Creating Rods and Tubes with a Circular Profile

You can use the Circular Profile option to create a solid rod or hollow tube along a sketch line, edge, or curve directly on a model without having to sketch. This sweep is available for Swept Boss/Base, Swept Cut, and Swept Surface features.

1. Open install_dir\samples\whatsnew\parts\sweep_part_1.sldprt.

   

2. Click Insert > Cut > Sweep to cut a tube into the part.
3. In the PropertyManager, under Profile and Path, click Circular Profile.
4. In the graphics area, select a curved edge for Path. Then set the Diameter to 50.00mm.
   In the PropertyManager, under Options, Show preview and Align with end faces are selected by default.

   

5. Click .

   The Cut-Sweep feature appears in the FeatureManager design tree.

   

6. Click Insert > Boss/Base > Sweep to add the solid rod.
7. In the PropertyManager, under Profile and Path, click Circular Profile.
8. In the graphics area, select the bottom edge of the part for Path.
9. In the PropertyManager set 20.00 mm for Diameter.

   Show preview and Merge result are selected by default.

10. Click .

    

    The Sweep feature appears in the FeatureManager design tree.