A High-Resolution Method for Flow Simulations with Block-Structured Cartesian Grid Approach

Transcription

1 20th AIAA Computational Fluid Dynamics Conference June 2011, Honolulu, Hawaii AIAA A High-Resolution Method for Flow Simulations with Block-Structured Cartesian Grid Approach Takashi Ishida 1 Soshi Kawai 2 and Kazuhiro Nakahashi 3 Department of Aerospace Engineering Tohoku University Aoba , Sendai, Miyagi , Japan ishida@ad.mech.tohoku.ac.jp A high-resolution numerical method for flow computations using Building-Cube Method (BCM) is developed. BCM is a block structured Cartesian mesh approach proposed as the next generation CFD algorithm by one of the authors. One of the critical problem of conventional Cartesian mesh approach is the wall boundary treatment. The gridless-type boundary treatment is construcrted to resolve boundary layer efficiently in a Cartesian grid. One of the attractive features of BCM is easy construction of high-order computational schemes. Compact differencing scheme with low-pass filtering and high-order Lagrange interpolation for the communication between cube blocks are constructed and the capability of the developed approach is demonstrated through a 2-D inviscid vortex advection problem. The proposed method is applied to the aeroacoustic problem. I. Introduction omputational fluid dynamics (CFD) has achieved a significant progress in its algorithms and applications in the Clast 40 years and become a necessary tool for understanding fluid mechanics and developing fluid machines. Among various approaches, a computational method using unstructured meshes is an attractive choice to handle three-dimensional complex geometries over the approaches using structured meshes 1, 2. However, there remains mainly two issues regarding the unstructured mesh CFD. One is that the unstructured mesh method always needs a water-tight geometry to start mesh generation. The mesh generation process can become time consuming if a geometry model is non-water-tight because of repairing and/or cleaning a dirty geometry which may involve cracks and/or overlaps before mesh generation. The other issue is the difficulties (and also high computational costs) in constructing high-order schemes because of its unstructured data construction. When we consider direct numerical simulation (DNS) or large-eddy simulation (LES) of turbulent flows, including mixing, sound-generation, unsteady load, etc. which may be of interest, these can be the bottlenecks of current CFD use. In these days, Cartesian mesh method is reviewed because of the progress of computer capability and ease of handling grid generation around complex geometries 3-6. In order to fully utilize the rapid progress of computers and the advantages of Cartesian mesh method, one of the authors developed a new block-structured Cartesian mesh approach named Building-Cube Method (BCM). BCM can easily handle complex geometries and moving/deforming bodies. The authors showed the efficiency and capability of the algorithm However, similar to the most of Cartesian mesh methods the numerical scheme used in BCM is limited to a conventional loworder upwind-biased scheme, such as MUSCL scheme with a limiter function. The use of high-resolution schemes is highly desirable for DNS and LES. We also believe that the advantage of Cartesian mesh methods can be fully utilized by using high-resolution finite-difference schemes. The objective of this study is to develop a high-resolution numerical method for BCM to apply the method to DNS or LES of turbulent flows. We first carefully assess the effect of numerical schemes and interpolation methods on the results through a 2-D vortex advection problem. We also construct a gridless type boundary treatment to 1 Ph.D. student, Department of Aerospace Engineering, Tohoku University (Currently, Japan Aerospace Exploration Agency:JAXA), Senior Member AIAA. 2 Postdoctoral Fellow, Center for Turbulence Research, Stanford University (Currently, Institute of Space and Astronautical Science:ISAS), Senior Member AIAA. 3 Professor, Department of Aerospace Engineering, Tohoku University, Associate Fellow AIAA. 1 Copyright 2011 by the, Inc. All rights reserved.

2 capture a smooth geometry in Cartesian mesh. Then the proposed method is applied to the aeroacoustic sound propagation problem. II. Building-Cube Method The BCM basically employs the equally-spacing Cartesian mesh approach because of the simplicity in the mesh generation, the solution algorithm and the post processing. The simplicity will become more important for largescale computations. The most critical problem of the conventional Cartesian mesh, however, is how to fit to the local characteristic flow length without introducing the complexity of the algorithm. Here, a flow field is divided into a number of sub-domains, called Cube as shown in Fig. 1. The geometrical size of each cube is determined by adapting to the geometry and the flow features like an adaptive refinement. In each cube, an equally-spacing Cartesian mesh is used. Fig. 2 shows an example of three-dimensional computational mesh around ONERA M6 wing model that consists of cells in each cube. All cubes have the same number of Cartesian mesh so that the local computational resolution is determined by the cube size. (a)cube Fig. 1 Cube(left) and Cell(right). (b)cell Fig. 2 The staircase representation of the wall boundaries of ONERA M5. 2

3 Loop for cubes III. Mesh Generation for BCM In the BCM, the computational mesh is generated in two steps; cube generation and the computational cell generation in each cube as shown in Fig. 3. A STL (stereolithography) file that is one of the CAD output formats is employed for the definition of the three-dimensional geometry. The advantage of the STL data is the simplicity since they contain only pure geometric information of the coordinates of each triangular facet and its corresponding unit normal vector. The Cube generation procedure is similar to the quadtree/octree method. Fig. 4 schematically shows the procedure, presenting a symmetry plane of the ONERA M5 wing-fuselage configuration. First, a computational domain is divided into a coarse Cartesian mesh [Fig. 4 (b)]. Then hexahedral cubes that include or cross the body surface are divided into eight cubes. This refinement procedure is repeated until the minimum cube size becomes less than a user specified value [Fig. 4 (c)]. The next procedure is a smoothing of the size differences among cubes. For this procedure, a cube whose adjacent cube is smaller than a quarter of its own size is detected and divided [Fig. 4 (d)]. At the end, the cubes inside the body are identified and removed [Fig. 4 (e-f)]. Fig. 4 (f) shows the completed cube mesh. Input CAD data (STL) Cube generation Cell generation Output of mesh data Fig. Figure 3 Flow 5. Flow chart chart of BCM of BCM mesh mesh generation. generation. (a) (b) (c) (d) (e) (f) Fig. 4 Cube generation procedure using a geometry-adaptive refinement for ONERA M5 fuselage: (a) computational domain, (b)-(d) refinements, (f) completed cube frame. After cube generation, Cartesian mesh (cell) that is equal-spacing and equal number of nodes in each cube is generated (Fig. 5). Intersection checks for cells that across the body surface and the inside/outside determination are performed in each cube. The intersection check calculation is done in the cut cubes which cross to the body surface. At the end, the mesh information which is necessary for the flow solver is constructed. 3

4 Fig. 5 Cell generation around NACA0012 wing. IV. Flow Solver for BCM A. Governing Equation A non-dimensional form of the compressible Navier-Stokes equations can be written in the conservative form as, ( 1 ) where,, are time, the coordinate, and the Reynolds number. The conservative vector, the inviscid flux vector, and viscous flux vector are defined by ( 2 ) ( 3 ) ( 4 ) where are the density, pressure, specific total energy, temperature and thermal conductivity of the fluid, respectively. represents the velocity component of the flow in the coordinate direction. This set of equations is closed by the equation of state for a perfect gas, ( 5 ) where is the ratio of the specific heats. The components of the viscous stress tensor are given by ( 6 ) where is Kronecker's delta symbol and is viscosity coefficient determined by Sutherland's relationship. 4

5 B. Spacial Discretization The compressible Navier-Stokes equations are solved by a finite difference scheme on equally spaced Cartesian mesh. In this study, 6th order explicit central difference schemes and 6 th -order compact differencing scheme 16 with 10 th -order low-pass filtering 17 is used to evaluate the derivatives. On the interior cube domain, the spatial derivative of any scalar quantity may be found at the node points in computational space by solving the tridiagonal system arising from the formula: ( 7 ) where,, for the sixth-order schemes. The second derivative is computed by applying the first derivative twice for the viscous flux vectors. Equation ( 7 ) uses a five-point stencil, and thus the derivatives at a location on or one point away from a boundary cannot be found using the centered formula. At these boundary points, high-order one-sided formulations are utilized to maintain the tridiagonal structure of the set of equations. Because the schemes generated by Eq. ( 7 ) are centered, they are non-dissipative in nature. Thus, numerical instabilities arising from poor grid quality, unresolved scales, or boundary conditions will be left to grow unchecked and can potentially corrupt the solution. For this reason, following tenth (2Nth)-order low-pass filtering scheme is used on the conservative properties once in each direction after each final Runge-Kutta step in order to ensure numerical stability: ( 8 ) where is the solution vector, is filtered quantity. The coefficient is a free parameter satisfying the constraint that may be used to control the spectral response of the filter. As the value of decreases from its maximum permissible value of where no filtering takes place, the filter becomes more dissipative as more of the higher wavenumber content of is removed. The coefficients on the right-hand side of Eq. ( 8 ) may be determined as a function of the free parameter based on the desired order-of-accuracy of the filter. The value of the coefficients for all centered filters employed in this study are given as a function of 17. A tenth-order filter requires data at eleven grid points, and thus could not be applied at nodes within five points of a boundary. At these points, special formulations are required to filter in this near-boundary region. Because of the proliferation in the number of computational boundaries when employing the domain decomposition strategy discussed in the following section, particular attention is paid here to those near-boundary filters. A one-sided filter equation for near-boundary points 2 through 5 may be written as: ( 9 ) The coefficients are given in Ref.17 for the orders of one-sided filters used in this study. The filter of Eq. ( 8 ) is implemented by filtering the conserved variables at each node once in each spatial direction after the final stage of the explicit time-integration scheme. The overall flow-solution procedure is shown in Fig. 6. 5

6 Fig. 6 Overall flow-solution procedure. C. Time Integration The classic explicit, fourth-order Runge-Kutta method is employed. To implement this method, the residual defined from Eq. ( 1 ) as a function of by: is ( 10 ) The RK4 method integrates from time step at time to time step at time through a four-stage approach as: ( 11 ) 6

7 D. Wall Boundary Treatment The basic concept for the boundary treatment is to couple the BCM solver and gridless type solver. Gridless method is applied to near the wall boundary with subgrid which is generated like a prismatic layer to resolve a boundary layer and the remaining domain is solved by BCM solver. Fig. 7 shows the sequence of grid generation for the coupling computation. The grid generation procedure is composed of two parts, BCM grid generation and subgrid generation near the wall boundary. At first, voxel, which is ordinary BCM grid, is generated around an input geometry. At this time, the Cartesian grid has flag information of identifying the wall and fluid regions as shown in Fig. 7 (a) (blue:wall cell, green:fluid cell). Then, the wall cell flag is extended to outward to the fluid region (Fig. 7 (b)). For the next step, the subgrid is generated near the wall boundary using normal information (Fig. 7 (c)). The subgrid is generated with a stretching factor and each boundary points have several subgrids in normal direction. After the subgrid generation, the fluid cell flag which is the nearest 2 cell from the wall cell is changed and grid point is generated (Fig. 7 (d)). These grid points work as communication grid points to send/receive physical values between BCM solver and gridless type solver. (a) (b) (c) Fig. 7 Subgrid generation near the wall boundary. (Red line: geometry definition) (d) 7

8 In the gridless method, derivatives are expressed by summation of surrounding grid points named cloud. Fig. 8 shows the example of a cloud around grid point i and the derivative of grid point i in x-direction is expressed by the following formula: ( 12 ) where represents the group of grid points which are included in a cloud of grid point. The coefficients are computed by using least-square method. Fig. 8 Cloud around grid point. Introducing the gridless approach, equation ( 1 ) can be written in the gridless form as: ( 13 ) where and represent the inviscid and viscous numerical fluxes between the grid point and. and are the primitive values on the mid-point of the grid point and. Numerical flux is also computed by using an approximate Riemann solver of HLLEW. The primitive variables on the mid-point of an edge are evaluated by the 2nd-order MUSCL scheme. Equation ( 13 ) is applied to the subgrid and communication nodes. Sets of cloud points affect the solution accuracy so that the cloud points have to be selected properly. Cloud points are usually selected with a control radius (Fig. 9). However, grid points are generated near the wall boundary with a stretching factor and lay in Cartesian grid with large aspect ratio in this study so that the simple searching using control radius results in bad sets of cloud points. Control radius has to be treated carefully. Thus, in this study, we propose to use the local Delaunay triangulation to reconstruct the sets of cloud points. Fig. 9 Cloud searching with control radius "r". 8

9 (a) (b) (c) Fig. 10 Cloud reconstruction using local Delaunay triangulation. (a)point searching for a cloud around the blue point with local radius r. (b)local Delaunay triangulation. (c)resulted points (shown in red) for a cloud. Fig. 10 shows schematics of cloud point reconstruction using local Delaunay triangulation. At first, candidate grid points are searched using local radius of r (Fig. 10 (a)). Then, local Delaunay triangulation is applied (Fig. 10 (b)). The grid points which is connected to the focused grid point is selected as a cloud (Fig. 10 (c)). 9

10 E. Cube Boundary Treatment Since present BCM adopts computational grid which has adjacent grid size jump twice/half as shown in Fig. 11, the data communication among cubes has to be treated cafefully. In the present study, high-order Lagrange interpolation is implemented for the data communication among cubes. Fig. 11 Overlapping cells in 2D. The interpolation used for the data communication among cubes is classified in two cases, L2S (Large cell to Small cell) and S2L (Small cell to Large cell). Fig. 12 shows the stencils used for the Lagrange interpolation in the present study. Physical values of first fringe near the cube boundary is interpolated by one-side difference like Lagrang interpolation. On the other hand, physical values of second and third fringe are interpolated by central difference like Lagrange interpolation. (a) S2L (4x4 stencils) (b) L2S (3x3 stencils) Fig. 12 Stencils for Lagrange interpolation in two dimensional case. V. Results 1. Vortex advection The first test case is an inviscid convecting vortex in non-uniform cubes. Since vortex preservation is sensitive to the numerical dissipation, this problem can be used to assess the capability of the present high-order scheme. The initial velocity and pressure filed of the zero net circulation vortex is given by the following relations 18 : ( 14 ) ( 15 ) 10

11 ( 16 ) where and are the and velocity components, is the static pressure, is the vortex core radius and is defined as ( 17 ) The uniform freestream Mach number, the non-dimensional vortex strength and center of the vortex are:, and. The density is assumed constant. Nine different levels of grid spacing are employed. The computational domain is and. The computational time-step size is set to that corresponds to a CFL number of 0.04 on finest grid. The results are discussed at times of where the vortex the vortex convects distances of. Periodic boundary conditions are applied on the x and y direction. Fig. 13 shows the computational grid. For the reference solution, the computational grid which is composed by uniform cube shown in Fig. 14 is used. Number of overlapping grid point is changed 0 to 3. Three types of Lagrange interpolation are used, 4/3s ( stencils for S2L and stencils for L2S), 6/5s ( stencils for S2L and stencils for L2S), and 8/7s ( stencils for S2L and stencils for L2S). Fig. 15, Fig. 16 and Fig. 17 show the comparison of error plot of each interpolation method. Fig. 18Fig. 19 and Fig. 20 shows the comparison of V profile. From the error plot, the interpolation without overlapping and high-order Lagrange interpolation resulted in unstable. On the other hand, 1 cell overlapping with 6/5s interpolation showed reasonable result in terms of computational costs compared with uniform cube result. Fig. 13 Non-uniform cube. Fig. 14 Uniform cube. 11

12 Fig. 15 Error plot of 4/3s. Fig. 16 Error plot of 6/5s. Fig. 17 Error plot of 8/7s. 12

13 Fig. 18 Comparison of V profile (4/3s, ). Fig. 19 Comparison of V profile (6/5s, ). Fig. 20 Comparison of V profile (8/7s, ). 13

14 2. Lid-Driven Cavity Flow The driven cavity flow in a square cavity was computed by the proposed method. This test case is chosen to examine the accuracy and effectiveness of the developed method for low-reynolds number viscous flow. In this computation, single cube domain is used and the angle of a cavity domain is set to 0, 15, 30 and 45 degree in the Cartesian grid (Fig. 23). The minimum grid spacing of BCM grid is set to and 3 layers of subgrid are generated around a wall boundary in each angle. This computation was performed at a Mach number of 0.2 and a Reynolds number of 400. Fig. 23 shows the computational grid and computed velocity contours for the flow field in driven cavity. Fig. 21and Fig. 22 show the profile for u-velocity component along vertical lines and v-velocity component along horizontal lines passing through the geometric center of the cavity domain. The solution of Ghia et al. (18), which is the reference solution of this cavity problem, is also shown for comparison. The computational results showed quite good agreement with that of Ghia in each angle. Fig. 21 U profile. 14

15 Fig. 22 V profile. (a) (b) (c) (d) Fig. 23 Computational grid (left side) and computed velocity contours (right side). 15

16 ((a):0 degree, (b):15 degree, (c):30 degree and (d):45 degree.) 3. Turbulent Flow around RAE2822 RAE2822 airfoil is commonly used as a test case for the newly developed flow solver as well as in turbulence models. We use this test case to investigate the performance of the proposed method coupled with RANS turbulent model on high Reynolds number turbulent flows. The inflow Mach number is set to The Reynolds number is 6.56 million, and turbulence flow is assumed over the whole flow region. Spalart Almarlous turbulence model which is one-equation model is used 20. The angle of attack is set to 2.79 degrees. Detailed flow conditions can be found in the experimental report by Cook et al 21. The computational grid is shown in Fig. 24. The total number of cubes is 274 with 16x16 cells in each cube. Therefore the total number of computational cells is approximatly Ten layers of subgrid are generated around a wall boundary like a prismatic layer with stretching factor of 1.5. The minimum grid spacing of BCM grid and the subgrid are set to and with respectively. This value is chosen to resolve the viscous sublayer at this Reynolds number. First-order LU-SGS implicit time integration is used both BCM solver and gridless type solver. The computed Cp distribution is compared with the experimental data and the result obtained by unstructured grid solver 22 in Fig. 26. The computed Mach contours and pressure contours in the flow field are shown in Fig. 25. The result of computation showed good agreement with the experimental data and unstructured grid solution. (a)whole view (b)leading edge (c)trailing edge Fig. 24 Computational grid around RAE

17 (a)pressure contour Fig. 25 Computational rsults. (b)mach contour Fig. 26 Cp distribution around RAE

18 4. Aeroacoustic sound propagation around a circular cylinder The scattering of sound from a single cylinder which is one of benchmark problem of 2nd CAA work shop is examined to validate the present method for CAA. This problem consists of a single cylinder of diameter centered at and insonified by a source with a spatial compactness parameter and. Source term is expressed by following formula: ( 18 ) The function is of the form: ( 19 ) and is used to ramp up the onset of the source over some specified time interval. is used in this section. Fig. 27 (left) show the computational grid used for this problem. The computational grid is composed of 113 cube with cells in each cubes. The minimum grid spacing of BCM grid and subgrid are and respectively. Four stage Runge-Kutta time integration is used for both BCM solver and gridless type solver and data communication is done in each Runge-Kutta stages. Free parameter for filtering is set to. Fig. 27 (right) shows the computed pressure contours. Fig. 28 shows the fluctuating pressure time history at the point. The ramping up of the source term, the transients generated by the initial reflection from the cylinder, and the eventual evolution of the filed into a time-periodic state may be easily seen. Fig. 29 shows the comparison of fluctuating pressure RMS and present result showed good agreement with the analytic solution. 18

19 (a) (b) (c) Fig. 27 Computational grid (left) and computed pressure contours (right). 19

20 P' P' Time Time Fig. 28 Fluctuating pressure time history at the point. Fig. 29 Comparison of around a circular cylinder. 20

21 VI. Conclusion High-order Lagrange interpolation, high-order compact finite differencing scheme and high-order space filtering were implemented to BCM and a computational approach for aeroacoustic problem was developed. Gridless boundary treatment was also developed for the realistic wall boundary treatment. The present approach was examined by 2D vortex advection. For the demonstration, present approach was applied to a 2D aeroacoustic sound propagation problem around a circular cylinder and present result showed quite good agreement with the analytic solution. In the present approach, each computation is closed by each cube and one-sided differencing scheme is used near the block boundary, however, numerical instability is suppressed by high-order space filtering. Acknowledgments This work is supported by the Grant-in-Aid for JSPS Fellows. References 1 Ito, Y. and Nakahashi, K., Direct Surface Triangulation Using Stereolithography Data, AIAA Journal, Vol. 40, No. 3, March 2002, pp Ito, Y. and Nakahashi, K., Surface Triangulation for Polygonal Models Based on CAD Data, International Journal for Numerical Methods in Fluids, Vol. 39, Issue 1, pp , May Aftosmis, M.J., Berger, M.J., Melton, J.E., Robust and efficient Cartesian Mesh Generation for Component- Based Geometry, AIAA Journal, Vol. 36, No.6, pp , Aftosmis, M. J., Solution Adaptive Cartesian Grid Methods for Aerodynamic Flows with Complex Geometries von Karman Institute for Fluid Dynamics Lecture Series , 28th computational fluid dynamics. 5 Ono, K., Aoki, H., Sato, S. and Shiozawa H., Construction of Rapid Simulation Tool for Automotive CFD, 8th International Conference on Numerical Grid Generation in Computational Field Simulation (2002) Ono, K., Tawara, T. (RIKEN), Yoshikawa, H. (Fujitsu Nagano Systems Engineering), Cartesian Grid Generation Towards Large-Scale Practical Flow Simulations, APCOM 07-EPMESC XI, 2007, Kyoto, Japan. 7 Nakahashi, K., High-Density Mesh Flow Computations with Pre-/Post-Data Compressions, AIAA paper, , Nakahashi, K., Kitoh, A., Sakurai Y., Three-Dimensional Flow Computations around an Airfoil by Building- Cube Method, AIAA paper, , Kamatsuchi, T., Turbulent Flow Simulation around Complex Geometries with Cartesian Grid Method, AIAA paper, , Takahashi, S., Ishida, T., Nakahashi, K., Kobayashi, H., Okabe, K., Shimomura, Y., Soga T., and Musa, A., Large Scaled Computation of Incompressible Flows on Cartesian Mesh Using a Vector-Parallel Supercomputer, Proceedings of 20th International Conference on Parallel Computational Fluid Dynamics, Lyon, France, pp , May Ishida, T., Takahashi, S., and Nakahashi, K., Efficient and Robust Cartesian Mesh Generation for Building- Cube Method, Journal of Computational Science and Technology, Vol. 2, No. 4, pp , Zeeuw, D. D., and Powell, K. G., An Adaptively Refined Cartesian Mesh Solver for the Euler Equations, Journal of Computational Physics, Vol. 104, 1993, pp. 56, Berger, M., and Aftosmis, M., Aspects (and Aspect Ratios) of Cartesian Mesh Methods, Proceedings of the 16th ICNMFD, 1999, pp. 1, Ogawa, T., An Efficient Numerical Algorithm for the Tree-data Based Flow Solver, Computational Fluid Dynamics 2000, 2000, pp. 337, Ogawa, T., An Adaptive Cartesian Mesh Flow Solver Based on the Tree-data with Anisotropic Mesh efinement, Computational Fluid Dynamics 2002, S. K. Lele, Compact finite difference schemes with spectral-like resolution, J. Comput. Phys., vol. 103, pp , M. R. Visbal and D. V. Gaitonde, High-order-accurate methods for complex unsteady subsonic flows, AIAA J., vol. 37, no. 10, pp , T.J. Poinsot, S.K. Lele, Boundary conditions for direct simulations of compressible viscous flows, Journal of Computational Physics, 101 (1), pp ,

22 19 S.Kawai, S.K.Lele, Localized artificial diffusivity scheme for discontinuity capturing on curvilinear meshes, Journal of Computational Physics, 227 (22), pp , November, Spalart, P. R. and Allmaras, S. R., A One-Equation Turbulence Model for Aerodynamic Flows, AIAA Paper , 1992, 21 Cook, P.H., McDonald, M. A., Firmin, M.C.P., Aerofoil RAE Pressure Distributions, and Boundary Layer and Wake Measurements, Experimental Data Base for Computer Program Assessment, AGARD Report AR 138, K. Nakahashi, Y. Ito and F. Togashi, Some challenges of realistic flow simulations by unstructured grid CFD, Int. J. for Numerical Methods in Fluids, 2003, Vol.43, pp ,