📐 1. Why Do We Use Canned Cycles?
Writing separate G01 linear coordinates for every single roughing pass on a complex shaft takes a long time, results in massive program files, and makes it incredibly easy to make a math error.
-
The Manual Way: You have to manually code the tool moving in, cutting across, retracting, moving back, plunging deeper, and cutting across again for every millimeter of stock removal.
-
The Canned Cycle Way: You define the final, completed shape blueprint profile just once. The Fanuc or Haas controller automatically calculates all the rough intermediate passes, depth steps, and retract clearances for you.
🛠️ 2. The G71 Outer/Inner Diameter Roughing Cycle
The G71 cycle is a multi-repetitive profile line template. It reads a two-block format on modern Fanuc controllers to strip away raw material rapidly.
The Two-Line Fanuc G71 Syntax
G71 U(d) R(e) ;
G71 P(ns) Q(nf) U(u) W(w) F(f) ;
Breaking Down the Variables:
-
U (d) (Line 1): Depth of cut for each individual pass (specified as a radius value). If U2.0, the tool removes 4 mm of total diameter per pass.
-
R(e) (Line 1): The escape/retract clearance distance. How far the tool lifts off the metal profile before rapid-jogging back to the start.
-
P (ns) (Line 2): The starting sequence number of your target profile design (e.g., P100).
-
Q (nf) (Line 2): The ending sequence number of your target profile design (e.g., Q200).
-
U (u) (Line 2): Finishing allowance left on the X-axis diameter for the finish tool (e.g., U0.5 leaves 0.5 mm of material).
-
W (w) (Line 2): Finishing allowance left on the Z-axis face for the finish tool (e.g., W0.1 leaves 0.1 mm of material).
-
F (f) : The cutting feed rate during roughing passes (e.g., F0.25).
🔄 3. The G70 Profile Finishing Cycle
Once the G71 cycle finishes clearing out the bulk stock, it leaves behind the small material allowance defined by your U and W values. The G70 cycle jumps in to execute a single, continuous, high-precision pass to clean up the profile to blueprint size.
The G70 Syntax
G70 P100 Q200 F0.12 ;
How it reads: The machine automatically references sequence blocks N100 through N200, ignores the roughing allowances, and runs the path perfectly at a crisp finishing feed rate (F0.12).