Mathematical Modeling of Thoracolumbar Spine using ANSYS

Transcription

1 Mathematical Modeling of Thoracolumbar Spine using ANSYS Lee Kim Kheng, Qiu Tian Xia, Teo Ee Chon, Ng Hong Wan, Yang Kai Abstract NANYANG TECHNOLOGICAL UNIVERSITY Over the years, finite element method has not only successfully evolved as surrogate tool, but also become useful adjunct to biomechanical studies as compared to other models; animal, physical and cadaveric. However, the finite element model must be accurately represented in these aspects; anatomy, material properties of the spinal components, boundary and loading conditions, and validated against appropriate experimental data. In this paper, we present how an anatomically accurate and detailed finite element model for an intricate thoracolumbar spine was accomplished in ANSYS from pre-processing to post-processing stage. Having the whole finite element model built and defined under ANSYS allows for ease of use between the stages and minimum data interchangeability problems. The digitized point, extracted by FaroArm, from embalmed cadaveric spine was imported into the F.E software, of which serves as keypoint for building volume mesh using bottom-up approach. The predicted results from the finite element model were validated under compression, flexion, extension, lateral bending and torsion and are found to correlate well with experimental data. The validated finite element model could then be a useful analysis tool in predicting intrinsic parameters and in vivo behaviors so as to understand clinical and biomechanical phenomena. Introduction For the past two decades, the finite element (FE) applications to thoracolumbar spine for biomechanical and clinical studies have resulted in better understanding of injury mechanisms as well as assessing spinal pathologies. A geometrically accurate, detailed and validated FE model will be able to provide intrinsic parameters (eg, stress distribution, strain, etc) in all constituent elements, in which are undetermined from experimental studies. Furthermore, it is capable of simulating clinically-related biomechanical behaviour and would increase our insight to delineate injury mechanisms and supplement biomechanical/clinical studies. To-date, many previous FE models of the thoracolumbar spine have over-simplified the geometry and material properties of their elements, thereby yielding results limited generalization. But it is so crucial to achieve accurate geometrical representation for the FE model in simulating the biomechanical behaviour of the spine as surface geometry of the vertebrae greatly defines the motion and its biomechanical response. Current predominant method used in generating FE thoracolumbar mesh makes use of Computer Tomography (CT) scans obtained at 1mm intervals, followed by digitizing the scans using imaging software and imported into pre-processor software (eg Page 1 of 7

2 PATRAN, PDA Engineering, Costa Mesa, CA) to reconstruct the three-dimensional geometry and mesh of the motion segment. Alternatively, the three-dimensional anatomy of the vertebrae obtained from quantitative-morphology literature is also used for FE construction. Nevertheless, the load-sharing and stress distribution predicted by the model, developed using the foregoing methods, may not be realistic due to coarse mesh and over-simplification of the vertebral geometry especially articulating surfaces of facets. Therefore, this paper would focus on how the anatomically accurate FE thoracolumbar spine being developed in commercially available finite element code, ANSYS, for volume and mesh construction. The acquisition process was done using an accurate and flexible digitizer, rather from CT scans, and has been presented elsewhere [1,2]. Geometrical, material and contact nonlinearity were also incorporated herein to predicting nonlinear responses of the motion segment under various loadings. Lastly, the developed FE model was validated against experimental studies under compression, flexion, extension, lateral bending and torsion to verify its accuracy in predicting in-vitro behaviour of the motion segment. Methods And Materials Modeling The acquisition process using direct digitization process would be briefly presented here. The main geometry of actual cadaveric specimen, which was free from spinal abnormalities, was being digitized using a highly accurate digitizer, FaroArm, as shown in Figure 1a. Because of its multi-axis arm, the digitizer has provided the needed flexibility in extracting the geometrical data of the intricate specimen in terms of point data. Figure 1b shows the point data of main cross-sections of L2 vertebra being captured by the FaroArm to be inputted for subsequent process. The coordinates of the point data were accordingly stored in a universal graphics data format (IGES) and imported into ANSYS. A. B. Figure 1 A - FaroArm, B Point cloud of L2 vertebra Page 2 of 7

3 The first step to the modeling of lumbar spine was to spell out the modeling objectives, determine the appropriate approach in building the model and choose appropriate element type for the FE model before initiating ANSYS. Here, a bottom-approach was used to building up the FE model. The captured points, deemed as keypoints, are used to define vertices of the captured cross section of the specimen. These are the "lowest-order" solid model entities and are used to define the "higher-order" solid model entities (that is, lines, areas, and volumes). In order to generate a cubic line representing the edges, the command BSPLIN was used to form a spline fit to these series of keypoints. Since mapped mesh was adopted for building the model and could only contain hexahedron elements, the line was divided into four lines by using LDIV command in order to form areas bounded by these lines for every cross sections. The divided lines of each cross section become guiding lines for which an area could be generated by skinning a surface through the lines using command ASKIN. With the shape of a brick, a volume bounded by existing 6 areas was generated using VA command. The foregoing steps were done to meet the requirement of the volume mapped meshing. These surface areas were visually inspected and compared occasionally with the actual vertebra for any further modifications to be made to ensure geometric integrity. Figure 2 shows a volume formed using this procedure. Figure 2 Volume formed by six bounded area In order to connect bony structures (for example, facet to lamina), the affected area of the volume was divided accordingly using ASBL command, followed by the use of command ACCAT to concatenate multiple, adjacent areas (the input areas) into one area (the output area) in preparation for the mapped meshing. The FE mesh of hexahedron elements was then obtained by discretising the solid model using the mapped mesh technique. The mesh exhibits a regular pattern with obvious rows of elements. In this study, eight-noded isoparametric solid elements (Solid45), instead of four-noded tetrahedron solid elements, were chosen to model the motion segment with finite elements. There is the often-held position that quadrilateral and Page 3 of 7

4 hexahedral shaped elements have superior performance to triangle and tetrahedral shaped elements when comparing an equivalent number of degrees of freedom. Use of hexagonal elements can also vastly reduce the number of elements and consequently analysis and post-processing times (Cook, 1997). In addition, hexagonal and quadrilateral elements are more suited for non-linear analysis as well as situation where alignment of elements is important to the physics of the problems, such as in the interverterbral disc where the fibers are oriented at ± 30 to the horizontal plane. All solid components including cortical and cancellous bone, endplates, annulus ground substance and posterior elements were simulated by a total of 8581 eight-node brick elements. The annulus fibers were simulated by three-dimensional (3D) cable elements that sustained tension only. The nucleus pulposus was modeled as an incompressible inviscid fluid by having a possion s ratio close to 0.5 and Young s modulus of 1 MPa. I Geometrical Nonlinearity To account for geometrical non-linearity exhibited by intervertebral disc, the annulus was modeled as a composite material comprising a series of fiber bands embedded in ground substance around nucleus as shown in Figure 3. It was assumed to consist of 3 consecutive laminar layers. In each layer, annulus fibers were oriented on average at ±30º to the endplate. Figure 3 - Collagen fiber arrangement in the annulus fibrosus layer in the finite element analysis. Contact Nonlinearity In order to appropriately model the changing areas of contact of facet articulating surface with increments in loading, facet articulations were simulated by sliding surface contact elements (3-D, 4-noded, lower-order quadrilateral element: CONTA173 and Targe170) that assumed frictionless. The pair of contact surface in each facet joint was assumed to be covered with cartilage material (0.5mm thick). Page 4 of 7

5 Material Nonlinearity All material properties were assumed to be linear except ligaments, which derived nonlinear stress-strain behavior from the experimental studies. The behavior was described by a piece-wise linear stress-strain curve using MELAS option. Figure 4 shows the finite element model of L2/L3 structure, which consists of about 8,000 solid 8- noded elements, 800 cable elements with 30,000 DOFS. Figure 4: FE Model of L2/L3 Segment Figure 4 Finite Element Model of L2-L3 model Results The predicted results from the FE model were validated under compression, flexion, extension, lateral bending and torsion and are found to correlate well with experimental data. For compression, all nodes pertaining to the bottom surface of the L3 vertebral body and spinous process were fixed, and a uniform axial compressive displacement (1.5mm) was applied in 6 increments to the top surface of the L2 vertebral body (displacement control). At each increment, the equivalent axial force was obtained by extracting the total reaction force on the constrained nodes at the L3 bottom surface and spinous process. For moment loadings, the model was preloaded with a compressive force of 400 N, representing the upper body weight of normal human subject. The moment was distributed as forces to the nodes on superior surface of top vertebra via RBE3 command, producing a pure moment with no net axial load. The entire inferior surface of bottom vertebra was fixed in all the three directions. The moment loads were increased incrementally from zero to predetermined maximum values (15 Nm). Page 5 of 7

6 Under compressive load, the predicted force-displacement curve was observed to be nonlinear and exhibited stiffening behaviour with increasing load, as shown in Figure 5. Figure 6 shows the overall responses predicted by the L2-L3 FE model under the different load configurations. The model predicted that the L2-L3 segments were least flexible in torsion and most flexible in flexion Axial Compressive Force (N) Displacement (mm) Figure 5 Axial compressive force versus axial displacement Flexion Lat-Bending Degree Extension Torsion Moment (Nm) Figure 6 Comparison of predicted results under various moment loadings Page 6 of 7

7 Conclusion In this paper, we show how the FE model of L2-L3 lumbar spine being developed in ANSYS for volume and mesh construction. Geometric, contact and material nonlinearities were incorporated into the FE model. This procedure has also been extended to thoracic spine for modeling. The model replicates the actual geometry of L2 and L3 vertebrae. The model included the cortical bone, cancellous core, endplate, lamina, pedicle, transverse process, and spinous processes of the vertebrae; the annulus fibrosus and nucleus pulposus of the intervertebral discs; the articular facet joints; and the anterior and posterior longitudinal ligaments, interspinous ligaments, capsular ligaments transverse ligaments, and ligamentum flavum. The predicted results yielded close correlation with biomechanical studies under compression, flexion, extension, lateral bending and torsion. Furthermore, with the solid geometry built in ANSYS and followed by volume mesh therein, the whole process lessens data interoperability problems, ensures geometry integrity and increases suitability for successful simulations. References 1) K. K. Lee, T. X. Qiu, E. C. Teo, 3-D finite element modeling of lumbar spine (L2/L3) using digitizer, International Workshop on 3D Digitization, Singapore, 25 Feb, ) E. C. Teo, K. K. Lee, An accurately represented finite element model of lumbar motion segment (L2-L3), Proceedings, International Conference on Biomedical Engineering, Kuala Lumpur; 2002, p ) R. D. Cook, Finite element modeling for stress analysis, John Wiley & Son, 1995, Canada. Page 7 of 7