If you insert a 3D annotation in
a sheet metal part, a Flat pattern annotation view is automatically created
in the Annotations 
folder. When you select the Flat
pattern annotation view, the Flatten
tool is unavailable.The Flat-Pattern1 feature is intended to be the last feature in the folded sheet metal part. All features before Flat-Pattern1 in the FeatureManager design tree appear in both the folded and flattened sheet metal part. All features after Flat-Pattern1 appear only in the flattened sheet metal part.
Some items to note about the flat-pattern feature:
New features in folded part. When Flat-Pattern1 is suppressed, all features that you add to the part automatically appear before this feature in the FeatureManager design tree.
New features in flattened part. You flatten the entire sheet metal part by unsuppressing Flat-Pattern1. To add features to the flattened sheet metal part, you must first unsuppress Flat-Pattern1.
Reorder features. You cannot reorder sheet metal features to go below Flat-Pattern1 in the FeatureManager design tree. So, you cannot order a cut with the Normal cut option underneath Flat-Pattern1.
Modify parameters. You can modify the parameters of Flat-Pattern1 to control how the part bends, to enable or disable corner options, and to control the visibility of the bend region in the flattened sheet metal part.
Sketches. You can transform sketches and their locating dimensions from a folded state to a flattened state and back again. The sketch and locating dimensions are retained.
If you insert a 3D annotation in
a sheet metal part, a Flat pattern annotation view is automatically created
in the Annotations folder. When you select the Flat
pattern annotation view, the Flatten
tool is unavailable.
To modify the parameters of the Flat-Pattern1 feature:
Right-click Flat-Pattern1 in the FeatureManager design tree, and select Edit Feature.
In the PropertyManager, under Parameters:
In the graphics area, select a face that does
not move as a result of the feature for Fixed
face 
.
Select Merge faces to merge faces that are planar and coincident in the flat pattern.
When selected, no lines are shown in the bend regions.
Select Simplify bends to straighten curved edges in the flat pattern.
Under Corner Options:
Select Corner Treatment to apply smooth edges in the flat pattern.
Select Add Corner-Trim to apply relief cuts in the flat pattern. When selected, you can choose from:
Break
corners. Cuts away material from an edge or a face. Click Chamfer 
or Fillet
as the Break type
and set the Distance 
or Radius 
.
Relief type. Sets the relief type for any relief cuts needed.
Radius
or Side length. Set the Radius or Side
length for the Relief type.
Ratio to thickness. Sets the relief type radius to a specified ratio of the sheet metal thickness. When selected, set the Ratio of radius/distance to sheet metal thickness.
Click OK 
.
To display sketch dimensions in flattened state:
Create a sheet metal part that includes a sketch with dimensions on a face.
Flatten the model.
In the FeatureManager design tree, under Flat-Pattern 
, expand Sketch Transformation 
.
Double-click the derived sketch to display the dimensions in a flattened state.
