CNC machining tutorial: 7 steps from CAD file to finished part

• 1
  What matters most
• 2
  What a CNC machining tutorial can and cannot fix
• 3
  DFM review: read the model like a machinist
• 4
  Stock, material, and the numbers behind them
• 5
  Workholding: the step that decides accuracy
• 6
  Toolpath, feeds, and surface finish
• 7
  Step by step: from CAD file to shipped part
• 8
  Which setup fits which part

A CNC machining tutorial is mostly about order of operations. The machine removes metal accurately; the drawing decides whether the part can be made at all. If a slot is 2 mm wide and 40 mm deep, no amount of spindle speed saves it. The tool has to reach the floor, and a Ø2 mm end mill at that depth will deflect long before it cuts cleanly.

Reader, this is for you if you design parts, review quotes, or approve first articles. By the end you should be able to look at a model and say which features need 5-axis, which need a second setup, and which should be redesigned. That judgment is what separates a smooth build from three rounds of rework.

Keep one rule in mind. Machining time scales with the number of setups, not with the number of holes. Ten holes on one face are cheap. Two holes on opposite faces can double the cost, because the part has to be flipped, re-datumed, and indicated in again.

The steps below are the sequence we run at GreatLight: DFM review, stock and material, workholding, toolpath, first article, inspection, finishing. Each step has a failure mode. Most failed parts die at step 3 or step 5, not at the spindle.

• 1
  Watch tool reachDepth-to-diameter above 4:1 needs a necked or reduced-shank cutter.
• 2
  Count setupsEach additional setup adds re-datum risk and labor.
• 3
  Separate critical from generalToleranced features get their own inspection line on the drawing.

Before quoting, we open the STEP file and look for three things: internal corners, thin walls, and features that sit on a non-orthogonal face. An internal corner drawn at R0.5 mm forces a Ø1 mm cutter. If the pocket is 30 mm deep, that cutter is unusable and the corner must open to R2 mm or larger.

Wall thickness matters more in plastics than in aluminum. A 0.8 mm wall in POM or PEEK will chatter and bow; 1.5 mm is safer. In 6061-T6, a 0.8 mm wall is workable if the height stays under about 10 mm and the toolpath uses light radial engagement.

Note the datum scheme on the drawing. If the datum is a curved surface or a cast boss, we cannot indicate it reliably. Move the datum to a flat machined face or a bored hole, and the whole inspection chain becomes repeatable.

DFM output should be concrete. We send a marked-up model or a short list: corner radii to open, walls to thicken, threads to move to a machinable face. Quotation and free DFM analysis land within 12 hours, so this review happens before any tooling decision is locked.

One more check: thread depth. A M3 thread needs roughly 2× diameter of engagement in aluminum, about 6 mm, and a pilot hole that can actually be drilled at that depth. Threads drawn to the bottom of a blind pocket usually get shortened.

• 1
  Corner radiusKeep internal radii at 1/3 of pocket depth or larger where possible.
• 2
  ThreadsAllow 2× diameter engagement and a relief at the bottom.
• 3
  DatumsUse flat faces or bored holes, not cast or curved surfaces.

Material choice drives feeds, speeds, and the finishing plan. Aluminum 6061-T6 machines fast and holds tolerance well. 7075 gives higher strength but is less forgiving of thin sections. Stainless 304 work-hardens, so the cutter must keep moving; a dwell of half a second will raise the surface hardness and dull the edge.

We stock or source 6061, 2024, 5052, 5083, 6063, 6082, 7075 and ADC12 in aluminum; 303, 304, 316, 316L, 420, 430, 431, 440C and 17-4PH in stainless; 1018, 1045, 4130, 4140, 4340 and A36 in steel; and titanium grades TA1, TA2 and TC4. Plastics include ABS, PC, PMMA, POM, PA, PEEK, PP, HDPE and carbon fibre.

Stock form changes the setup. Plate is easy to clamp and gives a flat reference. Bar stock suits turned parts on mill-turn centers. Castings and forgings carry skin and draft, so the first operation has to establish a clean datum before any tolerance is honored.

Leave stock allowance on purpose. For a 100 mm aluminum plate, 0.5 mm per side is enough for a cleanup pass. For stainless, allow 0.8 mm. If the part will be heat treated after roughing, allow 1.0 mm or more and plan a semi-finish cut after treatment.

On size limits: our largest travel is 4,000 × 400 × 150 mm, with medium envelopes of 750 × 1,150 × 550 mm and 600 × 600 × 600 mm, and compact envelopes of 500 × 500 × 450 mm and 500 × 310 × 200 mm. Parts near the edge of an envelope need a workholding plan, not just a bigger machine.

• 1
  Stainless 304Never let the cutter rub. Keep chip load up and coolant on the cut.
• 2
  Titanium TC4Low surface speed, high feed per tooth, plenty of coolant.
• 3
  PEEK and POMExpect movement after machining. Stress-relieve or finish in a second pass.

A vise and two parallels handle a large share of 3-axis work. The part sits on the parallels, the movable jaw clamps, and the top face becomes Z zero. Problems start when the part is taller than it is wide: clamping pressure lifts the far end, the first cut is flat, and the flip reveals a taper.

For thin plates, use a fixture plate with tapped holes and low-profile clamps, or hold the part on a vacuum chuck. For a 2 mm aluminum plate, side clamping will bow it. Soft jaws machined to the part profile spread the load and cut vibration.

Five-axis work usually runs on a Ø400 mm rotary table with a zero-point system. That lets us machine five faces in one setup. The benefit is not speed; it is that datums never change, so position tolerance between faces stays inside ±0.005 mm without stacking error.

Mind the clamp positions against the toolpath. A clamp that sits 3 mm from the finishing pass will either be hit or force the cutter to slow down and leave a witness mark. Draw the clamps in the CAM setup and check clearances at the widest tool diameter, not the nominal one.

Thermal drift is real on long cycles. A part that measured 50.000 mm at 08:00 can read 50.020 mm at 14:00 if the shop warms by 5 °C. For tight work, let the part cool before final inspection.

• 1
  Zero-point systemsRepeatable re-clamping within a few microns on 5-axis tables.
• 2
  Soft jawsMachine them to the part profile for thin or finished surfaces.
• 3
  Clamp clearanceCheck at maximum tool diameter plus 1 mm safety.

Roughing removes bulk with the largest cutter the geometry allows. On aluminum, a 12 mm three-flute end mill at 8,000 rpm and 3,000 mm/min is a normal starting point, with 0.5 mm radial engagement for high-efficiency paths. On 304 stainless, drop surface speed sharply and keep the feed per tooth up so the edge cuts instead of rubbing.

Finishing determines the surface callout. As-machined surfaces land around Ra 1.6–3.2 μm. A careful finishing pass reaches Ra 0.8–1.6 μm. Below that, we are talking about Ra 0.2–0.8 μm, which usually means a smaller stepover, a fresh cutter, and sometimes a polishing operation afterward.

Tolerance and finish interact. If a face is called out at ±0.005 mm and Ra 0.4 μm, the finishing pass has to be light and the tool has to be sharp. Spring passes help here: one extra contour at the same depth with zero stock removes deflection marks without changing the dimension.

Chip evacuation decides whether the finish holds. Deep pockets in aluminum need air blast or through-spindle coolant. In titanium, heat stays in the cut, so coolant must reach the edge, not just the part. If chips recut, the surface tears and the cutter wears on the flank.

Watch for tool engagement in corners. A cutter entering a corner at full radial width sees a sudden load spike. Trochoidal or constant-engagement paths keep the load steady, which protects both the tool and the wall tolerance.

• 1
  Aluminum 6061High speed, high feed, large radial stepover for roughing.
• 2
  Stainless 304Lower surface speed, no dwell, generous coolant.
• 3
  Titanium TC4Moderate speed, high feed per tooth, rigid setup.