Investigation of the Effect of a Realistic Nozzle Geometry on the Jet Development

Transcription

1 Investigation of the Effect of a Realistic Nozzle Geometry on the Jet Development Mehmet Onur Cetin a, Matthias Meinke a,b, Wolfgang Schröder a,b Abstract Highly resolved large-eddy simulations (LES) of a helicopter engine jet including the nozzle geometry are performed. A flow solver for compressible flow based on hierarchically refined Cartesian meshes and a conservative cut-cell method is used for the computations. The impact of the nozzle geometry on the jet development is analyzed for two variants of the nozzle geometry, a simplified geometry with only a center body and the full geometry of the engine nozzle including four struts which support the center body. A synthetic turbulence formulation is used to prescribe inlet boundary conditions for the nozzle, which mimic the exit conditions after the last turbine stage. To verify the numerical method, a single cold round jet is computed and the results are compared to reference data. Results for the helicopter engine jet are presented for the time-averaged velocity field and turbulence intensities. 1 Introduction Most studies for the prediction of jet flows have been conducted for simplified inlet conditions for the jet without taking into account the details of the nozzle geometry to keep the required computational resources within reasonable limits, e.g. [1, 2, 3]. However, the jet development in the near field of the jet with the potential core region, where significant noise sources are generated, is strongly influenced by the turbulence level and length scales at the nozzle exit. Therefore, it can be assumed that geometric details upstream of the nozzle exit generating a specific turbulence field should not be neglected and the engine nozzle should be included in the flow domain to obtain a more realistic jet flow field. In this study, the impact of a realistic helicopter engine nozzle on the jet development is studied by simulating the jet for two variants of the engine nozzle geometry, i.e., a baseline nozzle geometry including only a centerbody, referred to as Model 1, and a nozzle including the center body and four support struts, referred to as Model 2. The simulations that include the engine nozzle involve a high mesh resolution, since the boundary layers on the nozzle wall have to be adequately resolved to avoid, e.g., unphysical boundary layer separation in the divergent section of the nozzle, and also the larger scales of turbulent structures generated downstream of the centerbody have to be captured a Institute of Aerodynamics, RWTH Aachen University, Wüllnerstr. 5a, 5262 Aachen, Germany, office@aia.rwth-aachen.de b Forschungszentrum Jülich, Jülich, Germany, JARA High-Performance Computing 1

2 2 Cetin et al. accurately. To verify that the mesh resolution is adequate for the prediction, a grid convergence study for Model 1 is performed, where a fine mesh with 33 million cells and a very fine mesh with 197 million mesh cells are used. The numerical method, the computational domain, and the boundary conditions are briefly outlined in Section 2. First, the results for a validation test and subsequently, for a jet including the nozzle are discussed in Section 3. Finally, conclusions are drawn in Section 4. 2 Numerical Method A computational method based on a finite volume scheme is used to solve the spatially filtered Navier-Stokes equations for compressible, unsteady, and turbulent flow. An implicit grid filter is assumed and the LES model corresponds to the monotone integrated large-eddy simulation (MILES) approach [5], i.e., the dissipative truncation error of the numerical scheme is responsible to mimic the dissipation of the unresolved subgrid scale stresses. The convective fluxes of the governing equations are formulated by a low dissipation version of the advection upstream splitting method (AUSM) [8]. The cell center gradients are computed using a second-order accurate least-squares reconstruction scheme [9], i.e., the overall spatial approximation is second-order accurate. For stability reasons, small cut-cells are treated using an interpolation and flux-redistribution method developed by Schneiders et al. [1]. A second order 5-stage Runge-Kutta method is used for the temporal integration. This solution method has been validated and used successfully with several test cases, see e.g. [6, 7, 1]. A Cartesian unstructured fully parallel mesh generator with hierarchical mesh refinement is used for the grid generation [11]. Further details of the numerical methods, i.e., the discretization and computation of the viscid and inviscid fluxes, are given in [8]. 2.1 Computational Setup The inlet of the domain is located downstream of the last turbine stage. Corresponding flow conditions are set at the inlet boundary which are taken from the measurements of a full scale turbo-shaft engine [4]. Isotropic synthetic turbulence is generated at the inlet plane with a turbulence intensity of approx. 1% [12]. For the outflow and lateral boundaries of the jet domain, the static pressure is set to be constant and other variables are extrapolated from the internal domain along linearized characteristics. To damp numerical reflections at the boundaries, sponge layers are used [13]. At the nozzle wall, the no-slip condition with a zero wall-normal pressure gradient and adiabatic wall conditions are applied. Fig. 1 and 1 show the interior of the two nozzle variants. The ratio of the radii of the center body and the exit cross section is R cb /R =.42 and the ratio of the chord length and the maximum radial extent of the struts is C s /R s =.57. Two meshes, i.e., a fine and a very fine grid, are generated for Model 1 by a Cartesian unstructured grid generator [11] to analyze the impact of the grid resolution on the jet development. Computational details are

3 Numerical Investigation of the Effect of a Realistic Nozzle Geometry on the Jet Development 3 given in Table 1. The computation and sampling time are chosen large enough to ensure convergence of the statistical data. The domain possesses a streamwise and radial extent of 36 and 16 diameters for the validation study and 42 and 32 diameters for the jet with nozzle. There are 336 grid points in the radial direction at the nozzle-exit for the fine meshes. Fig. 1(c) illustrates the structure of the Cartesian mesh. x= z x y (c) Fig. 1 Geometry of the Model 2, geometry of the Model 1, (c) 2D view of a coarse Cartesian mesh with 41 million cells for the Model 2, where the zoomed view shows the resolution of the fine mesh. Model 1 very fine Model 1 fine Model 2 fine Validation Test Mach number Re number 7.5 x x x x 1 5 Mesh points 197 x x x x 1 6 Min. cell length x,y,z =.148D x,y,z =.297D x,y,z =.297D x,y,z =.19D Simulation time 44D/u 48D/u 48D/u 72D/u Mean flow sampling 21D/u 26D/u 26D/u 14D/u Number of samples Table 1 Simulation parameters. 3 Results 3.1 Validation Test To validate the numerical method, a round jet exhausting into a quiescent air at standard room conditions with M = U j a =.9 and Re D = ρu jd η = 4 x 1 5 is simulated, where U j is the inflow velocity at the centerline, a the speed of sound, D the jet diameter, ρ the density and η the dynamic viscosity. The results are compared to data from previous studies [1, 2, 14, 15]. To promote the transition to turbulence, the jet is forced via vortex rings [2] plus random perturbations, that are only introduced in the shear layer of the jets, defined by a hyperbolic-tangent velocity profile [2]. The streamwise velocity profiles are compared in Fig. 2. In agreement with the reference

4 4 Cetin et al. results, the velocity decays downstream of the potential core at about x 1R in Fig. 2, where R is the radius of the jet defined at the inlet of the computational domain R = D/2. The streamwise profile of the RMS value of the axial velocity fluctuations is illustrated in Fig. 2. The comparison shows a slight discrepancy of the axial location and the magnitude of the peaks, due to the different numerical method and the mesh resolution used for the present simulation. In general, however, it can be stated that there is a reasonable agreement between the reference data and the results of the present method U c /U j u rms /U j Fig. 2 Streamwise distributions of the axial velocity and axial turbulence intensity for: ( ) current simulation (M =.9, Re D = 4 x 1 5 ), (- -) Bogey et al. [2] (M =.9, Re D = 4 x 1 5 ), ( ) Koh et al. [1] (M =.9, Re D = 4 x 1 5 ), ( ) Lau et al. [15] (M =.9, Re D = 1 6 ) and ( ) Arakeri et al. [14] (M =.9, Re D = 5 x 1 5 ). 3.2 Influence of the Engine Nozzle LES of the helicopter engine jet including the engine nozzle are performed. The decay of the centerline velocity and the turbulence intensity profile of the streamwise velocity component are illustrated in Fig. 3 for Model 1 for the fine and very fine mesh, and for Model 2 for the fine mesh. The comparison of the results for the fine and very fine mesh for Model 1 indicates the results to be grid converged, since there are only slight differences in the results for the two meshes. Comparing the results for Model 1 and 2 shows that the jet develops substantially different until the end of the unperturbed core is reached, while downstream of the core the centerline velocity profile for the two nozzle geometries are quite similar. The presence of the 4 struts in Model 2 is obviously responsible for a higher turbulence intensity and consequently, an enhanced mixing, which leads to a smaller centerline velocity and a shorter core length of the jet. This result is confirmed by the results in Fig. 3, where the profile of the streamwise velocity fluctuations along the streamwise direction is shown. Two maxima in the turbulence intensity profile are visible, where the first peak occurs downstream of the centerbody in the nozzle due to the flow separation at approx. x 1.2R where R is the nozzle exit radius, where also a negative axial velocity occurs. The second peak occurs at the end of the core region at about x 1.5R. Comparing the values for the turbulence

5 Numerical Investigation of the Effect of a Realistic Nozzle Geometry on the Jet Development U c /U j.25 u rms /U j Fig. 3 Streamwise distributions of the axial velocity and axial turbulence intensity for: ( ) Model 1 fine, (- -) Model 1 very fine, ( ) Model 2 fine. 1 2 (c) Fig. 4 Cross section of the nozzle geometry for Model 2 at x 2.8R. Time-averaged countours of the axial velocity component for Model 2 at plane 1, (c) at plane 2. intensity for Model 1 and 2, a 2% higher turbulence intensity due to the struts can be observed in the region <, i.e., inside the nozzle. The turbulence intensity at the end of the core at 1 is 15% lower. This comparison shows that the wake of the struts interacts with the wake of the bluff-body, which amplifies the turbulent intensity upstream of the nozzle exit. The existence of the struts diminishes, however, the turbulence intensity at the end of the core. This is important, since the most dominant noise sources occur in this region. To analyze the mean flow field for Model 2 in more detail, contours of the axial velocity component are illustrated in two planes in Fig. 4. It can be seen that the effect of the non-axisymetry of the nozzle geometry on the flow field is still visible downstream of the nozzle-exit and only vanishes after the core region. Finally, Fig. 5 presents the radial profiles of the axial velocity and RMS axialvelocity fluctuations at the nozzle-exit for Model 1 and 2. It is obvious that the profiles for Model 1 and 2 differ substantially due to the four struts. Furthermore, Model 2 shows a strongly non-axisymmetric flow field. The wake of the struts reduces the magnitude of the velocity distribution such that an almost flat distribution is obtained at the nozzle exit. Between the struts in plane 2, the axial velocity shows a higher maximum value which is also located at a larger radius such that a stronger shear occurs in this region. The comparison of the axial turbulence intensity profiles in Fig. 5 shows the pronounced impact of the struts on the turbulence intensity.

6 6 Cetin et al U/U j u rms /U j r/r r/r Fig. 5 Radial distributions at the nozzle exit x/d= for axial velocity and axial turbulence intensity for: ( ) Model 1 fine, (- -) Model 1 very fine, ( ) Model 2 fine at plane 1, and ( ) Model 2 fine at plane 2. Due to the higher shear in plane 2 of Model 2 a higher turbulence intensity can be observed which peaks at a larger radius compared to Model 1. 4 Conclusion & Outlook LES results for a helicopter engine jet including details of the nozzle geometry were presented. A grid convergence study for a simplified nozzle showed a resolution with approx. 329 million cells to be sufficient for the simulation. Two geometries of the helicopter engine nozzle were used to analyze their impact to the jet development. The presence of four struts noticeably changes the results for the velocity distribution and the turbulence intensity in the core region of the jet. The struts enhance the turbulence mixing inside the nozzle and reduce the centerline velocity as well as the turbulence intensity of the axial velocity component in the core region of the jet. Next, the impact of the nozzle geometry on the aeroacoustic noise will be studied based on a hybrid LES-CAA method. Acknowledgements The research was funded by the European Community s Seventh Framework Programme (FP7, ) PEOPLE programme under the grant agreement No. FP (COPAGT project). The authors gratefully acknowledge access to the computing hardware of the High Performance Computing Center Stuttgart (HLRS) and FZ Jülich (JSC). References 1. S. R. Koh, W. Schröder, and M. Meinke, Computers & Fluids, 78, 24 (213) 2. C. Bogey, C. Bailly, AIAA journal 43(5), 1 (25) 3. J. B. Freund, Journal of Fluid Mechanics 438, 277 (21) 4. B. Pardowitz, U. Tapken, K. Knobloch, F. Bake, E. Bouty, I. Davis, G. Bennett 2th AIAA/CEAS Aeroacoustics Conference, (214) 5. J. P. Boris, F. F. Grinstein, E. S. Oran, & R. L. Kolbe, Fluid dynamics research, 1(4-6), 199 (1992) 6. M. Konopka, M. Meinke, & W. Schröder. AIAA journal, 5(1), (212) 7. N. Alkishriwi, M. Meinke, & W. Schröder. Computers & Fluids, 37(7), (28) 8. M. Meinke, W. Schröder, E., W., Krause, T. Rister, Computers & Fluids, 31(4), 695 (22)

7 Numerical Investigation of the Effect of a Realistic Nozzle Geometry on the Jet Development 7 9. D. Hartmann, M. Meinke, W. Schröder, Computers & Fluids 37(9), 113 (28) 1. L. Schneiders, D. Hartmann, M. Meinke, W. Schröder, Journal of Computational Physics 235, 786 (213) 11. A. Lintermann, S. Schlimpert, J. H. Grimmen, C. Günther, M. Meinke, W. Schröder, Computer Methods in Applied Mechanics and Engineering 277, 131 (214) 12. R. P. Kunnen, C. Siewert, M. Meinke, W. Schröder, & K. D. Beheng, Atmospheric Research, 127, J. B. Freund, AIAA journal, 35(4), V. Arakeri, A. Krothapalli, V. Siddavaram, M. Alkislar & L. Lourenco, Journal of Fluid Mechanics 49, 75 (23) 15. C. Lau, Jark, P. J. Morris, M. J. Fisher, Journal of Fluid Mechanics 93(1), 1 (1979)