The tolerance block on a CNC machining drawing is one of the most expensive pieces of text an engineer writes. A single change from ±0.1mm to ±0.025mm on a few critical features can double the part cost. And the frustrating thing — I see this all the time — is that many tight tolerances get specified out of habit, not because the feature actually needs them.
Here's what different tolerance levels actually cost, what's achievable in a real shop (not a brochure), and how to spec tolerances that get you the performance you need without paying for precision you don't.
What CNC machining can actually hold
This is based on a well-maintained modern CNC machine with a competent operator — not what the machine brochure claims:
±0.125mm (±0.005") — Standard commercial. Any professional shop hits this on virtually every feature, in any machinable material, without special effort. If your general tolerance is ±0.125mm, every shop quotes it, prices are competitive, scrap rates are low. This is where you want to be for non-critical features.
±0.05mm (±0.002") — Precision. Requires attention but is routine for competent shops. The machinist uses finish passes, maybe takes in-process measurements, monitors tool wear. Expect 20-40% cost increase over standard. Most shops hit this daily on aluminum, steel, and engineering plastics.
±0.025mm (±0.001") — Tight. This separates the serious shops from the rest. You need sharp tooling, temperature-stable environment (or thermal compensation), rigid fixturing, in-process probing, conservative cutting parameters. Not every shop quotes this. Those that do charge 50-100% more than standard tolerance work. Some features — deep bores, thin walls, large diameters — simply can't be held at ±0.025mm regardless of effort.
±0.01mm (±0.0005") — Approaching the limit. Temperature control is mandatory — a 1°C change in a 25mm aluminum feature shifts it by roughly 0.6μm. The machine must be in excellent condition. Tool wear must be monitored and compensated continuously. 100% inspection is standard, not sampling. Some features require grinding or honing rather than milling. Expect 3-5x cost versus standard tolerance.
< ±0.005mm (< ±0.0002") — Beyond CNC. At this level, you're beyond what most CNC mills and lathes can reliably deliver in production. You need grinding, honing, lapping, or EDM. If your drawing has tolerances this tight, verify the feature actually needs CNC machining — it probably needs a different process.
How tolerances scale with feature size
Tolerance capability isn't uniform. A 10mm hole can be held tighter than a 100mm bore.
| Feature Size | Comfortable | With Care | With Difficulty |
|---|---|---|---|
| < 25mm | ±0.05mm | ±0.02mm | ±0.01mm |
| 25–100mm | ±0.075mm | ±0.03mm | ±0.015mm |
| 100–250mm | ±0.10mm | ±0.05mm | ±0.025mm |
| > 250mm | ±0.15mm | ±0.075mm | ±0.05mm |
These are guidelines. Material, geometry, and fixturing all move the numbers.
Material affects what's achievable
Aluminum 6061: The easiest common metal for tight tolerances. Excellent stability, low thermal expansion, predictable. Our go-to when someone needs precision without drama.
Aluminum 7075: Harder, more cutting force, slightly more challenging than 6061. Tolerances are still achievable but demand sharper tools.
Stainless (303/304/316): Work-hardens during cutting. Higher thermal expansion than aluminum. Faster tool wear. Tight tolerances are doable but need conservative parameters and frequent tool changes.
Titanium (Ti-6Al-4V): Low thermal expansion helps stability. Low thermal conductivity means heat stays in the cut zone — accelerated tool wear. Tight tolerances are achievable but expensive because titanium is slow to machine regardless of tolerance.
Engineering plastics (PEEK, PEI, PPS): The challenge isn't machine capability — it's thermal expansion. PEEK expands ~5x more than aluminum with temperature. A part machined to ±0.025mm at 22°C may be out of tolerance at 30°C ambient. Tight plastic tolerances need temperature control, sharp tools, light cuts, and stress-relieved material.
PTFE and soft plastics: The material deforms under cutting pressure and springs back. ±0.05mm is the practical limit, and that takes careful parameter control. These materials aren't meant for precision applications.
The tolerance-cost curve
The relationship between tolerance and cost is closer to exponential than linear:
- ±0.25mm → baseline (1x)
- ±0.10mm → ~1.3x
- ±0.05mm → ~1.7x
- ±0.025mm → ~2.5x
- ±0.01mm → ~5x
- ±0.005mm → reconsider the process
Every shop is different, but the shape of the curve is universal: halving the tolerance band roughly doubles the cost.
How to spec tolerances (without wasting money)
The single most cost-effective thing you can do: use a generous general tolerance and call out tight tolerances only on features that need them.
A drawing that says:
General: ±0.25mm unless noted
Bearing bore Ø25mm: +0.02/-0.00
Dowel holes Ø6mm: ±0.01mm (2 places)
Seal face: flatness 0.02mm
...costs far less than the same drawing with ±0.05mm everywhere. The shop sees three features that need precision and focuses effort there.
A drawing that just says "All tolerances ±0.05mm" costs significantly more because the shop has to hit that on every single feature, including non-functional ones.
Common mistakes I see weekly
Tight tolerances on cosmetic features. That external corner radius? ±0.5mm is fine. The chamfer on a cable pass-through? ±0.25mm. Not everything on the drawing is functional — but if the drawing doesn't distinguish, the shop can't either.
Tight tolerances on plastic parts without thermal consideration. A PEEK part machined to ±0.025mm at 20°C changes size at 35°C ambient. Material expansion is real and predictable — account for it.
Copy-pasting from another drawing. The tolerance appropriate for a stainless aerospace bracket may be absurd for an aluminum enclosure. Review every tolerance — don't inherit blindly.
Tolerancing both sides of an assembly stack-up. If Part A fits into Part B, tolerance the interface, not every feature independently. The stack-up becomes unachievable fast. Use GD&T or communicate the functional requirement.
What to tell your shop
Submit the drawing and have a conversation about tolerances before locking the design. Tell them which features are functional and which are cosmetic. Ask: "Where can we loosen tolerances without affecting part function?" A machinist who makes parts all day knows things about tolerancing that a CAD model won't tell you.
Send us your drawing if you want a DFM review that includes specific tolerance recommendations. We'll flag where you're over-specifying and where you might need to tighten up — based on what the part actually needs to do, not generic rules.