# Fretting Fatigue Behavior under Tension-Bending Mixed-Mode Loading
## 3 Numerical Model and Method  
### Finite Element Model  
In order to investigate the fretting behavior of the cylindrical pad-on-flat specimen under tension-bending mixed-mode loading, a 2D plane strain finite element model (shown in Figure 2) is developed by employing ABAQUS software (version 6.14) along with MATLAB standard code. ABAQUS is used for pre-processing and solving the FEM model, and MATLAB code is used to perform the critical plane method to predict the fretting damage initiation. As is indicated in Figure 2, the left side of the specimen is set to a fixed constraint, and the pad is restricted to move just in a vertical direction. Normal load \(P\) is applied to the top of both cylindrical pads using a multi-point constraint (MPC). Oblique force \(F\) applied to the right end of the specimen is resolved into the tension load, \(F\)cos\(\theta\), and the bending load, \(F\)sin\(\theta\), to simulate the tension-bending mixed-mode loading. Four nodes, plane strain, and a reduced integration quadrilateral element (CPE4R) are used for the analysis. The master-slave algorithm is adopted to calculate the contact between the cylindrical pad and the specimen. Al2024-T351 with elastic modulus \(E_{1}\) = 74.1 GPa is used for the specimen, and the constant dimensionless parameters of the model are shown in Table 1. The material and geometric data of the model are derived from Ref. [13]. The cylindrical pad has the same Poisson's ratio as the specimen. The maximum Von Mises equivalent stress in all the cases is lower than the yield stress, so the elastic constitutive relation is implemented to simulate the mechanical properties of the material. The load sequence is shown in Figure 3, where the loads are applied in three steps, and the time increments in each step are small enough. Normal pressure, \(P\), is applied at the first step to establish contact and remains constant in the subsequent steps. The bending load, \(F\)sin\(\theta\), and the tension load, \(F\)cos\(\theta\), each with a stress ratio of 0.1, are simultaneously loading in the second step and unloading in the third step. According to the numerical observation, the equivalent stress of the specimen under tension-bending mixed-mode loading increased to the maximum at step 2. The node with the maximum stress is found at the leading edge of the contact interface (the contact edge, which is towards the cyclic load, as shown in the upper dashed rectangle of Figure 2), which is consistent with the fretting damage initiation location observed in many experiments [9; 13; 18; 21]. Therefore, the nodes on the upper contact interface of the specimen are defined as the path for stress analysis and calculating damage parameters. \begin{table}
\begin{tabular}{c c c c c} \hline \hline \(P/E_{1}t^{2}\) & \(\
u_{1}\) & \(\
u_{2}\) & \(\mu\) & \(R/t\) \\ \hline \(5.405\times 10^{-4}\) & 0.33 & 0.33 & 0.65 & 14.016 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Constant dimensionless parameters of the contact model. Figure 3: Loading sequence of the finite element model. Figure 2: Sketch of the finite element model. Table 2 shows the sixteen groups of numerical experimental data designed for simulating the tension-bending mixed-mode fretting fatigue. Based on the dimensional analysis, the experimental data are tabulated into three categories, \(\lambda\), \(\theta\), and \(\gamma\). Four levels of oblique loads, seven stiffness ratios, and seven mode angles are designed to investigate the effect of governing parameters on mixed-mode fretting fatigue. Due to the high stress gradient in the potential zone of fretting damage, an appropriate mesh size should be selected to obtain accurate stress in this zone while considering the calculation efficiency. The convergence study is carried out to obtain a suitable mesh size under the loading case of Exp. 4. Figure 4 shows the maximum Von Mises equivalent stress, \(\sigma_{\text{eff,max}}\), at each step for different mesh sizes.