# Analysis of Fatigue Performance of Spot-Welded Steel T-Profiles Under Cyclic Torsional Loading
## 2 XFEM Modelling  
A three-dimensional XFEM model of the spot-welded assembly under torsional loading was created in this study. Abaqus 2021 FE software [12] was used for this purpose. The geometric details of the assembly's component parts are shown in Figure 1. There are four main sections. During fatigue loading, Parts 1 and 2, which are the main parts, are supported by Parts 4 and 3, respectively. Figure 2 presents the details of the developed XFEM model. The assembly was subjected to the torsional loading \(T\) from the free ends of Parts 2 and 3 with a length of 75 mm, while it was fixed in all directions from the free ends of Parts 1 and 4 with the identical lengths. \(T\) was applied to the reference point depicted in Figure 2, which is situated at the geometric centre of the structure's loaded portion. This point (RP-1) controlled the concerned region by means of the coupling constraint defined in the model. XFEM was primarily specified in these areas of the parts brought together using spot welds, in accordance with studies in the literature demonstrating that the cracks primarily originate and expand around the spot welds joining the structure. Using Abaqus' tie constraint module, the interfaces of the parts on the welding side were set as master and slave surfaces in order to simulate spot welding. To form the assembly, different parts are joined together using a total of 38 spot welds. Twenty of them connected Parts 1 and 4, ten of them for Parts 2 and 3, six spot welds joined Parts 1 and 2, and two spot welds joined Parts 1 and 3 in the end. Using 25 Fourier terms, a direct cycle analysis was carried out to simulate the fatigue loading with load ratio of \(-1\). To trigger crack formation in the regions of stress concentration, \(T\) was applied to the structure in a separate static step prior to the loading cycle. Details of the mesh used in the model are presented in Figure 2. To ensure accuracy of the model, a mesh convergence study was performed. Three simulations were run when the assembly was subjected to the static \(T\) load, using three different mesh sizes: 1.25 mm, 0.625 mm, and 0.3125 mm. The highest von Mises stress value found in the element adjacent to the welding zones was compared from each model. When the mesh size was adjusted from 0.625 mm to 0.3125 mm, the difference of concern was less than 4.13%, and when the mesh was changed from the coarsest to the medium one, it was more  
Figure 1: Geometric details of the constituent parts of the T-profile assembly. than 10.0%. As a result, the model was discretized using 0.625 mm element sizes. Because XFEM results are independent of the mesh size utilized, it is vital to emphasize that this mesh study was conducted for the static analysis simulating the formation of the cracks. For the discretization, eight-node linear brick elements with reduced integration (C3 DBR) were employed. The XFEM formulation procedure is summarized in Figure 3. In XFEM, a displacement vector function \(u\) with the partition of unity enrichment is approximated as follows:  
\[u(x)=\sum_{i\in N}N_{I}(x)\left[u_{I}+H(x)\alpha_{I}+\sum_{\alpha=1}^{4}F_{ \alpha}(x)b_{I}^{\alpha}\right] \tag{1}\]  
where \(N_{I}(x)\) represents the typical nodal shape functions; \(u_{I}\), the typical nodal displacement vector associated with the continuous portion of the finite element solution, is the first term in the equation above that appears on the right side. Multiplying the nodal enriched degree of freedom vector (\(a_{I}\)) by the corresponding discontinuous jump function \(H(x)\) over the fracture surfaces yields the second term in the equation. The nodal enriched degree of freedom vector, \(b_{I}^{\alpha}\), and the associated elastic asymptotic crack-tip functions, \(F_{\alpha}(x)\), are multiplied to obtain the third term. In this case, the first term on the right covers every node in the model; the second term only covers nodes whose shape function support is cut by the crack interior; the third term only covers nodes whose shape function support is cut by the crack tip.