r - The Hong Kong Polytechnic University

Boundary Simulation
Three-dimensional shell elements S4R, were selected to simulate the whole beam, including beam web, flanges,
and stiffeners and the clip angle connection was modeled by using brick element (C3D8R in ABAQUS). As
lateral bracings were provided in the test, lateral displacement (U 3 =0) was prevented in the finite element
models at the positions of bracing as shown in Figure 2. Suitable boundary conditions were provided to the
finite element models to simulate the simply supported condition and point load was applied to simulate the
loading condition. Bilinear spring elements were used to simulate the bolts between the connection of beam and
the flange of supporting column. The tensile and compressive stiffness of the spring was set as 200 N/mm at
first 0.5 mm in order to account for the slip behaviour. Afterwards, the stiffness was changed to a relative large
value of 40000 N/mm per spring. Those spring properties were obtained by comparing the load versus
deflection curve of the numerical results and test results. In addition, at the edge of bolt hole, freedom of the
outer surface nodes was constrained to be zero on vertical and out of plane direction (U 2 =0,U 3 =0). To simulate
the welding near the clip angles and beam web, multi-point constraints (MPCs) were introduced. It allows
constraints to be imposed between different degrees of freedom of the model. MPC type BEAM provides a rigid
beam between two nodes to constrain the displacement and rotation at the first node to the displacement and
rotation at the second node. Two series of MPC BEAM were used in the models to link the corresponding nodes.
For the nodes associated as Group 1, it is needed to constrain all nodes at the clip angle edge to beam web
directly at the weld root. In order to account for the weld size, the nodes associated as Group 2 paralleled to the
angle edge was linked from a distance of angle thickness to the beam web at the weld leg to be consistent with
the measured weld sizes. Typical finite element mesh and boundary conditions were shown in Figure 2.
Nodes directly connected
to beam web (Group 1)
Using MPC element to
connect to the beam web
(Group 2)
Material Property
Figure 2 Typical finite element mesh and boundary conditions
The isotropic elastic-plastic material properties with the von Mises yield criterion were used for the FE analyses
to account for the effect of the material nonlinearities. As the input values of ABAQUS, the stress and strain are
p
required as true stress ( σ ) and true plastic stain (
true
ε ). Therefore, the nominal stress (
true
σ ) and nominal
nom
strain ( ε ) getting from the tension coupons tests of Zhong et al. (2004), were converted to true stress (
nom
σ )
true
p
and true plastic stain ( ε
true
), using Eqs. (4) and (5). It is emphasized that, the nominal stress ( σ ) and nominal
nom
strain ( ε nom
) were taken from the static stress-strain curves from the coupon tests.
σ
true
= σ
nom( 1+
ε
nom)
(4)
p
⎛ σ
true ⎞
ε
true
= ln( 1+
ε
nom
) − ⎜ ⎟
(5)
⎝ E ⎠
-466-