Materials Science and Engineering C 33 (2013) 691–698
Contents lists available at SciVerse ScienceDirect
Materials Science and Engineering C journal homepage: www.elsevier.com/locate/msec
Stress analysis in single molar tooth Ali Merdji a, Rajshree Mootanah b, Bel Abbes Bachir Bouiadjra a,⁎, Ali Benaissa c, Laid Aminallah a, El Bahri Ould Chikh c, Sam Mukdadi d, e a
LMPM, Department of Mechanical Engineering, University Djillali LIABES of Sidi Bel-Abbes, BP 89, Cité Ben m'hidi, Sidi Bel Abbes 22000, Algeria Medical Engineering Research Group, Faculty of Science & Technology, Anglia Ruskin University Bishop Hall Lane, Chelmsford, Essex, UK Laboratory LSTE, Department of Mechanics, University of Mascara, Algeria d Department of Mechanical and Aerospace Engineering, West Virginia University, USA e Center for Cardiovascular & Respiratory Sciences, West Virginia University, USA b c
a r t i c l e
i n f o
Article history: Received 18 February 2012 Received in revised form 15 September 2012 Accepted 28 October 2012 Available online 2 November 2012 Keywords: Stress Finite element method Molar tooth Biomechanics
a b s t r a c t The human tooth faces different stresses under environments of different loading conditions, these loading produces major factors in weakness of the tooth and bone structure. The need to save natural teeth has prompted the development of novel and complex techniques in endodontology, prosthodontics and periodontology. Despite a poor long-term prognosis and some prejudice to local bone, considerable efforts have been exerted for the realization of these techniques. Nowadays, the 3D finite element analysis (FEA) is one of the more recently used techniques for stress analysis in single human tooth under different loading cases. The von Mises stress distribution indicated that the greatest effort area of tooth lies at the base of crown up to the gingival line with varying intensities in the different loading cases. The highest stress in the cortical bone was predominantly found around the cervical region of the tooth and lowest in the cancellous bone and periodontal ligament (PDL). The PDL is a soft tissue, and it could function as an intermediate cushion element which absorbs the impact force and uniformly transfers the occlusal forces into the surrounding bone. © 2012 Elsevier B.V. All rights reserved.
1. Introduction Recently, mechanical aspects of various advanced materials have been paid much attention [1–3]. Especially, mechanical behavior of biological structures is a common subject of scientific research. The stress results of such investigations offer the precise insight into the biomechanical properties of biological structures and are useful for predicting their behavior when subjected to loading. Although known, there are mainly three different ways in which stress analysis can be performed: analytical, experimental and computational. In fact the most important one is the computational, in which the stress analysis would seem to be the most natural way to approach this problem. The experimental process can be simulated and repeated on the computer and be observed in virtual prototyping. It is convenient to change the material or shape properties and obtain the new results. Many researchers have used the computer to analyze dental structures, including human teeth. The primary computational method used for stress analysis today is finite element analysis (FEA). Many researchers [4–6] have also used photoelastic techniques to understand stress distribution under various loading conditions. While analytical approaches are not available for complex dental structures, experimental approaches are expensive and time ⁎ Corresponding author. E-mail address: [email protected] (B.A. Bachir Bouiadjra). 0928-4931/$ – see front matter © 2012 Elsevier B.V. All rights reserved. http://dx.doi.org/10.1016/j.msec.2012.10.020
consuming. Due to irregular geometry, complex material properties and complicated loading conditions are involved in dental structures. With the increase in computational power, the use of finite element method (FEM) can help to simulate with a great accuracy the functioning of the human tooth. FEA has been widely used in engineering since the 60s [7–10]. They are an important tool in the understanding of the mechanical behavior of materials used in industry. However, in dentistry this kind of analysis is rather recent. Although the first article published by Farah et al. [11] on the subject dates back to 1973, this technique is still little used. That is mainly due to (i) the difficulty associated with the model elaboration, for they present different shapes depending on the tooth to be analyzed, and (ii) to the difficulty involved in obtaining the mechanical properties of the tooth's constituent materials: enamel, dentin, cementum, pulp, spongy bone, compact bone and periodontal ligament. Furthermore, little is known about the contact areas between such materials and their degree of influence on the mechanical behavior of the tooth as a whole. For any FEA to be performed a computer model of structure under investigation has to be created. In this method a geometric model is developed and a “mesh” is created by subdividing the geometry into rectangular or brick-shaped elements. In all FEA studies there are four sets of parameters that completely define the model: geometry, material behavior, loading and boundary conditions. Once the model is completely defined and meshed, a stress analysis is performed and
692
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
Fig. 1. CT scan mandibular bone.
stress distributions are obtained (usually in graphical form). Lin et al. [12] cited that FEM analysis could predict detailed mechanical responses of structures and alter the parameters in a more controllable manner, and therefore have become a popular analytical tool in dental biomechanical studies. In contrast to other methods involved in dental studies, once when a mathematical model is made, it is possible using the computer to simulate different stress applications and also change the shape and design of structures in numerous ways in order to gain more scientific data [13,14]. Evaluation of published literature showed that researchers have used two-dimensional (2D) models in their studies [15,16]. Korioth and Versluis [17] claim that depending on investigated structure and boundary conditions, 2D modeling may be justified as reasonable, especially when simplicity and efficiency are concerned. Other authors have used three dimensional (3D) models in their investigations [11,18]. Tooth fracture results directly from combined acting intraorally. Masticatory stresses, the amplitudes of these stresses depend on factors including gender, age, state of teeth, as well as the hardness of food. Masticatory forces are the greatest in the region of the first molars. There is little research regarding the mechanical behavior of natural teeth [13]. The majorities of the previous studies were interested on the behavior of dental implants. However, the knowledge areas of stress concentrations in a natural manner are important to predict the lifetime of these teeth. In addition this knowledge can help practitioners of dental implant when restoring mandibular molars to ensure proper operation of the implant. The aim of this study is to analyze the stress distribution in the human molar tooth
using a finite element model. This study can help to create patientspecific FE models based on occlusal contact records and morphological measurements of each patient to analyze the stress and strain distributions in the periodontal structures of the molars. We also aimed to highlight the zones of stress concentration in order to predict the eventual damage in human molar tooth.
1.1. Geometric model of the tooth–PDL–bone system The problem of biomechanical behavior of a complex structure with irregular geometry such as the tooth can be analyzed using the FEM. In order to perform the FE study one is obliged to create a digital model of the structure under investigation. The initial 3D model of the molar section from the mandibular bone structures was constructed based on computerized tomography (CT) scan technology (Fig. 1). The individual scans were processed in Rhinoceros 3.0 and SolidWorks 3D, where the final 3D solid model of the bone was created with a layer of cortical bone of 2 mm thickness, and cancellous bone. The human molar tooth model employed in this study was constructed primarily using computer tomography (CT) images, digital edge detection technique and computer aided design (CAD) methods. The periodontal ligament (PDL) represented a considerably small volume as 0.2 mm of the molar tooth system and is assimilated into the volume of the alveolar bone (Fig. 2).
2. Material models The tooth is composed primarily of 3 materials: the dentin, the enamel, the cementum. The cementum and the enamel represent a considerably small volume of the tooth and are assimilated into the volume of the dentin. The PDL being a highly soft material, the hard dentin deforms little with respect to the PDL when the molar is loaded. All the materials were presumed linear, elastic, homogeneous, and isotropic for the analyses as widely adopted in existing literature [19–22], and the mechanical properties were taken from the literature as shown in Table 1.
Table 1 Mechanical properties of materials used in model of mandibular molar.
Fig. 2. Three dimensional models of mandibular bone, PDL and molar tooth.
Parts
Constitutive equation
Elastic modulus (E) (GPa)
Poisson ratio (ν)
Molar tooth Periodontal ligament (PDL) Cortical bone Cancellous bone
Isotropic linear elastic
20 0.05 14.5 1.37
0.3 0.49 0.323 0.3
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
693
Fig. 5. Meshing in the vicinity of the ligament. Fig. 3. Boundary conditions.
Although PDL is viscoelastic in nature, the isotropic elastic properties were assigned as the load response lies within the linear elastic range [23]. Bone in this study is also modeled isotropically since it was already stated that isotropic models of the mandible were able to distinguish meaningful strain differences when replicating functional loading [24], which have been widely accepted by clinicians when evaluating patients [25].
• The most coronal plane of the crown is subjected to a load of 3 MPa in either the lingual–buccal or mesial–distal directions or a load of 10 MPa in coronal–apical direction. • The other surfaces are treated as free surfaces, i.e. zero loads. The vertical load of 10 MPa and horizontal load of 3 MPa were applied at the surface central in the occlusal face of the crown (Fig. 3).
2.1. Interface conditions The interface between the tooth and the ligament, as well as between the cortical and cancellous bone are treated as perfectly bonded interface. 2.2. Boundary conditions In order to define the boundary conditions, a 3D coordinate system is defined by three forces in the coronal–apical direction, lingual–buccal direction and mesial–distal direction. For the boundary conditions, three zones are presented: • The inferior plane of the mandibular bone is defined as having zero displacement.
2.3. Finite element model In this study, the commercial code Abaqus (6.11) was employed for linear static analysis. The mesh of the components is simplistic and consists of linear tetrahedron elements with four nodes (Fig. 4). Since the ligament experiences the largest deformations under load, it is necessary to mesh this volume into small elements (Fig. 5). The tooth and the bone are meshed with increasingly larger elements as the distance from the ligament increases, with the size of elements in contact with the ligament being defined by the elements of the boundary mesh. The mesh of the components is verified for use in a finite element stress analysis. The characteristics for the meshes of each component are presented in Table 2. 3. Results For analysis in all simulations, the von Mises stress was used. The distributions of this stress in the bone surrounding the PDL and molar tooth were investigated. The von Mises stress is a scalar variable that is defined in terms of all the individual stress components and, therefore, is a good representative of the state of stresses. It has been extensively used in biomechanical studies of bone [26–28]. The distributions of overall stress state for each component in our model were shown under effect of axial and horizontal loading in the coronal–apical, lingual–buccal and distal–mesial. A qualitative and quantitative analysis was performed, based on a progressive visual color scale, pre-defined by the software used, ranging from dark
Table 2 Size and number of elements used for the bone, ligament and molar tooth.
Fig. 4. Mesh using linear tetrahedron elements of (a) the tooth, (b) the ligament and (c) the alveolar bone.
Component
Size of element (mm)
No. of elements
Molar tooth Periodontal ligament (PDL) The mandibular bone
0.25 0.25 0.25–1.00
195,514 220,155 142,305
694
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
and bone, however, deform only marginally. In the apical–coronal view shown in Fig. 9 the strain field at the surface of the ligament is relatively homogeneous, and no region undergoes a particular deformation. The bone–implant interface was capable of withstanding and absorbing the stress during axial loading. 3.2. Alveolar bone In the alveolar bone, stress distribution was almost similar to that in the PDL, but the values of stress distributed in the alveolar bone were approximately 10 times larger than those in the PDL. Furthermore, the highest stress in the alveolar bone, as a whole, was concentrated in the cortical bone, around the PDL. Because of a great difference between the stress values in the cortical and cancellous bone, the stress distributions in these bone regions are shown separately for better visualization.
Fig. 6. Different t stress levels.
blue to red (Fig. 6). The maximum stress values in each component under different loading are shown in Fig. 11. 3.1. Periodontal ligament (PDL) Fig. 7 represents the von Mises stress distribution within the ligament. It was seen that the periodontal ligament underwent a maximum stress at the cervical region of its contact with the tooth and alveolar bone. The stresses gradually reduced as we move towards the middle part of the periodontal ligament. The Von Mises strain of the PDL shown in Fig. 8 indicates that it is principally the ligament that undergoes strain deformation. The tooth
3.2.1. Cortical bone The cortical bone also experienced stresses along the same lines as that of the periodontal ligament. It was seen that the maximum stress in the alveolar bone was found at the cervical region where the tooth comes in contact with the alveolar bone through the periodontal ligament (Fig. 10a). 3.2.2. Cancellous bone Because of its low modulus of elasticity, minimal stress was generated compared to the cortical bone. The maximum stress was concentrated at the base of the roots. This stress diminished in magnitude towards the coronal end of the roots (Fig. 10b). 3.3. Molar tooth When applying a tipping load on occlusal surface of the tooth model, a region of relatively high equivalent stress was found at the surfaces of the root (Fig. 11). The maximum value was detected on
Fig. 7. Distribution of stresses within periodontal ligament (PDL): (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
695
Fig. 8. Distribution of strains within periodontal ligament (PDL): (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
the cervical level of the roots. The molar tooth also experienced stresses along the same lines as that of the cortical bone.
4. Discussion The finite element model of the maxillary second molar tooth that included alveolar bone was investigated for analysis of the stress distribution [28]. Previously, several researchers [29–31] constructed FE tooth models using a series of slice images of a tooth and performed stress analysis during tooth movements. However, these FE models were developed as general tooth models with an average size and shape of the crown and root. Subsequently, in a previous study, an automatic
Fig. 9. Maximum elastic strain observed in the ligament.
modeling system from CT image was developed for computer-aided diagnosis [32]. Finite element models have their current origin and real use in mechanical engineering analysis and design. Biological applications have been successful where mechanical principles would be of the most interest; for example in modeling human joints [33]. In dentistry, models have been used to determine the stresses in different biologic structures, such as jaws, facial skeleton, dentition, periodontal ligament, temporomandibular joint [34–37] and different dental restorative materials, for example, implants, composites etc. [38,39]. Most of the surveyed FEM studies analyzed the biomechanical behavior of individual structures or materials, while we have tried to investigate interactions of stresses in the biomechanical system, representing the main elements of human masticatory system. The objective of this study was to evaluate the influence of axial and horizontal loads on stress distribution when the molar tooth submitted to occlusal loading. Even with the simplifications of considering the bone and molar tooth system to be homogeneous, linearly elastic and static load. The maximum von Mises stress values in the molar tooth, periodontal ligament and alveolar bone are shown in Fig. 12. In general, lateral occlusal loads (lingual–buccal and distal–mesial) significantly increased the stress values when compared with axial occlusal load (coronal–apical). Irrespective of the direction and magnitude of loading, it has been demonstrated that the highest stresses were observed firstly on the tooth, secondly in the alveolar bone and thirdly in the periodontal ligament. These findings are due to the different mechanical properties of each structure. The tooth resists to maximum amount of stress compared to any other component of the model. The probable reason could be associated to its elastic modulus (E = 20,000 MPa), which is approximately one time and half the elastic modulus of cortical bone (E = 14,500 MPa), 14 times the elastic modulus of cancellous bone (E = 1370 MPa) and 400 times the elastic modulus of periodontal ligament (E = 50 MPa). In this study, an applied loading to the crown surface involves a high stress concentration in the higher part of the fixing zone of the
696
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
Fig. 10. Distribution of stresses within alveolar bone: (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
tooth system in contact with the cortical bone, i.e., superior area of the cortical layer. These were due to: • The evidence of the surface area between the tooth and the cortical bone is much smaller than the surface area between the tooth and the cancellous bone. Moreover, the cortical bone is more than ten times stiffer than the cancellous bone. These are the reasons that high stress increments were found in the cortical bone.
• The intimate contact at the cortical bone and tooth interface, the loading applied to the crown of the tooth is directly transmitted to the cortical bone. • This suggests that great importance is to be attached to the contact of the tooth system with the cortical layer of bone. The graph in the following Fig. 13, describes the effect of acting vertical and horizontal loads. During vertical loading, stress generated within the cortical bone was the least as compared to the stress
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
697
Fig. 11. Distribution of stresses within molar tooth: (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
generated during bucco-lingual and mesio-distal loadings. The reason being that the direction of load along the long axis of the tooth provides maximum cross-sectional area to withstand the stress. Indeed, we noted for a distal–mesial loading the highest stress concentration compared to the other loadings in the cervical areas of the cortical bone, the tooth, and the periodontal ligament. Fig. 13 illustrates this observation which is indeed not recorded for the cancellous bone. The latter being more sensitive to the compression loads. With our greater knowledge based on the realized study, this can be justified by the boundary conditions applied to the system
like by the wide form of the mandibular bone in the distal–mesial direction. Also, let us mention that the analysis carried out on only one molar tooth independently of the adjacent teeth on the dental arch, which generated the strongest stresses in the distal–mesial direction in the case of a single tooth. This justifies the importance of the replacement of the lost teeth by dental implants in order to minimize this type of stresses. 5. Conclusions The finite element method is the nearest possible method available today to simulate the oral cavity in vitro. It is a numerical method for addressing mechanical problems and therefore, is a powerful contemporary research tool. FE analysis provides a precise insight into the complex mechanical behavior of restored teeth affected by stress fields which are difficult to assess otherwise. Of particular importance is the possibility of examining the various parameters. The use of these theoretical engineering methods will certainly give answers to problems in restorative dentistry. Thus the results are practical and applicable, of clinical significance and reference value and give direction to experimental and clinical research. This initial FEM model has demonstrated that the computational modeling approach can be successfully used in the biomechanical study of stresses distribution in the constituent parts of the masticatory system. The 3D FEM analysis of tooth geometry characteristics and stress relationship suggested that von Mises stresses might increase with the increase of the distal–mesial loading. This explains why teeth are more predisposed to occlusal trauma. Acknowledgment
Fig. 12. Histograms of comparison of von Mises stresses for each component under the different load directions.
The authors extend their appreciation to the Deanship of Scientific Research at King Saud University for funding the work through the research group no. RGP-VPP-035.
698
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
Fig. 13. Distribution of cervical stresses within cortical bone under the different load directions.
References [1] W. Jianfeng, C. Qunfeng, Z. Tang, J. Chem. Soc. Rev. 41 (2012) 1111–1129. [2] C. Zhenguo, Z. Xiqi, X. Bingjia, Z. Xie, M. Chunping, Z. Yi, L. Siwei, X. Jiarui, J. Chem. Soc. Rev. 41 (2012) 3878–3896. [3] K. Ariga, T. Mori, J.P. Hill, J. Adv. Mater. 24 (2012) 158–176. [4] J.W. Farah, R.G. Craig, D.L. Sikarskie, J. Biomech. 6 (1973) 511–520. [5] T. Yamada, J. Sugawara, H. Itoh, T. Sasaki, E. Umezaki, in: 4th Asian Implant Orthodontics Conf, 2005, pp. 22–23. [6] T. Yamada, J. Sugawara, H. Itoh, T. Sasaki, K. Sasaki, E. Umezaki, in: International Congress Series, 1284, 2005, pp. 77–78. [7] M.J. Turner, R.W. Clough, H.C. Martin, L.J. Topp, J. Aeronaut. Sci. 23 (1954) 805–823. [8] O.C. Zienkiewicz, Finite Element Method, 3rd ed. McGraw-Hill, London, 1977. [9] M. Ameen, Computational Elasticity, Theory of Elasticity and Finite and Boundary Element Methods, Alpha Science International Ltd., Harrow, U.K., 2005. [10] S. Rao, The Finite Element Method in Engineering, 4th edition Butterworth Heinemann, USA, 2004. [11] J.W. Farah, R.G. Craig, J. Dent. Res. 54 (1975) 255–261. [12] C.L. Lin, C.H. Chang, C.H. Wang, C.C. Ko, H.E. Lee, J. Oral Rehabil. 28 (2001) 517–525. [13] B. Dejak, A. Mlotkowski, M. Romanowicz, J. Prosthet. Dent. 90 (2003) 591–597. [14] J.A. Hobkirk, H.W. Wiskott, Clin. Oral Implants Res. 17 (2006) 52–54. [15] J.S. Rees, J. Oral Rehabil. 29 (2002) 188–193. [16] M. Tanaka, T. Naito, M. Yokota, M. Kohno, J. Oral Rehabil. 30 (2003) 60–67. [17] T.W.P. Korioth, A. Versluis, Crit. Rev. Oral Biol. Med. 8 (1997) 90–104. [18] P. Ausiello, A. Apicella, C.L. Davidson, Dent. Mater. 18 (2002) 295–303. [19] J.S. Rees, M. Hammadeh, D.C. Jagger, Eur. J. Oral Sci. 111 (149–154) (2003). [20] H. Spiekermann, Color Atlas of Dental Medicine: Implantology, Thieme, New York, 1995.
[21] O.A. Abu-Hammad, A. Harrison, D. Williams, Int. J. Oral Maxillofac. Implants 15 (2000) 559–564. [22] B.H. Choi, Int. J. Oral Maxillofac. Implants 15 (2000) 193–196. [23] G. Pietrzak, A. Curnier, J. Botsis, S. Scherrer, A. Wiskott, U. Belser, Comput. Methods Biomech. Biomed. Eng. 5 (2002) 91–100. [24] I. Ichim, M. Swain, J. Kieser, J. Dent. Res. 85 (2006) 638–642. [25] U. Lekholm, G. Zarb, in: P.I. Branemark, G.A. Zarb, T. Albrektsson (Eds.), Tissueintegrated Prostheses, 2 ed., Quintessence, Chicago, 1987. [26] P. Kowalczyk, Dent. Mater. 25 (2009) 83–91. [27] P. Magne, Dent. Mater. 23 (2007) 539–548. [28] P. Magne, D.T. Tan, J. Adhes. Dent. 10 (1) (2008) 49–56. [29] M.L. Jones, J. Hickman, J. Middleton, J. Knox, C. Volp, J. Orthod. 28 (2001) 29–38. [30] P.D. Jeon, P.K. Turley, B.H. Moon, K. Ting, Am. J. Orthod. Dentofacial Orthop. 115 (1999) 267–274. [31] H. Qian, J. Chen, T.R. Katona, Am. J. Orthod. Dentofacial Orthop. 120 (2001) 272–279. [32] K. Maki, N. Inou, A. Takanishi, A.J. Miller, Orthod. Craniofac. Res. 6 (2003) 95–101. [33] J.J. Liau, C.K. Cheng, C.H. Huang, W.H. Lo, Clin. Biomech. 17 (2002) 140–146. [34] P.M. Cattaneo, M. Dalstra, B. Melsen, Am. J. Orthod. Dentofacial Orthop. 123 (2003) 367–373. [35] M.D. Gross, G. Arbel, I. Hershkovitz, J. Oral Rehabil. 28 (2001) 684–694. [36] S. Gomes de Oliveira, P.I. Seraidarian, J. Landre, D.D. Oliveira, B.N. Cavalcanti, J. Oral Rehabil. 33 (2006) 874–880. [37] S.R. Toms, A.W. Eberhard, Am. J. Orthod. Dentofacial Orthop. 123 (2003) 657–665. [38] I. Akpinar, N. Anil, L. Parnas, J. Oral Rehabil. 27 (2000) 538–539. [39] P.L. Boschian, S. Guidotti, R. Pietrabissa, M. Gagliani, J. Oral Rehabil. 33 (2006) 690–697.
Contents lists available at SciVerse ScienceDirect
Materials Science and Engineering C journal homepage: www.elsevier.com/locate/msec
Stress analysis in single molar tooth Ali Merdji a, Rajshree Mootanah b, Bel Abbes Bachir Bouiadjra a,⁎, Ali Benaissa c, Laid Aminallah a, El Bahri Ould Chikh c, Sam Mukdadi d, e a
LMPM, Department of Mechanical Engineering, University Djillali LIABES of Sidi Bel-Abbes, BP 89, Cité Ben m'hidi, Sidi Bel Abbes 22000, Algeria Medical Engineering Research Group, Faculty of Science & Technology, Anglia Ruskin University Bishop Hall Lane, Chelmsford, Essex, UK Laboratory LSTE, Department of Mechanics, University of Mascara, Algeria d Department of Mechanical and Aerospace Engineering, West Virginia University, USA e Center for Cardiovascular & Respiratory Sciences, West Virginia University, USA b c
a r t i c l e
i n f o
Article history: Received 18 February 2012 Received in revised form 15 September 2012 Accepted 28 October 2012 Available online 2 November 2012 Keywords: Stress Finite element method Molar tooth Biomechanics
a b s t r a c t The human tooth faces different stresses under environments of different loading conditions, these loading produces major factors in weakness of the tooth and bone structure. The need to save natural teeth has prompted the development of novel and complex techniques in endodontology, prosthodontics and periodontology. Despite a poor long-term prognosis and some prejudice to local bone, considerable efforts have been exerted for the realization of these techniques. Nowadays, the 3D finite element analysis (FEA) is one of the more recently used techniques for stress analysis in single human tooth under different loading cases. The von Mises stress distribution indicated that the greatest effort area of tooth lies at the base of crown up to the gingival line with varying intensities in the different loading cases. The highest stress in the cortical bone was predominantly found around the cervical region of the tooth and lowest in the cancellous bone and periodontal ligament (PDL). The PDL is a soft tissue, and it could function as an intermediate cushion element which absorbs the impact force and uniformly transfers the occlusal forces into the surrounding bone. © 2012 Elsevier B.V. All rights reserved.
1. Introduction Recently, mechanical aspects of various advanced materials have been paid much attention [1–3]. Especially, mechanical behavior of biological structures is a common subject of scientific research. The stress results of such investigations offer the precise insight into the biomechanical properties of biological structures and are useful for predicting their behavior when subjected to loading. Although known, there are mainly three different ways in which stress analysis can be performed: analytical, experimental and computational. In fact the most important one is the computational, in which the stress analysis would seem to be the most natural way to approach this problem. The experimental process can be simulated and repeated on the computer and be observed in virtual prototyping. It is convenient to change the material or shape properties and obtain the new results. Many researchers have used the computer to analyze dental structures, including human teeth. The primary computational method used for stress analysis today is finite element analysis (FEA). Many researchers [4–6] have also used photoelastic techniques to understand stress distribution under various loading conditions. While analytical approaches are not available for complex dental structures, experimental approaches are expensive and time ⁎ Corresponding author. E-mail address: [email protected] (B.A. Bachir Bouiadjra). 0928-4931/$ – see front matter © 2012 Elsevier B.V. All rights reserved. http://dx.doi.org/10.1016/j.msec.2012.10.020
consuming. Due to irregular geometry, complex material properties and complicated loading conditions are involved in dental structures. With the increase in computational power, the use of finite element method (FEM) can help to simulate with a great accuracy the functioning of the human tooth. FEA has been widely used in engineering since the 60s [7–10]. They are an important tool in the understanding of the mechanical behavior of materials used in industry. However, in dentistry this kind of analysis is rather recent. Although the first article published by Farah et al. [11] on the subject dates back to 1973, this technique is still little used. That is mainly due to (i) the difficulty associated with the model elaboration, for they present different shapes depending on the tooth to be analyzed, and (ii) to the difficulty involved in obtaining the mechanical properties of the tooth's constituent materials: enamel, dentin, cementum, pulp, spongy bone, compact bone and periodontal ligament. Furthermore, little is known about the contact areas between such materials and their degree of influence on the mechanical behavior of the tooth as a whole. For any FEA to be performed a computer model of structure under investigation has to be created. In this method a geometric model is developed and a “mesh” is created by subdividing the geometry into rectangular or brick-shaped elements. In all FEA studies there are four sets of parameters that completely define the model: geometry, material behavior, loading and boundary conditions. Once the model is completely defined and meshed, a stress analysis is performed and
692
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
Fig. 1. CT scan mandibular bone.
stress distributions are obtained (usually in graphical form). Lin et al. [12] cited that FEM analysis could predict detailed mechanical responses of structures and alter the parameters in a more controllable manner, and therefore have become a popular analytical tool in dental biomechanical studies. In contrast to other methods involved in dental studies, once when a mathematical model is made, it is possible using the computer to simulate different stress applications and also change the shape and design of structures in numerous ways in order to gain more scientific data [13,14]. Evaluation of published literature showed that researchers have used two-dimensional (2D) models in their studies [15,16]. Korioth and Versluis [17] claim that depending on investigated structure and boundary conditions, 2D modeling may be justified as reasonable, especially when simplicity and efficiency are concerned. Other authors have used three dimensional (3D) models in their investigations [11,18]. Tooth fracture results directly from combined acting intraorally. Masticatory stresses, the amplitudes of these stresses depend on factors including gender, age, state of teeth, as well as the hardness of food. Masticatory forces are the greatest in the region of the first molars. There is little research regarding the mechanical behavior of natural teeth [13]. The majorities of the previous studies were interested on the behavior of dental implants. However, the knowledge areas of stress concentrations in a natural manner are important to predict the lifetime of these teeth. In addition this knowledge can help practitioners of dental implant when restoring mandibular molars to ensure proper operation of the implant. The aim of this study is to analyze the stress distribution in the human molar tooth
using a finite element model. This study can help to create patientspecific FE models based on occlusal contact records and morphological measurements of each patient to analyze the stress and strain distributions in the periodontal structures of the molars. We also aimed to highlight the zones of stress concentration in order to predict the eventual damage in human molar tooth.
1.1. Geometric model of the tooth–PDL–bone system The problem of biomechanical behavior of a complex structure with irregular geometry such as the tooth can be analyzed using the FEM. In order to perform the FE study one is obliged to create a digital model of the structure under investigation. The initial 3D model of the molar section from the mandibular bone structures was constructed based on computerized tomography (CT) scan technology (Fig. 1). The individual scans were processed in Rhinoceros 3.0 and SolidWorks 3D, where the final 3D solid model of the bone was created with a layer of cortical bone of 2 mm thickness, and cancellous bone. The human molar tooth model employed in this study was constructed primarily using computer tomography (CT) images, digital edge detection technique and computer aided design (CAD) methods. The periodontal ligament (PDL) represented a considerably small volume as 0.2 mm of the molar tooth system and is assimilated into the volume of the alveolar bone (Fig. 2).
2. Material models The tooth is composed primarily of 3 materials: the dentin, the enamel, the cementum. The cementum and the enamel represent a considerably small volume of the tooth and are assimilated into the volume of the dentin. The PDL being a highly soft material, the hard dentin deforms little with respect to the PDL when the molar is loaded. All the materials were presumed linear, elastic, homogeneous, and isotropic for the analyses as widely adopted in existing literature [19–22], and the mechanical properties were taken from the literature as shown in Table 1.
Table 1 Mechanical properties of materials used in model of mandibular molar.
Fig. 2. Three dimensional models of mandibular bone, PDL and molar tooth.
Parts
Constitutive equation
Elastic modulus (E) (GPa)
Poisson ratio (ν)
Molar tooth Periodontal ligament (PDL) Cortical bone Cancellous bone
Isotropic linear elastic
20 0.05 14.5 1.37
0.3 0.49 0.323 0.3
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
693
Fig. 5. Meshing in the vicinity of the ligament. Fig. 3. Boundary conditions.
Although PDL is viscoelastic in nature, the isotropic elastic properties were assigned as the load response lies within the linear elastic range [23]. Bone in this study is also modeled isotropically since it was already stated that isotropic models of the mandible were able to distinguish meaningful strain differences when replicating functional loading [24], which have been widely accepted by clinicians when evaluating patients [25].
• The most coronal plane of the crown is subjected to a load of 3 MPa in either the lingual–buccal or mesial–distal directions or a load of 10 MPa in coronal–apical direction. • The other surfaces are treated as free surfaces, i.e. zero loads. The vertical load of 10 MPa and horizontal load of 3 MPa were applied at the surface central in the occlusal face of the crown (Fig. 3).
2.1. Interface conditions The interface between the tooth and the ligament, as well as between the cortical and cancellous bone are treated as perfectly bonded interface. 2.2. Boundary conditions In order to define the boundary conditions, a 3D coordinate system is defined by three forces in the coronal–apical direction, lingual–buccal direction and mesial–distal direction. For the boundary conditions, three zones are presented: • The inferior plane of the mandibular bone is defined as having zero displacement.
2.3. Finite element model In this study, the commercial code Abaqus (6.11) was employed for linear static analysis. The mesh of the components is simplistic and consists of linear tetrahedron elements with four nodes (Fig. 4). Since the ligament experiences the largest deformations under load, it is necessary to mesh this volume into small elements (Fig. 5). The tooth and the bone are meshed with increasingly larger elements as the distance from the ligament increases, with the size of elements in contact with the ligament being defined by the elements of the boundary mesh. The mesh of the components is verified for use in a finite element stress analysis. The characteristics for the meshes of each component are presented in Table 2. 3. Results For analysis in all simulations, the von Mises stress was used. The distributions of this stress in the bone surrounding the PDL and molar tooth were investigated. The von Mises stress is a scalar variable that is defined in terms of all the individual stress components and, therefore, is a good representative of the state of stresses. It has been extensively used in biomechanical studies of bone [26–28]. The distributions of overall stress state for each component in our model were shown under effect of axial and horizontal loading in the coronal–apical, lingual–buccal and distal–mesial. A qualitative and quantitative analysis was performed, based on a progressive visual color scale, pre-defined by the software used, ranging from dark
Table 2 Size and number of elements used for the bone, ligament and molar tooth.
Fig. 4. Mesh using linear tetrahedron elements of (a) the tooth, (b) the ligament and (c) the alveolar bone.
Component
Size of element (mm)
No. of elements
Molar tooth Periodontal ligament (PDL) The mandibular bone
0.25 0.25 0.25–1.00
195,514 220,155 142,305
694
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
and bone, however, deform only marginally. In the apical–coronal view shown in Fig. 9 the strain field at the surface of the ligament is relatively homogeneous, and no region undergoes a particular deformation. The bone–implant interface was capable of withstanding and absorbing the stress during axial loading. 3.2. Alveolar bone In the alveolar bone, stress distribution was almost similar to that in the PDL, but the values of stress distributed in the alveolar bone were approximately 10 times larger than those in the PDL. Furthermore, the highest stress in the alveolar bone, as a whole, was concentrated in the cortical bone, around the PDL. Because of a great difference between the stress values in the cortical and cancellous bone, the stress distributions in these bone regions are shown separately for better visualization.
Fig. 6. Different t stress levels.
blue to red (Fig. 6). The maximum stress values in each component under different loading are shown in Fig. 11. 3.1. Periodontal ligament (PDL) Fig. 7 represents the von Mises stress distribution within the ligament. It was seen that the periodontal ligament underwent a maximum stress at the cervical region of its contact with the tooth and alveolar bone. The stresses gradually reduced as we move towards the middle part of the periodontal ligament. The Von Mises strain of the PDL shown in Fig. 8 indicates that it is principally the ligament that undergoes strain deformation. The tooth
3.2.1. Cortical bone The cortical bone also experienced stresses along the same lines as that of the periodontal ligament. It was seen that the maximum stress in the alveolar bone was found at the cervical region where the tooth comes in contact with the alveolar bone through the periodontal ligament (Fig. 10a). 3.2.2. Cancellous bone Because of its low modulus of elasticity, minimal stress was generated compared to the cortical bone. The maximum stress was concentrated at the base of the roots. This stress diminished in magnitude towards the coronal end of the roots (Fig. 10b). 3.3. Molar tooth When applying a tipping load on occlusal surface of the tooth model, a region of relatively high equivalent stress was found at the surfaces of the root (Fig. 11). The maximum value was detected on
Fig. 7. Distribution of stresses within periodontal ligament (PDL): (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
695
Fig. 8. Distribution of strains within periodontal ligament (PDL): (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
the cervical level of the roots. The molar tooth also experienced stresses along the same lines as that of the cortical bone.
4. Discussion The finite element model of the maxillary second molar tooth that included alveolar bone was investigated for analysis of the stress distribution [28]. Previously, several researchers [29–31] constructed FE tooth models using a series of slice images of a tooth and performed stress analysis during tooth movements. However, these FE models were developed as general tooth models with an average size and shape of the crown and root. Subsequently, in a previous study, an automatic
Fig. 9. Maximum elastic strain observed in the ligament.
modeling system from CT image was developed for computer-aided diagnosis [32]. Finite element models have their current origin and real use in mechanical engineering analysis and design. Biological applications have been successful where mechanical principles would be of the most interest; for example in modeling human joints [33]. In dentistry, models have been used to determine the stresses in different biologic structures, such as jaws, facial skeleton, dentition, periodontal ligament, temporomandibular joint [34–37] and different dental restorative materials, for example, implants, composites etc. [38,39]. Most of the surveyed FEM studies analyzed the biomechanical behavior of individual structures or materials, while we have tried to investigate interactions of stresses in the biomechanical system, representing the main elements of human masticatory system. The objective of this study was to evaluate the influence of axial and horizontal loads on stress distribution when the molar tooth submitted to occlusal loading. Even with the simplifications of considering the bone and molar tooth system to be homogeneous, linearly elastic and static load. The maximum von Mises stress values in the molar tooth, periodontal ligament and alveolar bone are shown in Fig. 12. In general, lateral occlusal loads (lingual–buccal and distal–mesial) significantly increased the stress values when compared with axial occlusal load (coronal–apical). Irrespective of the direction and magnitude of loading, it has been demonstrated that the highest stresses were observed firstly on the tooth, secondly in the alveolar bone and thirdly in the periodontal ligament. These findings are due to the different mechanical properties of each structure. The tooth resists to maximum amount of stress compared to any other component of the model. The probable reason could be associated to its elastic modulus (E = 20,000 MPa), which is approximately one time and half the elastic modulus of cortical bone (E = 14,500 MPa), 14 times the elastic modulus of cancellous bone (E = 1370 MPa) and 400 times the elastic modulus of periodontal ligament (E = 50 MPa). In this study, an applied loading to the crown surface involves a high stress concentration in the higher part of the fixing zone of the
696
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
Fig. 10. Distribution of stresses within alveolar bone: (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
tooth system in contact with the cortical bone, i.e., superior area of the cortical layer. These were due to: • The evidence of the surface area between the tooth and the cortical bone is much smaller than the surface area between the tooth and the cancellous bone. Moreover, the cortical bone is more than ten times stiffer than the cancellous bone. These are the reasons that high stress increments were found in the cortical bone.
• The intimate contact at the cortical bone and tooth interface, the loading applied to the crown of the tooth is directly transmitted to the cortical bone. • This suggests that great importance is to be attached to the contact of the tooth system with the cortical layer of bone. The graph in the following Fig. 13, describes the effect of acting vertical and horizontal loads. During vertical loading, stress generated within the cortical bone was the least as compared to the stress
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
697
Fig. 11. Distribution of stresses within molar tooth: (a) coronal–apical load, (b) lingual–buccal load, and (c) distal–mesial load.
generated during bucco-lingual and mesio-distal loadings. The reason being that the direction of load along the long axis of the tooth provides maximum cross-sectional area to withstand the stress. Indeed, we noted for a distal–mesial loading the highest stress concentration compared to the other loadings in the cervical areas of the cortical bone, the tooth, and the periodontal ligament. Fig. 13 illustrates this observation which is indeed not recorded for the cancellous bone. The latter being more sensitive to the compression loads. With our greater knowledge based on the realized study, this can be justified by the boundary conditions applied to the system
like by the wide form of the mandibular bone in the distal–mesial direction. Also, let us mention that the analysis carried out on only one molar tooth independently of the adjacent teeth on the dental arch, which generated the strongest stresses in the distal–mesial direction in the case of a single tooth. This justifies the importance of the replacement of the lost teeth by dental implants in order to minimize this type of stresses. 5. Conclusions The finite element method is the nearest possible method available today to simulate the oral cavity in vitro. It is a numerical method for addressing mechanical problems and therefore, is a powerful contemporary research tool. FE analysis provides a precise insight into the complex mechanical behavior of restored teeth affected by stress fields which are difficult to assess otherwise. Of particular importance is the possibility of examining the various parameters. The use of these theoretical engineering methods will certainly give answers to problems in restorative dentistry. Thus the results are practical and applicable, of clinical significance and reference value and give direction to experimental and clinical research. This initial FEM model has demonstrated that the computational modeling approach can be successfully used in the biomechanical study of stresses distribution in the constituent parts of the masticatory system. The 3D FEM analysis of tooth geometry characteristics and stress relationship suggested that von Mises stresses might increase with the increase of the distal–mesial loading. This explains why teeth are more predisposed to occlusal trauma. Acknowledgment
Fig. 12. Histograms of comparison of von Mises stresses for each component under the different load directions.
The authors extend their appreciation to the Deanship of Scientific Research at King Saud University for funding the work through the research group no. RGP-VPP-035.
698
A. Merdji et al. / Materials Science and Engineering C 33 (2013) 691–698
Fig. 13. Distribution of cervical stresses within cortical bone under the different load directions.
References [1] W. Jianfeng, C. Qunfeng, Z. Tang, J. Chem. Soc. Rev. 41 (2012) 1111–1129. [2] C. Zhenguo, Z. Xiqi, X. Bingjia, Z. Xie, M. Chunping, Z. Yi, L. Siwei, X. Jiarui, J. Chem. Soc. Rev. 41 (2012) 3878–3896. [3] K. Ariga, T. Mori, J.P. Hill, J. Adv. Mater. 24 (2012) 158–176. [4] J.W. Farah, R.G. Craig, D.L. Sikarskie, J. Biomech. 6 (1973) 511–520. [5] T. Yamada, J. Sugawara, H. Itoh, T. Sasaki, E. Umezaki, in: 4th Asian Implant Orthodontics Conf, 2005, pp. 22–23. [6] T. Yamada, J. Sugawara, H. Itoh, T. Sasaki, K. Sasaki, E. Umezaki, in: International Congress Series, 1284, 2005, pp. 77–78. [7] M.J. Turner, R.W. Clough, H.C. Martin, L.J. Topp, J. Aeronaut. Sci. 23 (1954) 805–823. [8] O.C. Zienkiewicz, Finite Element Method, 3rd ed. McGraw-Hill, London, 1977. [9] M. Ameen, Computational Elasticity, Theory of Elasticity and Finite and Boundary Element Methods, Alpha Science International Ltd., Harrow, U.K., 2005. [10] S. Rao, The Finite Element Method in Engineering, 4th edition Butterworth Heinemann, USA, 2004. [11] J.W. Farah, R.G. Craig, J. Dent. Res. 54 (1975) 255–261. [12] C.L. Lin, C.H. Chang, C.H. Wang, C.C. Ko, H.E. Lee, J. Oral Rehabil. 28 (2001) 517–525. [13] B. Dejak, A. Mlotkowski, M. Romanowicz, J. Prosthet. Dent. 90 (2003) 591–597. [14] J.A. Hobkirk, H.W. Wiskott, Clin. Oral Implants Res. 17 (2006) 52–54. [15] J.S. Rees, J. Oral Rehabil. 29 (2002) 188–193. [16] M. Tanaka, T. Naito, M. Yokota, M. Kohno, J. Oral Rehabil. 30 (2003) 60–67. [17] T.W.P. Korioth, A. Versluis, Crit. Rev. Oral Biol. Med. 8 (1997) 90–104. [18] P. Ausiello, A. Apicella, C.L. Davidson, Dent. Mater. 18 (2002) 295–303. [19] J.S. Rees, M. Hammadeh, D.C. Jagger, Eur. J. Oral Sci. 111 (149–154) (2003). [20] H. Spiekermann, Color Atlas of Dental Medicine: Implantology, Thieme, New York, 1995.
[21] O.A. Abu-Hammad, A. Harrison, D. Williams, Int. J. Oral Maxillofac. Implants 15 (2000) 559–564. [22] B.H. Choi, Int. J. Oral Maxillofac. Implants 15 (2000) 193–196. [23] G. Pietrzak, A. Curnier, J. Botsis, S. Scherrer, A. Wiskott, U. Belser, Comput. Methods Biomech. Biomed. Eng. 5 (2002) 91–100. [24] I. Ichim, M. Swain, J. Kieser, J. Dent. Res. 85 (2006) 638–642. [25] U. Lekholm, G. Zarb, in: P.I. Branemark, G.A. Zarb, T. Albrektsson (Eds.), Tissueintegrated Prostheses, 2 ed., Quintessence, Chicago, 1987. [26] P. Kowalczyk, Dent. Mater. 25 (2009) 83–91. [27] P. Magne, Dent. Mater. 23 (2007) 539–548. [28] P. Magne, D.T. Tan, J. Adhes. Dent. 10 (1) (2008) 49–56. [29] M.L. Jones, J. Hickman, J. Middleton, J. Knox, C. Volp, J. Orthod. 28 (2001) 29–38. [30] P.D. Jeon, P.K. Turley, B.H. Moon, K. Ting, Am. J. Orthod. Dentofacial Orthop. 115 (1999) 267–274. [31] H. Qian, J. Chen, T.R. Katona, Am. J. Orthod. Dentofacial Orthop. 120 (2001) 272–279. [32] K. Maki, N. Inou, A. Takanishi, A.J. Miller, Orthod. Craniofac. Res. 6 (2003) 95–101. [33] J.J. Liau, C.K. Cheng, C.H. Huang, W.H. Lo, Clin. Biomech. 17 (2002) 140–146. [34] P.M. Cattaneo, M. Dalstra, B. Melsen, Am. J. Orthod. Dentofacial Orthop. 123 (2003) 367–373. [35] M.D. Gross, G. Arbel, I. Hershkovitz, J. Oral Rehabil. 28 (2001) 684–694. [36] S. Gomes de Oliveira, P.I. Seraidarian, J. Landre, D.D. Oliveira, B.N. Cavalcanti, J. Oral Rehabil. 33 (2006) 874–880. [37] S.R. Toms, A.W. Eberhard, Am. J. Orthod. Dentofacial Orthop. 123 (2003) 657–665. [38] I. Akpinar, N. Anil, L. Parnas, J. Oral Rehabil. 27 (2000) 538–539. [39] P.L. Boschian, S. Guidotti, R. Pietrabissa, M. Gagliani, J. Oral Rehabil. 33 (2006) 690–697.
