Give your job a title, e.g. ‘Cantilever Beam’.
Select a 2d elastic beam element.
Is this a good element choice? You can also look at the options for this element type.
Set Young’s modulus to 2.× 10 5 (in units of N/mm 2 ) and Poisson’s ratio to 0.3
Note that the vertical axis here is the z -axis, so the force will be applied in the z direction.
It is also a good idea to preview the section data summary to check that all the parameters are entered and calculated correctly.
The parameters of interest are:
Area = B × H = 5000
Second moment of area about y -axis
= I yy = B ×( H 3 )/12 = 0.41667× 10 7
Create two key points at:
KP 1 = 0, 0, 0
KP 2 = 2000, 0, 0
Create a line between these two key points.
Set global element size to 200
Mesh the line.
Fix all dofs at key point (or node) number 1
Apply a force of 10000 N in the minus Z direction on the node at the other end of the beam.
If necessary, rotate the axes so that the z-axis is pointing up:
Solve the system.
What is the maximum displacement at the tip?
I got 32.0 mm
Here is the list of displacements I obtained as a function of node x-position:
Node number | Node x-position | Displacement (Uz) |
1 | 0 | 0.000 |
3 | 200 | 0.4637 |
4 | 400 | 1.7914 |
5 | 600 | 3.8872 |
6 | 800 | 6.6549 |
7 | 1000 | 9.9986 |
8 | 1200 | 13.822 |
9 | 1400 | 18.030 |
10 | 1600 | 22.526 |
11 | 1800 | 27.213 |
2 | 2000 | 31.997 |
You can see that the maximum displacement is 32 mm (to 2 dp).
To look at the stresses in the beam we normally need to define an element table. You should read your FEA software’s help menu, particularly on your chosen element to determine the name (or identifier) of variables that give bending stresses.
I obtained the following values of axial and bending stresses for each element:
Element number (from constrained end) | Axial stress | Bending stress (stresses in both nodes are computed to be the same) |
1 | 0.00 | -228.0 |
2 | 0.00 | -204.0 |
3 | 0.00 | -180.0 |
4 | 0.00 | -156.0 |
5 | 0.00 | -132.0 |
6 | 0.00 | -108.0 |
7 | 0.00 | -84.00 |
8 | 0.00 | -60.00 |
9 | 0.00 | -36.00 |
10 | 0.00 | -12.00 |
Now you need to use your knowledge in beam theory to verify the results of your FE model. Follow the procedure below:
Calculate the maximum bending stress at the ends of each element using the classic Engineer’s Bending Equation,
For example, for element 1 you should get bending stresses of 240 MPa at node I and 216 MPa at node J which gives the average stress of 228 MPa for element 1. This is exactly what we achieved from your finite element model.
OpenLearn - Introduction to finite element analysis Except for third party materials and otherwise, this content is made available under a Creative Commons Attribution-NonCommercial-ShareAlike 4.0 Licence, full copyright detail can be found in the acknowledgements section. Please see full copyright statement for details.