Siemens CNC Milling | POCKET3 | Milling a Rectangular Pocket


POCKET3 Introduction

The cycle (POCKET3) can be used for roughing and finishing. 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 POCKET1

  • 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.
  • Three different insertion strategies:
    – vertically to the pocket center
    – along a helical path around the pocket center
    – oscillation on the center axis of the pocket
  • 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).

POCKET3 Format

POCKET3 (_RTP, _RFP, _SDIS, _DP, _LENG, _WID, _CRAD, _PA, _PO, _STA, _MID, _FAL, _FALD, _FFP1, _FFD, _CDIR, _VARI, _MIDA, _AP1, _AP2, _AD, _RAD1, _DP1)

Parameters

_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)
_LENG = Pocket length, for dimensioning from the corner with sign
_WID = Pocket width, for dimensioning from the corner with sign
_CRAD = Pocket corner radius (enter without sign)
_PA = Pocket reference point, abscissa (absolute)
_PO = Pocket reference point, ordinate (absolute)
_STA = Angle between the pocket longitudinal axis and the first axis of the plane (abscissa, enter without sign); ( Range of values: 0° ≤ _STA < 180° )
_MID = Maximum infeed depth (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); Values:
UNITS DIGIT: Machining process
1: Roughing
2: Finishing
TENS DIGIT: Infeed
0: Perpendicular to pocket center with G0
1: Perpendicular to pocket center with G1
2: On helical path
3: Oscillation on pocket longitudinal axis
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 dimension of pocket length
_AP2 = Blank dimension of pocket width
_AD = Blank pocket depth dimension from reference plane
_RAD1 = Radius of the helical path on insertion (relative to the tool center point path) or maximum insertion angle for reciprocating motion
_DP1 = Insertion depth per 360° revolution on insertion along helical path

POCKET3 Examples

POCKET3 CNC Program Example – 1

With this program, you can make a pocket with a length of 60 mm, a width of 40 mm, a corner radius of 8 mm and a depth of 17.5 mm in the XY plane (G17). The pocket has an
angle of 0 degrees to the X axis. The final machining allowance of the pocket edges is
0.75 mm, 0.2 mm at the base, the safety clearance in the Z axis, which is added to the
reference plane, is 0.5 mm. The center point of the pocket lies at X60 and Y40, the
maximum depth infeed is 4 mm.

The machining direction results from the direction of rotation of the spindle in the case of down-cut milling. Merely a rough machining operation is to be carried out.

Siemens CNC Milling POCKET3 Program Example

N10 G90 S600 M4 ; Specification of technology values
N15 T10 D1 ;
N17 M6 ;
N20 G17 G0 X60 Y40 Z5 ; Approach start position
N25 _ZSD[2]=0 ; Dimensioning the pocket via the center point
N30 POCKET3 (5, 0, 0.5, -17.5, 60, 40, 8, 60, 40, 0, 4, 0.75, 0.2, 1000, 750, 0, 11, 5) ; Cycle call
N40 M30 ; Program end
N10 G90 S600 M4 ; Specification of technology values
N15 T10 D1 ;