Chapter 10: Supersonic Flow Over a Wing

This tutorial includes:

 

10.1. Tutorial Features

In this tutorial you will learn about:

  • Setting up a supersonic flow simulation.

  • Using the Shear Stress Transport turbulence model to accurately resolve flow around a wing surface.

  • Defining a custom vector to display pressure distribution.

Component

Feature

Details

CFX-Pre

User Mode

General mode

Analysis Type

Steady State

Fluid Type

Air Ideal Gas

Domain Type

Single Domain

Turbulence Model

Shear Stress Transport

Heat Transfer

Total Energy

Boundary Conditions

Inlet (Supersonic)

Outlet (Supersonic)

Symmetry Plane

Wall: No-Slip

Wall: Adiabatic

Wall: Free-Slip

Domain Interfaces

Fluid-Fluid (No Frame Change)

Timestep

Maximum Timescale

CFD-Post

Plots

Contour

Vector

Other

Variable Details View

 

10.2. Overview of the Problem to Solve

This example demonstrates the use of CFX in simulating supersonic flow over a symmetric NACA0012 airfoil at 0° angle of attack. A 2D section of the wing is modeled. A 2D hexahedral mesh is provided that you will import into CFX-Pre.

The environment is 300 K air at 1 atmosphere that passes the wing at 600 m/s. The turbulence intensity is low (.01) with an eddy length scale of .02 meters.

A mesh is provided. You will create a domain that contains three regions that will be connected by fluid-fluid interfaces. To solve the simulation, you will start with a conservative time scale that gradually increases towards the fluid residence time as the residuals decrease.

If this is the first tutorial you are working with, it is important to review the following topics before beginning:

 

10.3. Preparing the Working Directory

  1. Create a working directory.

    Ansys CFX uses a working directory as the default location for loading and saving files for a particular session or project.

  2. Download the wing_sps.zip file here .

  3. Unzip wing_sps.zip to your working directory.

    Ensure that the following tutorial input file is in your working directory:

    • WingSPSMesh.out

  4. Set the working directory and start CFX-Pre.

    For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.

 

10.4. Defining the Case Using CFX-Pre

  1. In CFX-Pre, select File > New Case.

  2. Select General and click OK.

  3. Select File > Save Case As.

  4. Under File name, type WingSPS.

  5. Click Save.

 

10.4.1. Importing the Mesh

  1. Right-click Mesh and select Import Mesh > Other.

    The Import Mesh dialog box appears.

  2. Configure the following setting(s):

    Setting

    Value

    Files of type

    PATRAN Neutral (*out *neu)

    File name

    WingSPSMesh.out

    Options

    > Mesh Units

     

    m

  3. Click Open.

  4. To best orient the view, right-click a blank area in the viewer and select Predefined Camera > Isometric View (Y up) from the shortcut menu.

 

10.4.2. Creating the Domain

  1. Edit Case Options > General in the Outline tree view and ensure that Automatic Default Domain is turned on. A domain named Default Domain should now appear under the Simulation branch.

  2. Edit Default Domain and configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Location and Type

    > Location

     

    WING_Elements

    Fluid and Particle Definitions

    Fluid 1

    Fluid and Particle Definitions

    > Fluid 1

    > Material

     

     

    Air Ideal Gas

    Domain Models

    > Pressure

    > Reference Pressure [a]

     

     

    1 [atm]

    Fluid Models

    Heat Transfer

    > Option

     

    Total Energy [b]

    Turbulence

    > Option

     

    Shear Stress Transport

    1. When using an ideal gas, it is important to set an appropriate reference pressure because some properties depend on the absolute pressure level.

    2. The Total Energy model is appropriate for high-speed flows because it includes kinetic energy effects.

  3. Click OK.

 

10.4.3. Creating the Boundaries

 

10.4.3.1. Creating an Inlet Boundary

  1. Create a new boundary named Inlet.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Inlet

    Location

    INLET

    Boundary Details

    Flow Regime

    > Option

     

    Supersonic

    Mass And Momentum

    > Option

     

    Cart. Vel. & Pressure

    Mass And Momentum

    > Rel. Static Pres.

     

    0 [Pa]

    Mass And Momentum

    > U

     

    600 [m s^-1]

    Mass And Momentum

    > V

     

    0 [m s^-1]

    Mass And Momentum

    > W

     

    0 [m s^-1]

    Turbulence

    > Option

     

    Intensity and Length Scale

    Turbulence

    > Fractional Intensity

     

    0.01

    Turbulence

    > Eddy Length Scale

     

    0.02 [m]

    Heat Transfer

    > Static Temperature

     

    300 [K]

  3. Click OK.

 

10.4.3.2. Creating an Outlet Boundary

  1. Create a new boundary named Outlet.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Outlet

    Location

    OUTLET

    Boundary Details

    Flow Regime

    > Option

     

    Supersonic

  3. Click OK.

 

10.4.3.3. Creating the Symmetry Plane Boundaries

  1. Create a new boundary named SymP1.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Symmetry [a]

    Location

    SIDE1

    1. Symmetry, which can make a 3D problem into a 2D problem, can be used when geometry and mesh are invariant normal to the symmetry surface.

  3. Click OK.

  4. Create a new boundary named SymP2.

  5. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Symmetry

    Location

    SIDE2

  6. Click OK.

  7. Create a new boundary named Bottom.

  8. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Symmetry

    Location

    BOTTOM

  9. Click OK.

 

10.4.3.4. Creating a Free Slip Boundary

  1. Create a new boundary named Top.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Wall

    Location

    TOP

    Boundary Details

    Mass And Momentum

    > Option

     

    Free Slip Wall

  3. Click OK.

 

10.4.3.5. Creating a Wall Boundary

  1. Create a new boundary named WingSurface.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Wall

    Location

    WING_Nodes [a]

    1. If particular items do not appear in the drop-down list, click the Ellipsis   icon to see all available items.

  3. Click OK.

 

10.4.4. Creating Domain Interfaces

The imported mesh contains three regions that will be connected with domain interfaces.

  1. Create a new domain interface named Domain Interface 1.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Interface Type

    Fluid Fluid

    Interface Side 1

    > Region List

     

    Primitive 2D A

    Interface Side 2

    > Region List

     

    Primitive 2D, Primitive 2D B

  3. Click OK.

 

10.4.5. Setting Initial Values

For high-speed compressible flow, the CFX-Solver usually requires sensible initial conditions to be set for the velocity field.

  1. Click Global Initialization  .

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Global Settings

    Initial Conditions

    > Cartesian Velocity Components

    > Option

     

     

    Automatic with Value

    Initial Conditions

    > Cartesian Velocity Components

    > U

     

     

    600 [m s^-1]

    Initial Conditions

    > Cartesian Velocity Components

    > V

     

     

    0 [m s^-1]

    Initial Conditions

    > Cartesian Velocity Components

    > W

     

     

    0 [m s^-1]

    Initial Conditions

    > Temperature

    > Option

     

     

    Automatic with Value

    Initial Conditions

    > Temperature

    > Temperature

     

     

    300 [K]

  3. Click OK.

 

10.4.6. Setting the Solver Controls

The residence time for the fluid is the length of the domain divided by the speed of the fluid; using values from the problem specification, the result is approximately:

70 [m] / 600 [m s^-1] = 0.117 [s]

In the next step, you will set a maximum timescale, then the solver will start with a conservative time scale that gradually increases towards the fluid-residence time as the residuals decrease.

  1. Click Solver Control  .

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Convergence Control

    > Fluid Timescale Control

    > Maximum Timescale

     

     

    (Selected)

    Convergence Control

    > Fluid Timescale Control

    > Maximum Timescale

    > Maximum Timescale

     

     

     

    0.1 [s]

    Convergence Criteria

    > Residual Target

     

    1.0e-05

  3. Click OK.

 

10.4.7. Writing the CFX-Solver Input (.def) File

  1. Click Define Run  .

  2. Configure the following setting(s):

    Setting

    Value

    File name

    WingSPS.def

  3. Click Save.

    CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

  4. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

 

10.5. Obtaining the Solution Using CFX-Solver Manager

At this point, CFX-Solver Manager is running, and the Define Run dialog box is displayed, with the CFX-Solver input file set.

  1. Click Start Run.

  2. Select the check box next to Post-Process Results when the completion message appears at the end of the run.

  3. If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.

  4. Click OK.

 

10.6. Viewing the Results Using CFD-Post

The following topics will be discussed:

 

10.6.1. Displaying Mach Information

The first view configured shows that the bulk of the flow over the wing has a Mach Number of over 1.5.

  1. To best orient the view, select View From -Z by typing Shift +Z.

  2. Zoom in so the geometry fills the Viewer.

  3. Create a new contour named SymP2Mach.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Locations

    SymP2

    Variable

    Mach Number

    Range

    User Specified

    Min

    1

    Max

    2

    # of Contours

    21

  5. Click Apply.

  6. Clear the check box next to SymP2Mach.

 

10.6.2. Displaying Pressure Information

To display pressure information, create a contour plot that shows the pressure field:

  1. Create a new contour named SymP2Pressure.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Locations

    SymP2

    Variable

    Pressure

    Range

    Global

  3. Click Apply.

  4. Clear the check box next to SymP2Pressure.

 

10.6.3. Displaying Temperature Information

You can confirm that a significant energy loss occurs around the wing's leading edge by plotting temperature on SymP2.

  1. Create a new contour named SymP2Temperature.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Locations

    SymP2

    Variable

    Temperature

    Range

    Global

  3. Click Apply.

    The contour shows that the temperature at the wing's leading edge is approximately 180 K higher than the inlet temperature.

  4. Clear the check box next to SymP2Temperature.

 

10.6.4. Displaying Pressure With User Vectors

You can also create a user vector to show the pressure acting on the wing:

  1. Create a new variable named Variable 1.

  2. Configure the following setting(s):

    Name

    Setting

    Value

    Variable 1

    Vector

    (Selected)

    X Expression

    (Pressure+101325[Pa])*Normal X

    Y Expression

    (Pressure+101325[Pa])*Normal Y

    Z Expression

    (Pressure+101325[Pa])*Normal Z

  3. Click Apply.

  4. Create a new vector named Vector 1.

  5. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Locations

    WingSurface

    Variable

    Variable 1

    Symbol

    Symbol Size

    0.04

  6. Click Apply.

  7. Zoom in on the wing in order to see the created vector plot.