How to Write a Program for the CNC Milling Machine

• 1
  Key takeaways
• 2
  Read the drawing like a machinist
• 3
  Choose the right programming environment
• 4
  Set the work coordinate system and tool offsets
• 5
  Pick tools and cutting parameters
• 6
  Simulate, dry run and tune the first part
• 7
  Step-by-step programming sequence
• 8
  Programming choices by part type

The programming work starts on paper, not in CAM. Open the drawing and mark the functional surfaces: the faces that mate with other parts, the bores that carry bearings, the threads that take fasteners. Those are the features that set the tolerance stack. Everything else can float within general tolerances.

Next, list the datums. A bore that positions to a face can only be inspected if that face is machined first. If the drawing calls out a datum that cannot be touched in the first setup, you have to plan two operations and accept the re-fixturing error. Experienced programmers spot this before quoting. Fixing it after the program is written means rewriting the whole sequence.

Check for tool reach. A deep pocket with a corner radius of 3 mm needs a cutter small enough to fit, and a holder slim enough to clear the walls. If the wall is 60 mm tall and the pocket is 12 mm wide, a standard ER holder will rub. That is a 5-axis or long-reach toolpath, and it changes the program structure.

Finally, confirm the stock. For aluminium plate, 2 mm of allowance per side is normal. For a casting that already has bosses and cores, the programme cuts air in some areas and heavy stock in others. Write down the actual stock condition, because that number drives the first roughing pass.

• 1
  Mark functional facesThese carry the fit, so they set the tolerance stack.
• 2
  List datums in machining orderA datum that cannot be cut first forces a second setup.
• 3
  Check tool reachCompare pocket depth against holder diameter before you choose a cutter.
• 4
  Measure the real stockCastings and weldments are not uniform; the program must cover the worst case.

Manual G-code is still the fastest route for simple parts: a plate with a few holes, a face mill pass, a chamfer. On a 3-axis machine, a hand-written program of 40 lines is easier to verify than a CAM file with 4,000 moves. If the part is rectangular, has no complex curves and needs two or three tools, write it by hand.

CAM software takes over when the geometry gets curved. A sculpted rib on a robot joint, a tapered pocket, a 3D surface, a 5-axis toolpath, all need a CAM system. The software also handles stock awareness, rest machining and collision checks. That saves hours compared with writing point-to-point moves.

Whichever route you choose, the post-processor matters more than the software brand. A post that outputs the wrong G-code for your control will send the machine to the wrong place. We run 127 high-precision CNC machines, 16 of which are simultaneous 5-axis centres, and each machine family has its own post. Test the post on a scrap block before you trust it with production.

Keep a checklist of the control-specific quirks: how the machine handles G28, whether the tool change uses a safe Z, whether the spindle needs an M19 orientation before a probe. These details belong in the post, not in the operator's head.

• 1
  Manual G-codeBest for 2.5D plates, drilled holes and simple pockets.
• 2
  CAM softwareRequired for curved surfaces and 4-axis or 5-axis work.
• 3
  Post-processorOne per machine family. Test it on scrap before production.

The work coordinate system tells the machine where the part sits. Pick the corner or centre that the operator can touch with an edge finder or probe. On a vise, the fixed jaw and the top face are the usual choice. On a fixture plate, use a dowel pin hole. The rule is simple: the WCS must be reachable with the tools the operator actually has.

Use G54 for op 1 and G55 for op 2. Do not reuse G54 on a second vise unless the vises are dialled in together. If you have three parts on the table, give each one its own offset. This avoids the classic mistake of running a program on the wrong position and cutting into the fixture.

Tool offsets are separate from work offsets. Each tool needs its length measured and stored in the tool offset register. Radius compensation, when used, must match the cutter diameter in the program. If you program to the centreline, you do not need cutter comp, but you must adjust the toolpath when the cutter wears. For a ±0.005 mm bore, use cutter comp and adjust the offset after the first article.

Record the Z zero on the top of the stock or on a gauge block. Never leave the operator guessing which surface was used. Write the Z reference on the setup sheet, and note the tool number used to touch it off.

• 1
  G54 = op 1G55 = op 2. One offset per setup, not per program.
• 2
  Touch-off surfaceUse a face the operator can reach with a probe or edge finder.
• 3
  Cutter compUse it when the feature tolerance is tighter than the cutter wear band.
• 4
  Write it downPut the Z reference and tool number on the setup sheet.

Start with the smallest radius in the part. If the drawing shows a 4 mm inside corner, the largest cutter that can clean it is 8 mm, and you need a 4 mm or smaller tool for the corner itself. Choose the largest tool that fits the feature, because a bigger cutter is stiffer and removes metal faster.

For aluminium, a 3-flute carbide end mill at 12 mm diameter runs well at 8,000–12,000 rpm with a feed of 0.08–0.12 mm per tooth. That gives a chipload the cutter can survive and a surface finish near Ra 0.8–1.6 μm. For stainless 304, drop the surface speed to 80–120 m/min and keep the chipload above 0.03 mm per tooth. Too light a chip work-hardens the material.

Titanium and Inconel need more care. Ti-6Al-4V cuts at 40–60 m/min with high-pressure coolant and a chipload around 0.05 mm per tooth. Inconel is slower still, 20–30 m/min, and the tool must never rub. If the chips come off as dust, you are rubbing, not cutting. Increase the feed or reduce the speed.

Depth of cut matters as much as speed. For roughing aluminium, axial depth of 1 × D and radial width of 0.4 × D is a common starting point with a 3-flute cutter. For stainless, reduce axial depth to 0.5 × D. For finishing, take 0.2–0.5 mm radial and full axial depth to avoid witness marks.

• 1
  Largest tool that fitsStiffer cutter, fewer passes, better finish.
• 2
  Aluminium 60613-flute, 0.08–0.12 mm/tooth, 8,000–12,000 rpm at Ø12 mm.
• 3
  Stainless 30480–120 m/min, keep chipload above 0.03 mm/tooth.
• 4
  Titanium and Inconel40–60 m/min and 20–30 m/min. Never let the tool rub.

Simulation catches collisions, not bad cutting data. Run the CAM simulation with the actual holder and fixture models. Check that the tool does not hit the vise, the clamps or the table. If the simulation shows a rapid move through the part, fix the clearance plane before you post.

The dry run is the real test. Raise Z by 50 mm and run the program with the spindle off, feed override at 50%. Watch the tool path, the tool changes and the coolant. If the machine has a graphics mode, use it first, then do the dry run. A crash at this stage costs nothing but time.

For the first article, cut the part and measure every dimension on the drawing. Check the critical bores with a bore gauge, the flatness with a surface plate, and the surface finish against the Ra callout. If a bore is 0.02 mm undersize, adjust the cutter comp and run the finish pass again. Do not adjust the program geometry unless the error is consistent across the whole batch.

Once the first article passes, lock the program. Save it with the offset values, tool list and inspection report. The next run should not need a programmer. That is the difference between a one-off and a repeatable process.

• 1
  Simulate with fixturesHolder and clamp models catch the collisions CAM misses.
• 2
  Dry run at +50 mmSpindle off, 50% feed override, watch every tool change.
• 3
  Measure the first articleBore gauge, surface plate and Ra check against the drawing.
• 4
  Lock and archiveOffsets, tool list and inspection notes go with the program.