Initial stability and stress distribution of ankle arthroscopic arthrodesis with three kinds of 2-screw configuration fixation: a finite element analysis

Screw model and the fused tibia-talar joint model were assembled according to three kinds of 2-screw configurations for AAA. Three different forms of assembly were used to represent the 2 “home run”-screw configuration (2 screws are inserted from the lateral-posterior and medial-posterior malleolus into the talar neck, group A, Fig. 1a), crossed transverse configuration (the screw is inserted from the medial malleolus into the anterior talus and the other from the lateral tibia maintains posterior talus, group B, Fig. 1b), and 2 parallel screws configuration (2 parallel screws are inserted from the posteromedial side of the tibia into talus, group C, Fig. 1c). The three models were exported in x_t * format and imported in the finite element software (ABAQUS 6.13,Dassault Systems Simulia Corp., Providence, RI, USA). Since only the tibia near the fixation was important in this analysis, a 75-mm length was taken at the distal end of the tibia for later analysis. Tibia and talus bones were considered as linear elastic materials. Because of the elastic modulus of screws were much larger than that of the bone and in order to improve the computational efficiency of the model, the screws were set as rigid bodies. The corresponding material parameters are listed in Table 1.

A local coordinate system was created, with the origin chosen at the center point of the screw. In the local coordinate system, the Y direction was the axial direction of the screw, and the X and Z directions were two mutually perpendicular radial directions of the screw section. Both load and boundary conditions were created in the local coordinate system. A uniform pressure distribution of 50 MPa perpendicular to each screw top surface was applied to simulate the external force (Fig. 2a). The 6° of freedom on the lower surface of the talus was constrained (Fig. 2b), and the screws were restrained to move along their axes (Fig. 2c).

After the implantation, the load and boundary conditions were reserved. A moment of 10 Nm was applied to the upper surface of the tibia to simulate the load of varus, valgus, flexion, dorsiflexion, external rotation, and internal rotation respectively (Tables 2, 3, and 4).

Various contacting components were considered as interacting surfaces, including between talus-tibia, screw-talus, and screw-tibia. A contact pair was defined for each potential interacting surfaces, with the considerations in the normal direction with the default setting (hard contacts), and tangential direction with a friction coefficient. Furthermore, “finite sliding” was considered to model potential nonlinear effects. The details of all the contact pairs are shown in Table 5.

Due to the irregularity of the bone surface, tetrahedral mesh was used for the talus and tibia (C3D4: 4-node linear tetrahedron element), and hexagonal mesh for the screws (C3D8R: 8-node linear brick, reduced integration, hourglass control element). In order to improve the efficiency and accuracy of the finite element analysis, the mesh of contact surface of tibia and talus were refined. Group A was meshed a larger and a smaller number of nodes additionally for mesh sensitivity analyses. Both the maximum von Mises stress of the two models were differed from the standard model by < 3%.