Manufacturing processesReading time 15 min

Choose the Process Before You Quote the Part

The same geometry can be milled, turned, stamped or moulded at very different costs. Read the drawing for material, tolerance, finish and volume before committing to a process route.

01Three process families

Process selection starts with what happens to the material: it is removed, formed or introduced into a mould. Each route has a different balance of tooling cost, cycle time and achievable detail. The drawing narrows the options, while production volume determines which option is economical.

Family	Typical processes	Up-front cost	Cost per piece	Suits batches of
Cutting (removal)	Milling, turning, drilling, grinding, EDM	Low (fixtures)	High	1 to a few thousand
Forming (deformation)	Stamping, bending, forging, drawing, rolling	High (tooling)	Very low	Thousands upward
Moulding (filling)	Injection moulding, die casting, powder metallurgy	Very high (tooling)	Very low	Tens of thousands

Process cost depends on tooling, cycle time, material use and volume—not the drawing alone.

02Machining and its limits

Milling, turning, drilling and grinding all remove material. Cutting offers flexible geometry and tight control, but stock loss, tool wear and cycle time can make it expensive at volume. Compare these costs with the shape and tolerance the part actually needs.

The ladder of operations and accuracy

Operations	Typical tolerance	Typical Ra	What it asks
Rough milling / turning	±0.2 mm	6.3～12.5	Leaves stock, aims at removal rate
Finish milling / turning	±0.05 mm	1.6～3.2	Final cut for ordinary fitting surfaces
Reaming / boring	IT7 (±0.01 class)	0.8～1.6	Hole accuracy and cylindricity
Surface / cylindrical grinding	IT5～IT6	0.2～0.8	Hard material, finishing after heat treatment
Lapping / honing	IT4 and better	0.05～0.2	Sealing faces, gauges, cylinder bores

Tighter tolerances may require additional operations and inspection; choose only what function needs.

Five-axis and mill-turn

Every new setup introduces another opportunity for locating error. Multi-axis or mill-turn machines can keep more operations in one setup, which may help both cycle time and positional accuracy. Whether that advantage is worth the machine cost depends on the part.

03Forming and tooling cost

Stamping, bending, forging and drawing reshape material without cutting most of it away. Once the tooling is in place, cycle times can be short, but die cost and design constraints make production volume decisive.

Sheet-metal clues on the drawing

Uniform thickness. The whole drawing carries one thickness dimension; everything else is outline and hole positions.
Bend lines and bend radii. Too small a radius cracks; the usual floor is one material thickness for soft material and two for hard.
Flat pattern or developed length. Some customers supply the developed length; sometimes you must work it out.
Distance from hole to bend line. A hole too close to a bend distorts when formed; the usual requirement is more than 2.5 times thickness plus the radius.

The press brake, where most of a sheet metal part's shape is decided, which is why the flat length has to be right before anything is cut. — A press brake shapes much of a sheet-metal part, so the flat blank must be calculated before cutting.Wikimedia Commons・High-tonnage press brake・CC BY-SA 4.0

What a forging looks like on paper

A forging drawing may show a near-net outline beside the final machined profile. Draft, parting line and machining allowance reveal which surfaces need stock removed and where the process can hold tolerance.

04Moulding and wall thickness

Injection moulding is common for plastics and also has powder-based metal variants. Uniform wall thickness, draft, ribs, gates and ejector locations are clues that the part was designed around a moulding process.

Design item	Usual guidance	What happens if you ignore it
Wall thickness	Uniform, varying by no more than 25%	Shrinkage, sink marks, internal stress
Rib thickness	50–60% of the main wall	Sink marks at the rib root
Draft angle	0.5°–2° per side	Scuffing on ejection, stress whitening
Corner radii	Not less than half the wall thickness	Stress concentration, cracking
Gate position	Feed into the thick section, away from cosmetic faces	Short shots, flow marks, weld lines

Moulding rules can often be checked on the drawing before a trial tool is built.

05Drawing details that change cost

Tolerance grade. A general tolerance (ISO 2768-m) and an individually called-out IT7 are two different processes.
Surface finish. Ra 3.2 comes off a single milling pass; Ra 0.4 almost always means grinding.
Geometric tolerance. Position Ø0.05 may mean the whole feature has to be finished in one set-up.
Material. SUS304 machines far worse than S45C; tool life and cycle time both change.
Heat treatment. Placing it before or after finishing reorders the whole routing, and the distortion it causes has to be allowed for as stock on the drawing.
Surface treatment. Anodising, zinc plating and blackening all change dimensions. If the drawing does not say whether measurement is before or after treatment, there will be an argument at acceptance.