PSI - Issue 61

Onur Ali Batmaz et al. / Procedia Structural Integrity 61 (2024) 305–314 Onur Ali Batmaz et al./ Structural Integrity Procedia 00 (2019) 000 – 000

306

2

1. Introduction Low-velocity impact (LVI), which is typically characterized by impactor speeds below 10 m/s (Cantwell and Morton, 1991), presents unique challenges for composite structures. Unlike metals, which often exhibit visible plastic deformation near the impacted area in the form of dents, composites can develop internal damage that is either barely visible or completely undetectable from the outer surfaces (Adams and Cawley, 1988). To design load-bearing components capable of withstanding low-velocity impacts, it is essential to have an understanding of the underlying damage mechanisms and the ability to accurately simulate the impact events. In every numerical simulation, properly modeling the boundary conditions (BCs) to align with the actual experimental conditions is essential. This becomes especially critical in the low-velocity impact simulations because there is sufficient time for stress waves generated from the impact zone to propagate and reflect back from the supports (Naik and Shrirao, 2004). However, only a few studies deal with the effect of boundary conditions of composite plate specimens subjected to impact loading. Tiberkak et al. (2008) conducted a numerical investigation on the effects of BCs on clamped and simply supported plates, and their study showed that variations in BCs did not result in any significant changes in the global force response or central deflections. Similarly, Minak and Ghelli (2008) also obtained very similar global force-displacement responses at the beginning of the impact loading stages of clamped and simply supported specimen experiments. They attributed this similarity to the fact that elastic waves could not reach the boundaries, explaining the lack of significant differences. However, they observed that the clamped configuration exhibited a stiffer response led to smaller maximum impactor displacement later in the loading process. Yet, despite this difference in stiffnesses, the maximum contact force levels remained similar for both BCs. Taking an alternative viewpoint, Sun and Hallett (2017) explored the effect of different BCs by conducting off-center impact tests on the composite plates. Their findings revealed that the stiffness varied with different BCs, but the force levels at the initial load drop remained consistent, much like the results observed by Minak and Ghelli (2008). In this study, we construct a finite element (FE) model of the LVI experiments conducted on [0 5 /90 3 ] s CFRP beams by Bozkurt and Coker (2021). The numerical model is constructed in the commercially available FE software ABAQUS/Explicit. It includes a user-implemented ply damage model with LaRC05 criterion for matrix cracking, and the built-in cohesive zone method for delamination. The influence of experiment boundary supports on the global impact response is observed to be significant, therefore, we proposed a heuristic approach for modeling BCs that involves replicating the experiment's boundaries by incorporating spring elements, which are tuned using deformation and strain data obtained from digital image correlation analyses. The validity and influence of the proposed BCs modelling approach are assessed through detailed comparisons between numerical and experimental results. For further investigations on dynamic damage characteristics utilizing the BCs modeling approach proposed in this paper, readers are referred to the study by Batmaz et al. (2024). A schematic representation of the finite element (FE) model is presented in Figure 1. In this model, the semi cylindrical steel impactor is idealized as an analytical rigid body with a mass of 1.865 kg. It is positioned just above the beam, ensuring that the initial contact occurs at the midpoint of the composite beam. To replicate the free fall from a 0.5 m height, an initial downward velocity of 3.13 m/s is assigned to the impactor. The composite beam specimen is modeled as a three-dimensional deformable body, and we activate the nonlinear geometry option to account for large deflections that result in changes in stiffness. A representative meshed section of the composite laminate model is presented in Figure 1. 8-noded linear brick elements with reduced integration, enhanced hourglass control, and second-order accuracy (denoted as C3D8R in the ABAQUS library) are utilized for the ply material. For modeling delamination, we utilize 8-noded three-dimensional cohesive elements (denoted as COH3D8 in the ABAQUS library) at 0°/90° interfaces. As demonstrated by Batmaz et al. (2024) in a mesh size study for this material and layup combination, an in-plane mesh size of 0.20×0.20 mm² with an element thickness of 0.3 mm satisfies the stability criteria necessary for ensuring energy dissipation during the damage process. Batmaz (2023) further examined the influence of mesh refinement on global impact response and 2. Numerical simulations 2.1. Finite element model