## 3 Effect on Stress Characteristics by Numerical Simulation  
### Finite Element Modeling  
A finite element analysis was performed using Abaqus v6.16 to investigate the stress redistribution resulting from diaphragm collapse. The computational models incorporated both the steel bridge deck (Q345 qD steel, made in Jinan, China, \(E=206\) GPa, \(\
u=0.3\)) and pavement layer (60 mm thickness, \(E=1000\) MPa, \(\
u=0.3\)), with perfect bonding assumed at their interface. A linear elastic material behavior was adopted, as the study focused on stress characteristics rather than fatigue crack propagation.  
A comprehensive segmental bridge deck model was developed to assess the stress distributions across various wheel load configurations and establish sub-model boundary conditions. The global model encompassed five diaphragms spaced at 3200 mm intervals and six U-ribs with 600 mm spacings, spanning 12,800 mm in length and 4200 mm in width [11]. The structural components were modeled with the following specifications: (1) U-rib profile, 280 mm in height with 300 mm upper and 169.3 mm lower flange widths; (2) thickness parameters, 16 mm (deck), 10 mm (diaphragm), and 8 mm (U-rib web); and (3) mesh configuration, 50 mm eight-node hexahedral elements for all components  
The loading protocol employed a single wheel configuration from the JTG D64 standard fatigue vehicle [20], with a 0.5 MPa contact pressure distributed over a 600 \(\times\) 200 mm rectangular area (Figure 5). Consistent with the established practices [21; 22; 23], this simplified loading approach was implemented to evaluate the critical stress conditions. The longitudinal load positioning followed a 250 mm incremental scheme, covering the complete span of the longitudinal axis of the global model. While gravitational effects are inherently present in structural components, this study focused specifically on diaphragm deformation-induced stress variations at fatigue-prone details of orthotropic steel decks, and therefore, ignored the gravitational effects from the FE analysis [11; 24].  
The global modeling approach incorporated diaphragm deformation effects, with a particular focus on the central U-rib pair of the third diaphragm. From these, a representative sub-model was extracted for a detailed analysis (Figure 6). The model symmetry permitted simplification to a single U-rib for computational efficiency, while maintaining analytical rigor. The global model employed a 50 mm mesh consisting of eight-node linear brick elements (C3D8R), comprising 81,000 elements and 140,000 nodes. Fixed constraints (UX = UY = UZ = 0) were applied at cross-sections of the deck plate, diaphragms, and U-ribs to prevent rigid body displacements under vehicular loading. For the comparative analysis, two distinct sub-model configurations were established as follows: Type I (undeformed diaphragm reference case) and Type II (deformed diaphragm case). Both configurations maintained identical dimensions of 600 mm (width) \(\times\) 400 mm (length) to ensure consistent evaluation conditions. The mesh size was set to 25 mm, and the mesh size of the area of  
Figure 5: Model standard fatigue vehicle load.  
interest was defined to 1 mm (i.e., the number of elements in the direction of the diaphragm thickness was 10). The element type of the sub-model was the same as that of the global model. The sub-model was discretized using four-node linear brick elements (C3D10), with refined and unrefined regions containing 130,000 elements and 170,000 nodes, respectively. Displacement boundary conditions were applied at the sub-model cross-sections using the corresponding results from the global model analysis. Both the global and sub-models were implemented as three-dimensional models to ensure computational reliability [25]. The stress analysis employed the [PERSON] criterion [26], which effectively characterizes fatigue failure in metallic materials through its evaluation of equivalent stress distributions.