Creating a Sheet Metal Part Using Round Bends

When bending sheet metal, you can create round bends instead of sharp bends. The Insert Bends feature also allows you to create rips.

1. Sketch a closed or open profile.
2. Create a thin feature part.
   Depending on the type of profile, you can use tools such as Shell or Extruded Boss/Base to create thin features.

   
   
   
3. Click Insert Bends (Sheet Metal toolbar) or Insert > Sheet Metal > Bends.
4. In the PropertyManager, under Bend Parameters:
   1. Click a face or edge on the model for Fixed Face or Edge . The fixed face remains in place when the part is flattened.
      
      
   2. Set a value for Bend Radius .
5. Under Bend Allowance, select from: Bend Table, K-Factor, Bend Allowance, Bend Deduction, or Bend Calculation.
   • Set a value if you selected K-Factor, Bend Allowance, or Bend Deduction.
   • If you selected Bend Table or Bend Calculation, select a table from the list, or click Browse to browse to a table.
6. Select Auto Relief, then choose the type of relief cut to add relief cuts.
   If you choose Rectangular or Obround, set a Relief Ratio.

   The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
7. To use the rip feature with round bends, under Rip Parameters:
   1. Select internal or external edges (you can also select linear sketch entities).
      
   2. To insert a rip in only one direction, do one of the following:
      • Click the name of the edge listed under Edges to Rip , and click Change Direction.
      • Click the preview arrows.

      
      
      
   3. To change the gap distance, enter a value for Rip Gap .
8. Click .