FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Flow in Driven Cavity

Stationary and laminar incompressible flow in a square cavity (Reynolds number, *Re = 1000*). The top of the cavity is prescribed a tangential velocity while the sides and bottom are defined as no-slip zero velocity walls.

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Fluid Dynamics** > **Flow in Driven Cavity** 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.

First create a unit square for the geometry.

- 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
`0`

into the*x*edit field._{min} - Enter
`1`

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. - Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button. - Enter
`0.02`

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. Equation and material coefficients are be specified in

*Equation/Subdomain*mode. In the*Equation Settings*dialog box that automatically opens, enter`1`

for the fluid*Density*and`umax/l/R`

for the*Viscosity*. The other coefficients can be left to their default values. Press**OK**to finish the equation and subdomain settings specification.

Note that FEATool works with any unit system, and that the units here are non-dimensionalized.

- Press the
**Constants***Toolbar*button, or select the corresponding entry from the*Equation*menu, and enter the variables for the velocity*umax*, length*l*, and Reynolds number*Re*in the*Model Constants and Expressions*dialog box.

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

umax | 1 |

l | 1 |

Re | 1000 |

Boundary conditions consist of no-slip zero velocity conditions on all walls except for the top on which a constant x-velocity *umax* is prescribed.

- Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button. - Select
**4**in the*Boundaries*list box. - Select
**1**,**2**,**3**, and**4**in the*Boundaries*list box. - Select
**Wall/no-slip**from the*Navier-Stokes Equations*drop-down menu. - Select
**3**in the*Boundaries*list box. - Select
**Inlet/velocity**from the*Navier-Stokes Equations*drop-down menu. Enter

`umax`

into the*Velocity in x-direction*edit field.- Press
**OK**to finish the boundary condition specification. Now that the problem is fully specified, press the

**Solve***Mode Toolbar*button to switch to solve mode. Then press the**=***Tool*button to call the solver with the default solver settings.

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

- Press the
**Plot Options***Toolbar*button. - Select
**Vorticity**from the*Predefined surface plot expressions*drop-down menu. - Select the
**Contour Plot**check box. - Enter
`30`

into the*Number or specified vector of contour levels to plot*edit field. - Select the
**Arrow Plot**check box. Press

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

To evaluate the accuracy of the solution the vorticity at (0.53, 0.56) is evaluated. Either click directly at this point or use the *Point/Line Evaluation* functionality.

- Select
**Point/Line Evaluation...**from the*Post*menu. - Select
**Vorticity**from the*Evaluation Expression*drop-down menu. - Enter
`0.53`

into the*Evaluation coordinates in x-direction*edit field. Enter

`0.564`

into the*Evaluation coordinates in y-direction*edit field.Press

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

The computed vorticity at the evaluated point is -1.73 which is quite close to the reference value of -2.068, to achieve a better approximation a finer grid and higher order discretization would be necessary.

The *flow in driven cavity* 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] Botella O, Peyret R. *Benchmark spectral results on the lid-driven cavity flow*. Computers and Fluids 27(4):421-433, 1998.

[2] Erturk E, Corke TC, Gokcol C. *Numerical solutions of 2-D steady incompressible driven cavity flow at high Reynolds numbers*. Int- ernational Journal for Numerical Methods in Fluids 37(6):633-655, 2005.

[3] Nishida H, Satofuka N. *Higher-order solutions of square driven cavity flow using a variable-order multi-grid method*. International Journal for Numerical Methods in Engineering 34(2):637-653, 1992.

[4] Schreiber R, Keller HB. *Driven cavity flows by efficient numerical techniques*. Journal of Computational Physics 49(2):310-333, 1983.