In the actual process of gear meshing, the maximum contact stress usually acts on the tooth surface of the pinion. The results are consistent with the previous chapters. The crack mainly occurs because the stress on the gear is greater than the yield strength, so it expands. The fatigue crack propagation of gear is simulated under different working conditions, and the small cracks are preset in advance.

**1) Gear model**

The gear model is constructed in the three-dimensional Software Solidworks, and some assembly models are intercepted, exported into a general format and analyzed in ABAQUS. Select the center of the pinion as the coordinate origin, and its spatial coordinate system distribution is shown in Figure 1. The coordinate origin of the gear reference is the same as the origin of the coordinate system. The semi ellipse is the geometric contour of the simulated crack, the shell is the attribute set for it, its tooth width is the long axis of the semi ellipse, which is a fixed value of 710mm, and the mark A0 is the short axis, as shown in Figure 1.

**2) Cracked gear assembly**

In order to reduce the complexity of subsequent meshing and crack assembly, the gear needs to be cut into regular geometry. The gear assembly model is shown in Figure 2. The tooth root of the pinion is equipped with semi elliptical cracks.

**3) Meshing**

The meshing of the segmented gear assembly model is carried out. Using the structure division method, the mesh size is: the mesh size of the pinion is 4mm. The mesh at the crack of the gear is encrypted to reduce the mesh size, and the mesh size becomes half of the original. The unit type of c3d8r is selected, the size of the big gear mesh is 6mm, and the final mesh division is shown in Figure 3.

**4) Define material properties**

Set the material of the gear in the material attribute module. It is not necessary to consider the separate setting of crack local materials, assign the overall gear material, and set 42crm 〇 as the gear material. Set the maxprinciplestress value to 84.4e6pa, that is, according to the numerical standard, the maximum principal stress criterion is used as the standard for value selection. The type is selected as energy, the linear softening yield stress is selected, the degradation is selected as the maximum value, and the power law is set for the mixed mode behavior. Set the fracture energy of the crack surface, mainly in three directions, including one normal direction and two tangent directions. The fracture energy is set to 42200 n / m. The mixed behavior of the three fracture energies constitutes a power function, and the power exponent power is 1. In the process of crack propagation analysis, elastic waves will be generated, but the problem that leads to the failure of the static equilibrium equation in the propagation finite element can be solved by adding a viscosity coefficient. This viscosity coefficient is only to balance the elastic state equation. Set the viscosity stability coefficient as 5e-5 and adjust the value of the viscosity coefficient to improve the convergence of the model, So as to counteract the elastic wave generated during expansion.

**5) Analysis step settings**

The analysis step setting process of finite element software is, and the system will automatically generate the initial step. To set the second analysis step, you need to set its analysis step type and consider the linearity of the object under study. Static general is selected as the analysis type, and nlgem on is selected for the consideration of linear problems. In the incremental step option, set the initial incremental step to 0.005 to improve the convergence of model analysis. The reduction operation is adjusted to 50, the solution control is set, and the analysis step is created.

**6) Gear contact setting**

The gear is meshing transmission, so its contact part is mainly defined. The defined attributes include tangential penalty function penalty, friction coefficient friction coeff and normal hard contact “Hard” contact. Then, the two gears are constrained, and the constraints are established at the circle centers rp.1 and rp.2 of the pinion and big gear.

**7) Definition of fatigue crack**

For the definition of fatigue crack, the extended finite element method is selected to select the crack region.

**8) Boundary conditions**

When the boundary conditions are applied, the degrees of freedom of the two gears are constrained, and the pinion is fixed. In addition to the degrees of freedom of rotation about the z-axis, the big gear restricts the other five degrees of freedom, that is, the degrees of freedom of rotation around itself. The operation is to select the displacement / rotation type in the boundary condition manager, and select U1 = U2 = U3 = ur1 = ur 3 = 0. Apply a torque of 10e6pa at the center of the large gear, as shown in Figure 4.

**9) Initial fatigue crack setting**

The length of the crack from the tooth top is H0, the size of the long axis of the semi elliptical crack is A0, and the crack angle is α As shown in Figure 5.

**10) Simulation results of root crack propagation**

As shown in Figure 6, in the case of initial crack (initial crack H0 = 64, α＝ 5 °, A0 = 10). It can be seen from Fig. 6 that the stress distribution and the theoretically calculated plastic zone stress distribution are similar near the crack elements in the four growth stages, and Fig. 7 is the theoretically calculated plastic zone stress distribution.

The stress history curve of a tip element of a gear crack is shown in Fig. 8. It can be observed from Fig. 8 that the tip element of the gear crack participates in the whole process of fracture. The material damage criterion is the maximum principal stress criterion, and the allowable material failure is set when the maximum stress of the material exceeds 84.4mpa.

The numerical simulation is mainly divided into three processes: firstly, the crack tip element does not crack, as shown in the figure, the stress has been increasing in the early stage, but it is still less than the critical stress of damage in this process. Secondly, the crack tip element cracks, the stress continues to grow, reaches the critical stress at time 0.7858, and the crack starts to crack until it is completely disconnected, which is obvious in the figure After fracture, a non crack tip element without stress singularity is formed, and the stress decreases with time as shown in the figure. Finally, the crack is completely broken, and the stress shows a decreasing trend as shown in the figure.