The G75 cycle is one of the most efficient ways to perform radial grooving or parting-off on a CNC lathe. Instead of manually coding every single plunge and retract move, G75 allows you to define a wide groove or a series of grooves with just two lines of code.
Here is a guide on how to master this cycle for cleaner chips and faster cycle times.
Why Use the G75 Cycle?
Standard linear interpolation (G01) for grooving often leads to long, stringy chips that wrap around the workpiece or tool. The G75 cycle solves this by:
- Peck Grooving: Breaking chips automatically by retracting the tool periodically.
- Simplification: Reducing dozens of lines of code into two.
- Precision: Ensuring consistent side-shifts for grooves wider than the insert width.
The G75 Syntax (Fanuc Format)
The cycle is typically written in a two-line format:
G75 R(e);
G75 X(u) Z(w) P(∆i) Q(∆k) F(f);
Breakdown of Parameters:
First Line:
- R (e): The return amount (retract distance) after each peck to break the chip.
Second Line:
- X (u): The final diameter (target depth) of the groove.
- Z (w): The final position of the groove along the Z-axis (for wide grooves).
- P (∆i): The depth of each peck in the X-axis (measured in microns, radius value).
- Q (∆k): The stepping amount in the Z-axis (measured in microns). This is used if the groove is wider than the tool.
- F (f): The feed rate.
A Practical Example
Imagine you have a 3mm wide grooving tool and you need to cut a groove that is 10mm wide, starting at Z-20.0 and ending at Z-30.0, with a final diameter of 40mm.
G-Code
G00 X62.0 Z-20.0 ; Approach point (Start of the groove)
G75 R0.5 ; Retract 0.5mm after each peck
G75 X40.0 Z-30.0 P2000 Q2500 F0.1 ;
What happens here?
- X40.0: The tool plunges to the 40mm diameter.
- P2000: The tool pecks 2mm (radius) at a time, then retracts 0.5mm (R) to break the chip.
- Q2500: After reaching the bottom, the tool retracts, moves 2.5mm in the Z direction, and repeats the plunge until it reaches Z-30.0.
- Note: Since the tool is 3mm wide, a Z-step (Q) of 2.5mm ensures an overlap so no material is left behind.
3 Professional Tips for G75
1. The “Micron” Rule
One of the most common mistakes is forgetting that P and Q are written in microns.
- If you want a 1mm peck, you must write P1000.
- If you write
P1.0, the machine will either throw an error or perform a peck so small it’s invisible!
2. Clearance is Key
Always position your tool slightly above the material (in X) and exactly at the start of the groove (in Z) before calling the G75 block. The cycle uses your current position as the starting reference.
3. Chip Control
If you are cutting a deep groove in tough material (like stainless steel), keep the R value small (0.1 to 0.5mm). This keeps the tool close to the cut while still providing enough relief to snap the chip.