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.
Improvements to flattening sheet metal parts make flattening succeed for complex shapes which previously failed. These improvements also provide better flattened geometry for certain corner treatments, lofted bends, and in some cases where cuts intersect bend regions.
You can update existing flat patterns created prior to SOLIDWORKS 2011 to use the improved method. In the FeatureManager design tree, right-click
Flat-Pattern1 and click
Edit Feature. In the
Flat-Pattern PropertyManager, under
Parameters, select
Recreate flat-pattern.
You can create *.dxf files of sheet metal flat patterns without flattening the 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. You can define a grain direction to use when calculating the bounding box for sheet metal parts. The software determines the smallest rectangle (bounding box) that aligns with the grain direction to fit the flat pattern. |
| 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. |
| Multibody sheet metal parts |
Flat patterns of all bodies appear at the end of the FeatureManager design tree. When you expand the representation of a body in the cut list, the body's flat pattern appears at the end of its feature list. |
| Self-intersecting parts |
If a part cannot be flattened because it has self-intersecting geometry, a warning is displayed and the feature causing the problem is highlighted in the graphics area. |
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.