G73 pattern repeating cycle

When using roughing cycles on a CNC lathe we have a few options. The standard G71 cycle roughs the profile using linear moves along the Z-Axis. The G72 cycle is used for facing and the G73 pattern repeating cycle is used when we are machining a profile that is already cut. For example, a casting or a pre-machined part. Below we take a look at this G73 cycle and how it works.

What is the G73 pattern repeating cycle?

The tool will cut in the shape of the profile that we defined with a subroutine when using the G73 G-Code. If used on a billet, some of the tool paths will be cutting in fresh air. This is why it is normally used when we already have the profile of the part pre-cut or cast. The tool will cut the shape of the profile of the part on each pass, indexing in both X and Z by the amount that we add to the first G73 line after each pass until the finished size is achieved.

G73 pattern repeating roughing cycle

The G73 cycle block should look like this example.

Each part is broken down and explained below.

G73 U(1) W(1) R;
G73 P Q U(2) W(2) F;

G73 - PATTERN REPEATING CYCLE
U(1) - DEPTH OF CUT IN X-AXIS
W(1) - DEPTH OF CUT IN Z-AXIS
R - AMOUNT OF ROUGHING PASSES
P - FIRST LINE OF SUBROUTINE
Q - LAST LINE OF SUBROUTINE
U(2) - AMOUNT LEFT ON FOR FINISHING IN X
W - AMOUNT LEFT ON FOR FINISHING IN Z
F - FEED RATE

G73 tells the machine that we wish to use the pattern cycle

The first 'U' word defines the depth of cut of each roughing pass in the X-axis. 'W' is the amount that we wish to cut in Z-axis. The R is the number of passes we require.

The 'P' and 'Q' words let the control know the location of the subroutine of the profile that we are using. These values can be any value as long as it matches the 'N' numbers of the subroutine. This will look like the code below.

N150;
SUBROUTINE OF PROFILE;
N250;

In this example, 'P' would be P150 and 'Q' would be Q250 so they match the 'N' numbers.

The 'U' on the second G73 line is the amount of material that we wish to leave on for a finishing pass along the X-Axis and 'W' is the finishing allowance along the Z-Axis.

'F' is the command we use to specify a feed rate

G73 Program example

G73 U1.0 W1.0 R3;
G73 P150 Q250 U0.2 W.05 F0.25;
N150 G00 X22.0;
G01 G42 Z0.0 F0.2;
X23.0 Z-0.5;
Z-23.0;
X44.0 Z-34.0;
Z-70.0 ,R5.0;
X70.0;
N250 G40 X80.0 Z6.0 F250;

G73 U1.0 W1.0 R3

The first line tells the machine to take 1.0mm cuts in X (U) and to remove 1.0mm in the Z-axis on each pass. The R defines the number of passes that we wish to take.

G73 P150 Q250 U0.2 W.05 F0.25;

The 'P' value needs to match the N number at the start of the subroutine (N150) that we wish to cut and 'Q' matches the N number (N250) at the end of our subroutine.

U0.2 is our finishing allowance in X and W0.05 is our finishing allowance in Z. This defines how much material we leave on for our finishing tool to remove in a later operation.

F defines the feed rate. F0.2 will feed at 0.2mm per revolution of the spindle/part.

N150 G00 X22.0;

'N' shows our first line of the subroutine, G00 is our rapid travel G-Code and the X value moves the tool to the start of the profile.

G01 G42 Z0.0 F0.2;

G01 is our linear feed rate movement G-Code, G42 turns on tool nose radius compensation, Z moves the tool to the front of the part (We are assuming the datum or zero point is at the front face of the job) and finally, we give a feed rate of 0.2mm per revolution. The feed rate here will be ignored by our G73 cycle but it will be used for the finishing cycle that we would use the same subroutine for.

X23.0 Z-0.5;
Z-23.0;
X44.0 Z-34.0;
Z-70.0 ,R5.0;
X70.0;

This is our subroutine, it follows the profile of the part.

N250 G40 X80.0 Z6.0 F250;

This block of code is finished by defining the 'N' number, then G40 turns off cutter compensation, The X and Z movements move our tool away from the component using a fast feed rate.

Choosing the correct roughing cycle

We have three main roughing cycles available for us to use on a CNC Lathe.

G71 linear roughing cycle

G72 facing cycle

G73 pattern repeating cycle

The G71 roughing cycle is our main, go to operation when removing material from bar form, It cuts along the Z-axis in straight line moves to form the profile in steps. When complete, it will follow the contour of the part to clean up the steps produced by the cycle. You can read more about this cycle here.

The G72 cycle is a facing operation that acts similar to the G71 but removes material in a linear fashion in the X-axis. It is a straight line roughing cycle that forms the profile in steps just as the G71 does.

The G73 pattern repeating cycle moves the tool in the shape of the profile as it cuts. Perfect if we already have a profile that needs material removing before we finish with a G70 finishing sequence.