## Structural Responses of the Deck and Breakwater  
### Modelling of the Ship Bow Structures  
To investigate the structural response of the deck and breakwater structures under freak waves, it is essential to establish a finite element model of the ship. The dimensions of the container ship were identical to those detailed in Section 4.1. To reduce computational costs, the bow section was selected for the model. The slamming areas subjected to green-water wave loads lack a clear definition among classification societies across various countries. [PERSON] et al. [23] and [PERSON] et al. [24] conducted research on the slamming load characteristics from the bow to the superstructure area. According to the guidelines of DNV [53], BV [54], GL [55], and KR [56], the impact zone of the bow flare and bottom is situated at a range of 0.1 L from the FP (forward perpendicular) [29; 57]. Based on this information, the truncated region extending 0.1 L from the FP is selected as the slamming region to construct an FEM model of the ship's truncated bow, which is illustrated in Figure 14.  
The finite element model employs three types of elements: plate elements are primarily utilized to simulate the shell structures of various components, including the deck, side shells, longitudinal bulkheads, top transverse bulkheads, deck beams, transverse bulkheads, panels, transverse webs, hatch coaming and its panel, and elbow plates. The majority of plate elements are quadrilateral elements, with a minimal number of triangular elements used for component connections and arc transitions. Beam elements are mainly used to simulate large and continuous longitudinal members, such as stringers, stiffeners, and supporting materials, while accounting for beam cross-sections and eccentricities based on actual conditions. Rod elements are mainly used to simulate small-sized reinforcements, such as openings in panels and discontinuous stiffeners. With a total count of 44,476, the deck and breakwater were set to a grid size of 0.7 m, which is fine enough for finite element analysis [29; 57; 58; 59]. In addition, mesh convergence testing were conducted. Mesh sizes ranging from 0.3 m to 1.0 m were chosen, and Figure 15 shows the variation in the peak von Mises stress at Deck D111 and Breakwater B105 (the positions of D111 and B105 are shown in Figures 8 and 9) under different mesh sizes. It can be seen that the results converge when the mesh size is less than 0.7 m, and as the size is further reduced, the peak stress difference is less than 2%. Excessively small mesh sizes would significantly increase computational time, which means that a mesh size of 0.7 m can be considered appropriate for simulating the impact problem in this paper. The time step used for finite element analysis was 0.0045 s.  
Figure 14: Three-dimensional finite element model of ship bow. The computer used for the paper is equipped with two AMD EPYC 7402 2.8 GHz CPUs and 128 GB of memory. The time required for mesh independence verification was 624 min, and the average convergence time required per time step was 30 s when performing finite element analysis with a mesh size of 0.7 m.  
Reasonable boundary conditions are critical for calculating the dynamic response of structures subjected to slamming loads. [PERSON] et al. [29] used a six-degree-of-freedom constraint to determine the truncation position. [PERSON] et al. [58] indicated that only the aft-side of the model was fixed in six degrees of freedom to ensure that all forces could be balanced with minimal boundary effects on the six brackets. The approach described above was fixed in this article to constrain the ship bow, as illustrated in Figure 16.  
Parameters of the finite element model are as follows: elastic modulus \(E\) of 2.06 \(\times\) 10\({}^{5}\) MPa, Poisson's ratio \(v\) of 0.3, and material density \(\rho\) of 7.8 \(\times\) 10\({}^{3}\) kg/m\({}^{3}\). When subjected to slamming pressure, the constitutive behavior of the material differs from that observed under static loading conditions.