# Prediction of Deflection Due to Multistage Loading of a Corrugated Package
## 4 Finite Element Analysis for Multistacked Corrugated Packages  
### Validation of the FEA Material Properties  
To determine the material constants of the core defined in Figure 2, optimization was performed to minimize the errors in the FEA and test using HyperStudy and Abaqus [16; 20]. As an FE model, the BCT FE model of the corrugated package and the four-point bending FE models of the MD and CD of the corrugated fiberboard were composed using the Abaqus implicit dynamic quasi-static model. Similar to the test specifications [17] shown in Figure 5a, the four-point bending FE model is shown in Figure 10. The size of the model was 50 mm \(\times\) 500 mm, with a thickness of 5 mm, which was the same as those of the specimen used in the test. The element size of the corrugated fiberboard specimen was 5 mm, and it was composed of a continuum shell element to predict the changes over time. The number of nodes and elements in the four-point bending FE model was 2222 and 1000, respectively. In addition, the models of loading and supporting anvils were modeled to be similar to the actual size and shape of the jig (cylinder radius: 3.18 mm; length: 84 mm) during the test and consisted of rigid elements with a size of 2 mm. In the FEA, contact was defined between the corrugated fiberboard specimen and jigs, and the coefficient of friction was determined to be 0.4. For the boundary conditions, the lower supporting anvil was fixed and the upper loading anvil was forcibly displaced in the z-direction. The forced displacement was 15 mm for the CD and 5 mm for the MD, and these values were defined as the average values that could be estimated as linear intervals, regardless of the bending direction of the curves of each specimen's direction, as shown in Figure 5.  
The BCT FE model is shown in Figure 11. The modeling of the corrugated package was represented in 3D and based on the drawings of the package (external dimension: 730 \(\times\) 293 \(\times\) 336 mm), and was applied to the box compression and creep tests. After fabricating the middle surface based on this 3D model, the FE model was constructed in the manner shown in Figure 3. The number of nodes and elements in the BCT FE model was 111,650 and 55,832, respectively. If the degrees of freedom of rotation of the connector element of the box fold are free, convergence becomes difficult during FEA; if the box is not taped, the folded state does not remain because of the reaction force of the fold. Therefore, in this study, nonlinear rotating spring characteristics were applied to the fold to set the initial load due to the spring action in the box assembly (the box flaps were folded at an angle of 90\({}^{\circ}\)). In addition, an adhesive tape with a width of 30 mm and a thickness of 0.8 mm was modeled as a membrane element to maintain the folding state of the box, which was composed of rigid elements in the form of a surface at the top and bottom to apply a compressive load on the box. Contact was defined between the box flap and the flap and between the box flaps and the rigid surface, and a friction coefficient of 0.4 was applied [21]. A tie constraint condition was applied between the box and the adhesive tape. As for the condition of the boundary, the lower rigid surface was fixed and the upper rigid surface had a forced displacement of 0.75 mm applied in the z-direction; all other directions were fixed. HyperStudy was utilized to optimize the material constants [21]. The response set here was the difference in the area of the force-displacement graph of the test and analysis, and the \"area_between_two_curves\" function was used to calculate this; the \"global response search method\" was used to minimize this response. The initial value of the material  
Figure 10: Four-point bending FE model of 50 mm \(\times\) 500 mm. constants was obtained from the literature [15]. Table 1 lists the material constants of the applied liner.