G74

Introduction to G74

So imagine that you are going to drill a hole in the middle of a part and the hole has diameter 39 mm. You probably don't have a regular drill to drill a hole with that diameter but have short hole drill of 38mm. It is also possible to use the G74 to make hole of bigger diameters than the tool but more on that later.

Another way to use the G74 code is for making external circular grooves in the part but that will be touched on later.

G74 Basic use

Drilling a hole

In my experience the most common application of the G74 command is to drill holes of large diameters with a drill, either a regular drill or a short hole drill but it can also be used to drill holes with a regular drill. First let's assume you are using a regular drill to drill a hole in the middle of your part.

G97 S800 M08 M03

G00 X0 Z25 T0101 (Regular drill with any diameter)
G74 X0 Z-20 F0.1 D2 L4 K20

G00 X999 Z999 M5 M9

The code above will drill a hole of depth 20mm in the middle of the part, let's break down the code.

Explanation

Using the G74

- I start the operation by starting the spindle at 800 rpm, though you should check what is appropriate for you conditions. I also start the coolant.

G97 S1200 M08 M03

- Then I select the tool and approach the part, in this case the drill has position 1 in the turrent.

G00 X0 Z25 T0101 (Regular drill)

- On the third line I do the drilling with the G74 cycle. It is important that the value of X is zero both on the line with the G74 command and on the line before it, more on this later. The Z-value is the bottom of the hole, the F value is the feed, in this case mm/rotation. D is the depth before a small retract and L the depth before a "full" retract to the value in the line above, in this case Z25. K is the distance from that Z25 value to the point in Z were we start drilling.

G74 X0 Z-20 F0.1 D2 L4 K20

The final line is just a line were I returt to the home position and turn of the spindle and the coolant.

G00 X999 Z999 M5 M9

Drilling larger holes

First I will assume I have a short hole drill with diameter 38mm. In the simple case I want to make a hole with diameter 38 and then I write as above with the exception of the X-value which should be the diameter of the short hole drill. The lines that differ should look like:

G00 X38 Z25 T010101 (Short hole drill dia 38mm)

G74 X38 Z-60 F0.09 D999 L999 K20

Where Z is the depth, F is the feed, D is cutting depth and D and K has to do with the rapid movement distances.

Drilling even larger holes

- So imagine that you are instead going to drill a hole in the middle of a part and the hole has diameter 52 mm. You probably don't have a regular drill to drill a hole with that diameter and neither have a 52mm short hole drill either, only say a 38mm as above. As toolholderplaces are limited I will show you how to make the hole in a simple manner and let you save an internal roughing tool. Here is the code:

G00 X38 Z25 T070707 (SHORT HOLE DRILL DIA 28MM)

G74 X52 Z-60 F0.09 D999 L999 K20 I3

G00 X56 Z2
G1 Z0 F0.05 G41
G75 X52 L1
G1 Z-1.5

G1 X48
G40
G1 Z2 F0.5

First I select the tool and approach the part. I use a Z-value which is significantly much larger that zero in order to make sure that the tool does not crash in the part. I also let the X-value be the diameter of the drilling tool, this X-value is very important.

G00 X38 Z25 T070707 (select the tool)

But instead of writing X38 I want to make a hole with diameter 52. Then I write the G74 cycle and the end diameter of the hole, X52, the bottom of the hole, Z-60, the feed... and at last I write I3. What will happen is that the drill will start drilling a hole of diameter 38 and the increase the diametric X-value by I, in this case 3, and get to 41 were it will again drill to the depth of Z-60 and so on until it gets to 52 were it will drill one last time.

G74 X52 Z-60 F0.09 D999 L999 K20 I3

As you can see I can in this way replace a whole bunch of lines and maybe an entire tool by just one line of code, which by the the way I needed to use anyways. And to add a nice little feature on top of this I may write the following after the line with the G74 cycle:

G00 X56 Z2
G1 Z0 F0.05 G41
G75 X52 L1
G1 Z-1.5
G40
G1 Z2 F0.5

Thus making a contour using the short hole drill. This line allow me to break the edge of the hole and make a small chamfer so that I don't damage the fine internal tool.

G73 - Like G74 but in the other direction

As mentioned above you can use a similar method for the G73 cycle as we did for G74 essentialy replacing the role of I with K. However this works in a different manner and is covered on a different page.

G74 Expansion

Making axial circular grooves

Now you have been aquainted with the G74 command for okuma turning, now I will expand on the application of the command by demonstrating how to make grooves in the end surface around the Z-axis.

Consider the following code

G97 S1200 M03 M08 G95
G00 X80 Z12 T080808 (AXIAL BLADE 2.5MM)
G74 X90 Z-3 F0.09 D1 L4 E0.1 K10 I1.6 T18 (***T18***)
G00 X78 Z2 T08 (*****T08*****)
G1 Z0 F0.05 G42
G75 X80 L0.5
G1 Z-3
G1 X83
G40
G1 Z2 F0.5
G00 X92 Z2 T18 (*****T18*****)
G1 Z0 F0.05 G41
G76 X90 L0.5
G1 Z-3
G1 X86
G40
G1 Z2 F0.5
M09
G0 Z50
G0 X999 Z999 M9 M5

In the example above I am using the G74 command to make a round groove on the end surface of the part. Then I make two contours, one on either side of the groove.

Note that I leave a little bit of material during the G74 cycle to have some material to remove when making the contours, this is optional however and may be disregarded.

Note also that I'm switching between the tool places and have comments on those lines to make it easier to notice.