CNC machining skills: a 7-step method for parts that hold tolerance

• 1
  What matters most
• 2
  Read the drawing before you touch the machine
• 3
  Pick the material for the cut, not the spec sheet
• 4
  Plan workholding so the part stays still
• 5
  Set cutting parameters with a starting point, then adjust
• 6
  Inspect in-process and finish with purpose
• 7
  Step by step: from model to shipped part
• 8
  Which setup suits which part

CNC machining skills start on paper, not at the spindle. Read the drawing and mark every dimension that carries a tolerance tighter than ±0.05 mm. Those are the features that decide the setup plan, because a tight bore and a tight slot on opposite faces force you into one operation or a re-clamp with dial-in.

Next, list the datum features. A datum that only exists in the finished part cannot locate the first operation. If the drawing calls for a face that gets machined last, ask the designer which surface is allowed to be the practical zero. Most engineers will name a cast boss or a turned end.

Then check the smallest internal radius against the tool list. A 2 mm corner radius needs a 4 mm cutter to clear it. On a 60 mm deep pocket that is a length-to-diameter ratio of 15:1, which will deflect. Either open the radius or plan a wire-cut or EDM step.

Last, write down the finishing callout. Ra 1.6–3.2 μm comes straight off a sharp cutter. Ra 0.2–0.8 μm usually needs a separate finishing pass, a smaller step-over, or a polishing operation. Knowing this before quoting saves a second setup.

• 1
  Tolerance mapMark every feature tighter than ±0.05 mm.
• 2
  Datum checkConfirm a machinable zero point exists.
• 3
  Radius vs toolSmallest radius decides cutter diameter.
• 4
  Finish calloutRa 0.8 μm and below often needs a second pass.

Material choice drives tool life, cycle time and cost more than any CAM setting. Aluminium 6061-T6 machines clean at 300–600 m/min surface speed with carbide. Stainless 316 work-hardens if the cutter dwells, so keep feed per tooth above 0.05 mm and never let the tool rub.

Titanium TC4 (Ti-6Al-4V) is the opposite problem. It holds heat in the cut. Run surface speed at 40–60 m/min, flood coolant, and expect tool life measured in minutes, not hours. Inconel is worse; it is worth it only when the service temperature demands it.

Plastics behave differently again. POM and PEEK cut well but melt if you push rpm without clearing chips. Use sharp single-flute or two-flute cutters with high helix and air blast. ABS and PC are softer and tend to grab, so reduce depth of cut to 0.5 × diameter.

One practical rule: if the part does not need corrosion resistance or high strength at temperature, aluminium 6061 or 7075 will be cheaper and faster. Save stainless and titanium for the parts that genuinely need them.

• 1
  Aluminium 6061-T6300–600 m/min, carbide, easy chips.
• 2
  Stainless 316Watch work hardening, keep feed up.
• 3
  Ti-6Al-4V40–60 m/min, flood coolant, short tool life.
• 4
  POM / PEEKAir blast, low depth of cut, sharp flutes.

Chatter is usually a workholding problem, not a toolpath problem. A vise with 5 mm of jaw contact on a 200 mm part will ring no matter what feed you pick. Support the part close to the cut, and where a thin floor is coming, back it with a soft jaw or a sacrificial plate.

For five-axis work, choose the smallest fixture that still reaches the part. A Ø400 mm rotary table gives plenty of room, but a long part hanging off the table needs a tailstock or a steady. Overhang beyond 2 × diameter on a small end mill is where deflection shows up as taper.

Thin walls are the classic failure. Below 1 mm on aluminium, add tabs, fill the cavity with low-melt wax, or leave a roughing rib that you cut away in the last pass. Do not try to solve wall chatter with a slower feed; it usually makes it worse.

Clamping force matters on soft materials too. Aluminium and copper deform under vise pressure. Use brass shims or torque the vise by feel, then check flatness after unclamping. If the part springs, the setup was too tight.

• 1
  Support near the cutJaw contact within 20 mm of the feature.
• 2
  Minimise overhangKeep tool stick-out under 4 × diameter.
• 3
  Thin wallsTabs, wax fill or a roughing rib.
• 4
  Soft metalsBrass shims, moderate clamp force.

Use the cutter maker's chart as a ceiling, not a target. For a 10 mm three-flute carbide end mill in 6061, a common start is 12,000 rpm, 0.08 mm feed per tooth and 3 mm axial depth. That gives a chip load the tool can actually cut instead of rub.

The three variables interact. If you raise spindle speed, raise feed per tooth with it, or the tool skates and work-hardens the surface. If you must lower feed because of a thin floor, lower rpm to keep the chip load constant rather than letting the tool dwell.

Radial engagement is the lever most people forget. A 10 percent step-over with full depth beats a 50 percent step-over with a shallow pass. High-efficiency toolpaths trade radial width for axial depth, which spreads heat and keeps the cutter in the cut longer.

Listen and look. Chips that are thin and silver mean the parameters are close. Blue chips or a high-pitched squeal mean heat and vibration. Stop, drop the rpm 10 percent, and check the tool edge before continuing.

• 1
  Start point10 mm 3-flute in 6061: 12,000 rpm, 0.08 mm/tooth.
• 2
  Link rpm and feedChip load stays constant when both move.
• 3
  Radial vs axialLow step-over with deep passes runs cooler.
• 4
  Read the chipsSilver and thin is good; blue means back off.

Check while the part is still clamped. Measure the first tight feature after roughing and again after semi-finishing. If the bore has drifted 0.01 mm, you can correct it with a spring pass before the finishing cut rather than scrapping the part.

Use the right tool for the size. A caliper reads ±0.02 mm at best, which is not enough for a ±0.005 mm bore. Use a bore gauge, a micrometer, or a CMM for anything tighter than ±0.02 mm. Record the reading and the ambient temperature; aluminium moves about 0.023 mm per metre per degree Celsius.

Final inspection should match the drawing's critical list, not every dimension. Report the tolerance-critical features, the surface finish, and any deviation from the model. On request we supply inspection reports with the shipment.

Finishing is the last step, and it is where parts get damaged. Deburr by hand before any coating. Sharp edges under a 0.2 mm chamfer can flake an anodised layer. Mask threads and bores that must stay conductive.

• 1
  Measure clampedCatch drift before the part comes off.
• 2
  Right instrumentBore gauge or CMM below ±0.02 mm.
• 3
  Report the critical listTolerance features and finish, not everything.
• 4
  Deburr firstSharp edges flake coatings.