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Cam and get it

This month's tech tip will cover how to a create simple cam and follower assembly with Alibre Design; and how to manually articulate its motion. This tutorial is for moderate to advanced users of Alibre Design. Top-down design of parts within assemblies is employed in this tutorial.



To create a simple cam and follower assembly:

Creating the cam

  1. Open a new part workspace.
  2. Activate 2D sketch on the XY plane.
  3. Draw an ellipse with its center at the origin, its major axis along the X axis, and its minor axis along the Y axis. Place a dimension between the origin and the node governing the minor axis: enter a value of .75 inch. Place a dimension between the origin and the node governing the major axis: enter a value of 1.5 inches.

  4. Extrude the sketch with the Extrude Boss tool. For the Type, select Mid Plane; and for the Depth, enter a value of 1 inch. Then click OK.

  5. Save the part with a descriptive name like "cam"; and then close the part workspace.

Creating the assembly

  1. Open an assembly workspace.
  2. When prompted for an initial part by the Insert Part/Subassembly dialog box, browse to the part file for the cam that you created in the previous section. Select it and then click Open.
  3. With a preview of the cam part attached to your mouse cursor, left-click once in the work area to place a copy. Then click the Finished button in the Inserting dialog box.
  4. Position the mouse over the cam part, right-click with your mouse, and then select "Show Reference Geometry" option (near the bottom of the menu).

  5. Click on the Insert Assembly Constraint tool on the Assembly Modeling toolbar. It is located on the fly-out menu along with the Quick Constrain Mode toolbar button.

  6. Select the XY plane of the cam, and then the XY plane of the assembly workspace. Use the Align constraint, and set the Offset value to 0. Then click Apply.

  7. Select the Z axis of the cam, and then the Z axis of the assembly workspace. Use the Align constraint, and set the Offset value to 0. Then click Apply.

  8. Click the Close button on the Assembly Constraints dialog box. The Constraints section of the Design Explorer should now look like:

Creating the follower

  1. Click on the Insert New Part tool on the Assembly Modeling toolbar.

  2. Activate 2D sketch on the XY plane.
  3. Use the Project to Sketch tool to project the flat face of the cam part. Select the options for Create reference figure and Maintain association to source entity. Then click OK.

  4. Create a circle similar to the one shown in the figure. Notice that I did not allow the circle to be implicitly constrained at all (no tangency; center is not coincident to anything yet; etc).

  5. Place a dimension on the circle, and set its diameter to 1 inch. Using the coincident constraint, make the center of the circle coincident to the Y axis. Use the tangent constraint to set the circle tangent to the projected ellipse from the cam part. When complete, it should look like the figure (the view was rotated for clarity).

  6. Extrude the sketch with the Extrude Boss tool. For the Type, select Mid Plane; and for the Depth, enter a value of 1 inch. Then click OK.

  7. In the Design Explorer, right-click on the name of the assembly, and then select Edit Part/Subassembly from the menu.

Articulating the assembly

  1. Click on the Precise Placement tool on the Assembly Modeling toolbar.

  2. Click on the cam part to select it: it should now appear in the Selected component(s) entry box. Click in the Axis: entry box in the Rotation entry area of the Precise Placement dialog box; and then click on the Z axis (of the assembly workspace). Enter a value of 6 in the Angle Degrees: entry box (enter a negative value to rotate the opposite direction. Click the Apply button. Now the apply button is the default action for the Enter key on your keyboard. Press and hold the Enter key to continuously rotate the cam... and displace the follower.