FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Heat Induced Stress in a Brake Disc

This multiphysics model examines temperature and heat induced stresses for one braking cycle in a brake disc assembly, and involves coupling of the stress-strain and heat transfer physics modes. The braking process consists of applying a brake pad to the front part of the disc which induces heat through friction, and results in build up of stresses and strains in the brake disc. Both rotational and axial symmetry is used to reduce the computational cost. Simulations have been performed with the geometry and material parameters given in the reference [1] resulting in the final temperature and stress fields shown in the following figures.

The resulting temperature and stress curves on the disk surface at various times agree well with the results computed with the Nastran FEA software [1].

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Multiphysics** > **Heat Induced Stress in a Brake Disc** from the **File** menu.

- To start a new model click the
**New Model**toolbar button, or select*New Model...*from the*File*menu. - Select the
**Axi 2D**radio button. - Select the
**Axisymmetric Stress-Strain**physics mode from the*Select Physics*drop-down menu. - Press
**OK**to finish the physics mode selection.

The geometry only includes the cross section of the brake disc, and not the brake pad. Although this could be modeled with a single rectangle, the brake pad only touches part of the disc, so two rectangles are used to split the boundary into sections.

- Select
**Rectangle**from the*Geometry*menu. - Enter
`66e-3`

into the*x*edit field._{min} - Enter
`75.5e-3`

into the*x*edit field._{max} - Enter
`5.5e-3`

into the*y*edit field._{max} - Press
**OK**to finish and close the dialog box. - Select
**Rectangle**from the*Geometry*menu. - Enter
`75.5e-3`

into the*x*edit field._{min} - Enter
`113.5e-3`

into the*x*edit field._{max} - Enter
`5.5e-3`

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. - Enter
`0.0005`

into the*Grid Size*edit field. - Press the
**Generate**button to call the grid generation algorithm. - Switch to
**Equation**mode by clicking on the corresponding*Mode Toolbar*button.

The material parameters are taken from the reference assuming the brake disc is made of cast iron. Make sure that the material parameters are specified in both subdomain halves of the disc.

- Select
**1**and**2**in the*Subdomains*list box. - Enter
`0.29`

into the*Poisson's ratio*edit field. - Enter
`99.97e9`

into the*Modulus of elasticity*edit field. - Enter
`7100`

into the*Density*edit field. - Enter
`1.08e-5`

into the*Thermal expansion coeffient*edit field. - Enter
`T-(20+273.15)`

into the*Temperature*edit field. - Switch to the
**+**tab. - Select the
**Heat Transfer**physics mode from the*Select Physics*drop-down menu. - Press the
**Add Physics >>>**button. - Enter
`7100`

into the*Density*edit field. - Enter
`51/1.44e-5/7100`

into the*Heat capacity*edit field. - Enter
`51`

into the*Thermal conductivity*edit field. - Press
**OK**to finish the equation and subdomain settings specification. - Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button.

Symmetry with zero normal displacement is assumed at the lower *z = 0* boundaries.

- Select
**1**and**4**in the*Boundaries*list box. - Select the
**Fixed displacement, w**radio button. - Switch to the
**ht**tab.

The brake force is applied to the upper right section of the disc which magnitude is calculated as a function of the material of the disc and pad with a friction factor. See the reference for more details.

- Select
**6**in the*Boundaries*list box. - Select
**Heat flux**from the*Heat Transfer*drop-down menu. - Enter
`7109581.6204*r*(1-t/3.96)`

into the*Inward heat flux*edit field. - Press
**OK**to finish the boundary condition specification. - Switch to
**Solve**mode by clicking on the corresponding*Mode Toolbar*button. - Press the
**Settings***Toolbar*button.

Select *Time-Dependent* analysis with a simulation time of *3.96* seconds, and also set the initial temperature to *20 °C*.

- Select
**Time-Dependent**from the*Solution and solver type*drop-down menu. - Press the
**Expression**button. - Enter
`20+273.15`

into the*Initial condition for T in subdomain 1*edit field. - Enter
`20+273.15`

into the*Initial condition for T in subdomain 2*edit field. - Press
**OK**to finish and close the dialog box. - Enter
`3.96`

into the*Duration of time-dependent simulation (maximum time)*edit field. - Enter
`3.96/50`

into the*Time step size*edit field. - Press the
**Solve**button.

After the simulation has completed, inspect the stress and temperature distributions at different times. Especially for the early times it is very clear that both the temperature and stress are located at the interface between disc and pad, and later spreads throughout the disc.

- Press the
**Plot Options***Toolbar*button. - Select the
**Contour Plot**check box. - Press
**Apply**to plot and visualize the selected postprocessing options. - Enter
`T-273.15`

into the*User defined surface plot expression*edit field. - Enter
`T-273.15`

into the*User defined contour plot expression*edit field. - Press
**OK**to plot and visualize the selected postprocessing options.

The temperature has increased significantly at the final time, and should span between about *35* and *90* degrees.

The *heat induced stress in a brake disc* 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.

[1] Adamowicz A. *Axisymmetric FE Model to Analysis of Thermal Stresses in a Brake Disk*. Journal of Theoretical and Applied Mechanics, 53, 2, pp. 357-370, Warsaw, 2015.