Lathe G-Code: Turning, Facing, Threading, and Grooving

Lathe G-Code: Turning, Facing, Threading, and Grooving

Why Lathe G-Code Is Different from Mill G-Code

A CNC lathe rotates the workpiece while stationary tools move in two axes: Z (along the spindle centerline) and X (toward or away from the centerline). Because the part is round, X values are usually programmed as diameters, not radii, unless you switch to radius mode. Every Haas lathe control defaults to diameter programming, so X2.000 means the tool is at a 2.000 in. diameter, which is 1.000 in. from the centerline. Confirm your control's setting before you run any program.

Safety Before You Touch the Machine

Before loading a workpiece or setting up tooling, follow lockout/tagout (LOTO) procedures whenever you need to reach into the work envelope for a non-running task such as jaw changes or manual tool installation. Wear safety glasses with side shields at all times on the shop floor. Confirm the chuck jaws grip the stock with enough engagement—a rule of thumb is at least two-thirds of the jaw face in contact. Never stand directly in line with the spindle axis while the chuck is spinning. Keep the chip guard or enclosure door closed during any automatic cycle. When running a new program for the first time, use single-block mode and a feedrate override at 0–25 % so you can stop the cycle before a crash.

Facing and Rapid Positioning: G00 and G01

A facing cut removes material from the face of the stock to establish a clean, flat reference surface perpendicular to the spindle.

• G00 — Rapid traverse; moves the tool at maximum machine speed. Use only for positioning, never for cutting.
• G01 — Linear feed; moves at a programmer-specified feedrate (F word, in inches per minute or inches per revolution).

A typical facing block:

```

G00 X2.200 Z0.1; (rapid to just outside stock diameter, 0.1 in. clear of face)

G01 Z0.0 F0.012; (feed to face surface)

G00 X-0.05; (rapid across face to center; slight negative X cleans center burr)

G00 Z0.1; (retract)

```

Stock-Removal Cycle G71 and Finish Cycle G70

G71 is a canned rough-turning cycle. You define the finished contour in a series of blocks labeled with sequence numbers (N words), then call G71 with parameters that tell the control how much to hog off per pass and how much stock to leave for finishing.

Key G71 parameters (Haas format):

• P — sequence number of the first contour block
• Q — sequence number of the last contour block
• U — diameter stock allowance to leave for finish (positive leaves stock on the OD)
• W — Z-axis stock allowance to leave for finish
• D — depth of cut per rough pass (radius value, no decimal on some controls—check your reference)
• F — roughing feedrate

G70 is the finish pass cycle. It retraces the same P–Q contour blocks at a finer feedrate and removes the U/W allowance left by G71.

Contour blocks between P and Q describe the finished shape: diameters, tapers (G01 with both X and Z words), and radii (G02/G03). The control automatically calculates each rough pass offset.

External Grooving: G75

G75 is the peck-grooving cycle for the X axis. It plunges the grooving tool to a target X diameter in incremental pecks, retracts to clear chips, then advances in Z for multi-groove patterns.

Key G75 parameters:

• X — groove bottom diameter
• Z — Z-end of groove pattern (for multiple grooves)
• P — X peck increment (no decimal, in 0.0001 in. units on many Haas controls—verify)
• Q — Z step between grooves
• F — feedrate

For a single groove, set Z equal to the groove center position and Q to zero.

Single-Point Threading: G76

G76 is a two-block threading cycle that makes multiple passes, each one slightly deeper, until the thread is complete. The tool approaches on an angle (compound-style) to reduce chatter.

G76 Block 1 (cycle settings):

• P — three two-digit values concatenated: number of spring passes, thread runout angle (degrees × 10), thread profile angle (typically 60 for UN threads)
• Q — minimum depth of cut per pass (radius, no decimal, 0.0001 in. units)
• R — finish allowance (radius)

G76 Block 2 (thread geometry):

• X — minor diameter (root diameter for external thread)
• Z — Z end of thread
• I — taper offset; zero (I0.) for a straight thread
• K — thread height (radial depth from major to minor diameter)
• D — first-pass depth of cut (radius, no decimal)
• F — thread lead (= pitch for single-start threads), in inches per revolution
• A — thread profile angle (60 for UN/UNF)

Calculating K and minor diameter:

• For UN threads: K = 0.6495 × pitch (thread height, in inches)
• Minor diameter ≈ Major diameter − (2 × K)

Workflow: Writing the Complete Lathe Program

1. Face the part to Z0 datum.

2. Rough turn with G71; leave 0.010–0.020 in. (diameter) for finishing.

3. Finish turn with G70; use a finer feedrate (0.005–0.008 IPR is typical for a finish pass).

4. Groove with G75; index to the groove position, plunge to depth.

5. Thread with G76; calculate K, D (first-pass depth), and minor diameter before entering values.

Always simulate in CNCSimulator Pro before running on the machine. Verify the profile matches all drawing dimensions. Check that the threading cycle reaches the correct minor diameter and that the tool clears the groove on retract.