Influence of Morse Taper Angle and Bone Quality on the Biomechanical Behavior of Dental Implants: A Finite Element Analysis Study

Abstract

This study performed a finite element analysis to evaluate the biomechanical effects of implant connection geometry and bone quality (D2, D4) on stress distribution and structural stability. A mandibular model consisting of cortical and cancellous bone was generated, and implant components—including fixture, abutment, screw, and crown—were simulated. Two designs were analyzed based on Morse taper angle (11° or 15°) and the presence of an apical slot. A tightening torque of 32 N·cm and an occlusal load of 200 N were applied, with the lateral mandible constrained. The 11° taper with the non-slot design showed the highest von Mises stress (1048.81 MPa) in the fixture with D4 bone type and Tessera crown. In contrast, the 15° taper with the slot design improved stress distribution at the fixture–abutment interface, reducing fixture stress by 26.78% in D2 bone type. Localized stress near the slot was observed but did not compromise overall structural stability. Under oblique loading, stress concentrated primarily in the cortical bone, whereas D4 cancellous bone showed increased susceptibility to microdamage. Prosthetic materials demonstrated no significant differences in stress behavior. These findings suggest that connection design and bone density strongly influence biomechanical performance and should guide individualized implant selection.

1. Introduction

Mechanical complications associated with dental implants and upper prostheses are closely related to the design of the implant components, which may ultimately lead to biological problems such as peri-implant bone loss [1,2]. Previous studies have reported that screw loosening and fracture are the most frequent mechanical complications, and the resulting microgaps at the implant–abutment (I/A) interface increase the risk of prosthetic component fracture [3,4]. Screw-related complications are known to occur when the applied load on the I/A interface exceeds the clamping force (preload) of the fixation screw [5]. The I/A interface serves as a platform for transmitting loads to the implant and surrounding bone, making design strategies that reduce stress concentrations and promote uniform load distribution critical for minimizing implant failure risk [6,7]. Design concepts aimed at increasing the effective contact area of the I/A interface have driven the transition from early external connection-focused designs to internal connection systems. Internal connections enhance load distribution and interface stability through increased I/A contact area [8,9], and in particular, internal Morse taper connections have been reported to reduce micromovement and microleakage at the interface through frictional and wedge effects [10,11]. However, the taper angle of a Morse taper implant is in a trade-off relationship with the implant neck thickness: increasing the taper angle expands the I/A contact area but may reduce the supporting neck wall thickness. In fact, increasing the neck thickness from 0.45 mm to 0.50 mm has been shown to reduce peak stress by at least 12%, indicating that a balanced optimization between contact area expansion and structural strength is required [12,13]. Furthermore, the incorporation of a slot structure at the bottom of the connection can enhance the rotational stability of the abutment. Still, it may also induce localized stress concentrations, leading to mechanical complications [14].

In addition to implant structural design, the mechanical properties (elastic modulus) of prosthetic materials, as well as the quality and density of the peri-implant bone, influence load transfer and stress distribution. The choice of prosthetic materials such as zirconia, ceramic, or PFM can alter stress concentration patterns, with these differences primarily observed at the level of the implant components [15,16]. Moreover, in compromised or weak bone, repetitive loading accelerates stress absorption, reducing structural support and transmitting excessive stress to implant components, thereby increasing the risk of complications [17,18].

Meanwhile, in clinical settings, it is difficult to perform precise quantitative comparisons based on stress concentration. Therefore, finite element analysis (FEA) has established itself as an essential research tool that can reproducibly quantify stress and strain distributions under conditions that are difficult to reproduce clinically by integrating material properties and occlusal loads into a three-dimensional (3D) model of the jawbone and soft tissue [19,20,21]. Nevertheless, many dental FEA studies have primarily focused on the stress distribution within the fixture or comparisons between connection types, such as internal friction and external hexagonal [6,22,23]. Accordingly, the present study systematically evaluates the stress and strain responses of implant components and the biomechanical behavior of surrounding bone using I/A models incorporating Morse taper angles and slot designs. Specifically, this study aims to examine the hypothesis that increasing the Morse taper angle expands the I/A contact area and improves load distribution, thereby providing rational design guidance to minimize implant failure.

2. Materials and Methods

3D mandibular models were developed using modeling software (SolidWorks 2020, Dassault Systems, Velizy, France). The mandible was segmented into cortical bone and cancellous bone according to anatomical features. To thoroughly analyze the osseointegration interface, a virtual cylindrical layer with a diameter of 1.0 mm was created at the bone–fixture junction (Figure 1a). The implant was then virtually inserted into the bone by performing a subtraction of its geometry, establishing the bone–fixture interface for subsequent finite element analysis. The implant system used for analysis was a bone-level, internal connection fixture (length 10 mm, diameter 4.0 mm), positioned in the mandibular first molar site. Two types are modeled based on the Morse taper angle (11° or 15°) and the presence of an apical slot structure (Figure 1b). The finite element model was composed of four-node tetrahedral elements. The mesh size for the implant–abutment–bone complex ranged from 0.2 to 1.0 mm, refined at the implant–abutment interface and crestal bone regions [24]. The final mesh information, including the number of nodes and elements for each structure, is summarized in

Table 1. Number of nodes, elements, and mesh size for the FEA model.

Model Section		Number of Nodes	Number of Elements	Element Size (mm)
Fixture	* NS	247,531	48,908	0.2–0.25
	* S	221,928	44,220
Abutment	NS	119,080	24,572	0.2–0.25
	S	302,859	61,991
Screw	NS	50,433	10,323	0.2–0.25
	S	64,394	13,525
Resin cement		63,350	19,257	0.15
Crown		350,476	65,848	0.5
Cortical bone		46,564	10,538	0.2–1.0
Cancellous bone		239,391	44,959
Peri-implant cortical bone part	NS	30,621	6522	0.2
	S	30,997	6581
Peri-implant cancellous bone part	NS	281,084	54,769	0.2
	S	255,704	50,111

* NS: non-slot design, S: slot design.

.

All materials in the finite element model were assumed to be isotropic, homogeneous, and linearly elastic [25]. The bone model classified cancellous bone into D2 and D4 according to the classification of Misch classification, reflecting normal bone and reduced bone strength conditions such as osteoporosis [26,27]. The components of the implant include fixture, abutment, screw and crown. The abutment, fixture, and screw were all fabricated from commercially pure titanium grade IV, consistent with the manufacturer’s specifications (Osstem Implant, Seoul, Republic of Korea) [28]. The crown was reconstructed into a virtual model based on the natural tooth. Prosthetic crowns were using three materials: Porcelain-Fused-to-Metal (PFM), Tessera, and Zirconia [15,29]. A resin cement layer with a thickness of 0.1 mm was incorporated between the abutment and crown [30]. The elastic modulus and Poisson’s ratio for each component are shown in

Table 2. Material properties of the FE models.

Model Section		Young’s Modulus	Poisson’s Ratio	Reference
* Titanium		105,000	0.34	[28]
Resin cement		18,600	0.28	[30]
Cortical bone		13,700	0.3	[27]
Cancellous bone	D2	1370	0.3	[27]
	D4	690	0.3	[26]
Crown	Porcelain-Fused-to-Metal	149,450	0.34	[29]
	Tessera	103,000	0.229	[29]
	Zirconia	210,000	0.3	[15]

* Titanium: abutment, screw, fixture.

.

FEA was performed using Abaqus (Abaqus CAE 2025, Dassault Systems, Velizy, France). The simulation was conducted in two steps. First, a tightening torque of 32 N·cm was applied to the screw, generating pre-load at the screw–abutment interface [27,31]. In the next step, a maximum occlusal force of 200 N was applied to the total of the cusps and fossa in the direction of the tooth axis and the incline angle of 30 degrees (Figure 2) [32,33]. To simulate the support of the surrounding tissues for the mandible, both lateral sections of the bone model were fixed in all directions (x, y, z), restricting any displacement. Boundary conditions were defined as follows: the interfaces between fixture–abutment, abutment–screw, and abutment–cement were defined as “contact” with a friction coefficient of 0.3. The bone–fixture interface and all other interfaces were assumed to be completely “tie” [19].

3. Results

The yield strength of commercially pure Grade IV titanium (500 MPa) was used as a reference for analysis [28,34]. Yield strength is the maximum stress a material can withstand before plastic deformation occurs. The von Mises stress was employed to evaluate the distortion energy density and to predict potential structural failure. In addition, peri-implant strain values were calculated to assess the risk of fatigue failure. According to mechanostat theory, a strain threshold of 3000 με was applied, beyond which microdamage may accumulate faster than bone remodeling can compensate, potentially leading to microfracture and loss of healing capacity [35,36].

The stress distribution within the fixture was primarily influenced by the connection geometry rather than the crown material. While the crown type (PFM, Tessera, or Zirconia) had no significant effect, the fixture applied the slot design consistently showed lower maximum von Mises stress than the non-slotted design under both vertical and oblique loading conditions (Figure 3). The stress reduction was more pronounced under oblique loading conditions. On average, the slot design reduced maximum fixture stress by 264.18 MPa, likely due to the wider fixture–abutment contact area, which improved stress distribution.

The highest von Mises stress (1048.81 MPa) occurred in the fixture that applied the non-slot design in D4 bone type with the Tessera crown. Stress concentrations were observed primarily along the buccal and lingual contact areas along the loading direction (Figure 4). The abutment showed the highest stress (1271.99 MPa) in the D4 bone type with the Tessera crown, the highest value among all components. Nevertheless, when the slot design was applied, the maximum stress of the fixture was reduced by 26.78% in D2 bone type and 24.51% in D4 bone type, indicating improved stress distribution. Fatigue fracture analysis results showed that the volume fraction exceeding the critical strain (3000 με) remained below 3% in all models (Figure 5). Areas with a high risk of fatigue were primarily concentrated in the cancellous bone surrounding the implant, especially around the lingual implant, which is subject to oblique loading. As bone quality decreased, the strain-exceeding area expanded in D4 bone type in cancellous. The slot design exhibited the highest volume fraction (2.85%) in both the cortical and cancellous bone regions. However, this localized increase did not indicate significant structural damage. In D2 bone type, the volume fractions of cortical and cancellous bone were nearly 0%, and while slightly increased under oblique loading, they remained minimal.

4. Discussion

This study analyzed the stress and strain acting on dental implant components and the surrounding bone, depending on connection type and bone quality, to identify key factors. The results confirmed that increasing the Morse taper angle significantly improved load distribution and long-term implant stability by increasing the I/A bonding surface area.

Risk factors for mechanical complications include fixture design, inadequate abutment junction, cantilevered prosthesis design, and excessive occlusal forces due to patient habits such as bruxism or clenching [35]. Unexpected occlusal forces, either in magnitude or direction, may overload the implant-alveolar bone complex, potentially leading to implant failure. To address this limitation, widening the fixture–abutment interface has been recommended [37,38]. These mechanical-biological interactions vary depending on the bone quality and biological conditions of each patient. Therefore, comprehensive optimization is necessary, accounting for the biomechanical properties of the implant and bone tissue. Therefore, various factors need to be analyzed to achieve a balance between increasing the abutment bonding area and the implant neck thickness, depending on the bone tissue characteristics.

This study compared two abutment designs: one without a slot and one with a slot. The slot design, with a 15° taper angle and three slots at the apex, increased the contact area, improving load distribution and reducing micromotion. Analysis revealed that under vertical loading, the 15° slot design exhibited the lowest von Mises stress (<1048.81 MPa), which was significantly lower than the yield strength of titanium Grade IV (500 MPa). Under oblique loading, the slot design also showed 26.78% stress reduction in D2 bone type and 24.51% stress reduction in D4 bone type, demonstrating that the wide taper angle effectively distributed stress transfer. This is interpreted as the wide taper angle effectively dissipating stress transferred to the fixture. These results are consistent with previous fatigue test results and support the notion that a large taper angle increases the contact area at the fixture–abutment interface, alleviating stress concentration and enhancing structural stability [39]. The slot design abutment observed stress concentration in the apical slot under all conditions. However, the slot clinically contributed to preventing abutment displacement and maintaining proper hexagonal alignment, so the stress concentration was judged not to have a significant effect on stability. Although relatively rare, fixture fracture is considered a serious complication, as it carries a poor prognosis and requires complete removal. In contrast, abutment and screw fracture are considered relatively manageable complications [40]. Therefore, sacrificial failure at the abutment and screw may be considered a positive design concept to prevent fixture fracture.

Complications of dental implants arise from the complex interactions between biological tissues and mechanical components. Biological complications may lead to mechanical failure, while conversely, mechanical problems, such as fixture cracking, may promote biological responses, such as microbial infection. While consistent mechanical stimulation is essential for bone remodeling, stress concentrations in D4 bone type may accelerate bone loss. If functional loading exceeds the load-bearing capacity of the bone–fixture interface, osseointegration may be compromised, leading to implant and surrounding tissue failure. Previous studies have reported that maximum von Mises stress within the implant component significantly increases when marginal bone loss exceeds 2 mm [41,42].

In this study, strains remained below the physiologically acceptable limit (3000 με) in both cortical and cancellous bone when an occlusal force of 200 N was applied. Loading direction had a significant effect on the cortical bone surrounding the implant neck. oblique loading led to a larger fatigue failure zone across all bone types. In particular, the slot design showed the highest fatigue failure volume fraction (2.85%) in both cortical and cancellous bone, demonstrating that the connection structure influences stress distribution. Suppose occlusal forces are imbalanced or marginal bone loss exceeds physiological limits during the prosthetic stage. In that case, residual stresses may not be sufficiently absorbed by the bone and accumulate in the implant components, potentially compromising long-term stability. Furthermore, D4 bone type may exhibit reduced stress-dissipation capacity, thereby expanding the fatigue failure zone, leading to irreversible microcracks and progressive bone resorption. Such non-infectious bone loss may serve as a precursor to peri-implantitis. Stable stress distributions were observed in all three crown materials, with no significant differences between materials. However, factors such as cement type and thickness, metal-to-metal friction, and cyclic loading may affect long-term performance depending on the prosthetic material used.

In this study, we demonstrated the stress distribution and mechanical stability of the fixture with the slot design. While the slot design appears to be an advantageous option for improving fixture–abutment stability in most cases, it cannot be definitively regarded as optimal for all clinical situations. The selection of abutment geometry should be based on comprehensive clinical judgment, considering individual factors such as load transfer efficiency, implant placement position, and patient-specific occlusal patterns. In D4 bone type, limited load distribution capacity may induce micromovement at the bone–implant interface, potentially compromising implant stability. The results of this study demonstrated that an internal conical connection with a large contact area, particularly the slot design abutment, increased the contact area and more evenly distributed the load. Therefore, combining the slot design with a wide taper angle may effectively distribute stress between the implant components and surrounding bone, even in weak bone environments, thereby enhancing structural stability and long-term biomechanical performance. Nevertheless, the slot design requires regular clinical monitoring and maintenance to prevent damage or fracture in the slot area, where stress tends to concentrate.

This study precisely evaluated the effects of the fixture–abutment interface on implant components and surrounding bone by varying only the abutment geometry while maintaining constant fixture conditions. Fine meshing was applied to stress-concentrated areas to ensure convergence and reliability, and insights into mechanical-biological interactions were provided, considering clinical variables. However, this study has several limitations. First, all materials were assumed to be isotropic, homogeneous, and linearly elastic, which does not adequately represent the anisotropic and viscoelastic behavior of biological tissues. This simplification may have resulted in an over or underestimation of stress magnitudes, particularly in cancellous bone. Furthermore, experimental validation and long-term fatigue behavior were not evaluated, and systemic factors that affect bone remodeling were not considered. Second, although the applied load was within the normal physiological occlusal range, actual masticatory forces vary substantially in magnitude, direction, and duration. Such complex loading conditions could alter the predicted stress and strain distributions. Third, this study considered only cancellous bone densities (D2 and D4) and did not account for variations in cortical bone thickness, which can influence load transfer and stress concentration patterns. To address these limitations, future research should include experimental validation—such as in vitro mechanical testing or fatigue evaluations—to confirm the numerical predictions, and incorporate dynamic and cyclic loading conditions. Additionally, implementing time-dependent bone remodeling models and patient-specific bone morphology would allow for more realistic simulations and improve the predictive accuracy of finite element analyses.

5. Conclusions

This study evaluated FEA to determine whether bone type and implant–abutment connection design significantly influence the biomechanical stability of dental implants. A slot design employing a 15° Morse taper improved stress distribution, effectively reducing peak stress in the fixture and distributing stress through the abutment. While the slot design concentrated stress on the abutment, this was likely due to the efficient stress distribution. Under oblique loading conditions, stress concentration was more pronounced in the cortical bone region, and D4 bone type showed a higher risk of microdamage accumulation and bone loss. To ensure long-term biomechanical stability, it is crucial to optimize the implant connection geometry and consider the patient’s bone quality when developing treatment plans. Clinically, it is advisable to assess bone quality in advance and select a connection design that effectively distributes stress.