[qorka]

I simulate a water drop falling on the solid surface, but when the drop is near the bottom, it changes its form (see attachment)
I use surface tension and static contact angle = 90°

I use VOF explicite model with implicite body force
I tested this case with different solution methodes:
1)PISO-Green Gausse Node Based - Body Force W. - Second O. Momentum - Geo Reconstract
2)PISO-Green Gausse Node Based - Body Force W. - Second O. Momentum - Compressive
And also with PRESTO! pressure scheme

but the results are equal

Please, help me

[Tigrgrou]

Could you try a contact angle of 0 to see the effect on the result?

[qorka]

I set angle = 0
but the result is same

[Tigrgrou]

Do you have the same result if you switch the wall adhesion formulation and/or a finer mesh near the wall?

Sent from my ALE-L21 using CFD Online Forum mobile app

[qorka]

I turned it off
The results are better, but i think it is still wrong

The mesh is fine
0.05 mm
that means 40 elements in diameter of drop

[flotus1]

I simulate a water drop falling on the solid surface, but when the drop is near the bottom, it changes its form (see attachment)

Is this a problem? Are you sure that the deformation you see can not be a physical effect? What exactly did you expect and why?

The mesh is fine

No offense, but I heard that phrase a lot. And usually when it is stated like that the assumption is wrong. Your mesh might be fine enough to resolve the droplet itself, but it might be too coarse to resolve the scales of the impact.

[Tigrgrou]

If the mesh cannot b e refi.end because of calculaation time, eulerian wall film can be coupled with vof.

I agreed with flotus1. The mesh refinement should br tested.

Sent from my ALE-L21 using CFD Online Forum mobile app

[qorka]

Originally Posted by flotus1

Is this a problem? Are you sure that the deformation you see can not be a physical effect? What exactly did you expect and why?

Which the physical effect? Can you this explain from the physical point of view?

I think that circle must not be deformed before contact with the wall
it was falling 95% of the path with perfect shape, and near the wall it decided to change the shape?
I don't think so

[flotus1]

Is your droplet falling in a vacuum? Concerning the cell size: only one way to find out.

[qorka]

The mesh was refined by 66%
0.05 mm ->0.03 mm

Problem is the same (see att.)

i think that my mistake may be in setting of parametres or so on, because it changes shape always in the last row of cells

what can i change ??

[flotus1]

This does not convince me that the mesh you are using is fine enough to have no qualitative effect on the solution. For example I would argue that the distance between the two contact points is ~12 cells in both simulations.
If you can not afford a proper global mesh refinement study, it is sufficient to refine the mesh locally in the contact region.

Concerning the physical validity of the phenomenon you observe: you still did not answer the question if your droplet is falling in a vacuum. If there is a fluid surrounding the droplet, a similar deformation can actually occur under certain circumstances.
See for example http://pubs.rsc.org/en/content/artic.../SM/C4SM02474E and the references.
Looking at the pressure and velocty contours outside the droplet might shed some light on this issue.

[qorka]

Velocity in this paper is greater then 10 m/s
I have vel. less then 1 m/s

I tested mesh 0.01 mm, that means 200 elements in diameter of drop

And as i have already said, the problem is not in mesh, because the changes appear ONLY IN LAST ROW OF CELLS
in every case, that's why problem in case options, such schemes, URF and so on

can anybody help me with advice ?

[Tigrgrou]

Do you run the simulation in 2D?
I tried in 3D and I do not observe the behavior you mentioned.

[qorka]

Originally Posted by Tigrgrou

Do you run the simulation in 2D?
I tried in 3D and I do not observe the behavior you mentioned.

I tested only 2D

Sent from my Lenovo K50-t5 using CFD Online Forum mobile app

[Tigrgrou]

it could be the problem, specially if you use planar 2D solver

[qorka]

Originally Posted by Tigrgrou

it could be the problem, specially if you use planar 2D solver

And i can`t resolve it?

Sent from my Lenovo K50-t5 using CFD Online Forum mobile app

[Tigrgrou]

if you expect a solution that has physical meaning, your simulation has to be more representative of your real problem.
If it a spherical bubble, you can try the 2D axisymetry solver or 3D solver.

[qorka]

Originally Posted by Tigrgrou

Do you run the simulation in 2D?
I tried in 3D and I do not observe the behavior you mentioned.

i have built the same case but in 3D, but if i set in CFD post 3 contours and see XZ and YZ planes, i see the same effect

[qorka]

up this topic

[qorka]

update:

after discussion with ANSYS support it is clear a limitation of VOF method. they recommend to use Euler models and change BC for water phase to slip.