Bump (2D)

- Solver: simpleFoam
- 2D flow over a bump at a Reynolds number of \( 3 \times 10^6 \) (L=1m)
- Based on the description provided by the NASA Turbulence Modelling Resource
- $FOAM_TUTORIALS/incompressible/simpleFoam/bump2D

- 2D structured mesh created using blockMesh
- bump described
\[ y(x) = \begin{cases} 0.05 [\sin(\pi \frac{x}{0.9}-\frac{\pi}{3})]^4, & 0.3 \le x \le 1.2, \\ 0 , & 0 \le x \lt 0.3 \, \text{and} \, 1.2 \lt x \le 1.5. \end{cases} \]

- this has been set in the
`blockMeshDict`

using a`codeStream`

- \( U \) based on a Mach number of 0.2. Mach number, \( Ma \), is defined as:
\[ Ma = \sqrt{\gamma R T} \]

where \( \gamma \) is the ratio of specific heats, \( R \) the gas constant and \( T \) the temperarture. Using values for air at 300K, the inflow velocity is given as:\[ U = 0.2 Ma = 0.2 \sqrt{1.4 \times 287 \times 300} = 69.44 m/s \]

- The laminar viscosity is derived from the Reynolds number, i.e.
\[ \nu_\infty = \frac{|\u| L}{Re} = \frac{69.44 \times 1}{3 \times 10^6} = 2.31 \times 10^{-5} m^2/s \]

Velocity: `U`

Patch | condition | value |
---|---|---|

Inlet | fixedValue | 69.44 m/s in x |

Outlet | zeroGradient | |

Bump | noSlip | |

Walls | symmetryPlane |

Pressure: `p`

Patch | condition | value |
---|---|---|

Inlet | zeroGradient | |

Outlet | fixedValue | 0 Pa (static) |

Bump | zeroGradient | |

Walls | symmetryPlane |

- turbulence model: Spalart Allmaras

Turbulence viscosity: `nut`

Patch | condition | value |
---|---|---|

Inlet | `calculated` | |

Outlet | `calculated` | |

Bump | `nutUSpaldingWallFunction` | |

Walls | `symmetryPlane` |

Modified turbulence viscosity: `nuTilda`

Patch | condition | value |
---|---|---|

Inlet | fixedValue | based on \( 3 \nu_\infty\) |

Outlet | zeroGradient | |

Bump | fixedValue | 0 |

Walls | symmetryPlane |

The NASA Turbulence Modelling Resource employs a code comparison to show that the FUN3D and CFL3D codes produce equivalent results for this case. OpenFOAM and CFL3D results are presented in the following series of images, showing that OpenFOAM results compare very favourably.

Would you like to suggest an improvement to this page? | Create an issue |

Copyright © 2018 OpenCFD Ltd.