How to Reduce CNC Machining Cost: 12 Design Changes That Work

1. Design for fewer setups — the biggest lever

Every time a part comes out of the machine, gets flipped, re-indicated and clamped again, you pay for it twice: once in operator time, once in the accumulated tolerance risk. A housing that needs features on five faces looks reasonable on screen. On the floor it may mean four or five operations.

What helps: keep critical features reachable from as few directions as possible. Can two side faces be combined into one angled face? Can a hole pattern move to a face that's already being machined? On a 5-axis machine some of this dissolves — which is exactly why complex parts often cost less on 5-axis despite the higher hourly rate.

2. Tolerance only the features that matter

The most common thing we see in quotes that come back high is a drawing where every dimension carries a tight tolerance. When everything is ±0.01mm, the shop has to assume it all matters — slower finishing passes, climate-controlled inspection, higher scrap risk.

The fix takes ten minutes: mark the three or four dimensions that actually control the fit, and let the rest fall to the ISO 2768-m default. We published the numeric tables for what those defaults are — worth having open while you're marking up the drawing. If you're new to geometric tolerancing, our GD&T for buyers guide covers the six symbols that matter.

3. Internal corner radii — small change, big saving

A rotating cutter cannot make a sharp internal corner. If you specify R0 or R0.5 in an internal pocket, the shop has to drop to a tiny end mill to get anywhere near it, and tiny tools cut slowly — often five to ten times slower than a standard cutter.

Specify the largest radius the design can tolerate. As a rule of thumb, a radius slightly larger than half the pocket depth lets a rigid tool run at full speed. R3 or R5 costs a fraction of R0.5 on the same geometry.

4. Depth is expensive

Two related traps. Deep pockets force long, thin tools that need slow feeds and multiple step-downs — a 60mm deep pocket can take ten times longer than a 15mm one. Deep holes (beyond roughly 5× diameter for drilling, 10× for boring) push you into specialised tooling, pecking cycles and chip evacuation problems.

If a pocket only needs to be deep in one small area, consider machining the whole pocket to the shallow depth and using a smaller local feature only where required.

5. Use standard hole sizes

Every non-standard diameter means a drill, reamer or boring bar the shop may not have on the shelf. Standard metric drill sizes — or better, hole diameters that match a reamer they already own — avoid both tooling cost and the setup time to qualify a new tool. Same logic applies to thread sizes: stick with common ones.

6. Choose the material for the job, not for the datasheet

Titanium deserves special mention here: it can multiply part cost several times over. Our titanium machining guide explains why, and when to choose something else.

We compared the three most common families — aluminium, stainless steel and titanium — on specific strength, machining time and total cost.

Over-specifying material is common and expensive in two directions at once: the stock costs more and it takes longer to cut. Titanium is a frequent example — it can cost several times what an aluminium part costs for identical geometry, and if the application doesn't need the strength, temperature resistance or corrosion performance, you've paid for nothing.

We put together a comparison of the common aluminium grades if you're choosing within that family — 6061 is the right answer far more often than people expect.

7. Think about the stock you're starting from

If your part is 90 × 40 × 20mm and you design it out of 100 × 50 × 25 stock, that's fine — those are standard sizes. If it's 93 × 42 × 21, the shop is either buying oversized stock and removing more material, or cutting a custom blank. Both cost money. Designing to standard stock dimensions is a quiet, reliable saving.

8. Surface finish: call it out only where it does something

Our Ra roughness chart shows what each Ra level costs and which applications genuinely need it.

A blanket Ra 0.8 or Ra 0.4 across an entire drawing means extra finishing passes everywhere. Most faces on most parts are perfectly happy at the standard as-machined finish. Call out the sealing faces, bearing bores and sliding surfaces — leave the rest default. Our surface finish comparison chart shows what each finish actually adds, in cost and in thickness.

9. Give the machinist something to hold

It sounds mundane and it affects the quote directly. A part with no flat, parallel faces and no obvious clamping surface needs a custom fixture — and that fixture is priced into your job. A couple of flats, a parallel pair of faces, or even a sacrificial tab that gets removed at the end turns a custom fixture into a vise job.

10. Threads: depth and class

Beyond roughly 3× diameter, extra thread depth adds almost no joint strength but adds real machining time and tap breakage risk. Similarly, a fine thread class on a non-critical fastener is an inspection burden with no functional return. Standard coarse threads to a standard depth, unless there's a reason.

11. Consider consolidating parts

Sometimes two simple parts that bolt together are cheaper as one slightly more complex machined part — you eliminate a fastener, an assembly step and two sets of tolerances. Sometimes the opposite is true and splitting a complex part into two simple ones is far cheaper. This one genuinely depends on geometry, which is why it's worth asking rather than guessing.

12. Ask before you freeze the design

This is free and it's the highest-return item on the list. Send the drawing to the shop while you can still change it. Every one of the changes above is cheap before the design is frozen and expensive after — and a good shop will spot them in an afternoon.

We do this as part of quoting. If your drawing has something in it that's driving cost without adding function, we'll say so in the quote rather than after you've placed the order.

Send us the drawing at any stage — even a rough one. We'll flag anything that's driving cost without adding function, and quote two quantities side by side so you can see where the numbers turn. For a quick planning estimate before drawings even exist, try our free CNC cost calculator.

Upload Drawings & Get Quote All Technical Resources