Skip to main content

Fundamentals of G73

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.

Thanks for visiting.


Comments

Post a Comment

Popular posts from this blog

Fanuc Face grooving using G74

Fundamentals:- The cycle G74 stands for longitudinal cutting process. Where we remove material from face ether performing as drilling cycle or face grooving, the cycle is beneficial to cut stubborn materials like stainless steels. Because of complete material removal motion. In G74 cycle we can cut through along with 'Z' axis as well as 'X' axis, also can use on turnmill operations while drilling off centre drills. Format of G74:- ________ G74 R G74 P Q X Z F ________ R- retraction amount. P- shifting value while cutting along X axis in micron. Q- Depth of cut in micron. X- Cutting last destinations along X axis. Z- Cutting last destinations along Z axis. F- Feed. Note:- shifting value 'P' should not exceed the width of grooving tool. If tool width is 4mm then shifting value should be 3.5mm. Example:-   G00 X40.0 Z2.0; G74 R0.5 (shifting value); G74 P3500( 3.4 shift value) Q500 (depth of cut) X52.0 Z-7.0 F0.07; G00 Z10.0
Post a Comment
Read more

Fanuc grooving cycle G75

Fundamentals This cycle does a peck drilling operation for grooving or drilling perpendicular to the axis. The cycle can actually be used to cut multiple grooves, or (on a machine with a C-axis and live tools) drill multiple radial holes at various positions along the length, The explanation here is restricted to cutting a single groove. Structure ______ G75  R G75  X  P  F _______ R= Retreat amount after each peck, radial distance. X= X coordinate of groove bottom (Diameter to cut).  P= Peck depth, radial distance in micron. F= Feed rate. We can remove material performing single groove same as insert thickness as well as more than that. Example of single groove as insert thickness ________ G00 X54.0 Z-20.0; G75 R0.5; G75 X30.0 P1000 F0.1; G00 X100.0 Z50.0; _____ Example of Groove more than insert thickness Let the groove width is 5mm of the above drowning ________ G00 X54.0 Z-20.0;   (using 3mm insert thickness) G75 R0.5; G75 X30.0 Z-25.0 P1000 Q2500 ...
Post a Comment
Read more

Fundamentals of G72 Cycle

Introduction to G72 cycle This cycle generates a part shape from a cylindrical raw material, with cuts perpendicular to the axis. The cycle definition has the part shape, depth of cut, finish allowance and couple of other parameters. Fanuc G72 Facing Cycle If you have spent some time on cnc machine with fanuc control in cnc machine workshop, then you might surely have used  G72 Canned Cycle Facing  and cnc turning cycle G71. Because cnc cycle programming in fanuc cnc control is just easy. Why do we use cnc cycles read  pros and cons of cnc programming cycles . In this post I am going to elaborate the use, and programming of the  G72 Canned Cycle Facing  on Fanuc cnc control. Fanuc cnc control is widely used, no doubt one of the most favorite cnc control of cnc programmers, due to its ease of programming and durability. Programming G72 W R G72 P Q U W Parameters First Block Parameter Description W Depth of cut. R Return value after a cut is complete. Second Blo...
Post a Comment
Read more