FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Vortex Flow

Time dependent decaying flow for standing vortices with the following analytical solution to the Navier-Stokes equations

\[ \left\{\begin{array}{l} u = -cos(kx) sin(ky) e^{-2\nu k^2t} \\ v = sin(kx) cos(ky) e^{-2\nu k^2 t} \\ p = -\frac{1}{4}(cos(2kx)+cos(2ky)) e^{-4\nu k^2 t} \end{array}\right. \]

The two-dimensional flow problem is solved for a unit square with *k = 2π* and the exact solution as boundary and initial conditions.

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Fluid Dynamics** > **Vortex Flow** 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. - 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
`0.05`

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. - 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 viscosity, vortex period, and reference solutions.

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

nu | 0.0.1 |

k | 2*pi |

u_ref | -cos(k*x)*sin(k*y)*exp(-2*nu*k^2*t) |

v_ref | sin(k*x)*cos(k*y)*exp(-2*nu*k^2*t) |

p_ref | -1/4*(cos(2*k*x)+cos(2*k*y))*exp(-4*nu*k^2*t) |

Open the *Equation Settings* dialog box and enter `nu`

for the *viscosity* and the reference expressions as *initial conditions*

- Select
**Equation Settings...**from the*Equation*menu. - Enter
`nu`

into the*Viscosity*edit field. - Enter
`u_ref`

into the*Initial condition for u*edit field. - Enter
`v_ref`

into the*Initial condition for v*edit field. - Enter
`p_ref`

into the*Initial condition for p*edit field. - Press
**OK**to finish the equation and subdomain settings specification. - Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button.

Prescribe the reference velocities on all boundaries using the *Inlet/velocity* boundary condition.

- Select
**1**,**2**,**3**, and**4**in the*Boundaries*list box. - Select
**Inlet/velocity**from the*Navier-Stokes Equations*drop-down menu. - Enter
`u_ref`

into the*Velocity in x-direction*edit field. - Enter
`v_ref`

into the*Velocity in y-direction*edit field. - Press
**OK**to finish the boundary condition specification.

Also prescribe the reference pressure on all four points. Note that since no outflow is present in this model, a reference point with pressure *p = 0* has already been prescribed. This is necessary to ensure convergence and a unique pressure for stationary problems without any outflow boundary conditions.

- Select
**Add Point Constraints...**from the*Boundary*menu. - Enter
`p_ref`

into the four edit fields for the corners corresponding to the pressure. - Press
**OK**to finish and close the dialog box. - Switch to
**Solve**mode by clicking on the corresponding*Mode Toolbar*button. - Press the
**Settings***Toolbar*button. - Select
**Time-Dependent**from the*Solution and solver type*drop-down menu. - Enter
`0.01`

into the*Time step size*edit field. - Enter
`0.1`

into the*Duration of time-dependent simulation (maximum time)*edit field. - Press the
**Solve**button.

Plot the velocity field as arrows and pressure as contour plot to see the vortices of the flow field.

- Press the
**Plot Options***Toolbar*button. - Select the
**Contour Plot**check box. - Select
**Pressure**from the*Predefined contour plot expressions*drop-down menu. - Select the
**Arrow Plot**check box. - Press
**Apply**to plot and visualize the selected postprocessing options.

By plotting and visualizing the difference between the computed and reference variables, the overall accuracy of the simulation can be estimated.

- Enter
`u-u_ref`

into the*User defined surface plot expression*edit field. - Press
**OK**to plot and visualize the selected postprocessing options.

The *vortex flow* 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.