Flat Pattern
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.
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.
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.
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
to merge faces that are planar and coincident in the flat pattern.
When selected, no lines are shown in the bend regions.
Select
to straighten curved edges in the flat pattern.
Under Corner
Options, select
to apply smooth edges in the flat pattern.
Under Grain Direction,
click in Grain Direction, then
select an edge or line in the graphics area.
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.
