Thread Cutting - Cycle90 - Siemens SINUMERIK 840D Programming Manual

03.96
3
08.97
3.3

Thread cutting - CYCLE90

Programming
CYCLE90 (RTP, RFP, SDIS, DP, DPR, DIATH, KDIAM, PIT, FFR, CDIR, TYPTH,
CPA, CPO)
Parameters
RTP
real
RFP
real
SDIS
real
DP
real
DPR
real
DIATH
real
KDIAM
real
PIT
real
FFR
real
CDIR
int
TYPTH
int
CPA
real
CPO
real
Function
You can produce inside and outside threads with
cycle CYCLE90. The path in thread milling is based
on helical interpolation. All three geometrical axes of
the current plane which you define before calling the
cycle are involved in this movement.
The programmed feedrate F depends on the axis
grouping defined in the FGROUP instruction before
the cycle call
(see Programming Guide).
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (enter without sign)
Final drilling depth (absolute)
Final drilling depth relative to reference plane (enter without sign)
Nominal diameter, outside diameter of thread
Core diameter, inside diameter of thread
Thread pitch; Value range: 0.001 ... 2000.000 mm
Feedrate for thread milling (enter without sign)
Direction of rotation for thread milling
Value: 2 (for thread milling with G2)
3 (for thread milling with G3)
Thread type: Values:0= inside thread
1= outside thread
Center point of circle, abscissa (absolute)
Center point of circle, ordinate (absolute)
3.3 Thread cutting - CYCLE90
Milling Cycles
3
3-107