Examples of Finite Element Models of Steel-Concrete Composite Bridges - Finite Element Analysis and Design of Steel and Steel-Concrete Composite Bridges - page 632

simulating the wheel loads of one HS truck in each lane. The point load
locations were chosen to produce the maximum positive moment near mid-
span of the second span. The loads were applied at each of the eight load
points through a using 900 kN capacity center hold jack. Since the slab rein-
forcement and cross-frame details were not reported [ 7.31 ] , it was calculated
according EC2 [2.27] to be T16 spaced at 150 mm transversely and longi-
tudinally. The reinforcement steel bars were Grade 40 having a yield stress of
275 MPa (40 ksi). The top and bottom reinforcement bars had a cover of
40 mm. Cross-frame members were also calculated according to EC3
[2.11] to be two angles back to back of 120 120 12 spaced at average
distances of 7 m.
The full-scale steel-concrete composite plate girder tested by Burdette
and Goodpasture [ 7.31 ] was modeled in this topic using ABAQUS
[1.29]. In order to obtain accurate results from the finite element analysis,
all the bridge components must be properly modeled. The composite bridge
components comprise the steel beams, concrete slab decks, headed stud,
reinforcement bars, and support locations. The finite element analysis has
accounted for the nonlinear material properties and geometry of the com-
ponents as well as the interfaces between the components that allowed the
contact and bond behavior to be modeled and the different components to
retain its profile during the deformation of the composite bridge. The steel-
concrete composite bridge were modeled using a combination of 3-D solid
elements (C3D8 and C3D6) available in the ABAQUS [1.29] element
library. Only half of the composite bridge was modeled due to symmetry
as shown in Figure 7.17 . The total number of elements used in the model
was 9312 elements. Different mesh sizes were tried to choose the reasonable
mesh that provides both reliable results and less computational time. All the
nodes in the middle symmetry surface were prevented to displace in dir-
ection 1-1. The roller support nodes were prevented to displace in direction
3-3 only, while hinged supports were prevented to displace in directions
2-2 and 3-3 only. The load was applied in increments as concentrated static
loads at midspan using the Riks method, which is identical to the experi-
mental investigation [ 7.31 ]. The steel beams were prevented to displace lat-
erally in direction 2-2 at the locations of the lateral restraints. The nonlinear
geometry was included to deal with the large displacement analysis.
The shear forces across the steel beam-concrete slab interface of the
bridge test [ 7.31 ] were modeled following the same approach [2.68,2.69],
and the load-slip characteristic of the stud was inserted in the finite element
model ( Figure 7.17 ) using nonlinear springs in direction 2-2 at the location