## 5 Finite Element Analysis  
### Finite Element Modeling  
A three-dimensional finite element analysis (FEA) model was created using the ABAQUS/Standard module to represent the tested joint. Due to the symmetric conditions along the longitudinal plane, half of the connection was modeled to improve calculation efficiency. The material and geometric nonlinearities and complex contact interactions between the various elements were considered in the analysis. All parts were modeled using 8-node linear brick incompatible mode elements (C3D8R), which are a linear displacement interpolation solid (brick) based on reduced integration. The model was divided into seven parts: the end-plate, steel beam, steel tube wall, C-channel, concrete, bolt and sleeve. For model simplification, the bolt and nut were modeled as the same component, and the bolt heads and nuts were modeled as circular parts. The structured mesh control was adopted for all parts; the model assembly and mesh of the components are shown in Figure 23. The influence of the weld was ignored, and welding relationships between the steel components were achieved by tie constraints. The connections contain several different complex contact interfaces between the  
Figure 22: \(W_{\text{total}}\) and \(\xi_{\text{e}}\) versus the drift ratio. (**a,c**) Specimens SJ-1 through SJ-5; (**b,d**) Specimens SJ-3, SJ-4, SJ-6 through SJ-8.  
\begin{table}
\begin{tabular}{c c c c} \hline \hline
**Specimen Number** & \(\mathbf{E_{\text{e}}}\) & \(\xi_{\text{e}}\) & \(\mathbf{W_{\text{total}}}\) (kN-m) \\ \hline SJ-1 & 1.69 & 0.27 & 57.50 \\ SJ-2 & 1.77 & 0.28 & 56.82 \\ SJ-3 & 1.93 & 0.31 & 36.93 \\ SJ-4 & 1.41 & 0.22 & 18.81 \\ SJ-5 & 1.64 & 0.26 & 42.10 \\ SJ-6 & 1.06 & 0.17 & 21.83 \\ SJ-7 & 2.35 & 0.37 & 46.63 \\ SJ-8 & 2.33 & 0.37 & 31.19 \\ \hline \hline \end{tabular}
\end{table}
Table 5: Energy dissipation parameters of the specimens in the limit state.  
components, and surface-to-surface contact was employed in the FEA model to define those contacts, which consist of a contact pressure model in the normal direction and a Coulomb friction model in the tangential directions. The boundary conditions in the model were consistent with the actual boundary conditions of the specimens, and the symmetric boundary conditions were applied. As the test load was controlled through displacement, the load in the FEA was applied by establishing reference points coupled with the loading surface and applying a certain displacement value.  
A simplified trilinear model proposed by [PERSON] et al. [31] was proposed for the stress-strain relationship of the steel, as shown in Figure 24. The elastoplastic stress-strain relationship was based on the von Mises yield criteria and isotropic hardening rule. The damaged plasticity model was adopted for simulating the concrete properties in this study. The model allowed for the input of a multilinear uniaxial compression stress-strain curve and provided the general capability for the analysis of concrete under monotonic loading based on a damaged plasticity algorithm. This study adopted the uniaxial stress-strain relationship model proposed by [PERSON] et al. [32] for the core concrete in the ABAQUS software.