On a large share of the drawings that reach a CNC subcontracting workshop, tolerances have been assigned by habit rather than by functional analysis: the designer left the default ±0.01 from the CAD template, or thought "make it tight, it can't hurt". It does hurt: tolerance is the single decision that affects the unit price most. This article deepens the tolerance section of our DFM article and complements our ISO 2768 general tolerances article.
The Relationship Between Tolerance and Cost Is Not Linear
When the tolerance is halved, the cost does not double; it usually rises more. Because every time a tolerance band crosses a threshold, not only the machining time changes but also the required machine class, the measuring method, the ambient conditions and the scrap rate. Roughly:
| Tolerance | What is required | Measurement | Relative cost (±0.1 = 1.0) |
|---|---|---|---|
| ±0.1 mm (ISO 2768-m, 6–30 mm) | Standard CNC, single pass, normal tooling | Callipers | 1.0 |
| ±0.05 mm (ISO 2768-f) | Standard CNC, careful tool offset | Micrometer / callipers | 1.1–1.3 |
| ±0.02 mm | Well-maintained CNC, finishing pass, thermal stability | Micrometer, gauge | 1.3–1.7 |
| ±0.01 mm | Precision CNC, separate finishing, tool-life tracking, in-process measurement, temperature control | Micrometer (0.001), CMM, dial indicator | 1.8–2.5 |
| ±0.005 mm | Swiss-type or precision lathe, temperature-controlled environment, 100% inspection | CMM, air gauge, dial indicator | 2.5–4 |
| ±0.002 mm and below | Grinding, honing, lapping; air-conditioned measuring room | Precision CMM, optical measurement | 4–8+ |
The values are approximate for typical turned and milled steel/aluminium parts; geometry, material and quantity change them. But the direction is clear: going from ±0.1 to ±0.01 can roughly double the price, and going to ±0.005 can triple it.
Where Does the Cost Come From?
- Machining time: a tight tolerance requires a separate finishing pass, low feed and frequent tool offsetting.
- Measuring time: 5 seconds with callipers for ±0.1; minutes with a micrometer or CMM for ±0.01. In series production the inspection frequency also increases.
- Tool life: at tight tolerances the effect of tool wear on the dimension quickly reaches the limit; the tool is changed earlier.
- Thermal effects: steel expands 11–12 µm per metre per 1 °C; on a 100 mm part a 5 °C temperature difference means 6 µm. At ±0.005 that is half the tolerance. Machine warm-up and ambient temperature must be controlled.
- Scrap and rework: as the tolerance tightens, the out-of-tolerance rate rises according to the process capability (Cp); every scrap part is lost material and time.
- Documentation: tightly toleranced features usually go into the inspection report; report time is added.
How Is the Functional Tolerance Determined?
The question to ask for every dimension: "What happens if this dimension goes outside the tolerance?" If the answer is "nothing", the general tolerance is sufficient.
- Define the function: fit (shaft-hole), bearing seat, sealing, alignment, appearance, weight? Only dimensions tied to a function get a tight tolerance.
- Use the fit system: for shaft-hole relationships the ISO 286 fit system (H7/g6, H7/k6, etc.) assigns the tolerance according to function; write a standard fit instead of an arbitrary ±0.01. H7 on the hole and g6 or h6 on the shaft are combinations the manufacturer knows and produces economically.
- Calculate the tolerance chain: if several parts stack up in the assembly, their tolerances add up (worst case) or are combined as the root sum of squares (statistical). Shortening the chain is cheaper than tightening individual tolerances.
- Apply geometric tolerances only where needed: concentricity, perpendicularity and flatness are cost items independent of the dimensional tolerance; they must be measurable with a datum.
- Think about surface roughness separately: if Ra 0.8 and ±0.01 are requested together, the cost multiplies; except on sealing surfaces, Ra 1.6–3.2 is usually sufficient.
- Account for coating and heat treatment: hard anodising and plating change the dimension; heat treatment distorts. State in which condition the tolerance applies and plan post-grinding if necessary.
Realistic Tolerance Values: What Is Routine, What Is Special?
| Feature | Routine (no extra cost) | Achievable (extra cost) | Special process required |
|---|---|---|---|
| Turned diameter (CNC lathe) | ±0.02 | ±0.01 | Below ±0.005 (grinding) |
| Turned diameter (Swiss-type, Ø<20) | ±0.01 | ±0.005 | Below ±0.002 |
| Milled length/width | ±0.05 | ±0.02 | Below ±0.01 |
| Hole diameter (drilled) | ±0.05 / H12 | H9 (reamed) | H7 and below (reaming/boring/honing) |
| Hole position | ±0.05 | ±0.02 | Below ±0.01 |
| Thread | 6g / 6H | 4h / 5H | Special pitch, tight classes |
| Flatness (100 mm) | 0.05 | 0.02 | Below 0.005 (grinding/lapping) |
| Concentricity (single set-up) | 0.02 | 0.01 | Below 0.005 |
| Surface roughness Ra | 1.6–3.2 | 0.8 | 0.4 and below (grinding/polishing) |
Values are in mm and typical for steel/aluminium; at Tornelle, ±0.005 mm on Swiss-type lathes and ±0.01 mm on conventional lathes are within the routine production range. They are clarified at the quotation stage according to material and geometry.
Common Tolerance Mistakes
- The same tolerance on all dimensions: the default ±0.01 from the CAD template remaining on every dimension. Solution: general tolerance (ISO 2768-mK) + specific tolerances only on functional dimensions.
- Unmeasurable tolerance: definitions such as ±0.005 after coating or concentricity without a datum.
- Contradictory tolerance: the total in a chain does not match the sum of the parts; the manufacturer does not know which one to follow.
- Unnecessary unilateral tolerance: writing Ø19.975 ±0.025 instead of Ø20 +0.00/−0.05 makes targeting easier for the manufacturer; both define the same band, but the second is less error-prone.
- Surface and tolerance ignoring each other: asking for a ±0.005 tolerance on an Ra 6.3 surface is practically meaningless; roughness increases measurement uncertainty.
Discussing Tolerances with the Supplier
A good contract manufacturer points out expensive tolerances at the quotation stage and asks "is this dimension functional?". Giving a clear answer to this question reduces both the price and the lead time. In its quotation process Tornelle classifies tolerances by cost impact and makes recommendations; for the process see our how we work page. The other items that affect the price are covered in our 12 factors article.
Frequently Asked Questions
What happens if I do not specify a general tolerance?
The manufacturer either asks or applies its own assumption; a risk of dispute arises. Always write a general tolerance standard (for example ISO 2768-mK) in the drawing's title block.
Can ±0.01 mm be held in every CNC workshop?
With a suitable machine, measurement and process discipline, yes; but it requires extra cost and time. Ask your supplier for a sample inspection report at this tolerance.
Does a tighter tolerance mean higher quality?
No; quality is the reliable fulfilment of the function. An unnecessarily tight tolerance only brings cost and scrap; it does not contribute to the function.
How are tolerances assessed on inch drawings?
±0.001" ≈ ±0.025 mm, ±0.0005" ≈ ±0.0127 mm, ±0.0002" ≈ ±0.005 mm. The same cost logic applies; make sure rounding during conversion does not tighten the tolerance.
Conclusion
Tolerance is the most powerful cost tool in the designer's hands: making functional dimensions only as tight as necessary and giving the rest a general tolerance can reduce the part price by 20–50% without changing the function. To see which tolerances on your drawings are expensive, send your STEP and PDF files via our quote form; tolerance recommendations come with the quote.
