FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

PROGRAMMING
B–62764EN/01
4. INTERPOLATION FUNCTIONS
51
In the polar coordinate interpolation mode, program commands are
specified with Cartesian coordinates on the polar coordinate interpolation
plane. The axis address for the rotation axis is used as the axis address
for the second axis (virtual axis) in the plane. Whether a diameter or
radius is specified for the first axis in the plane is the same as for the
rotation axis regardless of the specification for the first axis in the plane.
The virtual axis is at coordinate 0 immediately after G12.1 is specified.
Polar interpolation is started assuming the angle of 0 for the position of
the tool when G12.1 is specified.
Specify the feedrate as a speed (relative speed between the workpiece and
tool) tangential to the polar coordinate interpolation plane (Cartesian
coordinate system) using F.
G01 Linear interpolation. . . . . . . . . . . .
G02, G03 Circular interpolation. . . . . . . .
G04 Dwell, Exact stop. . . . . . . . . . . .
G40, G41, G42 Cutter compensation . . .
(Polar coordinate interpolation is applied to the path
after cutter compensation.)
G65, G66, G67 Custom macro command. . .
G90, G91 Absolute command, incremental command. . . . . . . .
G94, G95 Feed per minute, feed per revolution. . . . . . . .
The addresses for specifying the radius of an arc for circular interpolation
(G02 or G03) in the polar coordinate interpolation plane depend on the
first axis in the plane (linear axis).
I and J in the Xp–Yp plane when the linear axis is the X–axis or an axis
parallel to the X–axis.
J and K in the Yp–Zp plane when the linear axis is the Y–axis or an axis
parallel to the Y–axis.
K and I in the Zp–Xp plane when the linear axis is the Z–axis or an axis
parallel to the Z–axis.
The radius of an arc can be specified also with an R command.
The tool moves along such axes normally, independent of polar
coordinate interpolation.
Actual coordinates are displayed. However, the remaining distance to
move in a block is displayed based on the coordinates in the polar
coordinate interpolation plane (Cartesian coordinates).
Before G12.1 is specified, a local coordinate system (or workpiece
coordinate system) where the center of the rotary axis is the origin of the
coordinate system must be set. In the G12.1 mode, the coordinate system
must not be changed (G92, G52, G53, relative coordinate reset, G54
through G59, etc.).
The polar coordinate interpolation mode cannot be started or terminated
(G12.1 or G13.1) in the tool offset mode (G41 or G42). G12.1 or G13.1
must be specified in the tool offset canceled mode (G40).
D Distance moved and
feedrate for polar
coordinate interpolation
The unit for coordinates
on the hypothetical axis is
the same as the unit for
the linear axis (mm/inch)
The unit for the feedrate
is mm/min or inch/min
D G codes which can be
specified in the polar
coordinate interpolation
mode
D Circular interpolation in
the polar coordinate
plane
D Movement along axes
not in the polar
coordinate interpolation
plane in the polar
coordinate interpolation
mode
D Current position display
in the polar coordinate
interpolation mode
Limitations
D Coordinate system for
the polar coordinate
interpolation
D Tool offset command

Leave a Reply

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