Manual CNC part programming: G and M codes

Why it matters

Even when CAM software writes most programs, the shop floor still runs on G and M codes. Operators edit them, setters prove them out, and anyone debugging a scrapped part reads them line by line. A wrong sign on an arc centre or a missing G90 can crash a machine, so knowing exactly what each word does is a basic skill for a production engineer.

Key ideas

Program structure. A part program is a sequence of blocks (lines). Each block is made of words: a letter address followed by a number.

• N — sequence number; G — preparatory function (type of motion or mode); X, Y, Z — coordinates; I, J, K — arc-centre offsets along X, Y, Z; F — feed; S — spindle speed; T — tool number; M — miscellaneous (machine) function; D/H — offset registers.
• Example: N40 G01 X60.0 Y10.0 F120 S1200 M03. The codes below follow the common ISO 6983 / Fanuc style; individual controllers differ, so always check the machine's programming manual.

Modal and non-modal codes. Most G codes are modal: they stay active until replaced by another code from the same group (G00/G01/G02/G03 are one group, G90/G91 another). Once G01 and F120 are given, the next block containing only coordinates still cuts at 120 mm/min. Codes such as G04 (dwell) act only in their own block.

Important G codes.

• G00 rapid positioning (no cutting; path may not be a straight line on some machines); G01 linear interpolation at feed F.
• G02 circular interpolation clockwise; G03 counter-clockwise — viewed from the positive end of the axis perpendicular to the plane (looking down −Z for the XY plane).
• G17/G18/G19 select the XY/ZX/YZ plane for arcs and compensation.
• G20/G21 inch/metric units.
• G90 absolute coordinates (from the work zero); G91 incremental (from the current point).
• G40/G41/G42 cancel cutter-radius compensation / compensate left / right of the path, looking along the direction of travel.
• G43 tool-length compensation; G54–G59 work-coordinate offsets; G28 return to reference point.
• G81 drilling cycle, G83 peck drilling, G80 cancel cycle (canned cycles compress a repeated drilling sequence into one block).
• Turning: G96 constant surface speed (S in m/min), G97 constant rev/min, G94/G95 feed per minute/per revolution (Fanuc lathes often use G98/G99 for the same pair).

Important M codes. M00 program stop; M01 optional stop; M02 program end; M03 spindle clockwise; M04 spindle counter-clockwise; M05 spindle stop; M06 tool change; M08 coolant on; M09 coolant off; M30 program end and rewind to the start.

Arc programming. With the I, J, K method, I and J are the distances from the arc start point to the arc centre along X and Y, and on most controls they are incremental even in G90. Alternatively R gives the radius (positive for arcs up to 180°). The end point must be at the same radius from the centre as the start point.

Work zero and offsets. Coordinates are written from a program zero chosen on the part (often a corner or the centre of a bore). The setter measures where that zero is on the machine and enters it in G54; tool lengths and radii go in the offset tables, so the same program works whatever tool is loaded.

Formulas

F = N · f

• F feed rate (mm/min); N spindle speed (rev/min); f feed per revolution (mm/rev). For milling F = N · f_z · z.

L = √(Δx² + Δy²)

• L length of a G01 move (mm).

L_arc = r · θ

• r arc radius (mm); θ swept angle (rad).

t = L / F

• t time for a feed move (min).

t = L_cut / (f · N)

• Turning-pass time (min) for a cut length L_cut (mm).

Worked examples

Example 1 (standard). A tool moves with G01 X100 Y100 F200 from (0, 0). How long does the move take? Then a lathe cut of 100 mm length runs at f = 0.2 mm/rev and N = 1000 rev/min; find its time.

1. L = √(Δx² + Δy²) = √(100² + 100²) = 141.42 mm.
2. t = L / F = 141.42 / 200 = 0.7071 min = 42.4 s.
3. Turning: F = 0.2 × 1000 = 200 mm/min; t = 100/200 = 0.5 min (30 s).

Example 2 (GATE level). The tool is at (10, 10) in the XY plane, in G90 and G17. Find the arc centre and the total cutting time of: N10 G01 X60 Y10 F120 N20 G03 X80 Y30 I0 J20 N30 G01 X80 Y70

1. N10: straight move from (10, 10) to (60, 10), L₁ = 50 mm.
2. N20: centre = start + (I, J) = (60 + 0, 10 + 20) = (60, 30). Start radius = |(60, 10) − (60, 30)| = 20 mm; end radius = |(80, 30) − (60, 30)| = 20 mm ✓. The start is below the centre and the end is to its right, so going counter-clockwise (G03) sweeps 90°. L₂ = 20 × π/2 = 31.42 mm.
3. N30: modal G01 and F120 still apply; (80, 30) → (80, 70), L₃ = 40 mm.
4. Total L = 50 + 31.42 + 40 = 121.42 mm; t = 121.42/120 = 1.012 min = 60.7 s.
5. The same path in G91: G91 G01 X50 Y0, G03 X20 Y20 I0 J20, G01 X0 Y40.

Common mistakes

• Reading I and J as absolute centre coordinates; on most controls they are measured from the arc start point.
• Deciding CW/CCW by looking from below or in the wrong plane.
• Forgetting that G01 and F are modal and accidentally cutting at a rapid-sized feed later, or forgetting to cancel G91 and drifting off the part.
• Confusing M02 and M30, or M03 and M04.
• Applying G41/G42 in the same block as an arc, or without a lead-in move long enough for the offset.
• Using the 3-D diagonal instead of the plane distance, or forgetting to convert minutes to seconds.

For GATE PI

Typical questions give a short program and ask for the final tool position, the arc centre or radius, the total path length or machining time, or the meaning of a code. Practise switching between G90 and G91, working out I and J, and reading CW/CCW correctly. Short MCQs test common G and M codes.

Quick check

1. Which code gives counter-clockwise circular interpolation?
2. What is the difference between M02 and M30?
3. In G91, the tool at (20, 30) executes G01 X15 Y−10. Where does it end?
4. A G02 semicircle of radius 25 mm is cut at 150 mm/min. How long does it take?
5. Which code cancels cutter-radius compensation?

Answers: 1. G03. 2. Both end the program; M30 also rewinds to the start. 3. (35, 20). 4. π × 25/150 = 0.524 min ≈ 31.4 s. 5. G40.