You send an RFQ, the quote comes back higher than expected, and you're not sure why. The part looks simple — no crazy geometry, standard material, reasonable tolerances. But the number on the quote is 40% more than you budgeted. We see this every week.

CNC machining cost is mostly locked in before the part ever touches a machine. Changing a 3mm internal radius to 6mm can cut cost by 30%. Reducing setups from four to two can cut it in half. These are design-level decisions you control. Here are the eight that move the needle most — starting with design, then material, then production strategy.

1. Internal corner radii — the biggest lever you're probably ignoring

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. If your design demands a sharp corner, the shop has to use EDM, broaching, or hand work — all expensive.

But even without sharp corners, the radius you pick matters hugely:

Small tools mean slow feeds, more deflection, more passes, higher breakage risk. Going from 1.5mm to 6mm internal radius can reduce cycle time on that feature by 60-80%.

The way I think about it: make every internal radius as large as your design allows. Default to 6mm or bigger on non-functional corners. If one pocket genuinely needs a small radius for stress relief or assembly fit, keep it localized — don't propagate it everywhere. A single small-radius pocket adds cost. An entire part designed around one is a budget disaster.

2. Undercuts — know the cost before you draw one

An undercut is anything a straight end mill can't reach: dovetail slots, T-slots, internal O-ring grooves, back-side chamfers. They need special tooling — dovetail cutters, lollipop cutters, keyway cutters. That means the shop has to have the tool or buy it, the toolpath gets complex, setup verification takes longer, and inspection is slower.

A part with undercuts typically costs 20-50% more than the same geometry without them.

Before putting an undercut on the drawing, ask: can this be an external feature instead? An external O-ring groove machined from the outside costs a fraction of an internal one. A bolted assembly might eliminate the snap-ring groove entirely. If the undercut truly has to be there, keep all of them to the same tool geometry — one T-slot width across the entire part, not three different ones.

3. Setup count — every re-fixturing costs money

Every time the part comes out of the machine and gets re-clamped, you pay for operator time, re-indication, and tolerance stack-up. A one-setup part is cheaper than a three-setup part. Always.

Setup changes drive cost three ways: operator labor to remove, clean, re-fixture, and re-indicate; positional error between setups (features drift relative to each other); and increased scrap risk from mis-loads or chip-in-fixture errors.

Design for the fewest setups possible. Look at the features from each face. Six-sided access = multiple setups on a 3-axis, or fewer on a 5-axis. If the part needs four or five 3-axis setups, ask the shop whether 5-axis brings it down to one or two — a 5-axis part in two ops often costs less than a 3-axis part in four, even at the higher 5-axis rate.

4. Deep features and thin walls — the aspect ratio problem

CNC machining works best at moderate aspect ratios. Deep pockets and thin walls drive cost up fast.

An end mill cuts to roughly 3-4x its diameter in depth before vibration takes over. A 10mm-deep slot with a 6mm end mill: fine. A 30mm-deep slot: long-reach tool, slower feeds, multiple depth passes, careful chip evacuation — easily 3-5x the cycle time.

Walls thinner than 0.8mm in aluminum or 1.0mm in most plastics chatter during machining and warp from residual stress release. The part distorts as material comes off, throwing tolerances on later features.

Keep pocket depth-to-width under 4:1 if you can. Stay above 0.8mm wall in aluminum and 1.2mm in engineering plastics. If you absolutely need a deep narrow pocket, see if it can be drilled and reamed instead of milled — drilling handles depth-to-diameter ratios that milling can't touch.

5. Material choice IS a cost decision

Material cost isn't just the raw stock price. Three things matter:

Machinability. 6061 aluminum cuts fast, tool life is long. 7075 is slower with more tool wear. Stainless and titanium are an order of magnitude worse on both. Engineering plastics need different parameters than metals but cut fine with sharp tools.

Raw price. At quantity 1-5, the dollar difference between 6061 and 7075 is noise. At quantity 500 or 5,000, it's real money. Choose accordingly.

Material utilization. How much of the billet becomes chips? A part hogged 80% out of a solid block wastes more material than one with 20% removal. At high volumes, this is why near-net-shape processes (casting, forging, extrusion) get paired with CNC finish machining.

Pick the cheapest material that meets requirements. Don't upgrade to 7075 because "stronger is better" unless your analysis says 6061 fails. Don't spec stainless because "it sounds higher quality" unless corrosion or strength genuinely demands it. The right material hits your performance targets at the lowest total part cost.

6. Tolerances — every decimal place is expensive

This is the cost driver engineers specify without realizing it. A drawing with ±0.1mm everywhere is a completely different part than one with a ±0.25mm general tolerance and ±0.05mm only on functional features.

The relationship isn't linear. ±0.25mm to ±0.1mm roughly doubles cost. ±0.1mm to ±0.025mm doubles it again. Below ±0.01mm, you may triple or quadruple it.

Tight tolerances mean slower cuts, in-process measurement pauses, more scrapped parts, and longer inspection. Put tight tolerances only on features that need them — mating surfaces, bearing bores, seal grooves. Everything else gets a generous general tolerance.

What I recommend: general tolerance ±0.25mm for non-critical features, ±0.05mm where fit demands it, ±0.01mm only for bearing fits and seal diameters. And always specify explicitly — if your drawing has no tolerance values, the shop defaults to their internal standard, which may be tighter and more expensive than you need.

7. Batch size and setup amortization

Setup cost is fixed — same time for one part as fifty. At quantity 1, setup might be 50% of part cost. At quantity 100, it might be 2%.

The biggest cost drop happens between 1 and 10 parts. The curve flattens between 50 and 500. Beyond 500, material and cycle time dominate.

If you'll eventually need 100 parts, don't order one prototype now and 99 later — you pay setup twice. Get 1-5 prototypes for validation, then batch the production order. If cash flow allows, combining prototypes and a small production buffer into one order can save 15-25%.

8. DFM feedback — the free money you're leaving on the table

Most shops will review your drawing before quoting, for free. Their DFM feedback is often the single most valuable cost input you'll get.

A good machinist sees things that designers miss: a 2.5mm radius lets them use a standard tool instead of a custom one. Flipping the part 180° eliminates a setup. A blind threaded hole changed to through-hole skips a bottom-tapping op. The surface finish specked on an internal non-cosmetic surface is unnecessarily expensive.

Send the drawing before it's finalized. Ask: "What would you change to reduce cost without affecting function?" This conversation costs nothing and routinely saves 10-30%.

How these stack

Apply all eight — generous radii, no unnecessary undercuts, minimum setups, manageable aspect ratios, appropriate material, sensible tolerances, efficient batch size, and shop DFM feedback — and expect to spend 30-50% less than a part designed without them.

The earlier you are in the design process, the more leverage you have. Changing a radius on a CAD model is free. Changing it after the first production run costs real money.

Send us your drawing — even preliminary — and tell us what the part needs to do. We'll review it for manufacturability, flag the cost drivers, and return a quote with specific suggestions for cost reduction, usually within 24 hours.