Tolerance callouts are where engineering intent meets manufacturing reality. Over-tolerancing is one of the most expensive habits in product development. Industry data suggests it accounts for 25-40% of unnecessary manufacturing cost on prototype and low-volume parts, and most engineers don't realize they're doing it.
What tolerances actually cost
Every tolerance on your drawing is a cost driver. The relationship between tolerance and cost is exponential, not linear. Here's what that looks like in practice:
- ±0.010" (2-decimal default). Any competent shop holds this on a manual mill. This is your cheapest option.
- ±0.005" (3-decimal default). Standard CNC territory. Most shops use this as their default when you don't call out a tolerance. Minimal cost impact.
- ±0.002" requires good CNC equipment and a capable operator. Expect a moderate bump in price.
- ±0.001" is precision machining. Slower feeds, more inspection, longer setup. Roughly 4x the cost of standard machining per feature.
- ±0.0005" enters grinding or lapping territory. The part has to sit in quality control for up to 90 minutes just to normalize to room temperature before inspection. 5-10x cost increase.
- ±0.0001" is specialty shop work only. Wire EDM, jig grinding, optical comparators, climate-controlled rooms. About 24x the cost of standard machining.
Going from ±0.005" to ±0.001" doesn't cost twice as much. It can cost five to ten times as much, depending on the geometry and material. That cost comes from slower cycle times, tighter process control, and the fact that a part machined in 15 minutes at standard tolerance might take 45 minutes at tight tolerance once you factor in setup, verification, and quality holds.
When tight tolerances matter
Tight tolerances are justified when:
- Parts mate with other components and clearance or interference fits are critical. Bearing bores, shaft fits, and seal grooves need precision. A bearing bore that's 0.0005" oversize will let the outer race spin, destroying the housing.
- The application involves high-speed rotation or vibration. A 0.002" imbalance on a 10,000 RPM spindle creates measurable vibration and premature bearing failure.
- Thermal expansion is a factor. An aluminum housing operating at 150°C grows roughly 0.002" per inch of length. Your room-temperature fits need to account for that differential growth.
- Regulatory or certification requirements demand it. Aerospace (AS9100), medical (ISO 13485), and defense specs often call out specific tolerances with mandatory inspection documentation.
When they don't
Most features on most parts don't need tight tolerances:
- Clearance holes for fasteners. A ±0.010" through-hole for an M6 bolt works fine. The bolt head and washer cover the slop.
- Non-functional surfaces. The outside dimension of a bracket that bolts to a frame doesn't need ±0.001". Nobody is measuring it in assembly.
- Cosmetic features. Unless it's a consumer product with tight fit-and-finish requirements, ±0.005" is plenty.
- Prototype runs. If you're still iterating on the design, don't over-constrain the machinist. One European automotive supplier discovered that relaxing non-critical features from ±0.01 mm to ±0.03 mm cut their machining costs by 22% with zero impact on assembly.
GD&T vs. bilateral tolerances
If you're still putting ±0.005" on everything, you're leaving money on the table. Geometric Dimensioning and Tolerancing (GD&T, defined in ASME Y14.5-2018) lets you specify exactly what matters functionally:
- Position tolerances control where features sit relative to datums. A bolt pattern needs its holes in the right position relative to each other, but each hole's diameter matters less.
- Profile tolerances control complex surface shapes without stacking up individual dimensions.
- Runout and concentricity control rotational accuracy for shafts, bores, and rotating assemblies.
- Flatness and perpendicularity control surface relationships for sealing faces and mating interfaces.
The real power is in MMC (Maximum Material Condition) modifiers. When you call out a position tolerance at MMC, the machinist gets bonus tolerance as the feature departs from its maximum material size. A hole drilled slightly larger than its minimum gives extra positional wiggle room. More parts pass inspection. Same functional result. Lower cost.
GD&T gives the machinist freedom on dimensions that don't affect function while tightening the ones that do. The result is lower costs, fewer rejects, and parts that actually work in assembly.
The conversation to have with your machinist
Before you finalize your drawing, ask your machining supplier:
- "Which tolerances on this part are driving your cost?"
- "Can you suggest looser tolerances on non-critical features?"
- "What's your standard machining tolerance if I don't call anything out?" (Most shops default to ±0.005" for metals, ±0.010" for plastics.)
- "Do you have the inspection equipment to verify these callouts?"
A good machinist will tell you where you're over-constraining the part. Listen to them. They see your drawing through the lens of what their machines can actually produce, and that perspective saves you money every single time.