Corner Break Parameters
Use the Corner Break Parameters dialog
box to automatically create radii or chamfers on all outer corners
of Lathe finish toolpaths. You can also set the feed rate when
the tool creates the radii or chamfers.
Creating a radius
When creating a radius, the angle of the original corner must
fall within the maximum and minimum range that you enter.
Creating a chamfer
When creating a chamfer, the angle of the outer corner must
equal 90 degrees. If it does not, you can compensate for the difference
by adjusting the angle tolerance. The angle tolerance determines
how far the corner can vary from 90 degrees and still have a chamfer
added. For example, if the angle tolerance is 5 degrees, the corner
can be between 85 and 95 degrees and still have a chamfer added.
Parameters
Radius corners
Select to create a radius on all sharp, outside corners of the toolpath and enter values in the Radius fields.
Chamfer 90 degree corners
Select to create a chamfer on all sharp, outside angle corners that measure 90 degrees
and are L-shaped. The corners cannot be 90 degrees and tipped. Enter values in the Chamfer fields.
Radius
Sets the radius on the corner.
Maximum angle
Enter the maximum angle for the corners. Mastercam creates a radius only on outer corners whose
angle values fall within the maximum and minimum ranges you enter.
Minimum angle
Enter the minimum angle for the corners. Mastercam creates a radius only on outer corners whose
angle values fall within the maximum and minimum ranges you enter.
Height/Width
Enter the height/width of the chamfer.
Radius: Chamfer
Enter the radius that you want to create on the chamfer's outer corners.
Angle tolerance
Determines how far the corner can vary from 90 degrees and still have a chamfer added.
For example, if the corner tolerance is 5 degrees, then each side of the corner can
vary by 5 degrees, allowing the corner value to be between 80 and 100 degrees so
a chamfer can be added.
Same as toolpath
Select to set the corner break feed rate to that of the toolpath feed rate.
Feed rate
Select this option and enter the feed rate to be used for the corner break moves
if they will be different from the toolpath. Select the feed rate units:
- in/rev or mm/rev: Calculates the value in inches or millimeters per revolution.
- in/min or mm/min:
Calculates the value in inches or millimeters per minute.
- micro-in or microns:
Lets you enter a theoretical surface finish value in micro-inches, or microns. Surface
finish refers to the depth of the grooves created on the surface of the part by the
insert and is determined by several factors including the insert corner radius, coolant,
machine vibration, and feed rate/revolution. The software converts the value you
enter to a feed rate/revolution that will give you a surface finish close to the
one entered. The feed rate calculation varies for different radius arcs, but is the
same for linear moves. Since microns are very small units, the numbers entered in
the feed rate text box will be relatively large.
Minimum number of revs
Select to set the feed rate for the corner break moves based on a set
number of revolutions. Enter a value to determine the minimum number of revolutions
while cutting the corner. When selected, this option slows down the feed rate on
the corner break only if it is too fast to make the minimum number of revolutions
while cutting the corner at the toolpath feed rate.