# Validation of a Modal Work Approach for Forced Response Analysis of Bladed Disks
## 3 Results and Comparisons
### LPT Bladed Rotor Test Case
#### 3.2.1 FEM Bladed Rotor Model  
The original CAD model of the rotor is based on a geometry already studied during the FUTURE European research project from an aeromechanical point of view [6; 7]. The turbine bladed disk consists of 147 profiles. The mechanical properties of the components are summarized in Table 3. The blade material is not a typical alloy for low-pressure turbine blade manufacturing, yet the aluminum alloy was chosen during the EU project to lower the blade row frequency in order to trigger free flutter occurrence during an experimental campaign within a cold flow rig [26].  
The discretization of the rotor bladed sector was carried out using the mesh generator available in the ANSYS Mechanical software. The number of elements and their minimum size were carefully selected after a sensitivity analysis, with the aim of minimizing computational costs while preserving a good mesh accuracy. A mesh refinement was performed at the blade surface, and the MATCH CONTROL option was used to obtain the mesh matching on the two cuts of the one-pitch sector, where the cyclic symmetry condition was applied. To accurately model the fir-tree attachment between the blade and the disk, a contact region was defined and the mesh is identical at the interface. The contact was modeled as bonded. The final mesh, shown in Figure 6, consists of around 70,000 10-node tetrahedral structural solid elements (SOLID187). A named selection, including the blade surface, was defined for the mean pressure mapping and the successive extraction of blade mode shapes.  
\begin{table}
\begin{tabular}{c c c c c c} \hline \hline  & **Maximum Amplitude of Total Displacement (m) for EO = 4** & & & \\ \hline  & **ND = 0** & **ND = +2** & **ND = +4** & **ND = +6** & **ND = +8** \\ \hline Tremor & 2.51 \(\times\) 10\({}^{-8}\) & 3.31 \(\times\) 10\({}^{-8}\) & 8.95 \(\times\) 10\({}^{-8}\) & 2.77 \(\times\) 10\({}^{-8}\) & 1.93 \(\times\) 10\({}^{-8}\) \\ ANSYS & 2.51 \(\times\) 10\({}^{-8}\) & 3.31 \(\times\) 10\({}^{-8}\) & 8.95 \(\times\) 10\({}^{-8}\) & 2.78 \(\times\) 10\({}^{-8}\) & 1.94 \(\times\) 10\({}^{-8}\) \\ \hline \hline \end{tabular}
\end{table}
Table 2: Tremor–ANSYS comparison (1 st family, out of resonance for EO \(=4\), case 3).  
\begin{table}
\begin{tabular}{c c c c} \hline \hline
**Item** & **Unit** & **Disk** & **Blade** \\ \hline Material & & Structural Steel & Aluminum \\ Young’s modulus & (GPa) & 200 & 72 \\ Density & (kg/m\({}^{3}\)) & 2810 & 7850 \\ Poisson ratio & (-) & 0.3 & 0.33 \\ \hline \hline \end{tabular}
\end{table}
Table 3: Material properties.  
In order to reproduce the constraints of the assembly, the following conditions were chosen and imposed in the FEM model: interlocking constraint at the base of the sector; axial and tangential constraint to reproduce the screw connection between disk and shaft. To perform the FEM analysis, specific commands were included in the modal module in order to define the cyclic symmetry of the model (CYCLIC) and to specify pre-processing (PREP7), solution (SOLU), mapping (MAP) and post-processing (POST1) options.