Place a cam relationship


The following procedures describe how to use the Cam command (Home tab→Assemble group→Path→Cam) to apply a relationship between a follower that maintains a tangential relationship with a transitional cam surface. The cam can be a closed tangential loop or a chain of curves that are merged into a single composite curve. For more information, see Using the Cam command bar.

Insert a new part

  1. To place a new part into the assembly, drag a placement part from the Parts Library into the assembly workspace.

    The system automatically opens the Assemble command and the associated Assemble command bar, and highlights the placement part (for more information, see Assemble parts (workflow)). Most often it takes more than a single relationship to fully assert a cam/follower relationship, with the Cam relationship being the last relationship to be applied (similar to a Mate relationship).

  2. On the Assemble command bar, select the Cam option from the Relationship Types list .

    For more information, see Using the Cam command bar.

  3. On the highlighted part being placed, select the sphere, cylinder, cone, or torus element to use to form the connection (the follower).

  4. Select the tangent assembly part that is to be used to form the relationship (the cam).

  5. On the command bar, select the cam tangency type:

    • Follower—Select a cylinder, plane, sphere, or torus to use as the follower in the relationship. The Plane option is invalid for a barrel cam.

    • Face—Choose this option to select a face for the cam. Multiple faces can be selected to define a complete tangential loop.

    • Face Chain—Choose this option to select a face chain for the cam.

    • Edge—Choose this option to select an edge to define the cam. Multiple edges can be selected to define a complete tangential loop.

    • Edge Chain—Choose this option to select an edge chain to define the cam.

  6. Based on the selected tangency type, select the element or elements to use to form the Cam relationship. Click Accept (✔) or press Enter to accept the selection. Choose Deselect (X) to cancel the selection.

    This option is active during the Placement Part Element and Target Part Element steps.

  7. To complete the action, press OK. The command bar remains open to apply the next relationship.

  8. Do either of the following:

    • To apply another relationship, continue with Create additional relationships.

    • To close the Assemble command, press the Esc key.

    Tip:

    Use the Flip command to have the follower maintain a tangential relationship on the opposite side of the defined cam surface after the relationship has been applied.

Create additional relationships

  1. To create another Cam relationship between two parts, you can do either of the following:

    • To create a relationship using the Assemble command bar, the Assemble command bar must be open. If not open, select the Assemble command (Home tab→Assemble group→Assemble). On the command bar, select the Cam icon from the Relationship Types list.

    • To create a relationship using the Cam command bar, the Cam command bar must be open. If not open, select the Cam command from the ribbon (Home tab→Assemble group→Path→Cam).

    The actions that can be performed are the same for each option. However, after the Cam command bar is opened, only a Cam relationship can be applied. The relationship type cannot be changed (see Using the Cam command bar).

  2. Select the relationship parts and features as described previously.

  3. To complete the action, press OK.

  4. To close the command and the command bar, press the Esc key.

Using the Tangent features on the command bar About the Cam relationship

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