Examples of Finite Element Models of Steel-Concrete Composite Bridges - Finite Element Analysis and Design of Steel and Steel-Concrete Composite Bridges - page 616

B1 and B2 are identical in profile except for the plate thickness in webs and
bottom flanges. The diagonal and horizontal bracings were modeled by a
combination of beam elements in the central part and shell elements at
the ends. Couplings of six degrees of freedom were used to join the beam
element with the shell elements at a distance of roughly 0.8 m from the bolt
connection. The preloaded high-strength bolt connections were assumed to
be rigid, realized by TIE constraint between bolt holes and gusset plate. TIE
option in ABAQUS is a surface-based constraint used to make all the trans-
lational and rotational degrees of freedom equal for a pair of surfaces. Three
types of segments were assembled one by one to build up the global finite
element model of the second span. The steel box girder was simulated by
shell element S4, and the bracings were modeled by beam element B31
in combination with shell element S4. The ballast was assumed as continuum
with material properties as found in literature [ 7.26 ]. The concrete deck and
the safety barrier were modeled by brick element C3D8. The shear studs
were not explicitly modeled and TIE constraints were applied to connect
the concrete deck to the top flanges of the steel box girder. The FE model
contained about 84,000 shell elements, 6400 solid elements, and 1800 beam
elements, resulting in more than 85,500 nodes. The symmetrical vibration
modes of the span were predominantly excited by the train passages. There-
fore, symmetrical boundary conditions were adopted at the ends of the span.
The longitudinal translations and rotations of the rails and the ballast
were restricted. The bridge bearing system included two fixed bearings,
three bidirectional sliding bearings, and one unidirectional sliding bearing.
The bearing system allowed relative movements due to thermal expansion
and accommodated the bridge to movements due to live loads. The train
was composed of a locomotive followed by eight-passenger cars and another
locomotive. In the static and dynamic finite element analyses, the moving
load model, in which the train axles were represented by a series of moving
constant forces, was adopted to simulate the train passage. An ABAQUS user
subroutine DLOAD coded by FORTRAN was used to realize the loading
scheme of the train.
Finally, Liu et al. [ 7.27 ] investigated the performance of composite joints
in a truss bridge with double decks. Fatigue tests of three composite joints
with different connectors such as headed studs, concrete dowels, and perfo-
rated plates under constant repeated loading were carried out. The responses
of displacement, strain distribution, crack development, relative slip
between concrete, and steel were observed after different loading cycles.
The experimental results showed that the deflection increased almost