## 2 Materials and Methods
### Finite Element Numerical Modeling
according to the following sequence: \(\alpha=0^{\circ}\), \(\alpha=5^{\circ}\), \(\alpha=10^{\circ}\), \(\alpha=12^{\circ}\), \(\alpha=13^{\circ}\), \(\alpha=14^{\circ}\), \(\alpha=15^{\circ}\), \(\alpha=18^{\circ}\), \(\alpha=20^{\circ}\), \(\alpha=25^{\circ}\), and \(\alpha=30^{\circ}\). Chamfer angles higher than \(30^{\circ}\) are considered inadequate from a technical point of view since the hub width at the upper surface becomes too small to be used. The maximum chamfer angle can be calculated as a function of the hub thickness as follows: \(\alpha_{\text{max}}=\text{atan}(l/l_{\text{r}})\). The revolute symmetry of the shaft-hub assembly (Figure 1) allows the reduction of the FE model to an axisymmetric case (Figure 3) with the corresponding saved time in terms of computing. In this way, the boundary conditions must be considered; null displacements in the radial direction were imposed in the nodes placed at the shaft axis. In addition, the geometry was also simplified taking into account the transversal plane's symmetry. The boundary conditions were completed, imposing null displacements in the axial direction of the nodes of the shaft and hub placed at this plane, \(z=0\) (Figure 3). No external forces were applied. Considering the aim of the study, attention was primarily paid to the hub-shaft interface. Thus, the radial interference at the hub-shaft interface corresponding to the selected interference fit was included in the FEM simulations by means of a built-in function of the FEM software used in this study (MSC.MARC) available in the definition of the contact type (named \"touching\") between the shaft and the hub. This option allows one to impose a given radial interference, causing contact pressure at the interface of the simulated interference fit. Contact is modeled as frictionless, taking into account the fact that friction has a negligible influence on stress distributions according to previous studies [27,35]. Conventional steel (AISI 1085) was chosen for both the shaft and the hub. The following material properties were considered in the simulations: Young's modulus \(E=210\) GPa, Poisson coefficient \(\
u=0.3\), and yield strength \(\sigma_{\text{Y}}=276\) MPa. The FE modeling parameters are summarized in Table 1.  
The geometry of both bodies (shaft and hub) was meshed using four-node quadrilateral elements. A non-uniform mesh was selected with an increasing meshing size out of the zones of interest, i.e., the shaft-hub interface and hub. In this way, a refined mesh was obtained at the interface without significantly increasing the computing time. Diverse meshes were considered up to reach the required convergence in the results. A mesh factor \(K_{\text{m}}\) defined as the ratio of the number of mesh elements and the number of base mesh elements was considered in the mesh convergence analysis. Thus, different meshes were applied, decreasing the size of the elements in terms of the mesh factor (\(K_{\text{m}}\)) following the sequence \(K_{\text{m}}=1\), \(K_{\text{m}}=2\), \(K_{\text{m}}=4\), \(K_{\text{m}}=8\), and \(K_{\text{m}}=16\). In this way, each mesh has double  
Figure 3: Scheme of two–dimensional finite element modeling of the interference fit with (a) a partial–chamfer hub and (b) a full–chamfer hub. Point A is located at the hub edge and point B is placed at the half cross section of the hub at the interface. the elements of the previous one.