CNC processing products: what decides whether a design machines cleanly

• 1
  What CNC processing products actually are
• 2
  How setup count changes geometry, not just price
• 3
  Tolerance, surface finish and where the cost sits
• 4
  Material choice and how it behaves at the cutter
• 5
  Five design checks before you release a drawing
• 6
  Which process fits which part

A CNC processing product is a metal or plastic part produced by controlled material removal. A rotating cutter follows a toolpath generated from your CAD model, and stock is cut away until the shape matches the drawing. Milling covers pockets, faces, slots and profiles. Turning covers cylindrical and threaded features. Most real parts need both.

The cutting tool is the constraint that shapes everything else. A Ø 6 mm end mill reaching 40 mm into a pocket will deflect, so the wall it leaves tapers and chatters. A Ø 0.5 mm cutter can reach fine detail but removes very little material per pass and breaks easily. Every feature you design has to be reachable by a tool that is stiff enough to cut it accurately.

That is why the same geometry can cost very different amounts at two suppliers. The part does not change, but the setup plan, the tool list and the number of re-fixturings do. A design that fits in two setups on a five-axis center is a different job from the same design spread across five setups on a three-axis machine.

Tolerance works the same way. Holding ±0.005 mm on a 20 mm bore is routine. Holding it across a 400 mm bolt circle, on a thin wall, in a soft aluminium alloy, is a different problem. The number on the drawing is not the whole story. Where it sits on the part matters just as much.

• 1
  Milling cuts flat and prismatic featuresPockets, slots, faces, contours and drilled holes.
• 2
  Turning cuts round featuresShafts, bushings, threads and grooves, usually from bar stock.
• 3
  Tool reach sets the limitDeep, narrow pockets force small cutters and slower feed rates.

Every time a part is unclamped and turned to reach a new face, two things happen. The part moves a small amount, and the operator has to re-establish the datum. On a three-axis machine, a part with features on five faces might need four or five setups. Each one adds a small positional error and a lot of handling time.

A five-axis machining center rotates the tool or the table instead. With a Ø 400 mm rotary table and simultaneous motion on two rotary axes, the cutter can approach the part from almost any direction in a single clamp. That removes the re-datuming error and keeps the relationship between features tight.

This is why some shapes are only practical on five-axis equipment. Impellers, turbine blades, angled ports and sculpted surfaces need the tool to tilt continuously as it follows the surface. A three-axis machine can only reach them by hand-fettling or by splitting the part into pieces that are later joined.

The trade-off is not free. Five-axis toolpaths are longer to program, the machine is slower to set up for simple work, and fixture design has to account for the table moving under the part. For a flat bracket with holes on one face, a three-axis machine is faster and cheaper. Use the right machine for the shape in front of you.

• 1
  One setup means one datumFewer re-fixturings keep feature-to-feature relationships tight.
• 2
  Simultaneous axes reach sculpted surfacesThe tool tilts continuously instead of stepping around the part.
• 3
  Simple parts do not need five axesPrismatic work on one or two faces runs cheaper on three-axis mills.

Tolerance and finish are two separate conversations, and mixing them causes trouble. A part can be dimensionally tight and still have a rough surface, or smooth and loose. Tolerance controls where the surface sits in space. Finish controls how smooth that surface is.

Our standard machining tolerance is ±0.005 mm (±0.0002 in). That is achievable on features with good tool access, rigid fixturing and stable material. It is not achievable on a 0.8 mm thin wall that flexes under clamping pressure, or at the bottom of a deep pocket where the cutter is unsupported.

Surface finish follows the same logic. As-machined parts run Ra 1.6–3.2 μm. A high-quality machined finish lands at Ra 0.8–1.6 μm with a controlled stepover and sharp tooling. Fine finishes at Ra 0.2–0.8 μm usually need a finishing pass with a small stepover, or a secondary operation such as lapping or polishing.

The practical rule is to specify the loosest tolerance and the roughest finish that still makes the part work. Tightening a tolerance from ±0.05 mm to ±0.005 mm across a whole drawing does not make the assembly better. It makes the part slower to cut, harder to inspect and more likely to be rejected at final inspection for a dimension that never mattered.

• 1
  Tighten only functional dimensionsBearing seats, mating bores, seal grooves and datum faces.
• 2
  Leave cosmetic faces looseNon-mating outer surfaces rarely need better than ±0.1 mm.
• 3
  Thin walls fight the toleranceBelow about 1 mm, clamping and cutting forces dominate the result.

Material selection is not only about strength. It decides how the part cuts, how it finishes and how stable it stays after machining. Aluminium 6061-T6 is the default for prototypes and fixtures because it machines fast, holds tolerance well and takes anodizing cleanly. 7075 offers higher strength but is gummier and harder on tooling.

Stainless grades 303 and 304 machine very differently. The 303 free-machining grade breaks chips cleanly and holds a good finish. The 304 grade work-hardens under a dull cutter, so the tool has to stay sharp and the feed rate has to stay high enough to cut rather than rub. 17-4PH gives high strength after heat treatment but needs more care on the finishing pass.

Titanium TC4 (Ti-6Al-4V) and Inconel sit at the difficult end. Both generate heat at the cutting edge rather than carrying it away in the chip, so tool life drops sharply and cutting speeds fall. They are still machinable, but the toolpath has to be planned around heat, not around cycle time.

Plastics behave on their own terms. POM and PEEK hold tolerance well and are stable. ABS and PP move with temperature and clamp pressure, so a tolerance that works on aluminium may not hold on a soft polymer. If the part has to be dimensionally tight, the material choice is part of that decision.

• 1
  Aluminium 6061-T6Fast to cut, stable, good anodizing base for most prototypes.
• 2
  Stainless 303 vs 304303 machines freely; 304 work-hardens if feed rates drop.
• 3
  Titanium and InconelHeat stays at the edge; slower speeds and shorter tool life.

Check tool access first. Look at every pocket and slot and ask what diameter cutter can reach the bottom. A pocket narrower than about four times the cutter diameter, and deeper than about three times the cutter diameter, will need a smaller tool and a slower pass. If the corner radius is smaller than the standard radius for that depth, the shop has to switch tools mid-operation.

Check wall thickness next. Walls under about 1 mm in aluminium, or under about 1.5 mm in stainless, tend to move during machining. They also move during anodizing or heat treatment. If a thin wall carries a tight tolerance, expect the shop to leave material and take a light finishing pass, which adds time.

Check the datum scheme. Pick three faces or features that a machinist can actually clamp and probe, and reference the drawing to those. A drawing dimensioned from a curved surface or from a feature that is cut late in the process forces the shop to guess, and guessing costs tolerance.

Finally, check the thread and hole callouts. Specify standard thread pitches, standard drill sizes and standard corner radii. Every non-standard callout means a special tool or a manual operation, and those are the steps most likely to introduce variation.

• 1
  Tool accessConfirm a cutter can reach the bottom of every pocket.
• 2
  Wall thicknessKeep thin walls above 1 mm where tolerance matters.
• 3
  Datum schemeReference to faces a machinist can clamp and probe.