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Using the Snap Hook and Snap Hook Groove

Snap Hook and Snap Hook Groove are two separate features. Lip/Groove combines both functions into a single PropertyManager to help you get results that work together more easily. Figure 24.3 shows the PropertyManager for the Snap Hook feature, along with a completed hook.

The workflow for the Snap Hook feature goes like this:

1. Select a spot on the model that will correspond to the center of the undercut edge where the hook intersects the part. It looks like you can select a face or an edge when you first create the feature, but the software always converts the selection to a 3D sketch point when the feature is accepted.

2. Select a vector (face, edge, axis, not a sketch) to set the vertical orientation of the hook, or the “top.”

3. Select another vector to define the “front” of the hook (the undercut side).

4. Choose to select a mating face or enter a number to define the height of the hook.

FIGURE 24.3

The Snap Hook PropertyManager with a completed hook feature

This feature uses a 3D sketch point where you made the selection in Step 1. You cannot dimension this point while setting up the feature, only by creating the feature and then going back and editing the 3D sketch absorbed under the feature. This is also the arrangement with the Lip/Groove. Remember that you cannot dimension 3D sketches the same way that you dimension 2D sketches. You may need to dimension to planes rather than edges or points to get the dimensions you really intend.

The Snap Groove PropertyManager interface is shown in Figure 24.4, along with a cross section of a finished Snap Hook and a Snap Hook Groove. To use the Snap Hook Groove feature, you must have already created a Snap Hook feature. The interface seems to imply that it requires the body the groove goes into to be in the same part as the body of the hook feature, but this is not the case. You can create this feature in-context between a part with a hook and the part to receive the groove, or in a multi-body part.

FIGURE 24.4

The Snap Hook Groove PropertyManager with a completed hook and groove

Note

Before designing extensive undercuts into a plastic part, it is advisable to talk to the mold builder if possible. They may have either limited or special capabilities that could impact on the practicality of one approach as opposed to another. I find it is frequently beneficial to work closely with a mold designer or builder on plastic part projects.

When I model plastic parts, rarely do situations call for a generic snap feature. Usually situations require more inventiveness due to space restrictions or curvature or material thickness considerations. The Snap Hook and Snap Hook Groove features are reasonably easy to use, but may not have the flexibility for application in all situations.

Using Lip/Groove

The Lip/Groove feature enables you to create a matching lip and groove in either a pair of parts in an assembly or a pair of bodies within a single part. Figure 24.5 shows the Lip/Groove PropertyManager creating a groove in a part. The same interface also creates the lip feature.

FIGURE 24.5

Using the Lip/Groove feature

The workflow for this feature goes like this:

1. Select the part or body to receive the groove.

2. Select the part or body to receive the lip. If you only want to create a groove, you can skip the lip steps.

3. Select a plane, planar face, straight edge, or axis to establish the direction of pull.

4. Select faces that represent the parting surface along the area to get the lip/groove.

5. Select edges that the lip/groove will affect.

6. Set dimensions for both lip and groove features.

In some cases, the automated tools may not be able to create what you need to create. You can employ one of several manual workarounds to make lips and grooves. Several techniques exist:

• On a planar parting line, you can use sketches offset from the edges and then extrude either a boss or a cut.

• Using a thin feature extrude (boss or cut) can