CNC parts manufacturing

• 1
  What happens inside CNC parts manufacturing
• 2
  3-axis, 4-axis and 5-axis: what each can reach
• 3
  Where tolerance and surface finish stop being free
• 4
  Features that make a part easier or harder to machine
• 5
  Material choice and setup count in real parts
• 6
  Which machine suits which part feature

CNC parts manufacturing starts with a solid block, bar or casting and removes material until the shape is left. A rotating cutter moves along programmed paths while the workpiece is held in a vise, chuck or fixture. Nothing is formed or pressed. The geometry comes from the tool path, so the drawing and the CAM file are the real limits on what you get.

Cutting heat is the quiet problem. Aluminium 6061 and 7075 carry heat away fast, so you can run aggressive cuts and still hold size. Titanium TC4 and Inconel hold heat at the edge, so speeds drop and tool wear climbs. Stainless 316 behaves in between. A shop that knows the material will change feeds, coolant and tool coating before the first chip, not after a scrapped part.

Roughing and finishing are separate operations for a reason. Roughing removes most of the volume and leaves stock for the finishing pass. Finishing takes 0.2–0.5 mm off the walls and controls the final size, surface finish and corner radii. If you see chatter on a thin wall, the fix is usually a lighter finishing pass, more support, or a change in the order of operations rather than a slower spindle.

Where a part sits in the machine decides what it costs. A part with features on one face is simple. A part with holes on five faces, deep pockets and tight true position needs the workpiece repositioned, and every reposition adds a setup and a chance for error. That is the core trade-off in CNC parts manufacturing: geometry drives setups, setups drive cost and lead time.

• 1
  Material moves heatAluminium runs fast, titanium and Inconel run slow
• 2
  Rough then finishFinishing passes set size and surface texture
• 3
  Setups follow facesMore machined faces usually mean more setups

A 3-axis machine moves the cutter in X, Y and Z while the part stays still. It is the right choice for plates, housings, brackets and any part you can reach from one direction. It is also the cheapest way to hold ±0.005 mm because the part is clamped once and the geometry stays rigid. If your part is mostly a flat face with pockets and through holes, 3-axis work is the honest answer.

A 4-axis machine adds rotation around one axis, usually A. That lets you machine a cylinder or a shaft in one setup: flats, keyways, cross holes and slots around the diameter. It removes the repositioning that a 3-axis machine would need for each side. Parts like manifolds, spools and rotary fittings are common 4-axis work.

A 5-axis machine adds a second rotary axis, so the cutter can approach the part from almost any angle while the tool stays short and stiff. This is what allows undercut walls, blended surfaces, impeller blades and deep cavities with a single setup. The benefit is not only reach. Short tools deflect less, so a 5-axis job can sometimes hold tighter size on a thin wall than a 3-axis job with a long tool.

The trade-off is programming and checking. 5-axis tool paths are harder to verify, and a collision is expensive. Use 5-axis when the geometry demands it, not because it sounds better. For a simple bracket, 3-axis work will be faster, cheaper and just as accurate. For a part with 12 angled holes on five faces, 5-axis is the only sensible route. We hold 16 simultaneous 5-axis centers, 12 four-axis mills and 27 three-axis machines, so the machine is matched to the part instead of the part being forced onto one platform.

• 1
  3-axisFlat faces, pockets, through holes, one clamp
• 2
  4-axisShafts and cylinders machined around the diameter
• 3
  5-axisUndercuts, blended surfaces, one-setup five-face work

Tolerance is a cost curve, not a switch. A general machining tolerance of ±0.1 mm is routine on most metals. Moving to ±0.02 mm means tighter control on the finishing pass and more frequent checks. Holding ±0.005 mm (±0.0002 in) means temperature, tool wear and clamping force all matter, so the part may need a warm-up cycle and an in-process measurement. That is achievable on our machines, but it is not the default for every dimension on a drawing.

Surface finish works the same way. As-machined surfaces sit around Ra 1.6–3.2 μm. A high-quality finish of Ra 0.8–1.6 μm usually needs a finer finishing pass and a sharper tool. Fine finishes of Ra 0.2–0.8 μm may need a dedicated finishing operation or a secondary process such as lapping or polishing. If a sealing face needs Ra 0.4 μm, say so on the drawing. If a clearance hole needs Ra 3.2 μm, do not ask for 0.4 μm across the whole part.

Only put a tight tolerance on the dimensions that matter. A bearing bore at ±0.005 mm makes sense. A bolt clearance hole at the same tolerance adds cost and inspection time for no benefit. Mark datum faces, critical dimensions and reference surfaces clearly. That single habit removes more back-and-forth than any other change to a drawing.

Inspection follows from the same logic. We check every part before shipment, with raw material verification, in-process monitoring and a final inspection, and we supply reports on request. If you need a first article inspection or a CMM report on a specific feature, list it on the drawing. A report costs time, so it belongs on the features you will actually measure.

• 1
  ±0.1 mmGeneral machining, most metals, no special control
• 2
  ±0.02 mmFinishing pass control and more frequent checks
• 3
  ±0.005 mmTemperature, tool wear and clamping all matter
• 4
  Ra 0.2–0.8 μmFine finish, may need a secondary operation

Internal corners are the classic trap. A pocket drawn with a sharp inside corner cannot be cut by a round cutter, so it comes out with a radius equal to the tool radius. Specify the corner radius you can accept, and keep it at least one third of the pocket depth so a reasonably stiff tool can reach the floor. A 2 mm radius in a 40 mm deep pocket forces a long, thin tool, and that tool will chatter.

Wall thickness matters more than overall size. A 200 mm aluminium plate with a 1.5 mm wall will move when the clamps come off, and no tolerance on the drawing can fix that. Keep walls above roughly 1 mm for aluminium and above 1.5–2 mm for stainless and titanium, and add ribs instead of thinning a wall further. If a thin wall is unavoidable, expect to machine it in stages and possibly stress-relieve between passes.

Threads and holes are cheap when they follow standard sizes. A metric or imperial thread in a standard pitch needs no special tool. A deep, small-diameter hole is a different story: past roughly 10× the diameter, chip evacuation and drill wander both get worse. Add a pilot hole and consider peck drilling. Blind holes should have a flat or conical bottom that the drawing states, because a standard drill leaves a cone.

Text and markings are usually added by laser after machining. Minimum character height is 1.5 mm; anything smaller may not read cleanly on a rough or curved surface. Serial numbers, logos and part numbers all fit that rule. Engrave on a machined flat where possible.

• 1
  Corner radiusAt least one third of pocket depth for tool stiffness
• 2
  Wall thicknessAbove 1 mm aluminium, 1.5–2 mm stainless or titanium
• 3
  Deep holesPast 10× diameter, add a pilot and peck drill
• 4
  Laser markingMinimum character height 1.5 mm

The material list is long, but the design decision is short. Aluminium 6061-T6 is the default for housings, brackets and fixtures: easy to cut, stable, and it anodizes well. 7075 gives higher strength for aerospace and tooling work but cuts slower and costs more. Stainless 303 machines freely, 304 and 316 are tougher, and 17-4PH gives high strength after heat treatment. Titanium TC4 and Inconel are for high-temperature and high-strength parts where the cost is justified by the application.

Plastics behave differently. POM and ABS cut cleanly and hold size. PEEK is stable at high temperature but abrasive and expensive. Carbon fibre wears tools fast and can delaminate at the edges, so it needs sharp tooling and light passes. None of these behave like aluminium, and a drawing that ignores that will produce a part that measures correctly on the machine and moves a day later.

Setup count is the hidden driver of both price and lead time. A part that is machined from four sides needs four setups, and each setup has a positioning tolerance. That is why 5-axis work can be cheaper on a complex part than 3-axis work: it collapses five setups into one. It is also why a simple part should stay simple. If you can reach every feature from two directions, do not design a part that needs five.

For low-volume and prototype work, no minimum order quantity applies, so a single part and a 10,000-part run use the same first step: a DFM review. We return a quotation and a free DFM analysis within 12 hours, and production can start within 24 hours once the drawing and material are confirmed. Parts ship in 3–5 days for standard scope. Those numbers assume the drawing is complete; missing tolerances and unclear datums are the usual cause of delay.

• 1
  6061-T6Default for housings, brackets and fixtures
• 2
  7075 and 17-4PHHigher strength, slower cutting, higher cost
• 3
  PEEK and carbon fibreStable or strong but abrasive on tooling
• 4
  SetupsEach extra setup adds position error and time