## 3 Numerical Modelling  
All simulations discussed hereafter are performed with the AVBP solver, which solves the three-dimensional compressible Navier-Stokes equations. Note that the buoyancy effect has been neglected as forced convection is predominant in this configuration. Wall-resolved LESs are targeted for all cases and a second order in time and space numerical scheme, the  
Figure 3: Comparison of the two configurations. Lax-Wendroff (LW) scheme [21], is chosen. Concerning the sub-grid-scale model, the \(\sigma\) model [22] is used. The correct behaviour of close-to-wall turbulent viscosity is correctly reproduced by this model, a requirement for wall-resolved simulations. The numerical domain corresponds to a section of the wind tunnel test section beginning at the perforated plate, as can be seen in Figure 1. At this location, the experimental data for the flow velocity are available. The coordinate origin is as indicated in Figure 1. The Navier-Stokes Characteristic Boundary Conditions (NSCBCs) formalism [23] is used for the inlet and outlet. For all of the simulations, a velocity profile provided by the experiment is imposed at the inlet (Figure 2) and the similitude relations are used to adapt the profile to the engine scale. Note that the engine scale inlet requires an additional treatment since an acoustic signal is superposed to the velocity profile. To investigate the effet of inlet turbulence, two different simulations are run on the similitude case: one with no turbulence injection at the inlet and one with an injection of fluctuating velocities. When turbulence is injected, the fluctuating velocity \(u_{rms}\) profile, adapted from the experimental data (Figure 2), is imposed at the inlet using the Kraichnan/Celik method [24]. Regarding the outlet, a constant pressure \(P_{0}\) = 101,325 Pa is imposed and the three-dimensional extension of the classical LODI (Local One-Dimensional Inviscid) formulation with space-averaged values as detailed in [PERSON] et al. [25] is used. The ceiling and side walls of the test section are far enough away from the perforated plate not to interact with heat transfer; thus, they are treated as slip walls. On the contrary, all other walls, i.e., the plate, the ducts, the lab scale pistons and the engine-scale cavity walls, are no-slip walls. For the lab-scale configuration, the ALE (Arbitrary Lagrangian-Eulerian) formalism [26] is used to simulate the piston motion. Finally, a constant heat flux is imposed on the perforated plate. The same method as [PERSON] et al., based on [PERSON]'s cooling law, is used to determine the heat transfer coefficient \(h\). Thus, for each of the configurations, two simulations are run with two different flux values. The different meshes used for both scales are composed of tetrahedra. An automatic mesh adaptation strategy, based on a double criterion inspired from [PERSON] et al. [27], is used. The idea is to run a simulation on a coarse, user-defined mesh to get preliminary results. Then, the mesh is refined in the zones of interest that are defined by a high velocity gradient (corresponding to the boundary layer and the synthetic jets) and high normalised wall distance \(Y^{+}\) (to target wall-resolved simulations). More information about this strategy can be found in [19] and the original and adapted meshes are illustrated in Figure 4. The adapted meshes contain around 66 million cells for the lab scale and 55 million cells for the engine scale. The adaptation was particularly efficient for the lab scale and led to a \(Y^{+}\) value averaged over the perforated plate equal to 3.7, while it is equal to 9.7 for the engine scale. The CPU costs for simulations along a period \(T\) on these adapted meshes with the IDRIS [PERSON] computer (Intel Cascade Lake 6248 processors, with 20 cores at 2.5 GHz) are approximately 57,000 hCPU and 9000 hCPU for the engine and lab scales, respectively.