CNC Machining Design Guide: DFM Rules from the Shop Floor

End mills are round, so internal vertical corners will always carry a radius. The mistake is making that radius unnecessarily small.

• Default rule: make internal corner radii at least 1/3 of the pocket depth — and larger if you can.
• Bigger radius = bigger tool = faster cutting. A pocket finished with a 1/2 in (12 mm) end mill costs a fraction of the same pocket finished with a 1/8 in (3 mm) tool.
• Radii smaller than 0.5× depth force long-reach tools, which deflect, chatter, and leave worse surface finish — while tripling cycle time.
• Don't call out "sharp corners" unless the function truly needs them. Sharp internal corners require EDM or broaching, which is a different price bracket entirely.

If a mating part has a square edge, relieve the corner with an undercut (dogbone or corner relief) instead of demanding a sharp internal corner.

For pockets, cavities, and drilled or reamed holes, tooling gets fragile fast past certain depth ratios:

• Pockets: keep depth under 4× the corner radius where possible. Deeper pockets need stepped-down tool diameters and multiple tool changes.
• Drilled holes: standard drills run comfortably to 5× diameter. Past 10× diameter you're in deep-hole drilling territory — peck cycles, specialized tooling, slower everything.
• Blind holes: leave drill-point allowance at the bottom. A flat-bottom blind hole needs a secondary operation; call it out only if it matters.

If you genuinely need a deep cavity, consider whether the part should be two pieces bolted or bonded together — it's often half the price.

Blanket tolerances are the most expensive line on most drawings. Our standard is ±0.005 in (±0.13 mm) on general features, with ±0.001 in (±0.025 mm) held on critical bores, datums, and mating features — quoted against the drawing.

A tolerancing strategy that saves real money:

1. Set the title-block tolerance loose — ±0.010 in or even ±0.020 in where cosmetics allow.
2. Tighten individually the dimensions that actually locate, seal, or mate.
3. Use datums and true position (GD&T) for hole patterns instead of tightening every linear dimension — it's clearer to inspect and often cheaper to hold.
4. Never tighten a tolerance "just to be safe." Every step tighter roughly adds inspection and process time; ±0.001 in features get CMM-verified on our side, which is exactly what you want for critical dimensions — and exactly what you don't want to pay for on a cosmetic cover.

See our tolerance standards for what we hold by default.

Every setup adds cost and stacks tolerance error. Help the machinist help you:

• Give us a clamping surface. Parts that are all finished surfaces and curves force custom soft jaws or fixtures — fine at volume, painful at prototype quantities.
• Consolidate features onto as few faces as possible. A part machined in two setups beats one needing five.
• Compound-angle features across multiple faces may route to 5-axis machining, which often costs less than multiple 3-axis setups — flag complex geometry in your RFQ and we'll route it correctly.
• Tool access:a feature a cutter can't reach straight-on needs special tooling or another setup. If a pocket wall blocks tool access to a hole, move the hole or open the wall.

Before you submit, run this list:

• ✓STEP file and 2D drawing at the same revision
• ✓Material specified to grade and temper (e.g., 6061-T6, not "aluminum")
• ✓Title-block tolerance as loose as function allows; critical dimensions individually toleranced
• ✓Internal corner radii ≥ 1/3 of pocket depth
• ✓Wall thickness ≥ 0.020 in (metal) / 0.060 in (plastic)
• ✓Thread depths ≤ 1.5–2× diameter; standard thread sizes
• ✓Finish callout includes type, color, thickness class, and masking if needed
• ✓A clamping surface exists, or you've noted it's okay to add fixturing stock
• ✓Quantity and annual volume stated — it changes our process recommendation

Send us files through the instant quote page and DFM feedback comes back with your quote, typically within 1–2 business days.

Upload your STEP files and drawings — our engineers will flag cost drivers and confirm manufacturability with pricing, typically within 1–2 business days. If the part is still on the drawing board, our CNC machining services overview shows the processes your design will be routed to.

Get an Instant Quote →