# Biomechanical Analysis of Two Types of Oseointegrated Transfemoral Prosthesis
## Materials and Methods
### 3D CAD Modelling and FEM Model  
Two different prostheses, a press-fit (OPL) and a screw type (OPRA), have been analysed. The CAD models of the prostheses (Figure 5) were created using a 3D parametric modelling software (SolidWorks, Dassault Systemes, Velizy-Villacoublay, France). Both models of the prostheses are composed of two main parts: an intramedullary stem (fixture) and a transcutaneous part (abutment).  
The CAD model of the bone was created using DICOM images from a CT-scan of a human femur. Subsequently, the main steps of the surgical implantation of the prosthesis have been virtually reproduced by means of SolidWorks. Final CAD models of the implant/bone assemblies of both prostheses are shown in Figure 6.  
Figure 4: Schemes and reference systems used to calculate loads at the bone/implant interface.  
Figure 5: CAD models of the prosthetic implants analysed: OPL (on the **left**) and OPRA (on the **right**).  
Considering that, nowadays, numerical methods ensure very accurate and reliable results and are commonly used to evaluate the behaviour of orthopaedic implants [41; 42; 43; 44; 45], numerical simulations have been performed on both models to investigate how stress distributions vary during a fall. In particular, a FEM-based approach has been used and virtual simulations [24; 46] have been performed using the commercial software Ansys Workbench (Ansys Inc., Canonsburg, PA, USA). To obtain highly reliable numerical models, the FEM models have been set up following a largely validated protocol [30; 47; 48]. Ten-node tetrahedral elements (SOLID187) were used to mesh the femur and the implant, and eight-node surface-to-surface (CONTA174 and TARGE170) contact elements [30] were used to mesh the bone/prosthesis interfaces (Figure 7).  
A preliminary convergence analysis (convergence threshold value: 5%) [28; 30] was performed to set the most suitable element dimension. The mesh has been refined at the interface between the intramedullary stem and the bone to improve the accuracy of the solution. The final meshes consisted of about 1,597,175 elements and 2,289,288 nodes for screw type implant, and 1,172,140 elements and 1,680,070 nodes for press-fitothesis. 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 [49], while the prostheses (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, \(\mathrm{E_{1}}\), \(\mathrm{E_{2}}\), \(\mathrm{E_{3}}\), \(\mathrm{G_{12}}\), \(\mathrm{G_{13}}\), \(\mathrm{G_{23}}\), \(\mathrm{n_{12}}\), \(\mathrm{n_{13}}\) and \(\mathrm{n_{23}}\), respectively, represent the Young's moduli (\(\mathrm{E_{i}}\)), the shear moduli (\(\mathrm{G_{ij}}\)) and the Poisson ratios (\(\mathrm{n_{ij}}\)) along the radial (1), transverse (2) and longitudinal (3) directions of the cortical bone [48; 50]. In Table 2, \(\mathrm{E}\), \(\mathrm{n}\) and \(\mathrm{\sigma_{y}}\) represent, respectively, the [PERSON]'s modulus, the Poisson's ratio and the yield tensile stress of the titanium alloy.  
Figure 6: CAD models of the implant/bone assemblies: OPL (on the **left**) and OPRA (on the **right**).  
Figure 7: Meshed model (screw type prosthesis).  
According to previous studies [52; 53], a bonded contact was imposed at the intramedullary stem/bone interface to simulate a total osseointegration. As for the contact algorithm, the augmented Lagrangian method was used [54]. As regards the boundary conditions, a fixed support constraint was applied to the proximal femur; the forces and the moments, calculated as described in previous Section 2.1, were applied on the end of the abutment.