PSI - Issue 28

Giovanni Meneghetti et al. / Procedia Structural Integrity 28 (2020) 1062–1083 G. Meneghetti/ Structural Integrity Procedia 00 (2019) 000–000

1079

18

 Interactive analysis. This method is designed to allow the analyst to select one or more specific lines on which the analysis will be carried out. Once the analyst selected the desired model’s lines, ANSYS – PSM is programmed to regain control of the analysis process, to evaluate selected lines as V-notch sites and perform PSM-related calculations on each detected V-notch tip-profile. ANSYS – PSM gains full-control of the Analysis workflow regardless of the analysis method, once a defined set of model’s lines is passed to the program (either all model’s lines in the case of a ‘full automatic analysis’ or a set of user-selected lines in the case of an ‘interactive analysis’). A looping section is started by ANSYS – PSM on selecting the first model’s line of the set. The analysis phase is carried out through the following steps: a) all nodes belonging to the considered line are selected and V-notch opening angle is locally evaluated on each nodal position. The V-notch identification sub-routine perform the following tasks:  evaluates the local orientation of the considered line;  defines construction circular areas at each nodal location along the considered line, each area being locally orthogonal to the line’s tangent direction;  intersects the model’s volume with the construction circular areas;  evaluates the material-side angles subtended by the resulting local circular sectors;  calculates the actual air-side V-notch opening angles from the conjugate material-side angles: only if the air-side opening angle is in the range between 0° and 150°, the line is considered as a V-notch tip profile. b) once the line is recognized as a V-notch tip profile, a local coordinate system is automatically defined and orientated on each nodal location. The automated algorithms allow to locally align z -direction (Z in Ansys) tangent to the notch tip profile, θ -direction (Y in Ansys) originating from the notch bisector line and r (X in Ansys) being the radial direction, according to the PSM requirements. c) peak stress components σ θθ,θ=0,peak , τ rθ,θ=0,peak and τ θz,θ=0,peak are evaluated node by node referring to the local coordinate system and stored in dedicated ANSYS® Arrays. d) in the case of FE meshes defined by adopting 10-nodes tetra or 4-nodes tetra elements, the calculated peak stress components are automatically elaborated into averaged peak stresses, according to Eq. (5). e) PSM-related parameters, i.e. stress singularity exponents and SED coefficients, are computed taking advantage of fitting equations (10) and (12), as a function of the model’s local geometry and material. After that parameters f wi are calculated at each nodal location by means of Eq. (7). f) peak stress values are combined into a local equivalent peak stress at each nodal location of the selected line, by mean of Eq. (6). g) local biaxiality ratio λ is evaluated on each node along considered model’s line by Eq. (8). A PSM fatigue design curve is univocally selected and addressed by ANSYS – PSM according to the local biaxiality ratio value and the minimum welded plates’ thickness (see Table 3). h) a fatigue life N f value is estimated on each analysed node belonging to the selected line. Fatigue life values estimated on analysed nodes are stored either within ANSYS – PSM Analysis Log, either within dedicated external .lis files, in order to be steadily available to further post-processing elaborations and results visualization. Once the selected line has been completely analysed, ANSYS – PSM loops to the following model’s line on the passed set, performing steps (a – h) from the beginning on the new line. Whether a line is not recognized as a V-notch site, steps (b – h) are skipped and the analysis moves to the straight-following line. The entire full-automated part of the Analysis Phase is tracked by means of an Analysis Progress Bar, designed in order to visualize progress increments in terms of number of currently analysed lines over all selected model’s lines. The Progress Bar is constantly visualized and updated by ANSYS – PSM and can be referenced by the analyst in order to estimate the process completion status and time-to-completion throughout the entire Analysis. Once all model’s lines have been analysed, ANSYS – PSM finalizes the Analysis Phase and enters post-processing phase in order to provide results elaboration and visualization. Fatigue analysis results are visualized in terms of graphical line contour plots displaying estimated fatigue life distributions along analysed V-notch tip profile. The Life Contour Plot is automatically elaborated and visualized on the screen at the end of the Analysis Phase and is designed to be consulted through a color scale, normalized with respect to the maximum detected fatigue life value throughout the entire model’s structure. The color bands are designed to range from red color, corresponding to the minimum fatigue life value, to blue color, corresponding to the maximum fatigue life value.