Section 5: Cast Lever Exercise

Introduction

In this exercise, we will conduct a linear static stress analysis of a simple lever arm part. We will use boundary conditions often found in entry-level CAD-based simulation systems. Note that in later exercises we will build on the steps performed here to refine the analysis setup and improve the overall accuracy of the simulation.

The model is a lever arm as shown:

• A 1000 N load is applied to the top-most hole (A).
• The lever is pinned at the center (B).
• We assume a rod passes through hole (C) and is locked against movement.
• The reaction force, R, balances the loads, so the part is in static equilibrium. A force summation results in R = 687.5 N.

1. Open the Model and Start the Autodesk Nastran In-CAD Environment

Start Autodesk® Inventor, and open Cast Lever.ipt from the Section 5 - Cast Lever sub-folder of your training exercises folder. (Get Started > Launch > Open).

You should see this:

From the ribbon, click the Environments tab, and click Autodesk Nastran In-CAD:

2. Define the Physical Property

1. Click Physical from the ribbon.
2. On the Physical Property dialog, click the New Material icon.
3. On the Material dialog, click Select Material.
4. On the Material DB dialog, expand the Autodesk Material Library list, and select Aluminum 1100-O from the list. Click Close.
5. Click OK on the Material dialog.
6. Click OK on the Physical Property dialog.

3. Constrain the Lever

1. Click Constraints from the ribbon.
2. Make sure the Fixed constraint is specified. (It is the default setting.)
3. Select the inside surface of the center hole (as shown), and click OK.

Note: Because the loads are balanced, we don't expect any rotation about this axis. This is why we have applied a fixed constraint at this location.

4. Define the First Load

1. Click Loads from the ribbon.
2. On the Load dialog, check the Total Force box.
3. Enter a load of -1000 for Fy.
4. Select the inside surfaces of the two holes as shown, and click OK.

5. Define the Second Load

1. Click Loads from the ribbon.
2. On the Load dialog, check the Total Force box.
3. Enter a load of -687.5 for Fx.
4. Select the inside surfaces of the two holes as shown, and click OK.

6. Mesh the Part and Run the Analysis

1. Click Global from the ribbon.
2. On the Mesh dialog, click Update.
3. After the mesh generates, click Run to start the analysis.

Note: While the simulation runs, the Model Tree changes to show the Autodesk Nastran Output. You may see red messages in the output. These indicate that Autodesk Nastran identified elements that are poorly shaped. We will ignore these warnings for this exercise.

When the run is complete, click OK on the message box that indicates that the solution is complete.

7. Review the Results

To plot displacement, right-click on Displacement from the tree, and click Display:

You should see this:

To animate the displacement, right-click on Displacement, and click Animate:

To stop animation, right-click on Displacement, and click Animate so that it is unchecked.

To plot von Mises stress, right-click on von Mises, and click Display:

To disable the element edges, right-click on von Mises, and uncheck Element Edges:

You should see this:

8. Probe for a Specific Value

1. Click the Probe command from the ribbon.
2. Hover over the a location on the lever arm. The results are displayed:

Summary

In this exercise we computed the engineering values needed to properly load and constrain the cast lever. The steps we used were similar to those used in the first exercise (cantilever beam), but the model was a real-world part. We also learned how to extract results including the use of the Probe tool.

Previous Topic: The User Interface

Next Topic: Modify Boundary Conditions Exercise