The Screw Loosening and Fatigue Analyses of Three Dimensional Dental Implant Model

The Screw Loosening and Fatigue Analyses of Three Dimensional Dental Implant Model M. Wierszycki 1,2, W. Kąkol 2, T. Łodygowski 1 1 Institute of Structural Engineering, Poznań University of Technology, ul. Piotrowo 5, Poznań, Poland 2 BudSoft, ABAQUS Inc. Representative, ul. Św. Marcin 58/64, Poznań, Poland Abstract: Dental restorations with the application of implants are very effective and commonly used in dental treatment. However, for more than fifty percent of patients, diverse complications can be observed. In some cases, these problems are caused by mechanical reasons such as loosening of the retaining screws or fracture and cracking of the dental implant components. We would like to focus on the complex biomechanical relations in dental implant simulations. A cyclic scheme of physiological occlusal loading and fatigue changes of dental material, bone loss phenomenon and changeability of boundary conditions are investigated. The implant structure poses a purely mechanical problem, but the loads and boundary conditions have already more complex, biomechanical grounds. The changes of the bone, especially bone loss phenomenon, have a great influence on implant behavior, stress distribution and therefore fatigue damage. The computer simulations of implant behavior employing of ABAQUS and fe-safe software enable us to consider all these phenomena. For the full simulation of implant structure behavior, a 3D model, which includes a spiral thread, is necessary. Only the 3D model allows a full simulation of kinematics of the implant, describing the multiaxial state of stress and, in consequence, the possibility of screw loosening. In the case of screw loosening simulation, the modeling of tightening is a crucial task. It is carried out in such a way that it describes a real physical process. The friction dissipated energy has been used as a measure of the retaining screw loosening resistance. The robustness, exactness and efficiency of complex contact analyses carried out with ABAQUS enables us to obtain valuable results and also serve for practical applications of these results in modern prosthodontics. Keywords: fatigue analysis, biomechanics, dental implant 1. Introduction Nowadays, the finite element method plays an important role in solving engineering problems in many fields of science and industry and can be successfully applied also in simulations of biomechanical systems (Będziński, 1997, Geng et al., 2001, Sakaguchi et al. 1993). The method 2006 ABAQUS Users Conference 527

is a well established one, used in biomechanical simulations for over 20 years so far. It allows taking into consideration the key features like material inhomogeneity and anisotropic mechanical properties of tissues as well as a very complicated geometry of human body parts (Swatrz et al., 1991). Furthermore, it is proved (Hędzelek et al., 2003) that function, failure, prediction of changes and remodeling of the biostructures are related to stress and strain fields in tissues and they may be calculated with the help of FEA. Thus, FEA is an efficient tool for testing biomechanical sets, like dental implants, but it is still often very difficult to obtain useful and valuable results of these kinds of problems. The main reason for this is the complexity of biostructures and the complexity of numerical simulations stemming from that. 2. Models of dental implant Implants are commonly applied treatment method of dental restorations. Unfortunately, numerous clinical observations point to the occurrence of both early and late complications. In many cases, these problems are caused by mechanical fractures of the implants themselves (Hędzelek et al., 2003, Kąkol et al., 2002). The most frequent complications are loosening of the connecting screw, fracture and cracking of the dental implant parts. While loosening of the connecting screw causes mostly a patient s discomfort in the implant usage, cracking leads to much more serious complications and makes further treatment extremely difficult. To understand the reasons of observed mechanical complications, it is necessary to know stress and strain fields in implant components as well as changes in boundary conditions. The cyclic loads and the character of the fracture indicate material fatigue as the basic cause of this fracture (Kocańda, 1985). The authors would like to confirm this proposition by means of numerical simulations of a dental implant system (Kąkol et al., 2003). The simulations were carried out with ABAQUS/Standard finite element program. For the fatigue calculations the fe-safe program was used (Safe Technology Ltd). a) b) Figure 1. Models of dental implant: a) axisymmetric with part of jaw bone, b) three dimensional with spiral thread. 528 2006 ABAQUS Users Conference

In the analysis of a dental implant, the implant structure is not trivial, however it is a purely mechanical problem. The loads and boundary conditions have already more complex, biomechanical reasons. The most significant complexities of finite element stress-strain and fatigue analyses are geometry and mesh preparation, fatigue material characteristics, implant assembly, physiological changes of loads and finally definition of boundary conditions describing it as a bone. 2.1 Geometry The numerical models were created on the basis of technical documentation of the commercial implantological system OSTEOPLANT. It is a commonly used system, consisting of an implant and abutment with a nonrotational hexagonal connection, assembled by a screw. For the full simulation of implant structure behavior, the geometrically complex three dimensional model is necessary. This model, which includes a spiral thread, enables taking into consideration a few important aspects such as full simulation of kinematics of an implant, describing the multiaxial state of stress and, the most important, the possibility of simulation of screw loosening. The most interesting result will be the relationship between torque moment, friction coefficient and loosening or fatigue life of the screw under cyclic loads. Unfortunately, a three-dimensional model is very large (ca. 500K dof). Due to the fact that most parts of an implant are axisymmetric, an axisymmetric concept of modeling is a good idea of simplification. ABAQUS/Standard offers axisymmetric solid CAXA elements, which are capable of modeling nonlinear asymmetric deformation, as well. The CAXA elements are intended for an analysis of hollow bodies, such as pipes, but they may also be used to model solid bodies with some limitations. These elements use standard isoparametric interpolation in the radial symmetry axis plane, combined with the Fourier interpolation with respect to the angle of revolution. The asymmetric deformation is assumed to be symmetric with respect to the radial symmetry axis plane at an angle equal 0 or π (ABAQUS Manuals, 2005). An axisymmetric model of an implant was created with the application of CAXA elements (Fig. 1). This approach reduces the geometry description of an implant model from a three dimensional to a two dimensional one. The threads of screw and implant body were simplified to axisymmetric, parallel rings. Thanks to this concept, the size of the problem (ca. 75K dof) and the cost of the calculation were significantly reduced. 2.2 Material properties The part of jaw is composed of two kinds of bones: the cancellous bone and the cortical one (Fig. 1). The problem of describing physical law of a bone is very complex. The mechanical characteristics and internal microstructure of cortical and cancellous bones are nonhomogeneous, anisotropic and variable in time. The changes of bone characteristics are caused by the phenomenon of remodeling tissues. It is very difficult to take these aspects into consideration in implant models. In finite element analysis, many concepts of description of mechanical properties of a bone could be applied. Starting from the very simple, isotropic, going on to the more complicated, transversely isotropic or orthotropic and ending with a very complex, anisotropic ones. The assumed material characteristics of the jaw bones are linear, homogeneous and isotropic (Tab. 3). This simplification is justifiable due to the role which the bone plays in fatigue analysis of an implant. The most important here is the influence of boneloss around an implant as well as bone flexibility on implant boundary conditions and implant fatigue life (Hędzelek et al., 2003). 2006 ABAQUS Users Conference 529

The implant is made of medical titanium alloy, the mechanical properties of which are nonlinear. Their description was based on the certificate of conformity (ASTM F136-98, ISO 5832 PT 2-93). Table 1. Material properties of implant model components. Implant's body (Titanium Grade 4) Screw (6AL-4V-ELI) Abutment (6AL-4V-ELI) Young's modulus [Mpa] 105 200 105 200 105 200 Poisson ratio 0.19 0.19 0.19 Yield [MPa] 615,2 832.3 802,8 Tensile Yield [MPa] 742,4 1004.0 970,4 2.3 Mechanical assembly The implant system is seemingly simple, but in fact it is quite a complex mechanical system (Kąkol et al., 2002, Sakaguchi et al., 1993). An important aspect of implant assembly is the modeling of tightening. For this purpose, it is necessary to define the contact surfaces between a root, an abutment and a screw. The friction characteristic on these surfaces is one of the key parameters influencing preload axial force, reduction of implant components mobility, resistance of screw loosening but also fatigue life of a whole implant. For the friction coefficient, a value ranging between 0.1 (as in a specially finished surface) and 0.5 (as in dry titanium to titanium friction) may be found in literature. In the present analyses, three different friction coefficients (0.1, 0.2 and 0.5) were considered. The friction characteristic is one of the key parameters influencing preload axial fores V, reduction of mobility of implant components and screw loosening resistance. The first step of the simulation is the tightening of the screw. In the case of the axisymmetric model, the middle part of the screw was subjected to temperature loading in order to simulate this. The thermal expansion property of the screw material was orthotropic. It was defined in such a way, that shrinking occurred only along the screw axis. The value of axial force in a tightened screw was calculated from the empirical equation. It is dependent on friction coefficient and torque moment. This force (ranging from 80 to 850 N) was changed into a temperature field (Kąkol et al., 2003). In the case of the three-dimensional model, the simulation of tightening can be defined in such a way that it describes a real physical process. However it creates a very complex contact problem. 2.4 Loads The external loads of an implant model were applied in the second step of the simulation. The values and directions of forces were taken on the grounds of a physiologically proven scheme. To estimate the least favorable distribution of stress, only the maximal realistic occlusal forces were taken into account. The loading of an implant is never axial. The vertical components of it are estimated at 600 N and the horizontal ones at 100 N. For the fatigue calculations, it is necessary to define the character of load changeability in the shape of a curve load-time, the socalled load signal. It is not easy to assume these characteristics and typical values of occlusal forces. In an applied low-cycled scheme of 24-hour loads, the average values were 60 N (Hędzelek et al., 2003, Kąkol et al., 2003). 530 2006 ABAQUS Users Conference

2.5 Boundary conditions In the first stage of implant analysis, all degrees of freedom at the bottom part of implant body were fixed. This assumption seemed to have its explanation in dental practice, where no movements of implants under physiological load are acceptable. However, the difference between infinitely stiff fixing and even low flexibility is significant, especially in the cyclic loading and fatigue damage context. In the next stage of implant analysis, the boundary conditions of implants are modeled as a small part of the jaw bone. The geometry of a small part of jaw surrounding the implant is very simplified but it enables us to take into consideration the changes in implant fixing conditions. The changing flexibility of the bone and boneloss phenomenon are also very important, especially because boneloss has a significant influence on implant behavior, stress distribution and therefore fatigue damage. The degree of encasement and osseointegration of the implant may not be 100%. It dependents on bone quality, stresses developed during healing and function, and the location of the implant in the jaw. This percentage may decrease to as low as 50%. This is caused by remodeling of bone phenomenon. In these analyses three levels of osseointegration were considered. In the case of the first level, the implant body is fully fixed in the jaw bone. In the next two, the degree of implant body embedding decreases to 75 and 50% respectively (Fig. 2) (Hędzelek et al., 2003). a) b) c) Figure 2. Boundary conditions of implant model levels of osseointegration: a) 100%, b) 75%, c) 50%. 3. Behavior of screw Full simulation of screw loosening can be performed only using a 3D implant model. Simulation of tightening can be performed in such a way that it describes a real physical process. 2006 ABAQUS Users Conference 531

3.1 Simulation of tightening The simulation of tightening defined in such a way that it describes a real physical process requires a complex contact analysis. If this analysis is performed using the implicit code, as ABAQUS/Standard, a lot of small increments and equilibrium iterations are usually required to reach a converged solution. In some cases it is very difficult to obtain any converged solution. For simulations of screw tightening, the quasi-static analysis using the explicit code, like ABAQUS/ Explicit, can be carried out, alternatively. The results presented on Fig. 3, Fig. 4 and Fig. 5 were obtained from the analyses performed with ABAQUS/Standard. The friction coefficient was assumed equal to 0.2. The analyses were performed using the displacement control technique. The screw was subjected to a rotational displacement equal to 1 radian, which in turn was applied to the reference point of a rigid body defined on the top surface nodes of the screw head. The Fig. 3 shows the time-history of the tightening moment. The expected zig-zag type curve was recorded at the point of applied displacement. Figure 3. Tightening moment [Ncm]. Fig. 4 shows nearly the linear evolution of normal force in the screw during a tightening process while Fig. 5 shows the comparison of total energies involved in the process, namely internal energy (ALLIE), plastic dissipation energy (ALLPD) and energy dissipated through frictional effects (ALLFD). 532 2006 ABAQUS Users Conference

Figure 4. Normal force in screw [N] Figure 5. Tightening energy balance [mj]. 2006 ABAQUS Users Conference 533

3.2 Screw loosening phenomenon In the first step of simulation the implant body was tightened. Two values of tightening moment (15 Ncm and 35 Ncm) and two friction coefficients (0.1 and 0.2) were taken into considerations. In the second step of simulation the torsional loading (asymmetric force) was applied to the top of the abutment to initiate a small movement of the implant system. To measure a resistance to screw loosening the frictional dissipation energy accumulated over a whole process was chosen. The energy dissipated by contact friction forces between the contact surfaces is as follows: where: v velocity field t f frictional traction S boundary (contact surfaces) E F = vt f ds S In the Fig. 6 the energy ALLFD is plotted for two different friction coefficients of a screw threads. It is seen that this energy can be a measure of work to be performed during the screw loosening process. Further investigations in this subject will be carried out. Figure 6. Comparison of ALLFD energy for different friction coefficients. 534 2006 ABAQUS Users Conference

4. Fatigue analysis Fatigue calculations were carried out in the fe-safe program, which uses advanced multiaxial fatigue algorithms incorporating a multiaxial plasticity model to estimate the life of fatigue. These algorithms are based on the stress results obtained from the finite element analysis (Fig. 7), variations in loading, hysteresis loop cycle closure, and cyclic material properties. Elastic stresses from the FEA model are translated into elastic-plastic stresses by means of a biaxial Neuber's rule and cyclic material properties. In order to estimate failure-free term of an implant, a designed life is defined. Fe-safe calculates the factor (FOS Factor Of Strength) by which the stresses at each node can be increased or reduced to give the required life. The above is the most interesting and vivid for our case. During a single analysis concerning each node separately, a 6-stress tensor is used to calculate the principal stresses and strains and their orientation. A stress concentration factor and scale factor are applied at this stage. A rainflow cycle counting algorithm is used to extract fatigue cycles. For biaxial fatigue methods in turn a critical plane procedure is used to calculate the orientation of the most damaged plane at the node (ABAQUS/Safe Manual, Bishop, 2000, Draper, 1999). Fatigue life of an implant screw was calculated for nine separate cases of loading, three cases of boundary condition schemes and three cases of jaw cancellous bone density. For all of these cases, the same cyclic scheme of loading was assumed. A twenty-four-hour changeability scheme was assumed as a signal, while the number of days corresponding to four years was assumed as the number of cycles. The FOS distribution analysis for particular cases indicates the axial forces in the screw and the changes in the scheme of boundary conditions, which have the greatest influence on fatigue changes. For different bone density and at the same time divergent stiffness of boundary conditions, significant differences of stress distributions present in the screw are noticeable. Yet, it does not lead to serious fatigue changes. For axial forces above 600 N, there is a noticeable increase in the areas endangered by fatigue failure. The degree of required stress reduction reaches ca. 30%. In the most unfavorable load case, the maximal axial force value is the result of a high torque moment and a very small friction coefficient on a screw thread. It is important to pay attention to the danger of increasing the tightening forces in an implant screw. In two-part implants, this high tightening force is motivated by biological and medical aspects. However, the increase in torsion moments and decrease in friction coefficients pose a danger for fatigue life of implant components. 4.1 Moment and friction vs. FOS Fatigue life of the implant screw was calculated for nine cases of loading. For all of these cases the same cyclic scheme of loading was assumed.(table 2). A twenty-four-hour changeability scheme was assumed as a signal while the number of days corresponding to four years was assumed as the number of cycles. 2006 ABAQUS Users Conference 535

Table 2. List of load cases and friction coefficient. Load case 1 2 3 4 5 6 7 8 9 Torque moment [Ncm] 15 15 15 25 25 25 35 35 35 Friction Coefficient (μ) 0.1 0.2 0.5 0.1 0.2 0.5 0.1 0.2 0.5 Axial force [N] 371.85 199.7 83.6 619.74 332.83 139.33 867.64 465.96 195.06 The FOS distribution analysis for particular cases indicates that fatigue changes for axial forces up to 200 N occur only in the neighborhood of the first thread twist. For stronger forces, however, the notch under the screw head is also a dangerous area. In all of those cases, stresses exceed the save range maximally in 5 10 %. For axial forces above 600 N (loading case 6 and 7) there is a clearly seen increase of fatigue failure endangered areas. Next points of fatigue changes appear. At the same time, the degree of required stress reduction reaches 30 %. In the most unfavorable load case, the maximal axial force value is the result of both the greatest torque moment and the smallest friction coefficient. The results obtained on this stage of fatigue analysis enable us to formulate some estimate of fatigue characteristic of the implant work. It is important to pay attention to the danger of increasing the tightening forces in implant screw. In two-part implants it is motivated by biological and treatment aspects. However, the increase of torsion moments and decrease of friction coefficient poses a danger for fatigue life of implant components. 4.2 Stiffness and levels of osseointegration vs. FOS The jaw bone is undergoing constantly changes processes; during few months the jaw bone can be completely renewed. This process is called as a bone remodeling. At the continuum level we distinguish, based on porosity, cortical bone and trabecular bone. The outer layers of a bone are of cortical type while inner layers of trabecular type with varying density. It can happen that a whole trabecular part is replaced by cortical one during a remodeling process. To choose an appropriate model of jaw bone remodeling is difficult task. Instead of employing any bio-remodeling theory we performed a series of simulations which addressed similar effects on a cortical as well as trabecular jaw bone with varying density and levels of osseointegration and their influence on the fatigue life of the implant system. Four different Young s modulus for a trabecular part were assumed to simulate a change of bone s stiffness, starting with a value close to a real measured one, through a small stiffness (hundreds of MPa) and ending with similar to stiffness of cortical part. The values used in simulations are listed in Table 3. 536 2006 ABAQUS Users Conference

Table 3. Stiffness of jaw bone. Bone Young's modulus [Mpa] Cortical all schemes 13 000 Cancellous 1st scheme 9 500 2nd scheme 5 500 3rd scheme 1 600 4th scheme 690 In the case of overloading a bone is undergoing a resorption process which leads to reduction in bone mineral content and can lead to an osteoporosis disease, as well. It is very difficult to take into account such phenomenon in the fatigue analysis. Again, instead of employing a theory of a removal by a bone itself, to estimate a fatigue life of the implant system, we performed simulations for four different levels of osseointegration. The simulations were performed for four different stiffness of cortical bone. The top level of cortical bone, according to the Fig. 2, was assumed as: a) entirely embedded to a bone (100%) b) 3mm below conical implant surface (75%) c) 6mm below conical implant surface (50%). A choice of levels of osseointegration expressed in assumed geometry (Fig. 2) was based on the following assumptions: a) the first level is a target position after a restoration treatment and was taken in all our previous simulations b) the second level corresponds to such a bone removal which uncover the first outer thread and where hexagonal abutment changes into inner thread c) the third level corresponds to such boundary conditions of a implant body for which bending is acting on its weakest cross-section. 2006 ABAQUS Users Conference 537

a) b) Figure 7. The Mises equivalent stresses distribution for three different levels of osseointegration: a) 100%, b) 75%, c) 50%. c) 538 2006 ABAQUS Users Conference

4.3 Verification The confirmation of numerical results is a case report of implant fracture and examination of fractured surface. The mechanical failure occurred in 55-year-old male patient after one-year period of using single crown replacing the first maxillar premolar. The fracture line passed through upper part of implant body and abutment screw. The failure was located transversally to the long axis between smooth and threaded part of the fixture. Radiograph showed also the bone loss down to the third thread of the implant. Scanning electron microscope examination presented fatigue striations, indicating the advancement of the crack front under cyclic loading. Fractography revealed obliteration and incrustation of some of the fracture features probably because of postfracture wear of contacting surfaces as a result of the component remaining joined together by abutment screw. On Fig. 8 (from Scanning Electron Microscope) fracture surface of dental implant is presented. The characteristic of fatigue damage changes like fatigue bands, called striations, can be observed. Fatigue striations are microscopic features on a fatigue fracture surface that identify one propagation cycle of a fatigue crack. It was possible to identify area with plastic deformation corresponding to final fracture. a) b) Figure 8. Fatigue fracture surface of dental implant (SEM pictures): a) 150x, b) 900x. 5. Conclusions FEA simulation of the behavior of a dental implant system was presented. It was shown that computational modeling and 3D simulation using ABAQUS and fe-safe software enable the realistic prediction of its behavior under restoration treatment as well as service loads. For screw loosening simulation, the modeling of tightening is a crucial task. It has to be carried out in such a way that describes a real physical process as much as possible. Only a 3D modeling 2006 ABAQUS Users Conference 539

allows a full simulation of kinematics of the implant, describing the multi-axial state of stress and, in consequence, the possibility of screw loosening. On the basis of the results of fatigue analysis, it can be claimed that the material fatigue is the basic reason of the observed complications. The application as a measure of loosening resistance, the energy dissipated through frictional effects, can lead to practical recommendations in prosthodontics. It is hoped that using presented approach an optimal implant shape can be derived further. 6. References 1. ABAQUS Analysis User's Manual, ABAQUS, Inc. Pawtucket, 2005. 2. ABAQUS Theory Manual, ABAQUS, Inc. Pawtucket, 2005. 3. ABAQUS/Safe User's Manual, HKS, Inc. Pawtucket, 2001. 4. Będziński R., Biomechanika inżynierska (in Polish), Oficyna Wydawnicza Politechniki Wrocławskiej, Wrocław, 1997. 5. Bishop N. W. M., Sherratt F., Finite Element Based Fatigue Calculations, NAFEMS, Glasgow, 2000. 6. Draper J., Modern metal fatigue analysis, HKS, Inc. Pawtucket, 1999. 7. Hędzelek W., Zagalak R., Łodygowski T., Wierszycki M., The effect of marginal bone loss and bone density on the risk of late implant components failures, 27th Annual Conf. of the European Prosthodontic Association, Geneva, September 4-6, 2003. 8. Kąkol W., Łodygowski T., Wierszycki M., Hędzelek W., Zagalak R., Numerical Analysis of the Behavior of Dental Implant, ABAQUS Users' Conference 2002, Newport, Rhode Island, 2002. 9. Koa C-C., Swiftb J. Q., DeLonga R., Douglasa W. H., Kima Y., Anc K-N., Changd C-H., Huangd H-L., An intra-oral hydraulic system for controlled loadingof dental implants, Journal of Biomechanics 35, pp. 863-869, 2002. 10. Kocańda S., Zmęczeniowe pękanie metali (in Polish), Wydawnictwo Naukowo-Techniczne, Warszawa 1985. 11. Merz B. R., Hunenbart S., Belser U. C., Mechanics of the implant-abutment connection: an 8- degree taper compared to a butt joint connection, The International Journal of Oral & Maxillofacial Implants, 15 (4), pp 519-526, 2000. 12. Natali A. N., Pavan P. G., Schileo E., Dettin M., Bagno A., Di Bello C., Dental implant osseo-integration: a coupled biochemical and biomechanical approach, Acta of Bioengineering and Biomechanics, 13th Conference of the European Society of Biomechanics, Vol. 4 Supp. 1, Wrocław, Poland, pp. 817-818, 2002. 13. Patterson E. A., Johns R. B., Theoretical analysis of the fatigue life of fixture screws in osseointegrated dental implants, The International Journal of Oral & Maxillofacial Implants, 7 (1), pp. 26-33, 1992. 540 2006 ABAQUS Users Conference

14. Sakaguchi R. L., Borgersen S. E., Nonlinear finite element contact analysis of dental implant components, The International Journal of Oral & Maxillofacial Implants, 7 (1), pp 655-661, 1993. 7. Acknowledgements The research was financed from the budget resources meant for science in the years 2005 and 2006. The financial support was provided by the Ministry of Science and Information Society Technologies Grant No. 3 T11F 026 28, BW-11-806/06. A part of the calculations was carried out in the Poznań Supercomputing and Networking Center. 2006 ABAQUS Users Conference 541