## 2 Materials and Methods
### Thermal and Structural Analysis
The elastic modulus and thermal expansion coefficient both depend on the body temperature, therefore linear interpolation of the experimental data was used to determine these properties at different temperatures. \[\sigma_{th}=E\alpha\Delta T \tag{1}\]  
Figure 7 shows the expected 1D thermal stress with respect to the body temperature of the AM inserts. Stress increases with the applied thermal load and reaches a maximum of 2800 psi around 220 \({}^{\circ}\)F. Above this temperature, the stress decreases slightly due to the proximity to the glass transition temperature and the resulting reduction in stiffness. This is accounted for in the temperature dependence of the elastic modulus. Due to the limited nature of 1D analysis, the direction of stress must be assumed. Thermal stress in a component with external constraints, such as the outer surface of the AM inserts, will be subjected to compressive stresses, while components under internal constraints, such as the inner diameter, will incur tensile stresses [12]. Since it is unclear which will dominate, the 1D results incorporated both stress states. If the inserts incur large tensile stresses, there is additional failure risk due to a stress concentration in the alignment pin notch. An appropriate stress concentration factor was calculated as 1.86 and applied to the maximum thermal stress value determined previously. Hence, the maximum anticipated tensile stress would be 5200 psi. The stress concentration factor was calculated using the formulas in [PERSON] textbook and the nominal CAD geometry [12]. Both maximum anticipated stress values are well below the ultimate strength and indicate that the design is likely feasible without any need for additional gaps between components. The limitations in the 1D analysis necessitate the use of commercial computational tools for higher-order analysis. ANSYS Mechanical 2022/R1 was used to develop computational models for the assembly in 2D and 3D. The 2D analysis was performed using an axisymmetric analysis of the adaptable fan casing cross-section. In the software, the axisymmetric analysis assumes a constant cross-section revolving around the center. This means that a more accurate solution for the entire insert can be developed compared to the 1D method. The 2D analysis lacks some key details that are resolved using the 3D analysis; however, it performs much better for design iteration when taking into account computational cost. The axisymmetric model can reach a solution in roughly 15 to 30 min depending on mesh size, while the 3D analysis requires hours. The goal was to use the 2D analysis results to gain insight into the predicted stress state and incorporate any design changes that would be required. Both analyses followed the same workflow to obtain results. First, the components were meshed using the ANSYS dedicated meshing tool. Expected temperature loads due to the fan flowfield were then applied and a steady-state thermal analysis was run to determine the temperature distribution in the inserts and metal components. The temperature distribution was then applied to the structural model along with other representative boundary conditions to obtain stresses that arise from the thermal loading. The cross-section used in the 2D analysis is shown in Figure 8. Thermal analysis boundary conditions consisted of an applied temperature distribution on the flowpath surfaces. Upstream of the fan leading edge region, the temperature was set to ambient conditions. Downstream of the trailing edge region, the temperature was set to approximately 200 \({}^{\circ}\)F, which represents the hottest allowable rotor exit temperature due to the material constraints. The ratio of these temperatures was roughly the value of the highest total temperature ratio that the fan achieves. Between these two regions, a linear temperature distribution was imposed to represent the effect of the total temperature rise through the rotor.