CNC Machined Part Fabrication Process

• 1
  What matters most
• 2
  DFM review: the questions asked before chips fly
• 3
  Material selection and raw stock preparation
• 4
  CAM programming and setup design
• 5
  Machining sequence: roughing, semi-finishing, finishing
• 6
  In-process inspection and post-processing
• 7
  The fabrication sequence in practice
• 8
  Stage-by-stage reference

A DFM review is not a courtesy check. It decides whether the part can be made at the tolerance on the drawing, on the machine that will actually run it. We start with the 3D model, the 2D drawing and the callouts for critical features, then walk the geometry feature by feature.

Internal corners are the first stop. A rotating cutter leaves a radius equal to its own, so a 90° internal corner in a deep pocket cannot be milled. The practical minimum is a corner radius of about one-sixth the pocket depth. Deeper than that and you need a smaller tool, which means slower feed rates and higher cost, or an EDM burn after milling.

Next come walls and floors. Aluminum walls under 0.8 mm and stainless walls under 1.0 mm tend to deflect or chatter during finishing. If the design needs a thin web, we look at whether a supporting rib or a temporary boss can be added and removed later.

Threads, holes and datums get their own pass. A tapped hole needs roughly 1.5× the nominal diameter in depth for full thread engagement. Blind holes should have a flat or conical bottom that a standard drill can produce. Datum features must be reachable in the same setup as the features they locate.

• 1
  Corner radiusKeep internal radii at 1/6 of pocket depth or larger.
• 2
  Wall thickness0.8 mm minimum in aluminum, 1.0 mm in stainless.
• 3
  Thread depth1.5× nominal diameter for full engagement.
• 4
  Datum accessDatums should be machinable in the same setup as located features.

Material choice is usually fixed by the application, but the stock form is not. Bar, plate, extrusion and forging behave differently under the same program. Plate is rolled, so it carries internal stress that releases when you remove material. A long, thin bracket cut from plate can bow 0.2–0.5 mm after the first roughing pass.

Grain direction matters on parts that see fatigue or impact. For 7075 and 17-4PH, we check whether the load path runs with or across the grain. Where it matters, we call out stock orientation on the setup sheet rather than leaving it to the operator.

Hard skin is the other common surprise. Extruded and hot-rolled stock often has a harder outer layer that dulls tools faster and shifts the first cut. We take a 0.5–1.0 mm cleanup pass on all faces before any finishing operation.

For castings and near-net forgings, we ask for the stock drawing and the allowance map. Inconsistent allowance means the first operation has to remove different depths around the part, which shows up later as warpage.

Material grades we run most often: 6061-T6, 7075, 304 and 316L stainless, 4140 steel, Ti-6Al-4V, and engineering plastics such as POM and PEEK.

CAM turns the model into toolpaths, but the setup plan comes first. We decide how many setups the part needs, which features are cut in each, and where the datums sit. Fewer setups means better positional accuracy because every re-clamp adds error.

Tool selection follows the geometry. A 12 mm carbide end mill roughs most aluminum pockets efficiently at 6,000–10,000 rpm and 0.1–0.2 mm/tooth feed. Finishing passes drop to 0.02–0.05 mm/tooth with a 6 mm or 3 mm tool to control surface finish.

Workholding is designed with the part, not after it. Thin plates go on a vacuum plate or get sacrificial tabs. Long parts that would chatter get support from a tailstock or steady rest. A part that moves during cutting will not hold ±0.005 mm no matter how good the program is.

We simulate every program with stock, fixture and tool holder modeled. Collision checks and remaining-stock analysis catch the gouges that would otherwise appear on the first article.

• 1
  Setup countEach re-clamp adds positional error; design for three or fewer.
• 2
  Roughing parameters6,000–10,000 rpm and 0.1–0.2 mm/tooth in aluminum.
• 3
  Finishing parameters0.02–0.05 mm/tooth with a smaller tool.
• 4
  SimulationModel the fixture and holder, not just the tool.

Roughing removes most of the volume fast and leaves a controlled allowance. In aluminum we leave 0.3–0.5 mm on walls and floors. In stainless and titanium the allowance is smaller, 0.2–0.3 mm, because the cutting forces are higher and deflection grows quickly with tool overhang.

Semi-finishing follows to even out the allowance. This pass is what makes the finishing cut predictable. Skip it and the finishing tool sees varying load, which shows up as chatter marks and inconsistent surface finish.

Finishing is where tolerance and surface texture are made. For a Ra 0.8–1.6 μm finish, use a sharp, coated tool, a 0.1–0.2 mm radial stepover on contours, and climb milling. For finer surfaces down to Ra 0.2–0.8 μm, we slow the feed, increase spindle speed, and sometimes add a separate polishing or lapping operation.

Multi-axis work changes the plan. On a 5-axis machine we can reach five faces in one setup and keep the tool normal to curved surfaces, which improves finish and reduces hand work. On parts with a rotary axis, continuous 4-axis motion cuts a cylindrical feature in one pass instead of indexing around it.

Thread milling is preferred over tapping for large threads and for materials above 35 HRC. It produces a cleaner thread, allows adjustment of the fit, and does not risk a broken tap inside the part.

In-process inspection catches drift before it becomes scrap. On a first article we check all dimensions against the drawing. On production runs we check the critical few every batch, and use in-machine probing where the tolerance is tight. A probe pass after roughing tells the operator whether the part moved and whether the allowance is still there.

Post-machining operations are scheduled by what they change. Deburring and edge breaking come first, because a raised burr will hold a part off a fixture face. Then heat treatment if the drawing calls for it. Stress relief between roughing and finishing is common on thin, long parts.

Surface finishing is last, and it is not cosmetic only. Bead blasting hides tool marks and creates a uniform matte surface. Anodizing adds a hard oxide layer, and hardcoat anodizing builds 25–50 μm per surface. If a bore must stay at size after hardcoat, we mask it or cut it undersize before coating.

Plating and coating thickness must be stated on the drawing. Electroless nickel at 10–25 μm will close a small hole; if the hole is a slip fit, the plater needs to know the final dimension.