CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Particle Interaction is CFX; Adding Interparticle Attraction such as Van Der Waals

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 6, 2013, 16:02
Default Particle Interaction is CFX; Adding Interparticle Attraction such as Van Der Waals
  #1
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
*The title should read "Particle Interaction "IN" CFX; Adding Interparticle Attraction such as Van Der Waals"* I hate typo's

Hi All,

I have been playing around with CFX for my PhD project the last 2 months. I am modelling a machine which resembles a high speed mixer with a bottom mounted impeller. The real fluid I wish to simulate is water with a suspension of particles. So far, I have managed to get the CFX simulations to match up to the actual performance of the machine in the lab with water as a first test case (water in the real machine and CFX), and now by using a Herschel-Bulkley model to model the actual fluid this machine typically processes.

The real fluid used in the machine is a shear-thinning fluid with a yield stress. Yesterday, I set up a Eulerian-Eulerian simulation according to the CFX Manual with the suspended solid particles as a dispersed fluid according to the below excerpt from the manual:

"It is possible to model the motion of a large number of solid particles in a gas or a liquid as an Eulerian-Eulerian two phase flow. Examples occur in pneumatic conveying, sedimentation in rivers, and fluidized beds. For example, the two phases may be Water, the continuous fluid (Continuous Fluid), and Sand, the dispersed fluid (Dispersed Fluid).

In such problems, you should assign the solid phase a small insignificant molecular viscosity. This is permissible, as the physics are dominated by inter-phase drag and turbulence effects. The solid phase should be assigned free slip boundary conditions at walls.
"

The volume fraction of particles is ~ 7% and I am modelling them as 0.5mm spheres. My results are very interesting. The suspension in the simulation is showing shear-thinning behavior which is very good as does the real suspension I am approximating. I am also able to get the rotor power required to pump particles around the tank vs. straight water.

Does anyone know if it is possible to model an attraction force between the particles such as a Van Der Waals force? If this could be implemented in CFX, I could account for the yield stress behavior of the real suspension. I am really not sure where to start as the available variables in CFX don't seem to account for particle to particle interaction, but I could be wrong. Any suggestions would be greatly appreciated.

Frank

Last edited by FrankS; November 6, 2013 at 16:05. Reason: typo
FrankS is offline   Reply With Quote

Old   November 6, 2013, 17:44
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
To model your attraction you are going to have to describe it in a Eularian framework. Does it mean that concentration gradients tend to amplify, resulting in the particles clumping together in regions of high concentration and vacating regions of low concentration? If so you could implement this by a source term (with linearisation) but it would need a bit of thinking to get it to work.
ghorrocks is offline   Reply With Quote

Old   November 6, 2013, 18:58
Default
  #3
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
I was thinking that the attraction force between the particles would be inversely proportional to the distance between them. If I remember right, off the top of my head, the Van der Waals force varies by 1/(Distance between particles)^6. I would want to go for something like this.

You mention having a source dependent on concentration and I have also read a brief statement in the CFX manual concerning this. I am looking at the CFX help documentation at Bulk Sources as I write this. Implementing a source for particle interaction in a Eulerian sense is a head-scratcher for me.

Inserting a Bulk Source point in to each of my domains requires the specification of a coordinates for the source point. Since a bulk source depends on concentration, I suppose it would affect the whole domain equally? I would just need to avoid any dependence on any spatial coordinates. is this the right way to think?

As an aside, this CFX software is fantastically stable for multiphase stuff. I have three phase going, water, suspended particles, and air at the open surface and as an emulsion. CFX just always seems to converge.

I will look in to this more and keep posting. Perhaps my trials and tribulations will help other people who are new to this software like me. Thanks for the direction Mr. Horrocks.
FrankS is offline   Reply With Quote

Old   November 6, 2013, 19:13
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I would be thinking more along the lines of a momentum source on the particle fraction. The momentum source could "simply" be a function of the local concentration gradient. So this would push the momentum of the particle volume fraction in the direction of the steepest gradient.

This is pretty easy to implement conceptually. The X momentum source is just a function of the local X concentration gradient and likewise for Y and Z. Then this gets applied locally so you get a variable momentum source across the entire domain.
ghorrocks is offline   Reply With Quote

Old   November 7, 2013, 22:05
Default
  #5
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
I have been thinking about your suggestion to use a momentum source and I think I have come up with something that may work. I have been reading in the CFX help about Particle User Sources in User Fortran. One example in the help gives code for a volume-fraction dependent drag coefficient. As you know, I am trying to model fluid yield stress which, as everyone knows, is dependent on fluid shear stress.

I have read that "shear strain rate" is a variable available in CFX. I could return from a Particle User Source routine a shear strain rate dependent drag coefficient for the particles. I could have the routine return a large drag coefficient for low shear rates to mimic solidification. I could tune this coefficient to match the solidification seen in my experiments. I could incorporate an "if" statement to return a drag coefficient based on some criteria like Schiller-Naumann for higher shear rates. This seems logical to me.

It looks like, from the help documentation, that when CFX calls my user routine that it will adopt the calculated drag coefficient from the routine in place of a chosen method from the CFD-Pre GUI interface.

Thanks again for the direction ghorrocks. Putting me on to the idea of using a momentum source will be very helpful for me I predict.
FrankS is offline   Reply With Quote

Old   November 7, 2013, 22:20
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
But your approach will just generate a drag, ie it will just slow down the existing slip velocities. It cannot create attraction, so it cannot increase slip velocities.

Doesn't your description mean that this attractive force should generate a slip velocity?
ghorrocks is offline   Reply With Quote

Old   November 8, 2013, 01:07
Default
  #7
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
I think you are right. I would just reduce the slip velocity by placing an artificially high drag on the particles.

Let's say I were to add a momentum source as a function of shear strain rate. I guess what you are suggesting is to force the velocity of the particles to zero, like a Dirichlet Condition?

What I am not clear on now is how to apply a source to a domain. CFX gives the option for a point of a surface.

I'll look in to this.
FrankS is offline   Reply With Quote

Old   November 8, 2013, 01:12
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Can you explain why you think shear strain rate is the key variable? I do not understand that bit either

If a particle is being pulled in all directions by the forces from all the particles around then a net imbalanced force on the particle would be due to there being more particles on one side of the particle than the other. This would show up as a gradient in the VF. That is why I suggested using the gradient of the volume fraction as the key variable.
ghorrocks is offline   Reply With Quote

Old   November 8, 2013, 16:14
Default
  #9
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
I guess I was thinking that in the real experiments, it appears that the volume fraction in the majority of the tank is constant. Even the simulation results show the only significant increases in volume fraction occurs in area where the fluid takes a sudden change in direction which only occurs at the rotor and on the baffles near the rotor (I'll post a picture later. I am at a public PC at my library). These are areas of high shear whereas in the real world, the fluid solidifies in the areas of low shear at the very top of the tank.

I am trying to come up with an inexpensive way to simulate the behavior of a medium consistency pulp fiber suspension (~5% by mass). To model the real suspension with a billion fibers which flex and move in 6 degrees of freedom. I was excited by the results of my first particle simulation as it mimicked the behavior I have seen in the lab with the pulp except for the yield stress.

The machine I am modelling is a repulper, like a giant blender for paper recycling. My goal is to design a more energy efficient rotor. I have identified which rotor design features cause the recycled paper to be broken down to fibers using high speed video. Based on what I have found out, promoting a high volume concentration of particles in certain areas around the rotor is important for energy efficiency. This is why I want to develop a Eulerian-Eulerian model the fluid behavior; it will show me things that a Non-Newtonian model won't.

The part I am really struggling with is that CFX does not seem to model any particle interaction (collisions etc.) so I don't understand how to implement a momentum source to do this. There are no variables available for particle interaction. It seems like CFX only models the interaction between the particles and the continuous fluid phase. Implementing interparticle friction would also achieve my goal but again, it doesn't look like CFX models this. I agree with you that particle interaction would be dependent upon volume fraction.

I really appreciate the responses and help. Don't worry about insulting me if I come up with a cockamamie idea. I won't be insulted. I appreciate any help from anyone who volunteers their time to help out. I am new at CFD in general but I am learning quick and I will also help others if I can.
FrankS is offline   Reply With Quote

Old   November 8, 2013, 20:12
Default
  #10
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
In my first post I quoted and excerpt from the help which stated that I should model a dispersed solid as a continuous fluid with a dispersed liquid acting as a solid.

I just changed the option in CFD-Pre from "dispersed fluid" to "dispersed solid" and options for particle to particle friction and collisions became available. I a simple function for the effective viscosity of the particles based on volume fraction and i am running a simulation right now. I will adjust these new parameters to see if I can get the behavior I want. Thanks for all the help.

Frank
FrankS is offline   Reply With Quote

Old   November 9, 2013, 05:27
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Good to hear. And by the way - if the particles are the size of paper pulp then the forces acting are not Van Der Vaals forces. These act on the atomic scale and paper pulp is far too big for that. There will be some other force causing emulsion/flocculation/dispersion or whatever is happening. The chemistry of these sort of particles is highly complex and it is almost certainly a surface chemistry thing.
ghorrocks is offline   Reply With Quote

Old   November 12, 2013, 20:53
Default
  #12
New Member
 
Frank
Join Date: Oct 2013
Posts: 26
Rep Power: 5
FrankS is on a distinguished road
I realize that its not a Van Der Waals force but I was sort of using the idea of a Der Waals force to illustrate what I want to do.

I did some experiments today to try to figure out the exact volume fraction of the fibers in my suspension. I think I have a better idea what is happening but I still need to do some investigation. The fibers clump and are hydrophillic so while the actual volume fraction based of dry fibers is ~ 3%, the real volume fraction is actually very high, to the point where the suspension is almost like a granular flow.

There is an expert in my research group who is well known in the Pulp and Paper industry, Dr. Richard Kerkes. He has done lots of work on fiber swelling, clumping etc. I am going to go have a chat with him and look in to some of his research papers on these topics. Perhaps I can come up with a basic model that will fulfill my needs by determining a "real" volume fraction and clump-to-clump interaction. There is no point in doing a simulation if I have the physics wrong.

Thanks again for the help.

Last edited by FrankS; November 12, 2013 at 20:54. Reason: typo
FrankS is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
injection problem Mark New FLUENT 0 August 4, 2013 01:30
Check particle impaction with User Fortran Julian K. CFX 3 January 12, 2012 10:46
DPM UDF particle position using the macro P_POS(p)[i] dm2747 FLUENT 0 April 17, 2009 01:29
Adding Van der Waals force by coding UDF Long Sang FLUENT 1 June 23, 2008 07:44
interaction time between particle and eddies Steve FLUENT 0 April 10, 2001 18:17


All times are GMT -4. The time now is 00:50.