Detailed Drawings > Working with Drawing Sketches > Sketching in Drawing > To Create a Chamfer
  
To Create a Chamfer
Chamfers are beveled edges or corners. Within drawings, you can sketch chamfers at the intersection of two draft entities.
The intersecting draft entities do not have to actually touch. The chamfer calculates the appropriate intersection. When you sketch a corner or edge chamfer, the existing intersection is deleted.
1. Click Sketch > Chamfer. The Select dialog box opens.
2. Select the first chamfer reference, such as a point on a model edge or draft entity. Ensure that you select a point close to the desired start point of the chamfer, as your selection point determines the default angle.
3. Press CTRL and select a model edge or draft entity that is the second chamfer reference. If the references are valid, the chamfer previews on the drawing.
 
* You can select multiple sets of references to sketch several chamfers simultaneously.
4. Middle-click or click OK in the Select dialog box to confirm the chamfer references. The Chamfer Properties dialog box opens.
5. Define how you want to dimension the chamfer:
◦ 45 x D—Create a chamfer 45 degrees from the first selected line and of dimension d along both selected lines (where d is determined by point selected on the draft entity)
◦ D x D—Use the same dimension value along both of the selected draft entities
◦ D1 x D2—Use a different chamfer dimension for each draft entity
◦ Angle x D—Use a chamfer dimension at an angle to the draft entity
6. By default, the most recently used chamfer dimension is selected. Select a chamfer dimension from the list or type a new value. If applicable, click to interchange the angle and dimension for the chamfer.
7. Select a trim style to define how to display the intersection being chamfered:
Full trim—Deletes the intersection, displaying only the chamfered intersection.
Thin line trim—Displays the intersection with thin lines, with the chamfer in normal pen width.
Solid line trim—Displays both the intersection and chamfer in the normal pen width, and any overlapping of intersecting chamfer references is trimmed .
Half trim—Displays half the intersection, while deleting one of the extending chamfer reference lines. The chamfer is displayed in normal pen width.
 
* Click to trim the remaining portion of the intersection.
No trim—Displays the entire intersection and chamfer in normal pen width; any overlapping remains.
 
* If you selected multiple sets of chamfer references, and the first and last reference physically intersect, you can select Complete loop to add the same chamfer to all the intersections within the selected references.
8. Click OK in the Chamfer Properties dialog box. The chamfer is created.
 
* You can modify individual chamfers. You can access the chamfer properties in any of the following ways: double-click the fillet, select the chamfer and click Edit > Properties, or right-click the chamfer and click Properties on the shortcut menu.