Siemens CNC Lathe | G77 - G90 Cycle | Cutting


Cutting Cycle Introduction

The cutting cycle (G90 or G77, sometimes also G20 depend on machine builder/parameter setting) is used for outside diameter (OD) cutting and has two kinds of cycles – straight cutting cycle and taper cutting cycle.

Straight Cutting Cycle

With the commands of “G… X(U)… Z(W)… F… ;”, straight cutting cycle is executed as indicated by sequence 1 to 4 shown in Fig. 4-1.

The cycle code can be change due to pre-selected G code system as below ( Selected by machine tool builder by parameter setting).

G code system A = G90
G code system B = G77
G code system C = G20
Fig. 4-1 Straight cutting cycle

Straight Cutting Format

G.. X… Z… F… ;

Since G90 (G77, G20) is a modal G code, cycle operation is executed by simply specifying in-feed movement in the X-axis direction in the succeeding blocks.

Straight Cutting Example

Fig. 4-2 Straight cutting cycle (G code system A)

N10 G00 X94. Z62. ;
N11 G90 X80. W–42. F0.3 ; Start of G90 cycle
N12 X70. ;
N13 X60. ;
N14 G00 ;
…..
…..

Taper Cutting Cycle

With the commands of “G… X(U)… Z(W)… R… F… ;” taper cutting cycle is executed as indicated by sequence 1 to 4 shown in Fig. 4-3.

The cycle code can be change due to pre-selected G code system as below ( Selected by machine tool builder by parameter setting).

G code system A = G90
G code system B = G77
G code system C = G20
Fig. 4-3 Taper cutting cycle

Taper Cutting Format

G… X… Z… R… F… ;

The sign of address R is determined by the direction viewing point A’ from point B.

Taper Cutting Example

Fig. 4-4 Taper cutting cycle (G code system A)

N20 G00 X87. Z72. ;
N21 G90 X85. W–42. R–10.5 F0.25 ;
N22 X80. ;
N23 X75. ;
N24 X70. ;
N25 G00 ;
….
….