Finite Element Analysis on Stress Development in Alveolar Bone During Insertion of a Novel Dental Implant Design

Featured Application

This study provides evidence that a modern dental implant design may optimize bone compression for achieving primary stability while at the same time leaving room for new bone formation. Ultimately, the biomechanical features of the studied novel dental implant can enhance osseointegration and minimize marginal bone level change resulting from surgical trauma.

Abstract

A novel macrodesign for a dental implant characterized by a non-monotonic variation in core diameter and thread shape has been described to produce lower stress levels during insertion as compared to conventional tapered implants. Two finite element models resembling the lower left molar region with preformed osteotomies were created based on a cone beam computed tomography (CBCT) scan. Insertion of both the novel and the conventional, tapered implant type were simulated using Standard for the Exchange of Product model data (STEP) files of both implant types. Von Mises equivalent stress, strain development, and amount of redistributed bone were recorded. The conventional implant demonstrated a continuous increase in strain values and reaction moment throughout the insertion process, with a brief decrease observed during the final stages. Stress levels in the cortical bone gradually increased, followed by a reduction when the implant was finally positioned subcrestally. The novel implant achieved the maximum magnitude of reaction moment and cortical bone strain values when the implant’s maximum core diameter passed the cortical bone layer at around 60% of the insertion process. Following a notable decrease, both the reaction moment and stress started to rise again as the implant penetrated further. The novel implant removed more bones in the trabecular region while the conventional implant predominantly interacted with cortical bone. Overall, the novel design seems to be less traumatic to alveolar bone during the insertion process and hence may lead to reduced levels of initial peri-implant bone loss.

1. Introduction

Achieving primary stability is still a major goal in dental implant surgery for ensuring osseointegration [1,2]. Alveolar bone quality present in a specific site, the properties of the implant system as well as the surgical technique used constitute the major determinants of primary implant stability [1,3].

In the past, maximizing primary stability was considered as being advantageous, especially for employing immediate or early loading protocols [4]. This was often achieved by undersizing the osteotomy relative to the implant diameter [5] and by using tapered implant macrodesigns [6], leading to compression of alveolar bone, particularly in the cortical layer. An extensive literature review [7] described initial bone resorption as occurring as a consequence of damage accumulation during implant surgery caused by thermal damage [8], underpreparation of an osteotomy [9], or by using a tapered implant compressing cortical bone [5]. At least in part, this may be seen as the reason for marginal bone level change [2,10] around freshly installed dental implants prior to prosthetic restoration in conventional loading protocols [11,12]. In extreme cases, the resulting high bone strains during implant installation [13] may even lead to fractures of the esthetically relevant buccal bone plate (Figure 1).

In order to overcome the problem of mechanically overloading cortical bone, the industry started offering implants which at least in the cervical region show a triangular/trioval cross-section [14,15]. This was done in order to reduce the stress generated in the buccal lamella of alveolar bone when the implant is placed in such a way that a flat surface of the implant coincides with the buccal aspect. However, with those implants having been in clinical use, initial reports suggest no significant difference compared to conventionally round implants [16].

As an alternative solution, a novel implant design with sharp, cutting threads in the apical and cervical portions but blunt, condensing threads in the middle portion of the implant body, coinciding with a shift in the core diameter of the implant, has been introduced [17]. This implant has been shown to require maximum insertion torque when its bulky portion passes the cortical layer of bone and primary stability is derived from compacting trabecular bone [18,19]. Based on two in vitro studies [17,20], this design results in reduced buccal bone deformation during the insertion process, while at the same time, greater stability can be gained in advanced clinical situations such as sinus lifting and immediate implant placement [20]. A recent animal trial has shown that the novel implant designs allow for better maintenance of existing alveolar bone, i.e., greater undersizing of osteotomies while not overstressing bone during the insertion process and hence leading to less marginal bone level change [21].

Finite element analysis (FEA) is an established numerical technique in engineering and materials science and has been extensively applied for addressing biomechanical problems in implant dentistry [22,23]. FEA allows for determining magnitudes of local stress, strain, and damage that occur during the insertion process and masticatory loading [24], thereby giving criteria to improve both implant design and insertion protocols. It was the goal of this finite element analysis to compare the novel implant design [17] to a conventional tapered implant design with respect to stress and strain generation during the insertion process. In addition, the amount of bone cut and transported during implant insertion has been quantified as an indicator of primary stability.

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 Systèmes 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 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 Guan 2011 [27], Dorogoy 2017 [19], and Demirbas 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. Material properties and threshold values for ductile damage used in FEA simulations.

	Titanium Implants	Cortical Bone	Trabecular Bone
Density [kg/m3]	4540	1900	1000
Young’s modulus [MPa]	120,000	12,247	692
Poisson’s ratio	0.3	0.35	0.35
Yield stress [MPa]		180	35
Threshold values for ductile damage
Fracture strain		0.004	0.011
Stress triaxiality		0.5	0.5
Strain rate [s−1]		1	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 Guan 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. After this onset point, the damage evolution is associated with stiffness degradation, which will further control the bone material’s behavior and finally induce element deletion [30].

The displacements in the mesial and distal borders of the bone segment (Figure 2b) were fixed, and stress-free conditions were applied elsewhere. For the boundary between the implant and the internal bone surface, a general contact algorithm was applied due to its capability of modeling multiple contact scenarios (edge-to-edge, edge-to-surface, etc.), which is applicable for the complex geometry of the threaded implants. A friction coefficient of 0.35 [28] was assumed between the implant and bone interface. The damage model applied here leads to a removal of overly strained elements after accumulating 100% damage, which represents the material removed by the cutting edges of the implant. It is noteworthy that the value of the removal criterion and friction coefficient are estimated here, but they significantly influence stress, strain, and torque evolution during insertion. For determining the amount of bone cut and transported by the implant during the insertion process, the status of all elements was checked and their volume summed up.

For evaluating von Mises equivalent stress during implant insertion, its maximum value was recorded step by step with increasing insertion time in the complete cortical and trabecular bone regions as shown in Figure 3a. Also, strain development in the most critical area, i.e., the thin cortical bone layer adjacent to the implant–bone interface, was investigated during the insertion process: the maximum strain values from three elements at a distance of roughly 1.2 mm from the border of the osteotomy (indicated in Figure 3b in red) were averaged and plotted over time (Figure 4).

3. Results

Due to the large contrast assumed for the elastic moduli of the two bone compartments, much greater stress values of up to 203 MPa were observed in cortical bone as compared to a maximum of 54 MPa recorded in trabecular bone. As stress can be transferred from cortical bone to trabecular bone, in both implant designs, increasing stress was already observed in trabecular bone when the implants started to compress the cortical bone layer. A stress rise in both bone layers was detected at insertion distances of 2 mm and 1.2 mm for the SCI and MT, respectively (Figure 4a,b). This difference was due to the later contact of SCI with the bone, which is attributed to its tapered macrodesign. Similarly, SCI and MT began to contact trabecular bone at distances of 4.2 mm and 3.2 mm, respectively. However, the influence of the trabecular bone is evident even before the direct contact. As shown in Figure 4a,b, the stress build-up in trabecular bone begins prior to the actual contact between trabecular bone and implants. This simultaneous appearance can be explained by the close interconnection between the cortical and trabecular layers of bone, transmitting stress between the layers despite the large elastic contrast. Please compare also the evolution of maximum strain for both implants (Figure 5) and the maps of von-Mises stress for mesial-distal and lingual-buccal sections given in Figure 6 for the SCI and in Figure 7 for the MT implant.

At an insertion distance of 6 mm, the cutting threads of MT pass through the cortical layer, leading to a decrease in stress levels. Around the same time, the stress in the trabecular bone reaches its maximum and remains relatively constant until the final insertion step. After this point, the maximum stress in the cortical bone begins to increase again (Figure 4a). At approximately 8.7 mm, the neck of the implant SCI, which has a constant diameter, enters cortical bone, resulting in a decrease in maximum stress (Figure 4b).

Due to its shape, MT induces high strain levels in bone at around 60% of the insertion process. In contrast, the strain values for SCI show a more continuous increase, with a decrease only occurring during the final stages of the insertion process when the implant was placed subcrestally, reducing contact with the cortical bone layer. The continuous rise in strain for SCI is likely due to its increasing diameter, which expands the osteotomy and causes higher strain in the surrounding areas of bone. This is exemplified in the continuous rise in the maximum strain value (SCI) determined from three selected elements representing buccal bone (Figure 3 and Figure 5) as a function of insertion depth. In contrast, the final insertion of the MT implant reduced the strain induced in its surroundings.

The volume of the bone damaged and removed by the MT implant exhibits a cylindrical and relatively denser geometry (Figure 8d), while the bone removed by the implant SCI resembles a truncated cone with its base in the cortical area and the cutting threads clearly visible (Figure 8c). As shown in Figure 9a, the volume of drilled bone increases more steadily with insertion time for the MT implant as compared to the SCI implant, which gradually removes more bone, as indicated by the gradient of the curve. This is a consequence of the faster diameter increase in the apical part of the MT implant, which accordingly cuts more bone material than the implant SCI, particularly in the trabecular bone region, as shown in Figure 9b. It must be noted that the link between the amount of bone removed during the insertion simulation and clinical implant stability is not obvious. In contrast to the damage model used in the simulation, the bone chips would not simply vanish in reality but be compacted in the implant–bone interface. We interpret the larger amount of bone removed as evidence for a stronger interaction with the trabecular region. This aligns with the design purpose of the novel MT implant, which achieves primary stability by predominantly engaging trabecular bone [17,20].

Figure 10a,b illustrate the stress distribution along a path at 1.2 mm distance from the osteotomy wall for different insertion depths of the implants, at the position shown in Figure 3a. Both figures indicate that the stress level in the cortical bone is higher than in the trabecular bone due to differences in yield points and stiffness. Therefore, a sudden drop in von Mises stress is observed at a true distance of 2.54 mm, which corresponds to the interface between the cortical and trabecular bone.

Figure 10 also demonstrates that when the implants interact solely with the cortical bone (within the displacement ranges of 2–4.2 mm for SCI and 1.2–3.2 mm for MT), stress can be transferred from the cortical bone to the trabecular bone (Figure 10a,b and stress distribution maps in Figure 6 and Figure 7). The stress level in trabecular bone generally increases as the implants approach it, as indicated by the red arrows in Figure 10a,b.

The stress level in the cortical bone increases as the implants penetrate further; the trabecular bone helps to reduce the stress in the cortical bone at some points. For instance, when the SCI implant interacts with the trabecular bone at a displacement of 4.2 mm, the stress in the cortical bone is relatively lower compared to the stress at 4 mm. This observation further supports the idea that the trabecular bone aids in redistributing stress within the cortical bone layer, similar to a sandwich structure in engineering.

Reaction moments were analyzed to evaluate the resisting torques throughout the insertion process. As shown in Figure 11, the results fluctuate due to the dynamic nature of the insertion process and potential element deletion procedures, similar to Dorogoy 2017 [19]. To indicate the trend, the data was smoothed by adjacent averaging over 5 points.

Due to the more gradual diameter increase along its length of the SCI implant, resistance to the insertion begins later compared to the MT implant. The moment increases monotonically to a much higher value of t 300 Nmm (as compared to 80 Nmm for the MT implant). At 6 mm insertion, the bulky part of the MT implant completes penetration of the cortical bone layer, temporarily reaching the maximum reaction moment. Beyond this point, the reduced stress in the cortical layer is almost compensated by the increased stress in the trabecular region, leading to a nearly constant torque. As the implant MT continues to interact with trabecular bone, the reaction moment gradually increases again. The absolute values of the reaction moments found here are about 25–40% smaller than in comparable experimental [18] and simulation studies [19]. This magnitude strongly depends on the friction between bone and implant, and the stiffness change defined in the damage model, which is hence a property to be adapted more precisely for future studies.

In contrast, the reaction moment of the implant SCI is continuously increasing until the final stage of the insertion process, where a drop can be attributed to the moment when the implant neck is seated subcrestally. Here, the primary stability is achieved by continuously compressing the cortical bone layer.

4. Discussion

While exact proof showing that high mechanical stress levels evoked during implant insertion inevitably cause bone resorption is still missing in the literature, growing evidence seems to indicate that less trauma during implant surgery reduces initial bone loss [2,5,9,10]. In this context, this FEA study aimed at comparing two different implant macrodesigns with respect to stress and strain generation in bone during the insertion process as well as the amount of bone cut and transported along the osteotomy walls.

As expected, the novel implant caused maximum stress and strain when the middle part with increased core diameter and blunt threads passed the cortical layer of bone. Less stress and deformation were observed during the final stages of implant insertion when the deeper and sharper threads engaged the cortical layer of bone. The conventional, tapered implant caused less stress during the initial phase of insertion, until reaching its cervical third, which then led to much greater stress as observed with the novel implant. This maximum stress state remained at its level upon seating the implant. This behavior is in accordance with previously conducted strain gauge studies using polyurethane foam as a bone surrogate material [17]. While not evaluated in this simulation, the engagement of cortical bone at low stress levels seen with the MT implant compared to implant designs featuring a cervical back taper [20] or triangular/tri-oval cross-section [14,15] seems advantageous in areas with limited bone quantity and bone quality. As per manufacturer recommendation, a 3.5 mm osteotomy was simulated for both implant types despite the conventional, tapered SCI implant having a 0.1 mm smaller diameter compared to the MT implant. This has to be considered as an additional variable when interpreting the findings presented, as even more favorable values could have been expected if the amount of undersizing had been equal for both implant types. An alternative would have been to harmonize the amount of undersizing of the osteotomy relative to the implant diameter.

As evidenced by the amount of bone cut and transported along the walls of the osteotomy, the MT implant engages bone almost over its whole length, while the conventional implant mainly engages bone in the cervical part. As such, this study appears to demonstrate that the novel implant derives primary stability through compression of trabecular bone instead of cortical bone [18,19] as observed in the conventional conical implant and recently described in an in vitro study [31]. This finding is also in line with two previous experiments conducted on bone surrogate materials using the MT implant [17,20].

As with every finite element analysis, specific limitations have to be considered, limiting the clinical validity of the data presented. Despite using a CBCT-derived bone model as well as exact implant geometries, this study only allows for relative comparisons between the two specific implants tested. Attempting to closely simulate clinical reality, assumptions had to be made with respect to cortical bone thickness, insertion velocity, and friction between implant and bone. Furthermore, bone was simulated as an ideal composite consisting of two distinct compartments, and the material properties of bone were modeled as being isotropic, elastic–plastic. This clearly constitutes a methodological limitation, as real bone at the continuum scale would show anisotropy and heterogeneous composition. To overcome these limitations, the material model could be improved by using bone density-related stiffness and including elastic transversal anisotropy. A more precise adaptation of the friction coefficient between implant and bone would be possible by matching the magnitude of created reaction moments with clinical observation of the specific implant during insertion. In addition, future work will include a sensitivity analysis to quantify the effect of the expected scatter of bone material properties among various patients.

The link between the parameter “bone volume drilled” and clinical implant stability may appear weak. When relying on simulation test procedures, the level of bone compression and surrounding bone density could be used as major indicators for primary stability. Contrarily, a higher amount of removed bone, which is a consequence of the damage model, could reduce stability. We interpret the larger amount of removed bone of the novel MT design as being equivalent to a stronger deformation over the yield level of predominantly trabecular bone. This drilled material would, in reality, be rather compressed than deleted from the material assembly as in the FEM model. In addition, damping capacity measurements and resonance frequency analysis have been used in previous in vitro studies for assessing primary stability of the MT implant compared to tapered implant types and confirmed superior performance [17,20]. Similarly, it may be questioned whether or not reduced mechanical stress during implant surgery reduces peri-implant bone loss. A recently published animal trial [21] confirmed the simulation results shown here, indicating better peri-implant bone maintenance for the MT implant.

Implant surgery and initial bone loss constitute only one episode in the lifetime of a dental implant, while long-term maintenance of marginal bone levels during masticatory loading [32] is assessed as equally important. This has not been addressed here, but these should be simulated with refined models as mentioned above in future studies.

5. Conclusions

All parameters investigated in this study indicate that the MT implant shows advantageous biomechanical performance during the insertion process. Deriving primary stability from compressing trabecular instead of cortical bone should reduce the necessity of increasing osteotomy diameters while leaving room for new bone formation. Ultimately, clinical trials are required for fully assessing the capabilities of the novel implant design.