CNC Machined Parts Explained: From CAD Model to Finished Metal

• 1
  What CNC machined parts actually are
• 2
  How a CNC machined part is made, step by step
• 3
  Milling, turning, and EDM: which process fits the feature
• 4
  How material choice changes what the machine can hold
• 5
  The real sources of tolerance error
• 6
  What makes a part easy or hard to machine
• 7
  Matching process and setup to the feature

CNC machined parts start as solid stock and end as a shape defined by a program. A rotating or stationary cutting tool removes material along a path calculated from your CAD geometry. Nothing is formed or cast. The final dimensions come from tool position, not from a mold cavity.

That single fact drives most of the engineering trade-offs. You can hold tight tolerances because the machine moves on ball screws with position feedback. You also pay for every cubic centimeter of material you remove, and for every setup the part needs.

Subtractive also means the tool must physically reach the surface. A deep pocket with a square internal corner cannot be cut by a round end mill. The corner radius equals the tool radius at minimum. Designers who forget this get a quote revision instead of a part.

The workflow is linear, but problems do not stay in their own step. A tolerance that looks fine in CAD can be impossible to hold on a 3-axis machine because of fixturing, not because of the machine itself. Below is what each stage contributes and where it can go wrong.

Design and CAM programming decide most of the cost before any metal is cut. Material choice then sets cutting speeds, tool life, and how much the part will move after machining. Setup and machining turn the program into geometry. Finishing changes surface and corrosion behavior but can also shift dimensions on thin walls.

• 1
  Design and modelSolid model plus a 2D drawing that states tolerances, datums, and critical features. A model alone is not a manufacturing instruction.
• 2
  CAM programmingToolpaths, feeds, speeds, and workholding are defined. Rest material and tool reach are checked here, not on the machine.
• 3
  Material selectionAlloy, temper, and stock form. The same geometry in 6061-T6 and 304 stainless behaves differently under the same cutter.
• 4
  Setup and fixturingHow the blank is held. Vise, soft jaws, vacuum plate, or a custom fixture. Datum transfer happens here.
• 5
  MachiningRoughing removes bulk, semi-finishing controls stock-on, finishing sets final size and surface.
• 6
  Post-processingDeburr, heat treat, anodize, plate, or laser mark. Sequence matters when heat treat follows tight tolerance.

Milling uses a rotating multi-point cutter against a workpiece that can move in three, four, or five axes. It handles pockets, slots, flat faces, and contoured surfaces. Prismatic parts and plate work belong here. A 5-axis center reaches features that would otherwise need two or three separate setups, and each eliminated setup removes a datum shift.

Turning rotates the workpiece against a single-point tool. It produces round parts fast and holds diameter tolerance well. Parts with a large length-to-diameter ratio need support, or the material deflects away from the tool and the middle of the part comes out oversized.

EDM burns material away with a spark across a small gap. It cuts hardened steel and square internal corners that a milling cutter cannot reach. It is slow, and it leaves a recast layer that may need removal if the part sees fatigue loads.

Drilling sits between these. It is fast for holes up to roughly 20 times diameter, but hole location depends on the spot drill and on how rigidly the part is held.

Aluminum 6061-T6 cuts clean and holds ±0.005 mm on a rigid setup. It also moves when you remove a lot of stock from one side, because internal stress releases as material leaves. Rough, stress-relieve, then finish. That sequence costs one extra operation and saves a scrapped part.

Stainless 304 work-hardens. A cutter that rubs instead of cutting raises local hardness and dulls the next pass. Feeds must stay aggressive enough to bite under the work-hardened skin. 303 machines far better because of added sulfur, but it welds less cleanly and is not ideal for every application.

Titanium Ti-6Al-4V conducts heat poorly, so the cutting edge absorbs it. Tool life drops and surface finish suffers if coolant and speed are not managed. Inconel is worse. Both are machinable, but the cost per part reflects the time, not the material price alone.

Plastics like POM and PEEK cut easily but deflect under clamping. A vise tightened like it holds steel will bow a thin plastic wall. Light clamping and sharp tools matter more than spindle speed here.

Machine accuracy is rarely the limiting factor. Thermal growth, tool deflection, and workholding dominate. A spindle warms up over the first hours of a shift and grows along Z. Shops that hold tight tolerance let the machine warm up or compensate in the program.

Tool deflection scales with length cubed. A long, thin end mill pushed too hard bends away from the wall and leaves a tapered pocket. The fix is a shorter tool, a smaller step-over, or a roughing pass that leaves uniform stock for the finisher.

Datum transfer is the quiet one. Move a part from vise to fixture and the new zero is not the old zero. Every extra setup adds stack-up. Five-axis work reduces setups and therefore reduces this error, which is why complex parts with many angled features often come out more accurate on a 5-axis machine than on three separate 3-axis operations.

A part is easy when the tool can reach every surface from a small number of directions, walls are thick enough to resist cutting forces, and tolerances are tight only where they matter. Blanket tolerances on a drawing raise cost without adding function.

Internal corners should carry a radius at least equal to the largest cutter that will finish the pocket. A nominal sharp corner forces EDM or a tiny tool that breaks. Threads and holes should be specified with standard sizes so the shop uses a tap or reamer on the shelf.

Deep pockets narrower than four times the tool diameter are slow. The cutter cannot clear chips, heat builds, and the operator has to peck. If the feature is not functional, open it up.

Hard parts are not bad parts. They just cost more. A part with an undercut, a thin floor, and a 0.4 μm finish requirement is achievable, but expect a longer quote review and a more careful inspection plan.