Part Modeling > Edit Features > Pattern > Curve Patterns > To Create a Curve Pattern
To Create a Curve Pattern
1. Select the feature that you want to pattern and click Model > Pattern. The Pattern tab opens.
2. Select Curve from the list of pattern types. The Curve pattern options open.
3. Select or create a sketched curve to define the pattern. To sketch a curve, click the References tab and click Define.
* In Sketcher, a read-only construction point is placed at the pattern leader origin, with horizontal and vertical construction lines passing through the point.
* Click OK to complete the sketch. When you select a curve or sketch a curve, a preview of the pattern along the curve is displayed, based on default values. Each pattern member is identified by .
4. Type a value for distance between pattern members in the box.
5. Type a number of pattern members in the box.
6. Click the Options tab to set one or more of the following optional parameters:
Regeneration option—Reduces regeneration time by selecting a more restrictive regeneration option, depending on the complexity of the pattern:
Identical—All the pattern members are identical in size, are placed on the same surface, and do not intersect each other or part boundaries.
Variable—The pattern members can vary in size, or be placed on different surfaces, but they cannot intersect each other or part boundaries.
General—There are no pattern member restrictions.
Use alternate origin—Uses an origin different than the default geometric center of the lead feature or geometry to place the pattern leader.
Follow surface shape—Positions pattern members to follow the shape of the selected surface. Click the collector and select a surface.
Follow surface direction—Orients the pattern members to follow the surface direction.
Spacing—Sets the way that the pattern leader and pattern members are projected onto the surface.
Follow curve direction—Places pattern members in the sketch plane to follow the curve.
7. To change the start point and direction of the curve, click the References tab and click Edit to enter Sketcher mode.
8. Select a curve end from the sketch as the start point for open sketches or select any vertex from the sketch for a closed sketch and click Sketch > Setup > Feature Tools > Start Point. The selected curve end or vertex is set as the start point.
9. To exclude a pattern member, click the corresponding black dot (). The black dot changes to white () to show that the pattern member has been excluded. To re-include the pattern member, click the white dot again. The pattern leader is identified by .
10. Click . The feature is patterned.