*3.3. Volume of Fluid*

The volume of fluid (VOF) multiphase model is a simple multiphase model. It is used to solve problems involving immiscible fluid mixtures, free surfaces, and phase contact. Figure 9 represents the elevation of the free surface in respect to the laboratory reference system, and shows how the VOF model is able to track difference phases and thus define the wave pattern behind the hull.

**Figure 9.** Wave pattern behind the hull for 3 m/s.

Due to its numerical efficiency, the model is suited for simulations of flows wherein each phase constitutes a large structure, with a relatively small total contact area between phases [31].

The spatial distribution of each phase at a given time is defined in terms of a variable that is called the volume fraction. A method of calculating such distributions is to solve a transport equation for the phase volume fraction. The method uses the STAR-CCM+ segregated flow model [32].

By default, the VOF free surface calculation is performed during the same time step as the other calculations. To ensure simulation stability, at free surface the value of CFL (Courant–Friedrichs–Lewy number) must be limited to 1, and better results with a sharp resolution of the two phases are obtained with a CFL around 0.5 [28,29]. However, such a limitation is overly restrictive, as other physics calculations with implicit solvers can run at a much larger CFL number. This reduces the computational efficiency of VOF free surface simulations.

The multi-stepping feature removes this limitation on the CFL number; this option applies temporal sub-cycling to the transport of volume fraction and can improve the resolution of the interface between two phases; however, multi-stepping cannot be used with second order time discretization in Star-CCM+.

To maintain the accuracy that only a second order time scheme can guarantee, the multi-stepping feature has been disabled; thus, the value of CFL at the interface between phases represents a real and strong limitation for the time step of the model.

#### *3.4. Dynamic Fluid Body Interaction (DFBI)-6DoF Solver*

The dynamic fluid body interaction (DFBI) module simulates the motion of a rigid body in response to forces exerted by the physic continuum.

The 6-DoF (degree of freedom) solver computes fluid forces, moments, and gravitational forces on a 6-DoF body; pressure and shear forces are integrated over the surfaces.

For time integration, the 6-DoF solver employs a trapezoidal scheme of second order accuracy. This is independent of the order of accuracy of the implicit unsteady solver for the momentum and continuity equations.

When working with body motion, it is convenient to provide a smoothing ramp, so that forces on the hull are released meekly and not impulsively.

If no ramp is set up, abrupt impulses generate both physical and numerical transients and oscillations that affect the kinematics of the floater, which damp out several seconds after the beginning of the simulation [30,31,33].

Therefore, although the additional ramp time must be added to the simulation, the computational time is shorter due to a faster and cleaner convergence.

We decided on a release time of one second and a ramp time of two seconds: The moving body remained fixed in all DoFs for the first second of the simulation, in order to allow the fluid field around the floater to assume more realistic values in respect to initialization with a constant speed all over the domain; then from seconds 1 to 3, all the forces were smoothly applied to the body until the full value was used when ramp time ended at 3 s. The simulation results converged 6 seconds after the end of the ramp time; thus, the total time simulated was 9 s, which was enough to fully develop the wave pattern behind the boat and to stabilize drag and trim reports to constant values.

#### *3.5. Turbulence and Law of the Wall*

The flux around the hull was fully turbulent since the Reynolds number was in the order of millions; thus, turbulence had to be modeled to accurately compute forces acting on the boat.

The K-epsilon model is recommended in VOF simulations as the computational cost is low and the accuracy in the discretization of the interface between the two phases is good enough [31,34].

In the present case, a realizable K-Epsilon model was used, which represented an upgrade of the standard model: A new transport equation was used for the turbulent dissipation rate; moreover, the turbulence viscosity was expressed as a function of mean flow and turbulence properties instead of being constant.

A two-layer wall treatment was used in combination with the realizable K-Epsilon model.

In this approach, the turbulence quantities were computed as a function of the wall distance in the near wall region, and evaluated solving the transport equation in the far field; values were smoothly blended between these two zones.

The two-layer approach allowed the use of different values for *Y*+ because it applied wall treatment when the mesh could not accurately solve the boundary layer, and solved without wall functions when the mesh was fine enough to discretize the sub-viscous layer near the wall.

The hull is designed with a hydrodynamic shape in order to disturb the flow around it as little as possible; thus, phenomena like vortex shedding and fluid vein detachment do not occur, at least not for the range of speeds tested. This made it possible to discretize the region near the hull with a coarse mesh. In fact, if the fluid remained attached to the wall, there was no need to finely mesh the sub-viscous layer; however, values of *Y*+ around 50 (first cell in the logarithm layer zone) or more could be used (Figure 10) [35].

**Figure 10.** Wall *Y*+ under the hull.

The discretization that guaranteed these *Y*+ values was the following: Thickness of the first cell for the 3 m/s simulation was 1 mm; 12 layers were used with a smooth growth factor of 1.2.

The thickness of the first cell near the wall changed for every simulation, in order to always aim for the same *Y*+ values when the speed changed.

#### *3.6. Time Discretization*

In Star-CCM+, the multiphase VOF solver requires an implicit time scheme and is not available when an explicit time scheme is used. Thus, a second order implicit time discretization was chosen because the first order was numerically diffusive, and the property of the waves was not transported correctly [32,33]. As a consequence, if a first order is used, waves behind the hull are significantly damped out a few meters behind the boat and the wave pattern results are much smaller than in real experience.

Time step for an implicit time scheme can be high because implicit is unconditionally stable; the CFL factor can be up to 10 and even more, while for an explicit approach, the CFL factor has to be below 1, otherwise the method becomes unstable. Nevertheless, when dealing with multiphase models and overset technology, two additional limitations must be satisfied:


The second condition is very important when simulating a hull in head sea and when deciding about the overset dimensions. The more severe limitation on the time step comes from the former, so the time step is a function of the speed of the test in order to aim for the same CFL at the sea

surface. The time step goes from 0.01 s for 1 m/s test, to 0.0033 s for the 3 m/s test, and it scales linearly with speed.
