FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Flow Over a Backwards Facing Step

Flow over a backwards facing step is a classic computational fluid dynamics test problem which is used extensively for validation of simulation codes. The test problem essentially consists of studying how a fully developed flow profile reacts to a sudden expansion in a channel. The expansion will cause a break in the flow and a recirculation or separation zone will form. To measure and compare results the resulting length of the recirculation or separation zone is used.

The stationary incompressible Navier-Stokes equations are applied with simulation parameters corresponding to a Reynolds number, *Re = 389*. The inlet velocity is given as *u _{inlet} = 4u_{max} (y-h_{step})(1-y)/h_{inlet}^{2}* where

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Fluid Dynamics** > **Flow Over a Backwards Facing Step** 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
**2D**radio button. Select the

**Navier-Stokes 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.

The backwards facing step geometry is generated by creating a larger rectangle for the channel from which a smaller section is removed to create the expansion step. Alternatively, the geometry could also be created by joining two rectangle slices, or directly using the *Polygon* tool.

First create the outer rectangle with the scaled dimensions *1/0.0101* by *1*, with the expansion step located at *x = 0*.

- 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
`-0.02/0.0101`

into the*x*edit field._{min} - Enter
`0.08/0.0101`

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

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

`1`

into the*y*edit field._{max}Press

**OK**to finish and close the dialog box.

Then create and subtract a second smaller rectangle with dimensions *1.9802* by *0.0049/0.0101* to create the step.

- 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
**R2**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
`-0.02/0.0101`

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

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

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

`0.0049/0.0101`

into the*y*edit field._{max}Press

**OK**to finish and close the dialog box.- Select
**R1**and**R2**in the geometry object*Selection*list box. Press the

**- / Subtract geometry objects***Toolbar*button.- Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button.

The default grid may be too coarse ensure an accurate solution. Decreasing the grid size and generating a finer grid gives a more accurate approximation.

- Enter
`0.1`

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. In the

*Equation Settings*dialog box that automatically opens, set the density to`1`

and viscosity to`u_max*2/3*h_channel/Re`

in the corresponding edit fields. In order to start with a better initial guess, set the initial condition for the x-velocity*u0*to`u_inlet*(y>h_inlet)`

. The other coefficients can be left to their default values. Press**OK**to finish and close the dialog box.- 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 channel, fluid parameters, and inlet velocity expression. Press*Enter*after the last expression or use the**Add Row**button to expand the expression list.

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

h_step | 0.0049/0.0101 |

h_channel | 1 |

h_inlet | h_channel-h_step |

u_max | 1 |

Re | 389 |

u_inlet | 4*u_max*(y-h_step)*(1-y)/h_inlet^2 |

- Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button. In the

*Boundary Settings*dialog box, first select all boundaries except for the right outflow and left inflow (numbers**1**,**3**, and**5-8**) in the left hand side*Boundaries*selection list box, and select the**Wall/no-slip**boundary condition from the drop-down menu.Select the leftmost boundary (number

**4**) and choose the**Inlet/velocity**boundary condition from the drop-down menu. When using the default built-in solver enter the previously defined`u_inlet`

expression in the edit field for the x-velocity coefficient*u0*.Finally, select the right outflow boundary (number

**2**) and select the**Outflow/pressure**boundary condition from the drop-down menu (alternatively one can prescribe the**Neutral outflow/stress boundary**condition). Finish by clicking the**OK**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. In the Solver Settings dialog box increase the

*Maximum non-linear iterations*to`75`

in the*Non-Linear Solver Settings*section 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. - Press the
**Solve**button.

After the problem has been solved FEATool will automatically switch to postprocessing mode and display the computed velocity field.

To see the recirculation zone clearer, open the *Postprocessing* settings dialog box and enter the expression for the normalized recirculation zone length `x/h_step*(u<0)*(y<h_step)`

in the *Surface Plot* expression edit field (Note that switch type expressions such as *a<b* evaluate to either *0* or *1*, and are used here to limit the plot to the lower half region for which the *u* velocity is negative). The *Arrow Plot* option can also be used to help visualize the flow field.

- Press the
**Plot Options***Toolbar*button. - Enter
`x/h_step*(u<0)*(y<h_step)`

into the*User defined surface plot expression*edit field. Press

**OK**to plot and visualize the selected postprocessing options.

The resulting plot shows a recirculation zone length of about *7.25* length units which is in the same range as the reference length of *7.93*.

The *flow over a backwards facing step* 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] Gresho PM, Sani RL. *Incompressible Flow and the Finite Element Method*. Volume 1 & 2, John Wiley & Sons, New York, 2000.

[2] Rose A, Simpson B. *Laminar, Constant-Temperature Flow Over a Backward Facing Step*. 1st NAFEMS Workbook of CFD Examples, Glasgow, UK, 2000.