Siemens CNC Milling | CYCLE77 | Circular Spigot Milling

In this article, we describe how to use CYCLE77 for circular spigot milling in Siemens CNC controlled milling (machine centre) machines with all details and examples.


CYCLE77 Introduction

Use this cycle (CYCLE77) 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.

You may be interested also:
“Siemens CNC Milling | CYCLE76 | Rectangular Spigot Milling”

CYCLE77 Format



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

CYCLE77 Examples

CYCLE77 CNC Program Example – 1

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

Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on forums and join us to get support, ask questions, improve a published article or give your opinion.

Previous articleSiemens CNC Milling | CYCLE76 | Rectangular Spigot Milling
Next articleSiemens CNC Milling | CYCLE75 | Transfer Island Contour