CNC processing requirements: what the machine needs from your drawing

• 1
  What CNC processing requirements actually mean on the shop floor
• 2
  Datum strategy and setup count drive the whole process
• 3
  Wall thickness, floor thickness, and tool reach limits
• 4
  Tolerance stack and where ±0.005 mm is realistic
• 5
  Material choice changes the requirements, not just the feed rate
• 6
  Inspection gates and the reports that come with the parts
• 7
  Which machine and setup the part shape calls for

A drawing says Ø40 h7, Ra 0.8, and 316L. That is geometry, not a process. CNC processing requirements are the extra conditions that let a machinist turn that geometry into a repeatable part: where the part is held, how much material is left after each pass, which surfaces get cut in the same setup, and how the finished feature will be measured.

These conditions rarely appear on the print. They come from the interaction between the part shape and the machine envelope. A 4,000 mm rail and a 12 mm bracket have almost nothing in common as processing problems, even when both carry the same tolerance callout.

Get them wrong and the failure is quiet. The first article passes. The tenth part drifts. By the time the CMM catches it, half a batch is scrap. Most of the cost sits in that gap, not in the cutting itself.

This page covers the requirements we check before releasing a program: datum strategy, setup count, wall and floor limits, tool reach, tolerance stack, and inspection gates. Each section states when the rule applies and when it can be relaxed.

Every re-clamp adds error. A part cut in three setups carries three times the locating error of the same part cut in one. On a 5-axis center, a single setup can reach five faces, which removes the re-clamp entirely. That is the main reason we quote complex housings on 5-axis rather than three orthogonal 3-axis operations.

The datum on the drawing and the datum on the fixture must be the same feature. If the print calls out a bore as datum A but the fixture clamps on the outer profile, the tolerance chain absorbs the offset between them. It works until the profile runs out of true.

Rule of thumb: pick a datum that can be probed in the same setup that cuts the critical feature. A flat face plus two dowel holes is easier to hold than a curved surface. Curved datums require a custom soft jaw, which adds lead time and cost.

When the part is thin or flexible, the clamping force itself becomes a processing requirement. We machine with light passes and support the web from below. A part that measures true on the machine can spring back once the vise opens, so inspection has to happen in the free state.

• 1
  One setup when possibleFewer re-clamps mean less stacked error.
• 2
  Probe the datum you cutKeeps print and fixture aligned.
• 3
  Flat datums over curvedNo custom soft jaws, faster setup.
• 4
  Inspect free-state for thin partsClamping masks spring-back.

Aluminium 6061 machines cleanly down to a 0.5 mm wall if the wall is short and supported. Stretch that wall past roughly ten times its thickness and it will chatter or deflect, no matter how sharp the cutter is. Titanium and 17-4PH are less forgiving; we treat 1.0 mm as the practical floor for unsupported walls in those materials.

Floor thickness follows the same logic. A 1.5 mm floor in a 40 mm deep pocket is a drum. It will ring under the cutter and may bow after stress relief. Adding a rib or leaving a temporary boss that gets removed later is often cheaper than fighting the vibration.

Tool reach sets the depth you can actually cut. A Ø6 mm end mill has an effective reach of about 30 mm before deflection ruins the finish. Deeper pockets need either a reduced neck tool with light radial engagement or a larger cutter, which may not fit the corner radius.

Check the corner radius against the tool library before releasing the model. A pocket with a 1 mm internal corner forces a Ø2 mm cutter. That cutter cannot clear a 50 mm deep pocket at production feed rates. Redesign the corner to R3 or accept a much slower cycle.

±0.005 mm is achievable on our 5-axis centers, but not everywhere on every part. It applies to a specific feature measured in a controlled setup, at 20 °C, with a probe or CMM. Apply it to a 600 mm span and thermal growth alone will eat the budget.

The practical split is simple. Critical mating features get the tight callout. Clearance holes, fillets, and non-functional surfaces stay at general tolerance. A drawing where every dimension is ±0.005 mm costs more and produces no better part.

Stack the tolerances before you release. If three features each carry ±0.05 mm and they chain into a single fit, the assembly sees ±0.15 mm worst case. Fix the chain on the drawing, not on the machine.

Surface finish and tolerance are linked. Holding Ra 0.8 μm on a deep bore needs a reaming or boring pass, not a finishing end mill. That extra operation changes the setup plan and the cycle time, so it belongs in the requirements from the start.

6061-T6 cuts fast and holds size well. 7075 is stronger but more prone to stress movement after heavy stock removal, so we rough, let it rest, then finish. 316L work-hardens at the cut, which means the tool must stay engaged and never rub.

Titanium TC4 (Ti-6Al-4V) and Inconel push the requirements further. Heat concentrates at the edge, so coolant delivery and tool path matter more than raw spindle speed. Wall thickness limits tighten and cycle times roughly double against aluminium.

Plastics behave differently again. POM and PEEK move with temperature, so a tight tolerance measured hot will not hold cold. We cut them with sharp, polished tools and let the part stabilize before final inspection.

The material list we run covers aluminium 6061, 2024, 5052, 7075 and ADC12; stainless 303, 304, 316L, 17-4PH; steels 1018, 1045, 4140 and 4340; copper and brass grades; and engineering plastics from ABS to PEEK. Each has its own wall and finish limits.

Inspection is a processing requirement, not a final step. We check raw material certificates on arrival, monitor critical dimensions in process, and run 100% inspection before shipment. Reports are available on request.

The in-process check matters most on tight-tolerance features. Waiting until the part is finished means the error is already cut into every piece behind it. A probe check after the first article and every twenty parts catches drift before it becomes scrap.

For regulated work, the quality system behind the inspection is part of the requirement. We operate under ISO 9001:2015, IATF 16949:2016, ISO 13485:2016, and ISO 27001:2022, which covers automotive, medical device, and information security expectations respectively.

Our measured qualification rate is 99.99%. That number comes from the inspection gates above, not from tighter tolerances on the print. If your drawing needs a first article report or full dimensional layout, say so at quoting so the inspection plan includes it.