Conventional tolerances
Control part size. They developed first, are easier to apply and interpret, and remain the more widely used of the two. For a rectangle, the width and height are controlled conventionally.
First principles
Variability is inherent, not exceptional
Manufacturing cannot produce a perfect form. The sources of variation are numerous and unavoidable: the skill of the machine operator, the accuracy and age of the machine, ambient conditions, and the condition and age of the cutting tool. Producing parts with exact dimensions would be impossible and, if approached, prohibitively expensive.
The engineering response is therefore to control variability rather than eliminate it. Alongside the physical measures — training operators, maintaining machines and tools — sits the design measure: specifying an acceptable range of variation for each dimension such that the part still performs its intended function. That range is the tolerance.
Tolerance is a cost decision
Every reduction in tolerance raises the cost of manufacture, the cost of inspection, and the scrap rate. Every increase raises the risk of assembly failure. A tolerance chosen without reference to function is either wasting money or accumulating risk, and in a large assembly it is frequently doing both.
Two families
Conventional and geometric tolerances
Geometric tolerances
Control part form — shape, orientation, location and runout. For the same rectangle, the corner angles and the parallelism of opposite sides are controlled geometrically.
Both are used for inspection after manufacture. Off-the-shelf inspection gauges check whether parts fall within the specified limits, the go/no-go gauge being the familiar example. A part that fails inspection is rejected and becomes scrap; a high scrap rate makes manufacturing more expensive and signals that the process needs better control. Inspection is one element of quality control and quality assurance, alongside visual inspection and surface roughness measurement.
Vocabulary
Concepts that have to be exact
These definitions come from the dimensioning and tolerancing standard, and using them loosely is the origin of a great deal of confusion.
- Nominal size
- A size without decimals — for example, 5.
- Basic size
- A nominal size written with decimals to indicate the required accuracy. 5.0, 5.00 and 5.000 share a nominal size but are not the same specification; they demand one, two and three decimal places of accuracy respectively.
- Actual size
- The measured value on the manufactured part. It must fall within the specified tolerance on the basic size, or the part is rejected at inspection.
- Maximum material condition (MMC)
- The limit of size at which the feature contains the most material — the largest permissible shaft, the smallest permissible hole.
- Least material condition (LMC)
- The converse — the smallest shaft, the largest hole.
- Datum
- A reference from which dimensions are measured. A datum is always an actual face of a part.
- Datum target
- A designated point, line or area of contact used to establish a datum. These are needed because a whole face cannot serve as a datum in practice: real faces are irregular, and inspection must contact them at defined locations to be repeatable.
Notation
Four ways to express a tolerance
| Method | Form | Practical note |
|---|---|---|
| Limit dimensioning | The minimum and maximum permissible values, shown one above the other. | Use maximum material condition to present the limits: for a shaft show the maximum above the minimum, and for a hole the reverse. The machinist naturally works to the value above the dimension line first, and this ordering minimises scrap — material can always be removed later, never added back. |
| Plus and minus | Basic size followed by a tolerance, bilateral or symmetric. | The most widely practised method, because machinists prefer it — the target is the basic size and the deviation is explicit. |
| Note against specific dimensions | A drawing note naming the dimensions it governs. | Useful for families of similar features; risky if the note and the dimensions drift apart across revisions. |
| General note or title block | A blanket tolerance by decimal place, applying to everything not otherwise toleranced. | Essential, and frequently the only tolerance a dimension ever receives. Set it deliberately in the template. |
Standardisation
Standard fits and limits of dimensions
Two questions sit behind standardised tolerances: why standardise, and how are the limits then calculated? Standardisation exists to make manufacture and inspection consistent, which in turn ensures interchangeability — the guarantee that a replacement part will fit as intended. Both ANSI and ISO have developed equivalent systems of standard classes of fit, each carrying standard tolerances that depend on the basic size being toleranced.
Clearance fits
A gap always exists between shaft and hole across the whole tolerance range. Running and sliding applications.
Transition fits
The assembly may end up with either a small clearance or a small interference, depending on where in the range the two parts fall. Location applications where accuracy matters more than free movement.
Interference fits
Interference always exists; assembly requires force, heat or cold. Used where the joint must transmit torque or resist separation without a fastener.
Method, not memorisation
The published fit tables are the authoritative source and should be consulted directly rather than reproduced from memory or from a secondary text. The engineering skill is choosing the right class of fit for the function and then looking up the correct values for the basic size in hand — and confirming which of the two systems, ANSI or ISO, the drawing is being produced under.
Accumulation
Tolerance accumulation and the dimensioning scheme
Accumulation — stack-up — is the chain effect of a series of tolerances, and it is controlled entirely by how the part is dimensioned.
Chain dimensioning
Each feature dimensioned from the previous one. The variation between the first and last features is the sum of every tolerance in the chain. Produces the maximum possible accumulation.
Baseline dimensioning
Every feature dimensioned from one common datum. Variation between any two features is limited to the combination of their two tolerances rather than the whole chain.
Direct dimensioning
The functionally critical distance is dimensioned directly, so it carries exactly the tolerance the designer assigned and nothing more.
Worked comparison
Take four components, each held to ±0.05 mm, stacked along one axis:
The worst-case method assumes every component sits at its extreme simultaneously and gives the assembly tolerance as the linear sum of the component tolerances. The statistical method combines them as the square root of the sum of the squares, on the reasoning that all components reaching their extreme in the same direction at once is vanishingly unlikely. For four equal tolerances the RSS result is half the worst case; for three it is about 58 per cent, and for six about 41 per cent.
Choose the method honestly
Worst case guarantees assembly and costs money. Statistical buys tolerance back but accepts a calculable rate of assemblies that will not go together, and it assumes the underlying processes are centred and in statistical control. Use worst case for safety-critical stacks and low volumes; use statistical for high volume production where the process capability is actually known and monitored.
Distribution
Statistical tolerancing
Specifying a tolerance on a dimension generates a normally distributed population of parts. The horizontal axis is the produced dimension and the vertical axis the probability of producing it. The mean of the distribution is the perfect form — the basic size. The two extremes correspond to the maximum and minimum sizes, and therefore to the maximum and minimum material conditions.
The distance from the mean to either extreme is conventionally three standard deviations. The area under the curve bounded by ±3σ contains 99.73 per cent of all parts produced under common-cause variation — which is to say roughly 2,700 parts per million will fall outside the specified limits even when nothing is going wrong. Tightening the process capability so that the specification limits sit at six standard deviations reduces that to a few parts per billion, which is the origin of the six sigma terminology.
Geometric tolerancing
True position, and why coordinate tolerancing under-controls
A hole has a size and a location. Tolerancing the size is straightforward and conventional. Tolerancing the location depends on how the centre is defined — and the intuitive approach turns out to be wrong.
Locating the centre by x and y coordinates and applying a tolerance to each produces a rectangular tolerance zone measuring 2Δx × 2Δy. The hole centre may sit anywhere in that rectangle, including at a corner — which is further from nominal than the designer intended. The permitted radial deviation along the diagonal exceeds the permitted deviation along either axis.
The arithmetic, for ±0.10 mm on each axis
| Quantity | Coordinate tolerancing | True position |
|---|---|---|
| Zone shape | Square, 0.200 mm on a side | Cylinder, 0.283 mm diameter |
| Zone area | 0.0400 mm² | 0.0628 mm² |
| Maximum radial deviation | 0.141 mm at a corner | 0.141 mm in every direction |
| Available tolerance | Baseline | 57 per cent greater, for the same worst-case deviation |
Replacing the square zone with a cylindrical zone whose diameter equals the square's diagonal keeps the worst-case deviation identical while increasing the usable tolerance area by about 57 per cent. Nothing has been given away; the zone has simply been made the right shape for a round feature.
The symbol set
Geometric tolerance categories
Geometric tolerances complement conventional ones by controlling location, form and profile of individual features. They divide by whether they apply to a feature on its own or in relation to a datum.
Geometric tolerance categories
Form — individual feature Straightness, flatness, circularity
(roundness), cylindricity. No datum required.
Profile — individual or related Line profile, surface profile.
Datum optional depending on what is being controlled.
Orientation — related Angularity, perpendicularity,
parallelism. Datum required.
Location — related Position, concentricity. Datum
required.
Runout — related Circular runout, total runout. Datum axis
required.
Applying a geometric tolerance
- Step 1 Specify the datums that dimensions will be measured from.
- Step 2 Decide which type of geometric control the feature actually needs.
- Step 3 Build the feature control frame: symbol, tolerance zone value, optional diameter symbol, material condition modifier, then the datum references in order.
- Step 4 Attach it to the feature, not to a dimension, and confirm the datum scheme is repeatable in inspection.
Interpretation is the whole point
The underlying principle is uniform: a tolerance defines a zone, and the toleranced feature may take any position and orientation within that zone. A flatness callout of 0.35 means the entire surface must lie between two parallel planes 0.35 apart. A position callout with a diameter symbol means the feature axis must lie within a cylinder of that diameter. Every geometric tolerance can be read this way, and reading it this way removes most of the mystique.
In the CAD system
Automated tolerance analysis
Tolerance studies come in two directions. Analysis — stack-up analysis — starts from known component tolerances and calculates the resulting assembly tolerance. Synthesis, or allocation, runs the other way: the assembly tolerance is known from design requirements and must be distributed sensibly among the components.
CAD tolerance analysis modules implement the analysis direction. A study is built in four steps: establish the measurement, which is a linear distance between two features; select the ordered set of parts forming the tolerance chain; define the assembly constraints; and evaluate. The output is a minimum and maximum worst-case stack, a minimum and maximum root-sum-squared stack, and a ranked list of the contributing features and tolerances.
Prepare the parts first
Automated stack-up depends on the parts carrying machine-readable tolerance data. A dimensioning module that inserts dimensions and tolerances onto manufacturing features such as holes and slots is normally used to prepare parts before the stack-up study will recognise anything. Learn that step first; the analysis is straightforward once the inputs exist.
Key takeaways
- Variability is inherent; tolerancing controls it rather than eliminating it, and every tolerance is a cost decision.
- Conventional tolerances control size; geometric tolerances control form, orientation, location and runout.
- Nominal, basic and actual sizes are distinct — the number of decimal places in a basic size is itself a specification.
- Order limit dimensions by maximum material condition to minimise scrap.
- Dimensioning scheme determines accumulation: chain is worst, baseline better, direct best for the critical distance.
- Worst-case stack-up is the arithmetic sum; RSS is the square root of the sum of squares and is only valid where processes are centred and capable.
- True position replaces a square coordinate zone with a cylindrical one, gaining about 57 per cent more usable tolerance at the same worst-case deviation.
- Every geometric tolerance defines a zone within which the feature may lie; read them that way.
Series
Continue the pathway
The SOLIDWORKS Design Approach series works through computer aided design as an engineering discipline, from first principles to manufacture.
KEVOS®
Precision to Vision
Engineering · Mechanical Engineering
Written by Kevin Jogin
10 min read