# Finite Element Analysis of the Effect of Tightening Torque on the Connection Stability of a Two-Piece Zirconia Implant System

Authors: Hyunsuk Choi; Min-Ho Hong
Journal: Advances in Materials Science and Engineering
 (2022)

---

## Abstract

Purpose. Loosening and fracture of abutment screws are one of the most common complications in implant-retained fixed prostheses. Thus, applying the proper tightening torque to the abutment screw is important for preventing the loosening effect of the abutment screw and ensuring the stability of the implant fixture-abutment connection. Therefore, in this study, we aimed to investigate the effect of the tightening torque of the abutment screw on the stability of the fixture-abutment connection in a two-piece zirconia implant system using finite element analysis (FEA). Materials and Methods. The two-piece zirconia implant structures used in this study were designed using the CATIA program. The abutment screws with tightening torques of 25 (TT-25), 35 (TT-35), and 45 (TT-45) N·cm were assumed to fix the abutment and fixture. Vertical (200 N) and oblique (100 N) loads were applied to the finite element model generated for FEA simulation, and the stress levels and distributions were investigated. Results. The TT-45 group exhibited the highest von Mises stress in the abutment and fixture, followed by the TT-35 and TT-25 groups. The von Mises and minimal principal stresses of the abutment screw were also highest in the TT-45 group, followed by the TT-35 and TT-25 groups. In all three groups, the area with the highest stress concentration was located at the point of contact with the bottom of the screw head. Furthermore, the TT-25 group showed the highest safety factor value. The TT-35 group showed a safety factor value similar to the safe minimum standard, while the TT-45 group showed a lower safety factor value. Conclusion. When a torque of 35 N cm was applied to the two-piece zirconia implant system, it showed a maximum stress value close to 660 MPa (75% of the yield strength of the Ti-6Al-4V alloy), which is the optimal preload recommended for abutment screws.


---

## Body

## 1. Introduction

Since a long time, various materials have been introduced for use in implants [1]. Zirconia is presently a widely used material owing to several advantages, including excellent biocompatibility, mechanical properties, and aesthetics, making it a good alternative to titanium [2]. The zirconia used in dentistry is an yttria-stabilized tetragonal polycrystal (Y-TZP), a tetragonal single phase stabilized by adding Y203, which has excellent physical properties such as fracture toughness, flexural strength, and hardness [3]. When external stress is applied to the zirconia and a crack develops, a phase transition from tetragonal to monoclinic occurs and a part of the fracture energy is absorbed. Because of the 3%–5% volume expansion that occurs during phase transition, a compressive stress layer is created at the crack site to suppress crack propagation [4]. Moreover, the excellent biocompatibility of zirconia has been reported in previous animal studies or retrospective studies [4–8].Zirconia implants can be classified into one- and two-piece implants [9]. Most of the early studies on zirconia implants were limited to one-piece implants because implementing the connection of the zirconia component and the abutment screw at the interface between the implant fixture and abutment was technically difficult [10]. Early studies on zirconia implants were limited to the one-piece type because of technical difficulties in implementing a screw-type connection at the implant fixture-abutment interface [10]. Moreover, there are several limitations to the use of one-piece zirconia implants in clinical situations. First, depending on the angle at which the implant is placed, the flexibility for fabricating a prosthetic restoration is insufficient. In addition, because it is one-piece, there is a disadvantage that stable osseointegration of the implant cannot be achieved through two-stage implant surgery if initial fixation is insufficient after implant placement [11]. By contrast, in two-piece zirconia implants, the unfavorable implant angle and position can be compensated through abutment, and two-stage implant surgery is also possible.A high success rate in short-term follow-up studies of two-piece zirconia implants has been reported [12, 13]. Despite the physical properties of two-piece zirconia implants being widely reported, there is a distinct lack of data derived from in vivo studies. In this situation, assessing the biomechanical properties of implant components is possible through finite element analysis (FEA), which is the previous stage of the in vivo experiment [14]. In FEA, stress and displacement of complex implant structures can be analyzed under controlled conditions through simulation.Loosening and fracture of the abutment screw are the most common complications in implant-retained fixed prostheses [15]. Abutment screw loosening occurs because of the following reasons: plastic deformation caused by an external load, insufficient tightening torque of the abutment screw, loss of preload, settling effect of the surface, and vibration occurring during mastication [16]. Preload is generated by applying a tightening torque when tightening the abutment screw; it affects the maintenance and stabilization of the implant system by firmly connecting the abutment screw and implant fixture [17]. This preload is lost when the external load is repeatedly and continuously applied to the abutment screw [15]. The resulting decrease in tension of the abutment screw is called the loosening effect [17].Abutment screw loosening generally follows a two-stage mechanism [18]. In the first stage, repeated loads are applied to the abutment screw, causing erosion at the connection part, and friction between the internal threads of the implant and the abutment screw results in loss of preload [19]. In the second stage, the preload decreases to a constant value and loosening begins as a rotational force is generated in the abutment screw due to external load and vibration [19]. Therefore, applying the proper tightening torque to the abutment screw is important for preventing the loosening effect of the abutment screw and ensuring the stability of the implant fixture-abutment connection. Previous studies have reported that the optimal tightening torque of the abutment screw should be approximately 75% of its yield strength to prevent abutment screw loosening [20].Recently, a study analyzed the biomechanical properties of a two-piece zirconia implant system using FEA [21]. However, studies on the effect of the tightening torque of the abutment screw in a two-piece zirconia implant system are lacking. Therefore, in this study, we aimed to investigate the effect of different tightening torques of the abutment screw on the stability of the fixture-abutment connection in a two-piece zirconia implant system using FEA. The null hypothesis was that an increase in tightening torque in the abutment screw would have only a minor influence on stress levels and distributions in the two-piece zirconia implant system under an external load.


## 2. Materials and Methods

### 2.1. FEA Modeling

Through three-dimensional (3D) point cloud data extraction, the mandibular right first molar-shaped 3D model was fabricated through reverse engineering (Figure1). The two-piece zirconia implant components employed in this study were designed using the CATIA program (Dassault Systemes, Vélizy-Villacoublay, France). Furthermore, the implant fixture used in this study was an internal hex connection implant (Anyone® Internal; Megagen, Daegu, Korea) with a diameter and length of 5.0 and 11.5 mm, respectively. A prefabricated milling abutment (Milling abutment, Megagen, Daegu, Korea) with a length and diameter of 4.5 mm and a Ø 1.8 × 8.5-mm abutment screw was used. The screw thread was positioned 5.1 mm from the head of the abutment screw. Through the cross-sectional imaging of the molar region of the human mandible, a bone block model that was 29.5-mm high and 14-mm wide was also fabricated; it comprised a spongy center surrounded by a 1.4–3.7mm thick cortical bone. The implant was then placed in the bone block. The finite element (FE) model was created and discretized in HyperMesh (Altair HyperMesh v17.0; Altair Engineering Troy, MI, USA) using the exact dimensions and material properties of the original structured implant systems and load conditions. In this study, the mesh convergence test created a mesh using the minimum number of elements at a reasonable level and performed finite element analysis. In previous studies, the results were found to be inappropriate when the element size was larger than 300 μm [21]. However, an element size of 150 μm or less extends the time required for analysis. Therefore, in this study, the average element size was set to 250 μm [21]. In the FE models created in this study, the cement thickness between the implant components was ignored.Figure 1
Finite element models of implant components and bone block (element numbers: abutment: 4732; screw: 6193; fixture: 21,419; cortical bone: 75,530; and cancellous bone: 85,114).In the present study, 10 nodes of quadratic tetrahedral elements with an average size of 0.25 mm were used in the models. The nodes, elements, and mesh sizes of the FE models are given in Table1. Specific software (Abaqus FEA v6.12; Dassault Systems Simulia Corp) was used to simulate the masticatory movement in each group. In each model, the materials were assumed to have homogeneity, isotropy, and linear elasticity to simplify the model and numerical calculation in FEA. In addition, the implant was assumed to be fully osseointegrated. The elastic modulus and Poisson’s ratio of implant components used in this study were based on the physical properties used in previous studies [22–24].Table 1
Nodes, elements, and mesh size of the FE models.
ComponentsNodesElementsMesh size (μm)Zirconia crown12,80958,892250Abutment55,93123,534Fixture96,05123,534Abutment screw12,06458,163Cortical bone60,134280,089Cancellous bone50,931247,142


### 2.2. Load Application and Preload Calculation

The material properties of the implant components and bone used in previous studies are given in Table2 [25, 26]. The implant was assumed to be completely osseointegrated to the bone, and the implant components were constrained in all directions (X, Y, and Z) on the implant surface. Table 3 lists the contact type (bonded and frictional) to describe the integration quality among the abutment, fixture, abutment screw interface and fixture, cortical bone, and cancellous bone. The friction coefficient was 0.3.Table 2
Mechanical properties of all simulated materials.
MaterialElastic modulus (GPa)Yield strength (MPa)Poisson’s ratioZirconia abutment/fixture210—0.30Abutment screw (Ti-6Al-4V)1108800.35Zirconia crown210—0.26Cortical bone13.7—0.30Trabecular bone1.37—0.30Table 3
Summary of the contacts between all components.
ComponentAbutmentScrewFixtureCortical boneCancellous boneAbutment—FrictionalFrictional——Screw——Frictional——Fixture———FrictionalFrictionalCortical bone————BondedThe suggested tightening torque follows the description and evaluation using a simplified method as described ahead. The equation for the screw-tightening torque is as follows:(1)T=K×D×F,where T is the screw-tightening torque (N·cm), D is the screw diameter (m), F is the screw preload (N), and K is the screw factor (or torque coefficient), which usually has a value of 0.2 [14]. By using equation (1), the screw preload value when a tightening torque is applied to the abutment screw can be calculated. Thus, when the tightening-torque value was 25 N cm, the F value of the screw preload was 418 N, and when the tightening-torque value was 35 and 45 N cm, it was 558 and 751 N, respectively (Figure 2).Figure 2
Boundary and loading conditions. (a) Screw preloading with the bone block fixed along all the axes; the yellow arrows indicate the preloading required to achieve a tightening torque of 25, 35, and 45 N cm. (b) External loading: 200 N vertically (at each of the 60 nodes on three pits) and 100 N obliquely (at each of the 30 nodes on three cusps).
(a)(b)In this study, when a tightening torque was applied to the abutment screw, the abutment and the implant were assumed to be fixed, and the tightening torque was classified into three groups, namely, 25 (TT-25), 35 (TT-35), and 45 (TT-45) N·cm, respectively. To simulate masticatory movement, vertical and oblique loads of 200 and 100 N, respectively, were applied to the three cusps of the mandibular molar (Figure2). The oblique load was set at 30° inclination to the long axis of the fixture [27].


### 2.3. Fatigue Analysis

For a long-term successful prognosis, the implant should satisfy the maximum or infinite fatigue life. As a method of evaluation, physical testing or fatigue analysis can be performed. In this study, the following equations were used to predict the fatigue life of the implants through FE modeling.(2)σa=Δσ2=σmax−σmin2,(3)σm=σmax+σmin2,(4)σaσe+σmσu=1n.Goodman’s theory of fatigue life can be defined usingσm (mean stress) and σa (stress amplitude). σe denotes the fatigue limit, σu represents the maximum tensile strength, and n denotes the safety factor. Considering that the fatigue cycle of Ti-6Al-4V is 107, the safety factor (SF) can be calculated by substituting 510 MPa as the fatigue limit in the above equation [28].


## 2.1. FEA Modeling

Through three-dimensional (3D) point cloud data extraction, the mandibular right first molar-shaped 3D model was fabricated through reverse engineering (Figure1). The two-piece zirconia implant components employed in this study were designed using the CATIA program (Dassault Systemes, Vélizy-Villacoublay, France). Furthermore, the implant fixture used in this study was an internal hex connection implant (Anyone® Internal; Megagen, Daegu, Korea) with a diameter and length of 5.0 and 11.5 mm, respectively. A prefabricated milling abutment (Milling abutment, Megagen, Daegu, Korea) with a length and diameter of 4.5 mm and a Ø 1.8 × 8.5-mm abutment screw was used. The screw thread was positioned 5.1 mm from the head of the abutment screw. Through the cross-sectional imaging of the molar region of the human mandible, a bone block model that was 29.5-mm high and 14-mm wide was also fabricated; it comprised a spongy center surrounded by a 1.4–3.7mm thick cortical bone. The implant was then placed in the bone block. The finite element (FE) model was created and discretized in HyperMesh (Altair HyperMesh v17.0; Altair Engineering Troy, MI, USA) using the exact dimensions and material properties of the original structured implant systems and load conditions. In this study, the mesh convergence test created a mesh using the minimum number of elements at a reasonable level and performed finite element analysis. In previous studies, the results were found to be inappropriate when the element size was larger than 300 μm [21]. However, an element size of 150 μm or less extends the time required for analysis. Therefore, in this study, the average element size was set to 250 μm [21]. In the FE models created in this study, the cement thickness between the implant components was ignored.Figure 1
Finite element models of implant components and bone block (element numbers: abutment: 4732; screw: 6193; fixture: 21,419; cortical bone: 75,530; and cancellous bone: 85,114).In the present study, 10 nodes of quadratic tetrahedral elements with an average size of 0.25 mm were used in the models. The nodes, elements, and mesh sizes of the FE models are given in Table1. Specific software (Abaqus FEA v6.12; Dassault Systems Simulia Corp) was used to simulate the masticatory movement in each group. In each model, the materials were assumed to have homogeneity, isotropy, and linear elasticity to simplify the model and numerical calculation in FEA. In addition, the implant was assumed to be fully osseointegrated. The elastic modulus and Poisson’s ratio of implant components used in this study were based on the physical properties used in previous studies [22–24].Table 1
Nodes, elements, and mesh size of the FE models.
ComponentsNodesElementsMesh size (μm)Zirconia crown12,80958,892250Abutment55,93123,534Fixture96,05123,534Abutment screw12,06458,163Cortical bone60,134280,089Cancellous bone50,931247,142


## 2.2. Load Application and Preload Calculation

The material properties of the implant components and bone used in previous studies are given in Table2 [25, 26]. The implant was assumed to be completely osseointegrated to the bone, and the implant components were constrained in all directions (X, Y, and Z) on the implant surface. Table 3 lists the contact type (bonded and frictional) to describe the integration quality among the abutment, fixture, abutment screw interface and fixture, cortical bone, and cancellous bone. The friction coefficient was 0.3.Table 2
Mechanical properties of all simulated materials.
MaterialElastic modulus (GPa)Yield strength (MPa)Poisson’s ratioZirconia abutment/fixture210—0.30Abutment screw (Ti-6Al-4V)1108800.35Zirconia crown210—0.26Cortical bone13.7—0.30Trabecular bone1.37—0.30Table 3
Summary of the contacts between all components.
ComponentAbutmentScrewFixtureCortical boneCancellous boneAbutment—FrictionalFrictional——Screw——Frictional——Fixture———FrictionalFrictionalCortical bone————BondedThe suggested tightening torque follows the description and evaluation using a simplified method as described ahead. The equation for the screw-tightening torque is as follows:(1)T=K×D×F,where T is the screw-tightening torque (N·cm), D is the screw diameter (m), F is the screw preload (N), and K is the screw factor (or torque coefficient), which usually has a value of 0.2 [14]. By using equation (1), the screw preload value when a tightening torque is applied to the abutment screw can be calculated. Thus, when the tightening-torque value was 25 N cm, the F value of the screw preload was 418 N, and when the tightening-torque value was 35 and 45 N cm, it was 558 and 751 N, respectively (Figure 2).Figure 2
Boundary and loading conditions. (a) Screw preloading with the bone block fixed along all the axes; the yellow arrows indicate the preloading required to achieve a tightening torque of 25, 35, and 45 N cm. (b) External loading: 200 N vertically (at each of the 60 nodes on three pits) and 100 N obliquely (at each of the 30 nodes on three cusps).
(a)(b)In this study, when a tightening torque was applied to the abutment screw, the abutment and the implant were assumed to be fixed, and the tightening torque was classified into three groups, namely, 25 (TT-25), 35 (TT-35), and 45 (TT-45) N·cm, respectively. To simulate masticatory movement, vertical and oblique loads of 200 and 100 N, respectively, were applied to the three cusps of the mandibular molar (Figure2). The oblique load was set at 30° inclination to the long axis of the fixture [27].


## 2.3. Fatigue Analysis

For a long-term successful prognosis, the implant should satisfy the maximum or infinite fatigue life. As a method of evaluation, physical testing or fatigue analysis can be performed. In this study, the following equations were used to predict the fatigue life of the implants through FE modeling.(2)σa=Δσ2=σmax−σmin2,(3)σm=σmax+σmin2,(4)σaσe+σmσu=1n.Goodman’s theory of fatigue life can be defined usingσm (mean stress) and σa (stress amplitude). σe denotes the fatigue limit, σu represents the maximum tensile strength, and n denotes the safety factor. Considering that the fatigue cycle of Ti-6Al-4V is 107, the safety factor (SF) can be calculated by substituting 510 MPa as the fatigue limit in the above equation [28].


## 3. Results

Figure3 shows the von Mises stress distribution in the abutment and fixture under different tightening-torque conditions. The TT-45 group exhibited the highest von Mises stress in the abutment and fixture, followed by the TT-35 and TT-25 groups. In the abutment, the stress concentration area was located at the point of contact with the bottom of the screw head.Figure 3
Von Mises stress distribution of the abutment and fixture under each tightening torque with the occlusal load.
(a)(b)Figure4 shows the von Mises and minimum principal stress distributions in the abutment screw under different tightening-torque conditions. Figure 4(a) shows the von Mises stress distribution in the abutment screw under different tightening-torque conditions after application of external loading. Overall, for all groups, the von Mises stress distribution was found to be the same as the result in Figure 3. Moreover, as the tightening torque increased, the von Mises stress was found to increase. In the TT-25 group, the von Mises stress value of the abutment screw was 300.7 MPa, which was lower by 65.8% compared to the yield strength of Ti-6Al-4V. In the TT-35 group, the von Mises stress value of the abutment screw was 639.3 MPa, which was lower by 27.4% compared to the yield strength of Ti-6Al-4V. Furthermore, in the TT-45 group, the von Mises stress value of the abutment screw was 896.7 MPa, which was higher by 1.9% compared to the yield strength of Ti-6Al-4V. Figure 4(b) shows the minimum principal stress distribution in the abutment screw under different tightening-torque conditions after application of external loading. In the TT-25 group, the minimum principal stress value of the abutment screw was 170.3 MPa. In the TT-35 group, the minimum principal stress value of the abutment screw was −270.9 MPa. Finally, in the TT-45 group, the minimum principal stress value of the abutment screw was −377.1 MPa.Figure 4
Von Mises and minimum principal stress distributions of implant components under external loading.
(a)(b)Figure5 shows the SF in each group under the application of external loading. The SF is usually calculated as the ratio of ultimate stress to design stress. Determining the safe minimum standard (SMS) as 1.5, the load generated on the structure was defined to reach the fracture limit. The TT-25 group showed the highest SF value, the TT-35 group exhibited an SF value similar to SMS, and the TT-45 group showed a lower SF value.Figure 5
Goodman safety factor value of the models in which the tightening torque and occlusal load of the abutment screw are applied.In the present study, as shown in Figures6 and 7, there were no significant differences in the stress values of each group in cortical and cancellous bones.Figure 6
Maximum and minimum principal stress distributions of the cortical bone.
(a)(b)Figure 7
Maximum and minimum principal stress distributions of the cancellous bone.
(a)(b)


## 4. Discussion

In this study, we investigated the effect of different tightening torques of the abutment screw on the stability of the fixture-abutment connection in a two-piece zirconia implant system using FEA. Accordingly, the stress levels in the implant components were found to increase when the tightening torque applied to the abutment screw increased under the external load. Therefore, the null hypothesis was rejected.When tightening the abutment screw, a tensile force is generated from the screw head in the direction of the screw thread, which is called abutment screw preload [28–30]. The abutment screw preload results in a clamping force due to compressive stress generated at the interface of implant components (abutment-abutment screw head, abutment-fixture, and abutment screw–internal thread of fixture) [16, 31].In three previous studies, the abutment screw preload was analyzed using FEA [16, 31, 32]. In one study, the screw preload was analyzed under the application of a contracting thermal load to screw joint components [32]. Another study simulated the clamping force generated by the elastic recovery of the fastened abutment screw [33]. Furthermore, a study analyzed the screw preload while maintaining the original dimension of the abutment screw by applying uniaxial thermal conditions to unthreaded screw shafts [16]. In the present study, the screw preload was calculated using equation (1).The abutment screw preload depends not only on the tightening torque but also on the friction coefficient at the contact interface of each implant component [34]. Under the same tightening-torque condition, the contact interface with a low friction coefficient exhibits a higher preload [35]. Factors affecting the friction coefficient at the interface of implant components are as follows: mechanical properties of the implant material, surface treatment method, and screw-tightening speed [36–38]. Therefore, in our study, the friction coefficient was selected as 0.2 based on the previous studies [14] and the effect of the friction coefficient on the preload was excluded.By tightening the screw, a tightening torque was applied as a moment of force (N·cm) to the abutment screw head in all groups. Then, the moment was transformed along the threaded surface of the abutment screw and fixture. The transformed force generates the contact force at the surface between the clamped abutment and fixture [35]. In addition, it can be confirmed that the compressive principal stress generated in all groups is transferred from the abutment screw to the abutment and the fixture (Figure 4(b)). Thus, the applied screw preload was properly reflected into the abutment screw of the FE model.For screw-type prostheses, the optimum preload of the abutment screw is important for the long-term prognosis of implant components. McGlumphy et al. reported that 75% of the yield strength of the abutment screw is its optimal torque value [31]. The abutment screw used in the present study was made of Grade 5 Ti-6Al-4V alloy with a yield strength of 880 MPa. Therefore, the optimum preload of the abutment screw was 660 MPa, which was 75% of the yield strength of 880 MPa. According to the result of stress distribution analysis by a torque of 25 N cm, application of a torque below this value could result in a minimal preload, which could cause screw loosening in the future. A loose screw may fracture over time and ultimately cause loss of the prosthesis [35]. By contrast, applying a torque of 45 N cm could exceed the proportional limit of the screw and cause it to deform irreversibly. This would initially reduce the preload and subject the screw to potential loosening but could also weaken the screw, leading to possible fracture [35]. However, when the tightening-torque value was 35 N cm, the maximum stress value was slightly lower than 75% of the yield strength of Ti-6Al-4V. Thus, within the experimental limits, the optimal torque was selected to be similar to or slightly higher than 35 N cm [39, 40].In studies using FEA, dynamic and static analyses of the implant components are essential for ensuring the safety of the experimental design. In most studies, the design of implant components is based on static analysis, which is mainly performed under the simulation where an external load is applied to the implant components. The results shown in Figure5 reveal that the SF of the Ti-6Al-4V material exceeds 1.0 (N = 107 cycles). Considering that the allowable SF on checking fatigue strength varies from 1.3 to 1.5, the SF calculated according to the maximum stress value at coupling components by simulation is approximately 1.5, which indicates sufficient strength. In the FEA of the present study, similar data were obtained for the SF [41]. To evaluate whether a dental implant is properly designed, it is subjected to standard fatigue tests under various loading conditions according to ISO 14801 [42]. However, the abovementioned tests are time-consuming and economically disadvantageous because the implant must be tested in a practical way until it is fractured. Therefore, in our study, Goodman’s theory was applied to predict the fatigue life of dental implants in a short period of time.Considering the limitation of the present study, the cement thickness between the implant components was ignored to simplify the FE models and focus on the stress concentrations in implant components. In addition, the model was designed as an approximation to the clinical situation. However, the study using FEA is influenced by various factors, such as physical properties of the material, boundary and loading conditions, interface definition, and approach to the mode. Therefore, the size quantification of the abutment and the preload analysis of dynamic loading are considered necessary for further study.


## 5. Conclusions

Within the limitations of this study, the following conclusions are drawn:(1)
When a torque of 35 N cm is applied to the two-piece zirconia implant system, it exhibits the maximum stress value closest to 660 MPa (75% of the yield strength of the Ti-6Al-4V alloy), which is the optimal preload recommended for abutment screws.(2)
Application of different torques to the abutment screw does not affect the von Mises and principal stress distributions of the cortical and cancellous bones.(3)
When applying the respective tightening torque in a two-piece zirconia implant system, the von Mises stress increases as the screw preload increases. The clamping force of the abutment appears to affect the implant abutment joint. Therefore, the two-piece zirconia implant system should observe an optimal tightening torque, which is considered by clinical functional loading.



---

*Source: 1456475-2022-10-21.xml*