# contact angle behavior in micro & nano dimensions

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 29, 2011, 08:11 contact angle behavior in micro & nano dimensions #1 New Member   Paolo Join Date: Nov 2011 Posts: 7 Rep Power: 5 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

 December 2, 2011, 09:06 #2 Member   Duong A. Hoang Join Date: Apr 2009 Location: Delft, Netherlands Posts: 92 Rep Power: 8 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

December 2, 2011, 10:24
case description
#3
New Member

Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
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??
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
 micro.jpg (49.8 KB, 17 views) nano.jpg (20.5 KB, 13 views)

Last edited by Jimbomet; December 2, 2011 at 10:45.

 December 2, 2011, 11:27 #4 Member   Duong A. Hoang Join Date: Apr 2009 Location: Delft, Netherlands Posts: 92 Rep Power: 8 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

December 2, 2011, 11:53
#5
New Member

Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
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;
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
 nano_init.jpg (23.5 KB, 5 views) nano_end.jpg (20.5 KB, 5 views)

December 5, 2011, 10:16
#6
New Member

Paolo
Join Date: Nov 2011
Posts: 7
Rep Power: 5
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
 mm.jpg (54.0 KB, 8 views) um.jpg (49.8 KB, 6 views) 100nm.jpg (40.5 KB, 6 views) 10nm.jpg (40.3 KB, 7 views) nm.jpg (20.5 KB, 8 views)

 December 6, 2011, 11:06 #7 Member   Duong A. Hoang Join Date: Apr 2009 Location: Delft, Netherlands Posts: 92 Rep Power: 8 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post JoaoMiranda OpenFOAM Running, Solving & CFD 3 August 26, 2014 11:29 rmousavibt Fluent UDF and Scheme Programming 10 March 7, 2014 08:00 gandesk Fluent UDF and Scheme Programming 14 October 29, 2012 14:58 hsieh Open Source Meshers: Gmsh, Netgen, CGNS, ... 32 September 13, 2011 05:50 sebastian_vogl OpenFOAM Running, Solving & CFD 3 June 22, 2009 12:25

All times are GMT -4. The time now is 00:11.

 Contact Us - CFD Online - Top