*3.1. Numerical Aspects*

The solver, Star-CCM+ version 13.06, employs the finite volume method to model the flow, which uses the integral form of the incompressible RANS equations and divides the computational domain into a finite number of adjoining cells. Continuity and momentum are linked via a predictor–corrector approach. Further details pertaining to the implementation and algorithms used can be accessed in Siemens [28] and Ferziger and Peric [29].

To account for turbulence within the fluid, the *k*–ω model of Wilcox [30] is used. This choice is made following previous work, which showed the particular model to be stable and provide the fastest solution time of all two-equation variants [31]. Benefits of using the *k–*ω model include its seamless application to low *y*<sup>+</sup> type meshes (*y*<sup>+</sup> < 1). This is a desirable feature, because it avoids the use of wall functions, or any other bifurcations of the solution, as is the case with the *k*–ε model [28]. Although wall functions can predict the forces acting on a body with good accuracy, they may introduce errors in the modelling of hydrodynamic properties in the wake of a ship. For instance, they are unable to account for flow separation [32]. To facilitate a good representation of turbulent properties, a second-order convection scheme is applied throughout all simulations.

To characterise the fluid interphase, the volume of fluid (VoF) method is used [33]. Moreover, Star-CCM+ offers a high-resolution interphase-capturing (HRIC) scheme to enhance the definition of the free surface, which is employed in this study [34]. Vertical ship movements, i.e., sinkage and trim, are not accounted for to reduce the complexity of the simulations. Instead, the ship's position in the x–z plane is adjusted prior to initiating the simulation according to the published results of Elsherbiny et al. [23,35]. This is done in an attempt to reduce the discrepancy between the experimental results and those derived herein. However, some difference is expected to persist since the experimental data, reported by Elsherbiny et al. [23], were determined for a free to sink and trim KCS model.

#### 3.1.1. Computational Domain

As stated previously, frame invariance is not used in this work. Instead, the ship is given the corresponding velocity, which can be consulted in Table 2 for each canal. To model the motion of the ship along the canal, the overset domain approach is used. Thus, the ship is towed in the virtual environment over a static fluid. This has two main consequences. Firstly, the computational domain can no longer conform to the recommendations of the ITTC [36] relating to the positioning and dimensions of the computational boundaries. Instead, an attempt is made to replicate the towing tank used for the experimental work, which is used as a benchmark. Specifically, the towing tank at the Kelvin Hydrodynamics Laboratory at the University of Strathclyde. Naturally, the width and depth of the computational domain must satisfy the test cases (given in Table 2). On the other hand, the length of the computational domain is set as 60 m long. The dimensions are kept the same across case studies (pertaining to the overset domain and the length of the tank). These are shown in Figure 3. The height of the static domain is set as 1.23 ship lengths from the undisturbed water surface in all cases to eliminate any possible effects stemming from the height of the domain.

**Figure 3.** Length of the computational domain and dimensions of the overset domain.

The dimensions of the overset domain, which are maintained identical across case studies, are also shown in Figure 3. It should be noted that for visualisation purposes the figures have been mirrored about the central plane. Other than the boundary, coincidental with the canal and ship centrelines where a symmetry condition is imposed, all other boundaries within the background domain are no-slip walls. This is in line with our goal of designing a more realistic representation of a towing tank. Specifically, so-called 'open boundaries' do not exist in reality [37]. Examples of such boundaries include velocity inlets and pressure outlets. Although it is easier to define the conditions at such boundaries mathematically, they are a definite source of modelling error as discussed earlier.

The manner in which the computational domain is constructed allows the removal of wave damping. Moreover, the definition of turbulent properties on boundaries (such as levels of inlet turbulence) of the fluid is not necessary since there are no inlets nor outlets present. However, it should be noted that the initial conditions in terms of turbulence in the fluid must be specified. In this study, a turbulent viscosity ratio of 0.1% is used, which decays rapidly and is effectively zero in the nondisturbed region of the domain at the end of the acceleration phase, limiting its influence to the early stages of the simulation.
