PSI - Issue 42

Nikola Milovanovic et al. / Procedia Structural Integrity 42 (2022) 362–367 Author name / Structural Integrity Procedia 00 (2019) 000 – 000

364

3

2. Model of Kaplan turbine shaft The aim of this research, partly presented in [24], was to conduct fatigue crack growth simulation on horizontal Kaplan turbine in hydropower plant Djerdap II. Crack lengths of 2100 mm were detected on the transition radius R80 after 163411 h of exploitation (Fig. 2). Appearance of the horizontal Kaplan shaft with in-service loadings and moments on it were also shown in Fig. 2. As it is mentioned, numerical analysis of shaft behavior included simulation of fatigue crack growth, using the principles of xFEM. Simulation was conducted in ABAQUS v6.11-3 software package, along with Morfeo/Crack software, with the aim of determining crack growth under dynamic loading, most dominant type of loading during its service life. Before simulation running, the input parameters were defined, i.e. the Paris coefficients C and m , as well as the stress ratio R . The aim of the whole study was to estimate the remaining service life of shaft before the final failure.

R80

Fig. 2 In-service loadings and momentums on the shaft

3. FE meshing and modelling Before running numerical simulation, it is necessary to generate a FE mesh. One of the major challenges related to the development of a numerical model and performing fatigue simulation represent FE meshing of the model, among all other things, due to the fact that crack models cannot use combinations of different types of elements (HEX or TET). Despite the axial symmetry of the turbine model, the meshing became possible only after the following changes: • All screw holes were removed from shafts surfaces, since they had no effect on the stress state (cause they were far enough away from the fatigue crack growth domain) • The total length of the shaft was reduced, since the length shaft itself has no effect on crack growth due to dimensional proportion. • Changes in the shaft cross-section of the longer axis were also removed, since they did not have impact on the results, but significantly complicated the FE mesh. • Boundary conditions of the shaft symmetric part have been introduced, as well as displacements limitation on axisymmetric model. An initial fatigue crack length was 37 mm, placed on the location causing the highest stress concentration, as can be seen in Fig. 3. Aforementioned approximations enable FE mesh generation, but another problem occurred that needed to be overcome - the calculation could not be performed on the whole model. In the first version of the model, a finer FE mesh around the crack was used, but this approach was rejected, since it was concluded that there is no need for such a fine mesh. The newly adopted model remesh and boundary conditions can be seen in Fig. 4. On this new model, loads settings were also changed, after several simulation attempts have been made. Simulations had shown that appropriate pair of forces instead of bending momentum distributed on shaft outer surface gave more reliable and realistic results of stress state and deformation. The intensity of such equivalent force was about 20 N/mm 2 , which had to be set in a pair as a new load that replaces the torque. As a consequence of all said, more realistic crack growth occurred. Crack propagation was in a direction very similar to real crack shaft in real working conditions, which was discovered after its failure. The load defined in this way is shown in Fig. 5 in the form of purple arrows at the end surface of the shaft model.