## 2 Numerical Simulations Method and Response of Structure
### Finite Element Modeling  
Several groups of numerical simulations were performed using the Abaqus/Explicit finite element package (Version 6.14), to verify the applicability of the proposed method in scaling the models distorted in the plate thickness and stiffener configuration. For all simulation cases, four-node shell elements (S4R) with five integration points throughout the thickness were used to model the stiffened plates and impact blocks. High-strength struck impact blocks enable the use of rigid-body restrictions [10]. The element size of the mesh significantly influenced the numerical simulations--that is, the fracture strain. Therefore, mesh size convergence analyses were conducted with the objective of determining the optimal mesh size for the FE model. Five mesh sizes were applied to the prototype specimen, as shown in Table 2. The same mechanical properties and load case were applied to the numerical simulation until the specimen separated from the indenter, and the acceleration of the indenter was obtained. The simulation \begin{table}
\begin{tabular}{c c c c} \hline \hline
**No.** & & **Prototype** & **Reference Model** \\ \hline Geometry dimensions & Attached plate dimension (mm) & 6400 \(\times\) 3400 & 640 \(\times\) 340 \\  & Attached plate thickness (mm) & 13 & 1.3 \\  & Stiffener & & \\  & dimension (mm) & \(\perp\frac{390\times 11}{125\times 15}\) & \(\perp\frac{35.0\times 1.1}{125\times 15}\) \\ Load case & \(M_{S}\) (t) & 3.29021 & 0.00329 \\  & \(R_{\text{f}}\) (mm) & 800 & 80 \\  & \(v_{0}\) (m/s) & 3 & 3 \\  & \(M_{\text{f}}\) (t) & 400 & 0.4 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Relevant parameters of prototype and reference model. Figure 3: Schematic and dimensions of prototype struck system (unit: mm). time and the corresponding resistance behaviors of the five mesh sizes were collected and compared. The results indicate that the mesh gradually converged from 100 mm to 15 mm. Compared with Case 5 (15 mm mesh model), the simulation deviation of Case 4 (20 mm mesh model) is minimal, while the time required is halved. Considering the simulation accuracy and calculation efficiency, the mesh size was selected as 20 mm for both the prototype stiffened plate and the impact block (R\({}_{\text{I}}\) = 800 mm) to sufficiently capture the large deformation characteristics, whereas the counterpart applied in the perfectly similar model with an overall scaling factor of 1/10 was 2 mm, to keep the mesh numbers the same as the prototype. A revolving rigid part was used to model the semispherical impact block. The x-, y-, and z-axes correspond to the plate length, stiffener, and vertical directions, respectively. Additionally, the initial impact velocity placed at the center of gravity of the impact block was assigned in the vertical direction. Furthermore, the impact block was initially positioned to strike the stiffened plate at a 20 mm offset along the \(z\)-axis from the center of the plate, to guarantee convergence time during impact simulations. Figure 4 illustrates the general model and constraints used in the numerical simulations. To match the experimental constraints, the boundary condition was selected to be fully clamped onto the four edges of the specimen. The contact of mild steel between the hemi-spherical indenter and the attached plate was modeled in Abaqus as General Contact, assuming a recommended friction coefficient of 0.23 [28], while the damping was neglected in the simulations. Because the boundary conditions and contact definition significantly influence dynamic behaviors in impact events, the same restrictions and properties were applied in all simulation cases. The prototype structure was designed to be manufactured using a mild steel similar to NVA shipbuilding mild steel, a material that is typically ductile. Material properties were determined based on the previous research conducted by [PERSON] and [PERSON] [29]. Across all scenarios, the material was modeled using a nonlinear elastic-plastic constitutive