Thread Milling - Cycle70 - Siemens SINUMERIK 840D sl Programming Manual

Note
The cycle is provided with new functions that are not on earlier software versions.
Consequently certain parameters in the input mask (
Multiple slots on one position pattern can be programmed using "MCALL" and calling the
desired position pattern, e.g. HOLES2.
18.1.24

Thread milling - CYCLE70

Programming
CYCLE70(REAL _RTP, REAL _RFP, REAL _SDIS, REAL _DP, REAL _DIATH,
REAL _H1, REAL _FAL, REAL _PIT, INT _NT, REAL _MID, REAL _FFR, INT
_TYPTH, REAL _PA, REAL _PO, REAL _NSP, INT _VARI, INT _PITA,
STRING[15] _PITM, STRING[20] _PTAB, STRING[20] _PTABA, INT _GMODE,
INT _DMODE, INT _AMODE)
Parameters
No. Param Param
mask internal
1 RP _RTP
Z0 _RFP
2
SC _SDIS
3
4 Z1 _DP
5 _DIATH
∅
H1 _H1
6
7 U _FAL
8 P _PIT
9 NT _NT
DXY _MID
10
11 F _FFR
12 _TYPTH
13 X0 _PA
14 Y0 _PO
Job Planning
Programming Manual, 03/2013, 6FC5398-2BP40-3BA1
Explanation
Retraction plane (abs)
Reference point of tool axis (abs)
Safety clearance (to be added to reference point, enter without sign)
Thread length (abs/inc), see _AMODE
Take account of runout at base of hole (at least half pitch)
Nominal diameter of the thread
Thread depth
Finishing allowance
Pitch (select_PITA: mm, inch, MODULE, threads/inch)
Number of teeth on the tool tip
Tool length is always with respect to bottom tooth.
Maximum infeed per cut
_MID > _H1: all in one cut
Milling feed
Thread type
0 = Internal thread
1 = External thread
Circle center 1st axis (abs)
Circle center 2nd axis (abs)
Programming cycles externally
18.1 Technology cycles
, ) are no longer displayed.
NUM, RAD INDA
681