FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Supersonic Flow Over an Obstacle

Steady inviscid flow over a cylindrical bump using the compressible Euler equations. The flow at the inlet is supersonic with *Ma = 1.4* resulting in a series of reflected shock waves as the flow hits the obstacle [1].

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Fluid Dynamics** > **Supersonic Flow over an Obstacle** from the **File** menu. Or alternatively, follow the step-by-step instructions below.

- To start a new model click the
**New Model**toolbar button, or select*New Model...*from the*File*menu. - Select the
**Euler Equations**physics mode from the*Select Physics*drop-down menu. - Press
**OK**to finish the physics mode selection. - To create a rectangle, first click on the
**Create square/rectangle***Toolbar*button. Then left click in the main plot axes window, and hold down the mouse button. Move the mouse pointer to draw the shape outline, and release the button to finalize the shape. - Select
**R1**in the geometry object*Selection*list box. - To modify and edit the selected rectangle, click on the
**Inspect/edit selected geometry object***Toolbar*button to open the*Edit Geometry Object*dialog box. - Enter
`-1`

into the*x*edit field._{min} - Enter
`4`

into the*x*edit field._{max} - Enter
`0`

into the*y*edit field._{min} - Enter
`2`

into the*y*edit field._{max} - Press
**OK**to finish and close the dialog box. - To create a circle or ellipse, first click on the
**Create circle/ellipse***Toolbar*button. Then left click in the main plot axes window, and hold down the mouse button. Move the mouse pointer to draw the shape outline, and release the button to finalize the shape. - Select
**E1**in the geometry object*Selection*list box. - To modify and edit the selected ellipse, click on the
**Inspect/edit selected geometry object***Toolbar*button to open the*Edit Geometry Object*dialog box. - Enter
`0.5 0.042-(0.5^2/0.042+0.042)/2`

into the*center*edit field. - Enter
`(0.5^2/0.042+0.042)/2`

into the*x*edit field._{radius} - Enter
`(0.5^2/0.042+0.042)/2`

into the*y*edit field._{radius} - Press
**OK**to finish and close the dialog box. - Select
**R1**and**E1**in the geometry object*Selection*list box. - Select
**Combine Objects...**from the*Geometry*menu. - Enter
`R1 - E1`

into the*Geometry Formula*edit field. - Press
**OK**to finish and close the dialog box. - Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button. - Enter
`0.05`

into the*Grid Size*edit field. - Press the
**Generate**button to call the grid generation algorithm. - Switch to
**Equation**mode by clicking on the corresponding*Mode Toolbar*button. - Enter
`rho0`

into the*Initial condition for rho*edit field. - Enter
`u0`

into the*Initial condition for u*edit field. - Enter
`v0`

into the*Initial condition for v*edit field. - Enter
`p0`

into the*Initial condition for p*edit field. - Press
**OK**to finish the equation and subdomain settings specification. - Press the
**Constants***Toolbar*button, or select the corresponding entry from the*Equation*menu, to open the*Model Constants and Expressions*dialog box. Enter the following expressions for the fluid parameters, and inlet velocity.

Name | Expression |
---|---|

Ma | 1.4 |

rho0 | 1 |

p0 | 1 |

u0 | Ma*sqrt(1.4*p0/rho0) |

v0 | 0 |

- Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button. - Select
**4**in the*Boundaries*list box. - Select
**Inlet/outlet**from the*Euler Equations*drop-down menu. - Enter
`rho0`

into the*Density*edit field. - Enter
`u0`

into the*Velocity in x-direction*edit field. - Enter
`v0`

into the*Velocity in y-direction*edit field. - Enter
`p0`

into the*Pressure*edit field. - Select
**2**in the*Boundaries*list box. - Select
**Neutral/no stress boundary/outlet**from the*Euler Equations*drop-down menu. - Press
**OK**to finish the boundary condition specification. - Switch to
**Solve**mode by clicking on the corresponding*Mode Toolbar*button. - Now that the problem has been defined, press the
**Solve***Mode Toolbar*button to switch to solve mode, and press the**Settings**button to open the*Solver Settings*dialog box. - Press the
**Settings***Toolbar*button. - In the
*Non-Linear Solver Settings*section of the*Solver Settings*dialog box increase the*Maximum non-linear iterations*to`50`

, and decrease the*Non-linear relaxation parameter*to`0.9`

, to allow for the non-linear problem to converge. - To start the solver with the chosen settings press the
**Solve**button, or press**OK**and then the**=***Toolbar*button.

After the problem has been solved FEATool will automatically switch to postprocessing mode and here display the magnitude of the computed velocity field where the shock pattern can easily be seen. Plot the mach number and verify that the minimum and maximum span between *Ma = 1* and *1.8*.

- Press the
**Plot Options***Toolbar*button. - Select
**Mach number**from the*Predefined surface plot expressions*drop-down menu. - Press
**OK**to plot and visualize the selected postprocessing options.

The *supersonic flow over an obstacle* fluid dynamics model has now been completed and can be saved as a binary (.fea) model file, or exported as a programmable MATLAB m-script text file, or GUI script (.fes) file.

[1] Lynn JF, van Leer B, Lee D. *Multigrid solution of the euler equations with local preconditioning*. In Fifteenth International Conference on Numerical Methods in Fluid Dynamics, Lecture Notes in Physics, vol 490, Springer, 1997.