0 votes
24 views
in cnc programming by (9.4k points)

In this article, we describe how to use Siemens CYCLE77 code on CNC machines with all details and examples.

Use this cycle to machine circular spigots in the machining plane. For finishing, a face cutter is required. The depth infeed is always carried out in the position upstream of the semicircle style approach to the contour.

Format

CYCLE77 (_RTP, _RFP, _SDIS, _DP, _DPR, _PRAD, _PA, _PO, _MID, _FAL, _FALD, _FFP1, _FFD, _CDIR, _VARI, _AP1)

The following input parameters are always required:
_RTP = Retraction plane (absolute)
_RFP = Reference plane (absolute)
_SDIS = Safety clearance (to be added to the reference plane, enter without sign)
_DP = Depth (absolute)
_DPR = Depth relative to the reference plane (enter without sign)
_PRAD = Spigot diameter (enter without sign)
_PA = Center point of spigot, abscissa (absolute)
_PO = Center point of spigot, ordinate (absolute)
_MID = Maximum depth infeed (incremental; enter without sign)
_FAL = Final machining allowance on edge contour (incremental)
_FALD = Finishing allowance at the base (incremental, enter without sign)
_FFP1 = Feedrate on contour
_FFD = Feedrate for depth infeed (or spatial infeed)
_CDIR = Milling direction: (enter without sign)
Values: 0: Down-cut milling
1: Down-cut milling
2: with G2 (independent of direction of spindle rotation)
3: with G3
_VARI = Machining type
Values: 1: Roughing to finishing allowance
2: Smoothing (allowance X/Y/Z=0)
_AP1 = Diameter of blank spigot

Example

Machining a spigot from a blank with a diameter of 55 mm and a maximum infeed of 10 mm per cut; specification of a final machining allowance for subsequent finishing of the spigot surface. The whole machining is performed with reverse rotation.

Siemens CNC Milling CYCLE77 Program Example

N10 G90 G17 G0 S1800 M3 D1 T1 ; Specification of technology values
N11 M6 ;
N20 CYCLE77 (10, 0, 3, -20, ,50, 60, 70, 10, 0.5, 0, 900, 800, 1, 1, 55) ; Roughing cycle call
N30 D1 T2 M6 ; Change tool
N40 S2400 M3 ; Specification of technology values
N50 CYCLE77 (10, 0, 3, -20, , 50, 60, 70, 10, 0, 0, 800, 800, 1, 2, 55) ; Finishing cycle call
N60 M30 ; Program end

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...