Base Flange

A base flange is the first feature in a new sheet metal part. When you add a base flange feature to a SolidWorks part, the part is marked as a sheet metal part. Bends are added wherever appropriate, and sheet metal specific features are added to the FeatureManager design tree.

Some additional items to note about a base flange feature:

• The Base-Flange feature is created from a sketch. The sketch can be a single open, a single closed, or multiple-enclosed profiles.

• The thickness and bend radius of the Base-Flange feature become the default values for the other sheet metal features.

To create a Base-Flange feature:

1. Create a sketch that meets the requirements above. Alternatively, you can select the Base-Flange feature before you create a sketch (but after you select a plane). When you select the Base-Flange feature, a sketch opens on the plane.

2. Click Base Flange/Tab on the Sheet Metal toolbar, or click Insert, Sheet Metal, Base Flange.

The controls on the Base Flange PropertyManager update according to your sketch. For example, the Direction 1 and Direction 2 boxes do not appear for a sketch with a single closed profile.

3. If necessary, under Direction 1 and Direction 2, set the parameters for the End Condition and Depth .

4. Under Sheet Metal Parameters:

• Set a value for Thickness to specify the sheet metal thickness.

• Select Reverse direction to thicken the sketch in the opposite direction.

• Set a value for Bend Radius .

5. Under Bend Allowance, select a bend allowance type.

• If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.

• If you selected Bend Table or Bend Calculation, select a table from the list, or click Browse to browse to a table.

6. Under Auto Relief, select a relief type. If you selected Rectangular or Obround:

• Select Use relief ratio and set a value for Ratio.

  - or -

• Clear Use relief ratio and set a value for Relief Width and Relief Depth .

7. Click OK .