## 2 Self-Centering Rocking Steel Bridge Pier Structure and Its Finite Element Analysis Model
### Finite Element Analysis Model and Verification  
To systematically investigate the seismic performance of each rocking steel bridge pier as shown in Table 1, a refined finite element model was established using the commercial software Abaqus 6.14. Figure 4 illustrates the finite element model of the pier. In the model, a rigid short beam is used to simulate the top portion of the pier. A horizontal cyclic displacement \(\delta\) and a constant axial force \(N\) was applied at the top of this short beam. The bottom of the short beam is connected to the shell elements below using multi-point constraints (MPCs). The interaction along the normal direction between the pier base and the concrete foundation is modeled through hard contact, while the interaction along the tangential direction is modeled with frictional contact using a friction coefficient of 0.2 [28]. One end of the prestressed tendons is connected to the foundation surface using MPC, while the other end is coupled to the upper end point of the short beam (i.e., the top of the pier) using a two-point coupling connection. The L-shaped buckling-restrained energy dissipating device is connected to one side of the pier using the tie connection, and the other side is connected to the foundation surface using the tie connection, while restraining its out-of-plane deformation. Meanwhile, the bottom of the foundation is fixed. The loading process consists of three static analysis steps. Step 1 applies the constant axial force \(N\) and the self-weight of the pier, step 2 applies the initial prestressing forces through the temperature reduction method, and step 3 applies the horizontal cyclic displacement \(\delta\). In the FE model, Q345 qC steel is used for the pier, and its hysteretic constitutive model adopts the Chaboche cyclic hardening hysteresis model that considers the Bauschinger effect and the cyclic reinforcement effect. Material properties and the parameters of the Chaboche cyclic hardening hysteresis model for Q345 qC steel have been calibrated in reference [29] and are directly utilized in this study. Q235 steel is employed for the energy dissipating component. The yield strength of Q235 steel is 235 MPa and the ideal elastoplastic model was employed as the hysteretic constitutive model of Q235 steel. Both the steel bridge pier and the energy dissipating component are simulated using four-node reduced integration shell elements (S4R). The prestressed tendons are simulated using truss elements (T3D2), while the reinforced concrete foundation is simulated using eight-node reduced integration solid elements (C3D8R). Figure 4: Finite element model of circular-section rocking steel bridge pier: (**a**) Geometric model (**b**) Element discrete method. This paper adopts displacement control to perform horizontal cyclic quasi-static loading on the bridge pier. Figure 5 shows the displacement loading system, where the \(Y\)-axis represents the normalized displacement \(\delta/\delta_{y}\), and the \(X\)-axis represents the number of cycles \(n\). The peak displacement value of each cycle increases incrementally, with the displacement increment being the yield displacement of the pier. To validate the effectiveness of the finite element analysis model used in this study, numerical simulations were conducted on the test rocking steel bridge pier with a base plate, designated as RP3-DT43-PT44-BP20 in reference [24]. The basic parameters of the pier are listed in the Table 2. The test pier was an unreinforced pier at the bottom, and the calibrated results of the Chaboche hysteresis model parameters for the steel material used are provided in reference [25], which were directly incorporated into the FE model in this study. To analyze the influence of pier element size on the calculation results, FE models of the test rocking steel bridge pier were established with shell element sizes of 15 mm, 40 mm, and 70 mm, respectively, for grid sensitivity analysis.