## 3 Finite Element Analysis  
The FEM analysis was conducted using Ansys Workbench 2020 R2 software [20]. Contacts were defined for the purpose of simulating mechanical contacts in all investigated models (see Figures 6 and 7). In principle, the contacts are the same in all the analyses, though there are differences between the healed and broken femurs, in the latter type there is also contact between the bone fragments (on the fracture surfaces). The contacts are shown in Table 3.  
For the healed femur, it was considered that bone tissue has grown around all parts of the screws and nails, which means that neither the nail as a whole nor any part of it moves within the femur, so the nail can be considered a part of the bone. For this reason, the contacts were defined as \"Bonded\". For the broken femur, the contact types were chosen in order to simulate a situation in which the patient begins to place weight on the affected limb. In normal circumstances, weight-bearing begins 6 weeks after the implant is fitted and the patient should place no more than one-third of their total body weight on the healing limb. (Information gained from consultation with doctors) In some cases, the bone may suffer renewed damage at the location of the fracture, as it has not yet completely healed. In such cases there is no  
Figure 8: Modifications of CAD models for FEM analysis. (**a**) Medin load screw; (**b**) Tantum load screw; (**c**,**d**) Fixation screws. Figure 9: Location of fractures in the anatomical CAD model of the femur (Spacecclaim). \begin{table}
\begin{tabular}{c c c c} \hline \hline  & **Element** & **Femur** & **Screw** \\ \hline \multirow{2}{*}{Healed femur} & Femur & (One body) & Bonded \\  & Nail & Bonded & Bonded \\ \hline \multirow{2}{*}{Broken femur} & Femur & Frictionless & Bonded \\  & Nail & Bonded & No separation \\ \hline \hline \end{tabular}
\end{table} 
Table 3: Contacts (Ansys Workbench Mechanical software). displacement of the bone fragments, though the fragments may move slightly against each other. For this reason, the contact was defined as \"Frictionless\"; this enables both tangential and normal displacement (separation). The contact is without a coefficient of friction, as the coefficient of friction between bones is not known. Moreover, in this case it is not necessary, as the entire movement of the bone is represented by the nail and its parts. Because this is a simulation of the state of the femur after 6 weeks of treatment, it is considered that the bone tissue has already grown around all the recesses on the nails and their parts; the contact is thus defined as \"Bonded\". For load screws and fixation screws, this contact would be provided by means of self-tapping screws during the initial implantation process. Other boundary conditions used in the FEM analyses are shown in Figure 10. The hip joint region is subjected to compressive force F (C) and this is also the location of a contact permitting displacement only in the direction of the force application (B). Force F replaces the transfer of the patient's weight--in this case a patient standing on one leg (extreme condition). For the purposes of the analysis, this force is considered to be static load with value of 1 N, and the necessary calculations are also carried out for other loading. In the knee joint region there is a boundary condition with a Winkler elastic foundation (D) with stiffness k = 0.13 N/mm\({}^{3}\) simulating the compressibility of joints (the reduction in the size of the spaces between the joints under loading) and a boundary condition only permitting displacement in the direction of the force application (A). Experiences of using elastic foundations were drawn from previous studies [1; 2]. The main element used in creating the finite element mesh was a ten-node quadratic tetrahedral element with three degrees of freedom in axes X, Y, Z in every node (solid 187, Ansys software [20]). This element is suitable for the meshing of irregular shapes, which is beneficial in this case.