We used the software Gambit to mesh our geometry. This mesh is cartesian and quasi uniform: it is a little bit concentrated in the middle (factor 0.95) where the gradients are stronger.

The mesh has the following characteristics:

Type:
Rectangular channel

Length: 2 m

Height: 0.5 m

One velocity
inlet in the left side

One outflow outlet in the right side

Wall
on the upper side

Wall on the lower side

The following picture represents the mesh

The following parameters were taken in the Fluent 5 database.

We took the
following constants for the gravitation and surfacic tension: g =
9.81 m/s^{2} and s =
0.0735 N/m. As we did not find the value of s
for these two fluids, we decided to keep the standard value
given by Fluent (water/air).

__Upper fluid:__ designated by the indice 1, fuel oil liquid
(C_{19}H_{30}), density: 960 kg/m^{3},
cinematic viscosity: 5E-05
m^{-2}.s^{-1}.

__Lower fluid:__ designated by the indice 2, water liquid (H_{2}O),
density: 998.2 kg/m^{3}, cinematic viscosity: 1E-06
m^{-2}.s^{-1}.

All this parameters are constants for every simulations. The velocities of the two fluids depend on the studied case. The two fluids have close densities to avoid numerical problems in the calculations (divergence).

This section describes the numerical parameters used for the simulations.

We performed
unstationnary simulations with a constant timestep of 0.01s, for
each case. This timestep allows a good precision and a good
resolution for the different cases.

The convergence criteria were
set to 0.001 for the residuals, the X-velocity and the Y-velocity.

All the simulations were realized with the laminar model, to have the possibility to see the development of the instabilities.

The multiphase model used is the VOF (Volume Of Fluid) model with the following options:

Scheme:
geo-reconstruct,

Courant number: 0.25,

Surface tension 0.0735
N/m

We choosed to use the standard schemes proposed by Fluent5 for the discretization:

Pressure: standard

Momentum: first
order upwind

Pressure velocity coupling: simple

The first simulations realized showed that the instability was unable to appear in the normal conditions (with different velocities of the two fluids). In order to force the appearance of the Kelvin-Helmholtz instability, we placed a vertical oscillator in the inlet.

The aim of this oscillator is to simulate a vertical beater which makes the interface between the fuel oil liquid and the water oscillate, with a given frequency and a given amplitude. With this beater, we were able to make a frequential study of the Kelvin Helmholtz instability.

This oscillator was introduced in the calculation by means of an User Defined Function, written in the C++ language adapted to Fluent 5. The input parameters are defined as constants in the beginning of the program. The source of this UDF is given below.

#include
"udf.h" |

The result of this beater is the creation of an oscillation of the interface between the fluids, which is convected and deformed by the flow.