About Flat Pattern Features
Flat patterns create a flattened version of one sheet metal body to prepare the body for manufacture. Only one flat pattern feature is created for a sheet metal body. When there is one body in the part, you can create a standalone flat pattern feature. When there is more than one body in the part, create a flat pattern manager feature. A flat pattern manager feature automatically creates a flat pattern for each sheet metal body with geometry in the part.
The flat pattern feature remains the last feature in the Model Tree. New features in the part are added to the Model Tree before the flat pattern feature. The flat pattern is suppressed when you add or redefine features in a design. It is automatically resumed after the features have been added.
When you create a standalone flat pattern feature, you must define a fixed surface or edge. You can save time and maintain consistency by setting at body-level a fixed geometry reference for all Unbend, Bend Back, and Flat Pattern operations in the Fixed Geometry dialog box. Use the General tab of the Sheetmetal Preferences dialog box to change the fixed geometry reference.
After you create a flat pattern of a body, use the 
Bounding Box Dimensions command on the View tab to toggle the display of the length and width dimensions of the unbent sheet metal body. The dimensions are associated with the SMT_FLAT_PATTERN_LENGTH and SMT_FLAT_PATTERN_WIDTH parameters.
Bounding Box Dimensions command on the View tab to toggle the display of the length and width dimensions of the unbent sheet metal body. The dimensions are associated with the SMT_FLAT_PATTERN_LENGTH and SMT_FLAT_PATTERN_WIDTH parameters.Keep in mind the following points when creating a flat pattern feature:
• You cannot manually select bent geometry.
• You cannot create a flat pattern for a body with more than one disjoint volume of unattached geometry.
• When surfaces are detected that require the creation of deformation areas, specify treatment of the areas as you would using the Unbend tool.
• You can project cuts added to forms to the flat pattern.
• Use the Flat Pattern Preview tool to open a window that displays the active body in an unbent condition, when there is no Flat Pattern feature in the model.
Legacy Flat Pattern Features
When you retrieve sheet metal parts created using a version earlier than Creo Parametric 11.0.0.0, it shows a single sheet metal body. This body contains all the sheet metal geometry in the part. It can have one flat pattern feature. When you add a sheet metal body to a legacy part with a flat pattern feature, you can create a flat pattern manager feature that contains a flat pattern for each sheet metal body in the part.
You can use standard Family Table commands for a legacy part with an Unbend or Flat Pattern feature. For more information, search the Fundamentals area of the Help Center.
Use legacy flat state instance commands for bent or unbent parts when the enable_flat_state configuration is set to yes or when there is one legacy flat state instance in your model.
When you add a new instance to a legacy flat pattern, you can only create a flat instance.