PSI - Issue 79

A. Bacco et al. / Procedia Structural Integrity 79 (2026) 335–341

337

2. FE model The finite element model was developed to simulate the welding process of a 60° single-V groove butt joint consisting of an S355 steel plate and a GJS500-7 spheroidal cast iron plate. The dimensions of both plates were 200x150x8.5 mm. The simulated welding corresponds to a Flux-Cored Arc Welding (FCAW) process using a filler material assumed to have the same properties as cast iron and applied to the chamfer in two passes. The process parameters and the depth of the two passes were experimentally determined and reported in Tab.1.

Table 1. Welding parameters. Parameter

Value for 1 st pass

Value for 2 nd pass

Voltage V [V] Current I [A] Welding efficiency η [-] Welding speed v [mm/s]

22

24.5 175

160

0.8 4.7 3.8

0.8 3.5 4.7

Depth [mm]

Uncoupled thermo-mechanical analyses were conducted, performing a thermal analysis to obtain the temperature distributions during the welding process, followed by a mechanical analysis to determine the resulting residual stresses. This made it possible to greatly reduce the computational load. The developed numerical model is tridimensional and employs 8-node brick elements (DC3D8), with temperature as the only degree of freedom at each node during the thermal analysis. Temperature-dependent thermal properties were taken from the literature for both the steel plate (Bhatti et al., 2015) and the cast iron plate (Borgström et al., 2021). The addition of filler material to the joint was simulated using the “Birth and Death” technique, which requires the creation of all the elements that are part of the model, including the weld bead elements that would be added during welding. In the first step, all the weld elements were deactivated by applying a penalty factor of 10e -6 to their stiffness, to simulate the two plates with chamfers ready for welding. The weld elements were then reactivated at regular intervals based on the welding speeds during the two passes. Heat input was simulated as already done in several works in the literature (Giannella et al., 2023, Sepe et al., 2015, Sepe et al., 2021b), by activating the elements already at the liquidus temperature. In order to simulate the process in line with reality, convective and radiative heat exchange boundary conditions with the surrounding environment were also imposed on all surfaces of the joint, this procedure is required to properly simulate heat dispersion during the welding process, including the cooling phase between the two passes (120 s) and the final cooling of the welded joint. The temperature histories obtained for the various nodes were then applied, in the form of thermal loads, during the mechanical analysis. The model used in the mechanical analysis was identical to that used during the thermal analysis in terms of both geometry and mesh refinement. During the mechanical analysis, 8-node elements with three degrees of freedom (C3D8) for each node were used, while the mechanical properties at different temperatures were also taken from the literature for both steel (Bhatti et al., 2015, Rikken et al., 2018) and cast iron (Borgström et al., 2021, Šamec et al., 2011). 3. Results The temperature distribution in the joint during the addition of material, obtained from the thermal analysis, is illustrated in Figure 1. As expected, heat propagates differently within the plates, since made of dissimilar materials