Siemens CNC Milling | POCKET3 | Milling a Rectangular Pocket

In this article, we describe how to use POCKET3 to machine rectangular pockets in Siemens CNC controlled milling (machine centre) machines with all details and examples.

0
586

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).
You may be interested also:
“Siemens CNC Milling | POCKET1 | Milling Rectangular Pockets”

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 ;


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 CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleSiemens CNC Milling | POCKET2 | Milling Circular Pockets
Next articleSiemens CNC Milling | POCKET4 | Milling a Circular Pocket