What Program Do CNC Machines Use?

• 1
  What a CNC program actually contains
• 2
  How a CAD model becomes a CNC program
• 3
  Why the same part needs a different program per machine
• 4
  When g-code is the wrong tool
• 5
  What this means for a shop's programming chain
• 6
  Which programming route fits which job

A CNC program is a text file. Each line is one block, and each block holds a letter address: G for preparatory commands, M for machine functions, X Y Z for linear moves, I J K for arc centers, F for feed, S for spindle speed, T for tool number. The controller reads the file top to bottom, one block at a time, and executes it. There is no compiler and no runtime library. The file is the program.

Almost every line you see is a motion command. G00 moves at rapid traverse to a position without cutting. G01 cuts in a straight line at the programmed feed. G02 and G03 cut arcs clockwise and counterclockwise. G81 through G89 cover drilling, boring, and tapping cycles. Everything else supports those moves: tool changes, coolant on and off, spindle start, program stop.

The M-codes are the machine-side switches. M03 starts the spindle forward, M05 stops it, M08 floods coolant, M09 kills it, M06 changes the tool. M30 ends the program and rewinds. A block like G01 X50.0 Y20.0 F250 is one straight cut at 250 mm/min. That is the whole idea.

File size surprises people. A roughing and finishing cycle on a 300 mm aluminum bracket might run 3,000 to 15,000 blocks. A five-axis impeller with a dense finishing pass can pass 400,000 blocks. Controllers stream these from memory or drip-feed them over a serial link, which is why block processing speed matters on old machines.

Nobody types that many lines by hand. The path is CAD to CAM to post-processor to controller. The engineer models the part in CAD, then imports a STEP or IGES file into CAM software. In CAM, they choose stock size, set the work origin, pick tools from a library, and define roughing and finishing strategies. The CAM kernel computes the toolpath and writes a cutter location file.

The cutter location file is machine-neutral. It knows the tool tip position in part coordinates, but it does not know that this particular machine has a rotary table on the right side, or that its controller wants a decimal point in every coordinate. That translation is the post-processor's job.

This is where a lot of quoting errors come from. A shop can own good CAM seats and still produce scrapped parts if the post-processor was never validated for that machine. When we onboard a new five-axis center, we cut a test artifact and check the rotary offsets, tool length compensation, and retract moves before the machine touches a customer part. Without that step, the first article becomes the test.

For simple turned parts, the chain shortens. Many lathes are programmed at the control with a few dozen blocks of G71 roughing and G70 finishing cycles. A shaft with two diameters and a thread does not need a CAM seat.

G-code is standardized on paper by ISO 6983, but no two controllers implement it identically. Fanuc, Siemens, Heidenhain, Mitsubishi, and Haas each have their own extensions and quirks. Some want G43 H01 for tool length offset and some accept G43 without the H word. Some use G54 through G59 work offsets, some allow G54.1 P1 for extended offsets on pallet systems.

Arc formatting differs too. Fanuc accepts I J K center offsets; Heidenhain conversational format wants radius and direction. A program written for a Haas mill will usually need edits before a Siemens 840D runs it cleanly. This is why shops keep a post-processor per machine family, not one universal post.

Rigid tapping is a good test case. On Fanuc, G84 with an M29 spindle-orientation command works. On other controllers, the same hole needs G84.2 or a floating tap holder instead. If the post is wrong, the tap breaks and the part may be scrapped.

The practical consequence for buyers: if you move a part between two shops, do not assume the program transfers. Send the 3D model and the drawing, not the g-code. From the model, each shop regenerates toolpaths that match its own machines and fixtures.

G-code is a low-level language. It describes motion, not intent. That is a strength for deterministic cutting and a weakness for anything that needs decisions during the cycle. If you want the machine to measure a feature and adjust the next pass by the result, plain g-code will not do it alone.

That job goes to macro programming, usually Fanuc Macro B, or to a probing cycle from the machine builder. A macro can read a probe result into a variable and shift a work offset. This is common on high-mix work where casting dimensions vary from lot to lot. It adds complexity and needs careful testing, so it is worth it only when the tolerance or the scrap cost justifies it.

Parametric CAD and CAM cover a different gap. If a family of brackets differs only in hole spacing, model it parametrically and let CAM regenerate. Hand-editing a g-code file per variant is how mistakes get made.

What g-code does not cover at all: closed-loop decisions based on real-time sensor data, in-process metrology with automatic re-cutting, and adaptive feed control beyond what the controller offers natively. Those are controller features or separate systems bolted onto the machine, not program features.

At GreatLight we run 127 high-precision CNC machines across three plants, including 16 simultaneous 5-axis machining centers, 12 four-axis mills, and 16 mill-turn centers. Each machine family carries a validated post-processor. That is the part of the chain that customers never see, and it is the part that decides whether a first article lands inside ±0.005 mm.

Programming feeds into the same inspection loop as the machines. Every part is checked 100% before shipment, with raw material checks, in-process monitoring, and final inspection. When a dimension drifts, the fix may be a tool offset in the controller, a change in the CAM stepover, or a new post for a different machine. Knowing which one to change is the difference between a two-hour fix and a two-day investigation.

Materials change the program as much as geometry does. Aluminum 6061 at 6,000 rpm and 2,000 mm/min behaves nothing like Inconel at 40 m/min surface speed. Feeds and speeds live in the CAM tool library and are rechecked at the machine. PEEK and carbon fibre bring their own rules on heat and dust extraction.

We hold ISO 9001:2015, IATF 16949:2016, ISO 13485:2016, and ISO 27001:2022. Those certificates shape how programs are version-controlled, approved, and stored, especially for medical and automotive work where a program change is a documented event.