G73 Cycle | Pattern Repeating

In this article, we describe how to use G73 Pattern Repeating Cycle for profile repetition of an already roughly formed casting material in CNC lathe machines with all details and examples.

0
1870

G73 Canned Cycle

G73 Cycle is a CNC code and used for profile repetition on CNC lathes. This cycle is generally used for profile repetition of an already roughly formed casting material. Shaped casting parts, pre-machined parts or casting mold parts are examples of include this. G73 CNC code is also called the closed loop or a profile copying cycle for CNC Lathe.

We highly recommend to continue read full of article with all details and examples but if you have not enough time to read all, click here to see overview of G73 CNC Code for CNC Lathe.
G73 CNC code used for pattern repeating in CNC lathe machines and used to re-machining a pre-formed profile.
G73 U.. W.. R..
G73 P.. Q.. U.. W.. F.. S..
First block:
U : Total depth of cut and direction (in radius – per side) in the X axis
W : Total depth of cut and direction in the Z axis
R : The number of repetition of the cycle
Second block:
P : First block number of the contour in program (N10, N20.. etc.)
Q : Last block number of the contour in program (N80, N90.. etc.)
U : Amount left for finishing in the X-axis (in diameter)

W : Amount left for finishing in the Z-axis
F : Cutting feedrate (in/rev or mm/rev) overrides feedrates between P block and Q block
S : Spindle speed (ft/min or m/min) overrides spindle speeds between P block and Q block
G70 Finishing Cycle:
G70 code is finishing cycle if you want to use different cutting tool, spindle speed or feedrate, and use in same program. Click here to jump G70 Cycle section.
G73 Cycle Examples:
Click here to jump G73 CNC Program Example section.

G73 Cycle Format

Like most of CNC cycles, G73 Pattern Repeating Cycle comes in two formats – a one-block (known as single line or type 1) and a double block format (known as also two line or type 2), depending on the control system, especially for Fanuc CNC controller. Even if it’s known for Fanuc CNC controller, most of other controller also using same structure for G73 cnc code.

Fanuc 6T/10T/11T/15T

The one-block (Single line – Type 1) programming format for the G73 canned cycle:
G73 P.. Q.. I.. K.. U.. W.. D.. F.. S..

Parameters

P : First block number of the contour in program (N10, N20.. etc.)
Q : Last block number of the contour in program (N80, N90.. etc.)
I : Total depth of cut and direction (in radius – per side) in the X axis
K : Total depth of cut and direction in the Z axis
U : Amount left for finishing in the X-axis (in diameter)
W : Amount left for finishing in the Z-axis
D : The number of repetition of the cycle
F : Cutting feedrate (in/rev or mm/rev) overrides feedrates between P block and Q block
S : Spindle speed (ft/min or m/min) overrides spindle speeds between P block and Q block

Fanuc 0T/16T/18T/20T/21T

If your control system requires a double block entry (Two line – Type 2) for the G73 pattern repeating cycle, the programming format is:
G73 U.. W.. R..
G73 P.. Q.. U.. W.. F.. S..

Parameters

First block:
U : Total depth of cut and direction (in radius – per side) in the X axis
W : Total depth of cut and direction in the Z axis
R : The number of repetition of the cycle
Second block:
P : First block number of the contour in program (N10, N20.. etc.)
Q : Last block number of the contour in program (N80, N90.. etc.)
U : Amount left for finishing in the X-axis (in diameter)
W : Amount left for finishing in the Z-axis
F : Cutting feedrate (in/rev or mm/rev) overrides feedrates between P block and Q block
S : Spindle speed (ft/min or m/min) overrides spindle speeds between P block and Q block

Note: In the two-block cycle entries, do not mix up addresses in the first block that repeat in the second block (U and W). They have a different meaning!

G70 Finishing Cycle

The G70 Finishing Cycle is used for finish cutting operations (final cleaning cutting) in CNC lathes. The G70 command is used to final cutting after any roughing cycles like G71 Turning Cycle, G72 or G73 cycle. It’s possible to proceed finish cutting with different tool, spindle speed or feedrate after roughing cycles, and use in same program. G70 cycle follows same tool path and contour with G73 CNC code but only once, not more.

It is not compulsory to use G70 after G73 cycle but in general, CNC machine users perform rough cutting with G73 cycle, and finishing cut with G70. The amount of finishing passes to be left for G70 is specified with the U and W values in second row of G73 cnc code.

G73 Cycle Example

G73 Pattern repeating cycle example for CNC Programming in CNC Lathe
G73 Pattern repeating cycle example for CNC Programming in CNC Lathe
O0009;
N10 G54;
N15 T0101 M04;
N20 G50 S1500;
N25 G96 S80;
N28 G99 F0.3;
N30 G00 X69 Z0;
N35 G01 X-2;
N45 G00 X69 Z4;
N48 G42;
N50 G73 U4. W4. R3. ;
N51 G73 P60 Q80 U0.5 W0.2 F0.2 ;
N60 G01 X20 Z0;
N65 G01 Z–10 F0.15;
N70 G02 X40 Z–20 R10;
N75 G01 Z–30;
N80 X60 Z–50;
N90 G40;
N95 G00 X200 Z200;
N100 T0202;
N105 G00 X65 Z3;
N90 G70 P60 Q80 ;
N95 G00 X200 Z200 M09;
N100 M05;
N105 M30;

 

“Click here to see all CNC program examples for G73 Pattern Repeating Cycle”

Things to Know

  • The G73 Cycle is generally used for profile repetition of an already roughly formed casting material. Shaped casting parts, pre-machined parts or casting mold parts are examples of include this. This is main difference of G73 cycle than G71 Turning Cycle and G72 Cycle.
  • The W value (we can say W1) written in the first line should be entered as 0 (zero) if the facing of the workpiece will not be machined.
  • F cutting feedrates given after the G73 cycle lines is used in the G70 finishing turning cycle.
  • G41 and G42 tool nose radius compensation cannot be used with the G73 cnc code. If written in the program, the G70 is used during the finishing cycle.
  • If the program is stopped during the G73 pattern repeating cycle and some manual axes movements are performed, it must be moved to the point where the program is stopped manually before starting the program again.
  • P and Q lines defining the finish profile must be written on the same line as G73 code.
  • The G73 canned cycle cannot be run under MDI mode.
  • M98 and M99 commands are not used in lines where G73 cycle is written.

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 articleG75 Cycle | Grooving and Parting Off
Next articleTypes of CNC Machine Tools