Index - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Drilling cycles
Example: G74
. . .
N1 M5
N2 T4 G197 S1000 G195 F0.2 M103
N3 M14
N4 G110 C0
N5 G0 X80 Z2
N6 G745 XK0 YK0 Z2 K80 Wi90 Q4 V2
N7 G74 ZS-40 R2 P12 I2 B0 J8
N8 M15
. . .
Parameter combinations for single holes without contour
description
XS, XE
XS, K
XE, K
The cycle is used for:
Single hole without contour description
Holes with contour definition (individual hole or hole pattern)
1. Boring depth P is used for the first pass. With each subsequent
pass the drilling depth is reduced by the Reducing value I, but
without falling below the Min.drill.depth J. After each pass, the
tool is retracted either by Return distance B or to the starting point
of the hole. If the inside Safety clearance R is defined, the tool is
positioned to this distance at rapid traverse inside the hole.
Feed rate reduction:
Indexable insert drill and twist drill with 180° drilling angle
A feed rate reduction is only effective if the parameter Tap/
Drill. lth A has been defined
Other drills
Beginning of hole: Feed rate reduction as programmed in V
End of hole: Reduction as of hole end point—length of first
cut—safety clearance
Length of first cut = tool tip
Set-up clearance
Further information:
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
ZS, ZE
ZS, K
ZE, K
"Safety clearance", Page 310
Drilling
4
379