You can create patterns of Creo Elements/Direct Machining features, Creo Elements/Direct Mold Design features, or face set features or parts.
To create a pattern of features or parts (elements),
1. Click Feature and then, in the Pattern group, click New.
2. Click Linear, Linear Grid, Radial, Radial Grid, Free. The Create Pattern dialog box opens. The options in the dialog box depend on your selection.
To open the Create Pattern dialog box, you can select a feature in the viewport and:
• Click , , , or on the Command Mini Toolbar (CMT) or
• Right-click and choose Create Pattern from the context menu.
3. Select the Source feature or part in the viewport or Structure Browser. This is the feature or part that will be repeated in the pattern. You can select more than one source feature or part. If there are parts as source elements or multiple features in different parts, the owner of the pattern is determined by searching for the lowest common assembly.
The features and parts used to create a pattern must belong to the same top-level assembly.
4. Type a Name or accept the default. This is displayed under the owner in the Structure Browser.
5. Select a Pattern Type (described above) and the appropriate options:
◦ Direction: The direction for a linear row of elements. Select a reference edge or line in the viewport to set the direction. To reverse the direction, hover over an edge or line and press TAB.
◦ Axis: The center and direction of the radial pattern. Select a point in the viewport.
◦ Number: The number of elements in the pattern or in the direction. Enter a value in the dialog.
◦ Distance: The distance between each element in the pattern. Enter a value or use the arrow in the viewport to drag the elements into position.
◦ Total Distance: The total distance between the first and last element. Enter a value in the dialog.
◦ Angle: The angle between each element in a radial pattern. Enter an angle in the dialog.
◦ Total Angle: The total angle of a radial pattern. The default is 360, but you can enter any angle value. The elements in the pattern are distributed evenly around this arc.
◦ Radius: The size of a radial pattern. Enter a value or use the arrow in the viewport to drag the elements into position.
6. If you create a Free pattern,
a. Click Add and position the new feature.
b. Click Pos Dyn if you want more positioning options.
c. Click Apply to finish adding the feature.
d. Repeat until you have the desired pattern.
e. Click Modify to move an element or Delete to remove an element. Select the element in the viewport.
7. If you want the pattern to start at a position different from the current position of the Source, click Start Pos and select a spot on the part in the viewport.
8. If you want to exclude pattern elements, click Exclude and select the pattern elements in the viewport. Excluded elements are shown in red.
• To include an element, select it again in the viewport.
• To include all elements, clear Exclude in the Create Pattern dialog box.
9. Click to complete the operation.
Limitations
• If you choose a source element that is part of another pattern, the element will be automatically excluded from the new pattern. The new pattern will not reference the initial source element.
• If features share a common face, you must select them in the order that they were created so the common face is created before a second feature is copied.
• You cannot select parts that are within an active configuration as elements of patterns. To understand configurations, see
Configurations overview.
• You cannot create a pattern of the following machining features:
◦ Outer thread with Clearance
◦ Outer thread with Groove
• Enhanced patterns (of parts and features) cannot be parameterized with parametric relations.
New.
Linear, 
Linear Grid, 
Radial, 
Radial Grid, 
Free. The Create Pattern dialog box opens. The options in the dialog box depend on your selection.
to complete the operation.