# A Study on the Seismic Performance of Steel H-Column and T-Beam-Bolted Joints
## 2 Establishment and Verification of Model
### Model Verification  
The unilateral bolted joints of T-shaped parts in the steel structure, as described in the literature [1], were simulated and calculated using ABAQUS (v.2022) [20]. The ABAQUS model was calibrated using the test results of JT141 specimens from [PERSON] et al. [1], ensuring consistency in failure modes and load-displacement responses (see Figures 6 and 7). The JT14-1 specimen from the relevant test was selected for verification purposes, and the calculated results were compared with the test results. The specimen's T-plate dimensions (T320 \(\times\) 200 \(\times\) 16 \(\times\) 24) and column wall thickness (14 mm) align with typical engineering practices for H-beam to square steel-column connections [4; 8]. Additionally, the cyclic  
Figure 5: Test loading device. (**a**) Test loading device. (**b**) Loading site. loading protocol followed AISC 341-16 guidelines, ensuring relevance to seismic design scenarios. The validity of the ABAQUS model was determined by comparing the failure modes, hysteresis curves, and skeleton curves of the specimens. Numerical comparisons show a stiffness deviation of \(\leq\)12% and peak load difference of \(\leq\)8% between the simulation and test results (Table 3). The equivalent viscous damping coefficient error was within 15%, confirming acceptable accuracy for hysteretic behavior prediction. The geometric lengths of the beams and columns and the detailed dimensions of the joints are presented in Figure 5a. In the test, a pseudo-static test method was adopted, and the test setup is shown in Figure 5b. Figure 6 presents the comparison results between the test failure and the finite-element simulation. The left-hand side depicts the test failure phenomenon reported in the literature [21], while the right-hand side shows the finite-element simulation result of this study. During the test, a fracture occurred at the upper flange of the T-shaped joint, and the same outcome was obtained in the ABAQUS simulation. Moreover, the degree of  
Figure 6: Comparison of experimental simulation results. (**a**) Failure mode. (**b**) Stress nephogram. Figure 7: Comparison of experimental and simulated results. (**a**) Hysteresis curve. (**b**) Skeleton curve. bending deformation of the T-shaped parts in the finite-element simulation is consistent with that of the test. Continuum Damage Mechanics (CDM) was used in ABAQUS simulation to simulate fracture behavior by defining material stiffness degradation criteria (such as plastic-strain threshold). Although the stress cloud map in Figure 6b does not show an explicit crack, the fracture location is indirectly reflected through the stress concentration region (\(\sigma\geq 510\) MPa, reaching the ultimate strength of Q355B steel) and the accumulation of plastic strain (not shown in the figure). This method conforms to the fracture prediction convention of continuum model in implicit analysis. Figure 7 compares the hysteretic curves and skeleton curves of the test and the finite-element analysis. In the finite-element simulation, the initial stiffness is relatively high. Because the material properties assumed in the finite-element model are relatively ideal, the stiffness degradation caused by the anisotropy of the steel under cyclic loading is not taken into account. In contrast, during actual tests, the steel often has initial defects, which cause a reduction in hardness. Additionally, the contact surfaces between components are not perfectly fitted, and the friction coefficient of the contact surface changes during the loading process, while in the finite-element analysis, the friction coefficient is set as a fixed value. The normal contact adopts hard contact, that is, the contact surface is not allowed to penetrate, and the normal stiffness is infinite. Tangential friction adopts the penalty method, the friction coefficient \(\mu=0.3\), allowing the contact surface to slip but the friction should be overcome. This setup is consistent with the study by [PERSON] et al.