Figure 6 Thermal properties of material dependent on temperature A;
variation of heat loss coefficient H with temperature B;
mechanical properties of material dependent on temperature C; stress vs.
strain curves with temperature D.
Mechanical analysis
Temperature history achieved by the thermal analysis has been used in
the mechanical analysis as thermal loads. An elasto-plastic material
model, based on the von Mises yield criterion and isotropic strain
hardening rule, has been considered, including the effects of the
temperature on the material properties.
The stress-strain relations can be written as:
\(\left[\text{dσ}\right]=\left[D^{\text{ep}}\right]\bullet\left[\text{dε}\right]-[C^{\text{th}}]\bullet dT\),
(17)
being:
\(\left[D^{\text{ep}}\right]=\left[D^{e}\right]+\left[D^{p}\right]\),
(18)
where: [Dep ] is the total stiffness matrix;
[De ] is the elastic stiffness matrix;
[Dp ] is the plastic stiffness matrix and
[Cth ] is the thermal stiffness
Moreover, as aforementioned, a particular attention must be paid on the
modelling of the symmetry boundary conditions. The transient thermal
field generated by the welding process introduces several deformations
inside the plates, leading to their interaction. Such interaction,
which increases as the plate
length increases (due to their rotation), has never been considered in
the FE models proposed in literature17,21,22,31,34,36,
by reducing this problem to a simple application of the symmetric
boundary conditions. This results into too many approximations in the
simulated residual stress-strain state, especially for long plates.
More in detail, when the first component is reactivated together with
its symmetric boundary conditions, the plate starts to rotate due to the
thermal loads, approaching, as a consequence, to the longitudinal
symmetry plane. By progressively reactivating the components, up to the
last components of the weld seam, the plate rotation may induce
components to find themselves significantly beyond the longitudinal
symmetry plane. Actually, such rotation is limited by the interaction of
the plate with its counterpart. All these considerations suggest
considering such phenomenon during the modelling, even if the modelling
involves both plates.
Moreover, the plate rotation may lead also to convergence issues,
especially as the plate length increases. The main reason of these
convergence issues can be addressed to the activation of the symmetric
constraints, which, under these conditions, would be applied to a more
deformed plate (with respect to the real test case), leading to an
increase of the residual stresses that can facilitate the lack of the
analysis convergence.
In order to take into account the interaction of both plates in the
proposed symmetric approach-based FE model, a row of finite elements
(green finite elements in Figure 7) has been placed along the left side
of the longitudinal symmetry plane (Figure 7A). This row of elements, of
the same length as the plate (248 mm), is made of 62 C3D8 finite
elements and 252 nodes; an arbitrary width (x direction) and a
height (z direction), slightly greater than the “root face”
(Figure 1), simulates the interaction with the two plates, also in case
of out-of-plane displacements. The mechanical material properties of
these finite elements are the same of the plate. Concerning the boundary
conditions applied on this row of elements, nodes placed on the
interacting surface (face looking at the longitudinal symmetry plane)
have been fully constrained.
In addition, the interaction between the plate and the work table, shown
in Figure 1D, has been numerically replicated by modelling the work
table as a rigid plane and by modelling the interaction between the
plate and the rigid plane by means of a surface to surface contact
algorithm. Moreover, in order to completely constrain the rigid motion
of the plate, the translation along the y and z axes of
the node (x = 0, y = 0, z = 0) of the seam and the
translation along the z axis of the node (x = 0, y= 248, z = 0) have been fixed.
The interaction between the modelled plate and the row of elements has
been defined through a surface to surface contact algorithm.
Specifically, at the first load step the interaction involves all
V-grove finite elements; subsequently, due to the progressive
reactivation of “components” of the first weld pass together with the
activation of the symmetric constraints along the x direction
(Figure 7), the interaction and the green finite elements belonging to
the row of elements are removed progressively as well (Figure 7B),
because not more useful. It must be highlighted that the simulation
strategy does not increase significantly the computational costs.
The translational constraints along the x direction are
progressively applied to the components nodes placed along the
longitudinal symmetric plane during the weld pass. This type of boundary
condition constrains also the rigid motion of the plate around yand z directions.