What Should Be Checked Before CNC Machining?

• 1
  Why geometry is checked before CNC machining
• 2
  Material and stock form are checked before CNC machining
• 3
  Datum strategy checked before CNC machining
• 4
  Tolerances and finish checked before CNC machining
• 5
  Tooling, fixtures and quantity checked before CNC machining
• 6
  Inspection and documentation checked before CNC machining
• 7
  Six checks and what each one protects

The first thing checked before CNC machining is whether the tool can actually reach the feature. A pocket with a 3 mm internal corner and a 20 mm deep wall needs a cutter no larger than 6 mm, and that cutter has an effective length-to-diameter ratio near 6:1. It will deflect. The drawing looks fine. The cut does not.

We read the model against the machine travel. Our largest envelope is 4,000 × 400 × 150 mm. A part that fits the table but needs a 5-axis tilt at the end of a long overhang is a different problem from one that fits in a 500 × 500 × 450 mm envelope. Setup access matters more than raw size.

Sharp internal corners are the most common DFM flag. If the corner radius is smaller than the smallest cutter that can reach the depth, you have three options: add a relief, accept a larger radius, or plan EDM. Two of those change the drawing. One changes the process. Say which one you want before the job is quoted.

Thin walls deserve the same treatment. A 0.8 mm wall on a 60 mm tall aluminium pocket will sing and move under cutting force. We check wall height against thickness. Ratios above roughly 15:1 usually need a support rib, a softer step-down, or a redesign.

• 1
  Corner radiusKeep internal radii at least one third of pocket depth where possible.
• 2
  Tool reachAspect ratios above 6:1 invite chatter; plan a shorter cutter or a stepped setup.
• 3
  Wall thicknessBelow 1 mm on tall walls, expect deflection without support.

Material grade changes cutting data, and cutting data changes cost. 6061-T6 aluminium machines at 3,000–6,000 rpm with light radial passes and runs clean. 7075 is stronger and gummier; it needs sharper tools and lower feed per tooth. 304 stainless work-hardens if the cutter rubs, so we keep the feed high enough to stay under the hardened skin.

Stock form matters as much as grade. Bar stock, plate and near-net forging all cut differently. A part hogged from 100 mm plate wastes material and time. A forging that is 2 mm oversize on a critical face saves both. For titanium and Inconel parts, the buy-to-fly ratio often decides the quote more than the machining itself.

Heat treatment and stress relief belong on the checklist too. Machining a plate that was not stress-relieved will release internal stress as you remove material, and the part moves after the final pass. If flatness is tight, specify stress-relieved stock or plan a rough-mill, stress-relieve, finish sequence.

We check whether the material is available in the size and grade specified. Substituting a grade without approval is not a decision a machine shop should make. If 6082 is in stock and 6061 is on a four-week lead, that is your call, not ours.

• 1
  Grade and temperT6, T4 and annealed stock machine differently; specify one.
• 2
  Stock formPlate, bar and forging each change setup count and material cost.
• 3
  Stress reliefUnsuitable for tight flatness without a rough and finish split.

A datum is the surface the inspector trusts. If the drawing does not name one, the machinist picks it, and the inspector may pick a different one. That is how a part passes the machine and fails the CMM. Before cutting, we confirm which faces are functional datums and whether they can be machined in the same setup as the features they locate.

The best datum is usually a face that is flat, accessible and already machined in the first operation. Locating on a raw casting surface adds variation. Locating on a face that gets milled later means the datum itself moves between operations. Both are workable if the drawing says so. Neither works if the drawing stays silent.

For parts with a tight position tolerance between two features, we prefer to machine both in one setup. Every re-fixture adds stack-up. On a 4-axis or 5-axis machine, we can often reach five faces from one clamp. That removes one datum transfer and one chance for error.

If the part is a weldment or an assembly, the datum question grows. We check whether the drawing controls the final assembly or the individual components. Tolerance applied at the wrong level either over-constrains the shop or leaves the functional fit uncontrolled.

• 1
  Name the datumOne primary flat face is enough for most parts; add secondary and tertiary only if needed.
• 2
  Same-setup featuresKeep tightly related features in one operation where the machine allows.
• 3
  Assembly levelState whether tolerances apply to parts or to the finished assembly.

Tolerance drives process, and process drives price. A general block tolerance of ±0.1 mm on a milled aluminium bracket is routine. A ±0.005 mm callout on the same bracket means grinding, temperature control and a slower cycle. Both are achievable here. They are not the same job.

We check whether tight tolerances are functional or inherited. Blanket ±0.01 mm on every dimension is a common habit from CAD templates. It triples inspection time and adds no value to features that only need clearance. If a slot holds a bearing, tolerance it. If it vents air, do not.

Surface finish follows the same logic. As-machined aluminium sits around Ra 1.6–3.2 μm. A fine finish of Ra 0.2–0.8 μm needs a different tool path, sometimes a different tool, and always more time. Deep pockets and internal bores are the hardest places to hold a fine finish, because the cutter has to reach and clear chips.

Threads, fits and callouts deserve a separate pass. We confirm thread class, whether the thread is milled or tapped, and whether a counterbore has clearance for the fastener head. A missing counterbore depth is a ten-second question at quote time and a scrap part at delivery.

• 1
  Tolerance by functionApply tight limits only where the fit or seal requires them.
• 2
  Finish by surfaceExternal faces reach fine finishes more easily than deep bores.
• 3
  Fastener clearanceCheck counterbore depth and head clearance on the model, not on the print.

Quantity decides tooling. One prototype and a 10,000-part run are different economic problems. For a single part, soft jaws and a vise are enough. For a run, a dedicated fixture pays for itself in cycle time and repeatability. The crossover usually sits somewhere in the low hundreds, depending on part complexity.

We check whether the part can be held without distorting it. A thin ring clamped in a three-jaw chuck will be round when clamped and oval when released. A vacuum plate or a purpose-built nest fixes that. Clamping force is a real variable, and it shows up as a roundness error on the inspection report.

Special cutters take time to arrive. A form tool or a custom reamer adds days to the front of the schedule. When we review a job, we flag any feature that needs non-standard tooling so the lead time is known before the order is placed, not after.

For 5-axis work, we check whether the part needs simultaneous motion or just positional indexing. Positional 3+2 work is faster to program and easier to verify. Simultaneous 5-axis is for contoured surfaces and undercuts that no indexed setup can reach. Choosing the wrong one wastes either capability or money.

• 1
  Soft jaws vs. fixtureBelow a few hundred parts, soft jaws usually win on cost.
• 2
  Clamping distortionThin rings and thin plates need low-stress workholding.
• 3
  Special toolingCustom cutters add lead time; raise them at quote, not at first cut.

Before the first chip, we agree on what gets measured and how. A first article inspection report on the critical dimensions costs little when planned up front. Reconstructing the measurement plan after the parts are made costs a lot, especially if the customer's inspection method differs from the shop's.

We check whether the drawing calls out a CMM report, a material certificate or a certificate of conformance. These are routine here. ISO 9001:2015, IATF 16949:2016, ISO 13485:2016 and ISO 27001:2022 cover quality, automotive, medical and information security respectively. If your industry needs a specific record, name it on the purchase order.

Sampling matters as much as method. We run 100% inspection before shipment, with raw material checks, in-process monitoring and a final pass. For high-volume runs, in-process gauging at the machine catches a drift before it becomes a batch of out-of-tolerance parts.

Finally, we check traceability. If a part goes into an automotive or medical assembly, the material lot and the machine record may need to follow it. That is a documentation task, not a machining task, and it has to start at the raw material receiving dock.

• 1
  First articleAgree the critical dimensions before the first cut, not after.
• 2
  CertificatesMaterial certs and C of C are available on request.
• 3
  TraceabilityAutomotive and medical parts may need lot-level records.