Using a Base Flange to Add a Body

You can create a body in an existing sheet metal part by using Base Flange/Tab to insert a tab without merging it with the existing part.

1. In a sheet metal part, click Base Flange/Tab (Sheet Metal toolbar) or Insert > Sheet Metal > Base Flange .
2. Draw a sketch on the plane containing the edge where you want to place the body.
   
3. Exit the sketch.
   
4. In the PropertyManager, under Sheet Metal Parameters, clear Merge result.
5. Click .

   Clearing Merge result creates a separate body in the cut list and adds the feature and its flat pattern to the FeatureManager design tree.	If you do not clear Merge result, the tab is added to the original sheet metal body and the FeatureManager design tree, but there is only one body in the cut list and one flat pattern.

6. Draw another sketch on the plane containing the sketches for the two sheet metal bodies, intersecting both bodies.
   
7. Click Base Flange/Tab (Sheet Metal toolbar).
   
8. In the PropertyManager, under Sheet Metal Parameters, click Merge result.
9. Under Feature Scope, select one:
   • All bodies - The added material is merged with both of the existing bodies, resulting in a single sheet metal body.

     

   • Selected bodies - Clear Auto-select to display the Solid Bodies to Affect field, where you can select the body to merge.

     If you select:	the new material is merged with the original body and the tab feature is added to the body's folder in the cut list:
     If you select:	the new material is merged with the body created in steps 1 through 5 and the tab feature is added to the body's folder in the cut list: