G73 cevrimi nasil calisir?
FANUC G73, "Sablon Tekrar" (Pattern Repeating) cevrimidir. Dokum veya dovme gibi onceden kabaca sekillendirilmis ham parcalarda kullanilir. G71'in aksine paso derinligi belirtilmez; tezgah, programlanan profilin AYNI SEKLINI, her seferinde biraz daha kucuk bir ofsetle tekrar tekrar izleyerek fazla stogu soyar.G73 U(Δi) W(Δk) R(d) — capta ve boyda toplam fazla stok miktari, ve kac pasoya bolunecegi (paso SAYISI, derinlik degil).
G73 P(ns) Q(nq) U(Δu) W(Δw) F(f) — profil baslangic/bitis satir no, capta ve boyda finis payi, ilerleme.
G70 finis cevrimi nedir?
G70 P(ns) Q(nq), G73'te birakilan finis payini alir. Ayni takimla veya farkli finis takimiyla, P-Q arasindaki profili izleyerek son olcuye tornalar. G71 modulundekiyle birebir aynidir.Profil nasil tanimlanir?
Her kademe icin cap (Ø), bittigi Z konumu ve onceki kademeye gecis tipi (duz kose / pah 45° / dis radyus / ic radyus / konik) girilir. Sistem bunlari N(ns)..N(nq) blogu olarak FANUC profiline cevirir — G71 modulundeki profil mantigiyla aynidir.Neden G41/G42 kullanmiyoruz?
Cogu FANUC kontrolde G41/G42 kaba cevrimde yok sayilir, sadece finiste calisir; bu da kaba pasoda hatali kesim riski dogurur. Bu yuzden sistem nose R telafisini elle hesaplayip koordinatlara gomer; daha guvenli ve ongorulebilir.With this free G73 pattern repeating simulator and NC code generator you can enter the raw stock diameter, profile stages, X/Z relief allowances and pass count, watch the live toolpath simulation and instantly generate FANUC 0i-TC compatible ready-to-run G-code (G73 + G70). For the theory see our G73 Pattern Repeating Rough Turning Cycle guide, for the differences from G71 our G71 Rough Turning Cycle article, and for facing the G72 Face Roughing Simulator. For longitudinal roughing from solid bar also try our G71 Rough Turning Simulator.
What G73 is and when to use it
The FANUC G73 pattern repeating cycle traces the programmed finished profile again and again, each time a little further in, peeling the excess stock away in profile-shaped layers. Where G71 cuts longitudinal steps and G72 cuts facing slices, G73 copies the shape itself, which is why its natural home is castings, forgings and pre-machined blanks: the stock is already close to the finished shape, carries an even 2–5 mm of surface allowance, and three to five repeats are enough to remove it. On a stepped shaft from solid bar the first G73 repeats cut air; there the G71 rough turning cycle is far more efficient. The theory is covered in the G73 pattern repeating guide; this page is about using the tool and reading the code it produces. One often overlooked advantage of G73 is that, unlike G71/G72, the profile does not have to be monotonic, so pockets and recesses can be roughed in a single call.
G73 compared with G71 and G72
| Feature | G73 | G71 | G72 |
|---|---|---|---|
| Material removal | Offset copies of the profile | Steps parallel to Z | Slices parallel to X |
| Pass input | Total allowance Δi/Δk + repeat count R | Depth of cut U(Δd) | Depth of cut W(Δd) |
| Suitable blank | Casting, forging, pre-machined | Solid bar | Solid disc / flange |
| Profile restriction | None, pockets allowed | Monotonic in X and Z (Type I) | Monotonic in X and Z |
| Finish | G70 P Q | G70 P Q | G70 P Q |
Using the simulator step by step
- Raw stock diameter and insert nose radius: Ø84 and 0.8 mm by default. The nose radius is used only for tool nose radius compensation (TNRC) in the G70 finish block; roughing passes ignore it.
- Number of stages and the stages themselves: enter the profile from the face towards the chuck, small diameter to large. The default has three stages: Ø30 to Z-15, Ø40 to Z-30, Ø50 to Z-45. Each stage can have a transition type (sharp corner, chamfer, radius, taper).
- X relief Δi: the total excess stock on the radius, not the diameter. On a casting measure how far the surface stands off the finished profile; a Turkish vocational example goes from a Ø100 casting to a profile whose smallest diameter is Ø38 with U31.
- Z relief Δk: the total excess stock in length. Enter 0 if the face is not machined.
- Repeat count R: how many repeats, a count rather than a depth. Dividing Δi by R is how you decide the stock per repeat: 3 mm in 3 repeats is 1 mm on the radius each time.
- Finish allowances U and W: the stock left for G70; 0.5 mm on diameter and 0.1 mm in length are typical.
- Material: the card sets Vc and f; the tool writes the program header with G96 constant surface speed and a G50 spindle limit.
- Start the simulation, watch the profile copies move inwards, then copy the code or download the .nc file.
Reading the generated program line by line
With the default values (Ø84 stock, three stages, Δi 3, Δk 2, R 3, U0.5 W0.1, steel) the tool produces:
O0001
G21 G99
G50 S2500
T0101 M08
G96 S130 M03
G0 X94. Z4.
G73 U3 W2 R3
G73 P10 Q20 U0.5 W0.1 F0.20
N10 G0 X30.
G1 Z0. F0.2
Z-15.
X40.
Z-30.
X50.
Z-45.
N20 X84.
G70 P10 Q20 F0.20
G0 X150. Z200.
M09
M05
M30
%| Block | What it does |
|---|---|
G0 X94. Z4. | Cycle start point: stock + 2×Δi + 4 mm on diameter, Δk + 2 mm in length. G73 returns here after every repeat, so the point must lie completely outside the profile. |
G73 U3 W2 R3 | First cycle block: 3 mm (radius) total allowance in X, 2 mm in Z, 3 repeats. U/W here mean allowance; in the second block they mean finish allowance. Same letters, different meaning. |
G73 P10 Q20 U0.5 W0.1 F0.20 | Profile between N10 and N20; 0.5 mm finish allowance on diameter and 0.1 mm in length; roughing feed 0.20 mm/rev. F values inside the profile are ignored by G73 and used by G70. |
N10 G0 X30. | The first profile block contains X only and must be G00 or G01 (PS0065). |
G1 Z0. … Z-45. | The finished profile: Ø30 face, then Ø30×15, Ø40×15 and Ø50×15 steps. |
N20 X84. | The profile ends by moving out beyond the stock diameter; this is the Q block. |
G70 P10 Q20 F0.20 | Finish cycle: traces the same profile with the allowance set to zero. TNRC (G41/G42) takes effect only here. |
How to work out Δi, Δk and R
Δi is the largest radial difference between the blank surface and the finished profile. On a casting you measure it with calipers; on solid bar it is (stock diameter − smallest profile diameter) / 2, which for Ø84 bar and Ø30 is 27 mm. The tool's default Δi = 3 is a teaching example that stands for a cast part; if you really want to take a solid Ø84 bar down to Ø30 you need Δi = 27 with R ≈ 9–12, or better, G71. The repeat count R comes from dividing Δi by a sensible stock per repeat: aim for 1.5–3 mm on the radius per repeat in steel. The vocational example makes this concrete: from a Ø100 casting to Ø38 with G73 U31 W2 R15, 15 repeats of about 2 mm each. This simulator starts the first repeat at the full Δi relief and moves each following repeat Δi/R further in; some controls place the last roughing repeat directly on the finish allowance line (step Δi/(R−1)). Check the diagram in your machine's manual once; thanks to G70 the finished size is the same either way.
Rules for defining the profile
The P block must contain X (or U) only and must be G00 or G01; add a Z and you get PS0065. The P–Q blocks must follow the G73 line immediately, with nothing in between. F, S and T may be written inside the profile but G73 ignores them; G70 uses them, so putting the finish feed on the first profile line is the right approach. In the same way G41/G42 are written inside the profile, are ignored during roughing and become active in G70. Subprogram calls (M98/M99) are not allowed inside the profile block (PS0066). The official FANUC training example shows all of these rules together: G73 U14.0 W14.0 R3, G73 P014 Q020 U4.0 W2.0 F0.3 S0180, N014 G00 G42 X80.0 Z2.0, N015 G01 W-20.0 F0.15 S0600 … N020 G40, G70 P014 Q020. The S values changing at each step inside the profile are there for G70 as well.
Alarms and problems seen on the shop floor
| Symptom | Cause | Fix |
|---|---|---|
| PS0061 ADDRESS P/Q NOT FOUND | P or Q missing from the second G73 block | Write P and Q in the second block |
| PS0063 SEQUENCE NUMBER NOT FOUND | The N numbers in P/Q do not exist or differ | Check the N10 and N20 sequence numbers |
| PS0065 G71–G73 FIRST BLOCK ERROR | P block is not G00/G01 or contains Z | Write the P block as N10 G0 X30. |
| PS0066 UNAVAILABLE COMMAND IN G71–G73 | M98/M99 or a forbidden G code inside the profile | Move the subprogram call outside the profile |
| First repeats cut air, cycle takes too long | G73 on solid bar with a small Δi, or an unnecessarily large Δi | Enter the real allowance; use G71 on solid bar |
| Tool broke on the first repeat | Δi smaller than the real casting allowance; first pass deeper than expected | Measure Δi at the thickest spot, increase R |
| Finished size wrong | U/W finish allowance missing from the second block, or G70 forgotten | Add U0.5 W0.1 and the G70 P Q block |
Six common mistakes
- Reading the U in the first block as a diameter; Δi is a radius, while the finish allowance U in the second block is a diameter.
- Treating R as a depth of cut and entering 2; R is the repeat count, and 2 removes a 3 mm allowance in two heavy bites.
- Choosing a start point close to the profile; every repeat starts there, so it must lie outside stock + Δi.
- Using G73 on solid bar; most of the cutting time goes into repeats through air.
- Writing G41/G42 in front of the G73 line; compensation belongs inside the profile block and works only in G70.
- Entering the profile from large diameter to small; G73 reads the profile from P to Q, face towards chuck.
Frequently asked questions
Is G73 never used on solid material?
It can be, but it is inefficient: since the stock does not resemble the profile, the first repeats mostly cut air. If the profile contains pockets or recesses (shapes G71 Type I does not allow), G73 is still a practical solution; otherwise choose G71.
Do Δi and Δk have to be equal?
Not necessarily, but because the FANUC cycle shrinks the X and Z offsets by the same proportion on every repeat, very different Δi/Δk values mean the repeats no longer keep the profile's shape exactly. Enter Δk = 0 if the face is not machined; otherwise keep Δk equal to the real length allowance.
Can I finish with a different tool in G70?
Yes. After G73, retract with G0 to a safe point, call the finishing tool such as T0303, enter its nose radius in the offset page and call G70 P10 Q20 again. G70 traces the same N10–N20 profile, this time with compensation; the F and S values you wrote inside the profile now apply.
Does constant surface speed (G96) cause problems with G73?
No; the RPM adjusts automatically as the diameter changes and removes the casting skin more evenly. The tool writes G96 S130 together with a G50 S2500 limit; if the RPM hits the ceiling on small-diameter steps the cutting speed drops, so raise the G50 value as far as your machine allows.