Universal Tapping Cycle G31 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Thread cycles

Universal tapping cycle G31

G31 machines single threads, successions of threads and multi-
start threads defined with G24, G34 or G37-Geo. G31 can also
machine a threading contour defined directly after the cycle call and
concluded by G80.
Parameters:
ID: Auxiliary contour – ID number of the contour to be
machined
NS: Contour start block no. – reference to basic element G1-
Geo (for successions of threads: block number of the first basic
element)
NE: Contour end block no. – reference to basic element G1-
Geo (for successions of threads: block number of the first basic
element)
O: Char.start/end – machine form element
0: No machining
1: At beginning
2: At end
3: At beginning and end
4: Only chamfer/rounding (requirement: the contour
section consists of a single element)
J: Thread orientation – reference direction
From 1st contour element
0: Longitudinal
1: Plane
I: Max. approach
No input and V = 0 (constant chip cross section): I = 1/3 * F
IC: Number of cuts – the infeed is calculated from IC and U
Usable with:
V = 0: Constant chip cross section
V = 1: Constant infeed
B: Run-in lgth
(No input: The run-in length is determined from the contour)
If this is not possible, the value is calculated from the kinematic
parameters. The thread contour is extended by the value B.
P: Overflow length
No input: The run-out length is determined from the contour. If
this is not possible, the value is calculated. The thread contour is
extended by the value P.
A: Approach ang. (range: –60° < A < 60°; default: 30°)
V: Type of infeed
0: Const. mach. X-section
1: Const. infeed
2: EPL with distrib. of cuts
3: EPL w/o distrib. of cuts
4: MANUALplus 4110
5: Constant infeed (4290)
6: Const. w/ distrib. (4290)
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
347