# Advanced Numerical Analysis of Transport Packaging
## 2 Materials and Methods
### Estimation of the Packaging Resistance to Transport Loads  
According to the aims presented in the previous paragraphs, a numerical tool was developed for calculating changes in the compression strength of a specific box, following representative environmental vibrations experienced during transportation. As illustrated in [30], the process begins with a buckling analysis, to describe a possible numerical imperfection field, followed by a static FEA of the box in a stress-free state. This initial step allows for the determination of \(BCT_{0}^{ij}\), which represents the compression strength of the box prior to the vertical random vibration test. Next, a modal analysis of the box is performed, and the results, along with Power Spectral Density (PSD) data, from standard ISO 13355 [24], serve as inputs for the random vibrations analysis. In the subsequent step, a displacement boundary condition, corresponding to a specific resonant frequency, is applied to the bottom of the box during a dynamic analysis that simulates fixed-frequency vibrations. After a selected number of cycles, a quasi-static compression test is numerically conducted. This final analysis yields to the updated (reduced) \(BCT^{ij}\), representing the compression strength of the box under a given transport condition, subjected to possible damages. Both the static and dynamic analyses of box testing mirror laboratory test conditions. In the developed finite element models (see, Figure 3), only the quarter of load-bearing walls of the packaging are considered, while the bottom and top flaps are simulated by applying suitable boundary conditions, namely with out-of-plane displacements at the bottom and top edges of the sidewalls constrained. The complete set of numerical analyses, conducted on the different models, account for three classes of simulations, namely random vibrations, static compressions and dynamic vibrations, which are also supported by buckling and modal analyses. Given the numerical difficulties related to the investigation of vertical random vibrations in the time domain, the research adopted an efficient approach for modelling the VRV test of corrugated board packaging, as proposed in [30], utilising modal analysis to identify resonant frequencies for subsequent employment in dynamic finite element analysis with a set vibration frequency. \begin{table}
\begin{tabular}{c c c c c c c c c} \hline \multirow{2}{*}{**No. **} & \( \begin{array}{c}\mathbf{E_{1}}\\ \textbf{(MPa)}\end{array} \) & \( \begin{array}{c}\mathbf{E_{2}}\\ \textbf{(MPa)}\end{array} \) & \( \begin{array}{c}\mathbf{v_{12}}\\ \textbf{(MPa)}\end{array} \) & \(\begin{array}{c}\mathbf{G_{1  
The box compression test was simulated by applying a vertical displacement to the top edges of the box. In addition to the static model, a rigid plate was incorporated into the dynamic analysis to replicate the standardised load utilised in an experimental test. Moreover, the dynamic analysis consisted of two computational steps, i.e., the application of gravity, enforcing the plate to descend onto the packaging, with contact interaction, and the imposed vibration of the bottom of the box, in the time domain, with the sinusoidal amplitude and frequency derived from the modal analysis. As introduced in previous sections, Sections 2.1 and 2.2, and in Figure 1, static and dynamic analyses were performed for thirteen corrugated board materials (Table 2) and three box geometries (Figure 1). In each run, the constitutive model employed was a linear elastic orthotropic material with Hill plasticity. The numerical analyses and the gathered computational results collected in the following section, Section 3, were developed employing the finite element software Abaqus 2020 [46]. For the modelling of the corrugated board boxes, 4-node quadrilateral shell elements, with a full integration scheme, were utilised. The computational burden of the analyses was kept limited, without coarsening the accuracy of the results, by adopting a global mesh size of approximately 10 mm.