Assembly Features
While in an assembly, you can create cut or hole 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 cuts or holes that are added after the components
are actually assembled and that affect more than one component. When you
want to add a cut or hole to a single component in an assembly, it is
better to edit the part in context than to use an assembly feature.
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.