Assembly Features

While in an assembly, you can create features that exist in the assembly only. You determine which parts you want the feature to affect by setting the scope. You can create a pattern of assembly features in the same manner as you create a pattern of features in a part.

This is useful for creating features that are added after the components are actually assembled and that affect more than one component.

When you want to add a feature to a single component in an assembly, it is better to create the feature in the part rather than the assembly. To do so, you can edit the part in context, or you can create the feature in the assembly and then propagate it to the part by selecting Propagate to part in the PropertyManager.

While it is not a requirement, it is good practice to fully define the positions of the components of the assembly, or fix their locations, before you add assembly features. This helps prevent unexpected results if the components are moved later.

Use assembly features  when you need to represent material-removal operations that are done after the components are assembled.

Examples of Assembly Features

• Welding. A design may specify that a plate and a tube are welded together, and then a hole is drilled through both parts - only after they are assembled - because welding is somewhat inexact. If the holes were pre-drilled, they might not line up after welding. If the designer had put the hole in each part document, instead of as an assembly feature in the assembly document, the hole would have shown up in the drawings for each part and would have been pre-drilled during manufacturing, which defeats the design intent.

• Grinding. A grinding operation occurs after welding. Because grinding is not exact, similar to welding, the grinding is done after the parts are assembled. No grinds should appear in the pre-assembled parts.

Assembly features are not associated with top-down design . The geometry of the parts (as they exist in the part files and drawings) has not been defined by geometry in the assembly (using a layout sketch, other parts, etc.). No external references have been created.

Generally, holes in assembly components such as bearings, gears, and components with bolt holes are manufactured in the parts before assembly. For these cases, create the holes in the part documents. If you then want to define the location of those holes based on assembly geometry, for example using a layout sketch or the geometry of a different part, that is top-down design.

Some designers create holes using assembly features when they really should be creating hole features in the individual parts. For these designers, the SolidWorks application has the Hole Series tool. This tool creates assembly feature holes, but the hole geometry is created in the individual part documents, not in the assembly.

Available Assembly Features

Hole Series

Hole Wizard

Simple Hole

Extrude Cut

Revolved Cut

Fillet

Chamfer

Weld Bead

Belt/Chain

Additionally, for assembly holes and cuts, you can create feature patterns using these tools:

Linear Pattern

Circular Pattern

Table Driven Pattern

Sketch Driven Pattern

Related Topics

Creating an Assembly Feature

Feature Scope in Assemblies

Saving Assemblies with In-context Features