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