About Point Patterns in Creo Flexible Modeling
Use a point pattern to create a pattern by placing pattern members at points or coordinate systems. Create or select any of the following references when you use a point pattern:
• Sketch feature that contains one or more geometry sketch points or geometry sketch coordinate systems
• Internal sketch that contains one or more geometry sketch points or geometry sketch coordinate systems
• Datum point feature
• Import feature that includes one or more datum points
• Analysis feature that includes one or more datum points
When you create a point pattern, the system creates pattern members by placing the origin of the lead feature or geometry at each of the points or coordinate systems. By default, the origin of the lead feature or geometry is at the geometric center. So, by default, the system places the geometric center of the lead pattern member at each of the point pattern locations. This can be seen in the pattern preview where the origin of the lead member is shown as a black dot with a white circle around it 
, and the locations where that origin will be placed for each additional pattern member are shown as a black dot 
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, and the locations where that origin will be placed for each additional pattern member are shown as a black dot .You have the option to tell the system to use an alternate origin when placing the pattern members. This gives you much greater control over how the pattern members are created, and can be used if you are not satisfied with the geometric center default.
If you use sketched entities, make sure they are geometry entities. Construction entities are sketching aids only, and they do not convey feature-level information outside Sketcher.
The sketch you reference can also include curves. When you select the Follow curve direction option on the Options tab, each pattern members is oriented to reflect the curve tangent direction, where its point coincides with the curve. If you clear the Follow curve direction check box, any curves present in the sketch are ignored.