Your quote is mostly machine hours
Material for an aluminum bracket rarely exceeds 15–20% of a prototype quote. The rest is machine time and the labor wrapped around it: programming, fixturing, tool changes, deburring, inspection. That is good news, because machine time is the one cost you can attack directly from the CAD seat. Most of the expensive geometry that lands in an RFQ pile was drawn by default, not by decision.
1. Loosen tolerances wherever the function allows
CNC machining reaches ±0.005 mm (±0.0002") routinely — the question is what that pass costs. Holding five-micron tolerances means finish passes at light depths of cut, slow feeds, temperature-stable measurement, and real scrap risk on every setup. Meanwhile, a shaft seat for a standard bearing usually needs only ±0.01–0.02 mm, and clearance holes are perfectly happy at ±0.1 mm. On a 6061-T6 housing, relaxing three non-critical faces from ±0.01 mm to ±0.1 mm commonly trims double-digit minutes off cycle time. Across a 200-piece order, one careless callout can out-price the material itself.
2. Open up the internal corners
An end mill leaves its own radius in every pocket corner. A 3 mm corner radius in a 20 mm deep pocket forces a small, fragile tool working through several spring passes; call out R6 in the same pocket and a robust 12 mm cutter clears it in one. Useful rules of thumb: keep the internal corner radius at least a third of the pocket depth, and never specify a sharp internal corner unless a separate EDM operation is genuinely intended — because that is what it will take.
3. Design out setups
Every time a part leaves the vise, the clock restarts: re-fixture, re-indicate, re-verify the datum. A setup change typically runs 15–45 minutes of non-cutting time, and five-axis machines exist precisely because one setup often beats three. You do not need to know the shop's machine list to help — just avoid features that can only be reached from the back of an otherwise one-sided part, keep hole patterns referenced to common datums, and be suspicious of deep pockets on both faces of a single plate.
Stock selection helps here too. If your part can start from a standard plate or bar size instead of an oversized blank, the shop skips a facing operation and wastes less material. And keep thin, unsupported walls in check: anything that vibrates under the cutter needs slower speeds, sacrificial supports, or extra tabs to hold it — all of which show up on the invoice as time.
4. Pick a material the shop cuts every day
- Aluminum: 6061-T6 is the industry workhorse — good strength, excellent machinability, sane price. Pay 7075's premium only when the stiffness-to-weight math actually demands it.
- Steel: 1018 for general work, 4140 when strength matters; both cut far more predictably than most stainless grades. If corrosion resistance is required, 303 machines noticeably better than 316 within the same family.
- Engineering plastics: POM and nylon 6 cut cleanly. PEEK and glass-filled grades are where tool wear and heat management start inflating the quote.
Exotic alloys are sometimes unavoidable — but half the time the "requirement" is inherited from an old drawing nobody has revisited in years.
5. Call out only the surface finish you need
A standard milled finish around Ra 1.6 µm is essentially free. Ra 0.4 µm on a sealing face adds finish passes, extra measuring, and occasional rework. Specify the fine finish on the seal groove — not the whole part — and leave cosmetic uniformity to bead blasting or anodizing rather than machining. If a face only matters because it bolts against another face, machined-as-milled is usually the right call.
6. Match the process to the quantity
CNC machining is superb at 1–100 parts and still sensible into the low hundreds. Somewhere around there, hard tooling starts to win: quoting the same bracket at 500 pieces as a die casting job can roughly halve the unit cost. Between those worlds, soft production tooling bridges the gap without a full production tool investment. And if you need first articles checked before committing to either route, our CNC machining service turns prototype batches in days — often the fastest honest answer to "is this design really manufacturable?"
7. Sanity-check the threads
Tapped holes deeper than 1.5–2× the nominal diameter add tap-breakage risk without adding pull-out strength; the extra threads below that depth carry almost no load. Avoid threads under M3 on production parts — M2 taps snap when an operator blinks — and prefer through-holes where geometry allows, since blind-hole chip evacuation is a quiet, persistent cycle-time killer.
The pattern behind all seven
Almost every lever above is a callout, a radius, or a material line on the drawing. None of them touches the function you actually need. That is the whole game in metal machining economics: the design decides the machine time, so the design decides the price. Ten minutes of DFM review — or a quote with honest feedback from the shop — is the cheapest optimization pass you will ever run.
