0 votes
in cnc programming by (9.4k points)

In this article, we describe how to use Siemens POCKET4 code on CNC machines with all details and examples.

Use this cycle to machine circular pockets in the machining plane either “plane-wise” or “helically”.
For finishing, a face cutter is required.
The depth infeed will always start at the pocket center point and be performed vertically from there; thus it is practical to predrill at this position.

New functions compared to POCKET2:

  • The milling direction can be specified via a G command (G2/G3) or as up-cut or down-cut milling from the spindle direction.
  • For solid machining, the maximum infeed width in the plane can be programmed.
  • Finishing allowance also at the base of the pocket.
  • Two different insertion strategies:

– vertically to the pocket center
– along a helical path around the pocket center

  • Short paths during approach in the plane when finishing.
  • Consideration of a blank contour in the plane and a blank dimension at the base (optimum machining of preformed pockets possible).
  • MIDA is recalculated during edge machining.
  • Helical machining of circular pockets.


POCKET4 (_RTP, _RFP, _SDIS, _DP, _PRAD, _PA, _PO, _MID, _FAL, _FALD, _FFP1, _FFD, _CDIR, _VARI, _MIDA, _AP1, _AD, _RAD1, _DP1,)

_RTP = Retraction plane (absolute)
_RFP = Reference plane (absolute)
_SDIS = Safety clearance (to be added to the reference plane, enter without sign)
_DP = Pocket depth (absolute)
_PRAD = Pocket radius
_PA = Pocket center point, abscissa (absolute)
_PO = Pocket center point, ordinate (absolute)
_MID = Maximum infeed depth or maximum pitch with _VARI = helical (enter without sign)
_FAL = Finishing allowance at the pocket edge (enter without sign)

_FALD = Final machining allowance at base (enter without sign)
_FFP1 = Feedrate for surface machining
_FFD = Feedrate for depth infeed
_CDIR = Milling direction: (enter without sign);
Values:0: Down-cut milling (corresponds to direction of spindle rotation)
1: Down-cut milling
2: with G2 (independent of spindle direction)
3: with G3
_VARI = Machining type: (enter without sign)
UNITS DIGIT: Machining process
1: Roughing
2: Finishing
0: Perpendicular to pocket center with G0
1: Perpendicular to pocket center with G1
2: On helical path:
THOUSANDS DIGIT: Milling technology
0: Plane-wise
1: Helical
The other parameters can be selected as options. They define the insertion strategy and overlapping for solid machining:
_MIDA = Maximum infeed width as a value in solid machining in the plane

_AP1 = Blank pocket radius dimension in reference plane (incremental)
_AD = Blank pocket depth dimension from reference plane (incremental)
_RAD1 = Radius of the helical path during insertion (referred to the tool center point path)
_DP1 = Insertion depth per 360° revolution on insertion along helical path


With this program, you can make a circular pocket in the YZ plane (G19). The center point is determined by Y50 Z50. The infeed axis for the depth infeed is the X axis. Neither finishing dimension nor safety clearance is specified. The pocket is machined with down-cut milling. Infeed is performed along a helical path.

Siemens CNC Milling POCKET4 Program Example

N10 G19 G90 G0 S650 M3 ; Specification of technology values
N15 T20 D1 ;
N17 M6 ;
N20 Y50 Z50 ; Approach start position
N30 Pocket4 (3, 0, 0, -20, 25, 50, 50, 6, 0, 0, 200, 100, 1, 21, 0, 0, 0, 2, 3) ; Cycle call
N40 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.