# Experimental & FEM Analysis of Orthodontic Mini-Inplant Design on Primary Stability
## 2 Materials and Methods
### FEM Analysis  
After obtaining all of the important geometric characteristics, according to the previously described procedure, 3D models of the mini-implants and the surrounding cortical and cancellous bone segments are created, with the CAD/CAM/CAE system CATIA. Cortical and cancellous bone segments are modelled as cylinders with a diameter of 7 mm, with a cortex thickness of 0.675 mm, which represents the average cortex thickness estimated by measuring. Then, the same models are imported into Abaqus software (V, Dassault Systemes, Velizy-Villacoublay Cedex, France, 2012), where their mechanical properties along with advanced surface contact features are implemented.  
Material properties are expressed with [PERSON]'s modules of elasticity, [PERSON]'s coefficients and densities. Real material behaviour under load conditions were considered, where the titanium alloy Ti6 Al4V is presumed to be homogeneous and isotropic, and cortical and cancellous bone are considered orthotropic [26; 27; 28; 29]. Table 2 shows material properties of mini-implants and bone segments used for FEM analysis.  
Figure 6a shows the 3D-designed implant-bone system with Tomas(r)-pin, and Figure 6b shows the 3D-designed implant-bone system with Perfect Anchor mini-implant.  
Figure 5: Mean values of pull-out forces of the 20 samples of both Tomas®-pin and Perfect Anchor mini-implants.  
FEM modelling is integrated in biomechanical research for the ability to reproduce behaviour of bones, joints or implants, and it is used as an alternative to in vitro experiments, which can be expensive and difficult to carry out [30; 31]. The National Agency for Finite Element Method has defined the finite element stress analysis as a \"theoretical method that can be used for calculating the behaviour of a real structure by performing algebraic  
\begin{table}
\begin{tabular}{c c c c} \hline \hline
**Material/Properties** & **Ti6 Al4V** & **Cortical Bone** & **Cancellous Bone** \\ \hline Density [g/cm\({}^{3}\)] & 4.510 & 1.94 & 0.55 \\ \hline E\({}_{\text{xx}}\) [GPa] & 105 & 11.30 & 0.3468 \\ \hline E\({}_{\text{yy}}\) [GPa] & 105 & 13.80 & 0.4572 \\ \hline E\({}_{\text{zz}}\) [GPa] & 105 & 19.40 & 1.1071 \\ \hline \(\
u_{\text{xy}}\) & 0.37 & 0.274 & 0.05 \\ \hline \(\
u_{\text{yz}}\) & 0.37 & 0.237 & 0.01 \\ \hline \(\
u_{\text{xx}}\) & 0.37 & 0.237 & 0.322 \\ \hline \hline \end{tabular}
\end{table}
Table 2: Properties of materials.  
Figure 6: 3D-designed implant-bone system (**a**): Tomas®-pin and (**b**): Perfect Anchor.  
solutions of a set of equations describing idealized model structure with finite number of variables\" [32].  
Discretization of mini-implants and bone segments is performed with C3D4 elements, i.e., linear tetrahedrons with 4 nodes. The complete system used uniform mesh with a maximum size of finite elements of 0.2 mm. Thus, the structures of Tomas(r)-pin and Perfect Anchor mini-implants were discretized with 485,429 and 481,524 finite elements containing 86,477 and 83,154 nodes, respectively.  
The movement of the bone's outer surfaces is disabled, while the movement of the threaded surface of the mini-implant and contact surfaces of cortical and cancellous tissue was enabled only in the direction of implant length. The interaction between contact surfaces of the implant and bone is realized with surface-to-surface contact with finite sliding. The section of the mini-implant above bone surface is excluded, so that model is \"less demanding\" and precise location of pull-out force impact is simulated. The upper surface of the implant is coupled with a node, and concentrated force is applied on this node [33].  
The comparative analysis between the two different mini-implant designs shows the magnitude of stresses within the implants and surrounding bone segments. The equivalent stress is considered because it represents a mean stress in its three components x, y and z directions [34].