system without surfactant evidently the air will get out of the mix because of its lower density. However, i can't eliminate the effect of gravity because I need to evaluate the air flow field in one specific region of my system.

My question is: How can I achieve that my air and liquid mix each other and the air does not go to the upper part of my simulation considerating all what I've already explained?

ghorrocks · October 7, 2015, 19:06

Rather than turning off physics which is present in the real system (ie gravity acting on the air bubbles), a better approach is to add the physics which stops gravity separating the bubbles out. That could be many effects:
* a mixing or turbulent mixing effect
* Brownian motion (if your bubbles are really small)
* A chemical effect where the bubbles repel each other
* The separation time of the bubbles is long enough that it is not significant
* Or many other factors.

Once you know what stops the bubbles separating then you add that physics to your model and your model is correctly modelling the important physics.

So, over to you - what stops gravity separating out your bubbles?

s-rod · October 11, 2015, 00:20

Glen thank you so much. Not only for this answers but for the other times where you have really help me.

Let me briefly explain to you the phenomena.

I need to form a stable emulsion between the air and a liquid. What we do in the reality is to force them to flow through a static mixer and add a powder that maintains the gas in a stable solution within the liquid.

The molecular structure of this powder has two parts. One of them is soluble in the liquid (it resembles the liquid molecular identity) and the other part is like air in structure (so it's soluble in air). What happens when we add it is that it places itself in the interphase that forms between the liquid (continuos phase) and the air (dispersed phase) and, the part of the powder molecule that resembles the liquid places itself in the liquid and the other part get placed in the air, resulting in a lower superficial tension than the one we had before the powder adding operation.

However, the original surface tension was neglected for me in the first simulation I did (my preliminar simulation) so, setting a lower superficial tension value is not a way I can take.

Graphically speaking, what we have seen is that the powder forms a film on the small air bubbles surface, covering the air zone and not allowing it to float as it would do normally.

Physically speaking, I just can think that when the surfactant places itself where I've already told you, it creates a force that can't be defeated by the small bubble lift and that is what allows the air to maintain in solution. However, if this is the case, obtaining the value of this force to use it in my momentum equations will not be really easy.

I hope this brief description allows you to better understand what the problem is, and help to think of the best approach for modeling this system.

I want to express my gratitude to you for all your help, again

ghorrocks · October 11, 2015, 05:15

You have described a surfactant. That will lower the local surface tension but should not have any effect on the overall net force on the bubble. So the only net force I can see on the bubble is gravity, and then drag once it starts moving.

Quote:

it creates a force that can't be defeated by the small bubble lift and that is what allows the air to maintain in solution.

So that is the crux of it. What is the "force"? I will make a big assumption and presume Yoda is not playing a role here.

...... OK, just had a bit of a think - this is an emulsion, right? In most emulsions the particles are very small - microns to nanometers. Is this is the case in your application? If this is the case then the bubbles are too small to be thought of as a multiphase flow, and the multiphase model is not appropriate. A more appropriate model is an additional variable or a multicomponent fluid approach. These models do not allow interphase slip and you won't get buoyancy effects.

s-rod · October 11, 2015, 11:12

The liquid I'm using is also an emulsion (liquid-liquid) Glen, but I treated it as a pure component for simplicity.

The liquid/air is an emulsion too, but only when the air bubble reaches the small sizes you just said.

It is important to consider that the air enters the system before the static mixer, through a device that I need to evaluate too, because people who designed it just used the first configuration that they though of. In this region, is possible that the air does not form the small bubbles needed to have the trapping effect of the surfactant so I would need the multiphase model, at least in this region. For that reason i first thought of the multiphase method.

ghorrocks · October 11, 2015, 18:27

The multiphase models only apply down to a certain size range. Typically that is a few microns for bubbles and particle as below this size you don't get interphase slip and molecular effects like Brownian motion become important (and the multiphase model does not have Brownian motion). So when the particles/bubble are smaller than a few microns you do not use the multiphase model but move to models like multicomponent models.

So yes, you have a multiphase flow, but the multiphase model implemented in CFX which is not applicable to your flow. You have to model these multiphase flow with a different model which is appropriate for small particles. This is the root cause of your problems in this model.

aee · November 5, 2015, 17:10

Simon,
I have a similar issue (although I am not using CFX). In pickering emulsions, interfacial tension alone does not describe the coalescence of bubbles/droplets. The surfactant in your case (and my case) also provides a steric hindrance to coalescence.

If anyone has found a useful way of modeling that, I would love to hear of it.

camad93 · November 9, 2019, 22:00

Quote:

Originally Posted by aee

Simon,
I have a similar issue (although I am not using CFX). In pickering emulsions, interfacial tension alone does not describe the coalescence of bubbles/droplets. The surfactant in your case (and my case) also provides a steric hindrance to coalescence.

If anyone has found a useful way of modeling that, I would love to hear of it.

Hi Sir,
Have found the way to model it? Would appreciate it if you could share it with me/us. Thanks in advanced!

aee · November 9, 2019, 22:07

I haven't gotten around to implementing it, but I always thought it would most easily be done as part of an IATE solver. I would also like to see a better IATE solver in openFoam (two-way). I am not doing CFD now, but would make use of such a model if available.

camad93 · November 10, 2019, 02:05

Quote:

Originally Posted by aee

I haven't gotten around to implementing it, but I always thought it would most easily be done as part of an IATE solver. I would also like to see a better IATE solver in openFoam (two-way). I am not doing CFD now, but would make use of such a model if available.

I see, but is there any possibility that I can simulate the emulsion (i.e., dispersed flow of oil-water with emulsion) using IATE solver? and to see the emulsion particles down to nano or micro scale?

Thanks in advanced aee!

aee · November 10, 2019, 02:32

No. Numerical methods can't do nano scale and macro scale at the same time. You can simulate a sample of a few thousand or tens of thousands droplets being carried in a flow (lagrangian solver). If you want a droplet size distribution, you have a few choices, all of which are computationally expensive and make simplifying assumptions. What you choose depends on exactly what aspect of the emulsion you are trying to model. The IATE model in openFoam was limited to light dispersed phase in a heavier continuous phase, although I have used it to model water in oil emulsions by inverting gravity.
Interfoam can simulate two droplets coalescing (without surfactants).

aee · November 10, 2019, 02:38

To be clear, a numerical model with 1 million cells can be 100x 100x100 cells, which is not very high resolution. If the shape is 10 cm wide, the cells might be 1 mm wide. If the emulsion has droplets 0.1 mm diameter, they are too small to model individually.

camad93 · November 10, 2019, 04:18

Quote:

Originally Posted by aee

To be clear, a numerical model with 1 million cells can be 100x 100x100 cells, which is not very high resolution. If the shape is 10 cm wide, the cells might be 1 mm wide. If the emulsion has droplets 0.1 mm diameter, they are too small to model individually.

Thank you so much for your great explanation!! Now I get the idea. Thank you again aee.

October 7, 2015, 09:05	How should I model the effect of a surfactant in CFX?	#1
s-rod New Member Simon Rodriguez Join Date: Nov 2014 Posts: 13 Rep Power: 11	Hi, I need to create an emulsion between air and a liquid using a static mixer. However, in the real system we add a surfactant that does not allow the air to get out of the emulsion once it mixes with the liquid. We checked the rhelogy of the system taking into acount this surfactant and it is exactly the same that we had with no surfactant at all. If a try to simulate this system without surfactant evidently the air will get out of the mix because of its lower density. However, i can't eliminate the effect of gravity because I need to evaluate the air flow field in one specific region of my system. My question is: How can I achieve that my air and liquid mix each other and the air does not go to the upper part of my simulation considerating all what I've already explained?

November 9, 2019, 22:07	Surfactant modeling	#9
aee Member Andrew Eisenhawer Join Date: Nov 2012 Location: Alberta, Canada Posts: 35 Rep Power: 13	I haven't gotten around to implementing it, but I always thought it would most easily be done as part of an IATE solver. I would also like to see a better IATE solver in openFoam (two-way). I am not doing CFD now, but would make use of such a model if available.

November 10, 2019, 02:32		#11
aee Member Andrew Eisenhawer Join Date: Nov 2012 Location: Alberta, Canada Posts: 35 Rep Power: 13	No. Numerical methods can't do nano scale and macro scale at the same time. You can simulate a sample of a few thousand or tens of thousands droplets being carried in a flow (lagrangian solver). If you want a droplet size distribution, you have a few choices, all of which are computationally expensive and make simplifying assumptions. What you choose depends on exactly what aspect of the emulsion you are trying to model. The IATE model in openFoam was limited to light dispersed phase in a heavier continuous phase, although I have used it to model water in oil emulsions by inverting gravity. Interfoam can simulate two droplets coalescing (without surfactants). camad93 likes this.

November 10, 2019, 02:38		#12
aee Member Andrew Eisenhawer Join Date: Nov 2012 Location: Alberta, Canada Posts: 35 Rep Power: 13	To be clear, a numerical model with 1 million cells can be 100x 100x100 cells, which is not very high resolution. If the shape is 10 cm wide, the cells might be 1 mm wide. If the emulsion has droplets 0.1 mm diameter, they are too small to model individually. camad93 likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
CFX Free surface Model	jthiakz	CFX	1	July 15, 2015 19:29
Periodic model for ansys cfx	jayendrajpatel	CFX	3	January 21, 2015 16:44
How to use non-equilibrium thermal model for porous medium in Ansys CFX 13.0?	Chander	CFX	3	November 28, 2011 14:26
How to use the competing reaction model in CFX 11	NewCoalman	CFX	0	May 5, 2008 03:15
Use of 1 equation turbulence model in CFX 4.3	Niels Deen	CFX	0	July 19, 2000 08:50

October 7, 2015, 19:06		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Rather than turning off physics which is present in the real system (ie gravity acting on the air bubbles), a better approach is to add the physics which stops gravity separating the bubbles out. That could be many effects: * a mixing or turbulent mixing effect * Brownian motion (if your bubbles are really small) * A chemical effect where the bubbles repel each other * The separation time of the bubbles is long enough that it is not significant * Or many other factors. Once you know what stops the bubbles separating then you add that physics to your model and your model is correctly modelling the important physics. So, over to you - what stops gravity separating out your bubbles?

October 11, 2015, 00:20		#3
s-rod New Member Simon Rodriguez Join Date: Nov 2014 Posts: 13 Rep Power: 11	Glen thank you so much. Not only for this answers but for the other times where you have really help me. Let me briefly explain to you the phenomena. I need to form a stable emulsion between the air and a liquid. What we do in the reality is to force them to flow through a static mixer and add a powder that maintains the gas in a stable solution within the liquid. The molecular structure of this powder has two parts. One of them is soluble in the liquid (it resembles the liquid molecular identity) and the other part is like air in structure (so it's soluble in air). What happens when we add it is that it places itself in the interphase that forms between the liquid (continuos phase) and the air (dispersed phase) and, the part of the powder molecule that resembles the liquid places itself in the liquid and the other part get placed in the air, resulting in a lower superficial tension than the one we had before the powder adding operation. However, the original surface tension was neglected for me in the first simulation I did (my preliminar simulation) so, setting a lower superficial tension value is not a way I can take. Graphically speaking, what we have seen is that the powder forms a film on the small air bubbles surface, covering the air zone and not allowing it to float as it would do normally. Physically speaking, I just can think that when the surfactant places itself where I've already told you, it creates a force that can't be defeated by the small bubble lift and that is what allows the air to maintain in solution. However, if this is the case, obtaining the value of this force to use it in my momentum equations will not be really easy. I hope this brief description allows you to better understand what the problem is, and help to think of the best approach for modeling this system. I want to express my gratitude to you for all your help, again

October 11, 2015, 11:12		#5
s-rod New Member Simon Rodriguez Join Date: Nov 2014 Posts: 13 Rep Power: 11	The liquid I'm using is also an emulsion (liquid-liquid) Glen, but I treated it as a pure component for simplicity. The liquid/air is an emulsion too, but only when the air bubble reaches the small sizes you just said. It is important to consider that the air enters the system before the static mixer, through a device that I need to evaluate too, because people who designed it just used the first configuration that they though of. In this region, is possible that the air does not form the small bubbles needed to have the trapping effect of the surfactant so I would need the multiphase model, at least in this region. For that reason i first thought of the multiphase method.

October 11, 2015, 18:27		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	The multiphase models only apply down to a certain size range. Typically that is a few microns for bubbles and particle as below this size you don't get interphase slip and molecular effects like Brownian motion become important (and the multiphase model does not have Brownian motion). So when the particles/bubble are smaller than a few microns you do not use the multiphase model but move to models like multicomponent models. So yes, you have a multiphase flow, but the multiphase model implemented in CFX which is not applicable to your flow. You have to model these multiphase flow with a different model which is appropriate for small particles. This is the root cause of your problems in this model.

November 5, 2015, 17:10		#7
aee Member Andrew Eisenhawer Join Date: Nov 2012 Location: Alberta, Canada Posts: 35 Rep Power: 13	Simon, I have a similar issue (although I am not using CFX). In pickering emulsions, interfacial tension alone does not describe the coalescence of bubbles/droplets. The surfactant in your case (and my case) also provides a steric hindrance to coalescence. If anyone has found a useful way of modeling that, I would love to hear of it.