# Fluent Simulations

Simulation parameters

The VOF model proposed by Fluent can model two or more immiscible fluids by solving a single set of momentum equations and tracking the volume fraction of each of the fluids throughout the domain. The VOF formulation relies on the fact that two or more fluids (or phases) are not interpenetrating.

To reconstruct the interface, Fluent offers different schemes. In the geometric reconstruction and donor-acceptor schemes, FLUENT applies a special interpolation treatment to the cells that lie near the interface between two phases.

As small velocities inlet are used in order to avoid turbulence, a laminar model is selected.

Concerning the boundary conditions:

• The outlet boundary condition is a pressure outlet initialized at 0 Pa.
• The gas injection is represented by a velocity inlet boundary condition.

The initialization of the domain is an important step in the preparetion of the simulation. The domain is first initialized with water evrywhere. Then, a region is created and which represents the initial position of the oil (Adapt/ Region... Mark). Then, the region is associated to the oil (Solve/ Initialized/ Patch... Oil Volume Fraction=1).

The convergence criterions are fixed at $1\times 10^{-6}$ and the maximimum number of iteration per timestep is 30.

Only the pressure-based solver can be used.The VOF model proposed by Fluent is not available with either of   the density-based solvers. Therefore, a pressure-based solver is used.

Nota Bene:

The VOF model does not allow void regions where no fluid of any type is present. However, this restriction is not an issue in the case as the cave is initially filled up with oil and water.

Moreover, only one of the phases can be defined as a compressible ideal gas. There is no limitation on using compressible liquids using user-defined functions.

First order versus second order

With Fluent, the second-order time-stepping formulation can only be used with the VOF implicit scheme. As Jadim is only available for a second-order formulation, the second-order implicit formulation is used for the comparison between Fluent and Jadim.

However, as explicit schemes are easier to program, with only simple calculations performed at each timestep, they required smaller timestep, and thus reduce the computational time of a simualtion.

A simulation is carried out with first a second order implicit scheme and then a first order explicit scheme and the results appeared to be similar. Thus, for the parametric study which require many heavy simulations, the choice has been made to use a first-order explicit formulation to reduce the computational time.

The implicit scheme is used for time discretization, Fluent's standard finite-difference interpolation schemes, QUICK, Second Order Upwind and First Order Upwind, and the Modified HRIC schemes, are used to obtain the face fluxes for all cells, including those near the interface.

In the explicit approach, Fluent's standard finite-difference interpolation schemes are applied to the volume fraction values that were computed at the previous time step.

Mesh impact study

Geometries and meshes are realized with IcemCFD .

As shown previously on a Jadim simulation, the influence of the mesh on the results can be important. Therefore, a mesh study is carried out in order to investigate the impact of the mesh in the three-phase flow case. Two simulations are compared, one using a coarse mesh and one using a refined mesh. The main parameters of the simulations are recap in the table below:

 Type of mesh Number of cells velocity Inlet Gas Reynold time step max Physical Time Coarse Mesh 70x88 0.1 m/s 260 $10^{-4}$ 2.41 Refined Mesh 140x176 0.1 m/s 260 $10^{-5}$ 2.43

In the two pictures below, the oil, gas and water contour are plotted at the same time. As observed for the Jadim simulations, a refined mesh reduces the phenomenon of numerical diffusion. Indeed, the interface between oil and the other phases obtained with a refined mesh is clearer and more accurate than the one obtained with a coarse mesh.

Refined mesh                                                                         Coarse mesh

The graph below shows that the oil and water volume fraction at the outlet are not the same for a coarse and a refined mesh. The coarse mesh  leads to an error of 7% on the results.

In conclusion, both local flow features and macroscopic data are affected by the mesh quality.  A refined mesh is necessary in order to have accurate results and to limit the numerical diffusion phenomenon.

Level Set method versus VOF method

Two simulations are carried out, one with the Level Set method and one with the VOF method. The graph below shows the outlet oil flow rate and oil and water remaining in the domain found. We can see that the results obtained are accurate and similar for the two methods: a maximum oil flow rate ratio of 11 is reach, which shows a good flow rate conservation and evolution of the oil and water volume fraction is relevant.

Therefore, the two methods can be used to simulate the problem. However, as the Level set method for a three-phase flow is not available on Jadim, all the Fluent simulations will be carried out with the VOF method.