## 2 Materials and Methods  
### Finite Element (FE) Model Generation  
A 13 mm long three-piece implant designed with internal hexagon Morse taper abutment connection secured with an abutment screw was selected as the evaluation type in this study. The investigated parameters included three implant sizes (implant diameters 4, 5, and 6 mm; D in Table 1) secured with 1.4, 1.6, and 1.8 mm abutment screw diameters (d in Table 1) to fit with three unilateral implant neck wall thicknesses of 0.45, 0.50, and 1.00 mm (t in Table 1). Twelve combinations of implant diameter, abutment screw size, and unilateral implant neck wall thickness were used (Table 1). Solid models of the 12 implant systems were constructed using a 3D CAD (computer Aided Design) system (Creo, Parametric Technology Co., MA, USA.) and exported into ANSYS (ANSYS Workbench v14, ANSYS Inc., Canonsburg, PA, USA) to assemble a simplified cylinder supporting bone with 16.5 mm length (including a 1.5 mm thickness cortical shell) and 10 mm diameter. The implant was exposed to the bone level at a length of 3 mm, and a hemispherical load cap was designed to cover the abutment according to the ISO14801 standard, which specifies a fatigue test method for single post endosseous dental implants of the transmucosal type and their premanufactured prosthetic components [23] (Figure 1). The test is most useful for comparing endosseous dental implants of different designs or sizes. The load center should also be designed according to the standard located at the free central longitudinal axis intersection of the connecting part and the plane normal to the implant longitudinal axis located 11 mm from the implant support level (Figure 1). Twelve corresponding combination FE mesh models were generated with quadratic 10-node tetrahedral structural solid elements (Solid 92) after the mesh convergence test while controlling for strain energy and displacement variations of \(<\)5% for models with different element sizes (Table 1). A bonded condition (continuous displacement) was assumed between the bone and implant to mimic bone/implant interface completion. Nonlinear frictional contact elements (defined as surface-to-surface, i.e., Contact 174/Target 170 in ANSYS) were used to simulate the adaptation between the abutment/abutment screw, abutment screw/implant, and abutment/implant interfaces. The contact \begin{table}
\begin{tabular}{c c c c c c} \hline \hline
**Diameter of** **Implant (D)** & **Thickness of Implant Neck (t)** & **Diameter of** **Abutment Screw (d)** & **Node** & **Element** & **Illustration of Implant Designed** \\ \hline \multirow{3}{*}{\(\mathcal{O}\)4.00} & \multirow{3}{*}{0.45} & \(\mathcal{O}\) 1.40 & 442424 & 296904 & \\  & & & \(\mathcal{O}\) 1.60 & 475068 & 319867 & \\  & & & \(\mathcal{O}\) 1.80 & 507375 & 342558 & \\ \hline \multirow{3}{*}{\(\mathcal{O}\)4.00} & \multirow{3}{*}{0.50} & \(\mathcal{O}\) 1.40 & 440134 & 294937 & \\  & & & \(\mathcal{O}\) 1.60 & 472225 & 317487 & \\  & & & \(\mathcal{O}\) 1.80 & 472896 & 317988 & \\ \hline \multirow{3}{*}{\(\mathcal{O}\)5.00} & \multirow{3}{*}{0.50} & \(\mathcal{O}\) 1.40 & 543691 & 369648 & \\  & & & \(\mathcal{O}\) 1.60 & 576516 & 392682 & \\  & & & \(\mathcal{O}\) 1.80 & 606135 & 413360 & \\ \hline \multirow{3}{*}{\(\mathcal{O}\)6.00} & \multirow{3}{*}{1.00} & \(\mathcal{O}\) 1.40 & 580837 & 395051 & \\  & & & \(\mathcal{O}\) 1.60 & 614518 & 418713 & \\ \cline{1-1}  & & & \(\mathcal{O}\) 1.80 & 643244 & 438669 & \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Combinations of implant sizes (**D**), implant neck wall (**t**), and diameter of abutment size (**d**) and their corresponding finite element (FE) models with node/element numbers used in this study. Figure 1: Solid models of our simulated models with different implant and abutment screw sizes in the right side and one of the simulated FE mesh models and loading condition in the left side. elements allowed the nodes to slip in the tangential direction with no penetration between different materials.