PSI - Issue 59

Ilham Bagus Wiranto et al. / Procedia Structural Integrity 59 (2024) 230–237 Wiranto et al. / Structural Integrity Procedia 00 (2019) 000 – 000

232

3

2.1. Geometry, FE mesh, and boundary condition The FEA was conducted using the dynamic explicit solver within ABAQUS 6.23. The models included a square flat panel measuring 400 x 400 x 3 mm and a crossbar stiffener measuring 400 x 50 x 3 mm, both constructed from carbon fiber composite material. These structures were composed of woven carbon fiber stacked plies, with each ply having a thickness of t = 0.25 mm. Initially, the model was established in ABAQUS, with the upper skin and stiffener treated as a single deformable shell element. In contrast, the impactor was represented as a discrete rigid body, ensuring that it does not deform during impact. Additionally, the simulation environment considered the indenter, specimen, and the rigid support facility (boundary condition). To optimize simulation accuracy and computational efficiency, a simplified model was developed. Before commencing the analysis, a study on mesh convergence was conducted, involving adjustments to the mesh size. The selection of the optimal mesh size was based on considerations of result convergence and total computation time. The impactor was positioned to strike the central area of the panel. Additionally, for simplification purposes, a boundary condition was applied to the impactor, restricting its displacement exclusively along the axis normal to the plane. In the simulation, the impactor's parameters were varied, encompassing three different impact velocities and corresponding masses (4.43, 6.26, and 7.67 m/s, coupled with masses of 50, 100, and 150 kg). 2.2. Material Properties The mechanical performance of composites hinges on the individual mechanical traits of each constituent. Furthermore, the interfacial bond between the matrix and fibers plays a crucial role in influencing the mechanical attributes of composite materials. Specifically, the composite skin panel is fashioned from carbon fiber reinforced polymer and comprises both an upper skin and a stringer, with respective thicknesses of 3 mm and 2 mm. The detailed mechanical properties of the carbon fiber component from a previous study (Ge et al. (2022)) can be found in Table 1. Material modeling is carried out within ABAQUS. Initially, the material properties for a single layer of woven carbon fiber are input into a composite layup section, and these layers are stacked to achieve the desired thickness. Subsequently, ABAQUS automatically generates a homogeneous material representation for the analysis. As a result, all layers are treated as isotropic materials, enhancing the robustness of this analysis.

Table 1. Mechanical properties of the woven carbon fiber reinforced plates based on Ge et al. (2022). Properties Values E 1 = E 2 (GPa) 62.3 E 3 (GPa) 8.5 ν 0.06 G 12 (GPa) 7.1 G 23 = G 13 (GPa) 3 Density (kg/m 3 ) 1467 Material Strength X t = Y t (MPa) 610 X c = Y c (MPa) 314.7 Z t (MPa) 55.6 Z c (MPa) 500

2.3. Hashin damage failure criteria In the fields of composite materials and structural mechanics, the Hashin Damage Criterion is a commonly used mathematical model to forecast failure or damage initiation in composite materials under varied loading situations (Hashin and Rotem (1973) and Hashin (1980)). It is especially helpful for failure prediction in fiber-reinforced composite materials since the behavior of individual layers or plies in these materials can be complicated. The growth