Issue 47

D. Benasciutti et alii, Frattura ed Integrità Strutturale, 47 (2019) 348-366; DOI: 10.3221/IGF-ESIS.47.26 359 such a “Von Mises approximation” is even hypothesized (implicitly) in some multiaxial criteria (e.g. [18]), which may thus lead to unrealistic estimations (see [4,8]). FE durability analysis an L-shaped structure under random acceleration The purpose of this second example is to illustrate how the PbP method can easily be embedded into a FE durability analysis of a structure undergoing random vibrations. The example considers an L-shaped structure made of steel, whose geometry imitates that one already studied in [18]; some dimensions have been slightly changed [19] to enhance stress concentration effect at the hole and two lateral notches. A finite element model with “shell” elements is used to discretize the structure. A mapped mesh is generated in the notch regions. The average elements size is 3.5 mm; the smallest element dimension of 0.8 mm appears in regions of mesh refinement at notch tip. The model has a total of 1529 elements and 1687 nodes. The structure is clamped at both ends, at which a random acceleration is imposed along the direction normal to the specimen plane. Input accelerations have a band-limited (rectangular) one-sided PSD, ranging from 1 to 200 Hz, with height 25π (m/s 2 ) 2 ·Hz -1 (as in [18]). Input accelerations applied at the two clamped ends are fully correlated (their cross- PSD is different from zero). Figure 6 : Geometry and finite element model of the L-shaped beam. Thickness is 0.5 mm. A frequency-domain spectrum analysis is carried out through FE simulations to determine the structure natural frequencies and the stress PSD matrix in every FE node. Stress spectra are next processed by the PbP method to determine the total fatigue damage caused, in each node, by the local multiaxial state of stress. The whole numerical analysis is performed by software Ansys with APDL language, which is also used to implement the PbP method. Appendix B provides more details on the numerical algorithm. This analysis strategy, in which all calculations are carried out in Ansys software, simplifies the overall data management and thus represents an enhancement of the two-phase procedure followed in [4], in which nodal FE results (PSD matrices) were first calculated in Ansys, then exported and post-processed in Matlab to apply the PbP criterion. The first five natural frequencies returned by modal analysis are: f 1 =16.1 Hz, f 2 =67.3 Hz, f 3 =82.2 Hz, f 4 =175.7 Hz, f 5 =178.6 Hz. In each node the state of stress turns to be biaxial. Fig. 7 displays an example of auto- and cross-PSDs in a node close to the round notch. Results refer to the “top” layer of shell elements. For fatigue damage estimation, two different types of material (Material 1 and 2) were considered for the structure. Material 1 (likewise material A in Tab. 2) is only sensitive to deviatoric stress components, whereas Material 2 (likewise material C in Tab. 2) is also sensitive to hydrostatic stress component. The material properties used in simulations are: σ A =300 MPa, τ A =300/  3=173 MPa, k  = k τ =8 (Material 1); σ A =300 MPa, τ A =290 MPa, k  =8, k τ =5 (Material 2). Fig. 8 displays the damage maps for either material. The damage is estimated by PbP-TB method in Eq. (16) and refers to the “top” layer of shell elements. Left Figs. (a) show the damage D in linear scale to better highlight the locations of the most damage points; right Figs. (b) show the logarithmic values log 10 ( D ) to allow the differences in the overall damage distribution to be appreciated best. The comparison of figures makes evident how the damage distribution does change