The Influence of Design on Stress Concentration Reduction in Dental Implant Systems Using the Finite Element Method

Abstract

Dental implant fracture is closely connected to the stress buildup surrounding the implant system during static loading. In areas where the cross-section of the implant rapidly changes or where the geometry of the implant system has discontinuities, stress concentrations arise. Therefore, the implant’s design is crucial in preventing early failure of the implant system, including fracture, screw loosening, and increased leakage, in addition to reducing stresses at the implant–abutment interface. In the current work, three-dimensional (3D) models of mechanically connected Ti6-Al-4V implant systems in various dimensions were constructed. Finite element analysis (FEA) was used to conduct a stress study of the created implants under actual acting force static loading conditions in accordance with ISO 14801. In the created models, design elements including implant screw type, thickness, and taper angle of abutment were modified in order to increase the longevity of the implants. The results show that the equivalent stress level was dramatically reduced from 596.22 MPa to 212.72 MPa in the implant model, which exhibits a more homogeneous stress pattern under static loading conditions. By increasing the implant wall thickness from 0.15 mm to 0.40 mm in the region adjacent to the abutment, the stress levels, especially at the internal screw, were significantly reduced. Also, the design modification in Model B, establishing contact between the abutment and the upper part of the conical surface of the implant, resulted in a decrease in stress in the internal screw. Thus, enhanced homogeneity in stress distribution not only improves the harmony between the implant and surrounding tissues, thus increasing patient comfort and reducing the risk of complications, but also holds promise for the development of new implants capable of withstanding the forces encountered in the oral environment due to the relatively smoother stress transmission observed in this model.

1. Introduction

For long-term and secure utilization of dental implants, it is essential to recognize that factors contributing to damage in implant technology emerge from both biological and mechanical aspects [1,2,3]. In addition to damage caused by biological factors, mechanical factors, such as excessive forces, improper occlusion, or suboptimal implant design, can result in mechanical damage, which may involve component fractures, implant loosening, or implant breakage [4,5]. Apart from biological factors, mechanical damage in the long-term use of dental implants can be minimized through an optimized design that reduces stress distribution. It is known that the fracture of implant components is directly associated with the concentration of stress around the implant system when subjected to repeated masticatory forces. Stress concentration arises at implant cross-sectional changes or geometric irregularities, reducing implant system resistance to fatigue fractures and leading to biomechanical implant failure. The stress distribution around an implant depends on various biomechanical factors, including design, load type, material properties, surface roughness, bone quality, and implant–bone interaction. Excessive loading can lead to direct stress transmission from the implant to the bone, causing destructive damage in the bone tissues [6,7,8]. Therefore, the longevity of dental implants is significantly influenced by the implant material and its geometry, as well as the optimization of biomechanical factors to ensure smooth stress transmission from the implant to the bone, which is crucial for long-term success.

Titanium alloys are widely prevalent and crucial in the construction of dental implants [9,10]. Among titanium alloys, Ti-6Al-4V alloy is preferentially chosen for dental implant construction due to its excellent biocompatibility, corrosion resistance, mechanical strength, and ability to osseointegrate with bone tissue, making it an ideal material for long-lasting and successful dental implant applications. Additionally, in light of the growing demand for customized dental implants, the meticulous design and subsequent FEA of patient-specific implants prior to fabrication have gained paramount importance [11,12]. In contrast to mechanical loading, which provides information about when and where damage occurs, FEA is a particularly effective analysis method for ensuring the safe operation of a system [13,14]. This is because it reveals the magnitude and distribution of the internal stresses developed within a structural composition, especially highlighting vulnerable areas to damage.

In addition, FEA is a powerful approach to simulate various parameters in a design model, allowing the investigation of their potential relevance in clinical implementation. It is also a mathematical tool for estimating the stresses in the vicinity of the implant and components within implant-supported frameworks. Moreover, based on the FEA study, optimizing implant design in conjunction with specific implant–abutment connections proved crucial in preventing overload situations and the resulting clinical complications [15]. Recently, finite element method (FEM) studies have explored the enhanced biomechanical performance of novel materials as potential alternatives to titanium in implant materials. Furthermore, the significant influence of material properties, including elastic modulus, anisotropy, surface properties, and bioactivity on stress values and distribution, was highlighted by FEM analysis results. The importance of supporting the material’s long-term functional stability through extensive clinical studies was emphasized [16,17].

While dynamic loading tests are more representative of real-world conditions, static loading remains a crucial component of materials testing. It offers a controlled and simplified environment for understanding fundamental material properties, and this understanding is vital when interpreting the more complex results obtained under dynamic loading conditions. It is widely acknowledged that static load testing demonstrates the fracture strength or bearing capacity of the implant, whereas fatigue life assessment reflects its mechanical resilience.

The earlier FEM study indicated the implant’s consistent durability, maintaining resilience under both static and dynamic loading conditions. The observed maximum stress values remained below the yield strength of the implant–abutment joint system [18]. However, an in vitro study and an FEA analysis revealed that implant lengths and loading angles strongly influenced the static strength and fatigue strength of dental implants under static and dynamic loading conditions [19]. Specifically, modifications in implant and abutment design surface as crucial factors impacting the success and durability of dental implant treatments. Optimizing the implant–abutment connection is crucial for stress distribution and preventing mechanical complications, including abutment and screw fractures, screw loosening, and increased leakage at the implant–abutment interface [16].

These modifications, strategically aimed at improving compatibility and resilience, prove essential for achieving long-term success. The importance lies in the improved harmony with surrounding tissues, a critical factor for treatment success and the sustained durability of implants. Furthermore, these design adjustments serve to mitigate the risk of complications, highlighting the importance of precise design considerations, such as optimal abutment selection and tapered angle optimization, in minimizing stress on surrounding tissues. Static analysis is undertaken with the objective of predicting a model’s response to a range of loading conditions, irrespective of time considerations. Thus, the present study focuses on investigating the behavior of dental implant models under static loading conditions.

The implant, abutment, and screw together form a mechanical structure of dental implants. In some studies, only a part of the dental implant system, especially the implant part, has been examined [20,21,22]. In this study, the stress and strain values of the complete implant system, including the implant, screw, and abutment, under specific load were examined. Two types of Ti-6Al-4V implants were developed, and their design parameters were optimized to enhance fracture resistance and prolong the service life of Ti-6Al-4V implants under 100 N static loading conditions, as commonly available in the literature [2,8,23]. The investigation also provided insight into the rationale behind these design changes, emphasizing their crucial role in the overall success of dental implant therapy. Additionally, the study demonstrates the practical application of FEM static loading analysis, underscoring its significance in assessing and refining design modifications for optimal treatment outcomes. This emphasis on analysis stems from the recognition that any deformations in the implant, screw, and abutment can adversely affect the operational efficacy of the dental implant system in real-world scenarios.

2. Materials and Methods

In this study, a CAD software package (Ansys Spaceclaim 2022 R2) was utilized to create 3D models of internally connected multi-part implant systems consisting of implants and abutments in various dimensions, as shown in Figure 1. The models were assumed to have linearly elastic, homogeneous, and isotropic materials, with their corresponding mechanical properties detailed in

Table 1. Materials and mechanical properties [15].

Material	Young’s Modulus (GPa)	Poisson’s Ratio	Yield Stress (MPa)
Ti-6Al-4V (ASTM Grade 5) (Alpha-Beta, Annealed condition)	113.8	0.342	880

.

As illustrated in Figure 2, two distinct implant models were created by altering both the implant diameter and the abutment diameter.

An implant diameter of 3.25 mm and abutment diameter of 3.8 mm were used in this study. The designs were created by combining distinct dimensions provided in Figure 3 in a physically suitable manner, resulting in the acquisition of two combinations of implant designs.

To comply with the stipulations of the adopted standard (ISO 14801), depicted in Figure 3, the implant systems must be secured in a stable clamping holder, commonly chosen as a steel block. Alternatively, before fixation, they may be embedded in an implant holder characterized by a modulus of elasticity exceeding 3 GPa, in line with the materials recommended in the literature [23]. Lastly, once the fixation procedure is established, the abutment, which is screwed onto the implant, is subjected to a 30° oblique force, as recommended by the relevant standard. In this investigation, the implants, abutments, and rectangular prism-shaped implant holders were assembled using the CAD software. Subsequently, the assembly was exported to ANSYS Workbench 2022 R2 (ANSYS, Inc., Canonsburg, PA, USA). The FEA technique provides dentists with various biomechanical properties, including stress transfer from implant to surrounding bone, micromotions, deformations of the implant system and bone tissue under different biting forces, effects of load types and magnitudes on the implant system, and influences of implant design parameters on stress transmission. Additionally, FEA allows for the determination of these biomechanical properties for any uniquely designed dental implant tailored to an individual.

The design differences between Model A and Model B are shown in Figure 3. The implants have a length of 16.0 mm (Model A) and 14.0 mm (Model B), featuring a non-threaded cylindrical neck with a height of 2.0 mm (Model A) to 1.5 mm (Model B) and a threaded part with a height of 14.0 mm (Model A) to 12.00 mm (Model B). In the implant tooth geometries indicated with the number 3, the screw pitch is increased in Model B in comparison to Model A. In region 4, the abutment conical connection has been strengthened, and the wall thickness has been increased. The wall thickness of the implant in the area near the abutment increases from the minimum value of 0.15 mm to 0.40 mm by changing the taper angle and shape of the abutment and implant. This change can be seen in the area indicated by the number 4 in Figure 3. In region 5, the screw length extends, and the thread diameter increases from 1.3 mm to 1.45 mm.

For this purpose, based on various studies considering a 100 N load within the range of normal bite forces, this study applied a 100 N load to the top surface of each design in both axial and 30° oblique directions using the finite element method, in accordance with ISO 14801. To create meshes with tetrahedral solid elements, geometries were imported into the finite element software package Ansys Workbench 2022 R2. The total number of nodes and elements of each model is shown in

Table 2. The number of nodes and elements used in models for FEM simulation.

Model A		Model B
Nodes	Elements	Nodes	Elements
55,026	31,210	55,194	31,654

.

Analyses were applied to determine the optimum number of nodes and elements in the created network structure. A change in the number of nodes of the strain was observed in the entire model created. The starting point of the horizontal course of the curve gives the optimal number of nodes [18]. The 3D models were assembled using a meshing software package, as shown in Figure 4 [24]. Mesh models are also known as finite element models consisting of nodes and element data. The accuracy of the finite element solution is directly proportional to the number of nodes and elements. Because the structure was complex, it was not possible to apply hexamesh; then, a tetrahedral mesh was used [19]. The mesh was created with 55,026 nodes and 31,210 elements for Model A and 55,194 nodes and 31,654 elements for Model B.

Isotropic and linear elastic properties were used as the element structure. Moreover, the strain results, serving as a suitable convergence analysis criterion in the FEA model, were brought to convergence tolerance 1 × 10⁻⁸ to align with potential real-world applications. As a result, the required mesh resolutions were achieved through multiple refinement processes for all models, as shown in Figure 4.

The types of elements used in the ANSYS software package are given in Figure 5, Figure 6 and Figure 7. While the finite element model is formed, Shell181 (linear shape function) with middle nodes closed, Solid186 element, Solid187 element, and B Shell181 are degree (linear) types of the elements that must be at the point of translation and rotation in x, y, and z axis with 4 nodes and 6 degrees of freedom in each node point (Figure 5). Also, SHELL181 is a versatile element used for analyzing thin to moderately thick shell structures. It is effective for linear, large rotation, and/or large-strain nonlinear applications, including layered applications like composite shells or sandwich construction [24].

Solid186 is a type of an element in which each node at the point of the x, y, z axes as displacement and rotation has 6 degrees of freedom, showing a 20-node point, and is of second-order type (quadratic) (Figure 6). This element supports various deformations such as plasticity, hyperelasticity, creep, stress stiffening, large deflection, and large strain. It also incorporates a mixed formulation to simulate deformations in nearly incompressible elastoplastic and fully incompressible hyperelastic materials [24].

SOLID187 is a 3D 10-node element with quadratic displacement behavior, designed for modeling irregular meshes, especially those generated from various CAD/CAM systems (Figure 7). SOLID187 offers versatility with plasticity, hyperelasticity, creep, stress stiffening, large deflection, and extensive strain capabilities. It also incorporates a mixed formulation for simulating deformations in nearly incompressible elastoplastic and fully incompressible hyperelastic materials [24].

The stress results in each analysis is presented in von Mises equivalent stresses, representing the comprehensive stress state at a given point. This enables accurate determination of critical stress concentration regions in the models subjected to the respective loads. Figure 8 provides a concise representation of the FEA conditions, illustrating loading conditions in accordance with the relevant standard. Components 2, 3, and 5 depicted in Figure 3 represent the implant, made of titanium, while parts 1, 4, and 6 are identified as steel materials. Furthermore, the position of the intersection (C) between the loading axis (Line AB) and the axis of the endosseous dental implant (Line DE) is precisely defined, allowing the measurement or calculation of the moment arm (y) [23].

The loading geometry and apparatus, designed in accordance with the EN-ISO 14801 standard, are illustrated in Figure 8a, while the simulation setup is depicted in Figure 8b.

3. Results and Discussion

3.1. Stress Analysis

Similarly to previous studies [1], the highest von Mises stress values in this work were identified at the first and second threads near the implant heads (see Figure 9). Consequently, the performance of implant systems (implant and abutment) was assessed based on stress concentrations in these threads. The von Mises stress results of implants were categorized by their diameters, assuming that the implant diameter is a crucial factor in the design process for ensuring smooth stress transmission. Smooth stress transition is crucial for implants to meet patients’ treatment expectations and align with bone tissue for load resistance. Achieving this requires meticulous design, fostering improved physical surface interaction between the bone and the implant for optimal stress distribution within physiological limits. Based on the findings, there is a tendency for von Mises stresses to decrease with an increase in taper angles. Furthermore, an increase in taper angle led to higher values of wall thickness. The distribution of stress on various surfaces is illustrated by the von Mises stress (Figure 9), indicating which areas were more prone to stress. The highest von Mises stresses are observed on the second thread of the implants in Model A. As a result of the finite element analyses, the maximum equivalent stresses are found to be 596.22 MPa and 212.71 MPa, respectively. It is evident that Model B demonstrates reduced von Mises values in contrast to Model A, with stress distribution across a broader area.

The internal screw seems to be less impacted by mechanical stresses. This result in Model B aligns with material properties, because the obtained stress value is significantly below the yield strength of Ti-6Al-4V (Grade 5, Annealed), which is approximately 880 MPa. Consequently, modifications were implemented for the implant, abutment, and screw depicted in Figure 2 for Model B. This led to a notable reduction in the maximum equivalent stress value in Model B to 212.71 MPa, signifying a substantial enhancement in the implant’s durability. In a finite element analysis of the mechanical failure of implants, it was reported that implant diameter and wall thickness are influential parameters in stress reduction [25]. In addition, changes in implant length and loading angle directly affect both the static strength and fatigue strength of the dental implant [26].

The decrease in the conical angle in the abutment conical area increases the wall thickness, which causes a decrease in the stress values, and the stress values decrease with the increase in the implant diameter. In addition, increasing the spacing and decreasing the taper angle of the implant screw threads reduces the stress. Accordingly, the minimum diameter of the connection screw was increased from 1.3 mm to 1.45 mm and this change significantly reduced stress. This implies that the reduction in stress improves the implant’s capacity to withstand bending and torsional loads, thereby preventing premature failure. Similarly to the findings of Satyanarayana et al. [20], the choice of abutment type was identified to significantly influence stress distribution. This is attributed to variations in load transfer mechanisms and differences in the contact area size between the abutment and the implant. According to the studies of Jeng et al., the increase in wall thickness provides a significant stress reduction in the implant, abutment, and screw [26]. It was attributed to the increase in wall thickness from 0.15 mm to 0.40 mm, being an important factor in reducing the stress. The significant reduction in equivalent stress levels enhances the material resilience of the implant, positively influencing overall treatment success. Specifically, the development of new implants capable of withstanding the forces encountered in the oral environment was suggested by Model B, owing to the relatively smoother stress transmission observed in this model.

Further finite element analyses were conducted on Model A and Model B as the oblique loads gradually increased until reaching the maximum critical load, initiating implant yielding. As indicated in Figure 10, the yield stress was reached at load values of 147 N for Model A and 410 N for Model B. Based on the obtained von Mises equivalent stress under static loading conditions, it was found that the implants undergo no plastic deformations up to these critical loads in the tested models.

3.2. Strain Analysis

The finite element analysis (FEA) obtained strain intervals within the elasticity of the modeled materials. The elastic equivalent strains are shown in Figure 11. The convergence criterion was set to less than 1% in the changes in the total deformation energy of all the elements [11]. The decrease in elastic equivalent strain indicates that the Model B implant undergoes less deformation than the Model A implant. In alignment with the research conducted by Darvish et al. [16], the present study similarly observed a reduction in strain corresponding to a decrease in stress. According to the literature, the minimum and maximum equivalent elastic strain amounts should fall within the range of 0.0015 to 0.0030 to create an optimal environment for bone growth without the risk of fracture [6]. The calculated strain value of 0.0029482 in Model B satisfies this condition, as indicated in

Table 3. Equivalent elastic strain results from the finite element simulation on the designed implant models.

	Model A	Model B
Maximum equivalent stress (MPa)	596.22	212.71
Maximum equivalent elastic strain (mm/mm)	0.0080867	0.0029482

. This implies that the reduction in strain values observed in Model B could contribute to minimizing the risk of complications, such as fractures or failures, and potentially ensure the long-term success of dental implant treatments.

4. Conclusions

The objective of this study was to identify essential design parameters for achieving an implant model with high fracture resistance and long-term stability. To fulfill this objective, diverse Ti-6Al-4V implant models of varying dimensions were created, and their stress–strain analyses were executed under common bite force (100 N) in accordance with ISO 14801. The findings and implications of this research can be summarized as follows:

-

Model B of the Ti-6Al-4V implant, characterized by a 3.25 mm diameter, 3.80 mm abutment diameter, and 11.4° taper angle, exhibited minimal stress concentration.

-

In comparison to Model A, Model B demonstrated a decrease in von Mises stress values of over 60% under a biting force of 100 N, measuring 212.71 MPa.

-

By increasing the implant wall thickness from 0.15 mm to 0.40 mm in the region adjacent to the abutment, the stress levels, especially at the internal screw, were significantly reduced.

-

Optimizing the implant design, particularly by increasing the implant wall thickness from 0.15 mm to 0.40 mm in the region adjacent to the abutment, was found to be highly effective in mitigating the stress distribution, especially at the internal screw.

-

Under static loading, the critical loads, where no yielding or fracture occurred for the designed Model A and B, were found to be 147 N and 410 N, respectively.

-

In Model B design, elastic strain decreased by about 63%, enhancing practicality and aligning with real-world applications, as verified through FEA model convergence analysis.

It is planned to perform dynamic analyses in Model B in the continuation of this study. A comparison will be made with existing implants. The dental implant developed in Model B will be produced. Prior to conducting physical in vitro tests, certain limitations should be acknowledged for the present study. It is crucial to note that the materials, including implants, abutments, screws, etc., were assumed to be ideal, free of structural defects, and with ideal contact surfaces. However, it is important to recognize that this assumption may not perfectly reflect the real-world scenario for every restoration. The finite element simulation results will be validated with these results. In order to apply the results in the newly developed Model B, the necessary tests will be carried out according to two standards, i.e., ISO/TS 13498:2011 (Torsion test of implant body/connecting part joints of endosseous dental implant systems, 2011) and ISO/TR 18130:2016 (Screw loosening test using cyclic torsional loading for implant body/implant abutment connection of endosseous dental implants, 2016). The results will be compared with other models.