## 2 Numerical Modeling
### Computational Geometry and Flow Solver
This twofold capability is especially desired for the present application. Indeed, a good capturing of the plasma-induced effects close to the walls, as well as of the interaction between the neighbouring blades, is needed here. The SST k-\(\omega\) Menter model combines the advantages of the k-\(\epsilon\) and k-\(\omega\). By means of a blending function--unitary close to the wall and zero elsewhere--it is possible to switch between the k-\(\omega\) and the k-\(\epsilon\) models. Namely, the k-\(\omega\) model, performing well close to the walls (chapter 11, [31]) is used near the blades. Conversely, the k-\(\epsilon\), which is more accurate for describing the external flow (chapter 11, [31]), is employed for the rest of the fluid domain. Notice that the k-\(\omega\) SST Menter model is used in other numerical works dealing with turbomachinery cascades. [PERSON] et al. [14] used the same solver and the same modeling to perform RANS computations on a compressor cascade equipped with plasma actuators, employed to control corner stall separations. [PERSON] et al. [2] used Ansys CFX\({}^{\textregistered}\) to carry out fully turbulent RANS computations closed with the k-\(\omega\) SST Menter model on a linear cascade featuring blades oscillating in pitch. For the present assessments, incompressible simulations are performed. This is consistent with the capabilities of the aeroelastic experimental rig of TU Berlin [22] and appropriate for the first assessments of the novel actuation system proposed here. Simulations in transonic conditions, closer to the actual flow in aero engine compressors, are scheduled as an outlook of this work. The temperature is set to 20 \({}^{\circ}\)C and the reference pressure to 101,325 Pa. For traveling wave mode simulation, a periodic displacement is imposed to the blades. With this aim, a mesh deformation algorithm is employed. Figure 2: Detail of the computational grid around one blade (**top**), and blowing up on the trailing edge area (**bottom**). Specifically, the harmonic motion of the blade nodes is specified via an external text file. This latter contains: (i) the node coordinates for the blades at their initial positions; (ii) the node coordinates related to the blade maximum displacements--positive and negative. The frequency and the phase of the motion are set directly in the flow solver. The motion of all remaining nodes is determined by the Displacement Diffusion mesh deformation model, the only one currently available in Ansys CFX(r). With this model, the displacements applied on domain boundaries or in subdomains are diffused to other mesh points by solving the diffusion equation \(\
abla\times(\Gamma_{\mathrm{disp}}\
abla\delta=0)\), \(\delta\) being the displacement relative to previous mesh locations and \(\Gamma_{\mathrm{disp}}\) the mesh stiffness. This quantity determines the entity of the motion in different regions of the domain. In this work, the stiffness is defined as the reciprocal of the cell volumes, so that the mesh deforms less where cells are smaller, e.g., close to the boundary layer. The diffusion equation is solved at the start of every time step of the simulation. Notice that the displacement diffusion model preserves the element distribution of the initial mesh. That is, if the initial mesh is relatively fine in certain regions of the domain, e.g., the boundary layer, then it will remain relatively fine also after solving the displacement diffusion equation. Further details on the algorithm can be found in [32; 33].