0 votes
200 views
in cnc programming by (9.4k points)

In this article, we describe how to use G94 cycle for facing (face cutting) in CNC lathe machines with all details and examples.

G94 Cycle Introduction

A cycle that is very similar to G90 is another simple turning cycle, programmed with the G94 command. This cycle is called the face cutting cycle. The purpose of G94 cycle is to remove excessive stock between the cutter start position and the coordinates specified by the X and Z axes. The resulting cut is a straight turning cut, normally perpendicular to the spindle center line. In this cycle, it is the X-axis that is the main cutting direction. G94 cycle is used primarily for facing cuts and can be used for simple vertical taper cutting as well, similar to the G90 cycle.

The G94 cycle is logically identical to the G90 cycle, except the emphasis is on the X-axis cutting, rather than the Z-axis cutting.

As the cycle description suggests, the G94 is normally used to perform a rough face-off of the part, towards the spindle center line or to face-off a shoulder.

G94 Cycle Format

G94 X(U).. Z(W).. F.. R(K)..

Parameters

X: Diameter value to be turned
Z: Length value to be turned
F: Progress
R: Taper depth mm (If there is no taper on the workpiece, this parameter is not used)

Addresses X and Z are used for absolute programming, addresses U and W are used for incremental programming, and the F address is cutting feedrate. The R(K) parameter if greater than zero, is used for taper cutting along the vertical direction.

G94 Cycle Examples

G94 CNC Program Example – 1

CNC Lathe G94 Cycle Face Cutting Program Example – 1

N100 T0101;
N110 G97 S500 M04;
N120 G00 X64. Z10.;
N130 G1 Z2. F0.5;
N140 G94 X48. Z-5.; ( No 1 motion )
N150 Z-12.; ( No 2 motion )
N160 Z-19.; (No 3 motion )
N170 Z-26.; (No 4 motion )
N180 Z-33.; (No 5 motion )
N190 Z-40.; (No 6 motion )
N200 G28 U0.;
N210 G28 W0.;
N220 M30;

G94 CNC Program Example – 2

CNC Lathe G94 Cycle Face Cutting Program Example – 2

G28 U0 W0;
G50 S2000;
G96 S200 M03;
G00 X85.0 Z2.0 T0101 M08;
G94 X40.0 Z–2.0 F0.2;
Z–4.0;
Z–6.0;
Z–8.0;
Z–10.0;
Z–12.0;
Z–14.0;
Z–16.0;
Z–18.0;
Z-19.7;
Z–20.0;
G28 U0 W0;
M30;

G94 CNC Program Example – 3

CNC Lathe G94 Cycle Face Cutting Program Example – 3

G50 S2000;
G96 S180 M03;
G00 X55.0 Z2.0 T0101;
G94 X15.0 Z-2.0 F0.2;
Z-4.0;
Z-6.0;
Z-8.0;
G00 X200.0 Z200.0;
M30;

G94 CNC Program Example – 4

CNC Lathe G94 Cycle Face Cutting Program Example – 4

O0020;
N320 G54;
N325 T0101 M04;
N330 G50 S2000;
N335 G96 S150;
N340 G99 F0.3;
N335 G42 G00 X62 Z0;
N340 G01 X–1.6;
N345 G00 X63 Z4;
N350 G94 X40 Z–3 F0.3;
N355 Z–6;
N360 Z–9;
N365 Z–12;
N370 Z–15;
N375 Z–18;
N385 Z–25;
N390 Z–28;
N395 Z–31; .
N400 Z–34; .
N405 Z–37; .
N410 Z–40; .
N425 G00 X45 Z3;
N430 G94 X16 Z–3 F0.3;
N435 Z–6;
N440 Z–9;
N445 Z–12;
N450 Z–15;
N455 G40 G00 X200 Z200;
N460 M05 M09;
N465 M30;

G94 CNC Program Example – 5 (Tapered)

CNC Lathe G94 Cycle Face Cutting Program Example – 5 ( Taper )

O0021;
N320 G54;
N325 T0101 M04;
N330 G50 S2000;
N335 G96 S150;
N340 G99 F0.3;
N40 G42 G00 X62 Z0;
N45 G01 X–1.6;
N50 G00 X65 Z4;
N55 G94 X40 Z–3 F0.3;
N60 Z–6;
N65 Z–9;
N70 Z–12;
N75 Z–15;
N80 Z–18;
N85 Z–21;
N90 Z–25;
N95 Z–27;
N100 G00 X45 Z3;
N105 G94 X16 Z–3 F0.3;
N110 Z–6;
N115 Z–9;
N120 Z–12;
N125 Z–15;
N130 G00 X40 Z–15;
N145 G94 X16 Z–15 R–6 F0.2;
N160 G94 X16 Z–15 R–10 F0.2;
N165 G94 X16 Z–15 R–12 F0.1;
N168 G00 X200 Z200;
N170 M05 M09;
N175 M30;


Need to more?

In this article, we described How to use G94 cycle for facing (face cutting) in CNC lathe machines with all details and examples. For more details;

For your comments, suggestions and questions, you can write to us from the “Comments Section” below without registration and please consider to share this post!

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...