# A Novel Digitized Method for the Design and Additive Manufacturing of Orthodontic Space Maintainers
## 2 Materials and Methods
### Finite Element Analysis  
Finite element analyses were performed by Ansys 2022 software to simulate a bending test on the space maintainer. The aim was to evaluate its mechanical behavior under static structural conditions, considering large displacements and elastic-plastic material properties. The purpose of the finite element analysis is to simulate the impact of unforeseen loading on the functionality of the device. Specifically, the analysis considers the possibility of out-of-plane loading, which could occur if external elements exert pressure on the device during occlusion movement. Practically, this loading condition was simulated using a rigid pin to emulate a bending test. The material properties used in the analysis were determined through experimental tensile tests. The linear-elastic behavior was modeled through [PERSON]'s modulus E of 2183 MPa and a Poisson's ratio (\(\
u\)) of 0.39, while the plastic material behavior was implemented by means of a multilinear isotropic hardening model, as presented in Table 1.  
\begin{table}
\begin{tabular}{c c c c} \hline \hline
**Plastic Strain (mm/mm)** & **Stress (MPa)** & **Plastic Strain (mm/mm)** & **Stress (MPa)** \\ \hline
0 & 5 & \(1.72\times 10^{-2}\) & 31.1 \\ \(8\times 10^{-4}\) & 10 & \(2.22\times 10^{-2}\) & 32 \\ \(21\times 10^{-3}\) & 15 & \(3.6\times 10^{-2}\) & 32.5 \\ \(3.7\times 10^{-3}\) & 21 & 0.1 & 35.5 \\ \(6.8\times 10^{-3}\) & 25 & 0.104 & 36 \\ \(1.27\times 10^{-2}\) & 29.5 & & \\ \hline \hline \end{tabular}
\end{table}
Table 1: Elastic-plastic material properties for “OD-Clear MF Bio monomer free” resin.  
Figure 4: Generative design main steps: (**a**) T-Spline surfaces generated from the portions of the intraoral 3D scan, (**b**) manifold thickened bodies, (**c**) volumes to be avoided during the procedure highlighted in yellow, (**d**) output from the generative design and (**e**) digital model of the space maintainer on the mesh of the 3D scan.  
A three-dimensional finite element model was created to simulate the teeth space maintainer, as illustrated in Figure 5. The geometry was discretized using brick elements with quadratic shape functions and a nominal dimension of 0.1 mm. The model consisted of 191,081 nodes and 108,912 elements, determined through a convergence study. Convergence criteria ensured that the maximum von Mises stress differed by less than 3% between successive mesh iterations. To simulate the bending test, appropriate boundary conditions were applied. A fixed support boundary condition was used to represent the contact between the space maintainer and the adjacent teeth (C and D surfaces of Figure 5). It is worth noting that constraints C and D were intended to model the cementation process between the device and the patient's teeth. Furthermore, a rigid cylindrical pin simulated the applied force caused by the external object. A frictionless contact formulation between the space maintainer and the pin was employed (A and B surfaces of Figure 5), eliminating the need for a friction coefficient. The finite element analysis assessed the mechanical response of the teeth space maintainers under bending conditions, yielding stress and displacement distributions that offer valuable insights into their behavior. Detailed results will be presented and discussed in a subsequent section, providing a comprehensive understanding of the space maintainer's performance.