FEATool Multiphysics
v1.10 Finite Element Analysis Toolbox |

Cylindrical Pressure Vessel

A long cylindrical thick walled pressure vessel is here subjected to both a high internal pressure and thermal expansion. The model and solution is symmetric and also suitable for modeling with the two-dimensional plane strain approximation. This problem allows for an analytical solution which is used to validate and test the accuracy of the simulation [1].

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Structural Mechanics** > **Cylindrical Pressure Vessel** 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
**2D**radio button. - Select the
**Plane Strain**physics mode from the*Select Physics*drop-down menu. - Press
**OK**to finish the physics mode selection.

To decrease the time and cost of the simulation, symmetry and and the plane strain approximation are used so that only a quarter of a 2D slice has to be modeled.

The geometry can be created by first subtracting a smaller inner from a larger outer cylinder. And the overlaying a rectangle and using the intersection operation to get the resulting quarter geometry section.

- To create a circle or ellipse, first click on the
**Create circle/ellipse***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. - Select
**E1**in the geometry object*Selection*list box. - To modify and edit the selected ellipse, click on the
**Inspect/edit selected geometry object***Toolbar*button to open the*Edit Geometry Object*dialog box. - Enter
`0 0`

into the*center*edit field. - Enter
`0.95`

into the*x*edit field._{radius} - Enter
`0.95`

into the*y*edit field._{radius} - Press
**OK**to finish and close the dialog box. - To create a circle or ellipse, first click on the
**Create circle/ellipse***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. - Select
**E2**in the geometry object*Selection*list box. - To modify and edit the selected ellipse, click on the
**Inspect/edit selected geometry object***Toolbar*button to open the*Edit Geometry Object*dialog box. - Enter
`0 0`

into the*center*edit field. - Enter
`0.2`

into the*x*edit field._{radius} - Enter
`0.2`

into the*y*edit field._{radius} - Press
**OK**to finish and close the dialog box. - Select
**E1**and**E2**in the geometry object*Selection*list box. - Press the
**- / Subtract geometry objects***Toolbar*button. - 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. - Select
**R1**in the geometry object*Selection*list box. - To modify and edit the selected rectangle, click on the
**Inspect/edit selected geometry object***Toolbar*button to open the*Edit Geometry Object*dialog box. - Enter
`0`

into the*x*edit field._{min} - Enter
`1`

into the*x*edit field._{max} - Enter
`0`

into the*y*edit field._{min} - Enter
`1`

into the*y*edit field._{max} - Press
**OK**to finish and close the dialog box. - Select
**CS1**and**R1**in the geometry object*Selection*list box. - Press the
**& / Intersect geometry objects***Toolbar*button. - Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button. - Enter
`0.02`

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. - Equation and material coefficients are be specified in
*Equation/Subdomain*mode. In the*Equation Settings*dialog box, enter`0.33`

for the*Poisson's ratio*and`2e11`

for the*Modulus of elasticity*,`1.3e-5`

for the*Thermal expansion coefficient*, and the expanded expression for the temperature field*(Ti-To)/log(ro/ri)*log(ro/r)+To*. The other coefficients can be left to their default values. - Enter
`(600-30)/log(0.95/0.2)*log(0.95/sqrt(x^2+y^2))+30`

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

To account for the symmetry, apply fix left vertical boundary by setting the displacement in the x-direction there to zero, and similarly fix the *y-displacement* on the lower horizontal boundary.

- Select
**3**in the*Boundaries*list box. - Select the
**Fixed displacement, v**radio button. - Select
**4**in the*Boundaries*list box. - Select the
**Fixed displacement, u**radio button.

Apply the normal pressure `6e7`

on the inner boundary and `2.5e7`

on the outer one. Note that these loads are scaled with the outward pointing unit normal vectors `nx`

and `ny`

in order to apply the forces normal to the boundaries.

- Select
**2**in the*Boundaries*list box. - Enter
`-nx*6e7`

into the*Displacement/load, x-component*edit field. - Enter
`-ny*6e7`

into the*Displacement/load, y-component*edit field. - Select
**1**in the*Boundaries*list box. - Enter
`-nx*2.5e7`

into the*Displacement/load, x-component*edit field. - Enter
`-ny*2.5e7`

into the*Displacement/load, y-component*edit field. - Press
**OK**to finish the boundary condition specification. - 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.

The analytical solution for the displacement and stresses in the radial direction are as follows

r = 0.2 | r = 0.95 | |
---|---|---|

r-displacement | 0.00068 | 0.00302 |

r-stress | -6e7 | -2.5e7 |

th-stress | -1.59e9 | 0.59e9 |

z-stress | -2.1e9 | 0.107e9 |

- Press the
**Plot Options***Toolbar*button. - Select
**Stress, x-component**from the*Predefined surface plot expressions*drop-down menu. - Press
**OK**to plot and visualize the selected postprocessing options.

To compare it is easier to either look at the horizontal x-axis (where the x-direction quantities correspond to the radial ones) or alternatively the vertical y-axis. Click anywhere on the surface plot to evaluate the expression in the chosen point. For a more clear representation one can use the *Point/Line Evaluation* functionality to study and plot quantities at points and lines.

- Select
**Point/Line Evaluation...**from the*Post*menu. - Select
**x-displacement**from the*Evaluation Expression*drop-down menu. - Enter
`0.2:0.01:0.95`

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

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

The *cylindrical pressure vessel* 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] Barber JR. *Solid Mechanics and Its Applications, Intermediate Mechanics of Materials*. vol. 175, 2nd ed. Springer, 2011.