## 3 Contact Analysis of Topologically Modified Internal Helical Gear Pair
### Finite Element Calculation Example Analysis  
The inner helical gear is regarded as the driving gear, while the external helical gear is the driven gear. The material of both gears is 20 CrMnTi, with a density of 7800 kg/m\({}^{3}\). The Young's modulus of elasticity is 1.4 \(\times\) 10\({}^{5}\) MPa, and the Poisson's ratio is 0.3. The permissible contact stress is 745 MPa, and the permissible bending stress is 510 MPa. Frictional contact exists in the meshing of internal helical gears pair, with a friction coefficient of 0.25. The unit type is (secondary unit) C3D8R, the number of hexahedral meshes of the internal helical gear is 62,352, and the number of hexahedral meshes of the external helical gear is 53,821.  
The contact analysis is carried out in three steps by the dynamic implicit method: the main analysis step is set to be 0.1/0.01. Firstly, the internal helical gear is fixed and the external helical gear is rotated to ensure contact and convergence. Secondly, the external helical gear is fixed and the internal helical gear is rotated to avoid excessive contact. Finally, the rotation degree of freedom of the two gears is released to simulate the rotation process of the external helical gear driven by the internal helical gear, in which the surface-to-surface contact is used to construct the connection relationship between the gears, the gear speed and torque are set in different analysis steps (taking the light load 50 N\(\cdot\)m as an example), and the torque is applied to the internal helical gear.  
A four-tooth simulation and analysis model, modeled in Abaqus, is shown in Figure 5. Python script files are embedded within the Abaqus2022 simulation software to extract and analyze the contact stresses during the meshing under a different speed and torque.  
After adjusting the modification coefficient, four sets of simulation settings are set to be consistent, and the tooth surface contact analysis is carried out. From Figure 6, it can be seen that the contact area of Case 0 along the tooth profile direction is larger and the contact area in the middle area presents a slender ellipse, indicating that it is caused by the smaller coefficient \(b_{h}\). After Case 1 increases \(b_{h}\) and decreases \(b_{m}\), it is found that the contact area along the tooth profile direction is larger. Case 2 increases \(b_{h}\) and decreases \(b_{m}\), and it is found that the contact area gradually moves closer to the middle. After re-adjustment, the contact area of Case 3 appears as an elliptical shape, and the contact area is mainly in the middle of the tooth surface. In the first three sets of simulation results, the contact area of the tooth surface is flat and long, causing edge contact, but. In Case 3, the tooth surface contact area is elliptical, and the meshing area appears in the middle of the tooth width. The two ends are sharp, the tooth surface contact stress is small, and the elliptical shape gradually decreases outward, so the bearing capacity is strong. Therefore, the tooth surface contact effect of Case 3 is the best. In addition, the red wire frame in the figure is the force area of the contact process, and the red dotted frame represents the main stress area.  
Figure 5: Four-tooth grid simulation model.