With this free G75 grooving simulator and NC code generator you can enter diameters, groove width, number of grooves, peck (P) and step (Q) values, watch the live toolpath simulation and instantly generate FANUC 0i-TC compatible G-code. For the theory see our G75 Grooving / Cut-off Cycle guide, and for another simulator the G72 Face Roughing Simulator. For axial peck drilling also try our G74 Peck Drilling Simulator.
What the G75 grooving cycle does and when to use it
G75 is the FANUC peck grooving cycle in X. The tool plunges P deep in X, backs off R to break the chip, plunges again; when it reaches the groove bottom it rapids out, shifts Q in Z and repeats until the groove width is finished. One cycle covers a deep single groove, a wide groove cut in overlapping plunges, and parting off. Instead of writing every G1 plunge and retract by hand, two blocks do the whole CNC grooving job.
| G1 plunge | G75 | G74 | |
|---|---|---|---|
| Direction | X (manual) | X (radial), stepping in Z | Z (axial), stepping in X |
| Chip breaking | None, written by hand | Automatic with R retract | Automatic with R retract |
| Wide groove | One block per plunge | Automatic with the Q step | Q for face grooves |
| Typical job | Single shallow groove | Circlip grooves, wide grooves, parting off | Face grooves, peck drilling |
If the groove is as narrow as the insert or narrower, one plunge is enough; if it is wider, the cycle sweeps it with the Q step. For axial drilling and face grooves use the G74 Peck Drilling Simulator; for parameter details and internal grooving rules see the G75 Grooving / Cut-off Cycle guide.
How to use the simulator step by step
- Outside diameter and groove bottom diameter: the diameter of the surface to be grooved and the bottom diameter of the groove. Groove depth is half the difference; the tool shows it at once. For parting off enter 0 (or slightly negative) as the bottom diameter.
- Number of grooves and positions: the face is Z0. Enter the Z of the first groove's right face (negative towards the chuck) and its width; raising the groove count opens a separate Z and width row for each extra groove, so several circlip grooves go into one program.
- Insert width: the width of your grooving insert (2, 3, 4 mm…). The tool derives the Q step and the final Z position from it; a wrong insert width gives a wrong groove width.
- Peck depth P and retract R: P is the depth taken in X per plunge (1–2 mm in steel), R the pull-back for chip breaking (0.3–0.5 mm). If ductile material wraps the chip, lower P and keep R at 0.5.
- Material and speed clamp: the material button brings in Vc and f; the program is written with
G96constant surface speed, so theG50clamp is essential: rpm runs away towards the groove bottom and especially towards centre when parting. - Simulation and code: a three-block group is generated for each groove; watch the peck moves and the Z steps in the toolpath, then download the program with ".nc".
How the simulator calculates Z and Q
The one assumption you must know is the tool reference: the programmed point is the left (chuck-side) edge of the insert. From that:
- Start Z = left face of the groove = right face Z − groove width. The tool plunges first at the chuck-side wall of the groove.
- Target Z = left face + (groove width − insert width). On the last plunge the right edge of the insert sits exactly on the right wall of the groove.
- Q step = 80% of the insert width. Because the step is smaller than the insert, the plunges overlap and no ridge is left on the groove bottom.
- If the groove width equals the insert width, Z and Q are omitted and a single-plunge G75 is generated.
If your tool offset on the machine is measured to the right edge of the insert, add the insert width to the start Z in the generated program or re-measure the offset to the left edge. Skipping this shifts the groove by one insert width.
Reading the generated program
G75 R(e) ;
G75 X(U) Z(W) P(Δi) Q(Δk) R(Δd) F(f) ;| Address | Simulator field | Note |
|---|---|---|
R(e) (first block) | Retract R | mm; chip-breaking pull-back after every P peck |
X(U) | Groove bottom diameter | absolute diameter; X0 or X-1 for parting |
Z(W) | Target Z (last plunge position) | omitted for a single-plunge groove |
P(Δi) | Peck depth P | microns, no decimal point: 2 mm = P2000, radius value |
Q(Δk) | Z step (0.8 × insert) | microns: 2.4 mm = Q2400; omitted for a single plunge |
R(Δd) (second block) | — | Relief at the groove bottom; not written by the tool, taken as 0 |
F | f (mm/rev) | 0.05–0.12 typical for grooving |
Worked example: 6 mm wide, 10 mm deep circlip groove on a Ø80 shaft
Outside diameter Ø80, groove bottom Ø60 (10 mm deep), width 6 mm, right face at Z−5, 3 mm insert, P 2 mm, R 0.5 mm, steel (Vc 130, f 0.10). The tool works out the left face at Z−11, the target Z as −11 + (6 − 3) = −8 and Q as 0.8 × 3 = 2.4 mm, and generates:
O0001
G21 G99
G50 S2500
T0303 M08
G96 S130 M03
G0 X84. Z-11. (stock + 4, left wall of the groove)
G75 R0.5 (break the chip with a 0.5 mm retract every 2 mm)
G75 X60. Z-8. P2000 Q2400 F0.10
G0 X84.
G0 X150. Z200.
M09
M05
M30What the cycle does: at Z−11 five 2 mm plunges from X84 to X60 (0.5 mm back between each), rapid out, 2.4 mm along Z (Z−8.6), five plunges again, then a last plunge at Z−8 for the remaining 0.6 mm. Fifteen plunges at three Z positions, all from two blocks. Set the groove count to 3 and enter the Z of the second and third grooves and the same three-block group is repeated for each.
Parting off, deep grooves and internal grooves
Parting off: enter 0 as the bottom diameter; on the machine it is common to go to X-1.0 so that no pip is left at centre by the nose radius (if the tool geometry allows crossing centre). Keep R at 0.3–0.5 mm; if the chip does not break, the insert jams in the slot. The speed clamp (G50) is vital here: with G96 the rpm tries to go to infinity as the tool reaches centre.
Deep grooves: once the depth exceeds 6–8 times the insert width the blade deflects and the groove walls come out tapered. Reduce P to 1 mm, cut the feed by 30% and take the last 0.2 mm as a separate finishing plunge; or cut the groove in two widths, narrow first, then full width.
Internal grooves: same logic, opposite direction: the start X is smaller than the bore, the target X is the (larger) groove bottom diameter. The tool is designed for external grooves; adapt the program by hand following the rules in the guide and feed coolant through the bar for chip evacuation.
Typical alarms and shop-floor problems
| Symptom / alarm | Cause | Fix |
|---|---|---|
| PS0062 "Illegal command in G71–G76" | P or Q negative / zero, or written with a decimal point | Write P and Q as positive microns (P2000, Q2400) |
| Ridges left on the groove bottom | Q step larger than the insert width | Q ≤ 0.8 × insert width; the tool applies this automatically |
| Groove one insert width too wide | Tool offset on the right edge, program written for the left edge | Add the insert width to the start Z or re-measure the offset to the left edge |
| Insert broken, chip wrapped in the groove | R=0 (no chip breaking) or P too large | R 0.3–0.5, P 1–2 mm; reduce the feed |
| Part flew off at the end of parting / burr | No speed clamp, rpm ran away at centre | A clamp such as G50 S2000; reduce rpm over the last 3 mm |
| Tapered groove walls, size drifts | Long blade, high depth-to-width ratio | Short blade, lower P, finishing plunge |
| Tool stepped the wrong way in Z | Target Z on the wrong side of the start | Check the right face Z and width; the tool steps from the left wall towards the right |
Six common mistakes
- Writing P and Q with a decimal point.
P2000, notP2.0. A decimal either raises an alarm or gives a 2 micron peck. - Treating P as a diameter value. P is the radial plunge depth; 10 mm of depth from Ø80 to Ø60 means five plunges at P2000.
- Entering the wrong insert width. With a 3 mm insert entered as 4 mm the groove comes out 1 mm narrow and the Q step is too large.
- Starting X too close to the stock. G75 rapids to the first plunge; stock + 2–4 mm is a safe clearance, the tool uses +4.
- No speed clamp in constant surface speed. Parting and deep grooves push the rpm up towards centre under G96; G50 belongs in every program.
- Using the grooving tool for other cuts. A grooving insert works only in X (and Q-wise in Z); a longitudinal turning load snaps it. The Z moves in the G75 blocks are rapid steps only.
Frequently asked questions
Can I cut several grooves in one program with G75?
Yes; raise the groove count in the simulator and enter the right-face Z and width of every groove. A G0 approach, G75 R and G75 X Z P Q F block group is generated per groove; grooves of different widths are cut with the same tool and different Q values.
What is the R in the second block for, and why does the tool not write it?
R(Δd) in the second block is the relief amount in Z when the tool reaches the groove bottom; it is used only in one-directional X plunges to avoid rubbing the bottom. In grooving it is left at zero, which is why the tool omits it. If you add it, check its sign and size against the groove width.
How do I put a radius or chamfer on the groove corners?
G75 cuts a flat bottom. Corner radii either come from a radiused insert or from a separate G1/G2/G3 profiling pass after G75. For circlip grooves take the bottom radius from the standard (e.g. DIN 471/472) and match it with the insert radius.
How do I choose feed and cutting speed for grooving?
Grooving is interrupted and chip evacuation is poor; 60–70% of the longitudinal turning Vc and 0.05–0.12 mm/rev feed are typical. Use the grooving values from the insert catalog and check rpm and power with the Lathe Speed and Feed Calculator.