# Stress Analysis on the Ankle Joint during Incline and Decline Standing
## 2 Materials and Methods
### Finite Element Model of Ankle Joint  
1. Meshing  
Meshing is a part of the engineering simulation process where complex geometries are divided into elements. Good meshing is required in critical areas such as areas of interest in stress distribution (ankle joint) to increase the accuracy of simulation results. Before meshing was performed, the model was exported in a STEP file and opened in ANSYS. The finite element model was meshed with the ten-nodes 3D-tetrahedral element for bone, cartilage, ligament, and ground support. The ligaments were modelled as a solid element to observe the stress distribution on it. Although most of the previous studies used a tension-only truss to model the ligaments [8; 11], there are also previous studies that used isotropic solid element, as mentioned by [14]. Two elements were set on the thickness of each ligament. The model was performed under linear static analysis. Figure 5 shows the complete meshing of the ankle joint model, and the magnified view of the ankle joint.  
2. Convergence test  
The number of elements was based on different sets of mesh sizes and types from the previous meshing. The meshing process of the model needs to be set with fixed mesh types but different sizes to obtain a different number of elements in each part. The solution made with a mesh discretization was observed and recorded. Then, it proceeded with finer mesh, and the results were compared with the previous test. If the results showed a different significant amount, the process was repeated with finer mesh. This step was repeated until the results were approximately similar for the mesh to be considered enough for the model. The increment of the element number resulted in a longer computational time due to the time-consuming nature of solving the mathematical models to complete the solution. Excessively large values of element size should be avoided because the result produced by ANSYS will be inaccurate and contain a higher percentage value of error.  
A simulation with an arbitrary load of 300 N was applied on top of the tibia for the convergence test. The influence of mesh size on the maximum von Mises stress of the model was recorded and the meshing process was repeated with a decrement of the mesh size by 0.1 mm (from 2.5 mm to 1.5 mm) as shown in Figure 6. The changes in mesh size only involve the structure of bone while the cartilages and ligaments stay constant. Based on the convergence test curve shown, the optimum element size obtained is 2.0 mm with 200,485 elements, where the graph starts to reach a constant at that mesh size.  
Figure 5: Complete meshed model with magnified view of the ankle joint.  
After the optimum mesh size was found, the material properties in each part of the ankle joint were defined. There were four central parts of material: bone, ligament, cartilage, and ground support. Each of these parts has different material properties. The material properties for the model can be directly imported from the engineering data of ANSYS. Bone, ligament, and cartilage have their own unique Young's Modulus and Poisson's ratio. However, there are no existing biological material properties such as ligament and cartilage in the engineering data. New material properties have to be added manually to the engineering data before defining these models. The material properties of bone, ligament, and cartilage are adopted from the literature [11] and tabulated in Table 1. The material properties were assigned to every component of the model to obtain accurate results.