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

In this article, we describe how to use G73 cycle for pattern repeating in CNC lathe machines with all details and examples.

G73 Cycle Introduction

The pattern repeating cycle is also called the Closed Loop or a Profile Copying cycle. In CNC turning machines, the G73 cycle is often used for machining materials that have been cast out for profile repetition. In this cycle, starting from the cutter (P) point, following the profile of the workpiece, it removes sawdust and returns to the point where the cutter cycle begins. Its purpose is to minimize the cutting time for roughing material of irregular shapes and forms, for example, forgings and castings. The G73 cycle is mostly used for machining parts that have a fixed chip share. The profile of such parts may have increasing or decreasing geometry. After the G73 cycle, the transaction is completed by taking the last pass share left with the G70 cycle.

G73 Cycle Format

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

The one-block programming format for G73 cycle:
G73 P.. Q.. I.. K.. U.. W.. D.. F.. S..

Parameters

P = First block number of finishing contour
Q = Last block number of finishing contour
I = X-axis distance and direction of relief – per side
K = Z-axis distance and direction of relief
U = Stock amount for finishing on the X-axis diameter
W = Stock left for finishing on the Z-axis
D = The number of cutting divisions
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 for the G73 cycle, the programming format is:
G73 U.. W.. R..
G73 P.. Q.. U.. W.. F.. S..

Parameters

First block:
U = X-axis distance and direction of relief – per side
W = Z-axis distance and direction of relief
R = Number of cutting divisions

Second block:
P = First block number of the finishing contour
Q = Last block number of the finishing contour
U = Stock amount for finishing on the X-axis diameter
W = Stock left for finishing on 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


In the two-block cycle entries, do not mix up addresses in the first block that repeat in the second block (U and W in the G73 example). They have a different meaning! 

Things to Know

In order to make the multiple repetitive stock removal cycles (contouring cycles) work properly and efficiently, observing the rules of their use is very important. Often a small oversight may cause a lengthy delay.

  • Always apply tool nose radius offset before the stock removal cycle is called
  • Always cancel tool nose radius offset after the stock removal cycle is completed
  • Return motion to the start point is automatic, and must not be programmed
  • The P block in G71 should not include the Z-axis value (Z or W) for cycle Type I
  • Change of direction is allowed only for Type II G71 cycle, and along one axis only (W0)
  • Stock allowance U is programmed on a diameter, and its sign shows to which side of the stock it is to be applied – sign is the X-direction relative to centerline:
    … U+ for turning – towards spindle centerline
    … U- for boring – away from spindle centerline
  • Feedrate programmed for the finishing contour (specified between P and Q points) will be ignored during roughing
  • Profile turning cycle is used to remove the pieces of cast iron by removing thin chips from the surface. It is not preferred for turning the profile by processing raw materials from scratch.
  • The total amount of chips to be removed from the surface of the part in the U (1) X axis is obtained by dividing the difference between the largest diameter and the smallest diameter of the part in two.
  • W (1) The total amount of chips to be removed from the surface of the part in the Z axis should be taken 0 (zero) if the face part of the part will not be processed.
  • Setting the Z value to 0 (zero) before starting the cycle will facilitate the creation of the part profile.
  • F cutting feedrate given in the start and end lines cannot be used in the G72 cycle. These feedrate are used in the G70 finishing turning cycle.G41 and G42 cutting tool nose radius compensation cannot be used with the G73 cycle. If written in the program, the G70 is used during the finish pass cycle.
  • If the program flow is stopped and some manual movements are performed during the G73 cycle, it must be reached 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. If other lines or lines are written in between, it will not be active.
  • The G73 cycle cannot be run under MDI code.
  • M98 and M99 commands are not used in lines where G73 cycle is written.
  • D address in one-block format only, does not use decimal point, and must be programmed for leading zero suppression format:

D0750 or D750 is equivalent to 0.0750 depth

  • Only some control systems do allow a decimal point to be used for the D address (depth of cut) in one-block G71 and G72 cycles.

G73 Cycle Examples

G73 CNC Program Example – 1 – Pattern Repeating

Figure 35-17 – Pattern repeating cycle G73 – program example O3507

There are three important input parameters in G73 cycle – U/W/R (I/KD). One parameter seems to be missing – there is no depth of cut specification! In G73 cycle, it is not needed. The actual depth of cut is calculated automatically, based on these three parameters:

  • U (I) : Amount of rough material to remove in X-axis
  • W (K) : Amount of rough material to remove in Z-axis
  • R (D) : Number of cutting divisions or repeats

Use this cycle with care – its design assumes an equal amount of rough stock to be removed along both the X and the Z axes. The cycle can still be used with a reasonable efficiency, but some ‘air’ cutting may be an unwanted side effect for odd shaped parts.
In the example, the largest expected material amount per one side will be chosen as 0.200 (U0.2) and the largest expected material amount on the face as 0.300 (W0.3). The number of divisions could be either two or three, so the program will use R3. Some modification at the control may be necessary during actual setup or machining, depending on the exact condition and sizes of the casting or forging.

This cycle is suitable for roughing contours where the finish contour closely matches the contour of the casting or forging. Even if there is some ‘air’ cutting, this cycle may be more efficient than the selection of the G71 or G72 cycles where too much empty cutting would take place. The program O3507 shows roughing and finishing with the same tool (as an example):

O3507 (G73 PATTERN REPEATING CYCLE)
N1 G20 M42
N2 T0100
N3 G96 S350 M03
N4 G00 G42 X3.0 Z0.1 T0101 M08
N5 G73 U0.2 W0.3 R3
N6 G73 P7 Q14 U0.06 W0.004 F0.01
N7 G00 X0.35
N8 G01 X1.05 Z-0.25
N9 Z-0.625
N10 X1.55 Z-1.0
N11 Z-1.625 R0.25
N12 X2.45
N13 X2.75 Z-1.95
N14 U0.2 F0.02
N15 G70 P6 Q13 F0.006
N16 G00 G40 X5.0 Z2.0 T0100
N17 M30

%

The number of passes R3 may be necessary to accommodate some rotating eccentricity, normally associated with castings and forgings. On the other hand, R2 may be necessary for the heavier cut, to ‘bite under the skin’ of the material, for better tool life. Schematically, Figure 35-18 shows three programmed cutting divisions (R3).

Figure 35-18 – Schematic representation of G73 cycle

Note that the pattern repeating cycle does exactly that – it repeats the machining contour (pattern) specified between the P and Q points. Each individual tool path is offset by a calculated amount along the X and Z axes. On the machine, watch cutting progress with care – particularly for the first tool path. Feedrate override may come useful here.

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.
...