## 2 Materials and Methods
### Numerical Simulation Analysis  
Creo Parametric 8.0 and Ansys 2022R1 [31] were used for 3D modeling and finite element analysis of EPS boxes under stacking load. The simulation analyzed three cases, namely Sim22, Sim23, and Sim23X, corresponding to test groups EPS-B22, EPS-B23, and EPS-B23X in the stacking strength test. Two types of materials were defined in Ansys--namely EPS 22 and EPS 23--corresponding to densities of 22 and 23 kg/m\({}^{3}\). Both materials were set as isotropic elastic with bilinear kinematic hardening in terms of elastic and plastic properties. The material parameters used in the simulation, except for density \begin{table}
\begin{tabular}{l l l l l} \hline \hline
**Test Group** & **Dimension (mm)** & **Weight (kg)** & \
\begin{tabular}{l} **Measured Density** \\ **(kg/m\({}^{3}\))** \\ \end{tabular} &
\begin{tabular}{l} **Amount for Stacking/Bottom** \\ **Strength Tests (pcs)** \\ \end{tabular} \\ \hline EPS-B22 & 400 \(\times\) 265 \(\times\) 126 & 0.110 & 22.7 & 5/5 \\ EPS-B23 & 400 \(\times\) 265 \(\times\) 126 & 0.115 & 23.8 & 5/5 \\ EPS-B23X & 400 \(\times\) 265 \(\times\) 122 & 0.113 & 23.8 & 5/5 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Details of EPS boxes for stacking strength and bottom strength tests. Figure 4: Strength test setups for EPS boxes. (**a**) Stacking load. (**b**) Bottom load. Note: in the bottom load test, the plate beneath was ring-shaped with a hole slightly larger than the top plate. Figure 5: Box dimensions of EPS-B22/EPS-B23. Unit: mm. and Poisson's ratio, were derived from experimental results. The parameters are given in Table 3. Note that if the Young's modulus and the tangent modulus were derived from literature, the values would deviate far from those of the experimental results. The 3D models were engineered in the static structural analysis component to reproduce the quasi-static stacking loading test. To shorten the time of calculation, only a quarter of the box was simulated and symmetrical boundary conditions were applied as shown in Figure 6a. Two rigid plates covered top and bottom surfaces in an imitation of evenly distributed load, and supports were modeled as individual entities. In pre-processing, virtual topology was approached to generate high-quality mesh, as shown in Figure 6b. Small features such as rounding were stitched to the adjacent surfaces to avoid skewness caused by size mismatch. In meshing, physical preference was set to nonlinear mechanical, and quadratic elements were used. Furthermore, the hex-dominant method, body sizing, face sizing, and contact sizing were applied. The element size was 4 mm, and a total of around 40,000 elements were generated in each case. The average mesh quality was controlled above 0.85, and the mesh is shown in Figure 6c; since the plates were rigid bodies, automatically-generated mesh was only used on the contact surfaces instead of overall. The box body and the lid were assigned as either EPS 22 or EPS 23, whilst the top and bottom plates were always structural steel with rigid behavior. There were three pairs of contact in the model--top plate and lid, lid and box body, box body, and bottom plate. To stabilize the calculation, penetration tolerance, normal stiffness, and stabilization damping factor were set up in contact pairs. The bottom plate was fixed to the ground, whilst the top plate was set as a translational joint and was moved downwards by 10 mm, imitating the setup of the experiment. In static structural analysis, a simulation may have convergence problems if the deformation is too high and the elements become highly distorted. At 10 mm displacement of the top plate, the boxes had already yielded and plastic strain occurred, which was sufficient for making comparisons with experimental results. Therefore, considering calculation efficiency and practical needs, the top plate was set to move 10 mm downwards. Figure 6: Pre-processing of 3D model of EPS box. (**a**) Symmetry setting, the areas in red represented planes of symmetry. (**b**) Virtual topology. (**c**) Mesh results.