## 2 Materials and Methods
### Numerical Modeling of Corrugated Board Packaging including Overhanging  
In order to examine the impact of overhang on the load-bearing capacity of the packaging, numerical models were created in commercial FE software (Abaqus Unified  
Figure 1: Graphical abstract of the study presenting the reference packaging and packaging with three types of overhanging. FEA 2020 [37]). A total of 1120 different packaging variants with possible combinations of overhanging were analyzed for each of the four selected cardboards, which gave a total of 4480 cases. In all of the 4480 numerical models, the linear elastic orthotropic constitutive model with Hill plasticity [38] was adopted. The Hill model is an extension of von Mises plasticity. The addition of the Hill potential indirectly decreases the strength of the cardboard in the machine direction. The material parameters of the boards were acquired using BSE System [5] via mechanical tests of bending, edge crushing, shearing and twisting. Five board samples were used for each test of the particular board to obtain a reliable representation of mechanical properties of the material for later use in numerical modeling. The final material parameters used in the study are presented in Table 1, where \(E_{1}\) is the Young modulus in the machine direction; \(E_{2}\) is the Young modulus in the cross direction; \(v_{12}\) is the Poisson ratio; \(G_{12}\) is the Kirchhoff modulus; \(G_{13}\) and \(G_{23}\) are the transversal shear stiffnesses; \(\sigma_{0}\) is the yield strength; and \(R_{11}\) is the yield strength factor according to the Hill potential, which is applied in the machine direction [37]. In the finite element method (FEM) model built in Abaqus FEA environment, only the load-bearing walls of the box were simulated. The top and bottom flaps were taken into account by applying appropriate boundary conditions, specifically blocking out-of-plane translational displacements at the top and bottom edges of the packaging. In preliminary analyses, the behavior of the packaging with modeled top and bottom flaps was checked. The resulting decreases in load capacity due to overhanging turned out to be smaller than those obtained in the main phase of calculations. It follows that replacing the flaps with appropriate boundary conditions places us on the safe side. To simulate the compression test, downward vertical displacement was applied to the upper edges until the maximum load capacity of the box was achieved. Moreover, depending on the presence or absence of overhanging, vertical displacement was blocked on the entire length of the bottom edges or only on their part depending on the overhanging magnitude assumed. In Figure 2, the boundary conditions and the finite element mesh for several overhanging variants for a \(300\times 150\times 300\) box are shown. The strength analysis of each packaging consisted of two stages. In the first step, a buckling analysis was performed, from which the shapes of global imperfections were obtained. In the second calculation step, the first mode from the buckling analysis was applied to the box, which was loaded kinematically with vertical displacement until the maximum load-bearing capacity was achieved. Buckling and compression analyses were performed for each of the 4480 variants of the material, geometry and overhanging, which gave a total of 8960 analyses. In all models, the four-node quadrilateral shell elements with full integration were applied, labeled as S4 according to Abaqus FEA [37]. For each variant, the FEM mesh was selected individually in order not to exceed 1000 finite element nodes. For example, for the \(300\times 150\times 300\) box with 20% diagonal overhang (shown in Figure 2d), a global mesh size of 19 mm was assumed, which resulted in 884 nodes, 768 elements and 5304 degrees of freedom. A thorough convergence study was conducted to ensure the accuracy of our results. Given the extensive computations involved--almost 9000 in total--a thoughtful choice was made regarding the number of finite element analyses.