How to Write Programs for CNC Machine

• 1
  Key takeaways
• 2
  Read the drawing and the model before writing a line
• 3
  Hand-written G-code or CAM output
• 4
  Speeds, feeds, and depth of cut
• 5
  Program structure that survives a shift change
• 6
  Common mistakes and how to avoid them
• 7
  Step by step: writing the program
• 8
  Hand-code or CAM: which fits the job

Most programming errors start before the editor opens. Open the STEP or IGES file and the 2D drawing side by side. Confirm the revision letter matches on both. We have scrapped parts because the model was rev C and the drawing was rev B, and the programmer trusted the file name.

Mark every tolerance tighter than ±0.05 mm. Those are the features that decide your setup count, your tool list, and whether you need a fourth or fifth axis. A bore held at ±0.005 mm cannot share a roughing pass with a pocket held at ±0.2 mm.

Look for features you cannot reach. A 4 mm deep slot with a 3 mm corner radius needs a 6 mm end mill, and the tool holder may hit the wall before the cutter does. Check the holder body diameter against the wall height before you commit to a tool.

Decide the datum now. Pick a face and two edges, or a bore and a face, and write them on the setup sheet. Every operation after that references the same zeros. Changing datums mid-program is the fastest way to lose 0.1 mm between operations.

• 1
  Revision checkModel and drawing must carry the same rev letter before programming starts.
• 2
  Tight tolerance listAnything under ±0.05 mm gets its own operation and its own tool.
• 3
  Holder clearanceHolder body diameter plus 1 mm must clear the wall before the cutter reaches depth.

Hand-written G-code works for simple work: face and turn a shaft, drill a bolt circle, cut a rectangular pocket. You can write it at the machine, prove it in a few minutes, and change one number when the operator calls. The whole program might be 40 lines and you can read it in one pass.

CAM output wins as soon as the geometry stops being planar. A curved surface with variable depth, a 5-axis swarf cut, or a part with 60 pockets will take days by hand and still be wrong. CAM software also gives you rest material tracking, so you know the tool is not cutting air for 20 minutes.

The practical rule on our floor: if the part needs more than three tools or has any non-planar surface, it goes to CAM. If it is a turned part with a couple of grooves and a thread, hand-code it. Mixing the two is normal, and a good programmer will hand-edit the CAM output for the first approach move.

Whichever path you take, the output is the same format: a text file of G and M codes with feed, speed, and tool call blocks. The machine does not care who wrote it. It cares that the numbers are consistent and the rapid moves clear the fixture.

Start from surface speed, not spindle rpm. For 6061 aluminium with a carbide end mill, we run 300–500 m/min surface speed. That puts a 10 mm cutter near 9,500–16,000 rpm, which most of our spindles reach. For 304 stainless, drop to 100–150 m/min, because the material work-hardens if you rub it instead of cutting it.

Feed per tooth is the number that breaks tools. In aluminium, 0.05–0.15 mm per tooth is normal for a 10 mm three-flute cutter. In stainless, use 0.03–0.08 mm per tooth and keep the chip load steady. If the chip looks like dust, you are rubbing. If it looks like a comma and comes off blue, you are close.

Depth of cut depends on radial engagement. Full-width slotting in aluminium is limited to about 0.5 × tool diameter axial depth. If you step over at 30% of the diameter, you can push axial depth to 1.5 × diameter or more. That is where high-efficiency milling comes from, and it is also why the same tool can run at two very different feed rates in one program.

Always check the machine limit before you post. A 16,000 rpm command on a spindle rated to 12,000 rpm will either alarm out or run at the wrong speed and burn the tool. Our 4,000 × 400 × 150 mm travel machines and our 500 × 500 × 450 mm compact machines have different spindle ranges, so the same program does not always transfer.

• 1
  Aluminium 6061300–500 m/min, 0.05–0.15 mm per tooth, full-width axial depth 0.5 × D.
• 2
  Stainless 304100–150 m/min, 0.03–0.08 mm per tooth, never dwell in the cut.
• 3
  Titanium Ti-6Al-4V40–60 m/min, 0.03–0.06 mm per tooth, flood coolant always on.

Put the setup sheet inside the program as comments. Tool list, work offset, stock size, and the datum face go at the top. The operator running the second shift has never seen your setup notes on paper, but they will read the first 20 lines of the program.

Use one work offset per setup. G54 for op 1, G55 for op 2, and so on. Do not shift the same offset mid-program unless you also comment why. When the part comes back for op 2, the operator can verify G55 against the setup sheet without guessing.

Call the tool, start the spindle, and move to the first position in separate blocks. It costs three lines and saves a crash. The pattern is: T5 M06, then S9500 M03, then G00 Z50, then G00 X Y. If the tool length is wrong, the machine alarms before it moves in X or Y.

Cancel cutter compensation and coolant at the end of every tool. G40, M09, then G00 Z50. A program that leaves G41 active and hands off to the next tool will cut a taper on the first pass, and the operator may not catch it until the part is out of tolerance.

The most expensive mistake is a wrong work offset. The program is perfect, the tool is perfect, and the machine cuts 50 mm into the fixture because G55 was set on the wrong corner. Always verify the offset with a dial indicator or a probe before the first cut.

The second is a missing G40 or a leftover G41. If cutter compensation stays active, the next tool cuts a part that is offset by the compensation value. On a 10 mm cutter with a 5 mm offset, that is a 5 mm error on every profile. Cancel compensation at the end of every operation.

The third is a feed rate that is too high for the radial engagement. A program that runs well at 30% stepover will break the tool at 100% stepover with the same feed per tooth. Recalculate the feed when you change the stepover, not just the spindle speed.

The fourth is forgetting to check the tool length after a change. A 0.2 mm difference in tool length shows up as a 0.2 mm step on the floor of a pocket. Measure every tool on the presetter or with a touch-off gauge, and update the offset before the program runs.

• 1
  Verify the offsetProbe or indicate the work offset before the first cut. Never trust the number from the last job.
• 2
  Cancel compensationG40 at the end of every operation, before the next tool call.
• 3
  Recheck feed after stepover changeFeed per tooth is not constant when radial engagement changes.