Tight tolerances cost more because they slow the cut, add set-up care and inspection, and raise the share of parts that are scrapped. Moving from a general tolerance to a few hundredths of a millimetre on several features can easily double the machining cost of a part. The fix is to keep tight tolerances on the features that mate with something and let everything else default to a general standard.
Key points
- Most dimensions can follow a general standard such as ISO 2768-m; only mating features need tighter values.
- Each step tighter adds finishing passes, inspection time and scrap risk, and the cost curve is steep.
- Tolerance and surface finish usually travel together, and both add time.
- Geometric tolerances (GD&T) and very tight values usually mean a drawing and a manual review.
- Before you send a part, ask which features actually touch another part.
What a tolerance is, and what “general” means
A tolerance is the amount a dimension may vary and still be acceptable. A hole drawn at 10 mm with ±0.05 mm may measure anywhere from 9.95 to 10.05 mm. No machine makes parts exactly to size; the tolerance tells the shop how close it needs to get.
Most drawings do not tolerance every dimension individually. Instead they cite a general tolerance standard, such as ISO 2768, in the title block. Any dimension without its own tolerance follows the class named there: f (fine), m (medium), c (coarse) or v (very coarse). The permitted deviation grows with the size of the feature, so a 500 mm length gets more room than a 5 mm one. ISO 2768-m is a common default for machined parts.
GD&T (geometric dimensioning and tolerancing) goes further: flatness, perpendicularity, position, concentricity and so on. It describes how features relate to each other, which a plus-or-minus value cannot.
Why tighter costs more
Each step tighter adds work in several places at once.
| Where the cost appears | General tolerance | Tight tolerance |
|---|---|---|
| Cutting | Roughing and one finishing pass | Extra semi-finishing and finishing passes, lighter cuts |
| Tools | Standard tools, normal wear limits | Sharper tools changed sooner, sometimes reamers or boring heads |
| Set-up | Standard workholding | More careful alignment, possibly a dedicated fixture |
| Machine | Any capable machine | A machine known to hold the band, warmed up, sometimes in a controlled room |
| Inspection | Calipers and gauges, sample checks | Bore gauges or a CMM, every part, with a report |
| Scrap | Rare | More parts fall outside the band and are rejected |
The first-article check makes this worse on small batches. Proving out a tight-tolerance part takes longer, and that time is part of the set-up cost, paid once per batch. Our article on CNC set-up time shows how that fixed time dominates small orders.
How the bands compare
The table gives a rough sense of what each band means on the shop floor. The boundaries are approximate and depend on the material, the feature size and the machine; treat them as a guide, not a specification.
| Tolerance on a small feature | What it usually takes | Relative effort |
|---|---|---|
| General, e.g. ISO 2768-m | Normal machining, hand-tool checks | Baseline |
| About ±0.05 mm | Careful finishing pass, measured with calipers or gauges | Modest increase |
| About ±0.025 mm | Dedicated finishing, bore gauges, more frequent checks | Noticeable increase |
| About ±0.01 mm or tighter | Reaming, boring or grinding, stable temperature, CMM inspection | Large increase, often a review |
Material matters too. Aluminium is easy to hold to size but moves with temperature. Plastics creep, absorb moisture and spring back after clamping, so tight tolerances on plastic parts are harder than the same numbers on metal. Thin walls deflect under the cutter and are hard to hold to any tight value.
Surface finish travels with tolerance
A tight tolerance on a rough surface is hard to measure and hard to hold, so tight tolerances usually come with a finer surface roughness requirement. A typical as-machined finish is around Ra 3.2 µm. Asking for Ra 1.6 or 0.8 µm means slower finishing passes, and finer still may mean grinding or polishing. Like tolerance, surface finish should be called out only where it matters: a sealing face or a sliding fit, not the whole part.
Worked example: the same part at two tolerance levels
The figures are illustrative assumptions, not market rates. A batch of 10 aluminium parts runs at €80 per hour. Version A uses ISO 2768-m throughout. Version B puts ±0.01 mm on four bores.
Worked example: cost per part, batch of 10 (illustrative rates)
| Line | Version A: general tolerance | Version B: four bores at ±0.01 mm |
|---|---|---|
| Base cycle time | 30 min × €80/h = €40.00 | 30 min × €80/h = €40.00 |
| Extra finishing passes | none | 4 bores × 3 min = 12 min × €80/h = €16.00 |
| Inspection | included in handling | CMM, 15 min × €60/h = €15.00 |
| Longer first-article check | none | 0.5 h × €80/h = €40.00 ÷ 10 parts = €4.00 |
| Subtotal | €40.00 | €75.00 |
| Scrap allowance | none | 5% of €75.00 = €3.75 |
| Cost per part | €40.00 | €78.75 |
Four tight bores nearly doubled the cost per part: €78.75 against €40.00. The scrap allowance is an assumption; a shop should use its own reject rate for the feature type. If only two of the four bores carry a bearing and the other two are clearance holes, loosening those two removes half the finishing and much of the inspection.
Stack-up: why one tight value can force others
Tolerances add up. If a bolt passes through three parts, the position of the hole in each part varies, and the variations combine. Designers sometimes respond by tightening every dimension in the chain, which multiplies the cost. Two better answers exist: dimension each feature from one common datum, so errors do not accumulate along a chain of dimensions, and open up the clearance hole instead of tightening its position. A slightly larger clearance hole is free; a tighter position on four parts is not.
The same logic applies inside one part. A feature dimensioned from another feature inherits that feature’s error. Dimensioning from the faces the part locates on keeps each tolerance independent.
When to loosen a tolerance
Tolerances are often tighter than they need to be because a CAD template applies one value to everything, or because the designer copied a previous drawing. Go through the dimensions and ask what each feature does.
| Feature | Usually needs | Usually fine at general tolerance |
|---|---|---|
| Bearing seats, press fits | Tight diameter and roundness | |
| Locating holes and dowel holes | Tight position | |
| Sealing faces | Flatness and finish | |
| Clearance holes for bolts | Yes | |
| External outline, non-mating | Yes | |
| Weight-saving pockets | Yes | |
| Chamfers, radii, cosmetic faces | Yes |
Two more habits help. Tolerance the function, not the shape: a positional tolerance on a hole pattern says what matters better than tight plus-or-minus values on every coordinate. And put tight tolerances on as few set-ups as possible: two features that must line up should be machined in one clamping where the design allows. The design for CNC machining guide covers this and other DFM habits.
How tolerances show up in a quote
An estimator reads the drawing, counts tight features and adds time for each. Instant quoting software for machining does the same with an explicit structure: the buyer picks a general class, adds counts of features at tighter values, and anything with GD&T or very tight values is routed to a person, with a drawing required. The CNC machining cost guide shows where this sits in the full estimate, and the CNC milling page describes how Quotometry prices it: the buyer picks one of the shop’s tolerance classes, each class slows finishing and adds inspection, and a class the shop marks for review sends the line to a person. Quotometry does not read GD&T from a drawing.
Questions people ask
What is a standard CNC machining tolerance?
Many shops work to a general tolerance standard such as ISO 2768-m (medium) for any dimension without its own tolerance on the drawing. In the medium class that is ±0.1 mm on dimensions up to 6 mm and ±0.2 mm from 6 to 30 mm, growing with size. Tighter values on specific features are possible, but each one costs something.
Why do tight tolerances cost more?
Holding a tight tolerance takes lighter finishing passes, more careful set-ups, temperature control, sharper tools and more measurement, often on a CMM rather than with hand tools. Scrap rises because more parts fall outside the band. Each of these adds time, and machining time is charged by the hour.
Which tolerances can I loosen without affecting function?
Usually the dimensions that do not touch another part: external outlines, pocket depths that only remove weight, clearance holes, chamfers and cosmetic faces. Keep tight tolerances on bearing seats, locating holes and mating faces. Asking which features actually fit against something is the quickest way to find dimensions that are tighter than they need to be.
Do I need a drawing if I upload a 3D model?
If every feature can be made to a general tolerance, a 3D model is often enough. If any feature needs a tighter tolerance, a thread, a surface finish or a geometric tolerance, send a drawing that calls it out: the model shows shape, not the accuracy you need. Shops usually route parts with drawing-only requirements to manual review.
Quotometry prices every part from your own machines and rates, on your website, in seconds.