FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Heat Exchanger

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 Navier-Stokes 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

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.

- Start MATLAB and launch FEATool by clicking on the corresponding icon in the MATLAB Add-Ons toolbar (or type
`featool`

on the command line from the installation directory when not using FEATool as an installed toolbox). - To start a new model click the
**New Model**toolbar button, or select*New Model...*from the*File*menu. In the

*New Model*dialog box, select**2D**for the*Space Dimensions*, and select**Navier-Stokes Equations**from the*Select Physics*drop-down menu. Leave the space dimension and dependent variable names to their defaults and press**OK**to finish the physics mode selection.

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.

- 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. 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 x-direction, and`0`

and`0.05`

in the y-direction.- Create an ellipse/circle and set its radius and center to
`0.003`

and (`0, 0.02`

) respectively. - Select
**Circle**from the*Geometry*menu. 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).- Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button.

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.- Switch to
**Equation**mode by clicking on the corresponding*Mode Toolbar*button. 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*(T-Tc)`

for the volume force in the y-direction,*F*._{y}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*drop-down 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 Navier-Stokes 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.

- 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. Press*Enter*after the last expression or use the**Add Row**button to expand the expression list.

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

rho | 22 |

mu | 2.8e-3 |

alpha | 0.26e-3 |

g | 9.81 |

Tc | 300 |

vin | 40e-2 |

k | 0.55 |

cp | 3.1e3 |

Th | 330 |

- 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.

First select the

**ns**tab, which allows for specifying boundary conditions for the Navier-Stokes 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.

- Continue with the top boundary (number
**3**) which is the outflow. Select**Outflow/pressure**for the Navier-Stokes physics mode and**Convective flux/outflow**for the heat transfer mode. - The bottom boundary (number
**1**) is the inflow and should be prescribed with the constant velocity`vin`

in the y-direction 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/no-slip**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 *(T-Tc)/w* over the outflow boundary (where *w = 0.0075* is the width of the domain) to find the change in the mean temperature.

- Select
**Boundary Integration...**from the*Post*menu. - Select
**3**in the*Boundaries*list box. Enter

`(T-Tc)/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 m-script text file, or GUI script (.fes) file.