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, u(y,L) = U_max4/h²y(h-y) is expected to develop at the outflow.

Tutorial

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. Note that the CFDTool interface differ slightly from the FEATool Multiphysics instructions described in the following.

1. To start a new model click the New Model toolbar button, or select New Model... from the File menu.
2. Select the 2D radio button.

3. Select the Navier-Stokes Equations physics mode from the Select Physics drop-down menu. (Note that for CFDTool the physics selection is done in the Equation settings dialog box.)

   
4. Press OK to finish the physics mode selection.
5. 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.
6. Select R1 in the geometry object Selection list box.
7. 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.
8. Enter 0 into the x_min edit field.
9. Enter 2.5 into the x_max edit field.
10. Enter 0 into the y_min edit field.
11. Enter 0.5 into the y_max edit field.

12. Press OK to finish and close the dialog box.

    
13. Switch to Grid mode by clicking on the corresponding Mode Toolbar button.

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

1. Enter 0.04 into the Grid Size edit field.

2. Press the Generate button to call the automatic grid generation algorithm.

   
3. Switch to Equation mode by clicking on the corresponding Mode Toolbar button.

4. Equation and material coefficients can 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 the Equation Settings dialog box may look different for CFDTool.)

   

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 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.

1. 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

1. 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.

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

5. Enter 2/3*umax into the Velocity in x-direction edit field.

   
6. Select 2 in the Boundaries list box.
7. Select Outflow/pressure from the Navier-Stokes Equations drop-down menu.
8. Press OK to finish the boundary condition specification.
9. 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 that 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.

1. 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 (available as the example ex_navierstokes1 script file), or GUI script (.fes) file.