## 5 Deterioration Model for Wire Load-Bearing Strength
### Finite Element Model for Wire Tensile Testing  
A large general-purpose finite element software called ABAQUS is used to establish the tensile finite element simulation model of the wire. Firstly, the finite element model of the unworn wire is established (Figure 6a), and the analysis results of the finite element model of the unworn wire are compared with the tensile test results to verify the correctness of the finite element model. Then, based on the results of the test, the actual wear mark size \begin{table}
\begin{tabular}{c c c c} \hline \hline \multicolumn{1}{c}{**Parameters**} & \multicolumn{2}{c}{**Fitting Equation**} & \multicolumn{1}{c}{**Goodness of Fit (R\({}^{2}\))**} \\ \hline \multirow{3}{*}{Contact load (N)} & 60 & \(D=2.28\times 10^{-14}\)\(N^{2}-6.88\times 10^{-9}\)\(N+0.9985\) & 0.9970 \\  & 80 & \(D=5.36\times 10^{-14}\)\(N^{2}-5.16\times 10^{-9}\)\(N+0.9977\) & 0.9965 \\  & 100 & \(D=6.43\times 10^{-14}\)\(N^{2}-3.43\times 10^{-9}\)\(N+0.9961\) & 0.9971 \\ \hline \multirow{3}{*}{Fatigue load peak (N)} & 1000 & \(D=2.3\times 10^{-14}\)\(N^{2}+6.52\times 10^{-9}\)\(N+0.0015\) & 0.9971 \\  & 1100 & \(D=5.20\times 10^{-14}\)\(N^{2}+5.98\times 10^{-10}\)\(N+0.0031\) & 0.9958 \\ \cline{1-1}  & 1200 & \(D=7.08\times 10^{-14}\)\(N^{2}+10.91\times 10^{-9}\)\(N+0.0033\) & 0.9982 \\ \hline \hline \end{tabular}
\end{table} 
Table 4: Fitting equation for damage degree of the fatigue wire (pair: wire). Figure 5: Fitting curves of damaged wire (pair: wire) damage degree under different contact loads (**a**) and different fatigue loads (**b**). of the worn wire is regarded as the damage gap of the three-dimensional model (Figure 6e). The worn wire's tensile finite element model is established (Figure 6c). The tensile fracture of the wire in the worn zone is the main concern of this paper. In order to improve the calculation efficiency of the tensile simulation model, the total length of the wire was selected as 25 mm after a lot of pretests. The material characteristics of the wire are shown in Table 5. The eight-node linear element (C3 DBR) is used for meshes, and the mesh of the worn area is encrypted. In the simulation model of the unworn wire, there are 56,000 finite element mesh elements and 61,997 nodes. The mesh number and node number of the finite element model of the worn wire were 95,400 and 104,526, respectively. As shown in Figure 6b,d, two reference points, RP1 and RP2, were established in the interaction module. Then, the reference point was coupled with the corresponding surface, and the constraint mode was in the motion-coupling mode to ensure that the established reference point was consistent with the corresponding surface displacement. In the finite element calculation model, three translational and three rotational degrees of freedom are constrained at the reference point RP1 at the bottom of the steel wire. All degrees of freedom, except in the Y direction at the reference point RP2 at the top of the wire, are constrained by applying a Y direction velocity of 5 mm/s. The stress-strain curve and tensile strength of the steel wire were obtained by extracting the force and displacement information at the coupling reference point RP2. As shown in Figure 7, the wire tensile strength obtained by the universal testing machine is 1651.1 MPa, compared to 1648.8 MPa obtained by the simulation experiment. The relative error is 1.4%. The minimum diameter of the experimental tensile fracture is 1209 mm, compared to 1170 mm obtained by the simulation. The tensile fracture is basically the same, and the relative error of the two is 3.2%. Therefore, the simulation model established in this paper has a certain degree of correctness, so the load-bearing strength of steel wire with different amounts of wear can be obtained according to the finite element simulation model.