PSI - Issue 5

Rui F. Martins et al. / Procedia Structural Integrity 5 (2017) 633–639 Diogo F. Almeida et al. / StructuralIntegrity Procedia 00 (2017) 000 – 000

636

4

Table 1. Results of residual stresses ’ measurement obtained by the hole-drilling method. Welded Joint σ max (MPa) σ min (MPa) θ (º) AISI 316L/316L 418 -205 -42

3. Numerical simulations

The numerical simulation of a welding process has a transient nature, it is a nonlinear type of analysis, and one of its key problems is the definition of the material model as close as possible to what happens during welding. The physical properties ’ evolution with temperature used in this study for AISI 316L SS (Fig. 3) were obtained from the works of Depradeux (2004), Bezerra (2006) and Pozo-Morejón et al. (2011), having been adopted the following range for the melting temperature: 1723 to 1773 ºK. The validation of the numerical method used in this work was carried out by replicating the work described in (Depradeux, 2004), and the results were quite satisfactory, with errors in the order of 5-9%. Detailed information can be found in (Almeida, 2012).

Fig. 3. Physical properties of AISI 316L SS vs. Temperature considered during the thermal analyses carried out. Units on the abscissa ’s axis are in ºK.

3.1. Thermal analyses

In this section all procedures carried out to perform the thermal analysis are presented, including the description of the analytical models relating to the heat source, the boundary conditions imposed on the thermal problem and other considerations used during the analysis, in order to simulate the welding process described in the previous sections. A three-dimensional numerical thermal simulation was carried out, considering two welding passes, one at each side of the plate under study (310x185x3 mm). A SOLID70 finite element from ANSYS® commercial software was used due to its three-dimensional thermal conduction capacity. This element has 8 nodes with a single degree of freedom (temperature). In weld bead ’ s region a refined finite element mesh was defined with finite elements having dimensions of 1.25x1.25x1 mm. At distant zones of the weld bead, it was not necessary to set such a refined mesh, and the finite element dimensions were smoothly increased until they reached the dimensions of 10x20x1mm. Additionally, based on the speed of the heat source, the duration of welding passes and the respective cooling time were defined in the Finite Element Analyses (FEA) (Fig. 4). As a heat source model (power density), a double Gaussian distribution - double ellipsoid (Fig.5) - proposed by Goldak and Akhlaghi (2005) was used with the front and rear areas of the arc with dimensions shown in Fig.5, which were based on the observation of the weld bead and some approaches suggested by Wentz (2008). In the numerical simulation, it was considered that the heat source moved at a constant speed. In order to simulate this movement, a routine in MATLAB®, responsible for distributing thermal loads to the elements covered by the heat source, was created. Those values were loaded as heat generation rates through the HGEN ANSYS® function. This was created with a total of 1983 tables, which characterize the power density applied to the elements as a function of time, as the heat source traverses them. The value of the power density was calculated for 32 elements and the time it takes the torch through each element was taken into account according to the progress of the welding process