## 2 Numerical Investigations
### Quasi-Static Bending Fatigue Simulation Analysis
\begin{table}
\begin{tabular}{c c c c} \hline \hline
**Parameter** & **Value** & **Parameter** & **Value** \\ \hline \(E_{n}(GPa)\) & 9.7 & \(\sigma_{n}^{0}\) (MPa) & 55 \\ \(E_{s}(GPa)\) & 6.5 & \(\sigma_{n}^{0}\) (MPa) & 120 \\ \(E_{t}(GPa)\) & 6.5 & \(\sigma_{t}^{0}\) (MPa) & 120 \\ \(G_{n}^{c}(N/mm)\) & 0.28 & \(\eta\) & 1.45 \\ \(G_{5}^{c}(N/mm)\) & 0.495 & \(\rho\)(kg/m\({}^{3}\)) & 1570 \\ \(G_{t}^{c}(N/mm)\) & 0.495 & & \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Material properties of prepreg interface elements. \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Parameter** & **Value** & **Parameter** & **Value** \\ \hline \(E_{1}\) (GPa) & 142 & \(X_{t}\) (MPa) & 1900 \\ \(E_{2}\) (GPa) & 9 & \(Y_{t}\) (MPa) & 51 \\ \(E_{3}\) (GPa) & 9 & \(Z_{t}\) (MPa) & 51 \\ \(v_{12}\) & 0.32 & \(X_{c}\) (MPa) & 1100 \\ \(v_{23}\) & 0.46 & \(Y_{c}\) (MPa) & 130 \\ \(v_{13}\) & 0.32 & \(Z_{c}\) (MPa) & 130 \\ \(G_{12}\) (GPa) & 4.6 & \(S_{12}\) (MPa) & 72 \\ \(G_{23}\) (GPa) & 3.08 & \(S_{13}\) (MPa) & 72 \\ \(G_{13}\) (GPa) & 4.6 & \(S_{23}\) (MPa) & 70 \\ \(G_{LT}\) (N/mm) & 50 & \(G_{LC}\) (N/mm) & 75 \\ \(G_{TT}\) (N/mm) & 0.25 & \(G_{TC}\) (N/mm) & 0.75 \\ \(\rho\) (kg/m\({}^{3}\)) & 1620 & & \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Material properties of FAW200 RC38 prepreg. allowing the loading indenter to separate from the shaft tube after the loading is completed. The loading indenter and the support seat are both rigid body parts. When setting the main contact surface of the contact pair, the side of the rigid body part in contact with the shaft tube should be selected as the main surface of the contact pair, which is conducive to the convergence of the calculation results. The boundary conditions of the finite element model of the CFRP shaft tube are shown in Figure 1. The three-point bending loading displacement of the shaft tube is 20 mm, and the loading speed is 1 mm/min. The mesh element shape of the axle tube is set to quadrilateral element, and the element type is S4R, which is meshed by structured meshing technology. The quasi-static simulation of the shaft tube using five sets of structural meshes with different degrees of density is shown in Figure 2, and the ultimate load of the output shaft tube is shown in Table 3 to analyze the mesh convergence. It can be seen from Table 3 that the limit load values of grid numbers 4 and 5 are not very different; the trend is stable, and the convergence is good. Therefore, the final grid for dividing the shaft tube finite element model is grid number 4 with the number of elements fixed at 20,792. The analysis step type of the quasi-static analysis is Dynamic Explicit, and the geometric nonlinear switch Nlgeom is set to ON; the automatic incremental step type is adopted, and the number of steps of the maximum incremental step is not limited. The mass scaling factor is set to 1000. The output of the field variable setting of the article is the stress field of the shaft tube, and the output of the historical variable is the displacement U2 of the reference point of the loading head and the support reaction force RF2. The stress field of the CFRP shaft tube quasi-static three-point bending is shown in Figure 3. It can be seen from the figure that there are dents in the contact parts of the shaft tube and the loading head and the supporting seat, and the dents at the shaft tube and the loading head are larger, indicating that the contact part of the shaft tube and the loading head is damaged. Therefore, the final crush failure of the shaft tube is the contact area between the shaft tube and the loading head. The quasi-static three-point bending simulation obtains the displacement-load curve of the CFRP shaft tube in the loading direction, as shown in Figure 4.  
Figure 1: Boundary conditions of finite element model of CFRP shaft tube. Figure 3: Quasi\(-\)static bending stress field of CFRP shaft tube.