This study analyzed stress and strain mediated by 2 different implant materials, titanium (Ti) and experimental fiber-reinforced composite (FRC), on the implant and on the bone tissue surrounding the implant. Three-dimensional finite element models constructed from a mandibular bone and an implant were subjected to a load of 50 N in vertical and horizontal directions. Postprocessing files allowed the calculation of stress and strain within the implant materials and stresses at the bone-to-implant interface (stress path). Maximum stress concentrations were located around the implant on the rim of the cortical bone in both implant materials; Ti and overall stresses decreased toward the Ti implant apex. In the FRC implant, a stress value of 0.6 to 2.0 MPa was detected not only on the screw threads but also on the implant surface between the threads. Clear differences were observed in the strain distribution between the materials. Based on the results, the vertical load stress range of the FRC implant was close to the stress level for optimal bone growth. Furthermore, the stress at the bone around the FRC implant was more evenly distributed than that with Ti implant.
Bone growth, remodeling, and adaptation are all believed to be partly regulated by the mechanical properties of the tissue. This phenomenon has been hypothesized to be driven by microscopic damage that stimulates bone adaptation to reconfigure optimal bone strength (Wolff's law). A significant modification of the bone's local stress and strain distribution is attained after reconstruction of occlusion with oral implants. The extent and nature of the remodeling process depends partly on the shape and rigidity of the occlusal scheme.
Fiber-reinforced composite (FRC) is a novel material with potential advantages for use in oral and craniofacial applications, as well as in orthopedics.1–3 Previous studies concerning the mechanical properties of FRC implants have shown good performance in the laboratory environment.4,5 Recently, in vitro and in vivo studies have shown that certain FRC material is biocompatible in the cell culture environment, and preosteoblasts have been shown to mature and proliferate well on the FRC substrates.6,7 However, the influence of occlusal loads on bone-remodeling phenomena around FRC implants has not been reported. The biomechanical connection between an FRC implant and bone under different loading conditions is not well known and is extremely difficult to measure in vivo. Three-dimensional (3D) computer modeling and subsequent finite element (FE) analysis make possible the simulation of biomechanical conditions involving an oral implant with different materials and directions of load.
The aim of this study was to analyze stress and strain mediated by 2 different implant materials on either the implant or on the bone tissue surrounding the implant. The secondary aim was to compare interfacial stresses between 2 different implant materials, titanium (Ti) and FRC, under 3 different directions of load.
Materials and Methods
Definition of structures and geometric conditions
A mandibular 3D FE bone model was created. A mandible of a 25-year-old man with missing premolar was captured from a dental computerized tomography (CT) system (3DX MCT-1 TYPE F, Morita, Tokyo, Japan). The mesiodistal dimension of tooth space was 8 mm, and the height of the mandible in the symphysis region was 30 mm. A mandibular simulation of the A-1-2–type bone structure (most of the alveolar ridge is present and a thin layer of cortical bone surrounds a core of dense trabecular bone of favorable strength), according to the classification by Lekholm and Zarb,8 was followed. The implant with a total length of 15 mm and a diameter of 4.1 mm was incorporated into the model. The implant was a cylindrical screw design with a rounded apical section (Figure 1). Two different implant materials, anisotropic continuous unidirectional E-glass FRC and isotropic Ti, were used. The FRC implant was composed of unidirectional long-axis E-glass fibers with pBisGMA-PMMA and resin (pBisGMA-pTEGDMA) screw threads, and the Ti implant was composed of commercial type 4 pure titanium. Each implant had an insertion length of 10 mm into the bone, while 5 mm remained as an abutment part above bone level. In all models, the implants were placed in the center of a mandibular crest and the middle of the mesiodistal plane. A prosthetic superstructure was not created. The coordinates of each point of the shape were then put into a preprocessor of an FE analysis program (ANSYS 11, ANSYS Inc, Houston, Tex) to build solid models for the mandibular bone and the implant.
Material properties used in this study were resin (Stick Resin, StickTech, Turku, Finland), commercially pure titanium (cp Ti), and cortical bone and cancellous bone as isotropic materials. The FRC (everStick, StickTech, Turku, Finland) was used as an anisotropic material. Most of the values describing the properties of the experimental materials (Table) were determined from the literature.9–12 Compared with Ti (isotropic material) and FRC (anisotropic material), the element situation was different for an orthotropic material. The engineering constants of a unidirectional continuous FRC can be predicted with various micro-mechanical models, starting from the properties of the matrix and fibers. A unidirectional continuous FRC is a special composite with a grade of isotropy in the plan transverse to the fiber direction (these materials are also referred as an anisotropic). Three Young's modulus, 3 Poisson's ratios, and 3 shear modulus are therefore independent and sufficient to describe the FRC mechanical behavior.9 Twenty-node brick element as solid 95 in ANSYS has the anisotropic material option. Anisotropic material directions correspond to the element coordinate directions. The element coordinate system orientation was altered to correspond with the fiber direction.
Mesh generation, boundary conditions, and data processing
To simulate the mechanical behavior of the mandible, total bonding between bone and implant (complete implant osseointegration) was assumed. To avoid quantitative differences in the stress value in the models, both solid models were derived from a single mapping mesh pattern that generated 140 280 elements (Solid 95 in ANSYS) and 197 170 nodes.
A load of 50 N was applied to the top of implants vertically and horizontally from the buccal direction. The 50-N load was assumed to be the normal masticatory force13,14 of an implant-supported prosthesis.15 The mandibular 3D FE bone model of mesial and distal surfaces was fixed in all directions. FE analysis was presumed to be linear static. FE model construction and FE analysis were performed on a PC workstation (Precision Work Station M90, Dell Inc, Round Rock, Tex). Stress and strain values were used to describe the biomechanical properties of bone and the bone-to-implant interface. Stress analysis was performed using Von Mises stress values,16 which summarize the effect of 6 stress components in a unique value. In the mathematical formula, considering the 3 principal stress components (σ1, σ2, and σ3), the von Mises stress value was defined as follows:
This approach is most amenable for interpreting FE analysis results.17 The von Mises stress values were measured at the implant-bone interfaces along the long axes of the loaded implants. Measurements were made at the lingual and buccal aspects of each implant. The stress was analyzed from the predetermined locations from the neck to the implant apex (stress path; Figure 2).
The stress and strain distributions between bone and implant surfaces are presented in Figures 3 through 6. In the figures, stress and strain are visualized by the pseudocolor of the geometrical model: the dark blue areas represent unstressed regions, while the red areas represent stressed regions. All color maps are compared with the same chromatic scale shown on the left side of the figures. Because of the symmetry of the analyzed systems, only half of the FE model is graphically represented.
Figure 3 shows the stress distribution and stress path of the FRC and the Ti implant under a 50-N vertical load. The FE analysis demonstrated an uneven stress distribution inside the bony socket around the loaded implants. The elements exposed to the maximum stress were located around the neck of the implant on the medial and distal rim of the cortical bone. This location was identical for both implant materials. However, in the cancellous bone, a stress value of 2.0–10 MPa was located on the top of screw threads of the Ti implant. In FRC, an implant stress value of 0.6–2.0 MPa was detected not only on the screw threads but also on the implant surface between the threads. A comparison of the stress path in bone with different materials showed distinct variances. The stress path showed an exponential regression curve, indicating a significant influence of the implant material on the stress distribution in the simulated bone. In cancellous bone, the Ti implant showed a high stress concentration at the screw threads, whereas the lowest stress was seen in the bone area between the screw threads. The FRC implant showed more even stress concentration in the bone around the implant body.
An uneven strain distribution was noted inside the bony socket around the loaded implants (Figure 4). Clear differences were observed in the strain distribution between materials. In the Ti implant, strain concentrations were located equally on the threads of the screw and on the bottom corner of the cancellous bone. However, the FRC implant showed more even strain concentrations within the cancellous bone. The area of high strain was not only reduced but also smaller at the top of the implant and higher at the bone area between the screw threads than that of Ti implant.
The FE analysis demonstrated uneven stress distribution inside the bony socket around horizontally loaded implants (Figure 5). The stress concentration occurred at the bone side of the interface between the implant and the upper cortical bone. In the Ti implant, maximum stress exceeding 16–20 MPa was detected in the bone around the neck of the implant, which peaked at a value of 18.6 MPa. In the FRC implant, maximum stresses exceeding 16–20 MPa were also located on the rim of the cortical bone around the neck of the implant, but the peak value reached 42.0 MPa. In cancellous bone, the Ti implant showed 0.3–0.6 MPa of stress at the apical part of the implant, whereas the lowest stress was seen in the bone around the mesial and distal sides of the Ti implant. However, an FRC implant stress value of 0.3–0.6 MPa was located at the upper half of the bony socket. A comparison of the stress path in bone with different materials showed similar variances. In the Ti implant, horizontal load did not affect the maximum stress values, whereas in the FRC implant, horizontal load elevated interfacial stresses 1.4 times. Maximum stress value was always highest at the crest of the cortical bone.
An uneven strain distribution was detected inside the bony socket around the horizontally loaded implants (Figure 6). In the Ti implant, strain concentrations were located equally around the neck of the implant on the cortical bone, on the top of the first screw thread on the cancellous bone and around the loading point. In the FRC implant, high strain areas were located equally in the cortical bone around the neck of the implant and within the neck part of the FRC implant. A comparison of the strain distribution showed that higher strain was detected in the cortical bone around the FRC implant than around the Ti implant. However, the FRC implant showed lower strain concentration in the cancellous bone.
A superstructure was not created in the FEM model because the aim of this study was to compare only the properties FRC and Ti implant materials under simulated loading conditions. If other variables would have been added, the simulated situation would have become too difficult to control. However, the stress in the jawbone predicted by a 2D model is less accurate than that predicted by its 3D counterpart,18 so a simple 3D model was selected to address the problem.
The fact that a biomechanical reaction differs for each patient means that it is impossible to model the percentage of osseointegration accurately. Many previous studies have evaluated either vertical or horizontal loads on implants assuming that 100% osseointegration was present.19,20 This implies that under any loading, the relative motion between bone and implant does not occur.21,22 A fixed bond between the bone and implant along the entire interface was therefore also assumed in our study.
Since FRC is a composite material of preimpregnated fiber embedded in a resin matrix, the analysis in this study was carried out from a macroscopic point of view.9 To demonstrate the intrinsic material properties of FRC, in addition to rectangular coordinate, a new local coordinate having a different point of origin was established.
The fact that maximum stress concentrations were located equally around the neck of the implant on the rim of the cortical bone in both implant materials and that overall stress decreased along the stress path toward the implant apex is in agreement with the results of previous studies.23–25 Nevertheless, none of these studies considered the influence of mandibular elastic deformation on the stress distribution along the implant. Stress concentration depends on the shape of the structure, which in our study was constructed to be the same for both implants. Only material properties were chosen to be different. Therefore, major differences in the stress concentration between the FRC and Ti implants were not observed. Maximum Von Mises stress value were different; however, the Ti implant showed 35% lower stress on the cortical bone around the neck of the implant compared with the FRC implant. In contrast, the stress was evenly distributed along the entire surface of the FRC implant, while stress was concentrated on the top of the screw threads in the Ti implant. This was due to the differing material properties of the implants.
Papavasiliou and coworkers26 investigated the implant-bone interfacial stresses of a Ti implant–supported fixed restoration and concluded that crestal osseointegration and axial loads minimized overall stress. The present study showed that palatal load did not affect the maximum stress value for the Ti implant. The maximum stress value of cortical bone with vertical load (19.05 MPa) was higher than that of palatal load (18.50 MPa) for the Ti implant. However, for the FRC implant, palatal load elevated interfacial stresses 1.4 times at the cortical bone crest. Comparison of vertical and palatal load in the FRC implant showed that the maximum stress value of cortical bone with vertical load (28.91 MPa) was lower than that of palatal load (41.57 MPa). However, in cancellous bone, the stress path showed that the stress value of cancellous bone with palatal load was lower than that of vertical in both implant materials. Ti and FRC have considerable differences in material properties of anisotropicity (FRC) compared with isotropicity (Ti). Ti did not exhibit different mechanical properties for various directions. However, mechanical properties of FRC depended on fiber direction. Mechanical properties varied along the fibers; that is, longitudinal direction was higher than in other directions. Under force from a transverse direction (palatal load in this study), the elastic modulus of FRC was lower than that of longitudinal direction (vertical load in this study). This is caused by the anisotropy of FRC.27
The long-time clinical performance of a dental implant is dependant on the optimum stress level within the surrounding bone. A sufficiently low stress would lead to bone loss, whereas large stresses can cause implant failures. Being a self-adaptive material, jawbone needs to be stimulated to be retained. Both Rieger and coworkers28 and O'Mahony and coworkers29 assumed that optimal bone stimulation is achieved between 1.72- and 2.76-MPa stresses. Hassler and coworkers30 showed that the optimal compressive stress level for maximum bone growth occurs between 1.8 and 2.8 MPa. This study found that the range of stress values at the top of the screw was 3.58–4.45 MPa (vertical load) and 0.09–1.48 MPa (palatal load) in the Ti implant and 1.70–2.00 MPa (vertical load) and 0.17–0.92 MPa (palatal load) in the FRC implant. In addition, the ranges of stress values between the screw threads were 0.32–0.86 MPa (vertical load) and 0.05–0.46 MPa (palatal load) in the Ti implant and 0.81–1.84 MPa (vertical load) and 0.14–0.67 MPa (palatal load) in the FRC implant. This result showed that the stress range of vertical load for the FRC implant was close to the stress level for maximum bone growth at the bone around the screw. In addition, the range of stresses at the bone around the FRC screw was more evenly distributed than that of the Ti implant.
Within the limitations of this study, the stress range of the FRC implant was close to the stress level for optimal bone growth. Furthermore, the stress at the bone around the FRC implant was more even than that of the Ti implant.