PSI - Issue 81

Mykola Stashkiv et al. / Procedia Structural Integrity 81 (2026) 143–150

147

Cross-sectional dimensions are as follows: profile width W = 280 mm, profile height h = 50 mm, flange width b = 25 mm, thickness δ = 3 mm, perforation opening width w = 120 mm, and L is crack length (ranging from 0 to 70 mm). The digital model was developed for the case of symmetrical cracks propagation in two diametrically opposite stress concentration zones using the ANSYS Workbench software. Since the lower chord of the sprayer boom (Fig. 7, a) has a longitudinal axis of symmetry only half of the element is considered to simplify the model, subjected to a normal tensile stress σ = 100 MPa with symmetry boundary conditions applied (Fig. 7, b). Under these modeling parameters, the normal stresses for a defect-free cross-section at the crack initiation location are σ ≈ 135 MPa. The Pre-Meshed Crack option of ANSYS Workbench was used to simulate the crack. The finite element mesh (5 mm) (Fig. 7, c) was generated using the Tetrahedrons method with the Patch Conforming algorithm. To ensure the required accuracy of the calculation, a section with a hexagonal mesh with element sizes of 0.5 mm was created along the crack face. Six concentric contours with a hexagonal mesh of finite elements of 0.1 mm size were defined around the crack front (Fig. 7, d). The crack was modeled in ANSYS Workbench using Analysis Type → Static Structural. The crack was implemented using the Fracture → Pre-Meshed Crack option. The global finite element mesh (Element Size → 5 mm) was generated using the Patch Conforming Method (Method → Tetrahedrons, Algorithm → Patch Conforming) (Fig. 7, c). To ensure sufficient calculation accuracy along the crack path, a region with a hexagonal mesh of 0.5 mm element size was defined. Around the crack tip, six concentric contours with a hexagonal finite element mesh of 0.1 mm element size were created (Fig. 7, d). Mesh refinement in these zones was performed using the Body Sizing → Element Size option. The analysis was performed with Solution Contours = 6 and Element Type → SOLID186. The Preconditioned Conjugate Gradient (PCG) iterative solver was used with the following parameters: Number of Steps = 1, Auto Time Stepping → Off, Define By → Substeps, Number of Substeps = 15, and Convergence Tolerance = 1.0×10 ⁻⁸ . The Stress Intensity Factor (SIF) extraction method was used by default to evaluate K I . In ANSYS, SIF extraction is primarily performed using the Interaction Integral Method (IIM), which calculates the SIF by analyzing the stress and displacement fields at the crack tip. IIM is preferred due to its higher accuracy.

Fig. 7. Crack simulation

The calculations were performed with a crack length increment of 5 mm. The results of the simulation for the mode I SIF K І for a symmetric crack of length L are given in Table 1.

Table 1. Results of the simulation for a symmetric crack.

С rack length L , mm 2 5 10152025303540455055606570 SIF value, MPa √ 9.9 16.6 23.0 28.4 31.3 33.9 36.5 39.1 41.7 44.3 46.9 49.5 52.1 55.3 61.2 The dependence of the mode I SIF K І on the crack length L is shown graphically in Fig. 8.