FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Thermo-Mechanical Bending of a Beam

Coupled thermo-mechanical multiphysics simulation of bending of a cantilever beam. The left side of the beam is fixed to a solid wall while the top side is subjected to an elevated external temperature through natural convection. The lower and left side are continuously held at the initial zero temperature. A two-dimensional plane stress approximation is also used, where the material is assumed to have a Poisson ratio of 0.25, modulus of elasticity 30 *GPa*, and convective heat transfer coefficient 10 *W/m/K*. All other coefficients are assumed to be equal to one. The temperature influx from the top boundary causes an increased internal temperature and also results in a downward deflection of the beam. After 10 seconds the top surface temperature has risen to 5 degrees and the beam has bent around 0.5-0.6 *mm* downwards.

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Multiphysics** > **Thermo-Mechanical Bending of a Beam** from the **File** menu. Or alternatively, follow the step-by-step instructions below.

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

Create a *1* by *5* rectangle to represent the beam geometry.

- Select
**Rectangle**from the*Geometry*menu. - Enter
`5`

into the*x*edit field._{max} Press

**OK**to finish and close the dialog box.- Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button. - Switch to
**Equation**mode by clicking on the corresponding*Mode Toolbar*button.

The material is assumed to have a Poisson ratio of *0.25*, modulus of elasticity *30 GPa*, and zero initial temperature. All other coefficients are assumed to be equal to one.

- Enter
`0.25`

into the*Poisson's ratio*edit field. - Enter
`30e9`

into the*Modulus of elasticity*edit field. - Enter
`12e-6`

into the*Thermal expansion coeffient*edit field. Enter

`T`

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

The left side of the beam is fixed to a solid wall while the top side is subjected to an elevated external temperature through natural convection with a heat transfer coefficient *10 W/m/K*.

- Select
**4**in the*Boundaries*list box. - Select the
**Fixed displacement, u**radio button. - Select the
**Fixed displacement, v**radio button. - Switch to the
**ht**tab. - Select
**1**and**4**in the*Boundaries*list box. - Select
**Temperature**from the*Heat Transfer*drop-down menu. - Select
**3**in the*Boundaries*list box. - Select
**Heat flux**from the*Heat Transfer*drop-down menu. - Enter
`10`

into the*Bulk temperature*edit field. Enter

`1`

into the*Heat transfer coefficient*edit field.- Press
**OK**to finish the boundary condition specification. - Switch to
**Solve**mode by clicking on the corresponding*Mode Toolbar*button.

Open the *Solver Settings* dialog box, set the *Time Step* to *1*, and *Simulation Time* to *10*.

- Press the
**Settings***Toolbar*button. - Select
**Time-Dependent**from the*Solution and solver type*drop-down menu. - Enter
`1`

into the*Time step size*edit field. Enter

`10`

into the*Duration of time-dependent simulation (maximum time)*edit field.- Press the
**Solve**button.

Plot and visualize the displacement in the y-direction and temperature.

After 10 seconds the top surface temperature has risen by *5* degrees and the beam has bent around *0.5-0.6 mm* downwards.

- Press the
**Plot Options***Toolbar*button. - Select
**y-displacement**from the*Predefined surface plot expressions*drop-down menu. - Select the
**Contour Plot**check box. - Select
**Temperature, T**from the*Predefined contour plot expressions*drop-down menu. - Select the
**Deformation Plot**check box. Enter

`1`

into the*Deformation scale factor*edit field.Press

**OK**to plot and visualize the selected postprocessing options.

The *thermo-mechanical bending of a beam* 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.