G72 Cycle | Stock Removal in Facing

In this article, we describe how to use G72 Facing Cycle for facing (face cutting) in CNC lathe machines with all details and examples.

0
1814

G72 Canned Cycle

G72 Cycle is a CNC code and used to facing (face turning) in CNC Lathe machines, in other words cutting parallel to the X-axis. G72 CNC code is one of the most commonly used CNC Turning cycles.

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 G72 Cycle for CNC Lathe.
G72 facing cycle is a CNC code and used to stock removal in facing for CNC lathe machines.
G72 W.. R..
G72 P.. Q.. U.. W.. F.. S..
First block:
W : Depth of roughing cut
R : Amount of retract from each cut
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.
G72 Facing Cycle Examples:
Click here to jump G72 Cycle Examples section.

 

It is used for roughing of a solid cylinder, using a series of vertical cuts (face cuts). The G72 Cycle generally processes the profile to be processed with the tolerances you specified in the program, and then finish with the G70 Finishing Cycle.

G72 Cycle Format

Like most of CNC cycles, G72 CNC code 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 G72 G code.

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

The one-block (Single line or Type 1) format for the G72 facing cycle is:
G72 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 : Distance and direction of rough semi finishing in the X-axis – per side (Optional)
K : Distance and direction of rough semi finishing in the Z-axis (Optional)
U : Amount left for finishing in the X-axis (in diameter)
W : Amount left for finishing in the Z-axis
D : Depth of roughing cut
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:
The I and K parameters are not available on all machines. They control the amount of cut for semi finishing, the last continuous cut before final roughing motions.

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

If the control requires a double block entry (Two line or Type 2) for the G72 facing cycle, the programming format is:
G72 W.. R..
G72 P.. Q.. U.. W.. F.. S..

Parameters

First block:
W : Depth of roughing cut
R : Amount of retract from each cut
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: Do not confuse
address W in the first block, depth of cut, and address W in the second block, amount left on Z axis for finishing. The I and K parameters may be used only on some controls and the retract amount R is set by a system parameter.

G70 Finishing Cycle

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 Facing Cycle or G73 Pattern Repeating Cycle. It’s possible to proceed finish cutting with different tool, spindle speed or feedrate after roughing cycles, and use in same program. G70 finishing cycle follows same tool path and contour with G72 CNC code but only once, not more.

It is not compulsory to use G70 after G72 cycle but in general, CNC machine users perform rough facing with G72 cnc code, and finishing cut with G70 cnc code. The amount of finishing passes to be left for G70 is specified with the U and W values in second row of G72 Cycle.

G72 Cycle Examples

G72 Facing Cycle Example

G72 CNC code Example for CNC Lathe
G72 CNC code Example for CNC Lathe
O4466;
N10 G00 X220.0 Z60.0;
N11 G00 X176.0 Z2.0;
N12 G72 W7.0 R1.0;
N13 G72 P14 Q21 U4.0 W2.0 F0.3 S600;
N14 G00 G41 Z-70.0 S750;
N15 X160.0;
N16 G01 X120.0 Z-60.0 F0.15;
N17 W10.0;
N18 X80.0 W10.0;
N19 W20.0;
N20 X36.0 W22.0;
N21 G40;
N22 G70 P14 Q21;
N23 G00 X220.0 Z60.0;
N24 M30;

G72 Turning Cycle Example

G72 Cycle Example for CNC Lathe
G72 Cycle Example for CNC Lathe
N5 T0101;
N10 M3 S1800;
N15 G0 X83 Z0;
N20 G72 W1 R1;
N25 G72 P30 Q60 U0.4 W0.1 F0.18;
N30 G1 X80;
N35 G1 Z-53;
N40 G1 X78 Z-48;
N45 G1 X60;
N50 G1 Z-23;
N55 G1 X50 Z-2;
N60 G1 Z0;
N65 G70 P30 Q60;
N70 G0 X150 Z150;
N75 G28 U0 W0;
N80 M30;

 

“Click here to see all CNC program examples for G72 Facing Cycle”

Things to Know

  • Return motion to the start point is automatic, and must not be programmed.
  • The program of profile which we want to cutting should be write from left to right. But the tool does the cutting profile from right to left.
  • For internal turning, finishing pass (U in second line) value must be given negative (-).
  • F cutting feedrates given after the G72 cnc code lines is used in the G70 finishing cycle.
  • G41 and G42 tool nose radius compensation cannot be used with the G72 cnc code. If written in the program, the G70 is used during the finishing cycle.
  • If the program is stopped during the G72 facing 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 G72 cnc code.
  • The G72 canned cycle cannot be run under MDI mode.
  • M98 and M99 commands are not used in lines where G72 cnc code 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 articleSafety Related to CNC Work
Next articleCNC Machines | Milling (Machine Centers)