FEATool Multiphysics
v1.14
Finite Element Analysis Toolbox

This example illustrates the multiphysics capabilities of FEATool with a simple heat exchanger model featuring both free and forced convection. The model consists of a series of heated pipes around which there is a lower temperature fluid flowing. Two kinds of physics are considered, fluid flow which is modeled by the NavierStokes equations and heat transport modeled by a convection and conduction equation for the temperature field. The Boussinesq approximation models the temperature effects on the fluid, and the flow field is coupled to and transports the temperature field. In this way the system is fully two way coupled, the fluid to the temperature and temperature to the fluid.
Due to symmetry one can simplify the full geometry and only study a two dimensional slice between the heated pipes. The geometry will therefore consist of a 0.0075 by 0.05 m rectangle from which a half circle with radius 0.003 m centered at (0, 0.02) is removed. The mechanism for heating the pipes is not taken in consideration and are thus assumed to be at a fixed temperature of T_{h} = 330 K. A cooling fluid flows from the bottom to the top and has an inlet temperature of T_{c} = 300 K. The other fluid and material parameters can be found in the model tutorial.
How to set up and solve the heat exchanger example with the FEATool graphical user interface (GUI) is described in the following. Alternatively, this tutorial example can also be automatically run by selecting it from the File > Model Examples and Tutorials > Quickstart menu. Note that the CFDTool interface differ slightly from the FEATool Multiphysics instructions described in the following.
featool
on the command line from the installation directory when not using FEATool as an installed toolbox).In the New Model dialog box, select 2D for the Space Dimensions, and select NavierStokes Equations from the Select Physics dropdown menu. Leave the space dimension and dependent variable names to their defaults and press OK to finish the physics mode selection. (Note that for CFDTool the physics selection is done in the Equation settings dialog box.)
The geometry of the heat exchanger cross section can be created by first making a square and a circle, and then subtracting the circle from the square.
The geometry object properties must now be edited to set the correct size and position of the rectangle. To do this, click on the rectangle R1 to select it which highlights it in red. Then click on the Inspect/edit selected geometry object Toolbar button, and change the min and max coordinates of the rectangle so they span between 0
and 0.0075
in the xdirection, and 0
and 0.05
in the ydirection.
0.003
and (0, 0.02
) respectively.Enter 0.003
into the radius edit field and press OK to finish and close the dialog box.
To subtract the circle from the rectangle first select both geometry objects by clicking on them so both are highlighted in red, and then click on the  / Subtract geometry objects button. (Alternatively, if the circle is obscured by the rectangle they can be selected by holding the Ctrl key while clicking on the labels R1 and C1 in the Selection list box, or in this case simply pressing Ctrl + a to select all objects).
The default grid may be too coarse ensure an accurate solution. Decreasing the grid size and generating a finer grid can resolve curved boundaries better.
Enter 0.0005
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 enter the following coefficients, rho
for the density, ρ, mu
for the viscosity, µ, and alpha*g*rho*(TTc)
for the volume force in the ydirection, F_{y}. (Note that the Equation Settings dialog box may look different for CFDTool.)
A heat transfer physics must also be added. To access the multiphysics selection and add another physics mode press the plus + tab and select Heat Transfer from the Select Physics dropdown menu. Add the selection by pressing the Add Physics >>> button.
Note that each physics mode will have its own tab for Subdomain and Equation settings, and Boundary conditions. Moreover, 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.
In the ht Equation Settings tab, set the density to rho
, heat capacity to cp
, and thermal conductivity to k
, respectively. The convective velocities should be coupled from the NavierStokes equations physics mode, to do this enter u
and v
in the corresponding edit fields (as these are the default names of the dependent variables for the velocities). Press OK to finish with the equation coefficient specifications.
The Model Constants and Expressions functionality can be used to define and store convenient expressions which then are available in the point, equation, boundary coefficients, and as postprocessing expressions. Here it is used to define the load force.
Name  Expression 

rho  22 
mu  2.8e3 
alpha  0.26e3 
g  9.81 
Tc  300 
vin  40e2 
k  0.55 
cp  3.1e3 
Th  330 
Boundary conditions are defined in Boundary Mode and describes how the model interacts with the external environment.
First select the ns tab, which allows for specifying boundary conditions for the NavierStokes equations physics mode. Then select all vertical boundaries (here 2, 4, and 7), and choose Symmetry/slip from the drop down box. Switch to the heat transfer physics mode by selecting the ht tab and choose the Thermal insulation/symmetry boundary condition.
The selected boundaries will be highlighted in red.
vin
in the ydirection by using the Inlet/velocity condition. The Temperature should here be fixed to the low temperature Tc
Lastly, the boundaries on the cylinder (5 and 6) are walls and should be prescribed with Wall/noslip boundary conditions for the velocity. For the Temperature the constant high temperature Th
should be prescribed.
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.
From the resulting flow field one can see that fluid is accelerated when it passes between the cylinders. To visualize the temperature field, open the Plot Options and postprocessing settings dialog box and select to plot and visualize the Temperature, T as both surface and contour plots.
The temperature plot show that the fluid is heated around the hot cylinder and follows the flow upwards.
FEATool also allows for advanced postprocessing such as boundary integration. Integrate the expression (TTc)/w over the outflow boundary (where w = 0.0075 is the width of the domain) to find the change in the mean temperature.
Enter (TTc)/0.0075
into the Integration Expression edit field.
Press OK or Apply to calculate and show the result of the boundary integration.
From the result one can see that the mean temperature has risen by about 1.7 degrees.
The heat exchanger multiphysics 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_heat_exchanger1 script file), or GUI script (.fes) file.