[sagnikmazumdar]

Hi, I am trying to model droplet deposition on a surface with a specific contact angle, just like:

http://aisberg.unibg.it/bitstream/10...2012_23-32.pdf

using OpenFOAM. I started with a simple 2D case, following the guidelines of the dambreak case setup and as suggested in the paper. I am specifying:

type constantAlphaContactAngle;
theta0 60;
limit gradient;


for the droplet deposition surface. I want the final steady state contact angle to be 60 (degrees) as done in the paper. But when I run the simulations with the given setup:

https://dl.dropboxusercontent.com/u/...oplet_case.zip


instead of depositing as a droplet, the liquid starts to flow as in the dambreak case. I wonder what is wrong with my setup.

Thanks a lot for all the help and guidance.

sincerely
Sagnik


PS: I have tried to contact the author of the paper but could not get in touch.

[michielm]

Hi Sagnik,
I have taken a look at your case and I have a couple of suggestions:

1) for the pressure on the boundary where you set constantAlphaContactAngle it is best to use

type fixedFluxPressure;
adjoint no;

2) In 2D cases that are surface tension dominated you will often have droplets running away due to spurious velocities. I cannot check this for your case because you didn't include any other directories than the 0 directory and your case is way too big to run quickly and the blockMeshDict you included is not the blockMeshDict for this case. Could you either (i) make a movie of the problem that you describe, (ii) provide the appropriate blockMeshDict so I can quickly remesh and rerun if necessary.

The last point is actually the main issue: I can't check everything because your blockMeshDict doesn't match the included mesh.

[sagnikmazumdar]

Hi Michiel:

Thanks a lot for your suggestion. Your pressure setting did the trick.

So that others can also benefit, I have simulated 2 cases with contact angles of 60 and 120 with 10000 cells only to show that it works. It can be downloaded from:

https://dl.dropboxusercontent.com/u/...coursemesh.zip

The folder contains the results at each 0.01s for 0.1s. The ppt in the folder shows the initial and final contours.

You could not see the correct blockmesh file as it was generated from a .msh fluent file using the 'fluentMeshToFoam' converter. The .msh file is in the contact angle 60 case folder.

I also wonder if we should use the same pressure BC for all the other walls in the domain as well !

Thanks for all the help.

Sagnik

[michielm]

Glad I could help!

Just a final suggestion. I'm not sure what your future plans with this type of simulation are, but if you are interested in the dynamics of droplet deposition than you should consider using a dynamic contact angle boundary condition. Also, if you are not going to do droplets falling from a height then you might want to cut a part of your mesh at the top, because you are simulating a lot of 'empty' space now.

[sagnikmazumdar]

Thanks Michiel. Yes, we do have plans to do extensive work on the topic. Do you have any suggestions for appropriate references on the topic especially related to OpenFOAM ! It would surely be of great help. I have looked a bit on the use of dynamic contact angle from:

http://www.cfd-online.com/Forums/ope...act-angle.html

Thanks again for all the help.

Sagnik

[elvis]

Hi,

I wonder why you do not consider the "Finite Area Method (FAM) which comes with OF 1.6-ext"
http://www.openfoamworkshop.org/2009...sak_slides.pdf
there is a "(not really) similar" method introduced with OF 2.0 http://www.openfoam.org/version2.0.0/surface-film.php but many say FAM has still an advantage

[akidess]

Elvis, the MMIT method is great, but does not include any contact angle implementation. Also if at any point topological changes are to be considered, things will get tough (but not impossible) with MMIT.

[kmou]

Hi Sagnik ,
would it be possible to get your test case as provided a few years ago? :-)
as I am trying to gather ideas on how to simulate a droplet splashing onto a wall with contact angle.
camille.bilger@free.fr