Geometric Dimensioning and Tolerancing

This is a learning note, not a handbook. The thesis of this file is that tolerancing is the place where design intent meets what a machine shop can actually hold. The gap between those two points is where most mechanical failures of assembly (not of strength) are born. GD&T is, in this framing, less a notation than a contract language.[fn:: A cynic would say it is a litigation language. The standards exist largely so that when a part arrives out of spec the buyer and the supplier can agree on whose fault it is. This is not wrong, but it is incomplete. The same contract language lets you write a better contract in the first place.] It is worth learning precisely because the cost of not learning it is paid in weeks of delay rather than in textbook exercises.

Intuition

A drawing with nominal dimensions and a generic plus or minus 0.1 mm tolerance is a lie of omission. It says nothing about which surfaces the tolerance is measured from, whether the tolerance zone is cylindrical, planar, or volumetric, whether a hole position may float outward as the hole grows, or whether form, orientation, and location are controlled independently or jointly.

The classical plus-or-minus tolerancing scheme answers none of these questions. It breaks down the moment a part has more than two functional features. Consider a plate with four bolt holes. Under plus-or-minus tolerancing, the holes individual positions are bounded. The pattern as a whole is uncontrolled. The worst case pushes all four holes to the same corner of their boxes. That configuration will not assemble with a mating four-hole flange even though every hole is in spec. GD&T exists to control the things plus-or-minus cannot. It controls the relationship of features to each other and to a defined reference frame.

When ambiguous tolerancing bites, it bites late. The part passes incoming inspection. The inspector measures what the drawing literally says. The part reaches assembly and fails to mate. Root-causing it then costs a week of meetings, a fixture re-machining, and a drawing revision that should have existed on the first print. The leverage here is high because the mistake is cheap to make and expensive to discover.[fn:: This is a general pattern in engineering. Errors that propagate downstream compound. A bad tolerance decision is a 10-minute decision whose consequence is a 10-day problem. The ratio is what makes it worth studying, not the absolute importance of the topic.] The rest of this note is the vocabulary you need to make that 10-minute decision better.

First principles

Datums and the datum reference frame

A datum is a theoretically exact point, line, or plane derived from a datum feature on the part. The datum reference frame (DRF) is the ordered set of datums. The primary datum is A, the secondary is B, and the tertiary is C. These three datums together fix six degrees of freedom. They define the coordinate system in which all geometric controls are evaluated. The order matters. The primary datum establishes three degrees of freedom as a plane. The secondary datum establishes two more degrees of freedom as a line on that plane. The tertiary datum establishes the last degree of freedom as a point on that line.[fn:: Some texts say primary equals 3 DOF, secondary equals 2, tertiary equals 1, summing to six. This is a mnemonic, not a derivation. The real content is that each successive datum removes the DOF the previous ones did not constrain. Mixing up precedence is the single most common error in reading a GD&T callout. It changes the tolerance zone shape, not merely its size.]

The DRF is not optional flourish. Without it, position is undefined. Position relative to what? Every location control on a drawing presupposes a DRF. The question is only whether the drafter wrote it down.

The fourteen geometric controls

ASME Y14.5 defines fourteen geometric characteristic symbols, organized by what they control:

Two structural facts are worth memorizing:

1. Form controls never need a datum. Flatness is intrinsic to a surface. A surface cannot be flat relative to datum B. This is a frequent drafter error and a frequent inspection error. It is uncheckable if a datum is wrongly invoked. 2. Profile is the universal control. Profile of a surface can, in principle, replace most other controls. It is the only control that can bound a complex freeform. The Y14.5-2018 revision leans on profile more heavily than earlier editions. ISO 1101 leans on it even more. The practical reason not to use it everywhere is that it is harder to inspect and harder to read on a drawing. Optimize for the reader, not for the elegance of the notation.

Concentricity and symmetry were removed from Y14.5 in 2018. They are statistically hard to inspect because they require median-point fitting. Position with MMC achieves the same functional intent more cheaply.[fn:: This is a rare case of a standard deleting a control rather than adding one. The lesson is that GD&T is not a fixed ontology. It is a moving target. Citing Y14.5 without a year is a tell that the speaker has not read the revision notes.] They survive in ISO 1101 and in legacy drawings. Expect to meet them. Do not expect to write them.

Material condition modifiers and bonus tolerance

Every feature of size (a hole, shaft, slot, tab) has a material condition. Least Material Condition (LMC) is the state of being as large as possible while still leaving the most material on the part. Maximum Material Condition (MMC) is the state of being as small as possible while still removing the most material (for a hole) as the largest as possible for a shaft. The naming is from the part perspective. At MMC a hole is at its smallest and a shaft at its largest.

The modifier symbols M (MMC, a circled M) and L (LMC, a circled L) appended to a tolerance allow the geometric tolerance to grow as the feature departs from the extreme material condition. This bonus tolerance exists because a hole that is larger than its MMC is easier to assemble through. The functional constraint is will it assemble, not is it at the extreme.

For a position callout position diameter 0.2 M on a hole diameter of 10.0 plus 0.1 minus 0:

• At MMC (diameter 10.0), bonus equals 0. The total position tolerance is diameter 0.2.
• At LMC (diameter 10.1), bonus equals 0.1. The total position tolerance is diameter 0.3.

The bonus is exactly the departure from MMC. This is not a fudge. It is the formal recognition that the worst case for assembly is when the hole is smallest. A bigger hole buys you positional freedom in equal measure. The common error is to assume bonus tolerance always helps. It helps the manufacturer because more parts pass. It is neutral-to-helpful for the function because assembly is the function. It is harmful to the analyst if you do a stack-up and forget that the bonus is conditional on the as-produced size.[fn:: The asymmetry is the point. Bonus tolerance shifts scrap rate down while shifting the variance of the as-built assembly up. Whether that matters depends on whether your downstream analysis cares about the mean or the tail. In a clearance fit it usually does not. In a kinematic linkage it sometimes does.]

Fits: clearance, transition, interference (ISO 286 / ANSI B4.2)

A fit is the paired specification of a hole tolerance and a shaft tolerance, written as H7/g6 (hole basis) or g7/h6 (shaft basis). The capital letter is the hole. The lowercase letter is the shaft. The number is the IT grade (fundamental tolerance grade). The hole-basis system is far more common because it is cheaper to make a shaft to a non-standard size than to ream a non-standard hole.

ISO 286 defines IT grades from IT01 (tightest) to IT18 (loose). The grade sets the tolerance magnitude as a function of nominal size. The letter sets the position of the tolerance band relative to the nominal. This position is called the fundamental deviation. A few useful anchors:

The H fundamental deviation is zero. The hole lower limit is the nominal value. H7/g6 and similar are almost all hole-basis. The fit class is determined by the relationship of the shaft band to the hole band. Clearance means the shaft is entirely below the hole. Transition means the bands overlap. Interference means the shaft is entirely above the hole.

Surface finish: Ra, Rz, Rt

Surface finish is a tolerance on geometry at short wavelength. It is independent of and typically much tighter than the macro-form controls above. The common parameters:

• Ra (arithmetic mean roughness): the average absolute deviation from the mean line. Cheap to measure, ubiquitous, and almost information-free. Two surfaces with the same Ra can have wildly different bearing capacity.
• Rz (ten-point height): average of the five highest peaks and five lowest valleys over a sampling length. More sensitive to extremes than Ra.
• Rt (maximum peak-to-valley): the single worst excursion in the evaluation length. Relevant for fatigue and sealing.

A specification of Ra 1.6 without a cutoff length, a measurement direction, and a functional rationale is a guess.[fn:: ISO 4287 and ISO 4288 specify the sampling and cutoff conventions. ASME B46.1 is the US analogue. They disagree on defaults. A drawing that does not declare which standard it is using is, again, a contract waiting to be litigated.] As a rule of thumb Ra correlates loosely with process: turning gives approximately 0.8 to 3.2, grinding gives approximately 0.2 to 0.8, lapping gives less than 0.1, and casting gives more than 6.3. The right way to set a finish spec is from the function (sealing, sliding, fatigue) backwards, not from the process forwards.

Stack-up analysis: worst-case vs RSS

A tolerance stack is the propagation of dimensional variation through a chain of features. Two methods dominate:

• Worst-case (WC): assume every contributor sits at its worst-case extreme simultaneously in the direction that maximises the output. The total is the arithmetic sum of the individual tolerances. Conservative. It guarantees assembly if every part is in spec. It is uneconomic for chains longer than about four features because the probability of all extremes co-occurring is astronomically small.
• Root-sum-square (RSS): assume each contributor is Gaussian and independent, so variances add. Total tolerance equals the square root of the sum of squares. Much tighter than WC. It reflects the typical assembly. It is wrong whenever the independence or Gaussian assumptions fail.

A practical rule: use RSS for cost-driven design. You accept a small scrap rate and tune the tolerances to a target yield. Use WC for safety-critical or low-volume hardware. One failure is too many, and the economic loss from a WC spec is bounded. The hybrid approach (RSS with a safety factor, or RSS times 1.5) is common in industry. It is honest about the fact that neither pure method is calibrated to reality.[fn:: The Monte Carlo stack, sampling each contributor from its actual measured distribution rather than a Gaussian, is the rigorous version of RSS. It is cheap to run in 2026. The main reason it is not standard practice is institutional inertia, not technical difficulty. If you have measured distribution data, use it.]

Worked example

A clearance fit: H7/g6 on a 25 mm shaft/hole

Nominal diameter is 25 mm. ISO 286 gives, for nominal in the 18-30 mm band:

• IT7 equals 21 um, IT6 equals 13 um.
• H fundamental deviation (hole) is 0. Lower limit is 25.000.
• g fundamental deviation (shaft) is -7 um. Upper limit of shaft is 25.000 minus 0.007 equals 24.993.

So:

Clearances:

• Maximum clearance equals hole max minus shaft min equals 25.021 minus 24.980 equals 0.041 mm (41 um).
• Minimum clearance equals hole min minus shaft max equals 25.000 minus 24.993 equals 0.007 mm (7 um).

This is a running fit (always clearance, never interference). It is suitable for a lightly-loaded journal at moderate speed. The 7 um minimum clearance is what you must keep free for the lubricant film. If your bearing design needs more, pick H8/f7 (minimum clearance 20 um) instead. The leverage of the fit choice over bearing life is large. The leverage of holding the tolerance one grade tighter is small and very expensive.

A three-feature stack: worst-case vs RSS

Consider a stepped shaft with three axial dimensions contributing to an overall length L:

• Worst-case: |0.1| + |0.15| + |0.1| + |0.05| equals 0.40 mm. So L total equals 75 plus or minus 0.40.
• RSS: square root of (0.1 squared + 0.15 squared + 0.1 squared + 0.05 squared) equals square root of 0.045, which is approximately 0.212 mm. So L total is approximately 75 plus or minus 0.21.

The RSS answer is roughly half the WC answer. If you designed to WC you would either over-tolerance every component (driving cost up) or accept a small fraction of non-conforming assemblies. The choice between WC and RSS is therefore not a technical choice. It is an economic and risk choice disguised as a technical one.

Tolerance zone schematic

Pitfalls

The high-leverage mistakes, roughly in order of cost:

1. Mixing datum precedence. A callout that reads A primary, B secondary produces a different tolerance zone from B primary, A secondary. The zones are not smaller or larger. They are differently shaped. Reading the precedence wrong is not a minor error. It changes what the part must be. Treat the order of letters in a feature control frame as load-bearing.

2. Assuming bonus tolerance always helps. It helps the maker. It can hide functional variation from the analyst. If you do a stack-up and take the bonus at its maximum (LMC) without modelling the size-position correlation, you have assumed the worst case twice in opposite directions. Your answer is internally inconsistent.

3. Treating worst-case stack-up as a design target. WC is a guarantee, not a specification. Designing every chain to WC yields parts that are over-toleranced by a factor of two to four. The cost scales roughly as the inverse square of the tolerance band. This is the single most common way mechanical designs become unaffordable.

4. RSS where the assumptions fail. RSS assumes each contributor is Gaussian and independent. Real manufacturing distributions are bounded (so not Gaussian in the tails) and often correlated (a single setup error shifts multiple features together). RSS on a correlated stack underestimates the true spread, sometimes badly. If you have measurement data, fit it. If you do not, at least inflate the RSS estimate by a factor that accounts for what you do not know.

5. Surface finish spec without a function. Ra 1.6 on every surface is not a spec. It is a default. The bearing journal needs Ra 0.4 or better, with Rz controlled. The non-functional cosmetic face needs Ra 3.2. The sealing land needs a lay direction specified. Specifying all surfaces to the tightest functional need is a tax on every part for no benefit.

6. Ignoring the ASME / ISO split. ASME Y14.5 and ISO 1101 agree on the symbols and concepts. They diverge on defaults and on edge cases. The meaning of a tangent plane modifier, the treatment of composite profile, and the rules for symmetry all differ. A drawing that mixes callouts from both without stating which governs is ambiguous in the strictest sense. A court would not be able to interpret it. Declare your standard on the title block, every time.[fn:: The deeper problem is that the two standards committees have been slowly converging for thirty years and remain not-converged. This is a coordination failure, not a technical one. You cannot solve it. You can only document which side you are on.]

7. Citing Y14.5 without a year. The 2018 revision deleted concentricity and symmetry. It changed the default tolerance zone for some controls. It re-numbered sections. A 2009 callout and a 2018 callout that look identical on the drawing can mean different things. The year is part of the spec.

References

• ASME, "Dimensioning and Tolerancing: Engineering Drawing and Related Documentation Practices", 2018
• ISO, "Geometrical product specifications (GPS) -- ISO code system for tolerances on linear sizes", 2024
• ISO, "Geometrical product specifications (GPS) -- Geometrical tolerancing", 2017
• ISO, "Geometrical Product Specifications (GPS) -- Surface texture: Profile method", 1997
• ASME, "Surface Texture (Surface Roughness, Waviness, and Lay)", 2019
• Alex Krulikowski, "Geometric Dimensioning and Tolerancing: Self-Study Workbook", SME, 1998
• Paul J. Drake, "Dimensioning and Tolerancing Handbook", McGraw-Hill, 1999
• O. Bjorke, "Computer-Aided Tolerancing", ASME Press, 1989 -- the classic RSS-vs-WC treatment

Related

• Fasteners -- clearance hole sizing, the practical lower bound on any positional tolerance you can sensibly write.
• Bearings (fit selection) -- the canonical consumer of IT-grade fits. Bearing bore/shaft seat tolerances are where H7/g6-style reasoning is most often applied.
• Optical microscopy -- surface finish measurement. Ra without microscopy (or profilometry) is a number written on paper, not a quantity measured on metal.
• Ruler, measuring instruments -- the metrology side: a tolerance you cannot measure is not a tolerance.
• Units -- tolerances are quantities and quantities carry units. Mixing mm and um in a stack is a typo that costs a week.