Towards a full-scale CFD guideline for simulating a ship advancing in open water

ABSTRACT Computational Fluid Dynamics (CFD) simulations of a ship’s operations are generally conducted at model scale, but the reduced scale changes the fluid behaviour around the ship. Whilst ideally ship simulations should be run directly at full scale, a guide has not been published to advise on the suitable setups that can provide accurate results while minimizing the computational cost. To address this, the present work explores an optimal approach for full-scale ship simulations. Extensive sensitivity studies were conducted on relevant computational setups to investigate their influences on the prediction of ship resistance, ship-generated waves as well as the boundary-layer flow of the hull. A set of CFD setups for full-scale ship simulations in open water was recommended. It was demonstrated that the ideal Y+ and Courant numbers in full scale are evidently different from those given in current model-scale CFD guidelines, indicating the necessity to establish full-scale CFD guidelines separately.


Introduction
Computational Fluid Dynamics (CFD) has developed into one of the essential tools for ship design, with its well-proven capabilities of predicting ship performance, including resistance, motions, manoeuvres and localized loads (el Moctar et al. 2012;Mucha 2017;Gatin et al. 2018;Huang et al. 2020). Yet most of the existing CFD work for ships is not performed at the real ship scale, as simulations are normally built at model scale to enable validation against experimental tests.
The downscaling brings about physical discrepancies though. Taking ship resistance in calm water as an example, in model experimental tests the scaling is based on a consistent Froude number (Fr), which scales the pressure component correctly but imposes errors within the friction component due to a changed Reynolds number (Re). This is because it is impossible to ensure that both Fr and Re are equal between the two scales. The mismatch in the frictional component is generally corrected using a standard extrapolation procedure of the International Towing Tank Conference (ITTC) (2008). Nevertheless, the extrapolation procedure is empirically based, thus it could provide inaccurate resistance predictions (Niklas and Pruszko 2019). Moreover, the changed Re number leads to unrealistic boundary layer and flow behaviours, which cannot be remedied by extrapolation.
By running CFD simulations directly in full scale, the scaling issues can be avoided, meaning that the fluid behaviours are replicated at the correct scale and empirically-based extrapolation procedures are not required. Detailed discussion on the scale effect between model and real ships has been documented by Terziev et al. (2022), showing the inherent errors in model-scale prediction and extrapolation is an outstanding problem for various ship design purposes. It causes incorrect reproduction of geometrical features, false prediction of flow properties such as turbulence/ wave characteristics, as well as a result of disparities in force ratios acting on the model and full-scale structures (Terziev et al. 2019). Based on a thorough review, Terziev et al. (2022) demonstrated that the application of full-scale CFD should be increasingly used to overcome the scale issue for ships and its development has become a primary interest of the shipping industry (Peric 2019).
However, ship simulations in full scale are still under exploration, since the best practice for fullscale simulations differs considerably from that for model scale, which means existing guidelines for ship simulations in model scale cannot be directly used, e.g. (ITTC 2014a). This is because a full-scale computational domain will be many times larger than a model-scale domain to fit the ship, but the fluids (water and air) are the same in both scales. This means that, whilst the domain size for full scale can be in the order of kilometres, the size of computational cells around the hull still needs to be millimetres to properly model the near-hull flow details. Consequently, the cell size around the hull needs to gradually increase towards the whole domain and sophisticated local mesh refinements are crucial, so a new meshing approach for full-scale ship simulations is required to solve the transition of cell size. This will cause other optimal setups to be different from those in model scale, such as the modelling of wall boundary layer (Peric 2019). In addition, the size of timestep will need to adapt to the full-scale meshing approach.
To provide an initial assessment on the best practice of full-scale ship simulations, Lloyd's Register (LR) (2016) organised the first-ever CFD workshop on a full-scale cargo ship, which provided a set of sea trial data as a benchmark for participants' blind simulation tests. Twenty-two sets of CFD results were received before the workshop, with various computational setups applied. The results showed generally good abilities of CFD on predicting full-scale ship performance, including resistance, power, propeller torque and vessel-generated waves. Nevertheless, the computational setups from the participants were based upon diverse strategies, and the resistance predictions differed by up to 16% from each other. Based upon analysing the inputs and outputs from the participants, the workshop concluded that further investigations are required to absorb the quintessence from each of the participants and make a set of ideal setups to be recommended for future users.
Full-scale CFD has been successfully applied to various ship hydrodynamic simulations. Niklas and Pruszko (2019) compared the resistance of a large carrier ship from full-scale CFD prediction, model test extrapolation and sea trial data. In their results, the full-scale CFD provided accurate predictions against the sea trial data for the complete examined range, while the extrapolated results from model-scale experiments were found to have large deviations in certain conditions. Haase et al. (2016Haase et al. ( , 2017) developed a full-scale CFD approach for the resistance prediction of largescale catamarans, and then performed a comparison between full-scale CFD prediction, model test extrapolation and sea trial data. Their results showed full-scale CFD prediction generally presented much smaller deviations against the sea trial data, compared with model test extrapolation. The above outcomes suggest that full-scale CFD simulations for deriving resistance equations may be a rational alternative method to model test extrapolation. Pena et al. (2020aPena et al. ( , 2020b presented detailed analyses of the flow field around an advancing cargo ship using full-scale CFD. Their results demonstrated the value of full-scale CFD for comprehensive ship design purposes, such as cavitation circumvention, flow control and hydroacoustic optimization. These analyses are not possible via model-scale CFD or experiments, since they require the flow to be kept at the correct scale. Huang et al. (2021b) simulated the slamming effect on a lifeboat by reproducing the surrounding flow at the correct scale, with computational results agreeing well with full-scale measurements. Based on sea trial data, Jasak et al. (2019) validated the performance of full-scale CFD in predicting the propeller performance of a cargo ship. They presented sophisticated local mesh refinements in their CFD model and compared it with several other mesh sets that caused inaccurate results. The work of Jasak et al. (2019) indicates an appropriate mesh setup is a key to achieving accurate full-scale CFD prediction for ships. The above types of full-scale simulation are important for structural design and hydrovibration investigations (McVicar et al. 2018;Smith and Ventikos 2022;Huang and Li 2022). Moreover, Tezdogan et al. (2015Tezdogan et al. ( , 2016, Nisham et al. (2021) and Terziev et al. (2021) applied full-scale CFD to analyse the behaviour of a ship in head-seas and restricted waters, which demonstrates such environmental conditions may contain significant fluid-ship interactions that need to be assessed in the real scale. Other examples of full-scale CFD for ship hydrodynamic simulations can be found as (Bhushan et al. 2009;Min and Kang 2010;Ponkratov and Zegos 2015;Liefvendahl and Fureby 2017;Bakica et al. 2020;Cheng et al. 2020) Despite that the aforementioned examples have shown full-scale CFD can provide significant insights for ships, the existing literature has all focussed on applications rather than CFD itself. A guideline for full-scale ship CFD is still lacking, without which, relevant simulations could be conducted with setups that are unassured or even inappropriate, especially considering the scarcity of full-scale measurements for validation. In this context, the present work aims to provide an exploration for any future full-scale CFD guideline for ships. The innovation of this paper is studying full-scale ship CFD itself by systematically performing simulations with varying setups to investigate the difference and derive an ideal configuration, which has not been included in any previous work.
The work is organised as follows: first, a full-scale computational model for a cargo ship advancing in calm water was established and validated against the LR sea trials data (2016). Then, relevant computational setups (e.g. mesh density, mesh transition ratio, mesh local refinements approach, timestep size, and the orders of discretisation) were systematically varied to investigate their influences on the ship performance prediction, focussing on the prediction of ship resistance, ship-generated waves and hull boundary layer. As a result, an accurate and cost-effective approach for simulating the case was derived, which was condensed into a set of recommendations for other CFD users.

Method
This section first introduces sea trials of a cargo ship that provide full-scale measurement data to be used as a benchmark for this study. Then a CFD model is built to simulate the sea trials, and the computational results are compared with the measurements to confirm the accuracy. Subsequently, a systematic research plan is proposed to investigate the sensitivities of essential CFD setups.

Benchmark ship and sea trials
A typical general cargo ship, Regal (Figure 1), was adopted as the ship object of this study. Sea trials of Regal were conducted in 2016 in the calm-water open ocean condition, during which ship power, torques and speed were recorded at three different shaft speeds (Lloyds Register 2016). The measurement uncertainties were reported to be minimal as the onsite sea condition was very calm. The main parameters of Regal and the sea trial conditions are given in Tables 1 and 2. Before the sea trials, the vessel was dry-docked, the hull was cleaned, and the propeller surface was polished. In this clean condition, the hull, rudder, and propeller were scanned with 3D lasers to obtain accurate geometric representations. The scanned geometries were imported into the CFD model presented in the following section.

Computational modelling
To reproduce the sea trials, an open ocean computational domain was built based on the STAR-CCM + software. Compared with model-scale CFD approaches, the full-scale simulation does not use different governing equations or boundary conditions, while the domain size is determined based on the real ship dimensions, as shown in Figure 2. The computational domain is three-dimensional, defined by the earth-fixed Cartesian coordinate system O-xyz. The (x, y) plane is parallel to the horizon, and the z-axis is positive upwards. The domain size is sufficiently large to avoid the ship-generated waves being reflected from the boundaries. The lower part of the domain is filled with seawater and the remainder is filled with air. The Regal hull is fixed at the free surface according to the design draught whilst its trim and squat are allowed through enabling the Dynamic Fluid Body Interaction (DFBI) module. The hull surface is modelled as a no-slip wall (velocity equals zero). The water was initialized as flowing with a constant velocity (U water ) against the bow of the hull, and a constant velocity condition was applied to the inlet boundary to maintain a stable water flow entering the domain. Thus, a relative velocity exists between the ship and water, where U water indicates the advancing speed of the ship in calm water (U water = U ship ). The top, boundary and side boundaries were also set with the same constant velocity to align this relative movement. The hydrostatic pressure condition was applied to the outlet, and the velocity here meets the zero-gradient condition. Taking advantage of the symmetry of the case, only half of the ship was put into the fluid domain, and the symmetry condition was applied on a boundary paralleling the centreplane of the ship, which can mirror the computed fluid field and save half the computational cost. The solution of the fluid domain was obtained by solving the Reynolds-averaged Navier-Stokes (RANS) equations for an incompressible Newtonian fluid: where v is the time-averaged velocity, v ′ is the velocity fluctuation, ρ is the fluid density, p denotes the time-averaged pressure, t = µ[∇v + (∇v) T ] is the viscous stress term, µ is the dynamic viscosity and g is gravitational acceleration set at 9.81 m/s 2 . Since the RANS equations have been adopted to account for the turbulent effects, a turbulence model needs to be applied to close the equations, for which, the Shear Stress Transport (SST) k − ω model (Menter 1993) was adopted. The logarithmic law wall function is applied to resolve the boundary layer (Peric 2019). The SST k − ω model has been demonstrated to be a robust RANS turbulence modelling strategy for ships due to its capability to model adverse pressure gradients and flow separation (Paterson et al. 2003). An adverse pressure gradient means the pressure increases in the direction of the flow, which can happen when a water flow encounters a hull, especially around the stern region (ITTC 2014a). The review of Pena and Huang (2021) shows the SST k − ω model is a comprehensive RANS scheme for ship hydrodynamic simulations in both model and full scales. The free surface between the air and water was modelled by the Volume of Fluid (VOF) method (Hirt and Nichols 1981). The VOF method introduces a passive scalar α, denoting the fractional volume of a cell occupied by a specific phase. In this case, a value of α = 1 corresponds to a cell full of water, and a value of α = 0 indicates a cell full of air. Thus, the free surface, which is a mix of these two phases, is formed by the cells with 0 < α < 1. The elevation of the free surface along time is obtained by the advection equation of α, expressed as Equation (3). For a cell containing both air and water, its density and viscosity are determined by a linear average according to Equation (4) and Equation (5). In this study, ρ water = 1010 kg/m 3 , µ water = 8.93 × 10 −4 N·s/m 2 , ρ air = 1.16 kg/m 3 , µ air = 1.86 × 10 −5 N·s/m 2 , according to measurements in sea trials where the seawater and air temperatures were respectively 25 and 30 degrees Celsius. The governing equations of the fluid domain were discretised and solved using the Finite Volume Method (FVM) (Versteeg and Malalasekera 2007); Figure 3 shows the mesh layout of the model, in which local mesh refinements are applied around the hull, to the free surface region and where Kelvin waves are expected to occur.

Verification and validation
Further verifications were conducted for the ship resistance to ensure that the numerical uncertainty is insignificant. This was also to choose a suitable mesh density to start with, minimizing the waste of computational resources. To perform the verifications, the shaft speed rpm = 106.4 was adopted, corresponding to 13 knots, which is close to the design service speed of Regal. The mesh of the CFD model was globally scaled into four sets of meshes, consisting of 7.5, 10.6, 15.2 and 21.1 million cells respectively, and then corresponding ship resistance results were obtained. According to Equation (6), the total resistance (R T ) is made non-dimensional into a total resistance coefficient (C T ).
The C T values predicted using the four sets of mesh are presented in Figure 4. It shows that C T achieved a monotonic convergence (Celik et al. 2008): it gradually approaches a certain value and the variance is not significant when the cell number is larger than 15.2 million. Thereafter, the mesh with 15.2 million cells was selected to start further investigations. The convergence of C T with this mesh set is presented in Figure 5. Minimal oscillation can be observed along with the convergence of the curve, where the oscillating level is less than 1% of the C T magnitude and this can be considered reasonable during numerical calculations. This oscillating level is sufficiently small to have no impact on the present result analysis. Therefore, the simulation was not run longer for analysis and the average value was taken from the last 20 s of data. For further cases tested in Section 3, all cases will be run for 200s and taken the last 20 s data to analyse the oscillating level when the CFD inputs changed. When a large oscillation occurs for a case (> 1%), the oscillating level will be plotted as an error bar. The timestep size for all of the four sets of mesh was controlled following a mean Courant number (Co), as expressed in Equation (7).
where Dt is the timestep size, u/DX is its normal velocity divided by the distance between the cell centre and the centre of the neighbour cell. The work started by setting Co ≤ 10, and this choice will be justified in Section 3.3.
Upon the verification, validation was conducted by comparing the propeller torque results from full-scale CFD with those measured during the sea trials. This validation was added as it was impossible to directly measure resistance in sea trials, thus comparison on the torque coefficient is legitimate. The comparison was performed for all three shaft speed conditions of the sea trials, as introduced in Table 2. In the CFD simulations, a Moving Reference Frame (MRF) is applied to simulate the propeller operation, where the propeller rotation is modelled by using the sliding mesh technique. A refined mesh (25% of the surrounding mesh) is applied around the propeller, as shown in Figure 6. The torque coefficient K Q was determined according to Equation (8): where Q is the propeller torque, calculated as the surface integral of fluid force in the y-direction times its distance to the propeller centre; D is the diameter of the propeller and n is the shaft revolutions (rotation per second). Figure 7 compares the sea trial K Q with that calculated from CFD, where good agreement was achieved. The deviation is less than 5%, which can result from combined errors from RANS, discretisation, uncertainties and statistics (Freitas 2002;Celik et al. 2008;Pena and Huang 2021). This deviation level is deemed to be small enough for the present study, while it is worth noting that the deviation from RANS could be further reduced by using a Detached Eddy Simulation    (DES) turbulence modelling method (Pena et al. 2020b). DES however would lead to a much higher computational cost, thus the current study focuses on RANS.
The ship-generated waves were also compared between full-scale CFD and the sea trials, as shown in Figure 8. Despite the sea trials do not have quantified measurements of the free surface elevation, it can be seen from the photo that full-scale CFD can reproduce the vessel-generated wave pattern with high fidelity, demonstrating that the fluid behaviours are correctly retained at the real-ship scale. This allows detailed analyses of localized flow behaviours and fluid-structure interactions, one of the advantages of running the simulation directly in full scale.

Investigation plan
The above work has built a model that can accurately reproduce a full-scale ship advancing in open water. The validated model is therefore now used as a base case (Case 1), which evolves into 34 other cases investigating different computational setups, as listed in Table  3. The 35 cases use systematically different computational setups. A progressive scale factor of 2 √ is used between the cases, since 2 √ is the standard ratio of varying computational setups for ship-related CFD (ASME 2009; ITTC 2017), which is supposed to detect notable influences. Specifically, Cases 2-4 investigate the overall cell number of the simulation, already presented in Section 2.3; Cases 5-17 ascertain the appropriate cell size for the free surface region and Kelvin wave region, to be reported in Section 3.1; Cases 18-28 determine the thickness of near-hull layer mesh and the expansion ratio of mesh thickness between layers, to be presented in Section 3.2; Cases 29-32 and 33-35 respectively study a suitable timestep size and the orders of spatial and temporal discretisations, as in Section 3.3. Considering these cases integrally, a set of ideal computational setups will be deduced in the end.

Study on ideal setups
Following the verification and validation, relevant computational setups are subtly and systematically  Varying total cell number 5-17 Varying mesh refinements in the free surface region and Kelvin wave region 18-22 Varying the thickness of near hull mesh layer 23-28 Varying the expansion ratio between the layers of the near hull mesh 29-32 Varying the Courant number to determine the suitable timestep size 33-35 Varying order of discretisations, as combinations of: Spatial 1st + Temporal 1st Spatial 1st + Temporal 2 nd Spatial 2 nd + Temporal 1st Spatial 2 nd + Temporal 2 nd varied to derive an ideal approach that can minimize computational costs, whilst maintaining the accuracy. This section investigates the least cell number, the largest timestep size and the least orders of discretisation that are required to accurately model the ship-generated wave, hull boundary layer and corresponding resistance components (pressure and friction). By combining the computationally cheapest but still accurate setups, a collective recommendation is formed for the full-scale ship simulation.

Ship-generated waves
Accurately modelling ship-generated waves requires an appropriate meshing approach for the free surface in the vertical direction and for the Kelvin pattern in the horizontal direction, which is important for correctly predicting the flow behaviour and ship resistance (especially the pressure component). For this purpose, it is recommended to refine the mesh in the key regions whilst applying relatively coarse meshes in other regions. This treatment helps minimize the computational cost, known as the local mesh refinement, which is especially useful considering the enormous domain dimension of full-scale ship simulations. Figure 9 demonstrated the mesh refinements recommended by this work, including the dimensions of each refining region. For both the vertical and horizontal directions, three refinement regions are applied to gradually transform the mesh. The gradual mesh scaling is for avoiding a dramatic change of cell sizes between a refined region and its outer region that can cause significant numerical errors and even lead to simulation divergence. Each horizontal-refining region consists of a circle area for bow waves, a triangle of a 20-degree acute angle to cover the Kelvin angle (∼19.47°), as well as a rectangular area for wave radiations accounting for the relative speed between ship and water, presented in Figure 9(a). Each vertical-refining region expands vertically from the waterline to both the upside and downside, as presented in Figure 9(b). The refined mesh is finest in the innermost region, gradually increasing outwards; following this order, the cell sizes in the horizontal regions are donated by DX 1 , DX 2 and DX 3 , where DY = DX in each level, and the cell sizes in the vertical regions are donated by DZ 1 , DZ 2 and DZ 3 . The corresponding overall mesh view can be seen in Figure 3.
To investigate the ideal mesh setups to model the ship-generated waves, the refinement mesh densities for the horizontal and vertical regions were evolved into six extra cases respectively, as listed in Table 4, in which, DX and DZ are nondimensionalised by ship beam (B) and ship draught (T). The results were analysed using the pressure resistance coefficient (C P ), converting from pressure resistance component (R P ) by C P = R P /0.5r water S w U 2 ship , since this is dominated by changes in the wave.
The changing trend of C P with different cell sizes in the mesh refinement regions is plotted in Figure 10. It shows the change in the horizontal direction is less sensitive than in the vertical direction. Also, with the mesh density being reduced, the convergence of C P changes from stable, as in Figure 11(a), to unstable, as in Figure 11(b) where C P oscillates at the tail. The upper and lower limits of the time-domain oscillation are plotted as error bars in Figure 10. When the mesh becomes sufficiently dense, the oscillating level becomes less than 1% of the magnitude, which is negligible and hardly distinguishable. Therefore, there are no error bars for those cases.
To keep an accurate resistance prediction while minimizing computational costs, the selected cell sizes are DX 1 = 0.044B (Case 7) and DZ 1 = 0.017T (Case 12); these are the suitable mesh densities for C P , which were tested separately.
Then, an extra test (Case 17) combines both the selected cell sizes from Case 7 and Case 12 to further confirm the accuracy, and the results were similar to the validated case (Case 1). By optimizing the mesh refinements for modelling ship-generated waves, the total cell number of the CFD model was successfully reduced from 15.2 million in Case 1 to 11.7 million in Case 17, while the two cases can get the same accurate results.

Boundary-layer flow around the ship
The boundary-layer flow around the ship is modelled by mesh layers built upon the hull surface, in which, the layer attaching to the hull is thinnest, and the thickness of each layer gradually increases outwards, so that the thickness of the outmost layer is close to the size of cells outside the mesh layers, as shown in Figure 12. To properly model the boundary layer flow, it is necessary to know (a) the total thickness of the layers (b) how thin the layers should be, and (c) what ratio should the layer thickness increase to. The boundary layer thickness on the majority of the wetted surface of a vessel at 13 knots is measured to be around d = 0.015 m (Ohta et al. 2008), while the thickness can progressively thicken towards the aft region (Pena et al. 2020a). Therefore, criterion (a), the total thickness of the layer-mesh region, was set at a conservative level of 0.1 m to capture the boundary-layer regions. For criteria (b) and (c), sensitivity analyses are performed to investigate their ideal setups, which is done through varying the thickness of the innermost near-wall layer, h, and the thickness expansion ratio between layers (E). The test cases are listed in Table 5, combining different sets of layer thickness and expansion ratio for the layer-mesh region; the optimized case from Section 3.1, Case 17, was adopted as the base case here. The results were analysed using the  Near-hull mesh setup: mesh layers were built between the hull geometry (upper right) and the regular mesh domain (lower left); dense mesh was applied near the hull surface, which gradually coarsens away from the hull surface. friction resistance coefficient (C F ), converting from friction resistance component (R F ) by C F = R F /0.5 r water S w U ship 2 , since this directly reflects the boundary layer effect. The influences of the layer thickness and expansion ratio on C F are shown in Figure 13. Figure 13 (a) shows that C F starts to diverge when h/ d is larger than 0.3. This means that the thickness of the innermost mesh layer cell should be less than 30% of the actual boundary layer thickness. Figure 13(b) shows that E should be no larger than 1.5 to secure the convergence of the solution. On account of these results, the setups in Case 25 are optimal, i.e. h/ d = 0.3 and E = 1.5.
To further check the accuracy of the friction prediction, C F predicted by the widely used ITTC57 empirical equation is also included in Figure 13(b), expressed as Equation (9) (ITTC 2014b). It can be seen that the CFD results are around 5-10% larger than the ITTC57 results. This agrees with the validation for full-scale ship simulations by Niklas and Pruszko (2019) and by Eça and Hoekstra (2008), both reporting their full-scale CFD prediction of C F is around 5-10% larger than the ITTC57 line. This is also the case for the LR workshop (2016), in which all participants reported that full-scale CFD predicts higher frictional resistance than the ITTC57 line. Thus, the contemporary ITTC formula appears to underestimate C F in full scale, which is reasonable as the formula is derived based on empirical data in model scale. This suggests an updated version of ITTC equations may be derived when more full-scale measurements and quality CFD data become available, e.g. through a similar   procedure as in (Huang et al. 2021a).
C F = 0.075/(log 10 Re − 2) 2 (9) The near-wall cell thickness h can be converted into a non-dimensional value Y + that is commonly used to guide the construction of the boundary layer mesh in CFD. The expression of Y + is taken from (ITTC 2014a) and given as Equation (10) here. Figure 14 presents the Y + is around 1000 for h/ d = 0.3, when accurate results were obtained in this work. Whilst the current ITTC guideline suggests Y + to be less than 100 for RANS simulations of the same case in model scale (ITTC 2014a), this result shows that it can be unnecessary to use such a low Y + value in full scale.
Particularly, this signifies a considerable waste of computational resources if following the model-scale standard to build full-scale simulations. This finding corroborates the inference of Peric (2019).
More detailed analyses of the boundary layer have also been conducted, in which ten frames (FR) were    identified on the ship, as shown in Figure 15, and the flow in each FR was investigated. The simulated boundary layers are shown in Figure 16, where the visualized boundary layers were filtered according to the criterion of horizontal velocity equals to or less than 0.99U water . A thickening boundary layer towards the downstream direction can be seen, and a bulge is formed and grows whilst the boundary layer thickens. Nonetheless, since the sea trial did not provide measurements on the ship's boundary flow details, specific CFD setup for this level of flow details cannot be investigated as part of this work, while a full report on the boundary layer analysis can be found in (Pena et al. 2020a).

Numerical schemes
There are two types of discretisation in the FVM computation, respectively in space and time. In space, the computational domain is divided into a set of nonoverlapping cells, known as a mesh; in time, the temporal dimension is split into a finite number of timesteps. For a single timestep, the solution of the governing equations can be obtained in each cell (e.g. v, P, α), and the whole fluid domain can be integrated by the solution obtained for all cells. Then, the fluid domain over a certain time duration is the composition of the fluid domain at each timestep. Following previous sections that investigated different mesh setups, this section studies how to set an appropriate Figure 19. C P and C F obtained with different temporal and spatial ODs; the percentages of friction and pressure components are approximated at 44% and 56% for the sensible cases (Cases 25 and 35). timestep size, Dt, and the Order of Discretisation (OD) in spatial and temporal domains. The corresponding test cases are shown in Table 6. The timestep size is controlled by prescribing the mean value of Courant number as given in Equation (8). Figure 17 shows the influence of the timestep size on the total resistance of the ship, in which the resistance is close to the verified value when Co ≤ 10 and a large change occurred when Co was increased to be larger than 10. Similar to the finding on Y+, the threshold value of Co in full scale (≤ 10, as shown in Figure 18) is much larger than that in the current model-scale guideline which suggests Co to be ≤ 1.
A further investigation was conducted on the OD. For CFD ship simulations, common-used ODs for temporal and spatial discretisations are 1st and 2 nd orders; details of the algorithms are given in (Kuzmin 2010). Therefore, there are four tests in this regard by the matrix of 1st and 2nd temporal ODs vs 1st and 2nd spatial ODs. Figure 19 shows that the four sets predict almost identical friction resistance, while 1st spatial OD induced a significant overprediction in pressure resistance (see Case 33 and 34). This means although all four sets of ODs are capable of modelling the hull boundary layer, 1st spatial OD is incapable of modelling ship-generated waves, which is further corroborated by Figure 20. Therefore, it is necessary to apply 2 nd spatial OD. For 1st and 2 nd temporal OD, they took similar computational time and have no notable difference between their computational results. Therefore, both 1st and 2 nd temporal OD are applicable; this finding is in line with the ITTC model-scale recommendation (ITTC 2014a).

Conclusions
There are clear benefits from running full-scale CFD simulations to predict ship performance as it can reproduce the ship hydrodynamics at the correct scale, which enables various design activities and avoid uncertainty from conducting model-scale extrapolation procedures. The accuracy of full-scale ship simulations is dictated by computational setups, and the suitable setups differ considerably from those in current model-scale guidelines.
To investigate ideal computational setups for fullscale ship CFD and contribute to its future guidelines, this work first developed a full-scale model for simulating a cargo ship advancing in open water and validated the model against sea trials. Subsequently, a series of simulations were performed to investigate the influences of most important computational setups on the simulation results. These setups include mesh density, mesh transition ratio, mesh local refinements, timestep size, and the orders of discretisations. Their influences are studied on the predictions of ship resistance, ship-generated waves and the ship's boundary layer flow.
An optimized set of setups were obtained that can minimize the computational cost whilst keeping the accuracy, as summarized in Table 7. The present work deduced the computationally cheapest but still accurate mesh density possible, resulting in a total cell number of around 11 million. In addition, it was shown that the most inner layer-mesh thickness around the hull should be less than 30% of the expected boundary layer thickness, while the stretching layers can gradually increase their thickness at a ratio of 1.5. Moreover, it was demonstrated that the 2 nd order must be used for spatial discretisation while either the 1st or 2 nd order can be used for temporal discretisation. In particular, the results highlight that the suitable Y + and timestep sizes for full-scale ship simulations can be approximately ten times those in the current model-scale guideline. Such differences in mesh and timestep selections indicate the importance to develop a separate guideline for full-scale ship CFD. Otherwise, there can exist significant wastes of computational resources, as users might just follow the model-scale guideline to set up fullscale cases.
The present methodology could also be applied to study the full-scale ship CFD for other applications, such as predicting a ship's seakeeping, manoeuvring, and performance in restricted waters. Noting that this work only investigated one hull form, the recommended mesh setup can be adapted to other hull forms, based on the given ratios between mesh densities and ship particulars. However, since the studied ship size is 138 m, for another ship that has a significantly different size, e.g. a small boat, some of the recommendations may need to be derived separately, as such a size difference could cause a scale effect.
In practical engineering design, the recommended full-scale CFD setups are beneficial in terms of helping users set up similar simulations with correct numerics and minimal computational resources, which has been a key element in contemporary developments for the Ship-generated waves Layout: Figure 8 Cell size: Case 17 in Table 4 Boundary layer Layout: Figure 11 Cell size: Case 25 in industry of ships as well as offshore structures (Lloyds Register 2016;Fazeres-Ferradosa et al. 2019Terziev et al. 2022). However, noting that the verification and validation in this work were conducted on a global quantity (resistance), the accuracy of the recommended CFD setup in local flow details was not evaluated. Other CFD setups might be needed for ship hydrodynamic applications that rely on local flow details, e.g. cavitation (Lu et al. 2012) and hydroacoustics (Smith and Ventikos 2021). It is expected that future ship operations will include more sensors to obtain local measurements on flow and structural details, which will provide essential data for validating the full-scale CFD of this field as well as inform the optimization of ship performance ).

Disclosure statement
No potential conflict of interest was reported by the author (s).