*2.2. Finite Element Model Development*

Finite element modeling was performed using the general-purpose finite element program LS-DYNA [24]. For the deck model, 8-node solid elements, 4-node shell elements, and 2-node beam elements are used for the concrete slab, steel girder, and reinforcing bars, respectively. The deck model consists of 288,332 nodes and 198,550 elements, and the edge lengths range from 0.05 to 0.15 m. The concrete slab of the model is divided into 5 layers of elements. Stay cables are modeled as solid round bar shapes with 8-node solid elements. The numerical models of the cable #37, 53, and 68 consist of 87,362, 39,668, 73,205 nodes and 77,686, 35,316, 65,232 elements, respectively. The overall edge length ranges from 0.10 to 0.50 m, and the finer mesh with 0.02 to 0.05 m of edge length is generated at the region of the application of the blast load. In the pylon model, there is a concrete part and a reinforcing bar part. The concrete part and the reinforcing bar parts consist of 8-node solid elements and 2-node beam elements, respectively, and the pylon model has 1,185,084 nodes and 917,438 elements. The section submitted to the blast load was modeled with smaller element sizes of 0.05 to 0.20 m. The remaining sections were configured using element sizes of approximately 0.5 m. For the rebars, the specifications in Table 2 were applied. The composite conditions for the concrete and rebars were implemented using the \*CONSTRAINED\_LAGRANGE\_IN\_SOLID command. The contact condition between the steel girders was applied considering the case of a large, load-induced deformation, using the \*AUTOMATIC\_SINGLE\_SURFACE command. Figures 3–5 illustrate the finite element models of the superstructure, cables, and pylon. –

**Figure 3.** Deck model: (**a**) slab, (**b**) steel girder, and (**c**) rebar.

–

(a) (b) (c) **Figure 4.** Cable model: (**a**) Cable no. 37, (**b**) Cable no. 53, and (**c**) Cable no. 68.

**Figure 5.** Pylon model: (**a**) concrete part and (**b**) rebar.

#### *2.3. Material Model*

— — When selecting a material model for blast analysis, various material properties—in particular, the strength increasing effect due to the strain rate—must be considered. Therefore, we selected the following material model from LS-DYNA:

For the concrete, the \*MAT\_CSCM\_CONCRETE material model was applied; this captures the nonlinear material behaviors of concrete, as well as its stiffness degradation arising from damage, erosion, and the strain rate effect [25,26]. A compressive strength (fck) of concrete was selected as 39.23 MPa, and 1.05 was used as the ERODE parameter, to simulate erosion of the concrete element in the blast analysis.

– To model the steel plates in the girders, rebars, and cables, the \*MAT\_PLASTIC\_KINEMATIC material model was applied. This model considers the strain rate effect, isotropy, and kinematic hardening of the material, and it assumes a bi-linear material nonlinearity. The material constants C and *p* (used in the Cowper–Symonds model, which describes the strain rate effect) were determined using the following equation, developed for high-strength steel [27]. Usually, the C value of 40 is applied to normal structural steel, but this value is known to overestimate the strain rate effect of high-strength steel. Therefore, the experimentally validated Equation (1) is used to calculate the C value in order to prevent overestimation of the strain rate effect.

$$\mathbf{C} = \begin{cases} 92000 \cdot \exp\left(\frac{\sigma\_0}{564}\right) - 194000, & \sigma\_0 > 270 \text{ MPa}, \\ & 40, \ \sigma\_0 \le 270 \text{ MPa}, \end{cases} \\ p = 5. \tag{1}$$

 = 5. σ0 where, σ<sup>0</sup> is the yield stress (MPa). In addition, the strengths selected for the steel plates in the girders were varied according to the thickness. The input parameters used for each material model are listed in Table 3.

–

ρ

ρ ε


**Table 3.** Material model input parameters.
