## 2 Materials and Methods
### Finite Element Modeling  
The loads and boundary conditions applied to all experimental pin configurations were replicated in the finite element modeling. The CAD geometry of the nylon bars were axially aligned and the CAD geometry of Schanz pins without the threads, but with the thread length included, were subtracted from the nylon bars using the Boolean operations of SolidWorks(r) (Dassault Systemes SolidWorks Corporation, Waltham, MA, USA). All the LRS external fixator components were created from the measurements of each physical component and using the CAD tools available in the SolidWorks(r). These CAD objects, as well as the Schanz pins, the nylon bars, and the two spheres, were posteriorly assembled considering the mean axis of the rail component as reference. The three-dimensional geometries of the two composite plates were created and connected to the nylon bars using two cylindrical bodies with 5 mm of diameter, simulating the physical bolts that were used in the experimental setup to connect the cell load to the nylon bars.  
Afterwards, the finite element (FE) model of all the components was created and the three displacements (DOF) of the nodal points placed on the bottom surface of one spherical body were fixed, while the load was applied vertically to the nylon bar through another spherical body. Experimental constraints were simulated assuming contact conditions without friction between the nylon bars and the spherical bodies, and a friction coefficient of 0.75 was used to model the interface between the untightened clamp and the rail of the LRS external fixator. The bolts of the experimental setup, which were used to secure the clamps onto the LRS rail and the Schanz pins within the clamps, were simulated with material continuity. Linear elastic isotropic and transversely isotropic material properties were applied, Table 2.  
The geometry of the numerical model was created in accordance with the geometry of the experimental setup and, afterwards, all the components, except the composite plates, were meshed with 8-noded unstructured regular hexahedral elements, with the incompatible modes effect included as additional degrees of freedom, and using an average element length ranging from 1 mm to 3 mm [21; 22]. The accuracy of this numerical model was verified previously by a mesh convergence study and by a comparison with the numerical solution obtained with 10-noded tetrahedral finite elements [23]. The composite plates were meshed with 20-noded regular hexahedral elements using an average element length of 1 mm and connected to the nylon bars, assuming material continuity with the cylindrical bodies. Nevertheless, the interfaces between the plates and the nylon bars were modeled without friction coefficient. Moreover, in the post-processing phase, these contact surfaces were selected to evaluate the average value of the force that passes through the callus. The two composite plates were  
\begin{table}
\begin{tabular}{c c c c c} \hline \hline
**Material Property** & **Carbon Epoxy** & **Nylon** & **Anodized Aluminum 7076-T6** & **AISI 316 L** \\ \hline E1 [GPA] & 101.40 & 8.30 & 71.70 & 200 \\ E2 [GPA] & 8.40 & 8.30 & 71.70 & 200 \\ E3 [GPA] & 8.40 & 8.30 & 71.70 & 200 \\ G12 [GPA] & 5.60 & 3.24 & 26.95 & 79.05 \\ G13 [GPA] & 5.60 & 3.24 & 26.95 & 79.05 \\ G23 [GPA] & 5.60 & 3.24 & 26.95 & 79.05 \\ \(\mathbf{v_{21}}\) & 0.33 & 0.28 & 0.33 & 0.265 \\ \(\mathbf{v_{31}}\) & 0.33 & 0.28 & 0.33 & 0.265 \\ \(\mathbf{v_{32}}\) & 0.46 & 0.28 & 0.33 & 0.265 \\ \hline \hline \end{tabular}
\end{table}
Table 2: Material properties of all materials used in the finite element (FE) model.  
connected using rigid links type constraints, which are available in the ADINA(r)[24] program. The complete finite element mesh was built with 263,651 nodes (degrees of freedom 263,651 \(\times\) 3 = 790,953) and 267,780 elements, using the rule-based (mapped) meshing algorithm with preferred hexahedral (brick) cell shapes, which is available in ADINA software, and simulations were also obtained using the ADINA standard solver.