[rmousavibt]

Dear FLUENT users;

I want to write a UDF for taking the dynamic contact angle into account. As you know, a contact line is the intersection of a solid wall and the interface of two fluids. The contact line is the angle between the wall surface and the tangent to the fluids interface at a point on the contact line. So, because that you have infinite points on the contact line, the contact angle is a local variable. There are several corrolation relating contact angle and the contact line speed (the fluid velocity at contact line).
I can write a UDF using a Define_Profile function, but I do not know that if I speak about the cell_velocity in my UDF, does FLUENT adopt the velocity of the cell for which the value of contact line is being calculated?

Many thanks for your attention,
Roozbeh

[ayyoubmehdizadeh]

Hi Roozbeh.
I am working on VOF model for a while. This would be really nice while in Fluent typically we are setting the static contact angle.
I think that you are finding an element with in which volume fraction is about 50% on the wall (interface place) and then extracting the x-velocity of that cell as the velocity of the interface?
Am I correct?

[oil&water]

Hi
is there anyone around with a working UDF for setting the value of the contact angle (CA) on wall faces as a time dependent function ? or as a delta_CA increase with respect the CA value in the previous iteration
Thank you in advance

[ghorrocks]

Hi:

Ayyoub's point highlights the dilemma here - with a no slip boundary condition the velocity at the wall is zero. So how then does the free surface move along the surface? If you use the velocity of the first cell in the domain then the velocity will be dependent on mesh size and your simulation will not converge as you refine the mesh.

Simulating a moving contact line along a no slip wall with a specified contact angle is an area of active research and I have not yet seen a "universal" approach. What I do know is that if you refine the mesh of a simulation which uses this effect to drive the flow (eg a capilliary driven flow) it is impossible to achieve a mesh converged solution - in fact all my tests are diverging with mesh refinement.

This means, in short, that the implementation of wall contact angles in Fluent (and also most other CFD codes I should add) is not physical and is not accurate. A leading researcher in this field is Shikhmurzaev (http://web.mat.bham.ac.uk/Y.D.Shikhmurzaev/)

Has anyone else looked into this issue? Have you checked the mesh size independence of these flows?

Glenn

[marzbali]

Hello!

As Glenn pointed out there is a singularity at the contact region where 3 phases meet. Hence, most numerical models make assunptions to calculate the contact line velocity. Recently Sikalo has tackled this issue and proposed a novel method. His article is titled :"Dynamic contact angle of spreading droplets: Experiments and simulations" published in physics of fluids in 2005. You may find it interesting.
Having said that, the question is now if it is possible to implement his methodology in FLUENT?!

[oil&water]

by experience ...
if you like dyn. contact angle .... use immiscible lattice Boltzmann (ILB) approaches rather than traditional CFD ... ILB Methods are also 2 (o even more) order of magnitude faster than CFD on multiphase - multicomponent applications

[marzbali]

ILB is a very powerful method, the thing is that is not offered in FLUENT

[subha_meter]

It's possible to capture the velocity at the interface in VOF simulation (FLUENT) and velocities thus obtained can be used to calculate the dynamic contact angle through an UDF.

[cfd^2]

Dears,

I have a question on this issue. Isn't the static contact angle implemented in FLUENT suficient to simulating multiphase flow, since when one sets no slip BC at the wall the velocity is zero... I mean, if we take some empirical correlations to account for the dynamic advancing and receding contact angle we see that they depend upon the capillary number, which is a dimensionless group which takes the fluid velocity into account. So, if the velocity at the walls is zero, the capillary number also is zero and the dynamic advanced and receding contact angle is equal to the static advanced and receding contact angle. The matter now is that which we enter in FLUENT is, in fact, neither the advanced or receding contact angle, but the static contact angle. So, in my vision, which could be done to improve this implementation has to do with setting an advanced and a receding CA.

[ghorrocks]

I do not understand your question. But if the wall/interface point is not moving you do not have the singularity and there is no problem - so of course it should work fine. It is only when the contact point is moving that there is a problem.

[cfd^2]

In my case I have flow of the two phases and I have set no-slip BC at the wall and a static contact angle, since this is the only available option in fluent. Does anyone knows if the assumption of a static contact angle is feasible and which is the limit of validity of this assumption? If it is not valid, I think a dynamic contact angle should be implemented, considering a moving contact line. At this point we have the problem, right? The non-slip BC could not be used anymore...

[siramirsaman]

A rough implementation here:

https://github.com/siramirsaman/Flue...-Contact-Angle

[brucelqs]

Originally Posted by siramirsaman

A rough implementation here:

https://github.com/siramirsaman/Flue...-Contact-Angle

Hello, do you know how to parallelize this UDF code? I encountered a problem when parallelizing this code and tried many times without success. If you can provide some hints, information or documents, it will be very helpful! Thank you!