FANUC Series 16/18/160/180-Model C for Lathe Operator Manual

PROGRAMMING
4. INTERPOLATION FUNCTIONS
B–62754EN/01
52
Before G12.1 is specified, a 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 nose radius compensation mode (G41 or
G42). G12.1 or G13.1 must be specified in the tool nose radius
compensation canceled mode (G40).
For a block in the G12.1 mode, the program cannot be restarted.
Polar coordinate interpolation converts the tool movement for a figure
programmed in a Cartesian coordinate system to the tool movement in the
rotation axis (C–axis) and the linear axis (X–axis). When the tool moves
closer to the center of the workpiece, the C–axis component of the
feedrate becomes larger and may exceed the maximum cutting feedrate
for the C–axis (set in parameter (No. 1422)), causing an alarm (see the
figure below). To prevent the C–axis component from exceeding the
maximum cutting feedrate for the C–axis, reduce the feedrate specified
with address F or create a program so that the tool (center of the tool when
tool nose radius compensation is applied) does not move close to the
center of the workpiece.
WARNING
Consider lines L1, L2, and L3. X is the distance the tool moves
per time unit at the feedrate specified with address F in the
Cartesian coordinate system. As the tool moves from L1 to L2 to
L3, the angle at which the tool moves per time unit corresponding
to X in the Cartesian coordinate system increases fromθ1 toθ 2
to θ3.
In other words, the C–axis component of the feedrate becomes
larger as the tool moves closer to the center of the workpiece.
The C component of the feedrate may exceed the maximum
cutting feedrate for the C–axis because the tool movement in the
Cartesian coordinate system has been converted to the tool
movement for the C–axis and the X–axis.
L : Distance (in mm) between the tool center and workpiece center when the tool center is the
nearest to the workpiece center
R :Maximum cutting feedrate (deg/min) of the C axis
Then, a speed specifiable with address F in polar coordinate interpolation can be given by the
formula below. Specify a speed allowed by the formula. The formula provides a theoretical
value; in practice, a value slightly smaller than a theoretical value may need to be used due to
a calculation error.
L1
L2
L3
θ3
θ2
θ1
X
F < L × R ×
180
π
(mm/min)
Even when diameter programming is used for the linear axis (X–axis),
radius programming is applied to the rotary axis (C–axis).
Restrictions
D
Coordinate system for the
polar coordinate
interpolation
D Tool nose radius
 
D Program restart
D Cutting feedrate for the
rotation axis
D Diameter and radius
programming

Leave a Reply

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