## 3 Finite Element Model  
The well-known non-linear finite element code ABAQUS was chosen in this study to predict the behavior of carbon fiber reinforced composite. The composite layup property editor provides a table that enables users to define each ply in the laminate separately including ply name, material, thickness, and orientation (for plies with [0/90\({}^{\circ}\)] orientation). The stratification of composite material is defined by using the composite layup feature of ABAQUS. The composite layup tool only allows surface discretized with shell elements to model stacking sequences instead of as many surfaces as the number of layers that constitutes the real stack. In the composite layup modulus, for each set of elements corresponding to specific zones of the specimen, it is possible to define: (1) the number of plies; (2) the material that constitutes the ply; (3) the orientation of the fibers; (4) individualply thicknesses.  
The profile geometry was modelled by using linear shell element S4R node doubly curved, reduced integration, hourglass control, and finite membrane strains. Both fixed and moving plates were modelled as linear discrete rigid element R3D4 bilinear quadrilateral. The element mesh size was 5 mm after conducting sensitivity analysis (maximize accuracy without increased computational time). The composite specimen was placed between two plates which had been modelled as rigid shell plates. The bottom plate was fixed in all directions and the motion in any direction was a constraint in all degree of freedom (U1=U2=U3=UR1=UR2=UR3=0) while the crushing speed assigned to the top plate (striker) with a mass of 78 kg had been uniformly applied. The top plate was modelled to move axially towards the specimen and restricted from moving in other directions. A trigger (chamfer) was applied at the top of the profile to ensure the stable progress collapse during the test (similar to experimental tests). Figure 6 depicts the FE model used.  
Figure 5: Zwick \(\pm\)250 kN Fatigue (**left**) and Instron Drop Tower (**right**).  
The contact interaction for the entire model was set as general contact and was used to avoid any interpenetration of the profile wall. The contact of the whole model was defined using a finite sliding penalty-based contact algorithm with contact pairs and \"hard\" contact. The friction coefficient value of all contact surfaces was set at 0.2 [38; 39]. An adhesive layer was used to attach the closure plate to the top-hat profile. Sixteen plies were used to simulate the profile [\(\pm\)45/0-90/90-0/\(\pm\)45] orientation as well as the closure plate with three integration points with overall thickness of 2.6 mm for the profile and the closure plate. Each shell represented one ply. Mechanical properties of the composite material used in the simulation procedure are listed in Table 1. To model the progressive failure of the composite structure, [PERSON]'s theory was utilized [40]. The Hashin criterion takes account of four independent modes of damage: fiber tension, fiber compression, matrix tension and matrix compression. When one of the damage initiation criterion is met, the elements are programmed to be deleted at the ply where the damage was detected (Hashin failure criteria). The element deletion is a very effective strategy in modelling progressive composite failure [40]. This failure criterion was adopted for its ease of implementation in the finite element software.