How to Make CNC Machine Step by Step

• 1
  Key takeaways
• 2
  What it takes to make CNC machine parts step by step
• 3
  Stock prep and workholding before you cut
• 4
  Tool selection and cutting parameters that hold tolerance
• 5
  When to use 3-axis, 4-axis, or 5-axis machining
• 6
  Surface finish, inspection, and what to check before shipping
• 7
  How to make CNC machine parts step by step: the 7-step sequence
• 8
  Machine choice and parameters by part type

Before any cutter spins, the part has to survive a design review. This is where to make CNC machine parts step by step either gets easy or gets expensive. A wall that is 0.4 mm thick in 7075 aluminum will chatter; the same wall in POM will deflect under clamping pressure. Review the drawing for minimum wall, corner radii, thread depth, and any feature that needs a tool to reach into a pocket.

The second gate is stock. Bar stock, plate, or near-net forging all change the setup count. A part cut from 25 mm plate may need two setups; the same part from a casting may need one. Stock allowance of 0.5–1.0 mm per side is normal for milled faces, more if the surface is as-cast or hot-rolled.

Third, pick the machine class. A 3-axis mill handles prisms and open pockets. A 4-axis or 5-axis center handles parts with features on four or five faces, undercuts, or complex contoured surfaces. At GreatLight we run 16 simultaneous 5-axis machining centers alongside 27 three-axis machines, so the sequence is chosen by geometry, not by what is free.

None of these steps involve cutting metal yet. That is the point. Most of the cost and most of the scrap risk are decided in this planning stage.

• 1
  Minimum wallKeep aluminum above 0.8 mm; steel above 1.0 mm where possible.
• 2
  Internal cornersMatch the corner radius to the cutter; a Ø6 mm end mill leaves a 3 mm radius.
• 3
  Thread depth1.5 × diameter in aluminum, 1.0–1.5 × in steel, is a safe rule.

Cut the stock to size with 1–2 mm of machining allowance on every face that will be finished. For plate, saw-cut edges often have 0.3–0.5 mm of bow, so face both sides before drilling. Skipping this step is one of the most common reasons a hole comes out off-position.

Workholding decides whether the tolerance in the drawing survives the cut. A vise with soft jaws is fine for a 100 mm bracket. A thin plate or a long part needs a fixture plate, toe clamps, or a vacuum chuck. For parts with a flatness call under 0.05 mm, clamp lightly and support the underside; over-tightening a vise will bow a 6 mm plate.

Fixtures also set the datum. If the drawing calls out datum A on a machined face, that face should be cut first and used for every later setup. Measuring from a saw-cut edge is a common mistake and it shows up as a 0.1–0.2 mm offset on the finished part.

For small runs, a modular fixture plate with a known hole grid saves setup time. For production runs above 1,000 pieces, a dedicated soft-jaw or hydraulic fixture pays for itself in repeatability.

• 1
  Face first, drill secondA flat datum face removes bow before any hole is located.
• 2
  Light clamp on thin plateA 6 mm plate bows 0.05–0.1 mm under normal vise pressure.
• 3
  Support long partsUnsupported overhang vibrates and leaves chatter marks.

Tool choice follows material and feature size. Aluminum 6061-T6 cuts well with 3-flute carbide end mills at 200–300 m/min surface speed and 0.05–0.15 mm feed per tooth. Stainless 304 and 316 work harden, so keep the cutter engaged, use 4-flute carbide with a coating, and cut at 60–120 m/min. Titanium Ti-6Al-4V runs slower still, 30–60 m/min, with copious coolant.

For deep pockets, use the shortest tool that reaches. A Ø6 mm end mill with 40 mm of flute length will deflect far more than one with 15 mm. If the pocket is deeper than 3 × diameter, step down in 0.3–0.5 × diameter increments rather than taking one deep pass.

Finishing passes should remove 0.2–0.5 mm radial stock. More than that loads the tool and hurts surface finish. To hit Ra 0.8–1.6 μm, a sharp finishing cutter with a 0.4–0.8 mm corner radius and a light pass is usually enough. For Ra 0.2–0.8 μm, add a separate finishing strategy or a light polishing step.

Coolant matters as much as speed. Aluminum likes flood coolant or high-pressure air. Stainless and titanium need flood coolant to control heat at the cutting edge. Dry cutting is fine for cast iron and some plastics, but not for gummy materials like 304.

• 1
  Aluminum 6061-T6200–300 m/min, 3-flute carbide, 0.05–0.15 mm per tooth.
• 2
  Stainless 304 / 31660–120 m/min, 4-flute coated carbide, flood coolant.
• 3
  Titanium Ti-6Al-4V30–60 m/min, sharp uncoated or AlTiN tool, heavy coolant.

A 3-axis machine cuts from one direction. It is the fastest and cheapest option for plates, brackets, covers, and any part whose features are all reachable from the top. Most parts under 500 mm fit this group, and the setup is simple: one vise, one datum, one program.

A 4-axis mill adds a rotary table, usually Ø400 mm or smaller. It lets you index the part to a second or third face without re-clamping, which removes the position error that comes from moving a part between setups. Use it for parts with features on two or three sides, or for round parts that need cross-drilling.

A 5-axis center moves the tool in two extra rotary axes while cutting. It handles contoured surfaces, undercuts, and deep pockets with a single setup. The trade-off is cycle time and programming effort. For a complex aerospace bracket, a single 5-axis setup often beats three 3-axis setups on total cost because it removes two re-clamps and two chances to lose position.

We run 127 high-precision CNC machines in total, including 16 simultaneous 5-axis centers, 12 four-axis mills, 27 three-axis machines, and 16 mill-turn centers. That mix means the machine is chosen by geometry and volume, not by availability.

• 1
  3-axisPlates, brackets, covers; all features from one direction.
• 2
  4-axisFeatures on two or three sides; round parts with cross-holes.
• 3
  5-axisContoured surfaces, undercuts, deep pockets; one setup instead of three.

Surface finish is a function of tool, speed, and pass depth, not just a final polish. An as-machined finish lands around Ra 1.6–3.2 μm. A careful finishing pass with a sharp cutter reaches Ra 0.8–1.6 μm. For Ra 0.2–0.8 μm, we add a separate finishing strategy or a controlled polish, and that step needs to be in the quote from the start.

Inspection should match the drawing's datums. Measure flatness on a surface plate, hole position with a CMM or a pin gauge, and thread depth with a depth micrometer. A part that measures well from a saw-cut edge but fails from datum A is a part that will fail at assembly.

For tight work, we hold ±0.005 mm (±0.0002 in) on critical features and inspect 100% before shipment. Raw material certificates, in-process checks, and final inspection reports are available on request. If a customer needs documented first-article inspection, that is planned into the routing, not added at the end.

Packaging matters for finished surfaces. Anodized or polished parts should be wrapped and separated. A loose part sliding in a box will scratch a Ra 0.4 μm finish in transit, and that is a defect the customer sees first.

• 1
  As-machinedRa 1.6–3.2 μm; fine for internal and non-cosmetic faces.
• 2
  High finishRa 0.8–1.6 μm; needs a light finishing pass and a sharp tool.
• 3
  Fine finishRa 0.2–0.8 μm; separate operation, quoted from the start.