# Computerized Generation and Finite Element Stress Analysis of Endodontic Rotary Files
## 3 Results
### Mesh Convergence Study  
A mesh convergence study has been conducted to establish the optimum size and type for the elements of the mesh. In this study, several finite element models are obtained for the endodontic file, in which the density of the mesh is progressively increased by varying the magnitudes of \(n_{\mathrm{\
u}}\) and \(n_{\mathrm{\theta}}\). Four different average element sizes have been considered in the analysis, which vary from 0.05 mm to 0.20 mm, and both linear and quadratic tetrahedral elements have been taken into account. Figure 6 shows one of the meshes used in this study, in which the endodontic file is meshed using quadratic tetrahedrons with an average element size of 0.10 mm (\(n_{\mathrm{\theta}}=24\) and \(n_{\mathrm{\
u}}=250\)). The resulting FE models were analyzed using ABAQUS [31] (Dassault Systemes Simulia Corp, Providence, RI, USA). As suggested by [PERSON] [32; 33], the convergence of the mesh can be assessed by means of an error energy norm \(E\). In this error estimator, the stress vector \(\mathbf{\hat{\sigma}}\) and the averaged stress vector \(\mathbf{\sigma^{*}}\) are used to determine a stress error vector \(\mathbf{\Delta\sigma}\):  
\[\mathbf{\Delta\sigma}=\mathbf{\sigma^{*}}-\mathbf{\hat{\sigma}} \tag{12}\] \begin{table}
\begin{tabular}{l c} \hline
**Name** & **Magnitude** \\ \hline Cross section & Squared \\ Diameter of the shaft, \(d_{sh}\) & 1.20 mm \\ Diameter of the tip, \(d_{ap}\) & 0.25 mm \\ Length of the active part, \(L_{ap}\) & 16.00 mm \\ Total length of the file, \(L_{total}\) & 25.00 mm \\ Taper, \(c\) & 6\% \\ Pitch of the active part, \(p_{z}\) & 2.00 mm \\ Parabola coefficient transition area, \(a_{sh}\) & 0.10 mm\({}^{-1}\) \\ \hline \end{tabular}
\end{table} 
Table 1: Definition of cases of study. Figure 6: Finite element mesh for the endodontic file; the average element size is 0.10 mm (\(n_{\mathrm{\theta}}=24\) and \(n_{\mathrm{\
u}}=250\)). Then, for a given element \(i\) of the mesh and following the ideas presented by [PERSON] [34], an element energy error \(e_{i}\) is determined as:  
\[e_{i}=\frac{1}{2}\cdot\int_{V_{i}}\mathbf{\Delta\sigma}^{T}\cdot\mathbf{D}^{-1}\cdot\mathbf{ \Delta\sigma}\cdot dV_{i} \tag{13}\]  
where \(\mathbf{D}^{-1}\) is the material elasticity matrix and \(V_{i}\) denotes the volume of element \(i\). The energy error \(e\) is estimated for the whole finite element model as the sum of the error contributions of all the elements in the mesh:  
\[e=\sum_{i=1}^{N_{e}}e_{i} \tag{14}\]  
where \(N_{e}\) denotes the number of elements in the mesh. Finally, and considering the total strain energy of the finite element model \(U\), the error energy norm \(E\) is calculated as:  
\[E=\sqrt{\frac{e}{U+e}} \tag{15}\]  
Figure 7a shows the evolution of the error energy norm \(E\) as a function of the average element size, determined for each load case (torsion and bending) and element type (linear and quadratic). In all the cases, it can be observed that reducing the average element size also decreases the error in energy norm. For any load case and average element size, the error energy norm is significantly smaller when the problem is solved using quadratic elements than when it is solved using linear elements. Figure 7b shows the maximum element energy error \((\max(e_{i}))\) determined for each load case (torsion and bending) and element type (linear and quadratic), as a function of the average element size. The trends observed in this figure are similar to the ones observed in Figure 7a. In general, the maximum element energy error is reduced as the average element size is decreased, and quadratic elements demonstrate a better performance than linear elements. In all the cases the element with the maximum element energy error is found in the vicinity of the encastre, indicating that this is the region of the finite element model where mesh refinement is more needed.