FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Stress Analysis of a Thick Plate

This is a benchmark and validation model for linear elasticity where an elliptical thick plate with a hole is subjected to a uniform pressure load of *10 ^{6} MPa* [1]. The outer surface is assumed to be constrained from expansion, in addition to the center line which is fixed in the z-direction. Symmetry is also utilized so that only a quarter of the geometry is modeled.

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Structural Mechanics** > **Stress Analysis of a Thick Plate** 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
**3D**radio button. - Select the
**Linear Elasticity**physics mode from the*Select Physics*drop-down menu. - Press
**OK**to finish the physics mode selection.

The elliptical shape can be constructed by first making two elliptical cylinders and subtracting the smaller inner one from the outer larger one.

- Press the
**Create cylinder***Toolbar*button. - Enter
`0 0 0`

into the*center*edit field. - Enter
`0.4`

into the*length*edit field. - Enter
`3`

into the*axis*edit field.

Approximation of curved boundaries can be improved by increasing the polygon resolution of the geometry object. This however will lead to an increased time and cost for performing geometry object operations.

- Enter
`32`

into the*resolution*edit field. - Press
**OK**to finish and close the dialog box.

An elliptical cylinder is easiest to create by scaling the unit cylinder.

- Select
**C1**in the geometry object*Selection*list box. - Press the
**Copy and/or transform selected geometry object***Toolbar*button. - Enter
`2 1 1`

into the*Space separated string of coordinate scaling factors*edit field. - Press
**OK**to finish and close the dialog box. - Press the
**Create cylinder***Toolbar*button. - Enter
`0 0 0`

into the*center*edit field. - Enter
`0.3`

into the*length*edit field. - Enter
`3`

into the*axis*edit field. - Enter
`32`

into the*resolution*edit field. - Press
**OK**to finish and close the dialog box. - Select
**C2**in the geometry object*Selection*list box. - Press the
**Copy and/or transform selected geometry object***Toolbar*button. - Enter
`3.25 2.75 1`

into the*Space separated string of coordinate scaling factors*edit field. - Press
**OK**to finish and close the dialog box.

To decrease the time and cost of the simulation, symmetry is utilized so that only a quarter of the geometry has to be modeled. To do this create a block overlapping one of the quarters, the use the *Intersect* tool to keep the overlapping objects.

- Press the
**Create cube/block***Toolbar*button. - Enter
`3.5`

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

into the*y*edit field._{max} - Enter
`-0.1`

into the*z*edit field._{min} - Enter
`0.5`

into the*z*edit field._{max} - Press
**OK**to finish and close the dialog box.

Subtract the outer from inner cylinder, while intersecting the resulting object with the block. Note that the edges and dimensions of the inner cylinder and block are larger than required instead of parallel and in-line, for more robust geometry operations.

- Select
**Combine Objects...**from the*Geometry*menu. - Enter
`TF2 - TF1 & B1`

into the*Geometry Formula*edit field. - Press
**OK**to finish and close the dialog box. - Select
**CI1**in the geometry object*Selection*list box.

In order to create edges at *z = 0*, on which to impose boundary conditions, two parallel objects can be created by copying the first and offsetting it to the lower half plane.

- Select
**Copy/Transform Object...**from the*Geometry*menu. - Select the
**Make copy of geometry object**check box. - Enter
`0 0 -0.3`

into the*Space separated string of displacement lengths*edit field. - Press
**OK**to finish and close the dialog box. - Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button. - Press the
**Settings***Toolbar*button.

The *Gmsh* external grid generation algorithm can be used for faster and more robust meshing. FEATool will automatically try to download and install *Gmsh* if it can not be found in the load paths.

- Select
**Gmsh**from the*Grid generation algorithm*drop-down menu. - Enter
`0.1`

into the*Subdomain Grid Size*edit field. - Press the
**Generate**button to call the grid generation algorithm. - Press
**OK**to finish and close the dialog box. - Switch to
**Equation**mode by clicking on the corresponding*Mode Toolbar*button. - Select both subdomains in the
*Equation Settings*dialog box and enter`0.3`

for the*Poisson's ratio*and`2.1e11`

for the*Modulus of elasticity*. - Press
**OK**to finish the equation and subdomain settings specification. - Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button. - Select the top boundary (number
**2**) and enter the`-1e6`

for the load force in the*z-direction*.

Also fix the *x* and *y* displacements on the outer boundaries.

- Select
**1**and**7**in the*Boundaries*list box. - Select the
**Fixed displacement, u**radio button. - Select the
**Fixed displacement, v**radio button.

Due to the symmetry the *x-displacement* should be fixed on boundaries **5** and **10**.

- Select
**5**and**10**in the*Boundaries*list box. - Select the
**Fixed displacement, u**radio button.

And similarly the *y-displacement* should be fixed on boundaries **4** and **9**.

- Select
**4**and**9**in the*Boundaries*list box. - Select the
**Fixed displacement, v**radio button. - Press
**OK**to finish the boundary condition specification. - Select
**Add Edge Constraints...**from the*Boundary*menu, and add the constraint*w = 0*to fix the displacement in the z-direction of the outer horizontal edge at*z = 0*(number**4**). - Switch to
**Solve**mode by clicking on the corresponding*Mode Toolbar*button. - Press the
**=***Toolbar*button to call the solver. After the problem has been solved FEATool will automatically switch to postprocessing mode and plot the computed solution. - From the reference the stress in the y-direction at the inner point
*p = (2, 0, 0.3)*should be*-5.38 MPa*. One can use the*Plot Options*to plot the*y-component stress*to visually confirm the solution. - Press the
**Plot Options***Toolbar*button. - Select the
**Surface Plot**check box. - Select
**Stress, y-component**from the*Predefined surface plot expressions*drop-down menu. - Press
**OK**to plot and visualize the selected postprocessing options. - Alternatively, the
*Point/Line Evaluation*functionality can be used to evaluate and extract numeric values in specific points and on lines. - Select
**Point/Line Evaluation...**from the*Post*menu. - Select
**Stress, y-component**from the*Evaluation Expression*drop-down menu.

Note that a small offset, such as *+/-sqrt(eps)* can sometimes be required to ensure the evaluation points are inside the domain.

- Enter
`2`

into the*Evaluation coordinates in x-direction*edit field. - Enter
`0`

into the*Evaluation coordinates in y-direction*edit field. - Enter
`0.3`

into the*Evaluation coordinates in z-direction*edit field. - Press the
**Apply**button. - Press
**OK**to finish and close the dialog box.

The *stress analysis of a thick plate* structural mechanics 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] Davies G, Fenner RT, Lewis RW. *NAFEMS Background To Benchmarks*. LE10 Thick plate - normal pressure, 1992.