Building the Foundation of the Design - Autodesk Inventor 2010: No Experience Required - page 60

Smooth This constraint is similar to Tangent but with a deeper mathematical
meaning. Rather than a simple relationship that affects the points where two
entities meet, Smooth causes splines to change downstream from the connec-
tion point to maintain the continuity of the curve. This constraint isn't placed
automatically in a sketch.
Symmetric This constraint is often overlooked but is very powerful when
you're working on symmetrical sketches whose size is in fl ux. As with Parallel,
any change made to one member affects the mirrored or symmetrical member
of the constraint.
Equal Using the Equal constraint can create a lot of interesting relationships.
You can keep any two (or more) like entities at the same value. Two lines can
maintain the same length, and two (or more) arcs can maintain the same radius.
This helps reduce the number of redundant dimensions that may be placed in a
sketch otherwise. The = key is the keyboard shortcut for this constraint.
Two additional options control how or whether constraints are placed auto-
matically in the sketch. The default is to have both options turned on so they
appear as engaged buttons:
Constraint Inference This controls whether Inventor recognizes conditions
such as Parallel or Perpendicular in the sketch. With the option off, tools such
as Line still appear to follow horizontal or vertical, but no glyph is displayed.
If you build a shape, any Coincident constraints are automatically added to
the sketch.
Constraint Persistence Turning this off prevents Inventor from capturing
any conditions in the sketch. With Constraint Inference on and Constraint
Persistence off, you can draw using parallelism and so forth; but when you fi n-
ish your sketch, no actual constraints (other than coincidence) will be included
in the sketch. You can't have a condition where Constraint Inference is off and
Constraint Persistence is on. Shutting off Constraint Inference automatically
disables Constraint Persistence.
You can tell Inventor to ignore inference and persistence momentarily by
holding the Ctrl key while sketching. Coincidence is still captured, but every-
thing else is ignored.
To review the constraints that exist in an entire sketch, right-click in the Design
window and select Show All Constraints from the menu or press the F8 key. If you
want to review the constraints placed on an individual geometry piece, select the
geometry segment, right-click, and select Show Constraints.