## 3 Cracking Simulation and Cracking Damage Range Analysis
### Finite Element Model  
The finite element analysis software ABAQUS is used to model the two-dimensional structure of a tunnel. The size of the tunnel section is shown in Figure 7. The solid structure was meshed with the four-node plane strain quadrilateral element, CPE4R \begin{table}
\begin{tabular}{c c c c c} \hline \hline \multirow{2}{*}{**Evaluation Index**} & \multicolumn{2}{c}{**Linear-Elastic Material**} & \multicolumn{2}{c}{**Hyperelastic Material**} \\ \cline{2-5}  & **Nominal** & **Real** & **Nominal** & **Real** \\  & **Stress-Strain** & **Stress-Strain** & **Stress-Strain** & **Stress-Strain** \\ \hline RMSE & 0.203 & 0.428 & 0.049 & 0.062 \\ MAE & 0.199 & 0.385 & 0.041 & 0.054 \\ R\({}^{2}\) & 0.926 & 0.971 & 0.996 & 0.999 \\ \hline \hline \end{tabular}
\end{table} 
Table 4: Evaluation and comparison of two constitutive models. Figure 6: Stress-strain curves obtained by two numerical simulation methods. (**a**) Nominal stress-strain curve. (**b**) True stress-strain curve. The element mesh was refined in the surrounding area of the tunnel. The element size is controlled within 0.05 m in the area of the composite lining, and the element mesh in the surrounding rock gradually becomes sparse from inside to outside. In order to improve the simulation accuracy of crack length, the tunnel's shotcrete was divided into two layers of elements, and the secondary lining is divided into seven layers of elements. The whole model takes the \(x\)-axis direction as the horizontal direction and the \(y\)-axis direction as the vertical direction. The number of nodes is 32,736, and the number of elements is 32,603. The finite element model is shown in Figure 8. To compare and analyze the cracking effect of the cohesive element, two finite element models with and without cohesive elements were established. For the finite element model with cohesive elements, the cohesive elements with a thickness of 1 mm were established every 15\({}^{\circ}\) along the circumferential direction of the tunnel. The cohesive elements penetrate from the lining surface to the boundary of the finite element model. The mesh of the finite element model without cohesive elements is unified with the cohesive model so that the influence of mesh is excluded in the comparison of subsequent simulation results. The material parameters of rock mass refer to the engineering geological report of Chuosijia Hydropower Station, and the surrounding rock of its diversion tunnel was mainly identified as the class III rock mass. After the excavation of the tunnel, C25 shotcrete was  
Figure 8: Two-dimensional finite element model of the tunnel. Figure 7: Tunnel profile in the simulation (unit: cm). sprayed with a thickness of 10 cm. Subsequently, the C30 secondary lining was poured, and the lining thickness was 35 cm. The mechanical parameters of the surrounding rock, shotcrete, and secondary lining concrete are shown in Table 5.  
The cohesive elements inserted in the model can be divided into three types: cohesive elements that simulate the fracture of surrounding rock, shotcrete, and secondary lining concrete, respectively named Cohesive-ROCK, Cohesive-C25, and Cohesive-C30. The cohesive element properties mainly include normal stiffness, tangential stiffness, crack initiation stress under the quads damage criterion (including normal crack initiation stress and tangential crack initiation stress), and the damage evolution fracture energy parameters using the energy form of BK criterion (including normal fracture energy and tangential fracture energy). The parameters used in the simulation are shown in Table 6.  
The simulated tunnel has a buried depth of 100 m, and its internal water pressure increases from 1 MPa to 5 MPa to investigate the fracture effect of the cohesive element.