Issue 47

F. Cucinotta et alii, Frattura ed Integrità Strutturale, 47 (2019) 367-382; DOI: 10.3221/IGF-ESIS.47.27 375 Figure 9 : Boundary conditions for impact test. Numerical models A finite element model was developed by exploiting ANSYS Workbench 17.1, to simulate the behaviour of the described composite materials under different loading conditions. In particular, quasi-static bending loading and impact loading were considered. The same modelling choices were made for the material representation under both loading conditions, in order to obtain a general model for these materials. The considered specimens are composed of a thick core of homogenous material and thin skins of composite laminates. The physics of the problem requires a high complexity finite element model to reproduce the anisotropic and not homogeneous material properties, the contact regions, the geometrical non-linearities and the complex constraint conditions. In order to reduce the computational effort, only the thick core was modelled with brick elements (Solid186), while the skins were modelled with shell elements (Shell181). The connection between skins and core was ensured exploiting several bonded contact pairs. This strategy allowed to drastically reduce the number of elements in the volume of the skins, characterized by a ratio between the thickness and the other dimensions of about 100. The material properties of the core were easily set as isotropic. On the other hand, each skin was modelled as a single surface, even if composed by layers of different materials. The actual properties were then implemented exploiting the “Layered Section” feature of the software, which allows to set the stacking sequence of layers in terms of layer order and thickness. Thus, only the non-isotropic properties of the single layers were set in the material library, while the resulting laminate properties were computed by the software. The loading during the experimental tests were chosen in order to investigate also the region of the load-displacement curve characterized by increasing damage in the specimen. The numerical simulation of the damaged material behaviour is highly challenging, thus the adopted model was aimed at obtaining a rough estimation of the consequences of both core and skins failure. The maximum stress damage initiation criterion was used, and the ultimate stress values (along with all the other material properties) were obtained by the material specifications provided by the manufacturer. Once the damage was initiated, a proportional stiffness reduction was applied to the damaged elements. This reduction coefficient was tuned basing on the comparison between experimental and numerical results of the bending test, exploring the range 0.7 – 0.95. In the following, a fraction equal to 0.9 of the undamaged stiffness was set for all the considered materials, which allowed to obtain the best experimental/numerical matching. For generality purposes, the value obtained for the bending test was also used for the impact test. It is worth noting that less reliable numerical results are expected in the regions of the curves were the damage is extended to a great portion of the specimens’ volume. Finally, for both bending and impact test simulation, a convergence analysis for mesh dimension was performed: the damage initiation criterion was deactivated, and the maximum Von Mises stress in the specimens was used as convergence parameter. This composite modelling was kept constant for both bending and impact test simulations, since it provided a reliable description of the material behaviour even in such different loading conditions. The simpler quasi-static bending test was simulated first. A static structural analysis was setup by modelling the entire 800x100 specimen, as schematized in Fig. 6. In order to enhance model accuracy, the machine punches were represented in the model as rigid surfaces. Thus, the specimen skin surfaces were geometrically divided in different areas, to provide contact regions for mesh refinement. The punches were used to represent test constraint (i.e. zero vertical displacement at the lower skin) and the loading (i.e. gradually