6.0

46 | Chapter 6 Creating Parametric Sketches
Creating Open Profile Sketches
You can create an open profile from single or multiple line segments, and
solve it in the same way as you solve a closed profile.
An open profile constructed with one line segment is used to define the loca-
tion of a bend feature on a flat or cylindrical part model. To bend an entire
part, you sketch the open profile over the entire part. If you sketch the open
profile over a portion of a part, only that portion of the part bends.
Open profiles constructed with one or multiple line segments are extruded
to form rib features and thin features. For a rib feature, the open profile
defines the outline of the rib, and is sketched from the side view. For a thin
feature, the open profile defines the shape of a wall and is extruded normal
to the work plane.
To learn more about open profiles in features, see “Creating Bend Features”
on page 163, “Creating Rib Features” on page 133, and “Creating Thin Fea-
tures” on page 136.
Creating Closed Profile Sketches
A profile sketch is a two-dimensional outline of a feature. Closed profile
sketches are continuous shapes, called loops, that you construct from lines,
arcs, and polylines. You use closed profile sketches to create features with cus-
tom shapes (unlike standard mechanical features such as holes, chamfers,
and fillets).
Profile sketches can be created from a set of objects, or a single polyline, that
defines one or more closed loops. You can use more than one closed loop to
create a profile sketch if the loops are nested within each other.
You cannot create profile sketches with loops that are
■ Self-intersecting
■ Intersecting
■ Tangential
■ Nested more than one level deep
profile for rib featureprofile for bend feature
profile for thin feature