Building the Foundation of the Design - Autodesk Inventor 2010: No Experience Required - page 70

Construction When you draw in Inventor, the geometry is normal geometry by
default. Normal geometry is intended to build shapes from which to make 3D
features. Construction geometry is ignored by 3D modeling tools but can be
used to defi ne the shape and location of the 2D sketch geometry.
Center Point Any geometry placed in a sketch has points included. You can
select these points for different functions. When the Center Point override is
selected, points that are placed in a sketch are automatically selected as a place
to put a hole feature. This option is typically switched on.
Centerline This option can convert any normal or construction geometry to
take on special properties as a centerline. Centerlines can be selected automati-
cally for creating round or turned shapes using the Revolve tool. They can also
change the behavior of dimensions, causing them to recognize a sectional pro-
fi le as having its size based on a diameter rather than a linear dimension.
Driven Dimension The dimensions you placed on the sketch in the previous
exercise are referred to as parametric dimensions. Their value changes the size
of sketch geometry. There are times where you want a dimension to simply show
what size something is but not be able to change the geometry. A driven dimen-
sion allows this. It even displays itself in the sketch in parentheses as a reference
dimension would be displayed.
NOTE Since Release 9, AutoCAD has had associative dimensions that
have the ability to change their values when the geometry they're attached to
changes. This is essentially how driven dimensions behave.
Now you'll fi nish the sketch so you're ready to create the fi rst feature of your
component. Let's start with a little experiment using a sketch override. Then,
you'll go back to the dimensions and constraints you're getting used to:
1. Use the Esc key to clear any tools that are active.
2. Click the angular dimension at upper right, and then select the
Driven Dimension override from the Format panel on the Sketch tab.
See Figure 2.18.
You'll see that there is more freedom on the angled line. Now, fully
constrain the sketch:
3. Start the Vertical constraint, and select the angled line. Note that the
driven dimension responds to the change and the angular DOF is
removed.