The BOX TAR model consisted of three components which were tibial, bearing and talar. The details of this model geometry were explained in Sect. 2.1. The BOX TAR was modelled in SOLIDWORKS, a computer aided design (CAD) software. The model was converted to .SAT format which was compatible to the commercial ABAQUS software created in order to generate the model in the ABAQUS/CAE tool.

All components generated required the definition of the material properties. The Young’s modulus and Poisson’s ratio were defined in the property module of the ABAQUS/CAE software. The tibial and talar components were assigned to be of Cobalt-Chromium (CoCr) where the Young’s modulus was 210 GPa and the Poisson’s ratio was 0.3. The bearing component was assigned to be of ultra-high molecular weight polyethylene (UHMWPE) where the Young’s modulus was 500 MPa and the Poisson’s ratio was 0.3.

In this simulation, the static responses were used. This is a single event that needed single analysis steps. Overall, the analysis consisted of two analysis steps where-by the ABAQUS/CAE generated an initial step automatically. The analysis step was created in the period of 0.625 s. The time period was determined by stance phase of time taken in the ankle gait cycle [7]. Stresses, displacements, and contact were requested in the field output while the energy was requested in the history output. All outputs requested for a whole model every 0.025 units of time. The output data required was contact pressure where by it was printed in the form of tables that was written in ABAQUS data (.dat) files.

The interaction was created using surface-to-surface contact, in which the contact property used was tangential behaviour. The friction coefficient between two articulating surfaces of the metal and bearing components were assumed to be 0.04 [8].

The tibial component was fixed in the distal tibia bone and the talar component was fixed at the articulating surfaces of the talar bone. In this simulation, the load created was an axial (vertical) load using concentrated force applied to the tibial component. The boundary condition of internal/external rotation was applied to the tibial component whereas the anterior/posterior force and plantar/dorsiflexion were applied to the talar component. The variation of load and boundary conditions of the stance phase of ankle gait cycle applied was utilized by creating tabular amplitude. The talar component was constrained using a tie at a point that was the center of articular surface of the talar dome as shown in Fig. 2.4. The applied boundary conditions and force predictions were based on previous work [9, 10]. Time histories of boundaries and force predictions of the stance phase of the gait cycle was considered to simulate wear predictions on the TAR model as shown in Fig. 2.5. The stance phase of gait cycle was divided into 25 instants.

There are hexa, wedge and tetra elements for the solid mesh element available in ABAQUS/CAE. Tetrahedral elements are geometrically versatile and used in many automatic meshing algorithms. It is very easy to mesh a complex shape with tetrahedral elements. It is known as a robust element and occasionally used as a rigid element. The hexahedral elements normally provide a good mesh with a solution of equivalent accuracy at less cost. However, tetrahedral elements are less sensitive to initial element shape, whereas first-order hexahedra perform better if their shape is approximately rectangular.

The metal parts of the tibial and talar components were modelled as four nodes which were three-dimensional tetrahedral elements represented as rigid triangles. The number of elements was 36,457 and 16,224 respectively. The tetrahedral element was stiffer than the hexahedral element. This was due to more points of integration in the hexahedral element than the tetrahedral element. Thus, the tibial and talar components, as hard parts, were assigned to use the tetrahedral element while the UHMWPE bearing was assigned to use 5760 element of eight node hexahedral elements as soft part.