Siemens CNC Milling | POCKET1 | Milling Rectangular Pockets

In this article, we describe how to use POCKET1 to machine rectangular pockets in Siemens CNC controlled milling (machine centre) machines with all details and examples.

0
556

POCKET1 Introduction

The cycle (POCKET1) is a combined roughing-finishing cycle. With this cycle, you can machine rectangular pockets in any position in the machining plane.
NOTICE: The cycle requires a milling cutter with an “end tooth cutting across center” (DIN844).

Note: The pocket milling cycle POCKET3 can be performed with any tool.

You may be interested also:
“Siemens CNC Milling | SLOT2 | Circumferential Slot”

Supported CNC Series

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

POCKET1 Format

POCKET1 (RTP, RFP, SDIS, DP, DPR, LENG, WID, CRAD, CPA, CPD, STA1, FFD, FFP1, MID, CDIR, FAL, VARI, MIDF, FFP2, SSF)

Parameters

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)
LENG = Pocket length (enter without sign)
WID = Pocket width (enter without sign)
CRAD = Corner radius (enter without sign)
CPA = Pocket center point, abscissa (absolute)
CPO = Pocket center point, ordinate (absolute)
STA1 = Angle between longitudinal axis and abscissa ( Range of values: 0<=STA1<180 degrees )
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

POCKET1 Examples

POCKET1 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 (difference between reference plane and pocket base) 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, the safety distance 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. Merely a rough machining operation is to be carried out.

Siemens CNC Milling POCKET1 Program Example

DEF REAL LENG, WID, DPR, CRAD ; Definition of variables
DEF INT VARI
N10 LENG=60 WID=40 DPR=17.5 CRAD=8 ; Value assignments
N20 VARI=1
N30 G90 S600 M4 ; Specification of technology values
N35 T20 D2 ;
N37 M6 ;
N40 G17 G0 X60 Y40 Z5 ; Approach start position
N50 POCKET1 (5, 0, 0.5, , DPR, LENG, WID, CRAD, 60, 40, 0, 120, 300, 4, 2, 0.75, VARI) ; Cycle call; Parameters MIDF, FFP2, and SSF are omitted
N60 M30 ; Program end


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 | SLOT2 | Circumferential Slot
Next articleSiemens CNC Milling | POCKET2 | Milling Circular Pockets