Chamfer, Rounding (Chf, Chr, Rnd, Rndm, Frc, Frcm) - Siemens Sinumerik 840D sl Programming Manual

Syntax
G63 X... Y... Z...
Meaning
G63:
X... Y... Z... :
Note
G63 is non-modal.
After a block with programmed G63, the last interpolation command programmed (G0, G1, G2,
etc.) is reactivated.
Feedrate
Note
The programmed feedrate must match the ratio of the speed to the thread lead of the tap.
Thumb rule:
Feedrate F in mm/min = spindle speed S in rpm * thread lead in mm/rev
Not only the feedrate, but also the spindle speed override switch are set to 100% with G63.
Example
In this example, an M5 thread is to be drilled. The lead of an M5 thread is 0.8 (according to
the table).
With a selected speed of 200 rpm, the feedrate F = 160 mm/min.
Program code
N10 G1 X0 Y0 Z2 S200 F1000 M3
N20 G63 Z-50 F160
N30 G63 Z3 M4
N40 M30
10.12

Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)

Contour corners within the active working plane can be executed as roundings or chamfers.
For optimum surface quality, a separate feedrate can be programmed for chamfer/rounding.
If a feedrate is not programmed, the standard path feedrate F will be applied.
The "Modal rounding" function can be used to round multiple contour corners in the same way
one after the other.
Fundamentals
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
10.12 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Tapping with compensating chuck
Drilling depth (end point) in Cartesian coordinates
Comment
; Approach starting point, activate spindle.
; Tapping, drilling depth 50.
; Retraction, programmed reversal of direction.
; End of program
Motion commands
239