Part Modeling > Edit Features > Pattern > Curve Patterns > About Curve Patterns
About Curve Patterns
A Curve pattern creates instances of a feature along a sketched curve. While creating or redefining a Curve pattern, you can set the following parameters:
Spacing—Type the increment value between the pattern members in the Pattern tab text box.
Number of pattern members—Type the number of pattern members to be created in the Pattern tab text box.
Skip pattern members—To skip a pattern member, click the black dot that identifies the pattern member. The black dot turns white. To restore the pattern member, click the white dot.
Pattern member orientation—Orient pattern members to reflect the curve tangent direction at an origin, or create pattern members with identical orientation to the pattern leader.
The distance or number of members parameter you set becomes a dimension after the pattern is created. You can edit this dimension to modify the space between the members or the number of members. You can also use this dimension in a relation.
The start point of the Curve pattern is at the start of the curve by default. To accurately align the pattern members along the curve, the pattern leader should be placed at the start of the curve. A yellow direction arrow identifies the start point and direction of the Curve pattern.
Internal Sketches for Curve Patterns
A Curve pattern can have all closed sections or all open sections, but not a combination of closed and open sections. You can also create a Curve pattern with more than one sketch curve section. To create successive sections, click Sketch > Setup > Feature Tools > Toggle Section in the Sketcher window.
For open sketches, the direction of the pattern is always from the start point of the curve towards the end point of the curve.
For closed sketches, the direction of the pattern can be from either side of the selected vertex.
For single entity closed sketches, divide the sketch to select the start point.