Siemens CNC Milling | POCKET4 | Milling a Circular Pocket

POCKET4 Introduction

Use this cycle (POCKET4) 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.

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 Format

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 (following) 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

POCKET4 Examples

POCKET4 CNC Program Example – 1

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