FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Turbulent Flow Over a Backwards Facing Step (OpenFOAM)

Flow over backwards facing steps are classic computational fluid dynamics test problems, and are often used for validation of simulation codes. This test problem consists of studying how the flow field 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 validate the results the computed length of the recirculation zone is compared with the experimental results of Pitz and Daily [1].

In this example the stationary incompressible Navier-Stokes equations are used to model the fluid with simulation parameters corresponding to a Reynolds number, *Re = 18145*. The flow is therefore fully turbulent, whereby a turbulence model closure must also be applied. Here the standard k-epsilon turbulence model is used which is available with the external OpenFOAM CFD solver integration built into FEATool Multiphysics.

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Fluid Dynamics** > **Turbulent 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.

This example is simplified by assuming variations in the z-direction are negligible resulting in a planar 2D approximation.

Press the

**2D**radio button and select the**Navier-Stokes Equations**physics mode from the*Select Physics*drop-down menu.- Press
**OK**to finish the physics mode selection.

The backwards facing step geometry features a slightly tapered outflow region which is easiest to create by directly by specifying the polygon coordinates.

- Select
**Polygon**from the*Geometry*menu and enter the following data into the**Point coordinates**table.

1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | |
---|---|---|---|---|---|---|---|---|

x | -0.0206 | 0 | 0 | 0.206 | 0.29 | 0.29 | 0.206 | -0.0206 |

y | 0 | 0 | -0.0254 | -0.0254 | -0.0166 | 0.0166 | 0.0254 | 0.0254 |

Press

**OK**to finish and close the dialog box. The geometry should now look like the following.- Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button.

The default grid will be too coarse ensure an accurate solution. For turbulent flows it is particularly important to ensure a fine resolution near walls which have boundary layers with steep gradients in the solution.

Enter

`2e-3`

into the*Grid Size*edit field, and press the**Generate**button to call the automatic 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 ρ to`1.293`

and viscosity µ to`18.1e-6`

in the corresponding edit fields. Press**OK**to finish and close the dialog box.- 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**1-4**, and**6-7**) in the left hand side*Boundaries*selection list box, and choose the**Wall/no-slip**boundary condition from the*boundary condition*drop-down menu. Then select the leftmost boundary (number

**8**) in the*Boundaries*list box, and choose the**Inlet/velocity**boundary condition from the drop-down menu. Enter`10`

in the edit field for the x-velocity coefficient*u*._{0}Finally, select the right outflow boundary (number

**5**), and select the**Outflow/pressure**boundary condition from the drop-down menu. Finish the boundary condition specification by clicking the**OK**button.- Now that the problem has been defined, press the
**Solve***Mode Toolbar*button to switch to solve mode. As FEATool does not feature built-in turbulence models the OpenFOAM external CFD solver must be used to solve this flow problem (see the corresponding OpenFOAM solver section in the FEATool Multiphysics User's Guide on how to install OpenFOAM). Press the

**OpenFOAM***Toolbar*button to open the*OpenFOAM*Solver Settings dialog box. and set the*Stopping criteria/tolerance for initial residuals*to`1e-4`

.- Select the
**k-epsilon***Turbulence model*from the corresponding drop-down menu, and press the**Edit**button to open a dialog box to specify the turbulence inlet quantities.

The *k* and *epsilon* inlet values can either be estimated from a prescribed turbulence intensity and length scale, or as here prescribed directly if these quantities are known.

Enter

`0.375`

into the*Turbulent kinetic energy*edit field,`14.855`

into the*Turbulent dissipation rate*edit field, and press**OK**to finish and close the dialog box.Press the

**Solve**button to start the OpenFOAM solver. The view will then switch to show the convergence process for the solution variables. During the solution process one can switch between the convergence tab and the solver output log. The solver will stop when the residual for all of the variables is below*1e-4*or the maximum number of iterations has been reached.

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

To better visualize the recirculation zone, open the

*Postprocessing*settings dialog box and enter the expression for the normalized recirculation zone length`(u<0)*x/25.4e-3`

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 turned on to help visualize the flow field.

The resulting plot shows a recirculation zone length of about *6.25* length units based on step height which is quite close to the reference length of *6.4*.

The *turbulent 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] Pitz RW, Daily JW. Combustion in a Turbulent Mixing Layer Formed at a Rearward Facing Step. AIAA Journal 21, 1983.