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Autodesk Inventor Tips & Tricks

Cylindrical Cams with Autodesk Inventor

Autodesk Inventor 2015
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By David Melvin, PE, TEDCF Publishing

Constructing a cylindrical cam using Autodesk Inventor may seem like a daunting task, but once you read this article you’ll see that it’s really quite simple. The example in this tip creates a slot that is parallel along the axis of the cylinder. To create a slot with parallel walls read my tip on Parallel Wall Cylindrical Cams with Autodesk Inventor.

The image above shows the size of features. We’ll use these sizes to create the cam.

If you unroll the cam portion in your mind’s eye you’ll understand the first step. You need to create a flat plate that will be rolled to form the cam portion. The width of the plate needs to be the full length of the cylinder, and the height needs to be the length of the circumference of the cam portion. Since the Core Diameter is 1 inch, the circumference is Pi.
The key to entering the circumference is to enter a value with too many places. That is, if the significant number of digits in your design is 3 places, enter a value with at least 4 places. You’ll see why in just a minute. In this case I’ve entered 3.14159.

The next step is to extrude the profile the thickness of the cam, which is .25 in.

The next step is to draw the cam shape. I’ve arbitrarily drawn the shape, so this is not a standard cam shape.
You can also use this technique to construct a barrel or end cam. All you have to do is draw the cam shape on the end of the plate instead of the middle.
Cut an extrusion of the profile through the plate. Use the Through All Extents option.
Make a sketch on the surface of the plate, and draw a line on the middle. Make sure to fully constrain the sketch.
Use the Bend Part command to roll the plate. The direction on the top-right of the dialog box is set to both sides. The radius in this case is 0.5 in, and the angle is 360 degrees.
This creates a cylinder with a small gap. In this case the gap is less than .00001 in. This is why the circumference is calculated with too many digits. It helps to create an insignificant gap. You can fill the gap by making a sketch on one side of it and then extruding to the other side.
Once you’ve finished the cam portion, extrude the core.

How is this Beneficial?

The Bend Part command is a powerful command that is quite often forgotten. This example shows how to create a cylindrical cam, but there are a lot of other shapes that can only be made using this command. It just takes a little bit of imagination.