Canned Cycle Grooving

I’m a big fan of canned cycles. They are used in many areas of machine programming, but today we’ll look at using the canned cycle code G75 for rough grooving. Canned cycles are easy to use and they can be helpful in reducing the stress found with conventional grooving.
     Programming a wide groove routine can be a lot of work. Reduce the amount of work by using an easy-to-handle routine like the one shown here.
     The main benefit of the G75 routine is the ability to “peck” the groove and break a chip. As grooving is predominately a “forming” operation, tool pressure and chip build up can be minimized by the automatic relief move built into this routine.
     Often a wide grooving insert is not used due to the increased tool pressure and the resulting tendency to generate chatter. In this example we are using a 0.093 wide insert and taking several cuts to produce the initial rough shape of this groove. A finish groove routine is programmed to produce the final shape with required chamfers and radii.

The G code activating the grooving canned cycle is G75. Let’s take a look at the following program sample.

G0	X1.550	Z-0.236	Starting position X and Z axis.
G75	R0.015
G75	X1.130	Z-0.335	P0350 Q0700	R0250 F.003

The first G75 shows an R code. This value indicates the return amount, the clearance for each cut.
     The second G75 provides much more information about the grooving cut. In the program line with the second G75:
     X = the final groove part diameter = 1.130 with stock for finish groove.
     Z = the Z position of the final groove. We have allowed the width of the groove insert to be incorporated in this value, with 0.005 stock on both sides, for the finish groove routine.
     P = the depth of each cut, note the value is given without a decimal point.
     Q = distance between grooves in the Z axis, note the value is given without a decimal point.
     R = retract amount at the end of the cut, note the value is given without a decimal point.
     F = the feed rate in IPR

     This G75 routine can be used to efficiently create numerous evenly spaced grooves.
     The P value is a depth-of-cut as a radius value and appears as 0.070 in your distance-to-go page. Once the first cut is completed, the tool jumps clear by the value defined in the first G75 line of R0.015, again this is a radius value which is added to the next depth-of-cut resulting in a value of 0.100 total, P0350 + R0.015 x 2 = 0.100
     The Q value in the second G75 line is the incremental “step-over” move and should be less than the insert width.
     The unusual thing to remember when using a G75 grooving routine is the three defined values that must be written without decimal points. Why did the control builder design it this way? There must be some logic behind it.
     We just need to remember to use a trailing zero format. I write these values as four numbers, making it easier to relate to the standard four decimal places used in inch format programming.
     This routine is easy to write and helps when producing wide groove features that require multiple passes. Just remember to ignore the decimal points on the P, Q and R values and life is groovy.