Studying the Fracture Strength of an Analogue Tibia with FEA

Plates and screws are common orthopedic devices used to stabilize fractured bones. When this hardware is removed, holes remain where the screws were located creating stress concentrations that can result in re-fracture.

This article is based upon a study conducted by Kimberly Reuters from the Center of Innovation for Biomaterials in Orthopaedic Research, National Institute for Aviation Research and others on using a FE model to simulate experimental research evaluating the torsional fracture strength of an analogue tibia with screw holes. Seven configurations of the FE model were analyzed, and the FE results were compared against the experimental data and between the different FE configurations. The objectives of the study were: To develop a FE model to simulate an ultimate torsional test of the analogue tibia with three screw holes; To investigate how long bone torsional fracture is affected by holes and rotation direction; and investigate how the FE results are affected by changes to the failure model, element size, and simplification of the model’s geometry.

The methodology used in this study is shown in Figure 1. A FE model is developed using the geometry of a human tibia, and the boundary conditions and loads applied are based on the interpretation of an experiment. The computational results are compared with those from the experimental torsion tests on the analogue tibia to validate the model, and then a parametric study is conducted on the model to study the effect of several parameters, including the existence of the screw holes, fracture limit, element size, rotational direction, and the simplification of the model geometry.

Figure 1. Computational and experimental methodology

Overview of Experimental Tests and Interpretation into a FE Model
Experimental torsion testing of the analogue tibiae with screw holes was performed at the Orthopaedic Research Institute in Wichita, KS (Figure 2.)

Figure 2. Experimental torsion test fixture

To simulate the laboratory model, simplifications, such as omitting the cancellous (soft) bone and small features like screw threads, are made to reduce the complexity of the computational analysis.

Configurations for Simulation
Seven configurations of the FE model are used to examine the impact of the fracture limitation, screw holes, element size, rotation direction, and simplification of the model’s geometry. The configurations are listed in Table 1 and illustrated in Figure 3.

Figure 3. FE configurations studied. Arrows indicate rotational direction and solid color at the ends show where the boundary conditions are applied.

Model Geometry Definition
Like the experimental specimen, the FE model is a 120 mm long section from the distal portion of an analogue tibia with three equally spaced holes, which pass through both cortical walls. The FE model was generated from the manufacturer provided surface geometry of the analogue tibia. The test section relative to the whole tibia is shown in Figure 4. The vacant screw holes (3.75 mm in diameter) were positioned as shown in Figure 5.

Figure 4. Section planes and the tibia. The length of tibia between the planes is utilized.

Figure 5. Position of the screw holes. (a) Proximal end (b) Medial surface

In Configurations F and G, a cylindrical tube represents a geometrically simplified bone. The polar moment of inertia of an object is related to the object’s ability to resist torsion; therefore, the inner and outer diameters of the tube were calculated to match the polar moment of inertia of the tibia section.

Construction of the Finite Element Model
The FE model was developed in Altair HyperMesh, processed with Altair RADIOSS, and post-processed in Altair HyperView.

FE Mesh Generation

All of the configurations were meshed in HyperMesh with solid four node tetrahedral elements (TETRA4).
The mesh quality of each model configuration was reviewed and found to be acceptable in terms of warpage, aspect ratio, skew, tetra collapse, minimum length, Jacobian ratio, volumetric skew, volume aspect ratio, and tria minimum and maximum interior angles.

Material Model

The cortical bone of the analogue tibia is a composite of short E-glass fibers and epoxy resin that is pressure injected around a foam core. In the experiment, the analogue tibia demonstrated some non-linear behavior.

A preliminary study was conducted on several material models before selecting an isotropic linear elastic material model to simulate the analogue tibia. This material model is commonly used for FE model comparisons and studies on long bones. The modulus and density of the analogue tibia were provided by the manufacturer, and Poisson’s ratio was assigned to be consistent with former composite long bone FE models.

Failure Models Utilized

Two failure models are employed during this study, one for Configuration A and another for Configurations B through G. For Configuration A, fracture is assumed to occur when the angle of twist reaches the average fracture angle determined by the experiment, 9.3 degrees. For Configurations B through G, fracture is assumed to occur when any element in the model reaches a maximum stress limitation in tension, compression, or shear.

Loads and Boundary Conditions

To simulate the fixation and loading used during the experiment, a 15N axial compressive load and rotational velocity are applied to the outer surface nodes on the proximal end as shown in Figure 7(a). Boundary conditions on the distal end constrain all degrees of freedom are applied to the outer surface nodes, shown in Figure 7(b).

The axial load is slowly ramped up and then held constant. The rotational velocity is delayed until the axial load is fully applied. When applied, the velocity is ramped up to 2.5 deg/ms in 0.5 seconds and then held constant.

Figure 7. Nodes subjected to loading, velocity, and/or constraints. (a) Nodes on proximal end (b) Nodes on distal end

Finite Element Modeling Results
The fracture torque, angle of rotation at fracture, and torsional stiffness of each configuration are summarized in Table 5. Torsional stiffness is determined from the slope of the torque versus angle curve.

Contours of major principal stress, minor principal stress, and maximum shear stress are shown in Figure 8, 9, and 10 respectively.

Figure 8. Major principal stress contours for each FE configuration.

Figure 9. Minor principal stress contours for each FE configuration.

Figure 10. Maximum shear stress contours for each FE configuration.

A finite element computer model of an analogue tibia was successfully developed to simulate a torsional fracture test and predicted a fracture torque within the standard deviation of the experimental results. The verified model was used for parametric studies to investigate the effects of screw holes, rotation direction, failure model, element size, and simplification of the model’s geometry. The FE model predicted a fracture strength reduction due to holes that agrees with previous testing, and changing the rotation direction shifted areas of high stress but did not affect the fracture torque. Changing the failure model from an angle of twist limitation to maximum stress resulted in a 55% lower fracture torque. Reducing the element size did not affect the results, indicating that the utilized element size was appropriate. Simplifying the geometry of the model to a cylindrical tube resulted in a higher fracture torque and torsional stiffness, and the tube model predicted a lower reduction in strength due to holes than the tibia model.

Overall the FE model is shown to be a useful tool for simulating a long bone torsional fracture test. For further advancement of the model, material properties representing human bone should be incorporated, and results should be compared to those obtained with cadaver specimens.

Useful Links: read the full paper at

Rejeesh Rajan
Latest posts by Rejeesh Rajan (see all)