In order to assess the reliability of the proposed FE model to evaluate
the welding distortion, the uz (Figure 2C)
displacements of the plate have been measured at some locations of the
joints, by means of a Coordinate Measuring Machine (CMM).
2. Finite element model
The numerical simulation of a welding process involves the investigation
of the thermo-mechanical response of the joint. This behaviour can be
simulated by a numerical method, by using an uncoupled approach
consisting of two consecutive analyses: the former, where the thermal
problem is solved independently on the joint mechanical response, under
a free-free configuration, to obtain the temperatures distribution; the
latter, consisting of a subsequent mechanical analysis, where the
temperatures history previously predicted at each node is used as
thermal load. Such uncoupled approach, which is well established in
literature for such type of analyses,17,22,34 allows
saving computational costs with respect to the coupled one, with a
comparable and an acceptable level of accuracy. All simulations have
been carried out by means of the finite element commercial code
ABAQUS® v. 6.14.
The same FE model has been used for both thermal and mechanical
analyses. Concerning the mesh, 8-nodes hexahedral 3D finite elements
have been used for both base and weld zones. More in detail, DC3D8
finite elements have been used for the thermal analysis, allowing
introducing the temperature as unique degree of freedom, and C3D8 finite
elements, characterized by the three translations as degrees of freedom,
has been used for the mechanical analysis. According to Figure 3, a
finer mesh has been developed for the chamfer region; a transition mesh
for the HAZ (Heat Affected Zone) region and a coarser mesh, with a
linear bias, for the other parts of the plate. As a result, FE model
counts a total of 11904 finite elements and 14175 nodes.