Compressible Flow Modeling in STAR-CCM+

Transcription

1 Compressible Flow Modeling in STAR-CCM+ Version 01/11

2 Content Day 1 Compressible Flow WORKSHOP: High-speed flow around a missile WORKSHOP: Supersonic flow in a nozzle WORKSHOP: Airfoil

3 Compressible Flow Modeling in STAR-CCM+ Version 01/11

4 Isentropic Compressible Flow Reference m A = T t T = 1 + γ 1 2 P t P = 1 + γ 1 2 γ R V = M M 2 γrt P t T t M 1 + γ 1 2 γ = c p c p R M 2 γ M 2 γ γ γ 1 where A Area m Mass flow rate M Mach number M Molecular weight P Static pressure P t R Total pressure Specific gas constant R Universal gas constant [8314 J/kmol K] T Static temperature T t V g Total temperature Velocity magnitude Ratio of specific heats R = R M 4

5 Mesh / Grid Resolution Vehicle / Blade surface resolution important At least 36 points around circle to obtain surface curvature resolution needed Aerodynamic surfaces (i.e. wings / winglets / blades) need to be resolved, especially at leading and trailing edges, curvature resolution does help, but at least 6 cells across trailing edge of surfaces needed Wake and/or shock regions may need additional grid refinement use volume sources if needed in areas where flow is important but no geometrical features exist on which to base furher grid refinement Prism/extrusion layers can be crucial, especially in external aero type analysis 5

6 Domain Extent Considerations External aerodynamic analyses Large enough domain aroung object / vehicle 10 spans width, spans for wake region All flows, recirculation at boundaries should be avoided, especially with shock present 6

7 Free Stream Boundary Typically used as far field boundary conditions for external aerodynamic problems Specify the flow direction, Mach number, static pressure, static temperature and turbulence quantities Flow direction may be specified by Flow Angles (see next slide), Components (in a specified coordinate system) or as Boundary-Normal (normal to the boundary surface) 7

8 Free Stream Boundary Flow Angles Flow Angle Properties Coordinate System The coordinate system to use. Cartesian Cylindrical Laboratory Spherical Specifies the Cartesian coordinate system. Specifies the cylindrical coordinate system. Specifies the laboratory coordinate system. Specifies the spherical coordinate system. Rotation Convention The order in which to apply the rotations specified by the angles. X Convention (Z-X-Z) Y Convention (Z-Y-Z) Yaw, Pitch, Roll Convention (Z-Y-X) For Euler angles (f, q, y), the first rotation is by angle f about the z-axis, the second is by angle q about the x-axis, and the third is by angle y about the z-axis. For Euler angles (f, q, y), the first rotation is by angle f about the z-axis, the second is by angle q about the y-axis, and the third is by angle y about the z-axis. For Euler angles (f, q, y ), the first rotation is by angle f about the z-axis, the second is by angle q about the y-axis, and the third is by angle y about the x-axis. Axes Convention How to treat the axes during rotations. Fixed Axes Moving Axes Makes all rotations relative to the original fixed axes. Makes second and third rotations relative to the rotated axes. Reference Vector Method A unit vector that is rotated to convert angles and rotation conventions to a direction. Specified as a single three-part, comma-separated number. Selects the method to use for specifying the angle data. Constant Field Function Table (iteration) Table (time) Specifies the angle as a single three-part, comma-separated number. A Constant node will be added as a child to this node. For two-dimensional cases, only your entries for the x- and y- directions will be relevant to the calculations Defines the angle using a field function (typically user-defined). A Function node will be added as a child to this node Defines the angle as a function of iteration number. A Table (iteration) node will be added as a child to this node. Defines the angle as a function of physical time. A Table (time) node will be added as a child to this node. 8

9 Stagnation Inlet Boundary Stagnation boundaries need special consideration in supersonic flows. Pressure ratio analysis needed to get correct inlet conditions, i.e. P tot / P stat = f ( Mach ) Specify the Supersonic Static Pressure, Total Pressure, Total Temperature and turbulent quantities Note that both the total pressure and supersonic pressure are relative to the specified reference pressure The supersonic static pressure is designed to establish incoming flow rate for a stagnation boundary that is supersonic (otherwise it is ignored) Be aware that if any time the boundary does go supersonic (even prior to convergence), this value will be used and the default or poor choice could lead to divergence 9

10 Mass Flow Inlet Boundary Most often used in conjunction with pressure outlets Specify the flow direction, mass flow rate, supersonic static pressure, total temperature and turbulence quantities Flow direction options are the same as for free stream boundaries Supersonic static pressure is used only where the inlet flow us supersonic (as with stagnation inlet boundaries) Mass flow rate may be negative (outflow) despite the name (see help for additional guidelines on this option) 10

11 Pressure Outlet Boundary Most often used in conjunction with stagnation inlet and mass flow inlet boundaries Specify the pressure, static temperature and turbulence quantities For subsonic outflow, the specified pressure is applied as a static pressure, while for supersonic outflow the boundary pressure is extrapolated from the cell adjacent to the boundary Where inflow occurs, the specified pressure is applied as a total pressure Boundary velocities are extrapolated from the interior in all cases 11

12 Initial Conditions Specify (static) pressure, static temperature, velocity and turbulence quantities Intializing pressure: If there are no pressure boundaries, the specified initial pressure must not result in a non-physical absolute pressure For free-stream flows, the initial pressure should equal the free-stream pressure For internal (duct) flows, the initial pressure should be chosen so that it is equal to or higher than the outlet pressure (helps to inhibit reversed flow at the outlet) It is a good idea to intialize the flow field prior to running and judge if it makes sense 12

13 Solver Controls The Coupled Implicit Solver is strongly recommended for all compressible flows (especially if Mach number is greater than ~0.3) For steady flows, the Courant Number is the key control parameter Default of 5.0 may be too high, especially for flows with shocks (lower this values to 1.0 or 2.0 and then ramp up over a few hundred iterations) For transient flows the choice of the time step is crucial Set the time step such that the convective Courant number is ~1 everywhere Set stopping criteria based on residual tolerances of key variables (especially continuity, momentum and temperature) Set sufficient number of inner iterations for all variables to converge (but not so many that the solution is inefficient) 13

14 Coupled Flow Model Advantages of the AUSM+ scheme Algorithmic simplicity and straightforward extension for complex conservation laws Accurate capture of shock- and contactdiscontinuity Numerical solutions that preserve positivity and satisfy entropy Reduced susceptibility to carbuncle phenomena AUSM+ recommmended for all compressible flows Explicit relaxation offers another way to relax coupled flow solution (alternative to Courant number) Change the Explicit Relaxation Factor from its default value (1.0) to a lower value, e.g

15 AMG Solver Controls If instability persists, then modify AMG Linear Solver settings Increase Convergence Tolerance to 0.1 (from default of 0.01) Increase V Cycle > Post-Sweeps to 3 (from default of 1) Decrease V Cycle > Max Levels to 2 (from default of 50) 15

16 Directional Mesh Reordering Directional reordering may improve solution convergence Reorder the mesh in the primary flow direction Optimizes solver performance due to the way it updates solution variables Also reduces the bandwidth of the solution, making the solver more efficient Right-click on Regions > [Regions name] > Reorder Mesh In the popup window check the Use directional reordering box and set the direction vector as desired 16

17 Turbulence Modeling General recommendations k-e are the models of choice for internal flows Spalart-Allmaras models are often the best choice for external flows with mild or no separation k-w models are a good alternative to Spalart-Allmaras for external flows, especially those with more severe separation Reynolds StressTransport models are recommended for flows with anisotropic turbulence The All-y+ wall treatment is recommended for any model for which it is available 17

18 Esitmation of Desired Near-Wall Cell Size We generally wish to target a specific value of y+ for the near-wall mesh, where y + = u y ν u = τ w ρ The wall sheat stress τ w can be related to the skin friction coefficient: C f = τ w ρu 2 2 The skin friction coefficient can be estimated from correlations For a flat plate For pipe flow C f 2 = Re L 1 5 C f 2 = Re D

19 Judging Convergence For steady state, is solution unchanging? Do shock locations remain constant? Do vortices/separation points/recirculation zones remain unchanging over a number of iterations? Constant temperature and pressure fields? For transients, is each time step converging to the prescribed inner iterations convergence criterion before reaching the maximum number of inner iterations? Key data monitor settle to a constant value External aero lift/drag forces or Cl/Cd coefficients level off at a constant value Flow rates settle to constant values (such as in turbomachinery cases) Any other engineering quantities of note (swirl, forces, moments, etc.) are monitored throughout and settle to constant values 19

20 Nozzle Best Practices Set initial conditions to have pressure and temperature values as they would be at Mach = 0.8 This will help provide an initial velocity in the flow direction that is somewhat representative and enables the flow to wash over the geometry Without doing so, there is risk of low pressure vacuum regions occuring which could lead to instabilities If convergence issues related to turbulence arise, try raising the turbulence intensity to 0.1 and the turbulent viscosity ratio to 1000 for the initial and inflow boundary conditions At startup, a lot can happen and the vast gradients between a near laminar startup and a turbulent flow early on could prove problematic for the solver If the values for turbulence happen to be known at the boundaries, use these if they are reasonable 20

21 Nozzle Best Practices KEY POINT: Ramp down exit pressure boundary conditions for temperature and pressure using field functions 21

22 Nozzle Best Practices Results! Note: The black and white d(rho)/d(p) result is obtained by turning on temporary storage for the coupled solver settings) 22

23 Analysis Output/Post Processing Contour Plots of Temperature Pressure Density Mach Number Velocity Magnitude - All these help examine the physical nature of the flow and if there are shocks, are great properties to visualize them! - Can also help judge convergence of the flow fields Velocity vector plots (to examine flow direction, swirl, wake, vortices, etc.) Reports Lift/Drag monitors and plots for forces and coefficients are almost assuredly needed to judge convergence and report results for external aero cases 23

24 Heat Transfer Coefficients & Adiabatic Wall Temperature For external high-speed (compressible) flows, the appropriate choice of fluid temperature is the adiabatic wall temperature An adjustment to the freestream temperature, it accounts for compressibility and viscous dissipation effects Adiabatic wall temperature is defined as: T aw = T r c γ 1 M 2 where T is the freestream temperature, g is the specific heat ratio, M is the Mach number and r c is the recovery factor The recovery factor may be approximated by: r c Pr 1 2 (laminar flow) r c Pr 1 3 (turbulent flow) 24

25 WORKSHOP: High-speed flow around a generic tactical missile Version 01/11

26 Outline Problem definition High-speed flow around a generic tactical missile (subsonic, transonic, supersonic) Various angles of attack may be simulated Key features Polyhedral meshing with prismatic layers Freestream boundary condition used around the missile Important boundary numbers Mach number: 1.5 Angle of attack (AOA): 20 deg Static temperature: 293 K Static presure: Pa Feel free to change the above conditions as desired! 28

27 Data import Load an existing simulation File > Load Simulation... or click on the load icon in the System toolbar Browse to tacmissile_tutorial.sim Click Ok 29

28 Set Scene Parameters Open the existing scene Right-click Scenes > Geometry Scene 1 > Open Using the camera icon toolbar select Look Down > +X +Y +Z > Up +Y Make scene transparent in the Vis Click on the transparent icon in the Vis toolbar 30

29 Save The Model It s a good idea to save the model every time you ve accomplished a specific set of tasks and you re pretty sure that everything is okay with the model On the main menu, under File, choose save or simply click on the icon in the System toolbar 31

30 Check Surface Check the surface Right-click on Geometry > Parts > tacmissile > Repair Surface... Click OK In the new tab click on Start Diagnostics, leave all defaults and click OK The check reveals that the surface has 5 Pierced Faces, 1916 Poor Quality Faces and 16 Close Proximity Faces but no other problems We will use the Surface Remesher to improve the quality of the surface 32

31 Mesh Settings Create a new mesh continuum and fill it with the models Right-click on Continua > New > Mesh Continuum Right-click on Continua > Mesh 1 > Select Meshing Models... We will create a polyhedral mesh with prism layers Surface Remesher Polyhedral Mesher Prism Layer Mesher 33

32 Mesh Reference Values Set the reference values, these will be the default mesh parameters used on all boundaries Right-click on Mesh 1 > Reference Values > Edit... Reference Values Base Size Value 0.2 m Prism Layer Thickness Relative 2% Surface Size: Tet/Poly Density Relative Minimum Size Relative Target Size Density Growth Factor 2% 20% Tet/Poly Volume Blending Blending Factor 0.8 Tet/Poly Density controls the overall volume mesh density, while the Growth Factor controls the rate of growth from fine to coarse areas Tet/Poly Volume Blending controls the rate of cell growth from volume sources 34

33 Boundary Mesh Values We will change the default mesh settings at several boundaries: The leading edges of the fins requires a much finer mesh than the rest of the domain Right-click on Regions > Body 1 > Boundaries > fin LE > Edit... Set the values according to the table Repeat this for fin TE Mesh Conditions fin LE fin TE Custom Surface Size Yes Yes Mesh Values Surface Size: Relative Minimum Size 0.05% 0.5% Surface Size: Relative Target Size 0.4% 1% 35

34 Boundary Mesh Values The mesh on the symmetry boundary needs to be able to grow from a small size near the missule surface to a much larger size further away Right-click on Regions > Body 1 > Boundaries > symmetry > Edit... Change the boundary type Boundary Type: Symmetry Set the values according to the table Mesh Conditions Custom Surface Size symmetry Yes Mesh Values Surface Size: Relative Minimum Size 1% Surface Size: Relative Target Size 2000% 36

35 Boundary Mesh Values The freestream boundary is the hemisphere sourrounding the one side of the missile The mesh here is large, so the Minimum Surface Size is left at its default while the Target Surface Size is set to a large value Right-click on Regions > Body 1 > Boundaries > freestream > Edit... Change the boundary type Boundary Type: Free Stream Set the values according to the table Mesh Conditions Custom Surface Size freestream Yes Mesh Values Surface Size: Relative Minimum Size 25% Surface Size: Relative Target Size 2000% 37

36 Volume Mesh Refinement STAR-CCM+ has the ability to locally refine the mesh in the region sourrounded by a volume We will do this around the missile Create the volume Right-click on Geometry > Parts > New Shape Part > Cylinder Start End X 0 m 0 m Y 0 m 0 m Z m m Radius 0.1 m Click Create 38

37 Volume Mesh Refinement Create a volumetric control with the cylinder as volume source Right-click Contina > Mesh 1 > Volumetric Control > New Right-click Volumetric Control 1 > Edit... Use the newly created cylinder as input part Part Group: Cylinder Set the values according to the table Mesh Conditions Polyhedral Mesher: Customize Surface Remesher: Customize freestream Yes Yes Mesh Values Custom Size: Relative Size 6% 39

38 Physics Settings Create a new physics continuum and fill it with the models Right-click on Continua > New > Physics Continuum Right-click on Continua > Physics 1 > Select Models... For high-speed compressible flow the coupled solvers are best We expect significant flow separation at this large angle of attack, so the SST (Menter) K-Omega model with All y+ Wall Treatment is chosen Three Dimensional Steady Gas Coupled Flow Turbulent K-Omega Turbulence 40

39 Solver Settings The AUSM+ FVS scheme is chosen for the coupled solver Physics 1 > Models > Coupled Flow Set AUSM+ FVS in the properties window as the scheme for Coupled Inviscid Flux 41

40 Air Material Properties Deceleration of the flow near the missile surface will create large static temperature gradients, so Sutherland s Law is used for Dynamic Viscosity and Thermal Conductivity Right-click Physics 1 > Models > Air > Material Properties > Edit... Choose Sutherland s Law, leave the default values Other properties have a weaker temperature dependence and are left constant 42

41 Air Reference Values All reference values will stay unchanged The reference pressure is set to the static ambient pressure: Pa 43

42 Air Initial Conditions The static pressure is relative to the reference pressure, so it is set to zero The static temperature is set to the ambient temperature The velocity components correspond to the specified Mach number, ambient temperature and angle of attack Right-click on Continua > Physics 1 > Initial Conditions > Edit... Initial Parameter Velocity Components Value [0.0, , ] m/s 44

43 Boundary Condition: Free Stream The physics conditions for the freestream boundary needs to be changed Right-click Regions > Body 1 > Boundaries > freestream > Edit... Physics Conditions Flow Direction Specification freestream Angles Physics Values Flow Angles: Reference Vector [0.0, 0.0, 1.0] Flow Angles: Constant [0.0, -20.0, 0.0] deg] Mach Number: Constant

44 Boundary Conditions The symmetry boundary is already if type Symmetry Plane No other settings are needed for this type of boundary All other boundaries are adiabatic, no-slip walls which is the default type Wall Summary of boundary types Boundary Name Boundary Type freestream symmetry Free Stream Symmetry Plane aft base body mid fin LE fin sides Wall fin TE nose scoop 46

45 Mesh Generation We are now ready to generate the mesh!!! We will generate the surface mesh and the volume mesh in two separate steps Generate the surface mesh See that is it generated successfully (no errors) Visually inspect it to see if density is as desired Only after these steps are complete should volume mesh generation be attempted Generate the surface mesh now this can be done in one of two ways On the main menu, select Mesh > Generate Surface Mesh Click the Generate Surface Mesh icon on the Mesh Generation toolbar Generate Surface Mesh Generate Volume Mesh 47

46 Surface Mesh To view the remeshed surface, create a new mesh scene Click on the scene icon in the Vis toolbar The mesh is coarse but acceptable for our purposes Accurate results would require a muchfiner mesh 48

47 Volume Mesh Now generate the volume mesh again in one of two ways On the main menu, select Mesh > Generate Volume Mesh Click the Generate Volume Mesh icon on the Mesh Generation toolbar To view the volume mesh create a new mesh scene 49

48 Volume Mesh Section Create a cut through the geometry Change the view using the camera icon in the Vis toolbar and select Look Down > +X > Up +Y Click on the Create Plane Section icon and create the section as shown Choose to create a New Geometry Displayer In the scene/plot tab disable Mesh 1 displayer Right-click Mesh Scene 2 > Displayers > Mesh 1 > Toggle Visibility 50

49 Volume Mesh Section Turn the mesh display on clicking on the globe icon in the Vis toolbar Note that there are two prism layers adjacent to the wall boundaries forming the surface of the missile Note also that there are no prism layers adjacent to the symmetry and freestream boundaries Once again the mesh is too coarse for accurate results, but acceptable for our purposes 51

50 Solver Settings Right-click on Solvers > Coupled Implicit and choose Edit To accelerate the convergence, increase the Courant Number to 10.0 All other settings can be left at their defaults 52

51 Stopping Criterion Click on Stopping Criteria > Maximum Steps and set the Maximum Steps to

52 Post Processing: Frontal Area Create a report to calculate the frontal area of the surface Right-click Reports > New Report > Frontal Area Rename this report frontal area Right-click frontal area > Edit The defaults for View Up, Normal and Units are acceptable For Parts, select all parts that comprise the missile surface Do not select Body 1: freestream or Body1: symmetry 54

53 Post Processing: Frontal Area Right-click Reports > frontal area and select Run Report The Output window should appear as follows (the exact value of area depends on the created mesh) 55

54 Post Processing: Drag Coefficient Report Create a Force Coefficient Report Right-click Reports > New Report > Force Coefficient Rename this report cd Set the Reference Density, Reference Velocity and Reference Area as shown Note that the computed frontal area has been used as the Reference Area Select Pressure + Shear as the Force Option The Direction is set to be aligned with the flow direction Select only the Parts that comprise the missile surface (same as for the frontal area) 56

55 Post Processing: Lift Coefficient Report Create a lift coefficient report The only difference here is the direction of the force, so we will simply copy and paste the cd report and change the direction vector Rename the report to cl 57

56 Post-Processing: Drag & Lift Coefficient Plots We must now create monitors and plots from these reports Click on Reports > cd, hold down the Ctrl key, and click on Reports > cl While continuing to hold down the Ctrl key, right click on either report name and choose Create Monitor and Plot from Report In the Create Plot from Reports window, select Multiple Plots (one per report) 58

57 Post-Processing: Velocity Vector Scene Create a new vector scene Rename it to Velocity Vectors Change the view - Look Down > +X+Y+Z > Up +Y Go to the scene/tab panel Select Regions > Body 1 > symmetry to be put in Parts Click on Displayers > Vector 1 and change the Vector Scale to Screen Size in the Properties window 59

58 Post-Processing: Streamline/Mach Number Scene We now compose a scene with several displayers, starting with an empty scene 1. Displayer: Scalar displayer showing Mach number on the missile surface 2. Displayer: Streamline displayer 3. Displayer: Geometry displayer showing the mesh on the missile surface 60

59 Post-Processing: Streamline/Mach Number Scene Create an empty scene Rename to Mach Number with Streamlines Change the view to Look Down > -X > Up +Y We will use a Symmetry Transform for all displayers, this was automatically created by STAR-CCM+ using the definition of the symmetry boundary 61

60 Post-Processing: Streamlines Define new streamlines and add them to a new displayer in the scene Right-click Derived Parts > New Part > Streamline Change the Seed Mode to Line Seed Set the starting and ending points for the line seed as shown, as well as the resolution Start End X 0 m m Y -0.9 m m Z -1.5 m -1.5 m Resolution 40 In the Display sub-window, select New Streamline Displayer Click Create Rename this derived part to streamline 62

61 Post-Processing: Streamline Displayer In the Scene Explorer of the Mach Number with Streamlines scene, make the following settings for the streamline displayer: Scalar Field: Pressure Coefficient Color Bar: invisible Transform: symmetry 1 63

62 Post-Processing: Scalar Displayer Create a new scalar displayer Right-click Displayers > New > Scalar For Parts, select only the parts that comprise the missile surface As Scalar Field function choose Mach Number Click on the Scalar 1 displayer and in the properties window change the Contour Style to Smooth Filled Set Transform to symmetry 1 64

63 Post-Processing: Geometry Displayer Create a new scalar displayer Right-click Displayers > New > Geometry For Parts, select only the parts that comprise the missile surface Click on the Geometry 1 displayer and in the properties window check the Mesh box, uncheck the Outline box Set Transform to symmetry 1 65

64 Run Simulation It s now time to run the analysis!!! This can be done in either of two ways: On the main menu, select Solution > Run Click the Run button on the Solution toolbar 66

65 Residuals Plot 67

66 Drag Coefficient Plot 68

67 Lift Coefficient Plot 69

68 Velocity Vectors Scene 70

69 Mach Number with Streamlines Scene 71

70 Summary An analysis of high-speed compressible flow around a missile at 20 AOA has been performed A polyhedral mesh with prism layers and local refinement around the fin leading and trailing edges has been constructed It was noted that production analyses should use a much finer mesh than what was used here The analysis and post-processing setup was performed 72

71 WORKSHOP: Supersonic Flow in a Converging-Diverging Nozzle Version 01/11

72 Outline Problem definition Steady 2D flow in a converging-diverging nozzle with shocks Key features Polyhedral meshing with prismatic layers Stagnation inlet and pressure outlet boundaries Coupled implicit solver Boundary condition ramping using field functions 74

73 Data import Start a new STAR-CCM+ session File > New Simulation... or click on the new icon in the System toolbar Click OK Import the mesh File > Import > Import Volume Mesh... Navigate to the workshop 2 folder, then seelct nozzle.ccm Click OK 75

74 Imported Mesh The imported mesh is 2D and consists of approximately 197K polyhedral cells As seen in the screenshot below, there are 3 prism layers adjacent to the duct walls 76

75 Physics Settings Fill the existing physics continuum with models Right-click on Continua > Physics 1 > Select Models... Note in particular the choice of the Axisymmetric, Ideal Gas and Coupled solver models for this analysis (you may need to disable Two Dimensional) Axisymmetric Steady Gas Coupled Flow Ideal Gas Turbulent K-Epsilon Turbulence 77

76 Solver Settings Change the settings of the coupled flow solver in its properties window Continua > Physics 1 > Coupled Flow - Explicit relaxation: Coupled Inciscid Flux: AUSM+ FVS 78

77 Boundary Condition: Axis Check that the boundary type for axis boundaries is set to Axis With the Ctrl key pressed, select Regions > Body_1_2D > Boundaries > far field axis and nozzle axis and check in the Properties window that Type is set to Axis The icons in front of the boundaries are also good indicators for the type of the boundary Summary of boundary types: Boundary Name pressure outlet stagnation inlet far field axis nozzle axis near nozzle vertical wall nozzle wall top slip wall Boundary Type Pressure Stagnation Inlet Axis No-slip Wall Slip Wall 79

78 Boundary Condition: Wall Ensure that the Shear Stress Specification for top slip wall is Slip Regions > Body_1_2D > Boundaries > top slip wall > Physcis Conditions > Shear Stress Specification: Slip 80

79 Boundary Condition: Stagnation Inlet The physics conditions for the inlet boundary needs to be changed Right-click Regions > Body 1 > Boundaries > stagnation inlet > Edit... Check that Type is Stagnation Inlet Set values according to the table: Physics Conditions Supersonic Static Pressure Total Pressure Total Temperature stagnation inlet 9E+05 Pa 1E+06 Pa 2300 K Turbulence Intensity 0.1 Turbulent Viscosity Ratio 1E+04 Note: Since the inflow is expected to be subsonic, the Supersonic Static Pressure value should not affect the final solution 81

80 Boundary Conditions: Ramping Functions Recall that a helpful strategy for starting up nozzle problems is to ramp the outlet conditions down from the inlet conditions To do this we will use field functions To define a field function, right-click Tools > Field Functions > New This creates a field function named User Field Function 1 We will create two new field functions, one for the pressure, one for the temperature Relative Pressure shall be ramped from 1E+06 Pa to zero over 1000 iterations Temperature is ramped from 2300 K to 300 K over 1000 iterations 82

81 Boundary Conditions: Ramping Functions Name Function Name Dimensions Definition P_Down pdown Pressure ($Iteration < 1000)? 1e6*(1-$Iteration/1000) : 0.0 T_down tdown Temperature ($Iteration < 1000)? ( *(1-$Iteration/1000)) :

82 Boundary Conditions: Pressure Outlet Set the field functions P_down and T_down as boundary condition for pressure outlet Right-click Regions > Body_1_2D > Boundaries > pressure outlet > Edit... Check that Type is Pressure Outlet Set values according to the table: Physics Conditions Pressure: Method Pressure: Field Function Temperature: Method Temperature: Field Function pressure outlet Field Function P_down Field Function T_down Turbulence Intensity 0.1 Turbulent Viscosity Ratio 1E+04 84

83 Physics: Initial Conditions The values set as initial conditions are basically the same as the conditions of the stagnation inlet The velocity is simply an estimate of the average velocity in the domain Pressure is set to a value that results in Ma=0.8 in the smallest part (P t = 10 6 Pa) P = P t 1 + γ 1 2 M2 γ γ 1 Initial Conditions Pressure E+05 Pa Temperature 2300 K Turbulence Intensity 0.1 Turbulent Velocity Scale 100 m/s Turbulent Viscosity Ratio 1E+04 Velocity [0.0, 0.0, 0.0] 85

84 Solver Parameters and Stopping Criterium We will decrease the Courant Number in the coupled solver Click on Solvers > Coupled Implicit and set the Courant Number value to 2.0 This will help to stabilize the convergence, especially in the early stages We will leave the Courant Number at 2.0 for the entire analysis, but we could have also ramped it from 2.0 to some higher value Set the Stopping Criteria > Maximum Steps value to

85 Post Processing: Transform We will define a transform so that we can view a serction through the full 3D axisymmetric geometry Right-click Tools > Transforms > New Graphics Transform > Simple Transform - This creates a new transform named Simple Transform 1 Set the Rotation Angle and Rotation Axis Transform Properties Rotation Angle 180 deg Rotation Axis [1, 0, 0] 87

86 Post Processing: Mach Number Scene We now compose a scene with two scalar displayers 1. Displayer: Scalar displayer showing Mach number 2. Displayer: Scalar displayer, same settings plus Transform 88

87 Post Processing: Mach Number Scene Create a new scalar scene Rename to Mach Number Note that the region is already added to Parts Click on the scene/plot tab Make the outline displayer invisible Right-click Displayers > Outline 1 > Toggle Visibility Settings for Displayer > Scalar 1 For Contour Style select Smooth Filled As Scalar Field choose Mach Number 89

88 Post Processing: Mach Number Scene Copy the Scalar 1 displayer This creates a new displayer named Copy of Scalar 1 Settings for Displayer > Copy of Scalar 1 Change Transform to Simple Transform 1 Uncheck the Visible box under Color Bar 90

89 Run Simulation Create other scenes as desired (e.g. for pressure, temperature, velocity vectors) Now run the simulation in either of two ways: On the main menu, select Solution > Run Click the Run button on the Solution toolbar Note: The simulation will run for 8000 iterations for about 3 hours on 4 processors. To get the following pictures it is necessary to run the simulation much longer. Increase the Courant number to 5.0 after the first 8000 steps and run it as long as necessary (approx. 30,000 iterations). 91

90 Mach Number 8,000 iterations 30,000 iterations 16,000 iterations 92

91 Absolute Pressure 8,000 iterations 30,000 iterations 16,000 iterations 93

92 Temperature 8,000 iterations 30,000 iterations 16,000 iterations 94

93 Summary The flow is fairly well-developed and we can see the shock at the nozzle throat and the beginning of the formation of shock diamonds downstream of the nozzle It was necessary to reduce the Courant Number for the coupled implicit solver to 2.0 (from the default value of 5.0) to start the solution, but it can probably be increased now that the important flow features are in place Field functions were used to ramp down the outlet conditions this is a useful approach for many high-speed compressible internal flow problems 95

94 96

95 CD-adapco training goes online For all trainings you attend you get online access to input files and presentation through the Training Center Visit to find this material under Past Courses Please fill in our online training feedback form that is located there too Copyright 2011 CD-adapco

96 STAR-CCM+ User Guide 7361 Transonic Flow over an Airfoil The tutorial simulates two-dimensional, turbulent, compressible, transonic air flow over an idealized airfoil, as shown below. The free-stream Mach number is and the angle of attack is 2.54 o. This corresponds to RAE2822 case 6 in Reference [272]. The free-stream flow is subsonic, becoming supersonic on the suction side of the airfoil and subsonic again through a shock wave. The lift and drag coefficients are monitored to help determine whether convergence is reached. The final distribution of the pressure coefficient on the airfoil is then compared to experimental data. Importing the Mesh and Naming the Simulation Start up STAR-CCM+ and select the New Simulation option from the menu bar. Continue by importing the mesh and naming the simulation. A one-cell-thick, three-dimensional, hexahedral mesh has been prepared for this analysis. The mesh corresponds to an angle of attack of 0 o in the default Laboratory coordinate system. Select File > Import > Import Volume Mesh... from the menus. In the Open dialog, simply navigate to the doc/tutorials/aerofoil subdirectory of your STAR-CCM+ installation directory and select file aerofoil.ccm which contains the mesh and boundary definitions. Click the Open button to start the import. STAR-CCM+ will provide feedback on the import process, which will take a few seconds, in the Output window. A geometry scene will be created in the Graphics window. Finally, save the new simulation to disk under file name aerofoil.sim. Version

97 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7362 Converting to a Two-Dimensional Mesh The mesh region can now be converted to a two-dimensional one. There are special requirements in STAR-CCM+ for three-dimensional meshes that need to be converted to two-dimensional. These are: The grid must be aligned with the X-Y plane. The grid must have a boundary plane at the Z = 0 location. The mesh imported for this tutorial was built with these requirements in mind. Were the grid not to conform to the above conditions, it would have been necessary to realign the region using transformation and rotation facilities available in STAR-CCM+. Select Mesh > Convert to 2D... In the Convert Regions to 2D dialog that appears, make sure the checkbox of the Delete 3D regions after conversion option is ticked, and click OK. Once you have clicked OK, the mesh conversion will take place and the Geometry Scene 1 display will show the two-dimensional geometry in the Version

98 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7363 Graphics window. (If the image does not appear immediately, simply click the (Reset View) button on the toolbar.) All the geometry parts will be shown, viewed from the +z-direction. The mouse rotation option is suppressed for two-dimensional scenes. Right-click the Physics 1 continuum node and select Delete. Click Yes in the confirmation dialog. Setting up the Models Models define the spatial and temporal solution methods and the physical properties of the flow. In this example, the flow is steady, turbulent and compressible. The default Spalart-Allmaras turbulence model and the ideal gas model will be used. The analysis will also use the coupled solver, which is recommended for all supersonic and transonic compressible flows. By default, a continuum called Physics 1 2D is created when the mesh is converted to two-dimensional. To use a more appropriate name: Right-click the Physics 1 2D node and select Rename...Change the name to Aerofoil. Version

99 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7364 The continuum definition will now be edited to select appropriate physical models for the fluid. Right-click the Aerofoil continuum node and select item Select models. The Physics Model Selection dialog will guide you through the model selection process by showing only options that are appropriate to the choices already made. Make sure that the Two Dimensional radio button is selected from the Space group box. Select Gas in the Material group box. Select Coupled Flow in the Flow group box. Select Ideal Gas in the Equation of State group box. Select Steady in the Time group box. Select Turbulent in the Viscous Regime group box. Select Spalart-Allmaras Turbulence in the Reynolds-Averaged Turbulence group box. Click Close. Inside the Continua node, the color of the Aerofoil node has turned from gray to blue to indicate that models have been activated. Open the Aerofoil node and then the Models node. Version

100 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7365 The selected models now appear within that node. Save the simulation. Setting Material Properties Open the Gas and Air nodes. The material properties for air are contained within. Select the Material Properties > Dynamic Viscosity > Constant node. In the Properties window, change the dynamic viscosity value to 4.61e-5 PaS. This corresponds to a Reynolds number of 6.5 x 10 6 [272]. Version

101 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7366 Setting Initial Conditions The initial velocity field will apply free-stream conditions across the entire domain, i.e. a velocity of m/s calculated using the equation: u M P ref = ref (1641) where M = 0.725, P ref = , ref = and = 1.4 To specify an angle of attack of 2.54 o for the initial velocity, we will create a new coordinate system. Open the Tools node at the bottom of the simulation tree and right-click the Coordinate Systems > Laboratory > Local Coordinate Systems node. Select New > Cartesian. Version

102 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7367 An in-place dialog will appear to help you create the coordinate system. In the Axis Definition group box, change the i Direction to the following: [0.999, , 0] Click Renormalize. The j Direction will change automatically to ensure that the axes are perpendicular. The i Direction may also readjust itself Version

103 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7368 slightly. Click Create, then Close. A node called Cartesian 1 will be created within the Coordinate Systems node. The resulting Properties window is shown below. This now defines a coordinate system that, when viewed down the +z-axis, has its x- and y-axes rotated anti-clockwise through an angle of 2.54 o compared to the laboratory system. Return to the Aerofoil continuum node and select the Initial Conditions > Velocity node. In the Properties window, change the Coordinate System property to Laboratory -> Cartesian 1. Select the Velocity > Constant node. In the Properties window, change the Value to [ , 0.0, 0.0] m/s. To specify the initial temperature: Select the Static Temperature > Constant node. Version

104 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7369 In the Properties window change the Value to 291 K. The default values for the remaining initial conditions are suitable for this problem. Save the simulation. Setting Boundary Conditions and Values The geometry used for this tutorial has only two boundaries: A wall boundary representing the surface of the airfoil. A free-stream boundary at the external edge of the solution domain. Open the Regions node, then right-click the Default_Fluid 2D node and select Rename... Enter the name Fluid and click OK. Select the Fluid > Boundaries > freestream > Physics Conditions > Flow Direction Specification node. In the Properties window, make sure that the Method property is set to Components. Version

105 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7370 Select the Physics Values > Flow Direction node. As for the initial velocity, change the Coordinate System property to Laboratory -> Cartesian 1. Select the Mach Number > Constant node. Version

106 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7371 Change the Value property to Select the Static Temperature > Constant node. Change the Value property to 291 K. All other conditions for the free-stream boundary and the default wall boundary conditions are suitable for this problem. Save the simulation. Setting Solver Parameters The simplicity of this problem allows a rapidly converging solution to be attained using a large Courant number. In problems involving more complex geometries or physics, attempting to shorten the run time in this way may cause the run to diverge. To increase the Courant number: Select the Solvers > Coupled Implicit node. In the Properties window, change the Courant Number to Save the simulation. Version

107 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7372 Visualizing and Initializing the Solution We will view the Mach number profile during the run to monitor the supersonic flow region above the airfoil. Start by creating a new scalar scene. Right-click on the Scenes node, and select New Scene > Scalar. The Scalar Scene 1 display will appear. Right-click on the scalar bar at the bottom of the display and select Mach Number > Lab Reference Frame from the pop-up menu. Initialize the run by clicking the Initialize Solution button in the toolbar, then use the middle mouse button to zoom in on the airfoil in the center Version

108 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7373 of the scalar scene. To change the style of the Mach number contours: Select the Scalar Scene 1 > Displayers > Scalar 1 node. In the Properties window, change the Contour Style property to Smooth Filled. Save the simulation. Plotting Graphs The lift and drag coefficients will be plotted to help in determining when the analysis has converged. Version

109 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7374 Right-click the Reports node and select New Report > Force Coefficient. A new report node named Force Coefficient 1 will be created. Rename this node Drag Coefficient then enter the information shown below in the Properties window. Right-click the Drag Coefficient node and select Create Monitor and Plot from Report. A new plot node will appear named Drag Coefficient Monitor Plot. Version

110 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7375 Double-click on the Drag Coefficient Monitor Plot node to display the empty plot in the Graphics window. Repeat the steps described above to create and display a plot for the lift coefficient. All settings should be the same as for the drag coefficient except that the report node should be renamed Lift Coefficient and its Direction property should be set to [ , , 0.0]. Experimental data for the pressure coefficient on the airfoil are provided in file aero_exp.xy in the doc/tutorials/aerofoil directory. These will be plotted on a graph alongside the results of the analysis. To plot the experimental data: Right-click the Tools > Tables node and then select New Table > File... Locate and open file aero_exp.xy Right-click the Plots node and select New Plot > X-Y. Open the XY Plot 1 node, then right-click the Tabular node and select Version

111 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7376 New Tabular Data Set. A new node named tabular will appear within the Tabular node. In the Properties window, select aero_exp for the Table property. Make sure that the X Column and Y Column properties are filled as shown below. A graph of the experimental data will appear in XY Plot 1. To add the numerical data to the same graph: Select the XY Plot 1 node. In the Properties window, click on the Parts property and select Fluid: wall in the Select Objects dialog. Version

112 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7377 Select the Y Types > Y Type 1 > Scalar node. In the Properties window, select Pressure Coefficient for the Scalar property. The initial pressure coefficient is shown in the XY Plot 1 as being zero everywhere. The pressure coefficient requires specification of a reference pressure and a reference velocity. Select the Tools > Field Functions > Pressure Coefficient node. In the Properties window, enter a Reference Density of kg/m 3 and a Reference Velocity of m/s, as shown in the following screenshot. Version

113 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7378 The usual convention in aerodynamics problems is to reverse the y-axis orientation in pressure coefficient plots. Select the XY Plot 1 > Axes node. Click on the Axis Orientation property and select the option shown below. The setup is now complete. Save the simulation. Version

114 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7379 Running the Simulation To run the simulation, click the (Run) button in the top toolbar. If you do not see this button, use the Solution > Run menu item. The Residuals display will be created automatically and will show the progress being made by the solver. You may observe the run progress by selecting one of the tabs at the top of the Graphics window. The Scalar Scene 1 display after about 50 iterations is shown below. During the run, it is possible to stop the analysis by clicking the (Stop) button in the toolbar. If you do halt the simulation, it can be continued again later by clicking the (Run) button. If left alone, the simulation will continue until 1000 iterations have been completed. Once this stage is reached, check that the solution has converged by examining the lift and drag coefficient plots. Select the Plots > Lift Coefficient Monitor Plot > Axes > Y Axis > Labels node. In the Properties window, change the Minimum and Maximum properties to 0.2 and 0.8, respectively, to zoom in on the relevant part of the graph. Version

115 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7380 Double-click the Lift Coefficient Monitor Plot node to display the results in the Graphics window. Version

116 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7381 Similarly, display the drag coefficient plot and adjust its y-axis scale. Both monitors have reached constant values so it is reasonable to conclude that the solution has converged. Save the simulation. Version

117 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7382 Visualizing the Results The Scalar Scene 1 display shows the Mach number profile at the end of the run. The profile shows the transonic flow around the airfoil, including the shock wave produced above it. Version

118 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7383 Validating the Results A graph showing the comparison between numerical and experimental data can be viewed by selecting the XY Plot 1 tab, as shown below with the X axis scale adjusted. Other than the shock position, which is in error as a result of the mesh coarseness and choice of turbulence model, the numerical pressure coefficients compare well with the experimental data. The lift coefficient determined experimentally for this case is [272]. To see the value calculated by STAR-CCM+: Version

119 STAR-CCM+ User Guide Transonic Flow over an Airfoil 7384 Right-click the Reports > Lift Coefficient node and then select Run Report. In the Output window, a tab named Lift Coefficient Report will display the relevant report and show a lift coefficient of 0.732, which is within 2% of the experimental value. Similarly, the drag coefficient report will give a value of , which also compares well to the experimental value of Summary This STAR-CCM+ tutorial introduced the following features: Defining models for compressible flow problems. Defining the material properties required for the selected models. Setting solver parameters for a steady-state run. Plotting graphs comparing results with experimental data. Initializing and running the solver to a specified stopping criterion. Analyzing the results using the built-in visualization facilities. Airfoil Tutorial Bibliography [272] Cook, P.H., M.A. McDonald, M.C.P. Firmin Aerofoil RAE Pressure Distributions, and Boundary Layer and Wake Measurements Experimental Data Base for Computer Program Assessment, AGARD Report AR 138, 1979 Version