**Meshing**

The first step of the numerical analysis is creating the mesh which will be our base to launch simulations. To do that, we used the software ICEM CFD, and we created a rectangular mesh representing the tank of water or retardant. The study is done in 2D.

Once the geometry created, we have to mesh it and to define the type of boundary conditions (only walls) before exporting it to FLUENT.

Initially, we worked with a rough mesh (5000 nodes) and then we refined it (up to 200 000 nodes), but the results were pretty much the same. So, to avoid longer calculation time, we opted for the rough mesh for all the simulations.

**Fluent - VOF Model**

The first step was to comprehend the diphasic mode on FLUENT, given the fact that we never used that mode before. There are different options in the diphasic model : Eulerian mode, mixture mode, and Volume Of Fluid mode. We chose to work with the VOF (Volume Of Fluid) option.

In the VOF model, the input are the following :

- number of phases
- volume fraction scheme (explicit or implicit)
- inclusion of the implicit body force formulation (optional)
- coupled level set with VOF (optional)
- inclusion of open channel flow
- inclusion of open channel wave boundary conditions
- inclusion of zonal discretization for applications such as diffused interface modeling in one zone and sharp interface modeling in another zone

Concerning our problem, we chose two phases, an explicit volume fraction scheme and the inclusion of the implicit body force formulation.

*The explicit scheme*

Explicit schemes can take on different forms :

used for hybrid meshes (containing twisted hexahedral cells)*time-dependent with the explicit interpolation scheme*:used if there is an interest in the time-accurate transient behavior of the VOF solution.*time-dependent with the geometric reconstruction interpolation scheme*:available only for quadrilateral and hexahedral meshes.*time-dependent with the donor-acceptor interpolation scheme*:gives interface sharpness of the same level as the geometric reconstruction scheme and is particularly suitable for flows with high viscosity ratio between the phase.*CICSAM scheme*:

In our case, we can use georeconstruct scheme or CICSAM scheme.

__Including body forces__

When large body forces (like gravity or surface tension forces) exist in multiphase flows, the body force and pressure gradient terms in the momentum equation are almoste in equilibrium, with the contributions of convective and viscous terms small in comparison. Segragated algorithms converge poorly unless partial equilibrium of pressure gradient and body forces is taken into account. That is why the optional "implicit body force" treatment has its interest in FLUENT. Indeed, this option account this effect and in this way make the solution more robust by achieving a realistic pressure field very early in the iterative process.

Then, after choosing the model and the options, we defined the phases : their material properties, interaction between them (here surface tension). In the VOF model, you can specify the primary and secondary phases as you prefer. In our case, we have air and water and it is preferable to specify the compressible ideal gas as the primary phase to improve solution stability. So the primary phase is air and the secondary is water.

If you have a difference between the densities of the two phases around 1000 or more of that, you have to choose, in the boundary conditions>operating conditions an operating density equel to 0 kg/m^{3}. This choice allow users to have a better convergence.

*Initialization*

- Initialize all the zone with a water volume fraction equal to 0
- Define a region of water (specifying the level of water) : >Adapt>Region and click on Mark
- Patch the water volume : Initialization>Patch. Choose, water volume function, value equals to 1, hewahedron-0. Click on Patch
- Check that the two phases are well defined : >Display>Contours>Phases>Water volum fraction (options : click on filled).