Basics of G Code for CNC: What New Machinists Need to Know

Every line in a CNC program is called a block. A block is a set of words, and each word is a letter plus a number. The letter tells the control what kind of information follows: G for a preparatory function, M for a machine function, X Y Z for linear position, F for feed rate, S for spindle speed, T for tool number. The control reads the block left to right and executes it as one instruction.

A typical block looks like N40 G01 X25.4 Y12.7 Z-3.0 F250. The N number is a sequence number, useful when you need to search or restart mid-program. G01 means linear interpolation at the programmed feed rate. The X, Y and Z words give the end point of the move. F250 sets the feed at 250 mm per minute. Change the F word and the same geometry cuts at a different speed.

Order inside the block matters less than people think, but consistency does. Most shops write the modal G code first, then coordinates, then feed. Modal means the code stays active until another code in the same group replaces it. G01 stays active for every block after it, which is why you rarely see it repeated on every single line.

A single wrong decimal is not a cosmetic problem. On a titanium part held to ±0.005 mm, an X word of 25.4 instead of 2.54 sends the tool 22.86 mm past where you intended. That is the difference between a finished part and scrap. Read the coordinate words before you press cycle start.

• 1
  NSequence number. Helps you find and restart a block.
• 2
  GPreparatory function: motion mode, units, offsets, canned cycles.
• 3
  MMachine function: spindle, coolant, tool change, program stop.
• 4
  XYZ / ABCAxis end points. A, B and C are rotary axes.

You do not need to memorize the full code list. A working set of about twenty codes covers most milling and turning work. G00 is rapid positioning, used to move the tool between cuts with no material contact. G01 is linear feed, G02 and G03 are clockwise and counterclockwise arcs. G17, G18 and G19 select the plane for arc interpolation, so an arc written in the XY plane behaves differently from the same words in the XZ plane.

On the setup side, G54 through G59 are work coordinate systems. They tell the control where the part origin sits relative to machine home. G43 applies tool length compensation from the offset table, and G41 or G42 apply cutter radius compensation left or right of the programmed path. If your part is consistently off by the radius of the cutter, you are probably missing G41 or G42.

M codes handle the machine itself. M03 starts the spindle clockwise, M05 stops it, M06 changes the tool, M08 turns coolant on, M09 turns it off. M30 ends the program and rewinds. M00 is a program stop that waits for the operator, which is how many shops insert an inspection pause before a finishing pass on a tight-tolerance feature.

Controllers are not identical. Fanuc, Haas, Siemens and Mitsubishi all use the same core words, but canned cycles, macro syntax and some M codes differ. A program posted for one control may run on another after edits, and it may also alarm. Always check the machine manual before you transfer a program between two brands.

• 1
  G00 / G01Rapid move and linear feed move.
• 2
  G02 / G03Arc interpolation, clockwise and counterclockwise.
• 3
  G54–G59Work coordinate systems, where the part origin sits.
• 4
  M03 / M05 / M08Spindle on, spindle off, coolant on.

G20 selects inch mode and G21 selects metric. This is the first thing to check when a program comes from an outside source. A part programmed in millimeters and run in inch mode will try to move 25.4 times further than intended, and most machines will hit a travel limit before the tool reaches the material. That is a lucky outcome. On a short move inside the envelope, the tool simply cuts in the wrong place.

Work offsets and tool offsets are separate systems, and both have to be right. G54 stores the part origin for the current setup. The tool offset table stores the length and radius of each tool. If you touch off a tool and load the wrong offset number, every Z move in the program is wrong by the difference. This is why shops verify the first article on a scrap block before running a production part.

Feed and speed words are where the program meets the material. F is feed in units per minute for milling, or feed per revolution for turning when G99 is active. S is spindle speed in revolutions per minute. Neither word knows what material you loaded. A feed and speed pair that works in aluminium 6061 will burn a 4 mm end mill in 316 stainless. The program is only as good as the cutting data behind it.

At GreatLight we run 127 high-precision CNC machines across three wholly-owned plants, and every program is proven on the setup before the run starts. Parts are held to ±0.005 mm and inspected 100% before shipment, with reports on request. A clean program is the first step in that chain, not the last one.

A 3-axis program moves the tool in X, Y and Z. The part stays still. That covers a large share of prismatic work: plates, brackets, housings with features on one or two faces. If the geometry can be reached from a single setup direction, 3-axis milling is usually the faster and cheaper route.

A 5-axis program adds two rotary axes, usually A and B or B and C, depending on the machine. The control coordinates linear and rotary motion in the same block. That lets the tool reach undercuts, blend fillets across a curved surface, and drill holes at compound angles without a second setup. On an impeller or a heat exchanger core, the alternative is several fixtures and several re-zeroing steps, each one adding error.

The programming changes more than the code list. Tool axis vectors, post-processor output, and collision checking all become part of the job. A 5-axis program also needs a machine simulation before it runs, because a rotary move that looks short on screen can swing the tool holder into the table. Our 16 simultaneous 5-axis machining centers, including DMG Mori mills, handle rotary work on a Ø400 mm table and travel up to 4,000 × 400 × 150 mm on the large machines.

Where a 5-axis program pays off: complex contours that need one continuous pass, deep pockets with drafted walls, and parts where tolerance stacks from multiple setups would eat the budget. Where it does not: simple plates, flat covers, and any part a 3-axis machine can finish in one setup. Match the program to the geometry, not to the machine's spec sheet.

When you open a posted program, read the header first. The tool list, the stock size, the work offset and the units mode are usually at the top in comment lines. If the header names a tool that is not in the machine, stop there. A missing T word in the tool change line is a common posting error and a fast way to break a cutter.

Next, scan the approach and retract moves. G00 blocks that pass close to the fixture are worth checking by hand. Most crashes happen in rapid moves, not in cutting moves, because the operator watches the cut and trusts the rapid. Set a safe Z height in the program and verify it against the tallest point of the part and the clamps.

Finally, look at the feed rates against the tool diameters. A 3 mm cutter running at a feed meant for a 12 mm cutter will snap. A 12 mm cutter running at a feed meant for a 3 mm cutter will rub, work-harden the surface, and wear out fast. The numbers in the program are a plan, and the machine does exactly what the plan says.

• 1
  Header commentsTool list, stock size, work offset, units mode.
• 2
  Rapid movesCheck clearance to clamps and fixture before cycle start.
• 3
  Feed vs tool sizeFeed written for one diameter is wrong for another.