The design rules for CNC machined aluminum parts are well-established, and most of them apply to any material. But there are a few aluminum-specific quirks that are worth knowing before you finalize a drawing.
These are the ten DFM rules we find ourselves explaining to customers most often. Follow them and your parts will cost less, arrive faster, and work better.
1. Internal corner radii — biggest lever you have
Internal corners can't be perfectly square on a milled part. The cutter is round, so every internal corner has a radius at least equal to the cutter radius. A 3mm radius lets the shop use a 6mm end mill — fast, rigid, cheap. A 0.5mm radius forces a 1mm end mill — slow, fragile, expensive.
Make every internal radius as large as your design allows. Default to 6mm or bigger on non-functional corners. A single small-radius pocket adds cost. An entire part designed around one is a budget disaster.
2. Wall thickness
Keep unsupported aluminum walls above 0.8mm, preferably above 1.5mm. Below 0.8mm, walls chatter during machining and warp from residual stress release. For tall walls (height-to-thickness above 8:1), add ribs or gussets for support.
3. Hole depth
Through-holes are cheaper than blind holes. For blind holes, keep depth under 4x diameter. Deeper than that needs peck drilling, slower feeds, and more risk of drill wander. If you absolutely need a deep hole, spec the straightness tolerance you actually need — the shop may need gun-drilling or EDM.
4. Threaded holes
Through-threaded holes are simpler than blind-threaded. For blind threads, allow at least 1.5x diameter of clearance at the bottom for the tap lead and chips. Threaded inserts (Heli-Coil, Keensert) are recommended for aluminum parts that will be assembled and disassembled repeatedly — aluminum threads wear and gall.
5. Undercuts
Every undercut needs specialty tooling — dovetail cutters, T-slot cutters, keyway cutters. The shop either has the tool or buys it. Avoid undercuts unless they serve a clear function. If you need one, keep all undercuts to the same tool geometry — one T-slot width across the part, not three different ones.
6. Tolerances
General tolerance ±0.25mm keeps costs low. ±0.05mm on critical features is routine for any competent shop. Below ±0.025mm, cost climbs fast. Put tight tolerances only on features that need them — mating surfaces, bearing bores, seal diameters. Don't copy-paste tight tolerances from another drawing out of habit.
Aluminum 6061 holds tight tolerances more easily than 7075 because it's more thermally stable and less prone to residual stress distortion.
7. Surface finish
Specify what you actually need. "As-machined, Ra 1.6 μm max on all surfaces" is a clean, specific note. "Good surface finish" means nothing.
Bead blasting hides tool marks and produces a uniform matte surface. Anodizing (Type II clear/black) protects and colors the surface — but it adds thickness (5-25 μm), so mask threaded holes and tight bores. Type III hard anodize is thicker (25-100 μm) and more wear-resistant but even more critical to mask.
8. Material selection
6061-T6 is the default for machined aluminum parts. Good strength, excellent corrosion resistance, welds well, anodizes beautifully. 7075-T6 is nearly twice as strong but has poor corrosion resistance, can't be welded, and anodizes with a yellowish tint. Don't spec 7075 unless you genuinely need the strength.
9. Setup count
Design for the fewest setups. Features on one face = one setup = lowest cost. Features on 6 faces = multiple setups = higher cost and more positional error between features. If the part needs features on multiple non-opposing faces, 5-axis may save money over multiple 3-axis setups.
10. Get DFM feedback before finalizing
The single most valuable cost-reduction step is sending a preliminary drawing to the shop and asking: "What would you change to reduce cost without affecting function?" This conversation is free and routinely saves 10-30%.
Common DFM suggestions we make: increase internal radii from 1.5mm to 6mm (eliminates small-tool ops), convert blind holes to through-holes (faster drilling, no chip packing), loosen non-functional tolerances from ±0.05mm to ±0.25mm (faster cutting, less inspection), and add a datum scheme for inspection reference.
Send us your drawing — even preliminary — and we'll give you specific, actionable feedback. Not generic rules, but what matters for your specific part.