Fanuc Series 15i/150i-MA (Programming) Operators Manual

4.INTERPOLATION FUNCIONS PROGRAMMING B-63324EN/03
- 92 -
- Choosing from two types of involute curves
When only a start point and I, J, and K data are given, two types of
involute curves can be created. One type of involute curve extends
towards the base circle, and the other extends away from the base circle.
When the specified end point is closer to the center of the base circle
than the start point, the involute curve extends toward the base circle.
In the opposite case, the involute curve extends away from the base
circle.
- Feedrate
The cutting feedrate specified in an F code is used as the feedrate for
involute interpolation. The feedrate along the involute curve (feedrate
along the tangent to the involute curve) is controlled to satisfy the
specified feedrate.
- Plane selection
As with circular interpolation, the plane to which to apply involute
interpolation can be selected using G17, G18, and G19.
- Cutter compensation
Cutter compensation can be applied to involute curve machining. As
with linear and circular interpolation, G40, G41, and G42 are used to
specify cutter compensation.
G40:Cutter compensation cancel
G41:Cutter compensation left
G42:Cutter compensation right
At each of the start and end points of an involute curve, an intersection
point with a straight line or arc is approximated. The involute curve
passing through the obtained intersection points at the start and end
points is used as the tool center path.
In involute interpolation mode, the G codes for cutter compensation,
which are G41, G42, and G40, cannot be specified.
- Automatic speed control
To improve the machining precision, an override can be automatically
applied to the specified feedrate during involute interpolation. See II-
5.5.1 for details.
- Specifiable G codes
The following G codes can be specified in involute interpolation mode:
G04:Dwell
G10:Data setting
G17:X-Y plane selection
G18:Z-X plane selection
G19:Y-Z plane selection
G65:Macro call
G66:Macro modal call
G67:Macro modal call cancel
G90:Absolute command
G91:Incremental command

Leave a Reply

Your email address will not be published. Required fields are marked *