What are tolerances? How much a dimension may vary, and what it costs
What are tolerances? A tolerance is the amount a dimension on a part may vary from its stated size and still be accepted. This guide covers how tolerances are written, where general tolerances come from, what common processes hold and why tighter ones cost more.
What a tolerance is
WisTech Open’s blueprint reading text defines tolerance as the allowable variation from a specified dimension. No part comes out at its exact theoretical size, so every dimension needs a range the part can fall within and still work.
The range has two ends. The upper limit is the largest size accepted and the lower limit the smallest, and the tolerance is the difference between them. A 25.00 mm dimension written ±0.05 accepts any part from 24.95 to 25.05 mm, a total tolerance of 0.10 mm.
Tolerances let parts fit and work together, let parts made at different times replace each other, and tell the inspector what to accept. A dimension with no tolerance of its own takes the general tolerance from the title block.
How a tolerance is written
The same range can be written in several forms, and WisTech Open’s text names each one.
−0.10
−0.05
24.95
- Equal bilateral. The size may vary by the same amount above and below the dimension, as in 25.00 ±0.05.
- Unequal bilateral. It varies both ways by different amounts. 25.00 +0.05 −0.10 accepts 24.90 to 25.05.
- Unilateral. It varies one way only, with zero on the other side. 25.00 +0 −0.05 accepts 24.95 to 25.00.
- Limit dimensions. The drawing gives the two limits instead of a plus-minus value, with the upper limit above the lower one.
- Single limit. Only a minimum or a maximum, written MIN or MAX, often on hole depths, thread lengths, radii and chamfers.
Two forms can describe the same range. A dimension of 25.00 ±0.05 and limits of 25.05 over 24.95 accept exactly the same parts.
General tolerances and the title block note
Many dimensions on a drawing carry no tolerance of their own. They take the general tolerance stated in the title block or a general note, which WisTech Open’s text calls unspecified tolerances.
On inch drawings, the note sets the tolerance by the number of decimal places, with separate values for fractions and angles. NASA Goddard’s drawing standards manual shows a sample that reads: unless otherwise specified, dimensions in inches, .XX ±.02, .XXX ±.005, angles ±1° and fractions ±1/16. WisTech Open’s title block example gives ±0.010 on three-place dimensions instead, so read the note on every drawing.
A metric drawing can cite a standard instead. ISO describes ISO 2768-1 as general tolerances in four tolerance classes, for parts made by metal removal or formed from sheet metal. BSI’s summary of the European edition, BS EN 22768-1, lists what it covers: external and internal sizes, diameters, radii, distances and chamfer heights. It excludes auxiliary dimensions in brackets and theoretically exact dimensions in frames.
Check the rest of the note too. ISO lists ISO 2768-2, the part for general geometrical tolerances, as withdrawn and revised by ISO 22081:2021. A drawing that still cites ISO 2768-2 points to a part ISO no longer lists as current.
Before you quote, read the units, the decimal places and any standard named in the tolerance note. Together they set the tolerance on every dimension that has none of its own. The title block guide shows where that note sits.
If you make the drawing yourself from a 3D model, the STEP to DXF converter lays out three views with overall dimensions. The tolerances are yours to add, and the general note covers every dimension you leave without one.
Fits between a hole and a shaft
A fit is how two mating parts go together, such as a pin in a hole. WisTech Open’s text describes two kinds. In a clearance fit, the inner part is smaller than the hole. In an interference fit, also called a press fit, it is larger.
ISO 286-1 sets the ISO code system for tolerances on linear sizes. It also defines the terms for fits and explains the basic hole and basic shaft principles. Sandvik Coromant’s drilling guide puts the code in practical terms. The IT grade is the width of the tolerance band. The letter is its position, a capital for a hole and a lower-case letter for a shaft. In H, the band runs from zero to plus.
The same guide places the common fits on one line: running fit, slide fit, drive fit and interference. The line runs from a hole larger than its shaft to a shaft larger than its hole. The fits at the first end give play, as in bearings. Those at the other end grip, as in fixed joints.
Geometric tolerances
A plus-minus tolerance controls size. GD&T adds controls for form, orientation, location and runout, each written in a feature control frame. ASME describes Y14.5 as establishing the symbols, rules and definitions for stating and interpreting GD&T. ISO 1101 defines the symbol language for the geometrical specification of workpieces.
One GD&T idea changes how a shop reads a hole: material condition. At maximum material condition, a hole is at its smallest size and a shaft at its largest. In WisTech Open’s example, a position tolerance of ⌀0.03 at the smallest hole size grows to ⌀0.04 when the hole is at its largest.
Engineering drawing symbols shows every characteristic symbol and how to read the feature control frame.
Tolerances by process
How tight a tolerance a shop can hold depends on the process. For holes, Sandvik Coromant, a cutting tool maker, publishes the tolerance its tools reach. Its drilling guide gives the width of each IT grade, and notes that the lower the IT number, the closer the tolerance.
| Process | Sandvik source | Hole tolerance | Band at 18 to 30 mm |
|---|---|---|---|
| Drilling, exchangeable-tip drill | CoroDrill 870 | H9 to H10 | 0.052 to 0.084 mm |
| Rough boring | Boring guide | IT9 or wider | 0.052 mm or more |
| Drilling, solid carbide drill | CoroDrill 860 | H8 to H9 | 0.033 to 0.052 mm |
| Reaming | CoroReamer 835 | H7 | 0.021 mm |
| Finish boring | Boring guide | IT6 to IT8 | 0.013 to 0.033 mm |
A reamed H7 hole holds a 0.021 mm band at that size. A hole from an exchangeable-tip drill holds 0.052 to 0.084 mm. Sandvik’s guides treat reaming and finish boring as finishing operations on a hole that already exists, so the tighter band takes a second tool.
The units matter as much as the number. At 20 mm, ±0.01 mm is a band of 0.02 mm, close to IT7 in Sandvik’s table, the grade a reamer holds. In inches, ±0.01 in is a band of 0.02 in, about 0.51 mm, wider than any drill’s range in the table.
For sheet metal, castings and molded parts, ask the process supplier which tolerances it holds, and put them in writing on the quote.
Why tighter tolerances cost more
WisTech Open’s text is direct about cost. The tolerance on a part directly affects what it costs to make. A tolerance closer than the part’s function needs raises the cost through extra time and often extra processes.
The hole table shows where that cost comes from. Moving a hole from H9 to H7 adds a reaming or boring pass after the drill.
Stack-up adds to it. WisTech Open’s text shows tolerances accumulating when one length is calculated from others: four chained lengths at ±0.01 give an overall length of ±0.04. Holding a tight overall length through a chain means tightening every link in it.
For an estimator, each tight tolerance is a cost driver to find before pricing. List the tightest tolerances on the drawing, the operation each one needs and the inspection it requires, then price those operations into the quote. Costing vs pricing covers how those operations become a cost, and the RFQ guide covers where they fit in a quote.
When a product is configured from rules, its drawing can come from the same rules. Turning your Excel builder into a CPQ app generates the quote drawing in your title block, with the dimensions the customer checks. A named person approves each one.