Siemens CNC Turning | CYCLE93 | Grooving Cycle

In this article, we describe how to use CYCLE93 to grooving in Siemens CNC controlled turning (lathe) machines with all details and examples.


CYCLE93 Introduction

With the grooving (CYCLE93) cycle, you can make symmetrical and asymmetrical grooves for longitudinal and face machining on straight contour elements. You can machine both
external and internal grooves.

You may be interested also:
“Siemens CNC Milling | CYCLE60 | Engraving Cycle”

CYCLE93 Format



SPD = Starting point in the facing axis (enter without sign)
SPL = Starting point in the longitudinal axis
WIDG = Groove width (enter without sign)
DIAG = Groove depth (enter without sign)
STA1 = Angle between contour and longitudinal axis; Range of values: 0 ≤ STA1 ≤ 180 degrees
ANG1 = Flank angle 1: on the groove side determined by the starting point (enter without sign); Range of values: 0 ≤ ANG1 < 89.999 degrees
ANG2 = Flank angle 2: on the other side (enter without sign) ; Range of values: 0 ≤ ANG2 < 89.999
RCO1 = Radius/chamfer 1, externally: on the side determined by the starting point
RCO2 = Radius/chamfer 2, externally
RCI1 = Radius/chamfer 1, internally: on the starting point side
RCI2 = Radius/chamfer 2, internally
FAL1 = Finishing allowance at the recess base
FAL2 = Finishing allowance at the flanks
IDEP = Infeed depth (enter without sign)
DTB = Dwell time at recess base
VARI = Machining type;  Range of values: 1…8 and 11…18
_VRT = Variable retraction distance from contour, incremental (enter without sign)
_DN = D number for 2nd edge of tool

CYCLE93 Examples

CYCLE93 CNC Program Example – 1 – Plunge Cutting

This program is used to produce a groove externally at an oblique line in the longitudinal direction. The starting point is on the right-hand side at X35 Z60. The cycle uses tool offsets D1 and D2 of tool T1. The cutting tool must be defined accordingly.

Siemens CNC Turning CYCLE93 Program Example

DEF REAL SPD=35, SPL=60, WIDG=30, DIAG=25, STA1=5, ANG1=10, ANG2=20, RCO1=0, RCI1=-2, RCI2=-2, RCO2=0, FAL1=1, FAL2=1, IDEP=10, DTB=1 ; Definition of parameters with value assignments
DEF INT VARI=5 ; Definition of parameters with value assignments
N10 G0 G18 G90 Z65 X50 T1 D1 S400 M3 ; Starting point before the beginning of the cycle
N20 G95 F0.2 ; Specification of technology values
N30 CYCLE93 (SPD, SPL, WIDG, DIAG, STA1, ANG1, ANG2, RCO1, RCO2, RCI1, RCI2, FAL1, FAL2, IDEP, DTB, VARI) ; Cycle call
N40 G0 G90 X50 Z65 ; Next position
N50 M02 ; 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 forums and join us to get support, ask questions, improve a published article or give your opinion.

Previous articleSiemens CNC Milling | CYCLE60 | Engraving Cycle
Next articleSiemens CNC Turning | CYCLE94 | Undercut Cycle