Milling Programming

CNC milling programming drives a 3-axis (or more) machine where the spindle holds the tool and the table holds the work. You move the tool through a sequence of straight lines, arcs and pre-built cycles to remove material.

This guide uses Fanuc-style syntax (Haas, Mazak Mill, and most controls share 95% of these codes).

1. The Milling Coordinate System

A vertical milling machine uses three linear axes — X (table left/right), Y (table in/out), Z (spindle up/down).

Right-Hand Rule

Point your right hand so the thumb = +X, index = +Y, middle = +Z. That's the machine convention everywhere on the planet.

2. Anatomy of a Milling Block

N40 G01 X25.0 Y10.0 Z-2.0 F250 ;
│   │   │     │     │     │
│   │   │     │     │     └── feed (mm/min with G94)
│   │   │     │     └── target Z (cutting depth)
│   │   │     └── target Y
│   │   └── target X
│   └── motion mode (linear feed)
└── line number

Key letter addresses for milling:

3. The Essential G-Code Reference (Milling)

Motion (Group 01)

Plane selection (Group 02)

Plane matters for arcs and cutter compensation — choose G17 for normal flat-table work.

Coordinate / unit modes

Tool compensation

Drilling / hole-making canned cycles

Return mode for cycles

M-codes you must know

4. Work Coordinate Systems (G54–G59)

The machine has two coordinate systems: machine zero (set at machine home) and work zero (set on each part by you). G54..G59 are six work-offset registers.

G54 G90 G17 G21    ; "Use work offset 1, absolute, XY plane, metric"
G00 X0 Y0          ; Goes to the X0 Y0 of work-offset 1 (i.e. part zero)

The operator sets G54 by jogging to the corner of the part and pressing "Set Work Offset" — then your program is portable: same G-code, different fixture position.

5. Tool Length & Cutter Radius Compensation

Length compensation (G43 H_)

Each tool has a different length. Instead of recomputing Z for every tool, the operator measures each tool and stores its length in an H-register (H01 for tool 1, H02 for tool 2…). Your program just calls:

T01 M06            ; load tool 1
G43 H01 Z25.0      ; "apply tool 1 length, go to Z25"

Radius compensation (G41/G42 D_)

Same idea for cutter diameter. You program the finished part edge; the control offsets the toolpath by D (radius register).

G01 G41 D01 X10.0 Y0.0 F300   ; comp LEFT (climb), use D01
    Y50.0
    X40.0
    Y0.0
    X-2.0
G40                            ; cancel comp before retract

Climb vs conventional:

CNC mills almost always climb (G41 around an outside contour going counter-clockwise; G42 going clockwise).

6. Drilling Cycles — In Depth

The format for every drilling cycle is the same:

G## X_ Y_ Z_ R_ Q_ P_ F_ ;
;   │  │  │  │  │  │  └── feed (mm/min)
;   │  │  │  │  │  └── dwell time (ms, for G82/G89)
;   │  │  │  │  └── peck depth (G83/G73 only)
;   │  │  │  └── R-plane = where rapid switches to feed
;   │  │  └── final hole bottom Z (in absolute or incremental)
;   │  └── Y of hole
;   └── X of hole

After the first call, every subsequent block of just X Y triggers another hole at the same depth — modal drilling.

G81 — Plain Drill

G90 G54 G00 X10.0 Y10.0      ; first hole position
G43 H03 Z25.0                ; tool length offset
M03 S1500
G99 G81 R2.0 Z-15.0 F180     ; drill: rapid to R, feed to Z, rapid out
    X30.0                    ; second hole — same depth
    X50.0
    X70.0 Y30.0
G80                          ; cancel cycle
G00 Z50.0

G83 — Peck Drill (deep holes, full retract)

For holes deeper than ~3 × diameter, peck to clear chips:

G99 G83 R2.0 Z-40.0 Q5.0 F120
;       │     │      │
;       │     │      └── peck depth = 5 mm each step
;       │     └── final depth -40 mm
;       └── R-plane (start of feed)

The tool feeds 5 mm, rapids back to R, rapids back to the previous peck depth, feeds another 5 mm, repeats until Z-40.

G73 is the same idea but with a small retract (typically 1 mm) — much faster, used when chip clearance is less critical (aluminium).

G84 — Tapping

G95                       ; feed/rev
G99 G84 R5.0 Z-15.0 F1.5  ; for M8 × 1.25 thread, F = pitch = 1.25
G94                       ; back to feed/min

The control synchronises spindle and Z so the tap doesn't tear the thread. Modern machines use rigid tapping — no floating tap holder needed.

7. Arc Programming (G02 / G03)

Two ways to define an arc — R (radius) or I/J (centre offsets):

; Arc from (10, 0) to (10, 20), centre at (10, 10), CCW, radius 10:
G01 X10.0 Y0.0 F250
G03 X10.0 Y20.0 R10.0          ; R-style
; OR
G03 X10.0 Y20.0 I0 J10.0       ; centre offset: 0 in X, +10 in Y from start

Use I/J for full circles — R can't define a 360° arc (ambiguous).

8. Subprograms (M98 / M99)

Repeated patterns belong in subprograms. Main program calls with M98:

; --- main ---
G54 G90 G00 X0 Y0 Z25.0
M98 P1000 L4              ; call O1000 four times
M30

; --- subprogram O1000 ---
O1000
G91                       ; relative
G81 X20.0 R2.0 Z-15.0 F180
G80
M99                       ; return

L (or K on some controls) sets repeat count. The subprogram drills four holes 20 mm apart along X — a hole pattern, defined once.

9. Two Complete Worked Programs

Program 1: 4-hole bolt pattern + counterbore

A 50 × 50 mm plate, four Ø6 mm bolt holes on a 30 × 30 mm pattern, each counterbored Ø10 × 5 mm deep:

%
O1001 (BOLT PATTERN)

(--- Tool 1: Ø6 drill, H01 ---)
T01 M06
G54 G90 G17 G21 G94
G43 H01 Z25.0 M03 S2200
M08

G99 G81 X10.0 Y10.0 R2.0 Z-22.0 F220
        X40.0 Y10.0
        X40.0 Y40.0
        X10.0 Y40.0
G80
G00 Z50.0 M09
M05

(--- Tool 2: Ø10 endmill for counterbore, H02 ---)
T02 M06
G43 H02 Z25.0 M03 S1800
M08

G99 G82 X10.0 Y10.0 R2.0 Z-5.0 P200 F300   ; G82 spot/c-bore with dwell
        X40.0 Y10.0
        X40.0 Y40.0
        X10.0 Y40.0
G80
G00 Z50.0 M09
M05

M30
%

Program 2: Profile a 60 × 40 mm pocket-edge with cutter comp

Mill the OUTSIDE profile of a 60 × 40 mm rectangle (fillets R5) with a Ø10 mm endmill, climb cutting:

%
O1002 (CONTOUR MILL — RECTANGLE 60x40 R5)

T05 M06                     ; Ø10 endmill, D05 = 5.0 mm
G54 G90 G17 G21 G94
G43 H05 Z25.0 M03 S2400
M08
G00 X-15.0 Y-10.0           ; start outside the part
Z2.0
G01 Z-5.0 F250              ; plunge to depth

G41 D05 X0.0 Y0.0 F600      ; engage comp going to corner (0, 0)
    X55.0                   ; bottom edge → corner before fillet
    G02 X60.0 Y5.0 R5.0     ; bottom-right fillet
    G01 Y35.0
    G02 X55.0 Y40.0 R5.0    ; top-right fillet
    G01 X5.0
    G02 X0.0 Y35.0 R5.0     ; top-left fillet
    G01 Y5.0
    G02 X5.0 Y0.0 R5.0      ; bottom-left fillet
    G01 X-15.0              ; lead-out clear of part
G40                         ; cancel comp
G00 Z25.0 M09
M05
M30
%

Two things to notice:

• The lead-in (G01 X0 Y0) is straight — required for G41/G42 to engage cleanly.
• All four corner arcs use G02 because we're going clockwise (so the comp side G41 keeps the cutter on the outside of the part).

10. Quick Cheat Notes

• Right-hand rule — thumb X, index Y, middle Z. Z is ALWAYS up.
• Set G54 first — every modern part program starts on a work offset.
• Always issue G43 H_ after a tool change before plunging in Z.
• G41 = climb (left of path), G42 = conventional (right of path).
• G80 cancels canned cycles — forget it and your next G00 will drill a hole.
• For arcs > 180° or full circles use I/J, not R.
• G99 stays at R-plane between cycle holes (fast); G98 returns to initial plane (clears clamps).
• M98 P_ L_ = call subprogram L times — the cleanest way to handle repeating patterns.
• Tap feed rate (with G94) = pitch × RPM. With G95, just F = pitch.
• Test with single-block + 25% rapid override the first run.