# Effect of High-Temperature Pavement Paving on Fatigue Durability of Bearing-Supported Steel Decks
## 4 Modeling of High-Temperature Pavement Paving  
### Coupled Thermal-Structural Analysis  
The residual temperature stress was analyzed based on numerical results. For this purpose, it is necessary to simulate the high-temperature pavement paving process first. In this study, the FE model for the coupled thermal-structural analysis was developed using ABAQUS. The dimensions of the model are given in Figure 7, and the FE model is shown in Figure 8. The model was composed of pavement, deck plate, base plate, 21 U-ribs (U1 to U21), four diaphragms (D1 to D4), and 18 bearings with nine at each section (S1 to S9). It should be noted that only the sublayer pavement (PGA) with a thickness of 40 mm was simulated here, neglecting the wearing course. The dimensions of the bearing were 600 (length) \(\times\) 600 (width) \(\times\) 20 (thickness) mm. To increase the computational accuracy, the asphalt surfacing, deck plate, U-ribs, base plate, and bearings were simulated by thermal-type solid elements (DC3D8), while the other parts were simulated by thermal-type shell elements (DS4). The global meshing size was 0.2 m, while the meshing sizes of asphalt surfacing, deck plate, bearing, and adjacent regions were refined to be 20 mm. In this case, the number of total elements and nodes are 161,195 and 229,375, respectively. The elastic modulus and Poisson's ratio of steel were set to 206 GPa and 0.3, respectively. In the process of asphalt pavement paving, the payer can be considered  
Figure 6: Monitored displacement of the bearings during the paving process. as a moving heat source, thus the space-time change law of local thermal field is presented in the steel bridge deck. Hence, the thermal field of the steel bridge deck during PGA paving is treated as the transient temperature field. Hence, the element deletion approach was adopted to simulate the dynamic process of PGA paving. The simulation procedure is summarized below. Firstly, the FEM simulating the segment of OSD was developed according to the geometric sizes. The boundary conditions and thermal parameters were applied to the FE model, which are introduced in the next section. Secondly, the pavement model was divided into 10 parts along the longitudinal direction, and all elements representing the pavement were deactivated. Subsequently, the first 10 steps were utilized to successively reactivate the pavement elements to simulate the dynamic paving process. The paving speed was controlled by the time period for each step. The paving speed of actual asphalt payer was controlled to be in the range of 2.0 to 2.5 m/min. Hence, the paving speed in the numerical simulation was set as 2.0 m/min. That is, the time period for each step was 60 s. Finally, the definition of 11 heat transfer steps was completed. The 11 th step was set to simulate the temperature variation when the paving process was completed. The total calculating process lasted for 7200 s (i.e., 2 h). The solutions time was about 8 h.  
The physical boundary conditions were the same with the actual situation. In NYRB, the OSD was placed on the girders using spherical tension-compression bearings, including bidirectional movable bearings, unidirectional movable bearings, and fixed bearings. Accordingly, in the numerical simulation, the displacements along the X, Y, and Z-axes of S1 were constrained to simulate the fixed bearing. The displacement along the Y-axis of S3, S5, S7, and S9 was constrained to simulate the bidirectional movable bearing. The displacement along the Y-axis and Z-axis of S2, S4, and S6 was constrained to simulate the unidirectional movable bearing. The temperature boundary conditions were also similar to the actual environment. The temperature of OSD was determined by the coupled effect of natural convective heat transfer, solar radiation,  
Figure 8: Finite element (FE) model as built (unit: mm). Figure 7: Geometric sizes of the model (unit: mm). and radiation heat transfer.