## 2 Finite Element Model of Prefabricated Modular RCS Composite Node
### Finite Element Analysis and Verification of Prefabricated RCS Composite joints  
We used ABAQUS software to perform finite element analysis on the prefabricated modular reinforced concrete column-steel beam composite node. The stress distribution of the concrete, steel beams, and connecting components was simulated using an eight-node three-dimensional solid element C3D8R. The internal reinforcement in the concrete was modeled using a two-node linear truss element T3D2. To improve computational accuracy, the mesh was densified in the node area and at the steel beam connections, with specific  
Figure 5: Framework model node selection. \begin{table}
\begin{tabular}{c c} \hline \hline
**Component Name** & **Component Materials and Properties** \\ \hline steel products & Q235B \\ steel section & NH350 \(\times\) 175 \(\times\) 7 \(\times\) 11 mm \\ short beams are embedded in the column & 590 mm \\ extruded steel beam & 1100 mm \\ steel stiffening rib & 332 \(\times\) 84 \(\times\) 10 mm \\ steel plate A & 345 \(\times\) 175 \(\times\) 8 mm \\ steel plate B & 345 \(\times\) 80 \(\times\) 8 mm \\ steel plate C & 330 \(\times\) 300 \(\times\) 6 mm \\ concrete strength & C30 \\ concrete column & 2200 \(\times\) 400 \(\times\) 400 mm \\ reinforcing bars in columns & HRB335 \\ column hoop reinforcement & HPB235 \\ High-strength friction grip bolt & Grade 10.9 M20 \\ \hline \hline \end{tabular}
\end{table} 
Table 3: Node component material parameters. dimensions of 50 mm for the concrete and steel beams, 30 mm for the connecting steel plates, and 10 mm for bolts. Figure 6 shows the meshing details. In the ABAQUS finite element analysis software, the analysis step module provides functional components for defining the analysis steps, setting result output parameters, and monitoring the solution process. In this study, the load application on the prefabricated RCS nodes consists of three main aspects: first, the application of pre-tension for high-strength bolts; second, the axial force applied to the column components; and finally, the low-cycle cyclic load applied at the ends of the beams. The entire analysis process includes six independent analysis steps, namely Initial, Step 1 to Step 5. In each analysis step, the geometric nonlinearity calculation option is enabled to account for deformation effects. In the initial analysis step (Initial), temporary fixed boundary conditions are applied to keep the various components of the node in their initial fixed state during assembly. Subsequently, in Step 1, an initial pre-tension of 5 Kn is applied to the bolts. In Step 2, the pre-tension of the bolts is gradually increased to 155 Kn. In Step 3, the current length of the fixed bolts is selected to maintain their pre-tension state. Following this, in Step 4, the temporary boundary conditions for the bolts are removed, and axial pressure is applied at the top of the column. Finally, in Step 5, a cyclic displacement load is applied to the reference point at the ends of the beams (refer to JGJ 82-2011) [28]. In the model, contact between components is defined through the Interaction module. The contact between the core area reinforcement cage and concrete is handled using the Embedded Region command. Surface contact is set between the steel beams, high-strength bolts, and pressure-bearing steel plates, with the stiffer surface being the primary contact surface, and the friction coefficient is 0.35 (Figure 7). The loading steps include initial boundary setting, a gradual increase in the bolt preload, and setting the column axis and applying cyclic load at beam ends; the loading and boundary conditions are adjusted according to the test conditions. To minimize the stress concentration and enhance the effectiveness of load application, reference points RP-1, RP-2, and RP-3 are established at the center of the column bottom of the RCS combination node, the center of the column top, and the loading center at the beam end, respectively.