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CHAPTER 1 Inventor DesIgn PhIlosoPhy
within the model, to achieve a complex design in the end. By creating a number of features
within the model, you are able to independently change or modify a feature without rebuild-
ing the entire model. An example of editing a feature would be changing a hole size. If you
create a base feature first and then create a hole feature in that base feature, you can makes
changes to both independently.
pa t t e r n a n D mi r r o r a t t h e Fe a t u r e le v e l
Although there are mirror and pattern (array) tools in the sketch environment, it is generally
best to create a single instance of the item in the sketch, then create a feature from it, and create
a mirror or pattern feature from that feature. The logic behind this is based on the previous two
ideas. First, this approach keeps the sketch simple. Second, should the mirror or pattern feature
need to be updated, it is much easier to do so as a separate feature.
cr e a t e sK e t c h -Ba s e D Fe a t u r e s a n D th e n pl a c e D Fe a t u r e s
Part features can be broken into two categories: sketch based and placed. Sketch-based features, as
you might guess, are created from sketches. Placed features are features such as fillets and chamfers
that are placed on model edges or faces and have no underlying sketch. Issues arise when placed
features are created too early in the development of the part, because you may then be required to
dimension to the placed feature, which creates a weak dependency, for instance, if you place fillets
along the edges of a part and then use the fillet edges to define the placement of a hole. But then
if you realize that machining capabilities require a beveled chamfer edge rather than a rounded
filleted one, the hole feature is sure to fail. Keep this in mind as you create placed features such as
fillets and chamfers, and reserve placed features for the end stages of the part.
un D e r s t a n D De p e n D e n t a n D in D e p e n D e n t Fe a t u r e s
Parametric model features are typically either dependent or independent of one another. A
dependent feature is dependent on the existence or position of a previously created feature. If that
previously created feature is deleted, then the dependent feature will either be deleted also or
will become an independent feature. Each part file contains default origin geometry that defines
the X, Y, and Z coordinates of the part. These origin features are used to create the first sketch in
every part by default. An independent feature is normally based on an origin feature or is refer-
enced off the base feature.
For instance, in order to create the base feature for the pivot link, you would create a sketch
on a default origin plane, such as the XY plane. Because the XY origin plane is included in every
part file and cannot be changed, your base feature is stable and independent of any other fea-
tures that may follow. To create a hole in the base feature, you would typically select the face of
the base feature to sketch on. Doing so would make the hole feature dependent on the base fea-
ture. The hole feature then, is inherently less stable than the base feature, because it relies on the
base feature to define its place in 3D space.
Although the specifics of how sketches, features, and parts are created will be covered in the
chapters to come, remember these principles concerning part file best practices, and you will
find Inventor (and any other parametric modeler) much more accommodating.
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