G90 cevrimi nasil calisir?
FANUC G90, en temel torna hazir cevrimidir. Her G90 satiri, takimi 4 adimda calistirir: (1) Hizli X hedefine git, (2) Z hedefine F ilerlemesiyle kes, (3) Hizli baslangic X'e geri don, (4) Hizli baslangic Z'ye geri don. Boylece bir "U" sekli cizer.Duz: G90 X(U)__ Z(W)__ F__
Konik: G90 X(U)__ Z(W)__ R__ F__
G90 vs G71 vs G94 — ne zaman hangisi?
G90 — Boyuna (Z'ye paralel) kaba tornalamada, basit ve az pasolu kademelerde. En temel; pasolari elle yonetirsiniz.G71 — Cok pasolu ve/veya kompleks profilli boyuna kaba tornalamada. Pasolari ve profil izlemeyi otomatik yapar.
G94 — Alina paralel (X'e paralel) kesme cevrimi; disk veya flansin alin yuzeyini adim adim tornalar. G90'in alindaki karsiligidir.
Modal cevrim ozelligi
G90 aktifken sadece X (veya Z) degistirilerek cevrim tekrar edilir. Bu, kaba pas pas X azaltirken cok az kod yazilmasini saglar. 01 grubundan G00 veya G01 girilirse modal mod iptal olur.To learn the full G90 syntax, incremental U/W usage and all the details, read our G90 Single Turning Canned Cycle guide.
Related tool: while G90 cuts longitudinally, for face and shoulder surfaces also try our G94 Face Turning Simulator and NC Code Generator.
Back to basics: to see step by step what the G90 canned cycle does internally, try our G0/G1 Basic Moves Simulator.
Which G90? Turning cycle vs. absolute positioning
People searching for "G90 G-code" usually mean one of two things. On a milling machine, or on a lathe running G-code system B or C, G90 selects absolute positioning: it produces no motion, it only tells the control how to read coordinates. On FANUC lathes using G-code system A (0i-TC, 0i-TD, 16/18/21T and most Asian lathe controls), G90 is the OD/ID single-pass cutting cycle: one block performs four moves (approach, cut, retract, return). This simulator covers the second meaning. On system B and C the same cycle is called with G77, and absolute/incremental is chosen with G90/G91. You can tell which system your machine uses from parameter 3401 bits 6–7 (GSB/GSC), or simply from the programs: if incremental moves are written with U and W instead of G91, you are on system A.
When to use G90, G71 or G94
| Cycle | Cutting direction | Who manages the passes? | Typical use |
|---|---|---|---|
| G90 | Parallel to Z (longitudinal), straight or taper | You: reduce X line by line | Single-step shafts, short shoulders, 2–8 passes, short programs |
| G71 | Longitudinal, following a profile | Control: automatic via U/W/R/P/Q | Multi-step profiles with radii and tapers |
| G94 | Parallel to X (facing) | You: deepen Z line by line | Flanges, discs, shoulder faces |
| G92 | Longitudinal, synchronised to the pitch | You | Threading (the threading version of G90) |
Rule of thumb: if the part has one step and the pass count fits on one hand, G90 is the fastest route. It is easy to write, easy to read, and an operator can edit one X value at the machine to take another cut. Switch to G71 once the profile gets complex. Do not force G90 onto a face; that is what the G94 face turning cycle is for.
Using the simulator step by step
- Raw stock and target diameter: to go from Ø60 stock to Ø40, enter 60 and 40. The 20 mm difference in diameter is 10 mm of stock on the radius; the pass count is calculated from that 10 mm.
- Start Z and end Z: Z2 is the safe point 2 mm in front of the face; Z-40 is the shoulder where the step ends. End Z is always negative.
- Turning mode: in OD mode X shrinks every pass; in ID (boring) mode the hole grows, X increases every pass, and the tool asks for the pre-drilled and finished bore diameters.
- Taper: leave R=0 for a straight shaft. For a taper enter R as the radius difference; the sign rule is explained below.
- Depth of cut: a radius value. 2 mm means the diameter drops 4 mm per G90 block. Reasonable ranges: 1.5–3 mm in carbon steel, 1–2 mm in stainless, 3–5 mm in aluminium.
- Finish allowance: leave 0.2–0.5 mm; the tool adds a final pass at a lower feed. Enter 0 and the roughing passes go straight to size.
- Material and G50: the material card sets Vc and f, the tool computes the RPM at the nominal diameter; G50 S is the spindle speed limit the machine may not exceed.
- Start the simulation, watch the toolpath, then copy the code or download it as .nc.
Reading the generated program line by line
With the default values (Ø60 → Ø40, Z2 → Z-40, 2 mm depth, 0.3 mm finish allowance, steel) the simulator produces this program:
O0001
G21 G99
G50 S2500
T0101 M08
G97 S955 M03
G0 X64. Z2.00
G90 X56.00 Z-40.00 F0.250
X52.00
X48.00
X44.00
X40.60
X40.00 F0.150
G0 X150. Z200.
M09
M05
M30
%| Block | What it does |
|---|---|
G21 G99 | Metric units, feed per revolution. The F0.25 in the G90 block therefore means 0.25 mm/rev. |
G50 S2500 | Caps the spindle at 2500 rpm; even with G96 this value is never exceeded. |
G97 S955 M03 | Constant RPM. For Vc 180 m/min at Ø60, n = 1000·180/(π·60) ≈ 955 rpm. |
G0 X64. Z2.00 | Cycle start point: 2 mm outside the stock (4 mm on diameter) and 2 mm in front of the face. Every pass returns here. |
G90 X56. Z-40. F0.25 | First pass: rapid to X56, feed to Z-40 at F0.25, rapid out to X64, rapid back to Z2. Diameter 60 → 56. |
X52. … X44. | Modal repeats: G90 is not rewritten, only a new X is given; Z-40 and F0.25 are remembered. Each line takes 4 mm off the diameter. |
X40.60 | Last roughing pass: Ø40 + 2×0.3 finish allowance = Ø40.6. |
X40.00 F0.150 | Finish pass: the 0.3 mm radial allowance is removed in one cut at a lower feed. |
G0 X150. Z200. | Leaves the cycle. G0 (group 01) cancels G90. |
How the pass count and finish allowance are calculated
The roughing pass count comes from the radial stock minus the finish allowance: (10 − 0.3) / 2 = 4.85, rounded up to 5 roughing passes. The tool takes the first four at the full 2 mm (4 mm on diameter), finishes the fifth with the remaining 1.7 mm at Ø40.6, and the sixth block is the finish cut. This arrangement avoids a paper-thin last roughing pass that only rubs the surface. Apply the same logic when writing programs by hand: equal passes, one remainder pass, then the finish. Dropping the finish feed to 50–60% of the roughing feed improves surface roughness noticeably; the tool moves from F0.25 to F0.15. To predict Ra in advance use the surface roughness calculator.
The sign of R in taper turning
The taper format is G90 X(U)_ Z(W)_ R_ F_. R is the difference between the radius where the cut starts and the radius where it ends; enter a radius, not a diameter. On a classic OD taper that is smaller at the free end (Z0 side) and larger towards the chuck, the tool starts cutting at the small diameter and moves towards the large one, so R is negative. For a taper narrowing from Ø50 to Ø44 over 40 mm, R = (44 − 50)/2 = −3. The FANUC training manual example uses the same convention: G90 X55.0 W-42.0 F0.25, then Z-12.0 R-1.75, Z-26.0 R-3.5, Z-40 R-5.25 — R grows in proportion to Z because the taper angle is constant. When you select "Taper (R≠0)" in the simulator and enter R, this sign rule is applied automatically; if you enter the wrong sign you will see the tool plunge into the face in the animation. In ID mode the sign is reversed. To get R from a taper angle, use the taper angle calculator.
Points to watch in ID (boring) mode
Boring follows the same logic with the directions reversed. The start point sits inside the hole, at an X slightly smaller than the existing bore and 2 mm in front of the face; X grows with every G90 block. Going from a Ø20 pre-drilled hole to Ø32, the tool starts at X18 Z2 and generates G90 X24. Z-40. F0.175, X28., X31.4 and then X32. F0.105 for the finish. The boring bar must reach the end Z, and its shank must be enough smaller than the bore that the retract (the cycle's third move pulls X back to the small start diameter) does not rub the bore wall. Reduce Vc by 10–20% compared with OD turning; a slender bar chatters. On a tapered bore the sign of R is the opposite of the OD case.
Alarms and problems seen on the shop floor
| Symptom | Cause | Fix |
|---|---|---|
| PS0011 FEED ZERO (COMMAND) | No F in the G90 block and none commanded earlier | Add F to the first G90 block (mm/rev under G99) |
| OT0500 / OT0501 (+X / −X overtravel) | Start point or the exit G0 exceeds a stroke limit | Start X = stock + 2 mm; check the exit point against the reference position |
| Tool plunges into the face, taper comes out reversed | Wrong sign of R, or R entered as a diameter | R = radius difference; negative on a classic OD taper |
| First pass far too deep, insert broke | Start X too far inside the stock, or first G90 X not close to the stock | Start X = stock + 2–4 mm; first X = stock − 2×depth |
| Cycle did not repeat, tool only moved in X | A G00/G01/G02/G03 (group 01) block was inserted and cancelled G90 | In repeat blocks give only X (and Z, R if they change) |
| Wrong motion on a system B/C machine | G90 was interpreted as absolute positioning | Use G77, or switch the control to system A |
Six common mistakes
- Treating the depth of cut as a diameter value and taking 4 mm instead of 2 mm; in G90 X is a diameter, the depth of cut is a radius.
- Choosing the start Z on the face (Z0); the tool hits the face as it starts cutting. Stay 2–3 mm in front.
- Using G96 constant surface speed without a G50 spindle limit; RPM runs away at small diameters.
- Going to size at the roughing feed with no finish allowance; the dimension is right, the surface is not.
- Inserting a G0 retract between modal repeat lines to check a dimension; the cycle is cancelled and the next X line becomes a plain rapid move.
- Forcing G90 where the shoulder needs a radius; G90 leaves a sharp corner, a radius needs G71 + G70 or a separate G1/G2 pass.
Frequently asked questions
What is the difference between G90 and G01?
G01 produces a single linear move; one pass needs four separate blocks (down in X, cut in Z, out in X, back in Z). G90 performs those four moves in one block and, because it is modal, the following passes are repeated with only an X value. A four-pass step is 16 blocks with G01 and 4 blocks with G90.
When are U and W used in a G90 block?
U and W are incremental values: G90 U-4. W-42. F0.25 means "4 mm on diameter inwards from the current X, 42 mm along Z from the current Z". They are useful in flexible programs that machine the same step from different stock sizes and in subprograms; while learning, absolute X/Z is the safer choice.
Can I use constant surface speed (G96) with G90?
Yes. With G96 S180 the RPM rises automatically as the diameter shrinks pass by pass, which gives a more even surface. The simulator outputs G97 constant RPM for teaching purposes; if you use G96 on the machine, always put a G50 S limit in front of it.
Does G90 clean up the shoulder at the end of the step?
G90 completes the cut at the end Z and retracts in X; the shoulder face is skimmed by the side edge of the insert, but if the tool's end cutting edge angle is less than 90° a small taper mark remains. If the shoulder face is toleranced, add a G94 pass or a G01 facing move at the end.