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

dynamic contact angle / contact line velocity

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 22, 2014, 09:33
Default dynamic contact angle / contact line velocity
  #1
New Member
 
Join Date: Oct 2013
Posts: 21
Rep Power: 3
ThomasN is on a distinguished road
Hello,

I know there are many discussions about this theme and it's problems but no approach about the contact line velocity.

The results of my two phase flow high dynamic simulation depend extremely on the value of the contact angle at the walls. So I want to use an approach for the dynamic contact angle. Everything works fine but I have to read the velocity of the moving contact line. (Currently I define a velocity u v w and the contact angle changes in response to the orientation of the contact line (normal of the free surface) and the velocity vector )

So there is the problem that a no slip boundary has no velocity. Therefore I want to use the velocity in a certain distance of the wall. Does anybody have an idea how to read the value of a variable with the coordinates x,y,z in CEL without defining a Monitor Point? Is there a way to implement something like that:

interface_vel=Oil.velocity (x, y, 0.001[m]) ?

Thanks!
ThomasN is offline   Reply With Quote

Old   September 22, 2014, 18:56
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You have found the well known issue that a contact line at a wall boundary should not move (because of the no slip condition), but it clearly does. This paradox is glossed over in just about all CFD codes and just ignored - I know CFX and Fluent have nothing to deal with this and I strongly suspect Comsol, StarCD and the others do not either.

The result of this is that simulated contact lines do not converge with grid refinement. The results they give are vaguely correct, but if you trying to be accurate it is impossible.

I cannot see how your suggestion will improve things either. Using a fudge to avoid a fundamental limitation in Navier Stokes multiphase simulation methodology sounds unlikely to be successful to me.

Can you describe what you are simulating? It is unusual to have simulations where contact angle is important but the length scale is larger than millimetres.

My recommendation would be to move to a simulation software which does not have fundamental limitation on moving contact lines. Unfortunately I cannot name one - but you might have some luck with a lattice Boltzmann solver (which does not use the Navier Stokes equations).
ghorrocks is offline   Reply With Quote

Old   September 23, 2014, 02:32
Default
  #3
New Member
 
Join Date: Oct 2013
Posts: 21
Rep Power: 3
ThomasN is on a distinguished road
Hello Glenn,

I'm not allowed to explain it in detail because it is not published for now. But I simulate a two phase flow between two rotating discs (rotating couette flow) where the gap between the discs is about 0,1mm and the rotating speed is 3000min^-1. The Domain size is 20mm. So the effects of the contact angle are significant.

I'm working on this problem with cfx for a long time and i have to solve it with this code (the results aren't that bad with a constant contact angle, I only want to improve them)
I know some approaches where they use the contact line velocity in a certain distance from the wall or the whole drop velocity.
Is it possible to use a velocity of a cell with specified coordinates for the calculation of another cell? So I could imagine that the cells at the wall use the velocity of the cells in a certain distance of the wall to determine the contact angle in response to the orientation of the contact line and the velocity vector.

Thomas
ThomasN is offline   Reply With Quote

Old   September 23, 2014, 03:27
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I cannot think of an easy way to implement the velocity condition you request. It will probably have to be done in fortran and it does not sound straight forward at all.

So my warning is simply that you if your results are close, you are going to have problems getting much better than that. For a simple example, do a simulation of flow in a capillary tube where the flow is pulled by a meniscus working its way along the capillary. This is a good example as it has an analytical solution. You will find that as you refine the mesh your results initially get more accurate, but then get worse and do not converge on the analytical solution.
ghorrocks is offline   Reply With Quote

Old   September 23, 2014, 03:46
Default
  #5
New Member
 
Join Date: Oct 2013
Posts: 21
Rep Power: 3
ThomasN is on a distinguished road
Ok thanks for the advices. I will try it. At the moment I experiment with a drop on a surface.
ThomasN is offline   Reply With Quote

Old   September 23, 2014, 06:00
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If the free surface interface does not move then the inconsistency does not occur. So if your drop is stationary it will run just fine. You need a moving interface for the problem to show up.
ghorrocks is offline   Reply With Quote

Old   September 23, 2014, 06:07
Default
  #7
New Member
 
Join Date: Oct 2013
Posts: 21
Rep Power: 3
ThomasN is on a distinguished road
The drop and the Interface are moving... the convergence is quite good.
ThomasN 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
Take derivative of mean velocity in paraFoam hiuluom OpenFOAM Paraview & paraFoam 12 February 4, 2014 06:46
Annoying issue of automatic "Rescale to Data Range " with paraFoam/paraview 3.12 keepfit OpenFOAM Paraview & paraFoam 60 September 18, 2013 03:23
How Can I calculate the Contact Line velocity in interface?? farhagim OpenFOAM 10 May 10, 2011 23:25
Problems of Duns Codes! Martin J Main CFD Forum 8 August 14, 2003 23:19
error while compiling the USER Sub routine CFD user CFX 3 November 25, 2002 16:16


All times are GMT -4. The time now is 05:28.