PSI - Issue 75

Kris Hectors et al. / Procedia Structural Integrity 75 (2025) 102–110 Hectors et al. / Structural Integrity Procedia (2025)

105

4

3.2. Preprocessing of the notch profile data To integrate the profile data into a finite element model, preprocessing was required. This involved translating every profile scan to the origin of a common coordinate system, in order to align the notch root of each specimen. Subsequently, only a segment of the high resolution profile data is retained by trimming sampling points with height values higher than 0.1 mm. Trimming the profile scan significantly reduces the number of sampling points and consequently, the computational complexity. This is done without losing information in the notch root, which is the main region of interest. Finally, the geometry of the specimen is completed by padding four additional points to the profile. These points are sufficient to encode the depth of the profile. To mitigate the influence of the boundary conditions when applying loads to the end points of the model, the specimen length is extended by four times the diameter of the specimen on each side of the notch. The preprocessing procedure is illustrated in Fig. 5.

Fig. 5: The preprocessing procedure for the notch profile data involves translating the notch profile to the origin and trimming and padding the profile to retain only the scan data within the zone of interest.

3.3. Finite element model Before importing the preprocessed profile data into the Abaqus/CAE 2023, the -values are vertically shifted. This shift is by a distance equivalent to the notch section radius, which is calculated as the difference between the specimen radius and the notch depth. Subsequently, a planar shell feature is generated by connecting the sampling points using splines and closing the sketch to create the full geometry of the specimen. Very small mesh elements are required to accurately capture the details of the notch profile. A carefully designed meshing strategy was essential to limit computational cost by maintaining a reasonable number of elements, while preserving the required level of detail in the notch region. A bottom-up meshing approach was employed to fulfil these requirements. A crescent partition was made near the notch root to create a fine mesh within the region of the notch with the highest expected stress gradient. The size of the partition was chosen as small as possible, but had to be large enough to contain the full notch root affected region and must contain all the sampling points originating from the profile scan. The mesh within this region was generated utilizing the medial-axis algorithm to ensure an evenly distributed mesh. The remainder of the part was meshed using a structured mesh technique and relatively coarse seeding. This planar mesh is then revolved by 360° with respect to the central axis, by a predefined number of times to obtain the final solid mesh. Quadratic elements were used throughout the solid mesh. Due to the way the mesh is constructed, the elements that coincide with the centre axis are wedge elements, all other elements are brick elements. The final mesh comprises a mix of C3D15 (15-node quadratic triangular prism element) and C3D20R (20-node quadratic isoparametric element with reduced integration). Boundary and load conditions were applied using a reference point at either side of the model. One side of the model was fixed by kinematically coupling a reference point to the end surface and constraining all displacements and rotations of the reference point. The other reference point was coupled to the opposite end surface using a continuum distributed coupling. Since the specimens are intended for rotating bending fatigue, a bending moment was applied to the reference point of this end face. The bottom-up mesh, boundary conditions and the applied bending moment are depicted in Fig. 6. To streamline the process of creating a finite element model for every scanned specimen, a Python script was developed to automatically generate the models.