Part Modeling > Engineering Features > Chamfer > Advanced Topics > Piece Management > To Extend Chamfer Geometry
To Extend Chamfer Geometry
1. Select the references for the chamfer and on the Model tab, click the arrow next to Chamfer, and click Edge Chamfer. The Edge Chamfer tab opens.
2. Click the Pieces tab and select the chamfer piece to extend from the Pieces table. Handles appear on the piece ends.
* If you have a closed-loop chamfer set, you need to open it by removing a patch. After you select the piece to trim, select a patch from the graphics window. The patch is removed, and handles appear.
3. Drag a handle to extend the piece. As you drag, the potential extension of the chamfer piece appears. Follow the extension up to the patch where you want to extend the piece. The chamfer piece is extended up to the patch. Notice that Edited appears in the Pieces table for the selected piece. Repeat the process if needed.
4. To extend another chamfer piece, repeat step 2. and step 3.
5. To return the piece to its original state, select Included from the Pieces table or on the Pieces tab shortcut menu.
6. The extended chamfer piece is complete. Close the Pieces tab to activate Sets mode and continue to work with chamfers.
7. When completed, click to create the chamfer and close the Chamfer tool.
If you extended multiple pieces in the current chamfer set and want to quickly restore all of them to their original state, select All included on the Pieces tab shortcut menu.
To quickly locate a piece on your model, place your cursor over each piece in the Pieces table and it is dynamically highlighted in the graphics window.