PSI - Issue 5

Sebastian Heimbs et al. / Procedia Structural Integrity 5 (2017) 689–696 Sebastian Heimbs, et al. / Structural Integrity Procedia 00 (2017) 000 – 000

691

3

4. Model development The modeling tasks involve the generation of an appropriate finite element (FE) mesh of the relevant parts from available CAD data and the development of accurate material, joint and boundary condition modeling methods. The software used for these simulations was Abaqus/Explicit 2016. All massive parts of the structure were meshed with 4-node linear tetrahedron solid elements (C3D4). All thin parts were meshed with 4-node thin shell elements (S4R). The mesh size was selected to be 3-5 mm as a typical compromise between accuracy and computational expense. All bolted joints or rivets were represented as 2-node connector elements (CONN3D2). The whole finite element model, consists of 501,233 elements. The task of defining and validating the models of the materials and connectors involved was based on the building block approach, which is state of the art to achieve high simulation accuracy and to demonstrate it to the authorities. This method is based on a step-by-step model development and validation along the test pyramid, starting on the bottom of the pyramid on coupon level. The material models are generated based on test data and validated by simulating the coupon tests afterwards. On the next level, the element level, slightly more complex models involving fasteners and material sheets are generated and again validated against test data. The complexity of the models increases successively. With this approach, a final full-scale structural simulation can be performed without having an actual test for validation, because all modeling details have been sufficiently validated so far. The aluminum material modeling with nonlinear plasticity is based on coupon test data of the different alloys, which have been performed under quasi-static and high-rate dynamic loading conditions as shown in Fig. 2. No significant strain rate effects are observed for AA2024 in this range of loading rates (see also Seidt and Gilat (2013)). The respective material modeling approach is visualized in Fig. 3. The elastic behavior as the initial part of the stress-strain curve only depends on the Young’s modulus and Poisson’s ratio. When the yield stress is reached, the plasticity regime begins, which is based on tabular input of stress vs. effective plastic strain, directly derived from experimental data. After necking, which is represented in the stress-strain diagram by a negative slope, localization occurs. In order to model the rest of the curve accurately, the weighted average method according to Ling (1996) was used to approximate the curve in the polyaxial stress state. The stress-strain curve ends with material failure when reaching the failure strain. Afterwards, the element is deleted from the calculation. The material model, which is developed according to this scheme, is then validated by simulating a coupon test and comparing the results to the target test results. The experimental stress-strain data for the welding aluminum alloy AA6061 were taken from De Matteis et al. (2014). This reference does not only cover the stress-strain response of the base material, but also of the heat-affected zone, which is very helpful for the modeling. Structural aluminum is weakened in the heat-affected zones adjacent to welds, which needs to be taken into account in the model, see Moore and Wald (2003). The affected region extends immediately around the weld, beyond which the strength properties rapidly recover their full values. High-rate dynamic test data of AA6061 up to strain rates of 1000 s -1 have been published by Niechajowicz and Tobota (2009). The results show that no significant strain rate effect occurs. Hence, it was also neglected in the model. 4.1. Aluminum material modeling

Fig. 2. Material characterization of aluminum AA2024 for constitutive modeling (from Heimbs et al. (2015)).