## 3 Results
### Stress Analysis Results
The magnitude was slightly higher at the outer diameter of the aft end compared to the 1D model and the 2D axisymmetric model. The results for Plane A are shown in Figure 13.  
Figure 11: ANSYS model of the AM insert geometry with results planes called out. Plane A includes the alignment notch and Plane B is free from geometric features. Figure 12: Von Mises stress contours obtained from the 3D analysis in Plane A. The most attention was given to the aft notch apex with very high predicted compressive stress. One option that was briefly considered was to increase the radius of the notch in this area. This was not possible as the notch is required to maintain the concentricity of the inserts surrounding the rotor. To achieve this, the alignment pin must fit tightly in the feature. As powerful and convenient FEA tools are, a critical aspect of the analysis lies in the ability to discern physical vs. nonphysical predicted stresses. Stress singularities can arise in FEA models due to geometric discontinuities. Increasing the element count will not necessarily fix the issue either as stress singularities will grow with more elements incorporated in the area. The mesh was refined locally near the notch, and increased stresses were incurred as a result. A closer examination of the 3D results was made to determine whether these high stresses were likely to be physical. Figure 14 shows the 3D ANSYS model of one of the AM inserts. Upon closer inspection of the results superimposed on the mesh, it becomes clear that the high stress is localized to a very small section (dark blue). Moving just one element over from the dark blue region reduces the stress by around 2000 psi (14 MPa). This instilled more confidence that the stress was artificially high due to the geometry. For a valid comparison of stresses predicted using all three failure criteria, a value of 7530 psi (52 MPa) was used for the magnitude of the minimum principal stress. This is the maximum stress value from one element away from the singularity. Stress analysis typically involves the use of a safety factor, which reflects the margin of error compared to the ultimate strength. The safety factor, \(S\), is defined in Equation (2). For each criterion, \(\sigma_{max}\) represents the maximum magnitude of stress. The ultimate strength is 8900 psi, \(\sigma_{ult}\). \[S=\frac{\sigma_{ult}}{\sigma_{max}} \tag{2}\]  
The results from the 3D analysis are summarized in Table 4 in the form of predicted stress and safety factors. The two lowest safety factors are associated with the von Mises stress and the minimum principal stress. Both values are greater than 1, which is a stringent requirement. The analysis represents the stiffest and highest stress state possible for the  
Figure 14: Three-dimensional view of the minimum principal stress in one of the AM inserts. Figure 13: Minimum principal stress contours obtained from the 3D analysis in Plane A.  
assembly since there were no gaps between the inserts themselves and the inserts and the metal components. In the actual assembly, some of the stress will be relieved due to very small gaps to account for manufacturing tolerances. The analysis provides confidence that even with a tight fight between inserts, the structure will perform well during operation. For similar applications, time can be saved by focusing more on the 1D and 2D analysis. If no fillets or geometric features are included that would be expected to result in stress concentrations, the 1D and 2D results match the 3D results well.