Thread Cutting - Siemens SINUMERIK 808D User Manual

See the following illustration for feedrate override G901 with internal/external machining:
C o rrected feedrate
● External machining:
F = F (r + r
corr. prog. cont tool
● Internal machining:
F = F (r - r
korr. prog. cont tool
r : Radius of the circle contour
cont
r : Tool radius
tool
Programming example
N10 G42 G1 X30 Y40 F1000
N20 CFC F350
N30 G2 X50 Y40 I10 J-7 F350
N40 G3 X70 Y40 I10 J6 F300
N50 CFTCP
N60 M30
11.5

Thread cutting

11.5.1 Thread cutting with constant lead: G33
Fu n ctionality
This requires a spindle with position measuring system.
The function G33 can be used to machine threads with constant lead of the following type: If an appropriate tool is used,
tapping with compensating chuck is possible.
The compensating chuck compensates the resulting path differences to a certain limited degree.
The drilling depth is specified by specifying one of the axes X, Y or Z; the thread pitch is specified via the relevant I, J or K.
G33 remains active until canceled by another instruction from this G group (G0, G1, G2, G3...).
R i ght-hand or left-hand thread
Right-hand or left-hand thread is set with the rotation direction of the spindle (M3 right (CW), M4 left (CCW) - see Section
"Spindle movements (Page 109)"). To do this, the rotation value must be programmed under address S or a rotation speed
must be set.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
) / r
cont
) / r
cont
; Tool radius compensation ON
; Feedrate override with circle ON
; Feed value acts on contour
; Feed value acts on contour
; Feedrate override OFF, programmed feedrate value acts at the
milling cutter center point
101