DLR-F6翼身组合体流场：计算报告与性能分析

1.DLR-F6翼身组合体

DLR-F6翼身组合体是DLR开发的一款现代运输机典型巡航构型。该模型是第二届和第三届AIAA阻力预测研讨会所采用的标准算例之一。DLR-F6外形由机身、机翼和发动机短舱构成。该飞机的设计马赫数为0.75，升力系数0.50。针对带短舱和不带短舱的两种构型，研究人员分别开展了风洞试验，获得了包括升阻力特性曲线、表面压力分布和油流图谱等试验结果。本文以DLR-F6构型为测试算例，检验SU2对于复杂外形流场的模拟能力。

640.webp (3).jpg

图1 DLR-F6翼身组合体（带短舱）风洞试验模型

表1DLR-F6翼身组合体外形部分参数

参数名称	数值
展长	1.1713 m
平均气动弦长	0.1412 m
参考面积	0.1453 m2
展弦比	9.5

2.网格生成

2.1 计算网格

本次计算所采用的网格是第二届AIAA阻力预测研讨会提供的的多块对接结构网格（ftp://cmb24.larc.nasa.gov/outgoing）。稀网格的单元数约为337万，密网格的单元数约为572万。

2.2 SU2网格生成

官方提供的网格为ICEM CFD源文件，需要将其转换为SU2求解器能够读取的网格存储格式。我们采用Pointwise V18.1 R1软件进行格式转换。具体步骤如下：

1）打开ICEM CFD源文件，输出plot3d格式文件。

2）打开Pointwise V18.1 R1软件，导入plot3d格式网格;

3）删除机翼、机身内部固体域的网格块；

4）运行Plot3dMerge.glf脚本，建立块之间的对接关系；

5）将求解器设置为SU2，并设置边界条件；

6）对网格进行旋转、缩放等操作。

7）导出su2格式文件。

3.SU2求解器设置

3.1 流场求解cfg文件设置

下面以马赫数为0.75、攻角为0.49°、湍流模型为SA的计算工况为例，介绍DLR-F6算例的参数设置。

1）问题定义

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------% % % Physical governing equations (EULER, NAVIER_STOKES, % WAVE_EQUATION, HEAT_EQUATION, FEM_ELASTICITY, % POISSON_EQUATION) PHYSICAL_PROBLEM= NAVIER_STOKES %不考虑粘性选EULER，考虑粘性选NAVIER_STOKES % % Specify turbulence model (NONE, SA, SA_NEG, SST) KIND_TURB_MODEL= SA %一般选一方程模型SA或两方程模型SST % % Mathematical problem (DIRECT, CONTINUOUS_ADJOINT) MATH_PROBLEM= DIRECT %不做优化选DIRECT % % Restart solution (NO, YES) RESTART_SOL= NO %重启动计算选YES，同时需要在后面设置重启动文件% Restart flow input file SOLUTION_FLOW_FILENAME % Regime type (COMPRESSIBLE, INCOMPRESSIBLE) REGIME_TYPE= COMPRESSIBLE %马赫数为0.75，对应高速可压缩流场 % % System of measurements (SI, US) % International system of units (SI): ( meters, kilograms, Kelvins, % Newtons = kg m/s^2, Pascals = N/m^2, % Density = kg/m^3, Speed = m/s, % Equiv. Area = m^2 ) % United States customary units (US): ( inches, slug, Rankines, lbf = slug ft/s^2, % psf = lbf/ft^2, Density = slug/ft^3, % Speed = ft/s, Equiv. Area = ft^2 ) SYSTEM_MEASUREMENTS= SI %采用标准单位

2）自由来流参数设置

% -------------------- COMPRESSIBLE FREE-STREAM DEFINITION --------------------% % % Mach number (non-dimensional, based on the free-stream values) MACH_NUMBER= 0.75 %自由来流马赫数 % % Angle of attack (degrees, only for compressible flows) AOA= 0.49 %来流攻角,注意SU2定义X+为流向（机头指向机尾方向），Y+为侧向（翼展方向），Z+为法向（垂直于翼面的方向）。 % % Side-slip angle (degrees, only for compressible flows) SIDESLIP_ANGLE= 0.0 %侧滑角，在本次算例中，SIDESLIP_ANGLE值实际为攻角 % % Init option to choose between Reynolds (default) or thermodynamics quantities % for initializing the solution (REYNOLDS, TD_CONDITIONS) INIT_OPTION= REYNOLDS % REYNOLDS，根据雷诺数计算自由来流参数；TD_CONDITIONS，根据温度和密度参数计算自由来流参数 % % Free-stream option to choose between density and temperature (default) for % initializing the solution (TEMPERATURE_FS, DENSITY_FS) FREESTREAM_OPTION= TEMPERATURE_FS %给定自由来流静温还是静密度 % % Free-stream temperature (288.15 K by default) FREESTREAM_TEMPERATURE= 300 %自由来流静温值 % % Reynolds number (non-dimensional, based on the free-stream values) REYNOLDS_NUMBER= 3.0E6 %参考长度为REYNOLDS_LENGTH（单位米）的自由来流雷诺数（无量纲） % % Reynolds length (1 m by default) REYNOLDS_LENGTH= 0.1412 %平均气动弦长，单位：米

3）气体常数（一般不作修改）

% ---- IDEAL GAS, POLYTROPIC, VAN DER WAALS AND PENG ROBINSON CONSTANTS -------% % % Different gas model (STANDARD_AIR, IDEAL_GAS, VW_GAS, PR_GAS) FLUID_MODEL= STANDARD_AIR % % Ratio of specific heats (1.4 default and the value is hardcoded % for the model STANDARD_AIR) GAMMA_VALUE= 1.4 % % Specific gas constant (287.058 J/kg*K default and this value is hardcoded % for the model STANDARD_AIR) GAS_CONSTANT= 287.058

（4）粘性常数（一般不作修改）

% --------------------------- VISCOSITY MODEL ---------------------------------% % % Viscosity model (SUTHERLAND, CONSTANT_VISCOSITY). VISCOSITY_MODEL= SUTHERLAND % % Sutherland Viscosity Ref (1.716E-5 default value for AIR SI) MU_REF= 1.716E-5 % % Sutherland Temperature Ref (273.15 K default value for AIR SI) MU_T_REF= 273.15 % % Sutherland constant (110.4 default value for AIR SI) SUTHERLAND_CONSTANT= 110.4

5）热传导常数（一般不作修改）

% --------------------------- THERMAL CONDUCTIVITY MODEL ----------------------% % % Conductivity model (CONSTANT_CONDUCTIVITY, CONSTANT_PRANDTL). CONDUCTIVITY_MODEL= CONSTANT_PRANDTL % % Laminar Prandtl number (0.72 (air), only for CONSTANT_PRANDTL) PRANDTL_LAM= 0.72 % % Turbulent Prandtl number (0.9 (air), only for CONSTANT_PRANDTL) PRANDTL_TURB= 0.90

6）参考值设置

% ---------------------- REFERENCE VALUE DEFINITION ---------------------------% % % Reference origin for moment computation 力矩参考点 REF_ORIGIN_MOMENT_X = 0.00 REF_ORIGIN_MOMENT_Y = 0.00 REF_ORIGIN_MOMENT_Z = 0.00 % % Reference length for pitching, rolling, and yawing non-dimensional moment用于力矩系数计算的参考长度 REF_LENGTH= 1.0 % % Reference area for force coefficients (0 implies automatic calculation) 用于升阻力系数计算的参考面积 REF_AREA= 0.0727 %采用半模计算，REF_AREA为全模飞机的一半参考面积 % % Compressible flow non-dimensionalization (DIMENSIONAL, FREESTREAM_PRESS_EQ_ONE, % FREESTREAM_VEL_EQ_MACH, FREESTREAM_VEL_EQ_ONE) %流场计算结果的无量纲方式 REF_DIMENSIONALIZATION= FREESTREAM_VEL_EQ_ONE

7）边界条件设置

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------% % % Navier-Stokes wall boundary marker(s) (NONE = no marker) %物面边界 MARKER_HEATFLUX= (body, 0.0, wing, 0.0 ) %远场边界 % Far-field boundary marker(s) (NONE = no marker) MARKER_FAR= ( inlet, outlet, up, down, right ) %对称边界 % Symmetry boundary marker(s) (NONE = no marker) MARKER_SYM= ( left ) % % Marker(s) of the surface to be plotted or designed %标记用于后处理或设计的边界 MARKER_PLOTTING= (body, wing ) % % Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated %标记用于升阻力系数监测的边界 MARKER_MONITORING= (body, wing )

8）数值求解通用参数

% ------------- COMMON PARAMETERS DEFINING THE NUMERICAL METHOD ---------------% % % Numerical method for spatial gradients (GREEN_GAUSS, WEIGHTED_LEAST_SQUARES) %梯度计算方法 NUM_METHOD_GRAD= GREEN_GAUSS % % Courant-Friedrichs-Lewy condition of the finest grid %最密层网格上的CFL数 CFL_NUMBER= 1.0 % % Adaptive CFL number (NO, YES) %是否采用自适应CFL CFL_ADAPT= YES % % Parameters of the adaptive CFL number (factor down, factor up, CFL min value, % CFL max value ) CFL_ADAPT_PARAM= ( 1.5, 0.5, 1.0, 100.0 ) % % Number of total iterations %最大迭代步数 EXT_ITER= 50000

9）限制器设置

% ----------------------- SLOPE LIMITER DEFINITION ----------------------------% % % Coefficient for the limiter VENKAT_LIMITER_COEFF= 0.05 % % Coefficient for the sharp edges limiter ADJ_SHARP_LIMITER_COEFF= 3.0 % % Reference coefficient (sensitivity) for detecting sharp edges. REF_SHARP_EDGES= 3.0 % % Remove sharp edges from the sensitivity evaluation (NO, YES) SENS_REMOVE_SHARP= NO

10）迭代参数

% ------------------------ LINEAR SOLVER DEFINITION ---------------------------% % % Linear solver for implicit formulations (BCGSTAB, FGMRES) LINEAR_SOLVER= FGMRES % % Preconditioner of the Krylov linear solver (JACOBI, LINELET, LU_SGS) LINEAR_SOLVER_PREC= ILU % % Linaer solver ILU preconditioner fill-in level (0 by default) LINEAR_SOLVER_ILU_FILL_IN= 0 % % Minimum error of the linear solver for implicit formulations LINEAR_SOLVER_ERROR= 1E-10 % % Max number of iterations of the linear solver for the implicit formulation LINEAR_SOLVER_ITER= 5

11）多重网格参数

% -------------------------- MULTIGRID PARAMETERS -----------------------------% % % Multi-Grid Levels (0 = no multi-grid) %采用几重网格 MGLEVEL= 0 % % Multi-grid cycle (V_CYCLE, W_CYCLE, FULLMG_CYCLE) MGCYCLE= V_CYCLE % % Multi-grid pre-smoothing level MG_PRE_SMOOTH= ( 1, 2, 3, 3 ) % % Multi-grid post-smoothing level MG_POST_SMOOTH= ( 0, 0, 0, 0 ) % % Jacobi implicit smoothing of the correction MG_CORRECTION_SMOOTH= ( 0, 0, 0, 0 ) % % Damping factor for the residual restriction MG_DAMP_RESTRICTION= 0.75 % % Damping factor for the correction prolongation MG_DAMP_PROLONGATION= 0.75

12）流场计算数值格式

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------% % % Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC, % TURKEL_PREC, MSW) %对流项格式 CONV_NUM_METHOD_FLOW= ROE % % Spatial numerical order integration (1ST_ORDER, 2ND_ORDER, 2ND_ORDER_LIMITER) %重构格式 MUSCL_FLOW= YES % % Slope limiter (NONE, VENKATAKRISHNAN, VENKATAKRISHNAN_WANG, % BARTH_JESPERSEN, VAN_ALBADA_EDGE) %限制器 SLOPE_LIMITER_FLOW= VENKATAKRISHNAN % Time discretization (RUNGE-KUTTA_EXPLICIT, EULER_IMPLICIT, EULER_EXPLICIT) %时间推进格式 TIME_DISCRE_FLOW= EULER_IMPLICIT % % Relaxation coefficient RELAXATION_FACTOR_FLOW= 0.9

13）湍流计算数值格式

% -------------------- TURBULENT NUMERICAL METHOD DEFINITION ------------------% % % Convective numerical method (SCALAR_UPWIND) %湍流对流项格式 CONV_NUM_METHOD_TURB= SCALAR_UPWIND % % Monotonic Upwind Scheme for Conservation Laws (TVD) in the turbulence equations. % Required for 2nd order upwind schemes (NO, YES) %湍流重构格式 MUSCL_TURB= NO % % Slope limiter (VENKATAKRISHNAN, MINMOD) %限制器 SLOPE_LIMITER_TURB= VENKATAKRISHNAN % % Time discretization (EULER_IMPLICIT) %湍流项推进格式 TIME_DISCRE_TURB= EULER_IMPLICIT % % Relaxation coefficient RELAXATION_FACTOR_TURB= 0.9

14）收敛准则

% --------------------------- CONVERGENCE PARAMETERS --------------------------% % % Convergence criteria (CAUCHY, RESIDUAL) CONV_CRITERIA= RESIDUAL % % Residual reduction (order of magnitude with respect to the initial value) RESIDUAL_REDUCTION= 6 % % Min value of the residual (log10 of the residual) RESIDUAL_MINVAL= -12 % % Start convergence criteria at iteration number STARTCONV_ITER= 10 % % Number of elements to apply the criteria CAUCHY_ELEMS= 100 % % Epsilon to control the series convergence CAUCHY_EPS= 1E-10 % % Direct function to apply the convergence criteria (LIFT, DRAG, NEARFIELD_PRESS) CAUCHY_FUNC_FLOW= DRAG % % Adjoint function to apply the convergence criteria (SENS_GEOMETRY, SENS_MACH) CAUCHY_FUNC_ADJFLOW= SENS_GEOMETRY

15）输入输出设置

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------% % % Mesh input file %网格输入文件 MESH_FILENAME= wb_coarse.su2 % % Mesh input file format (SU2, CGNS, NETCDF_ASCII) %网格格式 MESH_FORMAT= SU2 % % Mesh output file %网格输出文件 MESH_OUT_FILENAME= mesh_out.su2 % % Restart flow input file %重启动输入文件 SOLUTION_FLOW_FILENAME= restart_flow.dat % % Restart adjoint input file %重启动伴随输入文件 SOLUTION_ADJ_FILENAME= solution_adj.dat % % Output file format (PARAVIEW, TECPLOT, STL) %输出文件格式 OUTPUT_FORMAT= TECPLOT_BINARY % % Output file convergence history (w/o extension) %输出的残差历史文件 CONV_FILENAME= history % % Output file restart flow %输出的重启动文件 RESTART_FLOW_FILENAME= restart_flow.dat % % Output file restart adjoint %输出的重启动伴随文件 RESTART_ADJ_FILENAME= restart_adj.dat % % Output file flow (w/o extension) variables %流场体数据输出文件名 VOLUME_FLOW_FILENAME= flow % % Output file adjoint (w/o extension) variables VOLUME_ADJ_FILENAME= adjoint % % Output objective function gradient (using continuous adjoint) GRAD_OBJFUNC_FILENAME= of_grad.dat % % Output file surface flow coefficient (w/o extension) %边界数据输出文件 SURFACE_FLOW_FILENAME= surface_flow % % Output file surface adjoint coefficient (w/o extension) SURFACE_ADJ_FILENAME= surface_adjoint %文件输出频率 % Writing solution file frequency WRT_SOL_FREQ= 500 %残差信息输出频率 % Writing convergence history frequency WRT_CON_FREQ= 1 %

3.2 并行运算脚本sh文件设置

在算例cfg文件所在目录，创建如下内容的sh文件，采用sbatch命令提交即可。

#!/bin/bash #SBATCH -N 7 #并行节点数 #SBATCH -n 168 #并行cpu数，=24*节点数 #SBATCH --job-name=DLR-F6 #job的名称 #SBATCH --ntasks-per-node=24 #每个节点用到的cpu数，无需修改 #SBATCH --output=%j.out #算例运行过程中在屏幕上显示的信息 #SBATCH --error=%j.err #报错信息 mpirun SU2_CFD coarseAoA0.490.cfg #流场求解 mpirun SU2_SOL coarseAoA0.490.cfg #输出tecplot结果文件