# Computerized Generation and Finite Element Stress Analysis of Endodontic Rotary Files
## 2 Materials and Methods
### Development of an Fe Model for Stress Analysis of Endodontic Files  
This section describes a new procedure for the automated development of FE models for the stress analysis of endodontic files. This procedure covers the typical steps in the generation of an FE model for stress analysis, which include the discretization of the volume of the endodontic file into finite elements, the definition of the material properties for the finite elements of the model and the definition of the loading and boundary conditions of the model. In the first step, the volume of the endodontic file is discretized into tetrahedral elements by means of a constrained Delaunay tetrahedralization [24]. The constrained Delaunay tetrahedralization requires the boundary surfaces of the endodontic file to be represented by a set of triangles, which will constitute the external faces of the tetrahedrons once the mesh is generated. This boundary representation is achieved following these steps:  
1. The external surfaces that define the volume of the endodontic file are represented analytically considering the parametric equation \(\mathbf{q}_{r}(\theta,v)\) (Equation (11)), which provides the Cartesian coordinates of a point in the surface of the endodontic file from its parametric coordinates \(\theta\in[0^{\circ},360^{\circ}]\) and \(v\in[0,L_{total}]\);
2. The analytical determination of the position of the nodes in the surface of the endodontic file is performed, taking into account the number of desired elements in the longitudinal (\(n_{v}\)) and angular directions (\(n_{\theta}\)). Let us reiterate that all nodes of the FE mesh are determined analytically using Equation (11);
3. Discretization of the surface of the endodontic file into triangular faces is accomplished using the nodes determined previously. Using this boundary representation of the endodontic file, the tetrahedral mesh is constructed using the constrained Delaunay tetrahedralization implemented in the TetGen library [25]. This tetrahedralization does not change the position of the nodes defined for the endodontic file surface, and the resulting tetrahedrons keep the faces provided as input information. When the FE mesh is generated, mechanical properties are assigned to its elements. The mechanical response of a material in its elastic range can be defined by the elastic modulus \(E\) and the Poisson's coefficient \(\
u\). Assuming the endodontic file is manufactured using a NiTi alloy, these material parameters are established as \(E=36\) GPa and \(\
u=0.3\)[1]. Of course, the user can specify other values. In the last step, the loading and boundary conditions for the FE model are established. Endodontic files are usually tested for bending and torsional loads, and the typical procedure for these tests is described in [26] and summarized in Figure 4. In these analyses, the endodontic file is approached to a cantilever beam. A fixed support is defined at a distance \(d_{enc}\) from the tip of the endodontic file, in such a way that all the nodes below that dimension have all their degrees of freedom constrained. Typical magnitudes for \(d_{enc}\) are between 3 mm [2,20,22,27,28] and 4 mm [29], although other values could be considered [1,21]. Loads are specified at the other part of the endodontic file. For such a purpose, a rigid surface is defined comprising all the nodes within the end face. A reference node is defined at the center of this face, whose movements are coupled to the movements of the rigid surface by means of a multi-point constraint. Loads are applied directly over this reference node. Two different load cases are derived to study the bending (Figure 4a) and torsional (Figure 4b) response of the endodontic file. In the first of them (Figure 4a), a tangential load \(F_{t}\) is introduced over the reference node; in the second (Figure 4b), a torsional moment \(M_{z}\) is considered over this reference node. This procedure provides an input file for the FE solver that contains the entire definition of the FE model.