Finite element analysis and validation of the critical parameters influencing the mechanical behaviour of tibia bone with patient-specific implant for proximal end fracture.
Abstract: The common problems like discomfort and loosening of the implant with the currently available pre-fabricated implants can be reduced by designing patient-specific implants. In this paper an attempt has been made to optimize the mechanical behaviour of tibia bone with patient-specific implant for proximal end (B1 type) fracture by performing statistically designed experiments (DoE) using numerical analysis (FEA). Three parameters viz. material, thickness and position of implant were considered in this study. The CAD model of tibia bone and patient-specific implant were developed using the CT image. Numerical analysis as per Taguchi's [L.sup.9]([3.sup.4]) orthogonal array and the validation of optimum condition were performed on the bone-implant assembly using ANSYS 10.0. Based on the ANOVA, it is evident that the position of implant is more significant than the thickness and implant material.
Article Type: Report
Subject: Tibia (Care and treatment)
Finite element method (Research)
Implants, Artificial (Patient outcomes)
Prosthesis (Patient outcomes)
Authors: Devika, D.
Gupta, N. Srinivasa
Pub Date: 01/01/2012
Publication: Name: Trends in Biomaterials and Artificial Organs Publisher: Society for Biomaterials and Artificial Organs Audience: Academic Format: Magazine/Journal Subject: Health Copyright: COPYRIGHT 2012 Society for Biomaterials and Artificial Organs ISSN: 0971-1198
Issue: Date: Jan, 2012 Source Volume: 26 Source Issue: 1
Topic: Event Code: 310 Science & research
Product: SIC Code: 3842 Surgical appliances and supplies
Geographic: Geographic Scope: India Geographic Code: 9INDI India
Accession Number: 304842704
Full Text: Introduction

Tibia bone is one of the most important weight bearing and supporting element in the musculoskeletal system. Lower extreme limb is the second most frequent injury region. Over 60% of pedestrian accidents suffer from some kind of lower limb injury and often leads to long-term disability and impairments [1].

The articulating surface of a prefabricated implants are of generic shape and causes the problems like loosening of implant components, bone remodeling and bone loss due to stress concentrations under the load. The bond between bone and implant is achieved with the aid of bone cements or bent the implant according to bone anatomy or resurfacing the bone for implant during the surgery. This may be compromised either through deterioration of the bone cement itself or the remodeling of bone that takes place at the bone-implant interface. The gradual loosening and eventual failure of the implant is due to the progressive resorption of bone secondary to stress shielding and host inflammatory responses associated with the presence of wear debris around the implant [2]. In order to improve the bone fixation, orthopaedic prostheses manufacturers have developed a variety of surface treatments and coatings which are designed to promote better transfer of load between the implant and surrounding bone [3]. The biomechanics of human body deals with body movements with forces that some parts of the human body exchange internally or externally and with the effects that these movements and forces on the organs and on the tissues that form them [4].

Patient-specific implants are necessary for those situations when the standard size is not suitable. These are usually complex cases involving trauma or disease resulting in bone deformity or loss [5]. It is produced on a prescription basis and is unique for each patient. This eliminates the need to use bone harvested from a second site and time-consuming modification of off-the-shelf devices during the surgery [6].

Finite element Analysis (FEA) is one of the most widely used engineering analysis techniques in the world today. It is used to simulate how a physical system will respond to expected loading conditions. FEA is based on the fundamental physical principles that govern the behaviour of these physical systems. Since the biological systems must obey the same fundamental physical principles, the physical response of biological systems to known loading conditions can also be predicted using FEA. It is an accepted theoretical technique used in the solution of medical problems [7]. The distribution of forces in bone and implant has been investigated in several studies [5]. FEA modeling not only can simulate complex geometric shapes and material properties, but also can simulate various boundary conditions, which are very difficult to replicate in experiments [6].



Biomechanical models of bone are usually formulated as linear elastic problems, solved with static FEA. FEA is a computer-based method of stress analysis, which is used when the shapes, numbers or types of materials and the loading conditions are too complicated to yield to analytical methods [8]. In many aspects, the mechanical environment in bones is considered a major factor influencing biological processes and therefore vital for surgical procedures, healing processes as well as therapeutic regimens [9].

Design of experiments (DoE), based on Taguchi methods are used extensively in research for carrying out statistically designed experiments and predicting the optimum process parameters for the selected responses. Evaluation of the statistical significance of individual process parameters and the ability to find the interaction between factors are the additional benefits of performing statistically designed experiments. Statistical data analysis techniques are increasingly being relied upon to translate experimental data into useful knowledge [8]. Analysis of variance (ANOVA) yields the relative significance of factors in terms of their percentage contribution to the response characteristics.

Materials and Methods

Modeling of bone and patient-specific implant

Computed Tomography (CT) imaging is a useful method together with three dimensional physiological data such as geometry and density of bone in vivo. This image data can be used in manual segmentation of bone to generate idealized surfaces for creating finite element models. The Materialise's Interactive Medical Image Control System (MIMICS) (MIMICS 12.0, Materialise, Leuven, Belgium), an image processing software package is used to convert the CT data into a series of contours to simulate outer cortical and intramedullary cancellous surfaces by segmentation and 3D rendering objects as shown in Fig. 1. The input data of the modeling process represented by tomographic slices in Digital Image and Communications in Medicine (DICOM) format belongs to a 23 year old adult male with a body weight (BW) of 80Kg. For extracting the cortical and trabacular tibial bone features, threshold value was adjusted from 226 to 1956 Hounsfield units in the MIMICS. Then region growing was used to separate the region of interest (ROI) from the selected object.


Then Med CAD module in the MIMICS was used to export the 3D model data from imaging system to the CAD system as IGES file format. The transfer from solid to surface was done by the polylines, which determine the cortical and trabacular contour. For each section polylines have been generated. This IGES format is imported into CAD software CATIA (CATIA V5R15, Dassault systems, France) as polylines. CATIA is used to process the data in order to create Non Uniform Rational B-Splines (NURBS) surfaces, which are easily handled by Finite Element software [10]. After editing the data such as blending, joining, smoothing, filling gaps, etc. on the splines, the curves are wrapped as closed surfaces as shown in Fig. 2.

CAD model of the bone can be used as the base for implant design, so that the original shape of the articulating surface can be preserved. To take full advantage, it was decided to optimize the bone-implant interface by maximizing the even distribution of stress to minimize the problems faced while using the prefabricated implant. The bone-implant interface surface is designed to mimic the articulating surface as shown in the Fig. 3. The offset distance was kept uniform in order to create an implant with constant wall thickness.

Geometry interfacing and reconstruction

The 3D solid CAD model was then imported into HyperMesh (HyperMesh 9.0, Altair, USA), a preprocessing software, to clean up the imported geometry containing surfaces with gaps, overlaps and misalignments. HyperMesh provides high-quality mesh generation by eliminating misalignments and holes. By suppressing the boundaries between adjacent surfaces, the overall meshing speed and quality is improved. The size of the meshed element is 3 mm. Element type and Boundary conditions were applied to these surfaces for future mapping to underlying element data. FE model was developed for the entire length of the Tibial bone measured 415 mm in length as shown in Fig 4.


The model was divided into three regions named as thick shaft region as cortical bone, bone marrow inside the cortical as cancellous and spongy region in proximal and distal end of the bone as trabacular. During normal walking stance phase at full extension the peak load acting on the human tibial region is 3 times body weight of the person [11]. Hence, a loading condition of 2400 N (BW 80 kg) is applied on the proximal region which is splitted into 60 % (1470 N) of weight in the medial region and 40 % (980 N) in the lateral region of the model. The load is approximately distributed in the middle of the medial and lateral regions. The linear elastic, orthotropic and heterogeneous material property is assigned for the cortical region [12]. The linear elastic, isotropic and homogeneous material property is assigned for both trabacular and cancellous bone regions [13]. Poisson's ratio (o) for all the three regions is considered as 0.3. The degrees of freedom of the nodes in the distal end of the bone were totally constrained. The volumetric mesh obtained and the resulting finite element mesh of the tibial composed of 14,752 nodes and 67,764 elements.

Finite Element Analysis

The preprocessed model is imported into Finite Element Analysis software, ANSYS 10.0 (ANSYS 10.0, ANSYS Inc., Canonsburg, PA, USA) for post processing and solved. The interaction between the two fractured pieces is defined as 'bonded' augmented Lagrange contact without separation after contact. The contact element 'CONTA174' of 3D, 8node and surface-to-surface contact is used to represent contact and sliding between 3D 'target' surfaces and a deformable surface defined by this element. The contact behaviour of (KEYOPT (12) = 3) models 'bonded' contact, in which the target and contact surfaces are bonded in all directions for the remainder of the analysis in ANSYS. In order to simulate the effects of the threaded connections of the screws, the nodes on the medial side of the bone and the corresponding nodes on the holes of the implant were coupled using multipoint constraints with default parameters of the software. The screw hole near the fracture site is not coupled, as this may lead to further fracture when stressed. Pre Conjugate Solver (PCS) was used during the post processing of FEA.

Design of Experiments

Selection of process parameters

The objective of this study is to optimize the mechanical behaviors (responses) like displacement, stress and strain of bone-implant assembly. For the maximum comfort of the patients after the surgery for fixing the implant, it is desirable to have minimum displacement, stress and strain of bone-implant assembly. In the current study, three parameters viz. implant material, implant thickness and position of implant were considered. Table 1 shows the parameters and their levels selected for the study. Table 2 shows the [L.sub.9]([3.sup.4]) orthogonal array (OA) selected for designing the experiment trials with the corresponding responses obtained from ANSYS 10.0. and the overall evaluation criterion (OEC) values.

Overall Evaluation Criterion (OEC)

Multiple objectives that require evaluation by different criteria of evaluations are quite frequent in engineering projects [14]. For the "smaller is better Quality characteristic (QC)", formula (i) was used for the calculation of OEC.

[summation] (Best value - Test value) x (Relative Weighting)/(Reference Number) .. (1)

In the formula above, the relative weightings 33%, 33% and 34% were considered for displacement, stress and strain of bone-implant assembly respectively. Test value refers to the response value of that trial. Reference number is the absolute value of the difference between the best and worst values in that particular response.


Results and Discussion

Prediction of optimum condition

The responses considered were optimized using the "smaller is better" quality characteristics. OEC has been formulated using the results of individual responses and optimum condition is predicted by performing standard analysis using the average effects. The main effects based on the difference between the average effects at different levels of each parameter have been calculated using the OEC values of each trial. The average effects for various parameters are shown in the Fig. 5 and Table 3. From the main effect plots, the patient-specific implant made of Co-Cr with 2.5 mm thickness fixed at antero-lateral position was identified as the optimum parameter setting A3, B3 and C2.

Analysis of variance (ANOVA)

ANOVA has been performed to find out the relative percentage influence of parameters under study. The ANOVA results are shown in the Table 4.

Among the three parameters, the relative influence of implant material is the least with 0.792% and position of the implant has the most influence with 87.46% on the total variation. Based on the relative percentage influence of materials, it is evident that using Ti or SS in the place of Co-Cr will not significantly affect the optimum performance expected. Hence it was decided to perform validation of the optimum condition with Ti and SS also.


The validation results are shown in the Table 5. From the Table 5, it is evident that the parameter setting with Ti as implant material at 2.5 mm thickness fixed at anterolateral position results in the minimum stress and strain. Although the displacement of Ti bone-implant assembly is slightly higher than Co-Cr and SS, the value is well within the acceptable limit of 10 mm. [15]. Hence patient-specific implant fabricated using Ti with 2.5 mm thickness fixed at antero-lateral position for B1 type fracture will result in the minimum displacement, stress and strain.


The complex geometry of the human tibia bone and implant were modeled from the CT images using CATIA. The mechanical behaviors of tibia bone with patient-specific implant for B1 type fracture were optimized by performing statistically designed experiments using ANSYS. ANOVA revealed that among the three parameters, the relative influence of implant material is the least with 0.792%, and position of the implant has the most influence with 87.46% on the total variation. The optimum parameter setting with Ti as implant material at 2.5 mm thickness fixed at antero-lateral position resulted in the minimum displacement, stress and strain. The selection of patient specific implants for enhanced patient comfort can be achieved by integrating CAD, FEA and DoE techniques.


[1.] Amein Alsuezi, "Development and validation of an anatomically based plastic-kinematic finite element model of the knee joint for vehicle pedestrian collision injury investigation", International journal of Science Res., 15, 2005.

[2.] John Alan Hunt, Jill T. Callaghan, Chris J. Sutcliffe, Rhys H. Morgan, Ben Halford Richard A. Black, "The design and production of Co-Cr alloy implants with controlled surface topography by CAD-CAM method and their effects on osseointegration", journal of Biomaterials 26, 5890-5897, 2005.

[3.] Wei Sun, Pallavi Lal, "Recent development on computer aided tissue engineering", Journal of Computer methods and programs in biomedicine, 67, 85-103, 2002.

[4.] Marco Viceconti, Debora Testi, Fulvia Taddei, Saulo martelli, Gordon J. Clapworthy and serge van Sint Jan, "Biomechanics Modeling of the Musculoskeletal apparatus: Status and Key issues", Proceedings of the IEEE, 94, 4, 2006.

[5.] Harryson Ola LA, Yasser A Hosni and Jamal F Nayfeh, "Custom-designed orthopedic implants evaluated using finite element analysis of patient-specific computed tomography data: femoral-component case study", BMC Musculoskeletal disorder, 8, 2007.

[6.] Singare. S, "Customized design and manufacturing of chin implant based on Rapid Prototyping" Journal of Rapid Prototyping, 11/2, 113-118, 2005

[7.] Ming-Yih Lee, Chong-Ching Chang, Chao-Chun Lin, Lun-Jou Lo and Yu-Ray Chen, "Custom implant design for patients with cranial defects", IEEE Engineering in Medicine and Biology, 38-44, 2002.

[8.] Fazilat H. Dar, Judith R. Meakin and Richard M. Aspden, "Statistical methods in finite element analysis", Journal of Biomechanics 35, 1155-1161, 2002.

[9.] George N. Duda, Erich Schneider and Edmund Y. S. Chao, "Internal forces and moments in the femur during walking", journal of Biomechanics, 30/9, 933-941, 1997.

[10.] Petzold. R, H.-F. Zeilfofer and W.A. Kalender, "Rapid Prototyping technology in medicine--basics and applications", Journal of Computerized Medical Imaging and Graphics 23, 277-284, 1999.

[11.] Harrington, I.J., "A Bioengineering Analysis of Force Actions at the Knee in Normal and Pathological Gait", Journal of Biomech. Engineering, 11, 167-172, 1976.

[12.] Taylor W.R, Roland. E, Ploeg. H, Hertig. D, Klabunde. R, Warner. M.D, Hobatho. M.C, Rakotomanana. L and Clift. S.E, "Determination of orthotropic bone elastic constants using FEA and modal analysis", Journal of Biomechanics, 35, 767-773, 2002.

[13.] Rho. J.Y, Hobatho. M.C and Ashman. R.B, "Relations of mechanical properties to density and CT numbers in human bone", Journal of Medical Engineering Physics, 17, 347-355, 1995.

[14.] Ranjit K. Roy, "Design of Experiments using the Taguchi approach: 16 steps to product and process improvement", New york, Wiley--Interscience 2001, 54.

[15.] EI-Asfoury M.S. and EI-Hadek M.A, "Static and Dynamic three dimensional finite element analysis of pelvic bone", International journal of Mechanical, Industrial and Aerospace Engineering, 2-4, 2008.

D. Devika, N. Srinivasa Gupta

Division of Manufacturing Engineering, School of Mechanical Engineering and Building Sciences, VIT University, Vellore, India

Corresponding author:

Received 26 July 2011; Accepted 7 February 2012; Available online 8 February 2012
Table 1: List of process variables and their levels

Parameters          Level 1        Level 2           Level 3

Implant Material    Titanium   Stainless Steel   Cobalt-Chromium
(A)                   (Ti)          (SS)             (Co-Cr)

Implant thickness      2             2.2               2.5
(mm) (B)

Position of the     Lateral    Antero-lateral          --
implant (C)

Table 2: [L.sub.9] ([3.sup.4]) OA with responses and OEC

                 INPUT PARAMETERS

S. NO     Implant    Material     Position
          material   thickness   of implant

Trial 1      1           1           1
Trial 2      1           2           2
Trial 3      1           3           1
Trial 4      2           1           1
Trial 5      2           2           1
Trial 6      2           3           2
Trial 7      3           1           2
Trial 8      3           2           1
Trial 9      3           3           1


S. NO     Displacement   Stress    Strain     OEC
              (mm)        (MPa)

Trial 1      2.322       235.576   0.00608   88.44
Trial 2      2.124       185.725   0.00388   23.99
Trial 3      2.229       185.476   0.00616   62.91
Trial 4      2.154       254.164   0.00632   85.39
Trial 5      2.124       228.064   0.00635   73.41
Trial 6      1.908       168.02    0.0039    0.26
Trial 7      1.946       211.711   0.00392   20.03
Trial 8      2.094       236.951   0.00638   74.82
Trial 9      2.059       202.933   0.00641   59.41

Table 3: Average effects

Parameters   Average effect    Average effect    Average effect
             at level 1 (L1)   at level 2 (L2)   at level 3 (L3)

Material         58.446             53.02            51.419
Thickness         64.62            57.406             40.86
Position         74.063            14.759              --

Table 4: ANOVA results

Parameters   DOF      S          V       F - Ratio     S'        P%

Material      2     81.381     40.69       4.595     63.671    0.792
thickness     2    890.362    445.181     50.273     872.651   10.864
Position      1    7033.775   7033.775    794.307    7024.92   87.46
Error         3     26.565     8.855                           0.884
Total         8    8032.085                                     100

DOF--Degrees of freedom; S--Sums of squares; V--Variance; S'--Pure
sums of squares; P% - Relative percentage of influence

Table 5: Validation results of optimum condition

Description of        Displacement   Stress    Strain
                          (mm)        (MPa)

A3 B3 C2 (Predicted      1.876       173.146   0.00391
optimum condition)

A1 B3 C2                 2.067       161.694   0.00388

A2 B3 C2                 1.908       168.02    0.0039
Gale Copyright: Copyright 2012 Gale, Cengage Learning. All rights reserved.