## 3 Numerical Modeling Methodology of Composite Advanced Joint  
Several numerical techniques have been proposed in the literature for reproducing the orthotropic nature of composite materials [19; 20; 21; 22]. Recently, many numerical applications have been based on a ply-by-ply modeling technique of composite structures with the adoption of solid Hexa FE elements. [PERSON] et al. [23] modeled a composite-fastener joint with one through-thickness solid element for each composite ply. The proposed model was based on the application of the calibrated LS-DYNA material model MAT162 extracted from the preceding phase of the NASA ACC HEDI project [8; 9]. Moreover, [PERSON] et al. [24] proposed the same FE modeling technique to predict the strength of a composite-bonded joint under longitudinal tensile loads. However, the applicability of a ply-by-ply solid model is restricted to small samples and requires high computational resources. Finally, [PERSON] et al. [25] presented an FE model to predict the static progressive failure behavior of fiber metal-laminated bolted joints. A user-defined continuum-damage constitutive model was formulated and applied to a ply-by-ply solid numerical model. A complete stacked shell modeling technique (L2 DE-Cohesive), proposed and described by [PERSON] et al. [11], was considered for the present evaluation and it was validated against experimental evidence of a complex sandwich structure subjected to critical tensile loads. A shell-cohesive modeling approach can be considered to be a new and substantial step in simulating composites by means of LS-DYNA application, different with respect to the usual solid-cohesive procedure. Computational cost reduction and the possibility to simulate composites in a macro-scale environment can be viewed as an interesting consequence of this modeling technique. A brief description of such a modeling technique is summarized in the following paragraphs, as derived by [14] and presented in Figure 6.  
A single plane of 2D shell elements was introduced for each composite ply belonging to the laminate. The two-dimensional elements plane belonging to a single ply was placed at the geometric mid-surface of each physical composite layer. *PART_COMPOSITE was chosen to define each shell-ply that constituted the composite laminates. Structural continuity through the thickness was established with the application of interlaminar interface elements (CZM) properly connected node-to-node to the adjacent ply mesh structure. The introduction of defined cohesive elements restored the structural integrity and allowed the definition of transverse stiffness and toughness associated with the specific composite  
Figure 5: Experimental failure modes: (**A**) for the advanced joint, (**B**) for the not reinforced joint. A similar failure mode has been determined for the solid configuration. material [11]. ELFORM 20 cohesive formulation was applied for compatibility with a selected two-dimensional adjacent mesh. Solid metallic components, crushable core foam, and composite gripping sections were represented with solid Hexa FE elements. A fully-integrated shell element formulation (ELFORM 16) was selected to avoid energy dissipation from hourglass modes. Three integration points (IP) were defined through the thickness of each composite layer to correctly reproduce possible bending deformation modes in every single ply. An efficient fully-integrated solid element formulation (ELFORM-1) was selected for all solid-modeled components. A structured circular mesh was refined as the periphery of the bolt was approached to improve the aspect-ratio index of finite elements and improve energy conservation during the high-deformation fracture process observed in the experimental tests. A characteristic mesh length parameter was set between 0.35-1.4 mm (Figure 1) according to a previous FE evaluation, see [3; 4]. A finer mesh was applied around the circular hole region, pointing out stress variations around the hole (Figure 4).