How to Code a CNC Machine

• 1
  Key takeaways
• 2
  What G-code actually is and how a control reads it
• 3
  Set work offsets and tool data before writing a single cut
• 4
  How to calculate feeds and speeds that survive real material
• 5
  When to hand-code and when to post from CAM
• 6
  Structure of a clean program, line by line
• 7
  Common coding mistakes and how to avoid them
• 8
  Step by step: how to code a CNC machine from drawing to first article
• 9
  Hand-coding vs CAM posting: which to use

A CNC program is a plain text file. Each line is called a block, and each block holds words made of a letter address plus a value: G for preparatory commands, M for machine functions, X, Y, Z for coordinates, F for feed rate, S for spindle speed, T for tool number. The control reads blocks in order, from top to bottom, and executes them as soon as they are buffered. There is no compiler and no error list at the end. A bad line just moves the machine to the wrong place.

Most mills run in G17 (XY plane) with G90 absolute positioning and G21 metric units. Those three codes appear near the top of nearly every program. G91 incremental mode moves by distance from the current point instead of to an absolute coordinate, and it is easy to mix the two by accident. If a tool suddenly plunges to the table, check for a missing G90 before you check anything else.

A typical block looks like N40 G01 X25.0 Y12.0 Z-3.0 F250. The N number is a sequence label, useful when the operator needs to restart mid-program. The F word is modal, meaning it stays active until another F appears. The same is true for G codes in the same group. This is why one forgotten F can make the next twenty blocks feed at the previous value.

• 1
  G00 rapidPositioning move at machine maximum, never for cutting.
• 2
  G01 linearStraight cut at the programmed feed rate.
• 3
  G02 / G03Clockwise and counter-clockwise arcs, need I, J or R.
• 4
  G43 tool lengthApplies the tool length offset with H.

Coordinates in the program are not machine coordinates. They are positions inside a work offset, usually G54 to G59. The operator touches the part with an edge finder or probe, stores the X, Y, and Z origin in the G54 page, and the program runs relative to that point. Decide the datum before coding. On a milled plate, a common choice is the finished top face for Z0 and one finished corner for X0 Y0. On a turned part, Z0 is normally the finished face and X0 is the spindle centerline.

Tool length offsets are the second half of setup. Each tool has a length stored in the offset table, and G43 H01 pulls that value into the active position. If the length is wrong by 0.5 mm, the tool cuts 0.5 mm too deep. Renishaw-style probes and tool setters remove most of this risk, but the programmer still has to call the right H number. A mismatch between T03 in the program and H03 in the table is one of the most common crash causes in a job shop.

Write the setup sheet as you code. List every tool, its diameter, its corner radius, the holder, the offset number, and the Z depth it reaches. The operator reads that sheet, not your program. If a Ø6 mm flat end mill is listed as Ø6 mm but the CAM library says 5.8 mm, the wall will be undersized and no one will know until inspection.

Start with surface speed, not with a number copied from a chart. For aluminum 6061, a carbide end mill runs well at 300 to 500 m/min surface speed. For 304 stainless, drop to 60 to 120 m/min. For Ti-6Al-4V, stay near 30 to 60 m/min and keep the tool moving. Spindle speed follows from surface speed and tool diameter: rpm = (surface speed × 1000) ÷ (π × diameter). A Ø10 mm carbide tool in aluminum at 400 m/min gives roughly 12,700 rpm, which is why small tools need a fast spindle.

Feed per tooth is where most beginners go wrong. The formula is feed rate = rpm × number of teeth × chip load. A Ø10 mm three-flute carbide end mill in 6061 takes a chip load around 0.05 to 0.10 mm per tooth for roughing. At 12,700 rpm and three teeth, that is 1,900 to 3,800 mm/min. Writing F250 for that cut leaves a lot of cycle time on the table and rubs the edge instead of cutting it.

Depth and width of cut matter as much as speed. For a full-width slot in aluminum, keep axial depth around 0.5 × diameter. For a trochoidal or high-efficiency path, you can go 1 × diameter deep with 10 to 15 percent radial engagement. In stainless and titanium, reduce radial engagement and keep the cutter in the cut rather than letting it dwell. Heat leaves with the chip, so a heavier chip is often safer than a light one.

• 1
  Aluminum 6061300–500 m/min, 3-flute carbide, chip load 0.05–0.10 mm/tooth.
• 2
  Stainless 30460–120 m/min, 4-flute, chip load 0.02–0.05 mm/tooth.
• 3
  Ti-6Al-4V30–60 m/min, 4-flute, chip load 0.02–0.04 mm/tooth.
• 4
  POM and ABS150–400 m/min, 2-flute, watch for chip welding.

Hand-coding wins on simple work. A plate with six holes, a face, and an outside profile is often faster to write than to model, set up toolpaths, and post. The program is short, easy to read at the machine, and easy to edit when the operator wants to change a depth. Shops that do a lot of fixture plates, brackets, and one-off repair parts keep a library of hand-written templates for exactly this reason.

CAM wins once the geometry stops being 2.5D. A pocket with a drafted wall, a fillet that blends into a curved floor, or any surface described by a solid model needs a posted toolpath. The same is true for 5-axis work, where the machine has to coordinate two rotary axes with the linear axes. Writing that by hand is possible in theory and a waste of time in practice. Post-processor output also carries the correct G68.2 or TCPC codes for the specific control.

A mixed workflow is normal. Use CAM for the surfacing pass, then hand-edit the posted file to add the facing operation, the deburr pass, and a safe retract. Just remember that every manual edit is a chance to break the modal state. If you delete a G43 line, the next tool change runs without a length offset. Keep an original copy of the posted file and note what you changed.

A safe program starts with a header. Cancel any active compensation with G40, cancel cutter comp and offsets, call G17 G21 G90, then call the work offset. Bring the spindle up to speed only after the tool is clear of the part. A typical opening is G40 G49 G80, then G17 G21 G90, then G54, then G43 H01 Z50.0. That Z move puts the tool 50 mm above the datum before anything else happens.

Body blocks follow the operation order: face, spot drill, drill, tap, rough pocket, finish profile. Each tool change should include a safe Z retract, an M09 to stop coolant, an M05 to stop the spindle, then T and M06. After the change, restart the spindle with the correct S and direction with M03, turn coolant back on with M08, and re-apply the length offset. Programs that skip the retract before a tool change are the ones that drag a tool across the fixture.

End the program with M09, M05, a retract to a safe Z, and M30. M30 resets the program and rewinds it. If the machine has a chip conveyor or a bar feeder, the M-code sequence for those devices has to be checked against the machine manual. Do not assume M30 means the same thing on a Fanuc lathe and a Heidenhain mill.

• 1
  HeaderSafety cancels, units, plane, work offset, first tool length.
• 2
  BodyOne operation per section, with a comment line above each.
• 3
  FooterCoolant off, spindle off, retract, M30.

The most expensive mistakes are quiet ones. A missing decimal point turns X25.0 into X250. A G91 left active from a previous section makes every following move incremental. A tool length offset applied twice doubles the depth. None of these throw an alarm before the cut. The control does exactly what the block says, which is why the dry run is not optional.

Cutter compensation is another frequent source of scrap. G41 and G42 offset the path to the left or right of the programmed line, and they must be cancelled with G40 before the next rapid. If the compensation is active while the tool moves to a clearance plane, the control may alarm or, worse, swing wide into the fixture. Lead-in moves should be at least the tool radius long so the compensation has room to engage.

Finally, keep the program readable. Comments cost nothing and save hours during setup. Group operations, label the sections, and use consistent formatting. An operator who can read the program can catch a problem before it becomes a crash, and a programmer who can read it six months later can revise it without starting over.