Issue 78

S. M. Khalil et alii, Fracture and Structural Integrity, 78 (2026) 346-366; DOI: 10.3221/IGF-ESIS.78.20

capacity. Modifications such as outstanding flanges reduced stress concentration and lateral deformation, offering an economical way to strengthen existing steel closed girders without altering their dimensions. Overall, closed flange stiffening improved load distribution, reduced local buckling risk, and enhanced fatigue resistance, but the design must consider shear lag effects and optimal stiffener spacing for best performance (Sharma & Singh, 2023 [28], Singh, 2023 [29], and Ghaidak and Fadhil, 2012 [30]). Most studies focused on individual stiffeners added to the web of an I-section with a flange plate, while little research investigated strengthening the web by using a closed flange. In this paper, the study investigated the stiffeners of the web that act at the same time as part of the top flange, replacing the flange plate with a closed flange. A numerical study is performed covering the closed flange shapes of a triangle and a rectangle. More parameters are included for both stiffening shapes, such as patch loading lengths, stiffener and web thicknesses, and flange depth -to- web depth ratio. Hereafter, the paper first describes the finite element analysis that is used, along with verification to ensure the reliability of its results. Then, a parametric study is presented, including a discussion of the results. Finally, a conclusion is made with recommendations for future studies. he method used in the analysis is the finite element method. In structural engineering, the finite element model (FEM) has become an important and widely used tool for extending limited experimental data and conducting in depth parametric investigations. FEM can effectively replicate experimental results and predict both pre- and post buckling behaviour as a reliable analytical tool in steel structural research. The numerical simulations in this paper are created using the commercial finite element program ABAQUS [31], which has been used in previous studies and demonstrated success in simulating the point of research (Li and Young, 2017 [10], Chacón et al., 2019 [14], Loaiza et al., 2019 [16], Ć erani ć et al., 2022 [18]). The produced finite element model here is first validated against experimental results available in the literature in order to provide the most realistic stimulation possible. A mesh is a representation of the discretization of the overall structure into several smaller parts that are connected by nodes and have specific boundary conditions. These components can be described as one-, two-, or three-dimensional, or, in another meaning, beam, shell, and solid elements. The choice of element type depends on the required degree of accuracy and computing efficiency. The finite element models in this study are developed using the linear shell element S4R, with three translational and three rotational degrees of freedom at each node, similar to previous research by Chacón et al. (2019) [14], Ć erani ć et al. (2022) [18], and Kovacevic et al. (2019) [32]. This element employs a reduced integration scheme, which enhances computational efficiency. Mesh discretization is performed using an automatic mesh generation approach, with an average element size of approximately 5 mm, as shown in Fig. 2. The selected mesh size is adopted based on the h refinement convergence study reported by Ć erani ć et al. (2022) [18], in which element size was found adequate for longitudinally stiffened and unstiffened steel plate girders. Geometric nonlinearity is considered by activating the *NLGEOM parameter in the software library. The girders are simulated as simply supported with a constant span (a) equal to 500 mm for all species. A variable-length (W) is applied to each configuration, ranging from 0 (as a concentrated load) to 150 mm. A patch loading width is specified on the upper flange by using datum planes and applying the load on a reference point, which is linked to the specified surface of the upper flange by a rigid body type constraint. This is to ensure that vertical displacement is allowed and all other displacements and rotations are prevented. In order to prevent any local failure caused by stress concentration from the reactions, vertical transverse stiffeners are to be installed above the supports. End-support stiffeners are purposefully discretized using shell parts that match their physical dimensions to avoid premature bearing failure. To ensure actual load transmission and support, the stiffeners are completely confined to the web and flanges, and their thickness is selected to match the flange thickness (t f ). At one end of the beam, vertical and out-of-plane horizontal translation, as well as rotation about the longitudinal axis, are restrained, representing roller support. At the other end, all translations are restrained, representing hinged support. Horizontal out-of-plane support is applied along the upper flange to prevent lateral displacement of the flange and focus only on web buckling. All restraints and loading points are shown in Fig. 2. The modified Riks, as an incremental iterative solution technique, is used within the finite element analysis framework. An arc-length control method manages how the solution moves along the path of equilibrium. The iterative process utilizes the tangent stiffness matrix and applies the Newton–Raphson method with automatic load incrementation. Infinite strain, along with a high number of steps, is used to avoid termination of the analysis prematurely. The steel material uses the von Mises yield criterion. An elastic – perfectly plastic material curve is used, as shown in Fig. 3, with the elastic modulus of steel (E) as 205,000 MPa up to the yield point. The curve is modelled using the true stress-strain values from σ tr = σ E (1+ ε E ) and ε tr = T M ETHODS AND TOOLS

349