4. INTERPOLATION FUNCTIONS
The distance between an arc and the center of a circle that contains the arc
can be specified using the radius, R, of the circle instead of I, J, and K.
In this case, one arc is less than 180°, and the other is more than 180° are
considered. When an arc exceeding 180° is commanded, the radius must
be specified with a negative value. If Xp, Yp, and Zp are all omitted, if
the end point is located at the same position as the start point and when
R is used, an arc of 0° is programmed
G02R ; (The cutter does not move.)
For arc (1)(less than 180°)
G91 G02 X
20.0 R50.0 F300.0 ;
For arc (2)(greater than 180°)
G91 G02 X
20.0 R–50.0 F300.0 ;
The feedrate in circular interpolation is equal to the feed rate specified by
the F code, and the feedrate along the arc (the tangential feedrate of the
arc) is controlled to be the specified feedrate.
The error between the specified feedrate and the actual tool feedrate is
±2% or less. However, this feed rate is measured along the arc after the
cutter compensation is applied
If I, J, K, and R addresses are specified simultaneously, the arc specified
by address R takes precedence and the other are ignored.
If an axis not comprising the specified plane is commanded, an alarm is
For example, if axis U is specified as a parallel axis to X axis when plane
XY is specified, an alarm (No.028)is displayed.
D Punching (1–cycle pressing) is not performed in G02 and G03 mode.
D If T command is specified in G02 and G03 mode, however, when T
code is specified independently and NMG (No. 16181#0) is set, an
alarm (No. 4600) doesn’t occur.
D Arc radius