Part IV: Creating and Using Libraries
Creating a library feature
When creating a library feature, the first problem that you need to solve is how the feature will
be located on a new part. Does it need to be placed on cylindrical parts, rectangular parts, other
types of shapes, or does this matter at all? Will the feature be located by using dimensions or
sketch relations, or will it just be placed underdefined and later fully defined manually rather than
automatically?
You may have noticed in one of the earlier examples that the sample fluid power ports had two
versions of the same feature. One version is intended for the feature to be placed on the flat end of
a cylinder, and the other version is intended for the feature to be placed on a rectangular face.
A few limitations
Library features can contain multiple features of different types. They may add and remove mate-
rial, even within a single library feature. However, a few limitations exist. For example, they
require a base feature, and multi-body features and external references are not allowed, nor are
surfaces, sheet metal, weldments, or molds related features. In addition, you cannot add a scale
feature (a feature that affects the entire body) to the library, nor can you apply library features to
an assembly.
Creating a new library feature
To start a new feature, the first decision that you need to make is what shape to make the base. Is
the feature a type that is usually going to go onto a single shape or multiple shapes? Regardless of
your decision, you or whoever ends up using the feature will have the flexibility to change, or sim-
ply not use, the relations when you place the feature.
For this example, I use a rectangular base. The library feature that I want to create consists of two
boss extrudes, a cut extrude, and several fillets. Here is how it works:
First, you need to create a rectangular extrusion. The size should be bigger than the feature that goes
on it and representative of the face of the end part onto which this feature will typically be placed.
Next, in beginning to create the features that you want to reuse, it is very important that you pay
attention to any references outside of the sketch; these include absolutely anything outside the
active sketch, such as the sketch plane, references to edges, the Origin, other planes, other
sketches, and axes. Although these references are allowed, each reference to anything that is not
already part of the library feature must be reconnected when you place the feature on a new part.
The ideal situation is obviously a single drag-and-drop, but generally speaking, at least one other
step is usually needed. The initial drag-and-drop determines the face for the feature to start from,
and from there, you usually need to locate features, either by using relations or dimensions. A con-
centric relation locates the feature in a single reference selection of a circular edge (although it may
also need to be rotated), and dimensions typically require one dimension in the X dimension and
another one in the Y dimension.
