FEATool Multiphysics
v1.14
Finite Element Analysis Toolbox

Simulation of stationary and incompressible turbulent flow between two parallel flat plates at Reynolds number 42800. A fully developed turbulent velocity profile is formed at the outflow boundary which can be compared to experimental results (Laufer, J. 1950).
This example uses both the builtin algebraic mixing length turbulence model, as well as shows how to implement custom userdefined modeling expressions.
This model is available as an automated tutorial by selecting Model Examples and Tutorials... > Fluid Dynamics > Turbulent Channel Flow from the File menu. Or alternatively, follow the stepbystep instructions below.
Select the NavierStokes Equations physics mode from the Select Physics dropdown menu.
The first step is to create a 1 by 5 rectangle to represent the fluid domain.
0
into the x_{min} edit field.5
into the x_{max} edit field.0.5
into the y_{min} edit field.0.5
into the y_{max} edit field.Press OK to finish and close the dialog box.
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 wall boundaries which are expected to feature sharp flow gradients.
Enter 0.03
into the Grid Size edit field and press the Generate button to call the automatic grid generation algorithm.
Equation and material coefficients are specified in Equation/Subdomain mode. In the Equation Settings dialog box that automatically opens when switching to Equation mode, enter 1
for the fluid Density, 1/Re
for the Viscosity, and uin
for the initial velocity in the xdirection u_{0}.
Note that FEATool works with any unit system, and in this model nondimensionalized units are used. It is up to the user to use consistent units for geometry dimensions, material, equation, and boundary coefficients.
Press the Turbulence Model button and select the Algebraic (mixing length model). The algebraic mixing length model is available with the builtin solvers while the more advanced kepsilon and omega turbulence models requires using the external OpenFOAM CFD solver.
A convenient way to to define and store coefficients, variables, and expressions is to use 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.
Enter the expressions for the Reynolds number, Re = 42800
which reciprocal is used to define the viscosity, and inlet velocity, uin = 1
used in both the initial and boundary conditions.
Boundary conditions are defined in Boundary mode and describes how the model interacts with the external environment. Switch to Boundary mode by clicking on the corresponding button.
First select (noslip) walls for the top and bottom boundaries.
The fluid flows from left to right, so select an outflow condition for the right boundary.
Finally, set the left boundary as an inflow with xvelocity uin
.
Enter uin
into the Velocity in xdirection edit field.
As turbulent flow problems are very nonlinear, decrease the nonlinear relaxation and tolerances to in the Solver Settings dialog box to help with convergence.
0.5
into the Nonlinear relaxation parameter (ratio of new to old solution to use) edit field.1e3
into the Nonlinear stopping criteria for solution defects edit field.Enter 1e4
into the Nonlinear stopping criteria for solution differences (changes) between iterations edit field.
After the problem has been solved FEATool will automatically switch to postprocessing mode and here display the magnitude of the computed velocity field.
Select the Contour Plot check box.
One can see the the maximum velocity is about 1.2 along the center and that the profile looks quite flat with sharp gradients along the walls. Clicking anywhere in a surface plot also directly evaluates the surface expression at the location.
The Point/Line Evaluation menu option can be used to plot a cross section which can show the shape of the turbulent velocity profile more clearly.
Select 2 in the Boundaries list box.
The resulting turbulent velocity profile agrees quite well with the experimental results of Laufer, J. (1950).
A custom expression for the turbulence viscosity will be defined and incorporated so that the total viscosity equals the molecular plus the turbulent viscosity.
Enter 1/Re + miu_t
into the Viscosity edit field.
The expression for the custom mixing length model is here defined as rho*l_mix^2*sqrt(uy^2+vx^2)
where the mixing length l_mix is defined as min(kappa*l_wall,0.09*l_char)
. The von Karman constant kappa is 0.41
, l_wall is the minimum distance from the walls, and l_char the characteristic length is taken as the maximum of l_wall.
Name  Expression 

kappa  0.41 
l_char  0.5 
l_wall  0.5abs(y) 
l_mix  min(kappa*l_wall,0.09*l_char) 
miu_t  rho_ns*l_mix^2*sqrt(uy^2+vx^2) 
The new solution with a custom expression for the turbulence model is very similar to both the builtin model and reference.
The turbulent 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 mscript text file (available as the example ex_navierstokes17 script file), or GUI script (.fes) file.