The model used for numerical simulation of fatigue crack growth is the same as that of 42CrMo steel compact tensile specimen. Because the fatigue crack length is measured on the surface of the specimen in the fatigue crack growth test, and the specimen is uniformly stressed and the force is parallel to the plane of the specimen, this complex three-dimensional solid loading model is simplified as a plane stress  problem for analysis in the finite element modeling.
The model is created in the finite element software ABAQUS, as shown in Figure 1. The whole model includes more than 17000 nodes. In order to make the numerical simulation results more accurate, considering that the real crack propagation rate is relatively slow in the crack initiation stage and the initial stage of crack propagation, and the gradient of elastic-plastic stress-strain field near the crack tip is very large, it is necessary to subdivide the mesh around the crack tip when meshing, and the mesh fineness decreases layer by layer, The modified 6-node quadratic plane stress triangular element (cps6m) with high accuracy is used. Because of the singularity at the crack tip, the 1 / 4 node method is used to create the singularity at the crack tip. The 8-node quadrilateral quadratic plane stress fully integrated element (cps8) is used in other regions except the fatigue crack tip.
As the material of the compact tensile specimen is 42CrMo steel, the material parameters are set as follows: elastic modulus E = 2.12 × 105 MPa, Poisson’s ratio μ= The maximum principal stress is 84.8 MPa. According to the energy principle, the softening of yield stress is linear, the stiffness degradation is maximized, and the mixed mode behavior is power law. The fracture energy in three directions is 42200 n / m, and the power exponent is 1. In order to counteract the elastic wave, prevent the failure of the static equilibrium equation in the extended finite element method, and improve the convergence of the model, the viscous stability coefficient is set to 5 × 10-5。
In order to improve the convergence of model analysis, in the incremental step option, the maximum number of incremental steps is 1 × 106, the initial increment step is set to 0.01, and the minimum value is 1 × 10-8, the maximum is 0.1.
The x-direction fixed displacement constraint is applied at the top node of the two loading holes, and the x-direction and Y-direction fixed displacement constraints are applied at the left end of the specimen at the same time. Because the object of the numerical simulation is the stress intensity factor at the crack tip, the stress intensity factor at the crack tip collected in the experiment is very small Δ The value of K is the difference between the stress intensity factor at the crack tip under the maximum load and the minimum load in a cycle. Therefore, in the numerical simulation, the structural load is static load, and the static analysis of the structure is carried out. The difference of the stress intensity factor at the crack tip obtained under two static loads is the calculated value. The load is applied to two symmetrical circular nodes of the specimen in the form of concentrated force, and each node establishes a coupling relationship with its respective semicircle region. The coupling type is set as distribution to realize the average distribution of concentrated force in the loading hole. The maximum and minimum values of tensile stress are the same as the experimental values. The dynamic continuous propagation of fatigue crack is realized by resetting the crack length each time. The value of crack length in numerical simulation is consistent with that in experiment.