## 3 Materials and Method
### Design Phase
#### 3.1.1 Geometry Optimization: 2D FE Model
This is justified by the fact that the simulation was still in rate values under static conditions. The results from the _design phase_ FEAs can be plotted as _reaction force_ against the _rotation_, or _reaction force_ against the platform _displacement_. _Components modeling:_ The 3D CAD Model was imported into ANSYS by setting _3D_ as the analysis type. All isotropic parts were provided as solid to ANSYS, while composite parts were surfaces--Figure 11. All parts involved in contacts were modeled as flexible elements (platform, foot shell, lower blade, middle blade, upper blade, ankle frame and spring holder), while the parts connected with joints were modeled as rigid bodies (link and tube connector)--see Figures 12 and 13. Based on the results obtained from the 2D FE model in the previous step, the initial values of thicknesses and elastic properties of the composite parts were predefined and used as a reference to define the lamination sequences of layers of CFRP prepregs. Then, the types, the numbers, the orientations and the order of the layers of CFRP prepregs were changed until the targeted thickness and elastic properties (calculated with the _Classical Theory of Laminates_) were reached. Figure 11: Isotropic parts were provided as solid, while composite components were surfaces. The Össur lower blade was assumed as isotropic with approximated properties. The foot shell was simplified considering the areas underneath the lower blade only. Figure 10: The ISO 10328 dorsiflexion static test compared to the equivalent test with vertical actuator. The 3D CAD model of the foot prosthesis was provided to ANSYS in _Geometry_. The lamination sequences of the composite parts were modeled inside _ANSYS Composite PrePost_ (_ACP_). The main fiber direction for each of the composite parts is depicted in Figure 14 and it corresponds to the longitudinal direction of the foot prosthesis. Then, the composite parts were exported from _ACP_ to _Static Structural modeler_ as solid, with the final thicknesses. _Mesh modeling:_ The flexible components (platform, foot shell, lower blade, middle blade, upper blade, ankle blade and spring holder) were meshed. The elastic elements, including the lower blade and the foot shell, were mainly modeled with SOLID186 elements, which were 20-node elements with 3 degrees of freedom at each node and with quadratic behavior. SOLID187 elements (10-node elements with 3 degrees of freedom per node) were used for irregular areas. Ankle frame, spring holder and platform were modeled with SOLID185 elements, 8-node elements with 3 degrees of freedom at each node and linear behavior. The final 3D FE model of MyFlex-\(\gamma\) consisted of around 1,800,000 degrees of freedom (600,000 nodes) (Figures 12 and 13). Figure 14: Modeling of the composite parts. The lower blade was considered to be isotropic with elastic properties close to Ossur Pro-Flex Vivot’s sole blade. Figure 12: Mesh modeling of the components considered flexible in the analysis. The elastic elements, including the lower blade and the foot shell, were mainly modeled with SOLID186 elements (quadratic behavior). Ankle frame, spring holder and platform were modeled with SOLID185 elements (linear behavior). Figure 13: The 3D FE models for plantar flexion and dorsiflexion tests. _Contact modeling_: As in the 2D FE model, for parts that bend to each other with slight sliding, the contacts were modeled as _frictional_ using _pure penalty formulation_ and 0.1 was set as the _normal stiffness factor_ (the factor was set to 1 for normal dominated conditions). For contacts that could be modeled as glued/bonded, the _bonded_ contact type was used with _augmented Lagrange formulation_ and 1 was set as the _normal stiffness factor_. In MyFlex-\(\gamma\), the upper blade, the middle blade and the lower blade bend to each other with slight sliding when the foot is loaded. The contacts between the upper blade and the middle blade and between the middle blade and the lower blade were modeled as _frictional contact_ using _pure penalty formulation_.