# Assessment of Novel Modal Testing Methods for Structures Rotating in Water
## 3 Numerical Analysis  
A series of numerical structural and acoustic-structural models, to perform modal analysis and harmonic analysis, were built with the commercial software ANSYS(r) 2022R2.  
First, a numerical model only consisting of the structural parts of the test rig, the disk and the shaft, was built in order to calculate the natural frequencies of the non-rotating disk in air. The material of the shaft and the disk was considered standard stainless-steel, whose properties were already defined in the \"General Materials\" engineering data source of ANSYS(r). The discretization of the bodies was performed using a combination of tetrahedral and hexahedral elements. Subsequently, a mesh refinement process was performed to determine the optimal element mesh size that provided an accurate solution with a low computational cost. The optimal mesh used for the discretization of the structural part had a total of 43,826 elements and 88,796 nodes. The bearings were modeled using body-ground bushing connections and by adjusting the stiffness coefficients in the radial and axial directions.  
Second, the previous numerical model was enlarged with an acoustic region corresponding to the fluid domain, reproducing the surrounding water inside the tank in order to obtain the natural frequencies of the non-rotating disk in water. The density and the speed of sound of the water were considered to be 1000 kg/m\({}^{3}\) and 1430 m/s, respectively. The acoustic region was modeled through tetrahedral elements, which assumed that the fluid was inviscid, irrotational, compressible and without mean flow. The structural boundary conditions were the same as in the case of having the disk in air. The nodes of the solid elements in contact with the fluid were defined as a fluid-solid interface. In this case, the optimal mesh used for the discretization of both the structural and acoustic domains had a total of 495,222 elements and 829,056 nodes.  
For both air and water simulations, piezoelectric properties were added into the numerical models to simulate the excitation induced by a frequency-varying chirp applied to the PZT patch glued to the disk. The simulated piezoelectric patch (P-876.A12) was composed of a piezoceramic PIC255 layer, called the active layer, sandwiched between two thin encapsulating polymers, called the soft layer, which electrically insulated and applied prestress to the active layer (see Figure 7). The coupling of the acoustic, structural and piezoelectric physical models of the system was performed using the ANSYS(r) extension called \"Piezo and Mems\". The piezoelectric material's electrical behavior was defined by introducing the piezoelectric constants provided by the manufacturer in the stress-charge form [33]. Additionally, the polarized direction was set perpendicular to the disk surface. By doing so, a voltage between the two faces of the active layer of the patch could be defined, and the strain induced by the applied voltage to the patch could be simulated [34]. The boundary conditions were the same as in the case of having the disk in air or water. All in all, structural-piezoelectric and acoustic-structural-piezoelectric harmonic analyses were performed to simulate chirp excitations between 0 and 300 Hz.