## 2 Materials and Methods
### FEM Analyses  
Finite element method analysis is an important assisting tool used largely to evaluate the behaviour of orthopaedic implants [4; 8; 9; 26]. Such analyses can be used to estimate the displacement and load distribution of bones and implants [8; 26; 27]. Moreover, it has been shown that FE models can be used to predict fracture healing [26; 28; 29]. For these reasons, in this work, an FEM-based approach was used and virtual simulations [30; 31] performed using the commercial software Ansys Workbench R.18 (Ansys Inc., Canonsburg, PA, USA, 2018). All finite element analyses were performed using a Dell Precision T7810 workstation with a 24-core Intel Xeon E5-2670 processor and 128 GB of RAM.  
Figure 5: CAD model of the superior part of the plate and numbering of the screw holes.  
Figure 6: Schemes of the different configurations analysed (the screw angle is measured).  
Regarding the mechanical properties of the materials, the bone was considered as an orthotropic material, with the principal direction aligned along the long axis of the bone [32], while both screws and plate (T16A14V alloy) were considered as isotropic. The bone and the titanium alloy were considered as elastic linear hardening materials.  
Tables 1 and 2 report, respectively, the mechanical properties of the bone and of the titanium alloy T16A14V. In Table 1, E1, E2, E3, G12, G13, G23, n12, n13 and n23 respectively represent the Young's moduli (Ei), the shear moduli (Gij) and the Poisson ratios (nij) along the radial (1), transverse (2) and longitudinal (3) directions of the cortical bone [32]. In Table 2, E and n represent the Young's modulus and the Poisson's ratio of the titanium alloy.  
To avoid unrealistic high stress concentrations due to sharp discontinuities, mid-side node elements were used to model the curved boundaries. Moreover, to ensure a high accuracy of the results, aspect ratios were also checked during meshing to maintain all elements within acceptable distortion limits. Ten-node tetrahedral elements were used to mesh the implant-bone assembly, and eight-node surface-to-surface contact elements were used to mesh the bone/bone and bone/plate interfaces (Figure 7). A preliminary convergence analysis (convergence threshold value: 5%) [33] was performed to set the most suitable element dimension. The final mesh consisted of about 405,000 elements and 600,000 nodes.  
According to previous studies [17; 34; 35], a bonded contact was imposed at the screw/bone interface and a frictional surface-to-surface contact was used at the bone/plate and bone/bone interfaces. The friction coefficients of the bone/bone and bone/plate interfaces were 0.45 and 0.3 respectively [17; 34; 35]. As for the contact algorithm, the augmented Lagrangian method was used [36]. According to similar studies on the stability of fixation implants [34; 37], the following boundary conditions were imposed to the FEM models: the tibia was locked at its lower end, and a displacement along its main longitudinal axle was imposed on top of the fractured part of the tibia (Figure 8). In particular, a 0.5 mm displacement was  
\begin{table}
\begin{tabular}{c c c c c c c c c} \hline \hline
**E1 (GPa)** & **E2 (GPa)** & **E3 (GPa)** & **G12 (GPa)** & **G13 (GPa)** & **G23 (GPa)** & **n12** & **n13** & **n23** \\ \hline
6.91 & 8.51 & 18.4 & 2.41 & 3.56 & 4.91 & 0.49 & 0.12 & 0.14 \\ \hline \hline \end{tabular}
\end{table}
Table 1: Main mechanical properties of the cortical bone.  
\begin{table}
\begin{tabular}{c c c} \hline \hline
**Material** & **E (GPa)** & **n** \\ \hline T16A14V & 115 & 0.33 \\ \hline \hline \end{tabular}
\end{table}
Table 2: Main mechanical properties of the titanium alloy T16A14V.  
Figure 7: Particulars of the mesh of the proximal tibia.  
imposed. This value represents a threshold beyond which the implant may no longer be considered stable [37; 38].