Adding an Extruded Feature

To construct additional features on the part, you must draw sketches on the model faces or planes, and then convert them into features.

1. On the CommandManager, click Features > Extruded Boss/Base.
2. Click on the front face of the model.
3. On the CommandManager, click Sketch > Convert Entities.
4. Click on the circular edge of the model geometry.

1. On the Convert Entities PropertyManager, click OK.

1. On the CommandManager, click Sketch > Line.
2. Click on the circular edge to specify the first point of the line, as shown.

1. Move the pointer towards right.
2. Click on the other side of the circular edge; a line is drawn. In addition, another line is attached to the pointer.

1. Right-click and select End chain (double-click) to end the line.

1. Draw another line below the previous line.

9.Press Esc to deactivate the Line tool.

10.On the CommandManager, click Sketch > Display/Delete Relations > Add Relation.

1. Select the two lines.
2. On the Add Relations PropertyManager, under the Add Relations section, click Horizontal to make the two lines horizontal.
3. Under the Add Relations section, click Equal to make the lines equal in length.

1. Click OK on the PropertyManager.
2. On the CommandManager, click Sketch > Smart Dimension.
3. Select the two horizontal lines.
4. Move the pointer toward right and click to locate the dimension.
5. Type-in 12 in the Modify box and click OK.

1. On the CommandManager, click Sketch > Trim Entities.
2. Click the Trim to Closest icon on the PropertyManager.

1. Click on the arc portions of the projected entity.

The projected entities are trimmed.

1. Click OK on the Trim PropertyManager.
2. On the top right corner of the graphics window, select Exit Sketch.

1. On the Boss-Extrude PropertyManager, type-in 10 in the Depth box, and then click OK.