Medium CNC Machining: How Mid-Size Parts Are Cut

• 1
  What counts as medium in medium CNC machining
• 2
  Why 3-axis runs out of room and 5-axis takes over
• 3
  Fixtures and thermal drift decide the tolerance
• 4
  How material changes the cut on mid-size parts
• 5
  How to inspect a medium part without arguing
• 6
  Which setup fits which medium part

There is no standard definition. In our shop, medium starts where a benchtop mill runs out of travel and ends where the part needs a bed long enough to sag under its own weight. In practice that is roughly 300 mm to 1,200 mm in the longest dimension, and 20 kg to 400 kg in mass.

That band is awkward. Small parts sit in a vise, get cut dry, and hold ±0.005 mm without much thought. Very large parts get planned around from the first drawing. Medium parts look easy on paper and then fight you on the floor. A 600 mm aluminum plate expands about 0.014 mm for every 1 °C it warms up. Cut for two hours and the part is a different size than the one you probed.

So the question is not only which machine. It is which machine, which fixture, and which inspection point in the thermal cycle. Medium CNC machining is mostly a scheduling and setup problem wearing a machining costume.

Travel numbers matter more here than spindle speed. A 750 × 1,150 × 550 mm travel covers most brackets, housings, and manifolds in one setup. A 4,000 mm bed covers long beams and rails, but the part may need support every 800 mm to stop chatter.

• 1
  Typical medium envelope300–1,200 mm longest dimension, 20–400 kg
• 2
  Tolerance target±0.005 mm is reachable, but only with temperature control
• 3
  Main riskThermal drift and fixture deflection, not spindle capability

A 3-axis machine can cut a medium part well if every feature is reachable from the top. Add a side hole pattern at an angle, or a pocket that needs a long tool to reach 400 mm deep, and the setup count climbs. Each new setup adds a re-clamp, a new datum, and a fresh chance for error.

Five-axis simultaneous cutting removes most of that. The tool stays normal to the surface, so a Ø12 mm end mill can cut a curved wall instead of a Ø6 mm tool leaving scallops. Shorter tools mean less deflection. On a 500 mm deep pocket, the difference between a 4:1 and an 8:1 length-to-diameter ratio is often the difference between Ra 1.6 μm and Ra 3.2 μm.

It is not free. Five-axis programming takes longer, and the machine is slower to set up. For a flat plate with holes on one face, 3-axis is cheaper and just as accurate. For a housing with angled ports, blended radii, and a bore that must stay concentric to a face 600 mm away, 5-axis usually wins on total cost.

Our 16 simultaneous 5-axis centers handle medium parts in one or two setups. The rotary table is Ø400 mm, which sets the practical limit for parts that need full rotation. Beyond that, parts move to a 4-axis horizontal or get split across setups.

• 1
  Use 3-axis whenAll features face one direction, part is under 400 mm
• 2
  Use 4-axis whenCylindrical or rotary features, one index axis is enough
• 3
  Use 5-axis whenAngled faces, deep pockets, or tight concentricity across the part

A 300 kg steel block clamped on four corners will bow. The middle lifts, the cut measures correct on the machine, and the part springs back after unclamping. This is the most common failure in medium CNC machining, and it does not show up until final inspection.

The fix is not a bigger vise. It is a fixture that supports the part where the cutting forces push. Vacuum plates work well for thin aluminum up to about 25 mm thick. Tombstones and modular fixturing suit prismatic parts. For castings and weldments, we often rough, stress-relieve, then finish, so the part relaxes before the last pass.

Thermal drift runs in parallel. A spindle running at 12,000 rpm for an hour can move the head 0.02 mm. Coolant at 20 °C helps, but the part itself warms from the cut. On a 1,000 mm aluminum part, a 5 °C rise is about 0.07 mm of growth. That is 14 times our tolerance. So we probe, cut, and probe again, and we keep the shop at 20 ± 2 °C for tight work.

In-process probing catches both problems. If the probe says the bore moved 0.03 mm between roughing and finishing, we adjust the offset instead of scrapping the part. On a 10,000-piece run, that is the difference between 99.99% and a pile of rework.

• 1
  Support under the cutNot just at the corners
• 2
  Stress-relieve castingsRough, relieve, then finish
• 3
  Probe in-processCatch drift before the finish pass

Aluminum 6061 and 7075 cut fast and hold tolerance well, but they move. A 600 mm 7075 plate can warp 0.2 mm after face milling if the residual stress is uneven. We rough with 2 mm stock, let it sit, then finish. For thin walls under 3 mm, we climb-mill with a high-helix cutter and light radial engagement.

Stainless 304 and 17-4PH work-harden. On a medium part, a deep pocket in 304 needs constant feed, no dwell, and sharp tools. Stop in the cut and the surface hardens, then the next pass chips the edge. 17-4PH in the H900 condition is easier to finish but harder on inserts.

Titanium Ti-6Al-4V and Inconel 718 are where medium parts get expensive. Both hold heat, so the tool edge sees 800 °C or more. Cutting speeds drop to 30–50 m/min for titanium and 20–30 m/min for Inconel. Rigidity matters more than speed. A 400 mm long tool in Inconel will chatter no matter what the speeds and feeds say.

Plastics like PEEK and POM are simpler to cut but harder to hold. They expand with heat and clamp marks show. We use sharp single-flute cutters, air blast instead of flood coolant, and soft jaws. For carbon fibre, dust extraction and diamond-coated tools are not optional.

• 1
  AluminumRough, relax, finish to control warp
• 2
  StainlessNever dwell in the cut
• 3
  Titanium and InconelRigidity first, then speeds and feeds

A caliper is not enough. A 1,000 mm part needs a CMM or a laser tracker, and the measurement has to happen at a known temperature. If the part is 22 °C and the drawing assumes 20 °C, a 1,000 mm aluminum dimension reads 0.05 mm long. That is within our tolerance, so we record temperature with every inspection.

Datum choice matters more than the instrument. If the drawing calls out datum A on a face that gets machined in setup two, the inspector has to trust setup one. We prefer to machine datums first and protect them. On parts with a bore and a face, we check concentricity with a mandrel and indicator, not by measuring the bore diameter alone.

For medium runs, we inspect the first article fully, then sample at intervals. Every part gets a final check before shipment. Reports are available on request. If a customer needs PPAP or full dimensional reports, we build that into the process plan from the quote stage.

The 99.99% qualification rate we quote comes from this loop: probe in-process, measure at temperature, and correct the offset before the finish pass. It is not a claim about the machine alone.

• 1
  Record temperatureWith every critical measurement
• 2
  Machine datums firstThen protect them through the setups
• 3
  First article, then sampleFull inspection before shipment