## 2 Materials and Methods  
A freely downloadable CBCT (cone beam computed tomography) scan of a partially dentate human mandible and maxilla [25] was used as a basis for creating an FEA model (using the simulation software ABAQUS/CAE 2022, Dassault Systemes Simulia Corp., Providence, RI, USA). Processing of the CBCT scan (Meshmixer 3.5 and Autodesk Fusion 2024, Autodesk Inc., San Rafael, CA, USA) was performed in such a way that a mandibular section resembling the region of the lower left first molar was obtained. Bone was modeled with an outer cortical layer of 2 mm in thickness [26] and a core of softer, trabecular bone. An implant osteotomy was created in the center of the model with a diameter of 3.5 mm and a depth of 10 mm as recommended by the implant manufacturer (Figure 2a,b). STEP (Standard for the Exchange of Product model data) files of the novel implant (MT, AlfaGate, Bonn, Germany) and a conventionally tapered implant (SCI, AlfaGate) formed the basis for generating FEA models of the dental implants, shown in Figure 2c. The MT implant had a maximum diameter of 4.3 mm and a length of 10 mm while the maximum diameter of the SCI implant measured 4.2 mm with a length of 9.7 mm. The insertion of the implant, treated as a rigid body, was performed by combining longitudinal displacements for insertion with rotation, where longitudinal velocities of the implant SCI and MT were calculated with respect to their thread pitches and the angular velocity of 30 rpm reflecting a clinically realistic setting [19]. Four-node linear tetrahedra were used as elements for implants and bone with a general mesh size of 0.5 mm used for the implants and 1.7 mm used in both cortical and  
Figure 2: (**a**) Cutting of the mandibular section and creation of an osteotomy for the implant (black). (**b**) Meshing of the mandibular section, modeled as a two-phase composite structure with a 2 mm cortical layer. (**c**) Meshed novel implant design MT (**left**) and standard tapered design SCI (**right**). trabecular bone. A refined mesh with an element size of 0.2 mm was used in the bone surrounding the osteotomies (Figure 2b). The implants SCI, MT, and the bone model were meshed into 113,298, 15,261, and 229,515 elements, respectively. The mechanical properties of the Ti implant, densities of two different bone layers, fracture strain, and stress triaxiality were referenced from [PERSON] 2011 [27], [PERSON] 2017 [19], and [PERSON] 2021 [28]. Due to the high modulus of Ti as compared to bone, the implant was treated as a rigid body in the simulations. For the bone, an isotropic elastic--plastic constitutive model was selected, assuming homogeneous regions of cortical and trabecular bone, which, in this model, constitutes an idealized composite material. The properties assigned to both regions are given in Table 1. Ideally, bone elasticity should be modeled depending on the density and orientation of the microscopic trabecular fabric, resulting in heterogeneous and anisotropic elastic behavior. As this would necessitate knowledge about the local microstructure, we keep the description as an idealized homogeneous composite material, as is still common in the literature [29]. Bones show plastic deformation under higher stresses, which is related to damage resulting from microfractures. In the ABAQUS software, a ductile damage model has been configured, which calculates the equivalent plastic strain as a function of stress triaxiality and strain rate parameters, also given in Table 1. In ABAQUS, the damage of a material starts after surpassing damage initiation criteria, occurring here at total strains of 0.02 for cortical bone and 0.061 for trabecular bone. These values have been extracted from compressive stress-strain curves published in [PERSON] et al. [27]. In this work, ductile damage was used to represent the onset and progression of damage due to nucleation, growth, and coalescence of voids and microcracks.