The G72 face roughing cycle: cutting a flange with a large diameter difference in steps along Z
Compares the G72 face roughing cycle with G71 to show when to use it, why W in the first block is the Z depth of cut, how to write the profile blocks from the face inward, and how to choose the tool, using a flange example.
G71 and G72 cut 90 degrees apart
G71 feeds in a little at a time in X and repeats long cuts along Z (the length direction), which suits long, slender shafts. G72, by contrast, feeds in a little at a time in Z and repeats cuts along X (the diameter direction). It suits flanges, discs and bosses on the face side, where the diameter difference is large and the length short.
For a profile 10 mm long with a 60 mm diameter difference, G71 has to repeat short cuts more than twenty times, while G72 finishes with a few long facing cuts. The longer the tool stays in contact with the workpiece, the better the efficiency, so the basic rule is to choose the cycle whose cutting direction runs along the longer side.
What the addresses mean: W becomes the depth of cut
| Block | Address | Meaning in G72 | Compared with G71 |
|---|---|---|---|
| First block | W | Depth of cut per pass in Z | G71 uses U (X depth in radius) |
| First block | R | Retract amount after each pass | Same |
| Second block | P/Q | Numbers of the first and last profile blocks | Same |
| Second block | U/W | Finishing allowance in X (diameter) and Z | Same |
| Second block | F | Roughing feed | Same |
The profile blocks start with Z
Just as the P block of G71 commands only X, the P block of G72, N10 G00 Z0., normally commands only Z. The profile is written starting at the outer diameter on the face side and moving inward (to smaller diameters), while Z gets deeper in one direction only. A groove in the middle where Z comes back cannot be handled in the Type I format.
Flange example
Face roughing the front of Ø80 stock to a Ø50 taper and a Ø24 boss
O2005
T0101
G21 G90 G18 G99
G50 S2000
G96 S150 M03
G00 X82. Z2.
G72 W2. R0.5
G72 P10 Q20 U0.4 W0.1 F0.25
N10 G00 Z0.
G01 X80. F0.12
X50. Z-4.
X30. Z-4.
X24. Z-14.
N20 X20. Z-14.
G70 P10 Q20
G00 X150. Z100.
M30The figure above is the CNC Path Analyzer result for this program (rapid 27 segments, linear cutting 13 segments).
What to check in the toolpath drawing
- The long vertical lines are the facing cuts along X. Each pass goes 2 mm deeper in Z.
- The
X50. Z-4.section is a tapered face, so the upper passes are long and the lower ones become shorter where the profile stops them. - The diagonal down to
X24. Z-14.is the tapered side of the boss. Roughing stops at a contour offset by the finishing allowances W0.1 and U0.4. - The final
G70 P10 Q20follows the same profile once and removes the allowance. A change to a finishing tool can be placed in between, as in the example of the G70 article.
Tool and cutting conditions
Because G72 cuts with the tool moving in the diameter direction, it needs a tool whose cutting edge faces the facing direction, even among OD turning holders. Using an ordinary OD roughing holder as is can let the side of the insert or the holder body touch the face. Check the holder's approach angle and clearance angle, and use a dedicated facing holder if necessary.
In diameter-direction cuts, the cutting speed at the outside and near the center differs greatly even at the same spindle speed. Combining G96 constant surface speed control with a G50 maximum spindle speed limit, as in the example, reduces the problem of being too slow at the outer diameter or too fast near the center.
How many passes would the same profile need with G71?
The example profile has to remove 58 mm in diameter (29 mm in radius), from Ø82 to Ø24, but only 14 mm in depth along the length. Counting from the cycle start point Z2, that is 16 mm, so with G72's W2. it reaches the bottom in 16 ÷ 2 = about 8 passes (the first pass travels through the space in front of the face).
Cutting the same profile with G71's U2. (2 mm depth in radius) would need 29 mm ÷ 2 ≈ 15 passes, most of them short, at 4–14 mm of cutting length each. Since every pass adds approach, retract and return time, the actual cycle time difference is even larger than the difference in pass count. This is why simply choosing the cycle that cuts along the "long direction" of the profile greatly reduces non-cutting time.
| Cycle | Infeed direction | Passes needed (approx.) | Cutting length per pass |
|---|---|---|---|
| G71 U2. | X (2 mm radius) | About 15 | Short (4–14 mm) |
| G72 W2. | Z (2 mm) | About 8 | Long (up to 29 mm radius) |
When the tool blocks G72
If the profile direction does not follow the face roughing rules, or the cycle start point is inside the profile range, CNC Path Analyzer does not draw the path and shows the cause line. Formats that controllers interpret differently, such as a profile whose last block ends with G00, are blocked by default and shown only when the user explicitly selects a reference interpretation.