G74 cevrimi nasil calisir?
FANUC G74, "Kenar Gaga Delik Acma Cevrimi"dir (End-Face Peck Drilling). Parcanin alin yuzeyinden, eksen (Z) boyunca, periyodik geri cekmelerle (talas kirma) delik delmek icin kullanilir. Iki satir halinde programlanir:G74 R(e) — her paso sonu talas kirma icin geri cekme miktari.
G74 Z(w) Q(Δk) F(f) — Z: delik dibi konumu, Q: her seferinde inilen derinlik (mikron), F: ilerleme.
G74'un ikinci kullanim sekli
X(U) ve P eklenirse, G74 artik tek bir merkez delik degil, X ekseninde adim adim kayan bir yuzey/kademe peck cevrimine doner: G74 R(e) / G74 X(u) Z(w) P(Δi) Q(Δk) R(Δd) F(f). Bu modul, en sik kullanilan ve ogrenciler icin en temel olan SADECE Z EKSENINDE delik delme moduna odaklanir.Paso sayisi nasil hesaplaniyor?
Toplam delik derinligi, girilen paso derinligi Q'ya bolunerek kac pasoya ihtiyac oldugu hesaplanir. Her pasoda matkap Q kadar ilerler, R kadar geri cekilir, sonra bir onceki derinlikten devam ederek tekrar ilerler.Matkap ucu payi neden eklenir?
Standart bir matkabin ucu duz degil, konik bir sivri uca sahiptir (genelde 118°). Eger tam delik derinligi (silindirik kisim) istiyorsaniz, bu konik ucun boyu kadar fazladan ilerlemeniz gerekir. Sistem bu payi acidan otomatik hesaplar.With this free G74 peck drilling simulator and NC code generator you can enter the drill diameter, hole depth, peck depth Q and retract R, watch the live toolpath simulation and instantly generate the FANUC 0i-TC compatible two-block G74 program. For the theory see our G74 End-Face Peck Drilling & Grooving Cycle guide, for grooving along X the G75 Grooving Simulator, and for drill life the Drill Life & Cost Calculator.
What G74 is and its two forms
FANUC G74 is the end-face peck drilling cycle: it feeds the drill Q along Z, pulls back R to break the chip, feeds again and repeats until the programmed hole bottom. When X and P are added the same cycle becomes a face grooving / stepped facing cycle (G74 X(U) Z(W) P Q R F); this simulator concentrates on the form students and operators use most, straight peck drilling along Z only. The tool is a drill in the turret, the spindle turns the part, and the drill sits on the part axis at X0. Compared with a single G01 plunge, G74 breaks the chip regularly, lets coolant reach the bottom and prevents drill breakage, which makes it the standard method for holes deeper than 3×D. The grooving form and the U/W details are in the G74 peck drilling and face grooving guide.
G74 versus G01 drilling and the milling G83
| Method | Chip breaking | Retract | Suitable hole |
|---|---|---|---|
| G01 Z-… | None | None | Shallow holes (≤ 2–3×D), soft material |
| G74 R / G74 Z Q F | Every Q | Short retract R (chip breaking) | Lathe holes 3–8×D, steel and stainless |
| G83 (mill / machining centre) | Every Q | Full retract (chip evacuation) | Milling holes above 5×D with difficult chip evacuation |
The important distinction: the G74 retract is short; the drill does not leave the hole, it only breaks the chip. For very deep holes (over 8×D) where chips must be evacuated completely, add a G0 full-retract block every few pecks, or move to a through-coolant deep-hole drill as the tool maker recommends.
Using the simulator step by step
- Part diameter: drawing only; it does not appear in the code.
- Drill diameter: the basis of the RPM calculation. For Ø10 and Vc 25 m/min (HSS in steel), n = 1000·25/(π·10) ≈ 796 rpm. For carbide drills use Vc 80–120 m/min via the "Manual" card.
- Start Z: where the drill waits in front of the face, typically +2 mm. After each peck the cycle only backs off by R; the start Z is just the first approach.
- Hole bottom Z: written into the program as entered, and it is the position the drill point reaches. If you need full-diameter depth, add the point length yourself: for a 118° Ø10 drill the point is ≈ 0.3×D = 3 mm, so 30 mm at full diameter means Z-33.
- Drill point angle: lets the simulation draw the conical bottom and count the pecks correctly; 118° is standard, 135–140° for carbide and self-centring drills.
- Peck depth Q: entered in mm, written in microns (3 mm → Q3000). Q ≈ 1×D for HSS, 1.5–2×D for carbide, 0.5–0.7×D in stainless are good starting points.
- Retract R: the chip-breaking distance, 0.3–1 mm is enough. A larger value lengthens the cycle without breaking the chip any better.
- Start the simulation, watch the pecks, then copy the code or download the .nc file.
Reading the generated program line by line
With the default values (Ø10 drill, Z2 → Z-30, Q 3 mm, R 0.5 mm, steel) the tool produces:
O0001
G21 G99
G50 S2500
T0505 M08
G97 S796 M03
G0 X0. Z2.00
G74 R0.50
G74 Z-30.00 Q3000 F0.15
G0 X150. Z200.
M09
M05
M30
%| Block | What it does |
|---|---|
G97 S796 M03 | Drilling uses constant RPM; the drill diameter does not change, so G96 is pointless and would send the RPM to the ceiling at the centre. |
G0 X0. Z2.00 | Drill on the part axis (X0), 2 mm in front of the face. Any centre offset breaks the drill, so make sure X0 is set correctly in the tool offset. |
G74 R0.50 | First block: 0.5 mm retract after every peck. If omitted, the control uses the value in parameter 5139. |
G74 Z-30.00 Q3000 F0.15 | Second block: hole bottom Z-30, peck depth 3000 microns = 3 mm, feed 0.15 mm/rev. Q is written unsigned and without a decimal point. |
| (inside the cycle) | 32 mm total travel / 3 mm = 10.7 → 11 pecks. Each peck feeds 3 mm, rapids back 0.5 mm and continues at feed from where it stopped; at the bottom the tool rapids back to the start point. |
G0 X150. Z200. | Retract to the tool change position. |
The official FANUC training example has the same structure and shows a long hole: G97 S280 M03, G00 X0 Z5.0 T0202 M08, G74 R1.0, G74 Z-90.0 Q5000 F0.23, G00 X200.0 Z150.0 T0200. A 90 mm depth is drilled in eighteen 5 mm pecks.
Choosing Vc, f and Q
| Material | HSS drill Vc (m/min) | Carbide drill Vc (m/min) | f (mm/rev, Ø8–12) | Suggested Q |
|---|---|---|---|---|
| Carbon steel (1020–1050) | 20–30 | 80–120 | 0.12–0.20 | 1×D (HSS), 1.5–2×D (carbide) |
| Stainless 304/316 | 10–15 | 50–80 | 0.08–0.14 | 0.5–0.7×D |
| Grey cast iron | 25–35 | 90–140 | 0.15–0.25 | 1–1.5×D |
| Aluminium 6061 | 60–100 | 150–250 | 0.15–0.30 | 1.5–2×D |
| Brass | 40–60 | 120–180 | 0.10–0.20 | 1.5×D |
These are general starting ranges; the tool maker's catalogue always takes priority. Unlike drilling on a mill, lathe drilling is done with a stationary drill in a rotating part, so the risk of the drill wandering grows with its length: above 5×D spot the centre first, keep the first peck short and clamp the drill as short as possible. To check speed and feed quickly use the drilling speed and feed calculator, and for tool life and cost per hole the drill tool life calculator.
Grooving form: what happens when X and P are added
When X(U) and P are given in the second block the cycle turns into face grooving: G74 R(e) / G74 X(U) Z(W) P(Δi) Q(Δk) R(Δd) F. The tool pecks to the bottom in Q steps along Z, comes out, shifts P (microns) in X and plunges again until X(U) is reached. Δd is the side relief at the bottom (the cutting edge backing away from the wall); in the plain drilling form without X(U) it is taken as 0. This form is the face-side counterpart of the G75 grooving cycle: G75 plunges in X and shifts in Z, G74 plunges in Z and shifts in X.
Alarms and problems seen on the shop floor
| Symptom | Cause | Fix |
|---|---|---|
| PS0011 FEED ZERO (COMMAND) | No F in the second G74 block | Add F (mm/rev under G99) |
| Q block rejected / cycle went down in one plunge | Q written with a decimal (Q3.0) or in mm (Q3) | Q is an integer in microns: Q3000 for 3 mm |
| Drill broke on the first plunge | X0 off centre (offset error) or no centre hole | Check the tool X offset, spot with a centre drill |
| Hole bottom short of size | Z entered as full depth without the point length | Add 0.3×D (118°) point length to Z |
| Chips wrap around, surface scored | Q too large or feed too low (thin chip does not break) | Reduce Q, raise f, set R to 0.5–1 mm |
| Drill discolours, short life | Vc too high or coolant not reaching the bottom | Lower Vc, verify M08, reduce Q |
| Hole tapered / oversize | Drill runout or unevenly ground lips | Measure runout, replace the drill |
Six common mistakes
- Writing Q in millimetres; Q3 means three microns and the cycle performs thousands of tiny pecks.
- Drilling under G96 constant surface speed; the drill is at the centre, so the RPM runs to the ceiling. Use G97.
- Forgetting the point length; the Z value is the drill point position, not the full-diameter depth.
- Choosing a large retract R of 5–10 mm; the chip breaks within the first 0.3 mm, the rest is lost time.
- Starting with a long drill without spotting; on an uneven or rough face the drill walks.
- Placing the start Z on the face (Z0); the first peck starts with an impact. Stay 2 mm in front.
Frequently asked questions
Why is Q written in microns?
In FANUC the increment addresses of the multiple repetitive cycles (P and Q in G74/G75, P and Q in G76) do not accept a decimal point and are written in the least input increment, the micron. 3 mm = Q3000, 0.5 mm = Q500. The tool does this conversion for you; when writing by hand, do not forget the three zeros.
Is the G74 R block mandatory?
No. If it is omitted the control uses the retract amount stored in parameter 5139. Writing the R block is good practice so the program behaves the same on any machine; running a program on someone else's lathe without knowing which parameter value is active can produce surprises.
Can I add a dwell (G04) at the hole bottom?
G74 has no built-in dwell and G04 cannot be written in the cycle block. If a blind hole bottom must be clean, feed back to the bottom with G01 after the cycle and dwell briefly with something like G04 P500, or perform the last peck with a small Q in a separate G74 block.
How does the simulator count the pecks?
It divides the travel from the start Z to the hole bottom (including the point angle) by Q and rounds up; with the default values that is 11. The machine works the same way: the last peck is only as long as the remaining distance, and the cycle ends exactly at Z.