Civil Engineering Reference
In-Depth Information
cross girders (see
Figure 6.27
)
. Finally, it is found that approximately
153
260 mm ratio provides adequate accuracy in modeling the webs of
the stringers, while a finer mesh of approximately 96
260 mm was used
in the flanges of the stringers (see
Figure 6.27
). The hinged supports of
the bridge attached to the main plate girders, shown in
Figures 6.25
and
6.26
, were prevented from displacement in the horizontal direction (direc-
tion 1-1) and the vertical direction (direction 3-3). On the other hand, the
roller support of the bridge, shown in
Figures 6.25
and
6.26
, was prevented
from displacement in the vertical direction only (direction 3-3).
The developed finite element model shown in
Figure 6.27
can be now
used to analyze the bridge for any analysis, boundary conditions, geome-
tries, and loadings. As an example in this topic, the bridge was analyzed for
the unfactored live load case shown in
Figure 6.26
and analyzed to predict
the ultimate load that can be carried by the bridge up to complete failure.
The live load case was applied in increments as concentrated and distrib-
uted static loads, which is identical to the Load Model 71 adopted. On the
other hand, the ultimate load that can be carried by the bridge was pre-
dicted using the RIKS method to cause maximum deflection at midspan.
The nonlinear geometry was included to deal with the large displacement
analysis.
The stress-strain curve for the structural steel given in the EC3 [2.11]
was adopted in this study with the yield and tensile stresses of 275 and
430 MPa, respectively. The material behavior provided by ABAQUS
[1.29] (using the PLASTIC option) allows a nonlinear stress-strain curve
to be used (see Section 5.4.2 of
Chapter 5
). The first part of the nonlinear
curve represents the elastic part up to the proportional limit stress with
Young's modulus of (
E
) 200 GPa and Poisson's ratio of 0.3 used in the
finite element model. Since the buckling analysis involves large inelastic
strains, the nominal (engineering) static stress-strain curves were converted
to true stress and logarithmic plastic true strain curves as detailed in
Section 5.4.2.
An eigenvalue buckling analysis was performed for the whole bridge to
model initial geometric imperfections of the bridge. In
Figure 6.28
, the
buckling mode predicted from the eigenvalue buckling analysis detailed
in ABAQUS [1.29] is shown. It can be seen from
Figure 6.28
that a clear
web buckling mode due to bending was predicted at midspan panel for
the unfactored live load case shown in
Figure 6.26
.
Only the first buckling
mode (eigenmode 1) is used in the eigenvalue analysis. Since buckling
modes predicted by ABAQUS eigenvalue analysis [1.29] are generalized
Search WWH ::
Custom Search