# Flow reattachment: Flow over a backward-facing step¶

## Overview¶

The aim of this test case is to validate steady-state flow over a backward-facing step. The incompressible, turbulent case is validated with the experimental results of Driver and Seegmiller [1] as archived in the NASA Turbulence Modeling Resource [2]. The following parameters have been analysed:

- Velocity Profiles
- Coefficient of Pressure
- Reattachment Length

The geometry was meshed locally and a mesh upload to the platform was performed.

## Geometry¶

The geometry is constructed based on the reference case [1], as shown in Fig.1. The height of the step is \(h = 12.7\) cm, and the tunnel height is \(8h\). The origin is located at the base of the step. The face details have been given in Table 1.

Face(s) | Type |
---|---|

A | Inlet |

B+H | Symmetry |

C+D+E+G | Walls |

F | Outlet |

## Analysis type and Domain¶

The *blockMesh tool* was used to generate the mesh locally (see Fig.2. and Table 2.). A single-cell width was assigned in the z-direction to ensure a 2D mesh.

A typical property of the generated mesh is the \(y^+\) (“*y-plus*”) value, which is defined as the non-dimensionalized distance to the wall; it is given by \(y^+ = u^*y/\nu\). A \(y^+\) value of 1 would correspond to the upper limit of the laminar sub-layer.

Explicit resolution of the near-wall region: The first cell lies at most at the boundary of the laminar sub-layer and no further. Here, \(y^+\) value is 1 or below.Use of wall-functions to resolve the near-wall region: There is no need to place cells very close to the laminar sub-layer, and typically \(30 \leqslant y^+ \leqslant 300\).

A \(y^+\) value of 30 was used for the inflation layer. The \(k-\omega\) SST turbulence model was chosen, with wall functions for near-wall treatment of the flow.

**Tool Type** : OPENFOAM®

**Analysis Type** : simpleFoam

**Mesh and Element types** :

Mesh type | Number of volumes | Type |
---|---|---|

blockMesh |
\(5.5 \times 10^5\) | 2D hex |

## Simulation Setup¶

*Fluid:*

Kinematic Viscocity (\(\nu\)): \(1.4694 \times 10^{-5}\ m^2s^{-1}\)

The boundary conditions for the simulation are shown in Table 3.

*Boundary Conditions:*

Parameter | Inlet | Symmetry | Walls | Outlet |
---|---|---|---|---|

Velocity | \(44.2\ ms^{-1}\) | Symmetry | \(0.0\ ms^{-1}\) | Zero Gradient |

Pressure | Zero Gradient | Symmetry | Zero Gradient | \(0.0\) Pa |

\(k\) | \(5.336\ m^2s^{-2}\) | Symmetry | Wall Function | Zero Gradient |

\(\omega\) | \(182.399\ s^{-1}\) | Symmetry | Wall Function | Zero Gradient |

## Results¶

**Velocity Profiles**

Shown below in Figure 3 are comparisons of velocity profiles from SimScale simulation results with the reference [1] at different distances into the domain. All distances have been normalized with the step height \(h\), and the velocity is normalized with respect to the inlet velocity \(v_{in} = 44.2\ ms^{-1}\).

Fig.3. Vecloity profiles at different depths into the domain.

**Coefficient of Pressure**

Shown below in Figre 4 is the comparison of the cofficient of pressure \(C_p = \frac{P-P_{\infty}}{\frac{1}{2} \rho V_{\infty}^2}\) from SimScale simulation results with the reference [1] at the lower and upper walls.

Fig.4. Coefficient of Pressure at lower and upper walls

**Reattachment Length**

The reattachment length is the distance from the step at which the flow resumes in the positive flow direction all over the cross-section. The reattachment length was calculated to be \(6.82\ cm\), which lies within a \(12 \%\) error limit of the experimental value of \(7.74\ cm\) [2].

## References¶

[1] | (1, 2, 3, 4) Driver, D. M. and Seegmiller, H. L., “Features of Reattaching Turbulent Shear Layer in Divergent Channel Flow,” AIAA Journal, Vol. 23, No. 2, Feb 1985, pp. 163-171. |

[2] | (1, 2) Langley Research Center: Turbulence Modeling Resource - 2D Backward Facing Step |

## Disclaimer¶

This offering is not approved or endorsed by OpenCFD Limited, producer and distributor of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks. OPENFOAM® is a registered trade mark of OpenCFD Limited, producer and distributor of the OpenFOAM software.