Examples of Finite Element Models of Steel Bridges - Finite Element Analysis and Design of Steel and Steel-Concrete Composite Bridges - page 583

Figure 6.18 Finite element mesh of the full-scale built-up I-section plate girder T3.
at midspan, which is identical to the test T3. The load was applied in incre-
ments as concentrated static load using the RIKS method (see Section 5.5.4 of
Chapter 5 ) that is also identical to the experimental investigation. The non-
linear 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 measured values of the yield stress ( f ys ) and ulti-
mate stress ( f us ) used in the tests [ 6.8 ]. 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 inelas-
tic strains, the nominal (engineering) static stress-strain curves were con-
verted to true stress and logarithmic plastic true strain curves as detailed
in Section 5.4.2.
The same modeling approach [ 6.28 , 6.29 ] was followed in this topic
to model initial geometric imperfections of the plate girder investigated
T3. In Figure 6.19 , the buckling mode predicted from the eigenvalue buck-
ling analysis detailed in ABAQUS [1.29] is shown. 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
to 1.0, the buckling modes are factored by a magnitude of L u /1000, where
L u is the length between points of effective bracing. The magnitude of