What Tolerancing Is — and Why Not Every Feature Needs It
A tolerance states how much deviation is acceptable. Putting a tight one on a face that does no work is pure cost. A guide to deciding where accuracy is needed and where it is not.
No part is ever made exactly to the number on the drawing. That is not a defect; it is physics. A tolerance states how much deviation is acceptable.
What happens if you leave tolerances off
Nothing good. If the drawing says only 50, the maker is entitled to deliver 49.5 or 50.5 and has technically complied.
This is why a general tolerance goes in the title block — usually ISO 2768-m. It says that any dimension without a specific tolerance follows this table:
| Dimension range | Tolerance (class m) |
|---|---|
| 0.5–3 mm | ±0.1 |
| 3–6 mm | ±0.1 |
| 6–30 mm | ±0.2 |
| 30–120 mm | ±0.3 |
| 120–400 mm | ±0.5 |
| 400–1000 mm | ±0.8 |
One line in the title block settles ninety percent of the dimensions on the sheet.
The common mistake: "tighter is better"
It is not. Every step tighter raises cost non-linearly:
| Tolerance | Process | Relative cost |
|---|---|---|
| ±0.5 | Rough cutting and turning | 1× |
| ±0.1 | Ordinary turning | 1.5× |
| ±0.05 | Fine turning | 2.5× |
| ±0.02 | Reaming / grinding | 4× |
| ±0.005 | Precision grinding + temperature control | 10× and up |
Put ±0.02 on twenty dimensions and the price multiplies without the part working one bit better.
The simple test: what does this face do
For every dimension, ask:
Does this surface mate, rotate, seal, or act as a reference in the assembly?
If the answer is no, the general tolerance is enough.
On a typical part, two or three of twenty dimensions actually do work. The rest only have to exist.
Where a specific tolerance earns its place
1. Bearing and bushing seats. These need a defined fit, not a ±. For example Ø40 H7 for the housing and Ø40 k6 for the shaft.
2. Press-fit surfaces. If a part is pressed home, the interference must be specified.
3. Bolt-hole centre distances. If two parts join with four bolts, the patterns must agree or the bolts will not go in.
4. Sealing dimensions. An O-ring groove is toleranced; too deep and it leaks, too shallow and the ring is crushed.
5. Dimensions that stack in an assembly. Five parts in a row and every error adds up.
Bilateral, unilateral and fits
Symmetric bilateral — 50 ±0.1: 49.9 to 50.1. The most common form.
Asymmetric bilateral — 50 +0.2/−0: only oversize is permitted. Useful when one side must never go under.
Unilateral — 50 +0.3/+0.1: both limits on one side. For particular fits.
Standard fits — Ø40 H7: instead of writing numbers you use the ISO system. Capital letter for holes, lowercase for shafts. For rotational parts this is both more professional and more precise.
A worked example
A flange specified as:
Ø176 ← outside diameter, general tolerance is fine
Ø68 H7 ← central bore, a bearing sits in it
4× Ø18 ← bolt holes, general tolerance
Ø140 ±0.1 ← bolt circle, must match the mating part
32 ±0.1 ← thickness, affects assembly height
Ra 0.8 ← on the central bore only
Three of six callouts carry a specific tolerance. The rest come from the general table. That drawing is both accurate and inexpensive.
The point
A tolerance is an engineering decision, not a habit. Every number you put on a drawing should have a reason you can state out loud.
If you cannot explain why a face needs ±0.02, it probably does not.
The next step is GD&T — the system that controls form and position rather than dimensions alone.