Unable to render {include} The included page could not be found.

Exercises

Exercise 1: Distributed Load

Using ANSYS, find the deformation and maximum bending stress of the beam when the load is applied as a distributed load. The 8 kN load is applied uniformly across the span of the beam. Thus, the line force is 8kN/4m=2kN/m.

Hint: In order to carry out this exercise you can duplicate your original Static Structural project and then modify the duplicate. In the modifications you need to delete the original transverse force and apply the distributed load. In order to apply the distributed load right click on Static Structural, then select Insert and then click on Line Pressure as shown in the image below.

You will then need to apply the line pressure to the line, specify the magnitude and direction of the line pressure and lastly have ANSYS solve the system.

Exercise 2: Axial & Transverse Loading

In ANSYS, find the deformation and the stress of the beam when it is experiencing axial and transverse loading. Compare these results to those of the original problem.

Hint: Once again, you can make a duplicate of the original Static Structural and then modify the duplicate. In order to carry out the computations you will need to add the axial force to the beam and then have ANSYS solve the system.

Exercise 3

Consider a two-span beam shown above. The beam is subjected to uniformly distributed loading, point force at x=2m and moment at x=6m as shown. The beam bending stiffness is EI=2 x 10^7 Nm^2.

Using ANSYS, plot the deflection, bending moment, and shear force distribution of the beam. If you have four elements, what is the optimal mesh? Repeat the solution with the eight-element mesh, four for each span. Comment on the results. Is your solution right? How can you improve the finite element solution?

Tips:

In ANSYS, you need to specify E and I separately. You can pick them independently as long as you get the desired EI. You specify I by specifying the cross-section as we saw in the preceding tutorial. To keep things simple, just pick a square cross-section as in the tutorial.
Model the geometry using four lines. You will need to have vertices where you will be applying forces, moments or displacement constraints.
Apply a distributed load using Line Pressure as shown above.
Apply the simply supported constraints using Supports > Displacement. For example, the settings in the figure below can be used to apply the simply supported constraint at A or C. Note that ANSYS uses a generalized 3D beam formulation which includes z displacements. Since we don't have any deformation in the z direction, you can set the z displacements in simply supported conditions to zero.
ANSYS constructs the bending moment from the reactions rather than by differentiating the deformed shape. The former is a more accurate way of calculating the bending moment distribution The two approaches give the same result on a fine mesh.
ANSYS uses mid-side nodes by default which gives a higher-order interpolation than the common cubic interpolation. So you get mesh converged results with relatively few beam elements. To get the cubic interpolation for beam elements, you can drop mid-side modes. You don't need to do this for this problem.