## 4 Results and Discussion
### Preliminary Analyses
On the other hand, Continuum shell elements' models were more sensitive to the in-plane element size as the number of elements in the thickness direction increased. In particular, the numerical results of the Continuum shell model with 12 and 24 elements in the thickness direction associated to coarser mesh (size 2 mm or 4 mm) differed noticeably from the analytical results. This is mainly due to hourglass problems, which can be relevant for the reduced integration scheme elements. Unfortunately, the reduced integration scheme is mandatory in Abaqus/Explicit when Continuum shell elements were adopted. To alleviate hourglass deformation problems that could arise in the numerical models, the default hourglass controls available in Abaqus/Explicit [36] was adopted. In general, the results highlight that the best results were obtained by the Solid element model discretized with one element per py and an in-plane element size equal to 1 mm; however, a good numerical-analytical correlation was obtained also by the Continuum shell mode, discretized by 12 elements in the thickness direction and an in-plane element size equal to 1 mm. Indeed, this last configuration was chosen for the analysis presented hereafter due to its excellent compromise between low computational cost and agreement with the analytical solution. Despite their simplifications, the analytical models available in the literature well describe the behavior of a CFRP plate subjected to impact loading conditions. Hence, the numerical model was validated by comparisons with the analytical one, and the used modeling approach, neglecting in this preliminary phase the damages, has been assessed. Once the accuracy of the impact numerical model is verified, some considerations should be made about the relevant difference between the boundary conditions implemented in the analytical model and the ones implemented in the experimental test. Actually, simply supported conditions have been considered in the analytical and preliminary numerical models; however, the boundary conditions of the experimental test, suggested by the ASTM standards and reported in Figure 14, are substantially different. These boundary conditions are a consequence of a support fixture whose degrees of freedom are restrained and four rigid clamps, also modeled as rigid bodies, which hold the specimen still during impact and avoid any rebound. Figure 14: Boundary conditions. (**a**) Analytical; (**b**) experimental. Figure 3:0 Solid elements with 24 elements in the thickness direction: analytical–numerical comparison. A further numerical model obtained with the implementation of the Experimental boundary condition (BC-E) was introduced to understand the effects of boundary conditions on the numerical results. In Figure 15, the analytical, experimental and numerical results of the shell model obtained by considering both analytical (BC-A) and experimental (BC-E) boundary conditions were compared. In Figure 15, a comparison between experimental, analytical, and numerical results, in terms of force as a function of the time, is reported. The comparison shows that in the first part of the curve both numerical and analytical models were in agreement with the experimental results. However, after a first phase, the analytical model and the FEM BC-A numerical model greatly differed from the experimental result. On the other hand, the FEM BC-E numerical model was characterized by the same mechanical response in terms of stiffness of the laminate, up to the maximum force peak. Indeed, neglecting the damages in the numerical model resulted in grater force peak, if compared with the experiment. Once the accuracy of the numerical model, in terms of elastic response, was established, the numerical models which provided the best results compared to the analytical solution was considered for the final impact test: final Continuum shell model and Final 3D solid model. Since Abaqus does not provide any intra-laminar damage models for Solid elements, a VUMAT was introduced.