Siemens CNC Milling | CYCLE72 | Path Milling


CYCLE72 Introduction

With CYCLE72, you mill along any user-defined contour. The cycle operates with or without
cutter radius compensation.

The contour does not need to be closed; internal or external machining is defined by the position of the cutter radius compensation (central, left or right of contour). The contour must be programmed in the direction in which it is to be milled and must be located in one plane.

In addition, it must also consist of at least 2 contour blocks (starting and finishing point) because the contour subroutine is called directly within the cycle.

NOTICE: A tool compensation must be programmed before the cycle is called. Otherwise, the cycle is aborted and alarm 61000 “No tool compensation active” is output.

Functions of the CYCLE72

  • Selection of roughing (one-time circumnavigation parallel to the contour while taking into account a finishing allowance at several depths, if necessary, up to the finishing allowance) and smoothing (one-time circumnavigation of the final contour at several depths, if necessary).
  • Soft approach and return from the contour, either tangentially or radially (quadrant or semicircle).
  • Depth infeeds can be programmed.
  • Intermediary motions can be carried out in rapid traverse or with feedrate.

CYCLE72 Format

CYCLE72 (_KNAME, _RTP, _RFP, _SDIS, _DP, _MID, _FAL, _FALD, _FFP1, _FFD, _VARI, _RL, _AS1, _LP1, _FF3, _AS2, _LP2)

Parameters

_KNAME = Name of contour subroutine
_RTP = Retraction plane (absolute)
_RFP = Reference plane (absolute)
_SDIS = Safety clearance (to be added to the reference plane, enter without sign)
_DP = Depth (absolute)
_MID = Maximum infeed depth (incremental, enter without sign)
_FAL = Finishing allowance at the edge contour (enter without sign)
_FALD = Finishing allowance at the base (incremental, enter without sign)
_FFP1 = Feedrate for surface machining
_FFD = Feedrate for depth infeed (enter without sign)
_VARI = Machining type: (enter without sign)
Values:
UNITS DIGIT: Machining process
1: Roughing
2: Finishing
TENS DIGIT: Intermediate paths
0: Intermediate paths with G0
1: Intermediate paths with G1
HUNDREDS DIGIT: Retraction
0: Retraction at contour end to _RTP
1: Retraction at contour end to _RFP + _SDIS
2: Retraction at contour end by _SDIS
3: No retraction at contour end
_RL = Traveling around the contour either centrally, to the right or to the left (with G40, G41 or G42; enter without sign)
Values: 40: G40 (approach and return only in straight line); 41: G41 ;42: G42
_AS1 = Specification of the approach direction/approach path: (enter without sign)
Values:
UNITS DIGIT: Approach path
1: Straight line tangential
2: Quadrant
3: Semicircle
TENS DIGIT: Plane/3-D
0: Approach contour in the plane
1: Approach contour on a three-dimensional path
_LP1 = Length of the approach travel (with straight-line) or radius of the approach arc (with circle) (enter without sign)
The other parameters can be selected as options.
_FF3 = Retraction feedrate and feedrate for intermediate positions in the plane (in the open)
_AS2 = Specification of the return direction/retraction path: (enter without sign)
Values:
UNITS DIGIT: Approach path
1: Straight line tangential
2: Quadrant
3: Semicircle
TENS DIGIT: Plane/3-D
0: Return from contour in the plane
1: Return from contour on a three-dimensional path
_LP2 = Length of the retraction travel (with straight-line) or radius of the retraction arc (with circle) (enter without sign)

CYCLE72 Examples

CYCLE72 CNC Program Example – 1

This program is used to mill a contour as shown in the figure.

Siemens CNC Milling CYCLE72 Program Example

Parameters for the cycle call
_RTP Retraction plane = 250 mm
_RFP Reference plane = 200
_SDIS Safety clearance = 3 mm
_DP Depth = 175 mm
_MID Maximum depth infeed = 10 mm
_FAL Finishing allowance in plane = 1 mm
_FALD Finishing allowance in depth = 1.5 mm
_FFP1 Feedrate in the plane = 800 mm/min
_FFD Feedrate depth infeed = 400 mm/min
_VARI Machining type = Roughing up to finishing allowance; intermediate paths with G1, for intermediate paths retraction in Z to _RFP + _SDIS

Parameters for approach:
_RL G41 – left of the contour, i.e. external machining = 41
_LP1 Approach and return in a quadrant in the plane = 20 mm radius
_FF3 Retraction feedrate = 1,000 mm/min

Program :
N10 T20 D1 ; T20 Milling cutter with radius 7
N15 M6 ; Changing tool T20,
N20 S500 M3 F3000 ; Program feedrate and spindle speed
N25 G17 G0 G90 X100 Y200 Z250 G94 ; Approach start position
N30 CYCLE72 (“MYCONTOUR”, 250, 200, 3, 175, 10,1, 1.5, 800, 400, 111, 41, 2, 20, 1000, 2, 20) ; Cycle call
N90 X100 Y200 ;
N95 M02 ; Program end
%_N_MYCONTUR_SPF ; Subroutine for contour milling (for ;example)
;$PATH=/_N_SPF_DIR
N100 G1 G90 X150 Y160 ; Starting point of contour
N110 X230 CHF=10
N120 Y80 CHF=10
N130 X125
N140 Y135
N150 G2 X150 Y160 CR=25
N160 M17

CYCLE72 CNC Program Example – 2

(Milling around a closed contour externally)
With this program, the same contour is milled as in example 1. The difference is that the
contour programming is now in the calling program.

$TC_DP1[20,1]=120 $TC_DP6[20,1]=7
N10 T20 D1 ; T20 Milling cutter with radius 7
N15 M6 ; Changing tool T20,
N20 S500 M3 F3000 ; Program feedrate and spindle speed
N25 G17 G0 G90 G94 X100 Y200 Z250 CYCLE72 (“START:END”, 250, 200, 3, 175, 10,1, 1.5, 800, 400, 11, 41, 2, 20, 1000, 2, 20) ; Approach start position and cycle call
N30 G0 X100 Y200
N35 GOTOF END
START:
N100 G1 G90 X150 Y160
N110 X230 CHF=10
N120 Y80 CHF=10
N130 X125
N140 Y135
N150 G2 X150 Y160 CR=25
END:
N160 M02