**5. Experimental Set Up**

The experimental results were obtained from [10]. Please refer to this paper for detailed discussion upon the experimental set up. This section will, however, briefly detail the experimental testing that was undertaken.

The experimental work used a simple prismatic hull form, featuring a constant deadrise. It was tested in the fully planing condition in calm water. The lines plan is presented by Figure 1.

**Figure 1.** Lines Plan of Model (Linear Dimensions in mm).

The experimental test matrix was defined to cover a broad a range of hull positions, allowing a robust validation case for the CFD set up across a number of conditions. A total of 175 runs were completed, taking measurements for 12 test cases featuring three trim (τ) conditions and four speeds. The hull parameters for each test case are detailed in Table 1, where the draft given is the immersion of the transom once the model has been positioned correctly. Due to the speed limitations of the carriage, a small-scale testing methodology was employed.


The wake profiles was measured using sonic probes mounted on a gantry behind the model, as detailed in Figure 2. Additionally, the forces and moments were measured to allow further validation of the CFD simulation.

**Figure 2.** Gantry Step Up for One Sonic Probe.

#### **6. Numerical Set Up**

This section outlines the approach followed when developing the numerical simulation, giving the specific details of the final set up that was deemed the most appropriate for modelling this problem. Information regarding alternate set ups and the effect of these upon the simulations results is presented in the results section. Detailed information upon the inner numerical workings of the CFD code will not be discussed as the commercial solver Star CCM+ was used, and such details are not relevant to the scope of the work. Detailed information outlining the inner workings of a CFD solver can be found in [18]. The numerical set up was in the same scale and conditions as reported in the experimental study, ensuring that both the Froude and Reynolds numbers in both were identical.

#### *6.1. Physics Modelling*

It is commonplace to use a two-equation turbulence model for numerical studies into ship hydrodynamics, with [16] stating that they have been proven to give accurate predictions. Whilst more advanced models are available it was found by the ITTC following the analysis of entries to the Gothenburg 2010 Workshop, that there was no visible improvements to the accuracy of a resistance simulation when these are used.

The most widely used two-equation turbulence models for engineering application are κ−ε and κ−ω. Both are used when studying ship hydrodynamics; however, variants of κ−ω are far more prevalent, accounting for 80% of the submissions for the Gothenburg 2010 Workshop. When comparing the models the ITTC concluded that turbulence model selection has little impact upon the accuracy when analysing resistance [11]. A review of studies investigating planing hull performance through CFD found that there was no clear indication that one was more favourable than the other with both being used in a number of papers:


The κ−ω *SST* model is known to be more computationally expensive, with simulations taking up to 25% longer to run [28]. Despite this downside, studies have shown it to be superior when predicting separating flows and wake patterns [11,16]. Additionally, it has been shown to be the most prevalent turbulence model for use with marine hydrodynamics over the past two decades [29].

An investigation into turbulence model selection revealed that for low *y*<sup>+</sup> planing hull simulations turbulence model choice resulted in a notable variation in the calculated forces and moments. It was also shown to have reliable impact upon the accuracy of the calculated wake program. In this investigation κ−ω *SST* proved to be the most accurate, so this model was selected despite the fact that it is more computationally expensive.

The Volume of Fluid (VOF) method was used to model and track the position of the free surface. It is known for its numerical efficiency and is a simple-multiphase model that is well suited to simulating flows of immiscible fluids. The model introduces a 'volume fraction' variable, which is used to define the spatial distribution of each phase. A cell with a volume fraction of 0.5 contains a 50:50 mixture of air and water, and is used by the VOF method to define the free surface.

A known and documented problem when modelling planing hulls using the VOF method is that it can lead to Numerical Ventilation (NV), or Steaking, which may be considered one of the main sources of error in these numerical simulations [21,26] NV occurs when the free surface is not captured adequately and results in air falsely being introduced into the boundary layer flow adjacent to the hull. When NV occurs, it has a negative impact on the calculation of forces as it alters the fluid properties. Gray-Stephens et al. investigated a number of strategies to minimise NV [30]. All strategies that were found to be effective were employed in the setup of this simulation to ensure that NV did not affect its accuracy. Additionally, over the course of the current work it was found that including a surface tension model equal to 0.072 N/m helped to reduce NV further when used in conjunction with established methods.

The surface tension coefficient expresses how easily two fluids can be mixed, with a higher surface tension represents a stronger resistance to mixture. The coefficient itself is defined as the amount of work necessary to create a unit area of free surface [31]. For the most part the effects of surface tension are negligible with The ITTC Specialist Committee on Computational Fluid Dynamics stating that they may usually be neglected for ship hydrodynamics problems [32]. As this work adopted a small-scale testing approach, the surface tension forces are larger relative to the hydrodynamic forces than for a more conventional model size. It was thus necessary to determine if neglecting these forces was valid, or if they must be included in the simulations.

Including the surface tension model had a significant effect upon the forces calculated. This was achieved through a reduction in the level of NV (Figure 3), which changed the fluid properties in the near wall cells. It has been concluded a number of times that it is not possible to eradicate NV, however it is possible to reduce it to a level that is acceptable for engineering purposes [31,33]. This study presents a new viable strategy to reduce the levels of numerical ventilation. This is supported by [34], who investigated free surface flows with air entrainment and concluded that failure to include the surface tension model resulted in an increased level of air entrainment.

**Figure 3.** Numerical Ventilation (Left: Surface Tension On) (Right: Surface Tension Off).

All previous studies investigated planing hull hydrodynamics that were found over the course of the literature review followed a high *y*<sup>+</sup> approach, using wall functions to model turbulence. A low *y*<sup>+</sup> approach is desirable if an accurate prediction of the boundary layer velocity is required, for instance in drag calculations, and if the cell count and simulation time is not considered a critical issue [35]. Adopting a low *y*<sup>+</sup> approach almost doubled the cell count and increased the computational time required for convergence by a factor of three, however lead to a significant improvement in the accuracy of both the wake profile and forces.

As the cell count and simulation time were not considered critical issues the low *y*<sup>+</sup> approach was selected, primarily due to the improved the accuracy in calculating the wake profiles, however also as it reduced the comparison error in resistance to a more acceptable level. The low *y*<sup>+</sup> approach resolves the viscous sublayer and, as such, the simulation should be more representative of the physical phenomena occurring.

#### *6.2. Timestep*

A timestep may be selected to ensure that it satisfies the flow features of interest or that it satisfies the Courant–Friedrichs–Lewy (CFL) condition. For standard pseudo-transient resistance simulations, a timestep that satisfies the flow features of interest is usually selected when an implicit solver is employed. When the V & V study (as presented in Section 7) was performed, a number of timesteps were tested. The timestep study revealed that as the timestep was reduced by a factor of two, the calculated forces featured Monotonic convergence upon a solution. The average timestep convergence ratio for all forces was 0.27, and was as low as 0.016 for resistance. The selection of timestep was made to balance the computational run time against the accuracy of the solution. It was shown that when the timestep was reduced further there was no significant improvement in the results. A timestep (Δ*t*) that satisfactorily resolves the flow features as a function of the vessels speed (U) and the wetted length (*LK*(*m*)) of the hull was selected, such that:

$$
\Delta t = 0.02 \frac{L\_{K(m)}}{\mathcal{U}} \tag{1}
$$

It was ensured that the selected timestep was within the range suggested by the ITTC for such simulations in all cases [36]. Satisfying the CFL condition for all cells resulted in an impractically small timestep that would result in an unjustifiable increase in computational time. It would also have a negligible impact upon the results over a timestep that was selected to ensure that the flow features of interest were satisfied through a timestep independence study. The verification study determined that a timestep defined by Equation (1) is capable of resolving the flow features of interest, suitably balancing accuracy against computational time.

#### *6.3. Computational Domain*

It is well documented that for a CFD simulation to be accurate the choice of domain size must be appropriate, such that the boundaries are placed sufficiently far away to ensure they have no effect upon the solution through interaction with the wake. The ITTC recommend that the inlet and exterior boundaries are located 1–2 Length between perpendiculars (*LPP*) from the hull, with the outlet being placed 3–5 *LPP* downstream [37]. It is also important to ensure that wake does not intersect with the side boundary as this can cause reflections that influence the solution. Due to the narrow wake associated with a planing hull this is of less concern than for a conventional displacement simulation. The sizing of the computational domain was chosen in accordance with ITTC recommendations and may be seen in Figure 4. To ensure the domain was robust and suitable for all possible trim conditions the overall length of the model was used rather length between perpendiculars, or wetted length.

**Figure 4.** Domain Sizes and Boundary Conditions (*L* = Overall Length).

In addition to selecting an appropriately sized domain, the VOF Wave Damping option was enabled on the side and outlet boundaries to ensure that wave reflections did not impact the solution. The VOF Wave Damping option introduces a vertical resistance to vertical motion, and suppresses waves, and prevent them reflecting back into the simulation. A damping zone of one length overall (*L*) was chosen.

#### *6.4. Boundary Conditions*

The selection of appropriate boundary conditions is essential to ensure that the solution remains accurate whilst at the same time managing the computational costs of the simulation. The Dirichlet boundary condition was applied, simulating free flow. A common practice to reduce the size of the domain for calm water resistance simulations is to implement a symmetry condition on the x-z plane at the centreline of the hull. The nature of the wake profile was shown to include symmetrical elements of flow that crossed the centreline and interact with one another. As such, prior to employing this strategy, tests were undertaken to determine if it influenced the calculated wake profiles. It was shown that there was negligible impact upon the results and, as such, the symmetry boundary condition was utilised, halving the computational demand.

If the simulation were to be an accurate representation of the physical tank, the walls of the domain would be modelled using no-slip walls, the top as an inlet, the front as an inlet, and the rear as a pressure outlet. The modelling of no-slip walls requires the inclusion of a prism layer mesh, and this in turn requires volume mesh refinements to ensure the interface between the volume mesh and the prism layer mesh is appropriate, maintaining an acceptable volume change between cells. Such a selection of boundary conditions is impractical due to the significant increase in cells. A simplification to avoid this is to model the sides and bottom of the domain as inlets. The inlet condition is reported to be the least computationally expensive, whilst the selection of any appropriate combination of boundary conditions has no significant affect upon the flow results, provided they are located suitably far from the vessels hull [28]. The physical tank walls were far enough from the hull as to have no influence upon it, while the depth was great enough to consider the scenario a deep-water problem. Similarly, the domain of the simulation is large enough that the boundaries are far enough away to have no impact upon the result.

Extra consideration was given to the deep-water assumption. Before employing this assumption for the CFD case, the following were checked for the experimental test regime:

