Swept Flange PropertyManager

The Swept Flange PropertyManager creates compound bends in sheet metal parts.

To display this PropertyManager:

Open a part that has an open profile sketch as the profile, and a sketch or a series of existing sheet metal edges as the path.

The PropertyManager has different options available based on selections you make.

Sheet Metal Parameters From Material

Use material sheet metal parameters Uses sheet metal parameters attached to the selected material.

Profile and Path

Profile Sets the open, non-intersecting profile sketch used to create the sweep. Select the profile sketch in the graphics area or FeatureManager design tree.
Path Sets the path along which the profile sweeps. You can select a sketch or a series of existing sheet metal edges for the path. Select the path sketch in the graphics area or FeatureManager design tree. Select the path edges in the graphics area.

Path requirements:

  • The path can be open or closed, and can be a set of sketched curves contained in one sketch, a curve, or a set of model edges. If the path is a sketch, it must be an open profile. If the path is a selection of adjoining edges, the path can be a closed profile.
  • The start point of the path must lie on the plane of the profile.
  • A set of sketched curves (lines and arcs) must meet at end points (C0 - positional continuity). Any sharp corner is automatically filleted with appropriate radii. There are two different radii on each side of the path to create the swept flange. The filleting will fail if a fillet cannot be made for the round corner, usually because the edges to be filleted are too short. In this case, the swept flange will fail.
  • No additional filleting is created for a round corner, even if the radius of the round corner is smaller than the necessary radius to create the swept flange. If the radius of the round corner is too small, the swept flange will fail.
  Flatten along path

When selected, the profile is flattened. Then, the profile is rotated parallel to the plane of the path, but the path is not flattened. The result is a flat pattern shape similar to the shape of the path.

When you select Flatten along path, you can also select Material inside. Depending on the geometry, the flat pattern may only succeed when Material inside is selected or cleared. The flat pattern may fail for either choice of Material inside because of self-intersecting geometry on flattening.

When cleared, in flat patterns, the profile is flattened. Then, the profile is rotated perpendicular to the plane of the path. The path is flattened and the result is a rectangular shape.
Selected Cleared

For flat patterns, the software calculates a linear calculation. Compression and stretching of the material are not taken into account.

Flange Parameters

Use default radius Uses the bend radius from the original sheet metal feature.
Bend Radius Lets you change the bend radius from the original sheet metal feature.
Flange position Select a bend position.
Trim side bends Removes extra material in neighboring bends.

Start/End Offset

Lets you set a value for Start Offset Distance and End Offset Distance . (If you want the swept flange to span the entire edge of the model, set these values to zero.)

Custom Bend Allowance

Bend Allowance Type Lets you set a different value from the default value.

Custom Relief Type

Relief Type Sets the type of relief cut to be added: Rectangular, Tear, or Obround.
Use relief ratio If Relief Type is Rectangular or Obround and you select Use relief ratio, set a value for Ratio. If you clear Use relief ratio, set values for Relief Width and Relief Depth .

Cylindrical/Conical Bodies

Only available when the selected path along which the profile sweeps is a sketch.

Cylindrical/Conical Bodies When selected, propagates the sketch in the Cylindrical/Conical Edge field to the flat pattern feature as a fixed entity.
Cylindrical/Conical Bodies selected Cylindrical/Conical Bodies cleared
Cylindrical/Conical Edge Specifies the linear sketch entity to be propagated to the flat pattern feature.
Selected linear sketch entity

Sheet Metal Parameters

  Override default parameters Lets you change the bend radius or thickness from the original sheet metal feature.
Thickness Sets the material thickness.
  Reverse direction Changes the direction in which the sheet thickness is applied.
Bend Radius Set a value when Use default radius is cleared.

Bend Allowance

Override default parameters Lets you change the bend allowance from the original sheet metal feature.
Bend Allowance Type Lets you change the bend allowance from the original sheet metal feature.

Auto Relief

Override default parameters Lets you change the relief type from the original sheet metal feature.
Relief Type Sets the type of relief cut to be added: Rectangular, Tear, or Obround.
Use relief ratio If Relief Type is Rectangular or Obround and you select Use relief ratio, set a value for Ratio. If you clear Use relief ratio, set values for Relief Width and Relief Depth .