Every drawing lands on our desk with a tolerance block at the bottom. +/-0.05mm, +/-0.1mm, or the classic "unless otherwise specified." And almost nobody who sends those drawings has actually thought through what those numbers cost. A +/-0.005mm callout on a 200mm part doesn't make you look thorough — it makes you look like you've never paid for precision machining.

Here's what actually happens on the shop floor when tolerances tighten. And why your tolerance choices matter more than your material choices.

Let's start with what most shops consider "standard precision" — +/-0.01mm on a linear dimension. On our 3-axis and 4-axis machining centers, this is routine. We hold it all day long on features up to about 150mm. The tool doesn't need to be changed between parts, the inspection is quick (calipers or a mic), and the cost per piece is predictable.

But what about +/-0.005mm? That's where things get interesting. At 0.005mm, you're now at half a hair's width. Thermal expansion of the workpiece alone can eat your entire tolerance budget. A 100mm aluminum part that warms 3C from machining heat grows by 7 microns — and that's with flood coolant. On a 200mm part? 14 microns. Your entire tolerance band is gone before you even measure it.

This is why tight-tolerance parts get machined in a temperature-controlled environment (20C +/-1C), measured on a CMM, and often require multiple finishing passes. Setup time goes up. Inspection time goes up. Scrap rate goes up. The cost multiplier from +/-0.01mm to +/-0.005mm is typically 2-3x, and from +/-0.01mm to +/-0.001mm it's 5-10x.

Most machining cost guides show a nice smooth curve where cost increases exponentially as tolerance tightens. The reality is more like a staircase with a cliff.

The big jump isn't between 0.1 and 0.01. It's between 0.01 and 0.005. That's where you cross the line from "careful CNC machining" into "precision machining territory" where the entire process — fixturing, tooling, environment, inspection — changes.

Here's a scenario we see weekly. An engineer specifies +/-0.01mm on a bore diameter and +/-0.01mm on a bore position relative to a datum. The CMM report shows both within tolerance. The parts go to assembly. And they don't fit.

Why? Because the bore might be 0.01mm oversize (which is within tolerance) and the position might be 0.01mm off (also within tolerance), but the combined effect of both errors means the mating shaft can't drop in. This is why GD&T exists — it controls the functional relationship between features, not just individual dimensions.

GD&T callouts that actually matter on CNC machined parts:

• True Position (0.05mm MMC): For mounting hole patterns. If you're bolting two parts together, position tolerance matters more than hole diameter tolerance
• Concentricity (0.01mm): For rotating shafts and bearing seats. The axis needs to be shared, not just the diameter correct
• Flatness (0.02mm): For sealing surfaces. A gasket doesn't care if the surface is 0.02mm off position — it cares if it's flat
• Perpendicularity (0.01mm): For datum relationships. If face B isn't perpendicular to bore A, the assembly stacks up wrong

The cost of GD&T is roughly the same as equivalent linear tolerances — the inspection method changes (CMM instead of calipers), but the machining approach doesn't. The difference is that GD&T gives you functional parts instead of dimensionally correct parts that don't work.

The same tolerance callout costs different amounts on different materials. Here's what we see in production:

Aluminum 6061: The easiest to hold tight tolerances on. Low cutting forces, good chip clearance, minimal tool wear. +/-0.005mm is achievable on most features under 100mm.

Stainless Steel 304: Cutting forces are 2-3x higher than aluminum. Tool wear accelerates, and the first 10 parts might hold +/-0.01mm while the 50th part drifts to 0.02mm because the insert has worn. Tight tolerances on SS require aggressive tool change schedules.

Titanium Ti-6Al-4V: The material fights back. Springback after cutting means the finished dimension is slightly larger than the cut dimension. We compensate for this with spring-pass programming, but it adds setup time. +/-0.01mm is realistic. +/-0.005mm requires jig boring or grinding.

PEEK: Thermal expansion is the main issue. The part changes size measurably between the machining temperature and the room temperature. For tight tolerances, we machine, let it sit for 2 hours to equilibrate, measure, then do a skim cut. Adds cycle time but holds the tolerance.

After machining tens of thousands of parts, here's the approach that produces the best results at the lowest cost:

1. Only specify tight tolerances where they matter. Assembly interfaces, bearing seats, seal surfaces — these deserve +/-0.005mm to +/-0.01mm. Everything else? +/-0.05mm is probably fine. A non-critical wall thickness doesn't need the same tolerance as a bearing bore.
2. Use GD&T for functional relationships. If two features need to be aligned, specify position or concentricity relative to a datum. Don't just put tight linear tolerances on both and hope they line up.
3. Account for material behavior. Tight tolerances on long SS parts will cost more than tight tolerances on short aluminum parts. If your design allows, choose materials that are easier to machine precisely.
4. Specify the tolerance, not the process. Don't write "grind to +/-0.005mm" — write "+/-0.005mm" and let the shop decide if CNC milling, jig boring, or grinding is the most cost-effective method. Sometimes a skilled machinist with a sharp end mill can hold 0.005mm on a milling center, and grinding would be overkill (and more expensive).
5. Provide a functional description. If you tell us "this bore holds a 6205 bearing at a light press fit (0.01-0.02mm interference)," we can tolerance the bore appropriately (35.00-35.01mm) and select the machining method that holds it reliably. We don't need a +/-0.001mm callout to make your bearing fit. We need the right tolerance for the function.

A drawing with 200 tolerance callouts, half of which are +/-0.005mm, doesn't make your design robust. It makes your parts expensive and your lead times long. The best tolerance strategy is one that loosens every dimension as much as the function allows and tightens only the ones that truly matter.

We've seen projects where loosening 80% of the tolerances from +/-0.01mm to +/-0.05mm cut the part cost by 30% with zero impact on assembly quality. The tolerances that mattered — bearing bores, seal faces, datum relationships — stayed tight. Everything else was let go.

That's the point. Tolerance design isn't about making everything tight. It's about knowing exactly what needs to be tight and letting everything else breathe.