## 4 Test Results and Discussion
### FE Analysis  
Further detailed analysis was conducted using FE analysis. The numerical modeling and analysis were performed using ABAQUS 2021 for the nonlinear inelastic analysis of developed structures [24]. Figure 10 shows the FE model used in this study. The FE mesh of the target structure was constructed using C3D8s (the nodes' linear brick elements) to accurately predict the three-dimensional behavior of the structure. The stress-strain relationship of the steel used in the FE analysis was assumed to exhibit elastic-perfectly plastic bilinear behavior. The contact interface of the block and hinge connection was simulated using a small sliding contact element of ABAQUS. To define the tangential and normal characteristics of the contact between the surfaces, the penalty method and hard contact were assumed, respectively. In the FE model, a tangential friction coefficient of 0.3 was incorporated, as per the AISC specifications, specified for unpainted clean mill scale steel surfaces. Figure 10: FE model used in the analysis. (**a**) Overall; (**b**) Male connector (left) and female connector (right); (**c**) Upper pin (top) and lower pin (bottom). The mesh size varies in different areas of the model. The largest mesh size is 50 mm, which is used for beams and stiffeners in the area far from the connection region. The smallest mesh size is 5 mm, which is used for the bolts and the pin. A mesh sensitivity analysis was performed to obtain the optimal mesh size in the intersection area between the coarse and fine meshes. Hence, in this study, the authors used an overall mesh size of 30 mm in the intersection area (please refer to Figure 11). To apply boundary and load conditions more similar to the experimental conditions, the two lower rigid cylinders in Figure 10 were fixed in space, and a vertical displacement load was applied to the two upper rigid cylinders. Contact conditions were considered for all parts. Figure 12 compares the moment-rotation relationship from the test result with that from the FEM result, superimposed. This figure shows that the FE model used in this study has sufficient accuracy to describe the overall experimental results. In the case of the analysis model, a sudden slip appears immediately at the beginning when the pin is in contact with the pin plates. For the subsequent behavior, the FE model exhibits greater stiffness than the experimental results; however, the overall strength is consistent. Strain data were also compared with the measurement values, which showed that the strain data measured in the pin plates remained in the elastic state at the measurement points, as intended in our design. Similarly, for the strain measured in the lower flange of the beam, we were able to obtain plastic deformation beyond the elastic limit as intended. When considering the failure modes calculated in Table 2, the shear failure of the pin plate and the shear failure of the pin were the primary concerns. As anticipated, stress concentrations along the longitudinal direction of the pin plates and at the point where shear occurs in the pin were observed. Figure 13 illustrates the stress distribution based on the FE results. As depicted in Figure 13a, a plastic hinge forms where the beam is connected outside the connecting part. Additionally, within the connector parts, the applied moment at the mid-span of the beam is countered by stress concentration on the lower part of the pin plates and the upper part of the bearing blocks. Figure 13b,c detail the stress distributions of the male and female connectors, respectively. In the case of the bearing block, compressive stress is efficiently transferred to the upper flange of the beam through the upper flange and the web of connectors. Regarding the pin plates, both the male and female connectors withstand tensile forces, transferring stress from the periphery of the pin to the lower flange. Figure 11: Mesh sensitivity analysis.