Master CNC Machining 101

• 1
  What happens where the tool meets metal
• 2
  What 3, 4 and 5 axes each buy you
• 3
  Reading a tolerance block without over-specifying
• 4
  Material choice changes the whole process plan
• 5
  How a good shop controls the process
• 6
  Which setup fits which part

CNC machining is subtractive. A rotating cutter with defined edges enters the workpiece and shears material away as chips. The machine does not know what the part is. It follows coordinates from a G-code program, moving the spindle and table along axes while the tool turns at a set speed.

Three numbers control the cut. Surface speed is how fast the tool edge travels past the material, in meters per minute. Feed per tooth is how much material each edge bites off, in millimeters. Depth of cut is how far the tool buries itself. Get these right and chips leave the cut clean. Get them wrong and you hear it before you measure it.

The tool pushes material ahead of it, then shears it. A small amount of that material springs back against the flank of the tool. That springback is why a light finishing pass cuts more accurately than one deep roughing pass. It is also why a dull tool produces a larger hole than a sharp one.

Heat is the limiting factor. Most of the energy in a cut turns into heat, and the chip carries it away. If the chip is too thin, heat stays in the part and the tool. That is why an aggressive cut often runs cooler than a timid one. On aluminium such as 6061, cutters can run dry at high speed. On titanium TC4, coolant and lower surface speed are the norm.

A 3-axis machine moves X, Y and Z. The part stays in one orientation. Every face you cannot reach from the top needs a second setup, and every new setup adds a new datum error. On a simple bracket with two faces, that error is usually small enough. On a part with five angled faces, it stacks up fast.

A 4-axis machine adds rotation about one axis, normally A. The part turns while the tool cuts. This is the right answer for shafts, sleeves, cam profiles and anything with features distributed around a bore. A single setup covers all four sides, so concentricity stays where the turning left it.

A 5-axis machine adds a second rotary axis, so the tool can approach from almost any direction. Two variants exist. Table-table machines tilt the part. Spindle-tilt machines move the head. Both let you cut undercuts, deep pockets and contoured surfaces without re-fixturing. That matters most on parts with compound angles, impellers, and thin walls that would distort if moved.

More axes are not automatically better. A 5-axis cycle costs more per hour and needs more programming time. If a part fits in three setups on a 3-axis mill and the tolerance is loose, that is the cheaper route. We quote both when the geometry is borderline.

A general tolerance note of ±0.1 mm covers most of a drawing. Only the features that mate with something else need tighter numbers. When every dimension carries ±0.005 mm, the shop has to slow down, take more passes, and inspect more often. The price reflects that, and the gain is often zero.

±0.005 mm is achievable, but treat it as a per-feature callout, not a blanket note. It also depends on the feature. A bored hole Ø20 mm can hold it. A 300 mm long aluminium beam cannot, because thermal expansion alone moves the number. Aluminium grows about 23 μm per meter per degree Celsius. A 5 °C shop swing on a 1 m part is 115 μm.

Datums decide whether the tolerance is even measurable. If the drawing calls a hole position from a face that is never machined, the inspector has to guess. Pick machined faces as datums. This is the single most common cause of a part that measures in tolerance at the shop and out of tolerance at the customer.

Surface finish and tolerance travel together. A reamed hole at Ra 0.8–1.6 μm holds size better than a drilled one at Ra 1.6–3.2 μm because the finish pass removes the torn layer. For sealing faces, specify Ra 0.2–0.8 μm and expect a separate finishing operation in the routing.

Aluminium 6061-T6 is the default for prototypes and fixtures. It cuts fast, holds a good finish, and takes anodizing well. 7075 is stronger but more prone to stress movement after roughing, so we leave stock and take a second pass after a pause. 2024 behaves similarly and is common in aerospace brackets.

Stainless 303 machines cleanly and is the free-machining grade. 304 and 316 are tougher and work-harden if the tool rubs instead of cuts. Keep the feed per tooth up and never let the cutter dwell. 17-4PH in the H900 condition is often machined before aging, then heat treated, which avoids cutting at 40 HRC.

Titanium TC4 and Inconel sit at the other end. They conduct heat poorly, so the tool edge runs hot. Surface speed drops, coolant flow rises, and tool life shortens. These jobs are quoted with more cycle time and more tool changes, not because the geometry is harder but because the material is.

Finishing is a separate decision from machining. Anodizing adds a few micrometres and can round a sharp edge. Hardcoat anodizing builds about 50 μm and will close a tight tolerance if the drawing does not account for it. Laser marking needs a minimum character height of 1.5 mm. Call the finish on the drawing before the part is cut, not after.

Inspection is not a step at the end. Raw material arrives and gets checked against the cert. The first part off the machine is measured against the drawing before the run continues. In-process checks catch tool wear before it becomes a batch of scrap. Final inspection confirms the shipping parts match the first article.

Measurement equipment sets the ceiling on what a shop can prove. Calipers read to 0.02 mm. Micrometers and bore gauges read to 0.001 mm. A coordinate measuring machine reports position and form. If a drawing calls ±0.005 mm and the shop only has calipers, the number on the report is a guess. Ask what the inspection plan uses.

Certification matters when the part goes into a regulated product. ISO 9001 covers general quality management. IATF 16949 applies to automotive production. ISO 13485 applies to medical devices. ISO 27001 covers information security, which matters when the drawings themselves are confidential.

Every part we ship is inspected. Reports are available on request. For a program that runs to 10,000 pieces, the control plan includes a defined sample rate and a reaction plan if a trend appears. That is what keeps a qualification rate at 99.99% rather than a hopeful number.