Helix Interpolation: G2/G3, Turn; Feedrate Override For Circles: Cftcp, Cfc - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

8.4.4

Helix interpolation: G2/G3, TURN

Functionality
With helix interpolation, two movements are overlaid:
● Circular movement in the G17, G18 or G19 plane
● Linear movement of the axis standing vertically on this plane.
The number of additional full-circle passes is programmed with TURN=. These are added to the actual circle
programming.
The helix interpolation can preferably be used for the milling of threads or of lubricating grooves in cylinders.
Programming
G2/G3 X... Y... I... J... TURN=...
G2/G3 CR=... X... Y... TURN=...
G2/G3 AR=... I... J... TURN=...
G2/G3 AR=... X... Y... TURN=...
G2/G3 AP=... RP=... TURN=...
See the following illustration for helical interpolation:
Programming example
N10 G17
N20 G0 Z50
N30 G1 X0 Y50 F300
N40 G3 X0 Y0 Z33 I0 J-25 TURN= 3
M30
8.4.5

Feedrate override for circles: CFTCP, CFC

Functionality
For activated tool radius compensation (G41/G42) and circle programming, it is imperative to correct the feedrate at the
cutter center point if the programmed F value is to act at the circle contour.
Internal and external machining of a circle and the current tool radius are taken into account automatically if the tool radius
compensation is enabled.
This feedrate correction (override) is not necessary for linear paths. The path velocities at the cutter center point and at the
programmed contour are identical.
78
; Center and end points
; Circle radius and end point
; Opening angle and center point
; Opening angle and end point
; Polar coordinates, circle around the pole
; X/Y plane, Z standing vertically on it
; Approach starting point
; Helix
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014