Siemens CNC Milling | POCKET2 | Milling Circular Pockets

In this article, we describe how to use POCKET2 to machine circular pockets in Siemens CNC controlled milling (machine centre) machines with all details and examples.


POCKET2 Introduction

The cycle (POCKET2) is a combined roughing-finishing cycle. Use this cycle to machine circular pockets in the machining plane.

NOTICE: The cycle requires a milling cutter with an “end tooth cutting across center” (DIN844).

Note: The pocket milling cycle POCKET4 can be performed with any tool.

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

Supported CNC Series

Siemens CNC 802D, 810D, 840D, 840D sl, 840Di, 840Di sl series controllers.

POCKET2 Format



RTP = Retraction plane (absolute)
RFP = Reference plane (absolute)
SDIS = Safety clearance (enter without sign)
DP = Pocket depth (absolute)
DPR = Pocket depth relative to the reference plane (enter without sign)
PRAD = Pocket radius (enter without sign)
CPA = Pocket center point, abscissa (absolute)
CPO = Pocket center point, ordinate (absolute)
FFD = Feedrate for depth infeed
FFP1 = Feedrate for surface machining
MID = Maximum infeed depth for one infeed (enter without sign)
CDIR = Mill direction for machining the pocket ( Values: 2: (for G2); 3: (for G3) )
FAL = Finishing allowance at the pocket edge (enter without sign)
VARI = Machining type ( Values: 0: Complete machining; 1: Roughing; 2: Finishing )
MIDF = Maximum infeed depth for finishing
FFP2 = Feedrate for finishing
SSF = Speed when finishing

POCKET2 Examples

POCKET2 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, the pocket depth is entered as an absolute value. Neither finishing dimension nor safety clearance is specified.

Siemens CNC Milling POCKET2 Program Example

DEF REAL RTP=3, RFP=0, DP=-20, PRAD=25, FFD=100, FFP1, MID=6 ; Definition of variables with value assignments
N10 FFP1=FFD*2 ;
N20 G19 G90 G0 S650 M3 ; Specification of technology values
N25 T10 D1 ;
N27 M6 ;
N30 Y50 Z50 ; Approach start position
N40 POCKET2 (RTP, RFP, , DP, , PRAD, 50, 50, FFD, FFP1, MID, 3, ) ; Cycle call; Parameters FAL, VARI, MIDF, FFP2, ;SSF are omitted
N50 M30 ; Program end
DEF REAL RTP=3, RFP=0, DP=-20, PRAD=25, FFD=100, FFP1, MID=6 ; Definition of variables with value assignments

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 | POCKET1 | Milling Rectangular Pockets
Next articleSiemens CNC Milling | POCKET3 | Milling a Rectangular Pocket