Sketch Driven Patterns
Using sketch points within a sketch, you can specify a feature pattern.
The seed feature propagates throughout the pattern to each point in the
sketch. You can use sketch driven patterns for holes or other feature
instances.
Bodies to Pattern. For multibody
parts, select a separate body to create a sketch driven pattern.
To build a sketch driven pattern:
Open a sketch on the face of a part.
-
Create a seed feature on the model.
-
Click Point 
or Tools, Sketch Entity,
Point and add multiple sketch points to represent the pattern you
want to create, based on the seed feature.
Close the
sketch.
Click Sketch
Driven Pattern 
on the Features toolbar, or click
Insert,
Pattern/Mirror, Sketch Driven
Pattern.
Under Selections,
do the following:
If necessary, use the flyout FeatureManager design
tree to select a Reference Sketch
to use as the pattern.
Click either Centroid
to use the
of the seed feature, or Selected point
to
as the reference point.
If you chose Selected
point as the reference point, select a Reference
Vertex 
in the graphics area.
You can use the centroid of the seed feature, the sketch
origin, a vertex, or another sketch point as a reference point in a sketch
driven pattern.
Do one of the following:
-
To create the pattern based on the feature, under Features
to Pattern 
, select the feature in the graphics area.
NOTE: If the feature to
pattern includes fillets or other additions, use the flyout FeatureManager
design tree to select these features.
To create the pattern based on the faces that
make up the feature, under Faces to Pattern
, select all the faces in the graphics area. This is useful
with models that import only the faces that make up the feature, and not
the feature itself.
When using Faces
to Pattern, the pattern must remain within the same face or boundary.
It cannot .
For example, a cut across the entire face or different levels (such as
a raised edge) would create a boundary and separate faces, preventing
the pattern from propagating.
Under Options,
set these options:
Geometry pattern. Creates the pattern
using only the geometry (faces and edges)
of the features, rather than patterning and solving each instance of the
features. The
Geometry
Pattern option speeds
up the creation and rebuilding of the pattern. You cannot create geometry
patterns of features that have faces merged with the rest of the part.
Geometry
pattern is not available with Bodies
to Pattern.
Click OK 
.
|
|
|
|
Sketch pattern with Centroid as the reference point |
Sketch pattern with Selected
point as the reference point |