1 Acquisition of ankle CT images
One healthy adult volunteer with no previous history of injury, such as ankle fracture or dislocation, or pathological conditions, such as ankle arthritis, bone disease or bone tumour, was selected. The right ankle joint of the volunteer (60 kg and 28 years old) was imaged with thin-section CT, with a scanning layer thickness of 0.625 mm, resulting in 657 images of 512 × 512 pixels that were saved in DICOM format. During the CT scan, the volunteer's ankle was nonweight-bearing in the supination position.
2 3D reconstruction and optimization
DICOM format images were imported into Mimics 21.0 software (Materialise, Belgium); the images were segmented; and the tibia, talus, and fibula were reconstructed. Multiple bones (including the calcaneus, navicular cuneus, mediolateral cuneus, dice cuneus, and mediolateral cuneus) beneath the talus were fused to reconstruct their 3D models (Fig. 1). The following processes were carried out in proper sequence: (a) Automatic threshold segmentation and differentiation are carried out according to the grey value of different tissues, and the bone tissue is preliminarily separated, (b) a mask is used to establish the structure model of each part, (c) the manual layer editing tool is used to eliminate the redundant part or fill in the missing part, and (d) the model is wrapped and smoothed, the hole and smooth surface are filled, the corresponding three-dimensional model is preliminarily established, and the model data file is exported in STL format.
We import the STL format file generated by Mimics into Geomagic Studio 2017 software, erase the nails and redundant features of the model, and then smooth the model. Then, the accurate surface module is used to detect the contour line of the model, any deformed or unreasonable contour line is edited, and additional contour line is added appropriately to facilitate the generation of surface patches. After the surface patches are generated successfully, the surface is fitted, and the fitted model is exported to a general STEP format model data file.
3 Establishment of the finite element model
We import the optimized 3D models into SolidWorks software, carry out feature recognition and surface diagnosis on the geometric model, repair the problematic surface, construct the articular cartilage model by using the stretching and segmentation commands on the part interface, draw 3D lines in the 3D sketch to simulate the ligament model, and finally establish a complete three-dimensional ankle model including tibia, fibula, talus, calcaneus, cartilage and ligament and then save the model as a 3D geometry file in X_ T format. The obtained geometric models are imported into ABAQUS software (2018, Dassault, Providence, RI, USA) to build finite element models with the help of the attachment points and anatomical locations of ligaments determined from reference documentation; there were a total of 362,351 nodes and 261,420 units (Fig. 1). Bone and ligaments are simplified into isotropic, homogeneous linear elastic materials, and the material parameters are listed in Table 19,10. In brief, bonding contact is used between the ligament and bone, calcaneus and talus, while face-to-face contact is used for the talus, tibiofibula and calcaneus cartilage and bone. The friction formula is the penalty function algorithm, the normal contact stiffness is "hard" contact, and the friction coefficient is 0.2 to establish the finite element analysis model.
4 Research on grid convergence
The normal supination and external rotation ankle joint model is divided into grids of different levels. The grid levels are divided into coarse, semi coarse, fine and very fine. Then, the same boundary conditions and loads are applied to the four grid models. The stress and displacement results obtained from the analysis are shown in the table below (Table 2):
Table 1
|
Elastic modulus (MPa)
|
Poisson’s ratio
|
Bone
|
14000
|
0.3
|
Cartilage
|
15
|
0.46
|
Ligament
|
260
|
0.49
|
Table 2
Research on grid convergence
Grid level
|
Element quantity
|
Max. stress (MPa)
|
coarse
|
143507
|
68.5
|
semi coarse
|
201317
|
95.55
|
fine
|
264023
|
83.73
|
very fine
|
369803
|
77.76
|
It can be seen from the above table that the stress results of the fine grid level are similar to those of the very fine grid level, so the subsequent analysis adopts the fine grid model as the finite element analysis model based on the comprehensive consideration of calculation accuracy and calculation time.
5 Verification and analysis of the finite element model
In this part, the model loading parameters are based on a fixed lower surface of the talus, and a dead weight loaded between the tibia and proximal fibula and the internal rotation force are used to simulate the post rotation-external rotation-type injury situation. Three directional fixation restraints are set with full degrees of freedom in XYZ at the under-surface of the talus, and a reference point is established near the upper surface of the tibia and fibula, coupled with the upper surface degrees of freedom, the application of a dead weight load (480 N compression on the upper surface of the tibia and 120 N compression on the upper surface of the fibula) and an internal rotation force (gradually increasing internal rotation force, simulating an IV stage injury). A 600 N vertical compressive load is applied to the upper sections of the lower tibia and fibula of the model, where the calcaneus is fixed and the talus is constrained (Fig. 2). The maximum contact stress of the ankle joint surface is 2.1059 MPa, the contact area is 373.658 mm2 (Fig. 3), and the model is validated as effective11. The calculations of outcomes are based on the maximum stress location and pressure on the articular surface.