CNC made parts: how stock removal sets tolerance and finish

• 1
  What actually happens when a cnc made part is cut
• 2
  Why ±0.005 mm is a process limit, not a wish
• 3
  Surface finish: what Ra actually costs
• 4
  Which shapes suit machining and which do not
• 5
  Material choice changes the cutting parameters
• 6
  Matching the feature to the right process call

A CNC machine does not shape metal. It removes it. A cutter with defined edges rotates at a set speed and travels along a programmed path, and the material left behind becomes the part. Everything else on this page follows from that one idea.

The cutter pushes against the workpiece with real force. A 16 mm end mill in 6061 aluminium might see 800 N of cutting force at a 3 mm depth of cut. That force goes into the part, the fixture, and the machine frame. If the part is thin, or held only at one corner, the metal deflects under load and springs back after the cutter passes. The dimension you measure afterward is not the dimension the toolpath asked for.

Heat is the second effect. Chips carry most of it away, but the cutting edge and the machined surface still rise in temperature. Aluminium can reach 200–300 °C at the edge without coolant. Steel cuts hotter. Thermal growth moves the part a few micrometres, then it shrinks back as it cools. On a ±0.005 mm callout, that movement matters.

So a cnc made part is the result of a mechanical system in balance: cutter, workpiece, fixture, and machine. Change any one of them and the numbers on the drawing shift. This is why a shop asks about wall thickness and fixturing before it quotes a tight tolerance.

• 1
  Cutting force deflects thin wallsBelow 1.5 mm wall thickness in aluminium, expect to add support or light passes.
• 2
  Heat moves the partCoolant and dwell time control thermal drift on tight bores.
• 3
  The fixture is part of the processA soft jaw or vacuum plate can matter more than the machine spec.

Tolerance is a budget, and every element in the machining system spends part of it. Machine positioning, spindle runout, tool wear, thermal drift, and fixturing error each take a slice. On a well-kept 3-axis mill, positioning alone can hold ±0.002 mm. Spindle runout adds 0.002–0.005 mm. Tool wear grows over a run. By the time you finish, ±0.005 mm is realistic only when the geometry is simple and the setup is rigid.

That is the number we hold on production parts: ±0.005 mm, or ±0.0002 in. It is achievable on bores, flats, and slots where the cutter approaches from one direction. It is not achievable on a deep pocket with a 4:1 depth-to-diameter ratio, because the tool shanks deflect. Nor is it achievable on a long, slender shaft held at one end, because turning force bends it.

Here is the part most drawings get wrong. A tolerance is only meaningful if the feature can be measured. If a callout references a datum face that the setup cannot reach, or a true position on a hole pattern that sits on a curved surface, the inspection result becomes a debate. We ask for the functional requirement instead: which surfaces mate, which holes take a pin, which face seals.

General tolerances also cost differently from local ones. A drawing that states ±0.1 mm everywhere and ±0.005 mm on two bores is cheaper than one that states ±0.005 mm globally. The shop can run normal passes over most of the part and slow down only where it matters. Tightening a tolerance you do not need is the most common way to double the price of a cnc made part.

• 1
  Tight where it functionsReserve ±0.005 mm for mating and locating features only.
• 2
  Loosen the restTitle-block tolerances of ±0.1 mm keep cycle time down.
• 3
  Check the datum is reachableIf the CMM cannot touch it, the callout is unenforceable.

Surface finish on a cnc made part comes from the toolpath, not from a coating. A standard carbide end mill at a 0.05 mm feed per tooth leaves a scallop pattern that measures around Ra 1.6–3.2 μm as machined. That is fine for brackets, housings, and most internal parts. It is not fine for a seal face or a sliding bore.

To reach Ra 0.8–1.6 μm, the shop reduces feed per tooth and increases spindle speed, then often adds a finishing pass with a smaller stepover. Cycle time rises, sometimes by 20–40 percent on the finished area. To reach Ra 0.2–0.8 μm, you need a dedicated finishing pass with a small-nose or wiper insert, or a secondary operation such as lapping or fine grinding. At that level, inspection moves from a visual check to a profilometer.

Coating and blasting change appearance but not the underlying Ra. Anodizing adds 5–15 μm of oxide on aluminium and can round a sharp edge. Bead blasting produces a matte surface around Ra 1.6–3.2 μm and hides tool marks, which is why it is popular on visible parts. Polishing removes material, so never specify it on a feature with a tight tolerance unless the shop knows to leave stock.

The practical rule: pick the coarsest finish that meets the function. A Ra 0.8 μm seal face and a Ra 3.2 μm bracket can come off the same machine in the same setup, and only the seal face needs the slow pass.

• 1
  As machinedRa 1.6–3.2 μm. Default for structural and internal parts.
• 2
  Fine finishRa 0.8–1.6 μm. Seal faces, sliding surfaces, visible panels.
• 3
  Precision finishRa 0.2–0.8 μm. Needs a finishing pass or secondary operation.

A CNC cutter is a rotating cylinder. It reaches along its axis and from the side, but it cannot turn a corner inside a closed pocket. That geometry rule decides most feasibility questions. A pocket with a sharp internal corner needs a cutter radius, so the drawing should specify the corner radius the tool leaves, typically 0.5–3 mm depending on depth.

Undercuts and internal channels are the classic problem. If a feature sits behind a lip and no tool can approach it from any direction, it cannot be machined without a special tool or an EDM step. Cross-drilled holes that meet inside a part are fine. A curved internal passage with a 90° bend is not. The same applies to features on the back of a part that is too large to flip in the work envelope.

Five-axis machining removes many of these limits. With 16 simultaneous 5-axis centers, we can tilt the tool and reach angled faces, deep cavities, and complex contours in one setup. That cuts repositioning error and often removes a second operation. It does not remove the physics: a tool still needs clearance, and a cavity still needs an entry path.

Size sets the outer boundary. Our largest travel is 4,000 × 400 × 150 mm, and we also run 750 × 1,150 × 550 mm and 600 × 600 × 600 mm envelopes. Parts beyond those limits need to be split and joined, which changes the design, not just the process.

• 1
  Internal corners need a radiusMatch the drawing radius to the cutter you can afford.
• 2
  No blind undercutsIf no tool can approach it, add an EDM step or redesign.
• 3
  Check the work envelope earlyMax processing size is 4,000 mm on our largest machine.

Aluminium is the default for cnc made parts because it cuts fast and holds tolerance well. Grades 6061 and 6061-T6 cover most brackets, housings, and fixtures. 7075 machines to a better finish and takes higher stress, but it costs more and can distort after heavy stock removal. 2024 is strong and machines cleanly, though it needs a coating for corrosion. Cast grades such as ADC12 behave differently and often need a slower feed.

Stainless steel is where cycle time jumps. 303 is the free-machining grade and the easiest to run. 304 and 316 are tougher, work-harden if the cutter dwells, and need sharp tools and steady feed. 17-4PH holds strength after heat treatment and is common in aerospace and medical work. If a part needs both corrosion resistance and a tight bore, 316L is usually the right call, though expect longer lead time on the finishing pass.

Titanium and Inconel sit at the hard end. TC4 (Ti-6Al-4V) has low thermal conductivity, so heat stays in the cutting edge. Tool life drops, feeds slow down, and cost rises accordingly. Magnesium AZ31B and AZ91D cut very fast but need chip control because fine magnesium dust is a fire risk. We machine them, but the setup rules are strict.

Plastics behave like a separate process. POM and ABS cut cleanly. PEEK holds dimension at high temperature and is common in medical and semiconductor parts, but it is expensive and abrasive on tools. Carbon fibre needs diamond-coated tooling and dust extraction. The material choice is usually made for function first, then we adjust parameters around it.

• 1
  Aluminium 6061-T6Default for most structural and enclosure parts.
• 2
  Stainless 303 vs 316L303 for machinability, 316L for corrosion and medical use.
• 3
  Titanium TC4Low thermal conductivity, short tool life, higher cost.
• 4
  PEEK and carbon fibreFunction-driven choices with special tooling needs.