# Modelling of High-Velocity Impact on Woven Carbon Fibre-Reinforced Plastic Laminate
## 4 Simulation Results  
Two finite element models of a quarter of the sphere impact tests are shown in Figures 6 and 7. Two perpendicular symmetry planes were defined through the impact direction in terms of appropriate boundary conditions (x displacement constrained in x = 0 plane and y displacement constrained in y = 0 plane). High-velocity impact is driven by the local effects, and to reduce computational costs, the in-plane target dimensions of the FE model were smaller than the dimensions of the real specimens, with the transparent (non-reflecting) boundary conditions applied around the model edges. These boundary conditions do not affect the local physical process that drives deformation and failure of the target. In all FEM models, the CFRP plate was modelled with three solid elements per thickness of the ply in order to capture delamination and bending of the plate properly. A quarter of the 6 mm target plate was modelled by 96,000 solid elements with one integration point, whilst a quarter of the sphere projectile was modelled with 4864 solid elements. The 12 mm thick plate, comprising 32 plies, was modelled with 192,000 solid elements. The plate was modelled as a quasi-orthotropic material, with the material properties given in Tables 2 and 3. The Mie-Gruneisen EOS data are given in Table 4.  
Figure 5: Post-impact images of 12 mm thick target plate in the vicinity of impact (C3): (**a**) impact face and (**b**) rear face. Figure 6: (**a**) FEM model of a quarter of the sphere impact on woven CFRP composite target—6 mm thick target plate and (**b**) stack sequence of 6 mm thick woven CFRP composite plate. Figure 7: FEM models of a quarter of the CFRP target plates, were the different colors represent different plies: (**a**) 6 mm thick composite A3 and (**b**) 12 mm thick composite C3 modelled. \begin{table}
\begin{tabular}{c c} \hline \hline Density & 1500 kgm\({}^{-3}\) \\ Elastic modulus in longitudinal direction E\({}_{\text{a}}\) & 68.465 GPa \\ Elastic modulus in longitudinal direction E\({}_{\text{b}}\) & 66.534 GPa \\ Elastic modulus in longitudinal direction E\({}_{\text{c}}\) & 10.0 GPa \\ Poisson’s ratio \(\upsilon_{\text{ba}}\) & 0.0039 \\ Poisson’s ratio \(\upsilon_{\text{ca}}\) & 0.0044 \\ Poisson’s ratio \(\upsilon_{\text{cb}}\) & 0.0045 \\ Shear modulus G\({}_{\text{ab}}\) & 4.57 GPa \\ Shear modulus G\({}_{\text{bc}}\) & 3.57 GPa \\ Shear modulus G\({}_{\text{ca}}\) & 3.57 GPa \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Material elastic properties of woven carbon fibre composite [40]. The simulation programme consisted of four simulations: (1) impact on 6 mm thick CFRP target plate at 194 m/s; (2) impact on 6 mm thick CFRP target plate at 354 m/s; (3) impact on 6 mm CFRP target plate at 1200 m/s and (4) impact on 12 mm CFRP target plate at 1219 m/s. These test cases were chosen to cover a range of velocities which correspond to different dominant damage/failure mechanisms. The sphere, 12 mm in diameter, was fully annealed stainless steel with isotropic properties. It was modelled by using the Johnson-Cook material model (material 15 in DYNA3D [6]) with material properties given in Table 5.  
The contact algorithm used in the simulation is SAND (Slide surfaces with Adaptive New Definitions), which is available in DYNA3D as contact type 11. Simulation of the first impact case at 194 m/s revealed a damage area in all plies normal to the impact, elliptical in shape, similar to the experimental observations. The damage area in the FEM models was calculated as the sum of the areas of the sides of the fully failed elements for each individual ply. The experimental result was obtained from the image processing of the tomography data in the interface plane. A comparison of the simulation results through the thickness and the experimental results is given in Figure 8.