Design for Manufacturability (DFM) Master Checklist for CNC Parts

Wall thickness directly affects manufacturability. Too thin = vibration during machining, deflection, broken tools. Too thick = wasted material, longer machining time.

• ▸Aluminum: Minimum 0.8 mm for wall up to 10 mm tall. 1.5 mm for taller walls. Add 0.5 mm safety margin for high-aspect-ratio walls.
• ▸Steel/Stainless: Minimum 1.0 mm for wall up to 10 mm tall. 2.0 mm for taller walls. Steel doesn't deflect as easily but tooling pressure is higher.
• ▸Titanium: Minimum 1.5 mm. Titanium's high modulus makes thin walls deflect under tool pressure.
• ▸Engineering plastics: Minimum 1.0 mm for PEEK, POM. Polymers deform if too thin.

Internal corners in CNC parts MUST have a radius — a sharp 90° internal corner can't be machined by any cutting tool. The radius equals at least the tool radius.

• ▸Standard internal corner radius: 1.5 mm (for 3 mm end mill) or larger.
• ▸Smaller corners (down to 0.5 mm): Require smaller end mills, increase machining time 2-3×.
• ▸Very tight corners (< 0.5 mm): Require wire EDM, increasing cost significantly.
• ▸External corners: No restriction — sharp external corners are fine.

Holes that are too close to an edge or each other can crack the part during machining or cause tool deflection.

• ▸Hole-to-edge minimum: 1.5× hole diameter. For an M6 hole (≈ 5 mm tap drill), minimum edge distance ≈ 7.5 mm.
• ▸Hole-to-hole minimum: 2× the larger hole diameter. Closer holes risk breakdown during drilling.
• ▸Hole near a slot: Treat slot edge as the hole edge. Apply 1.5× rule.

Pockets (recessed areas) have a maximum depth-to-width ratio. Deeper pockets require longer end mills, which deflect and vibrate, producing poor surface finish and dimensional drift.

• ▸Aluminum/Steel pockets: Max depth = 4× tool diameter. So a 5 mm wide pocket can be ~20 mm deep max with standard tooling.
• ▸Stainless/Titanium pockets: Max depth = 3× tool diameter. Harder materials cause more tool deflection.
• ▸Deep pockets (depth > 4× width): Require multiple plunge passes, longer tool life issues, and may need specialty long-flute end mills.
• ▸Very deep pockets (>10× width): Consider redesigning — perhaps as two parts, or using EDM cavity instead.

Internal threads have specific manufacturability constraints based on the thread size and material.

• ▸Thread engagement length: 1.5× thread diameter is standard. So M6 thread (1 mm pitch) needs 9 mm engagement. Longer than 3× diameter doesn't add strength and risks tool breakage.
• ▸Tapped vs thread-milled: Thread tapping is faster but produces lower-quality threads in stainless, titanium, hardened steel. For these materials, thread milling produces better results but takes longer.
• ▸Form taps vs cut taps: Form taps (no chips) work in ductile materials (aluminum, brass). Cut taps work everywhere but produce chips that can damage threads.
• ▸Through-hole vs blind threading: Through-hole threading is preferred. Blind threading requires bottom-tap with chip relief — costs more.
• ▸Thread coatings: Specifying threadlock, dry-film lubricant, or self-lubricating coating affects assembly. Note on drawing if required.

Undercuts (features that cannot be machined with a vertical tool approach) significantly increase manufacturing cost.

• ▸Standard undercut: 90° undercut into a vertical wall is the easiest. Requires angled tool or 4th-axis access.
• ▸Deep undercut: Multiple setups, complex fixturing.
• ▸Back-machining: Drilling or facing from the opposite side. Often requires a second setup adding 30-50% to cycle time.
• ▸Solution: If possible, redesign as two parts that bolt together, eliminating the undercut.

Surface finish requirements drive machining strategy. Better finishes require finer cuts, more passes, longer cycle time.

• ▸Ra 6.3 µm (general machined surfaces): Standard finish from CNC milling/turning. No special operations needed.
• ▸Ra 3.2 µm (good visible finish): Finishing pass with smaller depth-of-cut. ~15% cost premium.
• ▸Ra 1.6 µm (precision surfaces): Finishing pass with very fine cut. ~25% cost premium.
• ▸Ra 0.8 µm (excellent surface): Multiple passes, smaller depths. May require grinding finish. ~40% premium.
• ▸Ra 0.4 µm (mirror-like): Grinding + polishing required. 2-3× cost.
• ▸Ra 0.1 µm (mirror polish): Manual polishing. Very expensive.

Specifying cosmetic surfaces (visible to end user) requires additional considerations.

• ▸Define 'cosmetic' on drawing: Use cross-hatched fill or 'A' marking to identify cosmetic surfaces.
• ▸Toolmarks: Cosmetic surfaces should be deburred and toolmark-free. Specify on drawing.
• ▸Anodizing prep: Aluminum surfaces for anodize should be free of grease, deep scratches, oxidation. Surface texture (bead blasted, brushed) must be defined.
• ▸Color matching: Specify Pantone or RAL number. Allow ±3 CIE Lab units for matching.

Frequent mistakes that drive up cost:

• ▸Specifying ±0.005 mm on dimensions that don't need it — quote your supplier 30-50% extra for unnecessary precision.
• ▸Calling out a special material 'just in case' — using exotic materials when standard 6061-T6 would work doubles cost.
• ▸Specifying 'mirror polished' finish on a non-visible surface — adds significant cost with zero functional benefit.
• ▸Internal sharp corners (R=0) — forces small tools, breaks them frequently, increases scrap rate.
• ▸Very deep pockets with thin walls — vibration during machining, dimensional drift, poor surface finish.
• ▸Inconsistent tolerance datum references — confusing inspection, may require re-machining.
• ▸Missing material spec — supplier guesses, may use wrong material, fail incoming inspection.
• ▸Drawings without GD&T — over-relies on plus-minus tolerances, ambiguity for assembly fits.