Main Steps
Select Step
Defines the features or geometry you want to pattern.
Select Curve Step
Specifies the curve for the selected elements to be patterned along.
Path Curve Step
Specifies the curve for the pattern to follow.
Advanced Definition Step
Specifies advanced definition for the pattern. During this step, you can specify transformation and rotation type, as well as control occurrence behavior.
Select Parts Step
Specifies the parts which are included in the pattern feature. Parts that lie within the range of the profile and the extent are automatically selected. You can also deselect parts by holding the CTRL key and selecting parts that are highlighted. When you add parts to a pattern feature that were not in the parent feature, the parts also must be added to the parent feature. This option is available only in the Assembly environment.
Preview/Finish/Cancel
This button changes function as you move through the feature construction process. The Preview button shows what the constructed feature will look like, based on the input provided in the other steps. The Finish button constructs the feature. After previewing or finishing the feature, you can edit it by re-selecting the appropriate step on the command bar. The Cancel button discards all input and exits the command.
Select Options
Smart
Constructs the feature using the Smart option. The Smart option takes longer to process, but can handle more cases. The Smart option can be used when individual members encounter different geometry than the feature being patterned. This option is available only when the Select option is set to Feature.
Fast
Constructs the feature using the Fast option. The Fast option processes very quickly, but it cannot be used if any members encounter different geometry than the feature being patterned. If a fast pattern fails, select the Smart option and recompute the feature. This option is available only when the Select option is set to Feature.
Select
Specifies the type of element you want to pattern. This option is not available in the Assembly environment.
Single—Allows you to select one or more individual elements, such as edges or surfaces.
Chain—Allows you to select a endpoint connected set of elements by selecting one of the elements in the chain.
Body—Allows you to select a design body.
Feature—Allows you to select a feature, such as a protrusion, cutout, or hole feature.
Note:
When constructing and editing pattern features, you cannot have more than one element type in a single pattern. For example, you cannot pattern a hole feature, a design body, and a curve in one operation.
Deselect (x)
Clears the selection.
Accept (check mark)
Accepts the selection.
Select Curve and Path Curve Options
Pattern Curve
Specifies the curve for the selected elements to be patterned along.
Anchor Point
Specifies the point on the curve at which you want occurrence alignment to begin.
Pattern Type
Specifies how occurrences are placed in the pattern. When set to Fit, the pattern operation places the number of occurrences specified by the Count option, equally spaced. When set to Fill, the pattern operation places as many occurrences as will fit on the curve, with the distance specified by the Spacing option between each occurrence. When set to Fixed, the pattern operation places occurrences using both the Count and Spacing options.
Count
Specifies the number of occurrences to be placed in the pattern. Count is not available when Pattern Type is set to Fill.
Spacing
Specifies the space between occurrences in the pattern. Spacing is not available when Pattern Type is set to Fit.
Offset
Specifies the offset distance from the selected point. Offset is available on the command bar after you have selected the anchor point.
Advanced Definition Step Options
Transformation Type
Sets the transformation type for the pattern.
Linear—Occurrences are oriented based on the orientation of the features being patterned.
Full—Occurrences are oriented based on the input curves.
From Plane—Occurrences are oriented based on the projection of the initial occurrence and a target occurrence onto a plane, where a measured angle defines occurrence orientation.
Rotation Type
Sets the rotation type for the pattern. Rotation Type is available on the command bar when Transformation Type is set to Full or From Plane.
Curve Position—Occurrences are placed according to the position of the path curve.
Feature Position—Occurrences are placed according to the position of the initial occurrence.
Reference Point
Specifies the point in the pattern at which transformation begins. By default, the reference point is the anchor point. To select a difference reference point, click Reference Point and click a new point on the pattern.
Suppress Occurrence
Suppresses pattern occurrences. After you select Suppress Occurrence, click the occurrence points for the occurrences you want to suppress. You can suppress individual occurrences, or you can use a fence to suppress adjacent multiple occurrences.
Insert Occurrence
Inserts a pattern occurrence. After you select Insert Occurrence, click a keypoint to insert an occurrence.
Offset
Specifies the offset distance from the selected point. Offset is available on the bar after you have selected Insert Occurrence.