PSI - Issue 57

9

Yuri Kadin et al. / Procedia Structural Integrity 57 (2024) 236–249 Kadin et. al / Structural Integrity Procedia 00 (2023) 000 – 000

244

The displacement boundary conditions are applied on the roller domain (see Fig. 10) in the following way: i) The nodes of x = ± l /2 are constrained in all direction (clamped). ii) The nodes of z = D w /2 are clamped. iii) The nodes of y =0 are constrained in y -direction (corresponding to the symmetry boundary conditions). The nodes on the roller raceway ( z =0), chamfer and end face ( y = L /2) are not constrained, but are used to apply the moving contact pressure in terms of stress boundary conditions. The semi-analytically evaluated contact pressure is applied on the FE domain and “animated” (the contact pressure moves from left to right along the x -coordinate, see Fig. 8) using the standard ABAQUS subroutine UTRACLOAD (see Kadin et. al (2022)). Due to this “ animation ” a single over-roll is simulated, which is needed to evaluate the SIF ranges (  K II ,  K III and  K I ) and to assess the risk of fatigue crack growth. The FE model in Fig. 10 indicates the varying mesh density across the solution domain. It increases at the crack front in order to get sufficiently accurate displacement solution for the prediction of SIF, while the rest of the domain is coarser meshed. In total the model comprises of around 90,000 linear elements: approximately 20,000 elements belong to the crack domain and the rest to the roller domain. Whether the mesh density along the crack front is sufficient was verified by mimicking a penny crack in infinite space subjected to tension. For this exercise, an analytical solution is available, and it is given by the equation (see e.g. Tada et. al (2000)): K I =(2/  ) ⋅  ൉ሺ  a ሻ ͳȀʹ (where  is the tensile stress, and a is the crack radius). The FE model of a penny crack is created from the two solution domains connected at the chamfers by the constraint interaction “Tie”, as is shown in Fig. 11. Both domains have identical meshes, which is achieved by copying the original domain and rotating the new (additional) one by 180 ° . With this strategy, the mesh configuration in the test model gets similar to the model to be used for the current RCF analysis. The boundary conditions in the test model are applied on the nodes of x = ± l /2, in terms of tensile stress in the x -direction (  xx ). It is important to note, that the difference between the real and the test model is primarily due to the crack size: to mimic the infinity conditions properly (for which the analytical solution is valid), the vertical crack of sufficiently small size (relatively to the chamfer) is defined in the test model. Starting from a rough mesh, its density along the crack front was progressively increased, while the rest of the model (in roller domain) remained unchanged. After each modification, K I was computed and compared to the analytical solution. The mesh convergence analysis was stopped when the numerical solution was sufficiently close to the analytical one (similar analysis was performed by Zolotarevskiy et. al (2020)). As is indicated in Fig. 11, the numerically predicted K I is around 3.5 % below the actual value, which is caused by the increased stiffness. This is because the stiffness of a FE discretized elastic body is higher compared to the actual one, having infinite amount of degrees of freedom. Finally note, that by running the mesh convergence analysis the proper FE model is created. It provides satisfactory numerical accuracy, and comprises of reasonable amount of elements such that computational time is in practical framework. 5. Results and discussions The contact conditions in the current simulations are defined as such, that the “worst case scenario” is satisfied. The contact pressure, corresponding to the extreme loading conditions is presented in Fig. 12. Due to high contact load and misalignment, the pressure penetrates out of the raceway and gets locally extremely high (up to 6 GPa). The contact pressure peak in Fig. 12, is the result of the contact zone truncation, for which the transition from the raceway to chamfer acts as a stress raiser. Note, that the contact pressure in Fig. 12 is over-estimated at the truncation peak due to assuming purely elastic behavior of the counter-face (bearing ring). In reality, however, this high pressure is supposed to mitigate due to local plastic flow at the steel ring surface. The main goal of the current parametric study is to explore the effect of crack configuration (size, location and orientation) on the SIF range values. Later these numerical results can be used to define specifications for optical inspection. Some parameters defining the problem, are fixed while few others are parametrized – see Table. 1. The FE results corresponding to the SIF range distributions along the crack front are presented in Figs. 13 for the vertical (  =90 ° ), in Figs. 14 for the horizontal (  =0 ° ), and in Figs. 15 for the inclined (  =45 ° ) crack orientation. Multiple curves in the figures correspond to the various crack locations, defined in terms of the distance, S 1. The SIF ranges