Precision CNC machining Berkshire: how metal removal really works

• 1
  What precision CNC machining Berkshire shops actually control
• 2
  How the tool edge removes material, and why that sets tolerance
• 3
  Where ±0.005 mm holds, and where it does not
• 4
  Surface finish is a separate decision from tolerance
• 5
  Material choice drives the process more than the drawing does
• 6
  Setup count and part quantity decide the real cost
• 7
  Which machine class fits your part

Precision CNC machining is not one operation. It is a chain of decisions: which spindle, which tool, which fixture, which pass depth. Each decision moves the part closer to or further from the drawing. When a UK engineer sends a drawing to us in Dongguan, the first question is never about tolerance. It is about how the part will be held while the tool pushes against it.

A three-axis mill moves the cutter along X, Y and Z only. That covers a lot of work: plates, brackets, housings with features on one face. The part is repositioned by hand or in a vise between setups. Every repositioning adds error. Two setups double the chance of a stack-up, and a 0.02 mm shift between faces is normal on a manual flip.

Four-axis machining adds rotation around one axis, usually A or B. The workpiece turns while the tool stays in position. Holes on a cylinder, slots around a shaft, or features on four faces of a prismatic block can be cut without re-clamping. Positional error between faces drops because the datum never moves.

Five-axis adds a second rotation. The tool can now approach the part from almost any direction, and the table tilts to keep the cutter normal to the surface. That is what makes undercuts, deep pockets with drafted walls, and contoured impeller blades machinable in one setup. It also means fewer fixtures, which is often worth more than the tighter tolerance.

• 1
  Three-axisFlat faces, through holes, simple pockets. Lowest cost per part.
• 2
  Four-axisCylindrical and multi-face parts, one rotation axis.
• 3
  Five-axisUndercuts, 3D contours, one-setup complex geometry.

Every cut is a controlled fracture. The edge pushes into the workpiece, the material shears along a plane ahead of the tool, and a chip slides up the rake face. Heat leaves with the chip. If the chip is too thin, the edge rubs instead of cutting, and the surface tears. If the chip is too thick, cutting force spikes and the part deflects.

Chip load per tooth is the number to watch. In aluminium 6061, a 10 mm carbide end mill typically runs 0.05–0.15 mm per tooth at 300–500 m/min surface speed. Drop below roughly 0.02 mm per tooth and you are burnishing, not cutting. The finish may look good, but tool life falls and the subsurface work-hardens.

In stainless 304 or 17-4PH, the same cutter runs far slower, often 60–120 m/min, with 0.03–0.08 mm per tooth. Stainless work-hardens fast, so the edge must stay sharp and the feed must stay high enough to bite under the hardened layer. A dwell in the cut is what kills the insert.

Titanium TC4 (Ti-6Al-4V) is worse on both counts. Thermal conductivity is low, so heat stays in the edge. Cutting speeds drop to 40–60 m/min and coolant must reach the tip, not just the part. This is why titanium parts cost more per cubic centimetre removed, regardless of geometry.

• 1
  Chip too thinRubbing, work hardening, poor finish.
• 2
  Chip too thickDeflection, chatter, tool breakage.
• 3
  Right windowStable force, heat leaves with the chip.

We hold ±0.005 mm on turned and milled features when the part is rigid, the material is stable, and the feature is reachable in one setup. A 30 mm aluminium shaft turned in a collet is easy. A 4,000 mm long aluminium extrusion is not. Length is the enemy: thermal expansion of aluminium is about 23 μm per metre per degree Celsius, so a 2 °C shop swing moves a 1 m part by 0.046 mm.

Thin walls are the second limit. Below roughly 1 mm wall thickness in aluminium, cutting force pushes the wall away from the tool, then it springs back. The cut is undersized and the wall is tapered. We usually rough with a light radial step-over, leave 0.3–0.5 mm, then finish in two passes with a sharp cutter and air blast to clear chips.

Deep pockets with small tools are the third. A 3 mm end mill reaching 20 mm deep has an aspect ratio near 7:1. Deflection at the tip can exceed the tolerance on its own. Options are a shorter reach, a relieved shank, or high-speed machining with small step-over and reduced radial load.

Tolerance also depends on measurement. A micrometer on a curved surface reads a chord, not a diameter. A CMM with a 2 mm stylus cannot enter a 3 mm slot. When a drawing calls for ±0.005 mm, we need to know which feature matters and how it will be verified at goods-in.

• 1
  Rigid, short, one setup±0.005 mm is routine.
• 2
  Long or thinExpect ±0.02 mm unless the process is controlled.
• 3
  Small deep featuresTool deflection, not machine error, sets the limit.

Ra is an average roughness, not a peak-to-valley figure. A surface can read Ra 0.8 μm and still have a 6 μm scratch that fails a seal. If the part has an O-ring groove or a sliding bore, specify Rz or Rmax as well. Otherwise the number on the drawing does not describe the surface the seal touches.

As-machined aluminium from a sharp carbide cutter lands around Ra 1.6–3.2 μm. That is fine for brackets and covers. A finer pass with a smaller step-over and a wiper insert reaches Ra 0.8–1.6 μm on flat faces. Below that, on most metals, you are looking at lapping, polishing or a coated insert run at reduced feed.

We can hold Ra 0.2–0.8 μm on sealing faces and bearing bores when the geometry allows a finishing pass with a rigid setup. The cost is time. A mirror finish on a 100 mm face may take longer than the roughing and semi-finishing combined. Ask whether the function needs it.

Two other finishes are easy to confuse. Bead blasting hides tool marks and gives a matte look, but it can round a sharp edge. Anodizing adds a layer, typically 5–25 μm, and that layer grows outward and inward. A ±0.01 mm bore becomes smaller after hardcoat. Tell us the finish before we cut the feature.

• 1
  Ra vs RzSeals and bearings need peak values, not averages.
• 2
  Coating growthAnodizing shifts dimensions; plan the allowance.
• 3
  BlastingHides marks, breaks sharp edges.

Aluminium 6061-T6 is the default for machined parts because it cuts fast, holds tolerance well, and takes anodizing cleanly. 7075 is stronger but gummier and more prone to stress movement after heavy stock removal; parts with tight flatness usually need a stress-relief cycle between roughing and finishing.

Stainless 303 machines freely because of its sulfur content, which is why it is common for shafts and fittings. 304 and 316 weld and resist corrosion better but machine slower and work-harden. 17-4PH gives high strength after aging, and it is the usual pick for aerospace brackets and medical instruments that need both.

Titanium TC4 and Inconel sit at the hard end. Heat stays at the edge, tool life is short, and the cycle is long. For these, the design decision that matters most is access: can the tool reach every feature from a stable direction? If not, the part may need five-axis work or a redesign.

Plastics behave differently again. POM and PEEK cut cleanly but move with temperature. A PEEK part machined at 25 °C can shrink measurably when it cools after the cut. For thin plastic parts, we rough, let the part rest, then finish. It costs a day and saves the part.

• 1
  6061-T6Fast, stable, anodizes well. Default for housings.
• 2
  303 vs 316303 for machinability, 316 for corrosion.
• 3
  TC4 / InconelSlow speeds, short tool life, design for access.

A single prototype on a three-axis mill may take three setups and two hours of fixturing. The same part on a five-axis center, with a Ø400 mm rotary table, may take one setup and twenty minutes of fixturing. The machine rate is higher, but the total is often lower. This is the trade most buyers miss.

For one to fifty parts, fixtures are usually soft jaws, a vise, or a vacuum plate. For hundreds to thousands, a dedicated fixture or a tombstone pays back quickly. A tombstone on a four-axis mill lets you load four or eight parts per cycle and cut while you load the next set.

In-process probing changes the picture. A touch probe can find the datum on each part, compensate for casting variation, and record the result. On castings and forgings with ±0.5 mm stock variation, probing is often the difference between a scrap rate of a few percent and a rate near zero.

We run 127 high-precision CNC machines across three wholly-owned plants, 7,600 m² total, with 16 simultaneous five-axis centers, 12 four-axis mills, 27 three-axis machines and 16 mill-turn centers. Maximum processing size is 4,000 mm. That mix matters: the right machine class for the geometry, not the biggest one.

• 1
  1–50 partsSoft jaws and vises; keep fixture spend low.
• 2
  500+ partsDedicated fixture or tombstone pays back.
• 3
  CastingsProbe each part; stock varies.