CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

contact angle behavior in micro & nano dimensions

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

Like Tree1Likes
  • 1 Post By duongquaphim

Reply
 
LinkBack Thread Tools Display Modes
Old   November 29, 2011, 08:11
Default contact angle behavior in micro & nano dimensions
  #1
New Member
 
Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
Jimbomet is on a distinguished road
Hi all foamers,
I am a new entry in the world of OF and I'm trying to simulate the formation of a liquid meniscus between two flat surfaces (2D) as a process of merging of two drops.
I'm using InterFoam and I initialize two liquid half drops that intersect themselves, with their base on the two surfaces.

My domain dimension is very small (order of nanometers), and, working with these dimensions I encountered a strange behavior in the contact angle, in the sense it not respects my BC at the wall.
Dealing with micro dimensions I obtain a meniscus (but without the correct angle, that I imposed null), but when I try with nano dimensions the meniscus becomes a "cylinder" with infinite curvature (as if I Imposed alpha1=90)
Could someone help me?Any suggestion to solve this behaviour?... I can't understand what could be wrong in my case..?
Thanks in advance

Paolo
Jimbomet is offline   Reply With Quote

Old   December 2, 2011, 09:06
Default
  #2
Member
 
Duong A. Hoang
Join Date: Apr 2009
Location: Delft, Netherlands
Posts: 92
Rep Power: 8
duongquaphim is on a distinguished road
Send a message via Yahoo to duongquaphim
Hi,

I won't expect any difference between these two scales in the simulation if your mesh is fine enough. If possible, please post some figures and your case then we can talk more on that.

Cheers,

Duong
duongquaphim is offline   Reply With Quote

Old   December 2, 2011, 10:24
Default case description
  #3
New Member
 
Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
Jimbomet is on a distinguished road
Thanks for your reply Duong,
I have not solved my problem yet, I tried with a 3D simulation without changes in my behaviour...
My case consists in two flat plate at certain distance, and I want to simulate the formation of a liquid meniscus between them... : I initialise (with funckySetFields) a certain part of the domain with liquid phase (in particular two semi-sphere that intersect themselves, attached to the two surfaces), and I evaluate the equilibrium solution for each distance...my aim is to calculate the variation of pressure between wall with distance (but this is an other topic...).
My liquid is ethanol and the other phase is air. I'm using InterFoam solver. There are naturally no gravity forces in my problem.
I imposed a null contact angle at the walls and buoyant pressure.
In the 2D case I found the difference shown in the attached figures, when dealing with micro and nano scale

I thinks that behaviour is due to the very high drop of pressure at the interface of the two fluids at the interface (at nanoscale more than microscale), and perhaps the interface-compression can't correctly manage it, but I am not an expert at all... What could I do to solve that behavior, or it is the correct one and there is nothing to solve??
Thanks in advance
Paolo

I forgot to give the dimension of the domain: respectively 3nm and 7.5nm for the two sides of the rectangular domain, and the same measures but in micron for the "bigger" case
Attached Images
File Type: jpg micro.jpg (49.8 KB, 17 views)
File Type: jpg nano.jpg (20.5 KB, 13 views)

Last edited by Jimbomet; December 2, 2011 at 10:45.
Jimbomet is offline   Reply With Quote

Old   December 2, 2011, 11:27
Default
  #4
Member
 
Duong A. Hoang
Join Date: Apr 2009
Location: Delft, Netherlands
Posts: 92
Rep Power: 8
duongquaphim is on a distinguished road
Send a message via Yahoo to duongquaphim
Hi Paolo,

As I understood, in nano case, you initialized two semi-sphere and after getting to steady state, the interface become flat. It is a little bit strange. Are you using constantAlphaContactAngle or dynamicsAlphaContactAngle bc?

Also a good check might be a couple of simulations with different width from micro to nano scale (let's say 10micro, 1micro, 100nano and 10nano) to see when you observe this behavior.

regards,

Duong
duongquaphim is offline   Reply With Quote

Old   December 2, 2011, 11:53
Default
  #5
New Member
 
Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
Jimbomet is on a distinguished road
I know it is a bit strange. I attach the first time step and the last one for the nano problem.
I use constant contact angle. my condition is:

boundaryField
{
leftWall
{
type constantAlphaContactAngle;
gradient uniform 0;
limit none;
theta0 0;
value uniform 0;
}

Moreover, it is normal that when I initialise with funckySetFields only one of my wall have a
value nonuniform List<scalar>
...



I don't know where I'm wrong because performing a simulation in a bigger scale (say mm) it seems to change with respect to micro one (the contact angle seems to become smaller, more similar to null angle ).

Thanks for your suggestion, I'm going to try with dimensions between the two scales (I have only to find the correct time scales for each case...10^-9 for the nano-dimensions).
Thank you again, and good weekend
Attached Images
File Type: jpg nano_init.jpg (23.5 KB, 5 views)
File Type: jpg nano_end.jpg (20.5 KB, 5 views)
Jimbomet is offline   Reply With Quote

Old   December 5, 2011, 10:16
Default
  #6
New Member
 
Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
Jimbomet is on a distinguished road
Hi,
I've tried, as you suggested me, to run some simulation at different scale between nano and micro dimensions. I attach what I found in the range from mm to nm.
In the dimension of mm the BC contact angle seems to be respected while at smaller scales it seems not.
I tried to lower the viscosity in one case (100nm) case without apparent improvements for the moment...
Any suggestion?

Thanks
Paolo
Attached Images
File Type: jpg mm.jpg (54.0 KB, 8 views)
File Type: jpg um.jpg (49.8 KB, 6 views)
File Type: jpg 100nm.jpg (40.5 KB, 6 views)
File Type: jpg 10nm.jpg (40.3 KB, 7 views)
File Type: jpg nm.jpg (20.5 KB, 8 views)
Jimbomet is offline   Reply With Quote

Old   December 6, 2011, 11:06
Default
  #7
Member
 
Duong A. Hoang
Join Date: Apr 2009
Location: Delft, Netherlands
Posts: 92
Rep Power: 8
duongquaphim is on a distinguished road
Send a message via Yahoo to duongquaphim
Hi Paolo,

From your simulations, contact angle boundary condition worked pretty well in the scale of mm and micrometer but not in the scale of nanometer. And it is understandable since VOF is built on continuum mechanic. If you go to nano-scale, Knudsen number go to 1 and then molecular force becomes important. In that situation, you might want to use MD simulation rather than this VOF which is a continuum-based method.

I think that is the explanation for the outcome of your simulation. And I think I was wrong previously when saying that "I won't expect any difference between these two scales".

Cheers,

Duong
styleworker likes this.
duongquaphim 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
InterFoam contact angle JoaoMiranda OpenFOAM Running, Solving & CFD 3 August 26, 2014 11:29
Dynamic contact angle rmousavibt Fluent UDF and Scheme Programming 10 March 7, 2014 08:00
help with UDF for contact angle based on contact line velocity gandesk Fluent UDF and Scheme Programming 14 October 29, 2012 14:58
Import netgen mesh to OpenFOAM hsieh Open Source Meshers: Gmsh, Netgen, CGNS, ... 32 September 13, 2011 05:50
Theoretical background of formula for dynamic contact angle in interfoam sebastian_vogl OpenFOAM Running, Solving & CFD 3 June 22, 2009 12:25


All times are GMT -4. The time now is 12:10.