Solid Thinking: Using Functional Features to Build Plastic Parts

15 Nov, 2005 By: Greg Jankowski Cadalyst

SolidWorks' fastening, vent and area fill features help automate the task of creating features that are functional in nature.

SolidWorks 2006 introduced a number of features designed to assist in building plastic part features. These features are defined within the context of the assembly, so the software uses other assembly part features to construct and define the location and size of the fastening features based on the design.

To edit a part within the context of the assembly, select the part in the Feature Manager design tree, right-click and select Edit Part. The other parts should remain visible and transparent. The setting for the assembly transparency is set within the Display/Selection area of the Tools / Options / System Options dialog box. This setting lets you set the display of the other assembly components to your preference. I use a force assembly transparency level of 75%.

Mounting Boss
When creating a design, you can use a mounting boss to support and attach different components. Figure 1 shows a mounting boss with a locating pin. The mounting boss has a number of options and a post or hole.

Figure 1. Mounting boss added to support the PC board.

You can set all the mounting boss attributes (figure 2). The example shown in figure 1 uses the selected face Face<1>@PC Board-1@Air Remote, where PC Board-1 is the part referred to with the assembly Air Remote.

Figure 2. The Mounting Boss Property Manager tool.

Start with the options from top to bottom and define what your design requires. The position field defines the face for the base of the mounting boss, the direction of the mounting boss (vertical) and the center location for the hole.

Figure 3. FeatureManager design tree for the mounting boss feature.
The mounting boss is located by a 3D sketch point. Figure 3 shows the Feature Manager design tree for the mounting boss feature. Add a dimension to the location if the location is not driven from other geometry. The example shown in figure 1 does not need a locating dimension because the location is driven from the center of the PC board mounting hole. The 3D sketch is the origin of the mounting boss and is driven from the PC board. The -> sign after the feature or sketch indicates that there is an external reference.

Figure 4 shows the external reference created by the mounting boss feature. When a feature is driven from an external reference, it means that when the original feature changes, the mounting boss will change also. To open the External References dialog box, select the feature within the Feature Manager design tree, right-click and select List External Refs.

Figure 4. External references created by the Mounting Boss feature.

While external references are a powerful feature, they take more time to process. One way to get your cake and eat it too -- lock the external references using the Local All button (figure 4). This means the references are still there, but they do not update automatically. So if the design does change, open the External References dialog box again and select Unlock All.

Snap Hook
Snap hooks are added to plastic part designs secure two or more parts together without the use of fasteners. Creating designs without fasteners will make the final product easier and less expensive to assemble.

Figure 5 shows an example snap hook added to a plastic part. The location of the snap hook is defined using a 3D sketch point similar to the mounting boss. But in many cases, unlike the mounting boss, you want to define the exact location for the snap hook. To edit the snap hook, select the 3D sketch under the snap hook feature within the Feature Manager design tree, right-click and select Edit Sketch. Then add the dimensions for the 3D sketch point.

Figure 5. Snap hook example (before and after).

Figure 6 shows the options available when creating the snap hook. The first field is used to define the location and references for the snap hook. The second field is used to size the snap hook.

Figure 6. Snap hook options.

Snap Hook Groove
Once you have made a snap, now you need to add it to the mating part. The snap hook groove feature takes the existing snap hook and adds a relief in the mating part. Figure 7 shows a cross section of the design with the two snap hook groves highlighted. These grooves are tied to and based on the snap hook in the mating part.

Figure 7. Snap hook example shown in a cross-section.

Figure 8 shows the Snap Hook Property Manager. You need to make two selections: the reference hook in another part and the body in the current part to add the snap hook relief. The remaining options are for clearance for the snap hook.

Figure 8. Snap Hook Groove Property Manager.

The fastening, vent and area fill features are meant to help automate the task of creating features that are functional in nature. In-content references are a powerful tool, and you can managed, lock and unlock the references to control what gets updated and when.

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Lynn Allen

In her easy-to-follow, friendly style, long-time Cadalyst contributing editor Lynn Allen guides you through a new feature or time-saving trick in every episode of her popular AutoCAD Video Tips. Subscribe to the free Cadalyst Video Picks newsletter, and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!

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