G73

Introduction to G73

When a part has been completed you may use the G73 code to cut of the part and let it fall into the catcher or just down in the chip collector. This allow you to automate more of the lathing process by opening up the possibillity for the machine to make saveral parts unattended.

Another way to use the G73 code is for making external and internal rectangular grooves in the part. I will start with the first and then explain the latter.

G73 Basic use

Cutting of the finished part

In my experience the most common application of the G73 command is to cut of a finished part. Let's say that the part has a diameter of 40mm and length 52mm and no hole going through, then we use the following set of code to approach and open up the part for cutting.

G97 S1200 M08 M03

G00 X45 Z-52.4 T221222 (PARTING OFF BLADE 3MM WIDTH)
G73 X20 Z-52.4 D2 L4 F0.05 E0.05

G0 Z-49
G1 X40 F0.1 G42
G75 Z-52 L0.5
G1 X12
G40
G1 X12.2 F0.2
M77
G97 S300
G1 X-1 F0.04 (part gets cut off)
M76
G0 X100
X999 Z999 M9 M5
M02

Explanation

Using the G73

- First with G97 we set the spindle speed and on the same line I start the spindle and the coolant.

G97 S1200 M08 M03

- Then I select the tool and approach the part, in this case the tool has position 12 in the turrent.

G00 X45 Z-52.4 T221222 (PARTING OFF BLADE 3MM WIDTH)

- Notice also that I have written T221222 which means that I load the tool data from position 22 instead of 12, this is to allow the left side of the blade to have position 12 and the right side position 22. Notice that I choose an X-value that let me stay a few millimeters outside of the part just to be sure to not crash into the part. I have also selected a Z-value which is 0.4mm behind the end of the part to have a little bit of material for later.
G73 X10 Z-52.4 D2 L4 F0.05

- On the third line I use the cycle G73 to cut in the part. I don't want to use the cycle to cut of the part just jet and I will explain why in a minute. I will go to X10 to let the part have some material to sit in, I could let X be -1 and cut of the part but I prefer to do it this way. I select the same Z-value as before, otherwise I will run into difficulties. The D-value let me choose how much I want to go into the part before a small retraction of 0.5mm and the L-value is the same but for retractions where I return to the X-value given earlier(X45 written on the previous line). F is the feed in this case in mm/rotation.

Finishing the part

- Now I have made a groove in the part and want to finish it and cut it off. I will do this by making a contour which will let me get a nice finish on the back of the part.

G0 Z-49
G1 X40 F0.1 G42
G75 Z-52 L0.5
G1 X9
G40
G1 X9.2 F0.2
M77
G97 S300
G1 X-1 F0.04 (part gets cut off)
M76
G0 X100
X999 Z999 M9 M5
M02

- Notice that I end the contour on X9 and then do a small retract after having turned of the radial compensation on the path. This is to leave the part hanging when using M77 to "approach" the part with the parts catcher and then cut of the part when going to X-1 and then "retract" the parts catcher with M76.

Then I simple exit the part and return the machine to the ending position and finally I end the program with M02. If you for some reason don't want to end the program after having cut of the part you may skip the M02.

Tips and tricks

How to utilize the K variable with G73 to cut external and internal grooves in the part.

Now we have learned how to use the G73 command for parting when turning in Okuma, let me give you another feature of G73 to unlock it's full potential. Assume for a moment that you are making a part with an external groove with a rectangular shape.

Assume the groove goes from X40 to X50 and from Z-20 to Z-40.

We make the groove and round of with a contour to give it a good finish.

G00 X53 Z-20.2 T221222 (PARTING OFF BLADE 3MM WIDTH)
G73 X40.2 Z-39.8 D2 L4 F0.1 K2.1 T12

G0 Z-18 T22
G1 X50 F0.1 G42
G75 Z-20 L0.5
G1 X40

G1 Z-31
G40

G0 X53

G0 Z-52 T12

G1 X50 F0.1 G41

G75 Z-40 L0.5

G1 X40

G1 Z-29

G40

G0 X100
X999 Z999 M9 M5

Code breakdown

Now I will go over the code part by part and explain their purposes.

G00 X53 Z-20.2 T221222 (PARTING OFF BLADE 3MM WIDTH)

First I select my tool and approach the part, notice that I want to be outside the part in X. Notice also that I am using T221222 to load the data from tool spot 22 but load the tool placed at spot 12(I usually have 12 spots in the revolver). This allow me to have two seperate tool positions for my blade tool, more on that in another article.

G73 X40.2 Z-39.8 D2 L4 F0.1 K2.1 T12

The next line is the cutting of the groove itself. I started at X53 Z-20.2 which means that I am 0.2mm into the groove, this is in order to leave some material to remove in the contouring later. I select on the G73 line the X40.2, this works in the same way as the previous example.

Similarily I choose Z-39.8, this works about the same as the X-value but we move in Z instead. D, L and F has been covered before so I leave them for now.

Then we have the K-value, this is very important when cutting this kind of groove in the part. The K-value is the length in Z that me tool will travel after having made a cut down to the final X-value(in this case X40.2).

In my code the machine will first travel to Z-20.2, from the previous line, and there it will make a cut in the same way as in the first example. Then the tool will travel in Z by my K-value, I have K2.1, and then make a cut in the same way with the same X-values. I will remark here that as Z-20.2 comes first and is larger than Z-39.8 the tool will make a cut and then travel by 2.1mm(K) in the Z- direction, this can be reversed if the first Z-value is larger than the latter.

It is also important to note here that I end the line by writing T12 to switch from the right side of the tool to the left.

G0 X55

G0 Z-18 T22 (***T22***)
G1 X50 F0.1 G42
G75 Z-20 L0.5
G1 X40

G1 Z-31
G40

Moving on I let the tool exit the part and then move it in position for the contour. Notice also that I swap to the right hand side of the blade and on the same line I write a comment (***T22***). This is because I have been in situations were these tool data swaps were not noticed when I ran the machine. What can happen if you don't notice this swap is that the tool can easily crash into the part, hence the comment.

Then I make a simple contour in tha same way as any other contour and move just a little over the middle when setting G1 Z-31.

G0 X53

G0 Z-52 T12 (***T12***)

G1 X50 F0.1 G41

G75 Z-40 L0.5

G1 X40

G1 Z-29

G40

Next I retract the tool from the part and move into position for the contour on the left side. I swap back to T12 from the tool data as I want to use the conrner on the left side of the blade and then make the contour. I go a little further than the middle again to ensure that the whole groove has a nice contour.

G0 X100
X999 Z999 M9 M5

Finally I retract to outside the part to X100 to be sure to not crash into the part when retracting to the end position. Then I return to the end position and turn of the coolant and the spindle.