1. Introduction
The requirements for efficient and sustainable maritime transport are a pressing issue in the face of global climate change. A significant contributor to this challenge is the hydrodynamic performance of ships, which directly impacts their fuel consumption and, consequently, their carbon emissions. Accurate prediction of ships’ hydrodynamic performance is, therefore, a critical aspect of ship design and operation, especially in the context of decarbonization of the shipping industry [
1]. This aligns with the global commitment to reduce greenhouse gas emissions and mitigate the impacts of climate change on sustainable development.
Ship hydrodynamic performance is traditionally predicted by extrapolating the model-scale measurements or numerical results to full scale to predict full-scale power requirements [
2]. This process involves a series of steps, including data reduction, form factor calculation, blockage corrections, speed correction, and finally, extrapolation using conventional International Towing Tank Conference (ITTC) methods. However, this approach has some limitations and uncertainties due to scaling effects and empirical assumptions. The scale effects resulting from the significant size difference between the model and the full-scale ship, along with the inherent uncertainties in measurements and extrapolation, all contribute to potential inaccuracies in the predicted performance. Furthermore, these procedures primarily address the model scale and often overlook the validation against actual full-scale data, leading to potential discrepancies between the predicted and actual performance of the ship. As such, the accuracy and reliability of full-scale performance prediction remain areas of ongoing research and development in the field of ship hydrodynamics.
Extrapolation procedures are empirical methods to correct the scale effects by applying scaling laws and correction factors to the model-scale data [
3,
4]. However, these methods are based on assumptions and simplifications that may not be valid for all ship types, speeds, and sea conditions. Moreover, these methods do not account for the nonlinear and viscous effects that are significant at full scale. The scale effect arises due to the discrepancy in force ratios experienced by a model compared to the actual ship. Scale effects arise when the model-scale experiments do not accurately represent the full-scale ship phenomena, due to different Reynolds and Froude numbers, boundary layer thicknesses, flow separation, wave breaking, etc. [
5,
6]. Therefore, further research and exploration in this area are necessary to improve the accuracy of predictions, to better understand the complex intercorrelations between scale effects and ship hydrodynamics, and to develop methods to account for scale effects. Computational fluid dynamics (CFD) simulations can play a significant role, allowing for more accurate scaling and prediction of full-scale performance.
A review of the existing methods for extrapolating the total resistance has been reported in [
2]. The authors approached the problem of predicting full-scale ship performance based on model-scale experiments and scaling laws, which are subject to uncertainties and limitations due to the complex nature of fluid flow and scale effects.
Terziev et al. [
5] challenged the assumptions imposed as part of the currently accepted ship resistance extrapolation procedure, which relies on experience-based approaches and large datasets accumulated from years of operation. Their findings suggest that a degree of uncertainty exists in the calculated full-scale resistance, depending on the approach considered. Scale effects on the wave resistance, frictional resistance, and form factor, using different methods and corrections, were extensively investigated. They found that the wave resistance and the free-surface effects on the frictional resistance are not scale-invariant, and that the form factor depends on both the Reynolds and Froude numbers, as also reported in [
4]. The authors concluded that the assumption of geometric similarity in ships’ wave patterns and resistance components is not valid, and that a more scientific extrapolation procedure is needed. Based on comparison of towing tank experiments, full-scale CFD simulations, and sea trial measurements for the ship, Niklas and Pruszuko [
7] found that the choice of form factor and friction line had a significant influence on the extrapolation of the towing tank results to full scale, leading to variations of up to 19% in the predicted resistance.
The comprehensive study of Bhushan et al. [
8] revealed the versatility of a two-point, multilayer wall function model for computing model- and full-scale ship flows with wall roughness and pressure gradient effects. The wall function model was validated for smooth flat-plate flows at Reynolds numbers up to 10
9, and it was applied to the Athena R/V for resistance, propulsion, seakeeping, and maneuvering simulations. The wall function model showed good agreement with the near-wall turbulence model and experimental data for resistance, propulsion, and boundary layer profiles. The study proved that there is a viable alternative to the near-wall turbulence model for ship hydrodynamics applications, especially for full-scale simulations where the near-wall grid resolution is prohibitive.
Tahsin et al. [
9] used a fully nonlinear unsteady RANS CFD method to predict the ship motions and added resistance of a full-scale KCS in regular head waves, at design and slow-steaming speeds. They validated their results against experimental data and estimated the increase in effective power, fuel consumption, and carbon dioxide (CO
2) emissions due to operation in waves. Their study contributes to the literature by providing a comprehensive and detailed analysis of the scale effects in ship hydrodynamics using a state-of-the-art CFD method.
The nominal wake field is important for propeller design and performance, as it affects the efficiency, cavitation, and hull–propeller interaction. However, few studies have focused on how the nominal wake field is influenced by sailing in waves, which is a common situation for most ships. Mikkelsen et al. [
10] simulated the KCS at model scale and estimated the ship’s motions and wake field in regular waves with a wavelength equal to the ship length.
The work of Bart Schuiling et al. [
11] investigated the scale effect on the prediction of hull pressure fluctuations induced by cavitating propellers. The authors discussed the challenges and limitations of designing and testing non-geosim (geometrically similar) models with prescribed wake characteristics. The scale effect of the nominal wake field of the KCS container ship was investigated by Zhang et al. [
12] using the RANS method. Their scope was to solve the viscous flow field of the KCS ship at different scales without considering the free-surface effect. The authors compared the numerical results with experimental data and investigated the relationship between the average axial wake fraction, the Reynolds number, and the propeller radius. The nominal wake characteristics of the KCS at model and full scale were examined by Delen and Bal [
13] based on Telfer’s GEOSIM method using CFD. The results showed better accuracy in predicting full-scale performances than other conventional extrapolation methods. The GEOSIM method was found to be more accurate and reliable compared to the 1978 ITTC method for predicting the full-scale effective wake fraction, as it captures the viscous effects in the wake region more accurately [
14]. A detailed numerical flow assessment of the boundary layer and wake of a full-scale cargo ship using an IDDES approach was reported in [
5].
CFD simulations can predict scale effects in ship hydrodynamics by providing more accurate and detailed representation of the fluid flow in the vicinity of the ship compared to traditional model-scale experiments and extrapolation procedures. CFD simulations can be performed at both model scale and full scale and can consider the nonlinear and viscous effects that are significant, especially at full scale. Therefore, CFD simulations should be used in conjunction with other methods and tools, such as model scale experiments, towing tank tests, and then compared to the full-scale measurements, to obtain a comprehensive and reliable prediction of the ship’s hydrodynamic performance.
This study presents a comprehensive comparison of model- and full-scale ship hydrodynamic flow characteristics, computed using CFD. The disparity between model- and full-scale simulations, primarily due to Reynolds number effects, Froude number effects, and scale effects on roughness, often leads to discrepancies in predicting the actual performance of the ship. Taking advantage of the CFD capabilities, this study aims to bridge this gap, providing a deeper understanding of the flow phenomena around the ship hull under various conditions. The findings of this research have important implications towards the design and operation of more efficient and sustainable ships, contributing to the broader goal of decarbonization in the shipping industry.
The KRISO (Korea Research Institute of Ships and Ocean Engineering) Container Ship (KCS) is the subject of the present study. In order to determine the wave added resistance, the first set of simulations are performed in calm water conditions. In the case of regular head wave simulations, several cases are analyzed comprising four wavelengths, including short and long waves, and three wave heights, for both calm water and regular head wave conditions. The ship speed is set to the design speed corresponding to a Froude number value of 0.261. A total number of twenty-eight simulation cases are performed and reported, following the proposed cases in the Tokyo 2015 Workshop on CFD in Ship Hydrodynamics. The objective is to estimate the wave added resistance, heave, and pitch motions in regular head waves. Also, the comparison between model and full scale for free-surface and wake flow in the propeller plane is investigated in order to understand the scale effect on the ship’s performance in calm water and specifically in waves. The numerical results are validated using the experimental data provided in the Tokyo 2015 Workshop. To evaluate the numerical errors, a verification study was conducted based on a grid and time step convergence test.
2. Numerical Approach
The numerical simulations are performed utilizing the ISIS-CFD solver, developed by the EMN (Equipe Modélisation Numérique) and implemented in Fidelity Fine Marine software version 11.1. This solver employs the finite volume method, a numerical technique used for the spatial discretization of transport equations [
15]. The primary purpose of this method is to solve the incompressible unsteady Reynolds-Averaged Navier–Stokes (RANS) equations.
The Unsteady Reynolds-Averaged Navier–Stokes (URANS) equations are equations of motion for fluid flow that are time-averaged to model turbulence. The principle behind these equations is the Reynolds decomposition, where an instantaneous quantity is broken down into its time-averaged and fluctuating quantities.
For a stationary flow subjected to external forces, the time-averaged continuity and momentum equations can be expressed in a Cartesian coordinate system as follows:
where
denotes density,
represents the vector of relative averaged velocity between the fluid and the control volume,
signifies the Reynolds stresses,
represents the mean pressure, and
is the mean viscous stress tensor component for a Newtonian fluid under the assumption of incompressible flow, and it can be written as:
where
is the dynamic viscosity.
Turbulence closure, a critical aspect of fluid dynamics simulations, is accomplished using the k-ω Shear Stress Transport (SST) model [
16]. This model employs a near-wall resolution based on a wall function, which is a strategy to manage the computational complexity near the wall in turbulent flow simulations.
The construction of unstructured meshes, which are flexible and efficient for complex geometries, is facilitated by a generalized three-dimensional face-based method. This method allows for the creation of meshes that can adapt to the geometry of the problem, improving the accuracy of the solution.
The coupling of velocity and pressure, two fundamental quantities in fluid dynamics, is achieved using the Semi-Implicit Method for Pressure-Linked Equations (SIMPLE) [
17]. In this approach, the velocity field is derived from the momentum conservation equations, while the pressure field is extracted from the mass conservation constraint, also known as the continuity equation [
18]. This constraint is then transformed into a pressure equation.
The simulation of free-surface flow, which is the flow with a free surface at its boundary such as the waterair interface, is conducted using a multi-phase flow approach. This approach is based on the volume-of-fluid (VOF) method, a popular method for capturing the free surface in computational fluid dynamics.
The modeling of incompressible and non-miscible flow phases, where the fluids do not mix and maintain a constant density, is performed using conservation equations for each volume fraction of phase/fluid [
19]. This approach ensures the accurate representation of each phase or fluid in the flow.
The convection and diffusion terms in the RANS equations, which represent the transport of quantities due to bulk fluid motion and random molecular motion, respectively, are discretized using a second-order upwind scheme and a central difference scheme. These schemes provide a balance between accuracy and computational efficiency.
For time discretization, an implicit scheme is applied. This type of scheme offers stability for larger time steps, making it suitable for unsteady computations. Furthermore, a second-order three-level time scheme is employed for time-accurate unsteady computation, ensuring the accuracy of the solution in time-dependent problems [
20].