FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Laminar Channel Flow

Stationary and incompressible laminar Poiseuille flow in a two- dimensional rectangular channel. With a constant inflow profile *u(0,y) = U _{max}* and fixed no-slip walls, a fully developed laminar parabolic profile,

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Fluid Dynamics** > **Laminar Channel 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
`2.5`

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

into the*y*edit field._{min} - Enter
`0.5`

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.

The default grid may be too coarse ensure an accurate solution. Decrease the grid size to generate a finer grid that better can resolve the curved boundary.

- Enter
`0.04`

into the*Grid Size*edit field. Press the

**Generate**button to call the automatic 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`0.001`

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 it is up to the user to use consistent units for geometry dimensions, material, equation, and boundary coefficients.

A convenient way to to define and store coefficients, variables, and expressions is using the *Model Constants and Expressions* functionality. The defined expressions can then be used in point, equation, boundary coefficients, as well as postprocessing expressions, and can easily be changed and updated in a single place.

- In order to define an expression for the reference velocity profile at the outflow, press the
**Constants***Toolbar*button, or select the corresponding entry from the*Equation*menu, and enter the following variables in the*Model Constants and Expressions*dialog box.

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

h | 0.5 |

l | 2.5 |

umax | 0.3 |

uref | 4*umax*(y*(h-y))/h^2 |

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

Boundary conditions are defined in *Boundary Mode* and describes how the model interacts with the external environment.

- Select
**1**and**3**in the*Boundaries*list box. - Select
**Wall/no-slip**from the*Navier-Stokes Equations*drop-down menu. - Select
**4**in the*Boundaries*list box. - Select
**Inlet/velocity**from the*Navier-Stokes Equations*drop-down menu. Enter

`2/3*umax`

into the*Velocity in x-direction*edit field.- Select
**2**in the*Boundaries*list box. - Select
**Outflow/pressure**from the*Navier-Stokes Equations*drop-down menu. - 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. One can clearly see the the maximum velocity is about *0.3* along the center line as is expected. Clicking anywhere in a surface plot also directly evaluates the surface expression at the location.

One can also visualize the error between the analytical solution and the computed one. To do this, open the postprocessing settings dialog box by clicking on the

**Plot Options***Toolbar*button, and enter the expression`abs(sqrt((uref)^2)-sqrt(u^2+v^2))*(x>3/4*l)`

in the*Surface Plot*expression edit field. Press**OK**or*Apply*.

The visualization shows the error towards the outlet, and has an acceptable magnitude around *5·10 ^{-3}*.

The *laminar channel 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.