Issue 9

T. Marin et alii, Frattura ed Integrità Strutturale, 9 (2009) 76 - 84; DOI: 10.3221/IGF-ESIS.09.08 78 therefore overcome. Elemental stresses or stresses extrapolated to the nodes are in fact influenced by the element formulation and by the geometric characteristics of the finite elements, whereas nodal forces directly derive from the equilibrium of the structure. Nodal forces (and moments) for each element are calculated from the stiffness matrix and the nodal displacements (and rotations). The displacements are the primary output of displacement-based FE codes and the equilibrium at each node in the mesh is satisfied regardless of the element size and element formulation. A few different variants of this approach have been proposed and they mainly stem from the automotive field for either spot or seam welds, see for example Fermer and co-workers [6] . The literature reports also a recent implementation of a similar approach in the commercial code Femfat, [7]. Researchers, headed by P. Dong at Battelle Institute, have formulated an effective procedure for the calculation of the structural stress from forces and moments at the nodes of a finite element mesh, based on work-equivalence considerations, [8]. In Dong’s method, first distributed line forces (and moments) are determined along the edges of the weld toe lines starting from balanced nodal forces (and moments), then at each node the structural stress is calculated as: 2 6 t m t f x y b m s         (1) where t is the section thickness of the plate, f y is the line force in the local y direction orthogonal to the weld line and in the plane of the shell; m x is the line moment in the local x direction tangent to the weld line. Forces and moments have to be preliminarily rotated into local coordinate systems defined at the nodes of the weld line. The resulting line forces (and moments) are continuous along the weld toe lines and so is the structural stress. The detailed procedure is described in several publications, for example [8-9] . Even if these concepts can be applied to solid elements (2D and 3D), the approach is particularly suited for shell elements. Thus, since shell and plates are often the preferred choice for modeling the response of engineering structures that are obtained using welding (for example truck frames, ships, cranes, bridges, etc.), the potential applications of the method are many. It must be emphasized that the finite element simulations have to be linear elastic therefore a fatigue assessment of the welded joints in the components can be a precious additional outcome of a standard stress analysis. The only specific requirement concerns the modeling of the welds because the fillets must be explicitly included to correctly represent the stiffness of the joints. This can be done using inclined elements, as shown in Fig. 2a which reports an example of a T-joint connection between two tubular parts. Several strategies for a realistic modeling of partial and complete penetration seam welds are collected in Fig. 2b. The authors acknowledge that the manual creation of the elements in the welds is a tedious and time consuming part of the procedure and the automation of the welds definition has to be pursued. Note in Fig. 2a how for a given fillet both the two toe lines have to be analyzed since a priori it is not know which one is the most prone to fatigue propagation and where. Figure 2 : a) Tubular connection (T-joint) modeled with shell elements; b) fillet welds with partial and complete penetration. The mesh-insensitivity of the structural stress claimed above, is demonstrated through the illustrative numerical example of Figure 3. Here a curved thin profile is joined on the outer side to a flat plate by a full penetration fillet weld. The main dimensions of the flat panel are 100x100 mm, the two sides of the curved plate are 50 mm long and the thickness is 5 mm. A uniform traction is applied longitudinally to the curved profile and transverse loading acts on the top edge as shown in Fig. 3a; top and bottom nodes of the flat plate are pinned. Three different meshes are studied, the first one is shown in Fig. 3a together with the resulting V.Mises stress on the visible surfaces of the shells. This is a rather coarse