## 2 Finite Element Simulation
### Methodology  
The steps shown in Figure 5 are required for numerical simulations using the finite element software ABAQUS [11]. In numerical simulations, the model can abort the calculation in a variety of ways. The reasons for this could all be related to the ways in which certain steps are set up in the model, causing it to fail to converge (see the area indicated by the \"No\" arrow). The following are the steps of the experiment simulated in this paper:  
Step 1. Create model: Modeling based on the geometry given in the experiment. Step 2. Material property settings: The properties of the materials are input as described in the experiment. The damage plasticity model is used to describe the concrete, and its input parameters must be calibrated, as explained in Section 2.4. Step 3. Assemble the components: The assembly of the components requires attention as to the direction of the coordinates. Step 4. Mesh: The model is divided into meshes that need to be cut into regular shapes in advance. The concrete and reinforcement elements need to be typed. One element type is the completely integral element, and when the element has a regular shape, the number of Gaussian integral points used is sufficient to precisely integrate the polynomial in the element stiffness matrix. The disadvantage is that under bending load there will be shear self-locking, resulting in the element being too rigid, even with the division of a very fine grid, so the calculation accuracy is still very poor. The other type is the reduced integral element, which uses one less integral point in each direction than the normal full integral element, has only one integral point in the center of the element, and is too soft due to the hourglass value problem (Figure 6). When a linear integral element is used to simulate a structure subjected to bending load, at least four elements should be divided along the thickness direction. According to the grid sensitivity test conducted by [PERSON] (2015) [17], the smaller the grid size, the earlier the component is destroyed--that is, the smaller the deflection or rotation. After experience verification, it is sufficient to ensure 4 grids in the thickness direction. Therefore, the mesh sizes of the two experimental models simulated in this paper were 45 and 40, respectively, as shown in Figure 7. The 8-noded \begin{table}
\begin{tabular}{c c c c c} \hline \hline \multirow{2}{*}{**Specimen**} & \multirow{2}{*}{\(f_{c}\)**, MPa**} & \multicolumn{2}{c}{**Distance of the First Row of Studs**} & \multirow{2}{*}{**Studs’ Spacing, mm**} & \multicolumn{1}{c}{**Number of Studs on Each**} \\  & & & **from the Column Surface, mm** & & **Steel Plate** \\ \hline P1 & 24 & 68 & 101 & 4 \\ \hline P2 & 24 & 68 & 75 & 7 \\ \hline P3 & 25 & 47 & 68 & 9 \\ \hline P4 & 25.1 & 54 & 78 & 9 \\ \hline P5 & 25.3 & 47 & 68 & 7 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Characteristics of the [PERSON] and [PERSON] test slabs. Figure 5: Simulation flowchart. hexahedral (brick) reduced integral elements, C3D8R, were used for simulating concrete, where C represents the solid element, 3D means three-dimensional, 8 is the number of nodes in this unit, and R represents this unit as a reduced integral unit. The 2-node linear truss element, T3D2, was used to model the reinforcement. The choice of the element type of shear studs needed to be trialed, as shown in Figure 8, using solid and truss elements to simulate the shear studs. The load-displacement curves (Figure 9) show that the solid elements failed prematurely, did not contribute to the strength of the slab, and were less ductile. The results of the truss elements simulating the shear studs were similar to the experimental values. Therefore, truss elements were used for the simulation of shear reinforcement in this study. Figure 8: Different element types for shear studs: (**a**) solid elements; (**b**) truss elements. Figure 6: Linear reduced integration element subjected to bending moment. Figure 7: Mesh division: (**a**) Model of [PERSON] et al.