## 2 Case Study of Cracked Rotor Using a Three-Dimensional Finite Element Model  
As a case study, a cracked rotor was investigated using a three-dimensional (3-D) finite element analysis in Abaqus/CAE. This study was conducted to show that non-symmetric bending principles should be used when analytically modelling the breathing response of a crack. The 3-D finite element model of the cracked rotor was devised in which the shaft is idealised as a beam with pin-roller supports and features a transverse crack at its mid-span as shown in Figure 1. The geometric and physical properties of the shaft are as follows: length \(L=0.725\) m, radius \(R=6.35\) mm. The shaft material was assumed to have a density \(\rho=7800\) kg/m\({}^{3}\), Poisson's ratio \(v=0.3\) and Modulus of Elasticity \(E=200\) GPa. Due to the shaft's weight a uniformly distributed load of 9.69 N/m acts on the shaft along its entire length, where m is the mass of the shaft and g is the gravitational acceleration constant. The model does not consider dynamic loads so to simulate weight-dominant crack breathing [25]. As such, only the weight force is considered and is applied as a body force by specifying the material density and a gravity vector. A transverse crack with a depth equal to 70% of the shaft radius was simulated by partially joining two solid shafts at one end by a tie constraint. This partially joined region, highlighted in Figure 2a, is representative of the undamaged (intact) section of the shaft. The purpose of the tie constraint is to lock the nodal displacements of the adjoining surfaces so no relative motion occurs between the two surfaces. The remaining unbonded regions represent the crack surfaces. A non-linear contact surface, highlighted in Figure 2b, is placed on one crack surface so that normal stress may be transmitted between the crack surfaces. Due to the excessive local deformation and stress concentrations caused by directly applying pin-roller support boundary conditions at particular nodes, a rigid analytic surface was created as a separate part and bonded to the ends of the shaft using tie constraints, as shown in Figure 3. Furthermore, the degrees of freedom of the rigid analytical surface were constrained to a line and a point on the surface as shown, where the line constraint locked the mid-plane of the shaft end into the X-Z plane and prevented rotation about the Z axis and translation about the Y axis. The end of the shaft was still free to rotate about X and Y directions and free to translate in the X and Z directions. The point constraint locks the remaining translations leaving the shaft still free to rotate about the X and Y axes. Translation in the Z direction was only constrained at one end of the shaft to simulate an idealised pin and roller setup. Figure 1: Two-dimensional representation of the three-dimensional cracked rotor model showing static loading. Figure 2: Transverse slice taken at crack location highlighting the (**a**) undamaged area and (**b**) fractured area via the shaded regions, for which the crack depth was set to 70% of the shaft radius. To reduce simulation time, the cracked region was modelled separately to the bulk of the shaft and then bonded to the bulk using tie constraints. Furthermore, the model's element mesh was refined both radially and axially in the vicinity of the crack, where the degree of refinement was determined using a convergence test. The goal of the convergence test was to minimise simulation time without sacrificing too much simulation accuracy. The accuracy of the simulation was determined by analytically calculating the crack closing area and shaft deflection and comparing these to the FEA probed results. A summary of the convergence test is seen in Table 1. Mesh 9 (177,000 elements) was selected as it offered a high degree of refinement local to the crack whilst reducing the number of elements for the shaft bulk.