Guide
What changed from the 2009 edition in ASME Y14.5-2018, and what does it mean for drawings sent to suppliers?
ASME Y14.5-2018 is the current edition of the American standard for dimensioning and tolerancing, which replaced ASME Y14.5-2009 and was reaffirmed in 2024. Its main changes for a drawing sent to a supplier are the removal of the concentricity and symmetry symbols, a new dynamic profile modifier and from-to symbol, a single default rule for stabilizing a rocking datum feature, and a stronger push toward profile and position instead of plus-and-minus tolerances for locating surfaces.
By Saola Manufacturing engineering team · Published · Updated
Most engineers who learned GD&T on the 2009 edition can read a 2018 drawing without trouble, and that is by design: the foreword of the 2018 edition states that no tolerancing concept was reversed, to keep the move from 2009 simple. The trouble starts at the boundary between the two. A part family released over ten years carries prints from both editions, a CAD template still offers the concentricity symbol, and an inspector sets up a CMM program the way the last job was done. This guide is written for the design engineer who signs the drawing and the buyer who sends it out for machining. It lists what changed, what a supplier does differently for each change, which edition a new drawing should cite, and how to handle a package that mixes editions. It summarizes the standard; it does not replace the document, which ASME sells.
On this page
What changed between ASME Y14.5-2009 and ASME Y14.5-2018?
The 2018 edition removed two geometric characteristics, concentricity and symmetry, added the dynamic profile modifier and the from-to symbol, defined one default way to establish a datum from an unstable datum feature, and recast its fundamental rules around tolerancing features rather than dimensions. Most other changes are clarifications, new 3D model figures and a renumbered layout.
The document grew considerably, but the growth is mostly figures. ASME describes the revision as adding model views to many figures because industry relies less on orthographic views, emphasizing profile for location tolerances applied to surfaces, and restructuring the content so that form, orientation and profile each have their own section. The listed areas of important change are the concept of a feature of size, datum references and degrees of freedom, composite position tolerances, surface and axis interpretations, profile tolerances, and symbols and modifiers.
For a shop, the table below is the practical version. Each row names a change and the action a supplier takes when the drawing in hand cites the 2018 edition. Rows marked as carried over from 2009 are included because buyers often assume they are new, and because they matter when an older print is revised.
What does each change mean for the supplier who machines and inspects the part?
Most changes alter how the drawing is read and inspected rather than how the part is cut. The supplier’s job is to apply the rules of the edition the title block names, query anything that edition does not support, and report results the way that edition defines them.
The rows below follow the order a reviewer usually meets them on a print: symbols first, then profile modifiers, then datums and general rules.
| Topic | 2009 edition | 2018 edition | What the supplier does |
|---|---|---|---|
| Concentricity and symmetry | Defined, as controls of opposed median points | Removed: term, symbol and concept | Query the symbol on a 2018 print; ask for position, runout or profile instead |
| Dynamic profile | Not available | Triangle modifier after the profile value; controls form without size | Evaluate shape with the zone free to grow or shrink; check size separately |
| From-to profile | Non-uniform zone shown by sketched boundaries | From-to symbol with two values in the frame; zone width tapers between the two named points (sketched boundaries still allowed) | Program a varying zone; report pass/fail along the feature |
| Unequally disposed profile | Circled U modifier, or phantom-line sketch of the zone | Circled U modifier only | Read the value after the U as the amount toward added material |
| Unstable datum feature | Candidate datum set: several acceptable seatings | One default solution that minimizes separation from the true geometric counterpart | Use the default stabilization in the CMM, or a note that states another method |
| Free state on datums | Free state symbol on tolerances and datum feature references; restraint by note | Restraint notes covered in more detail; a free state datum reference releases only that datum feature while the rest of the part stays restrained | Fixture exactly as the restraint note says; release the flagged datum |
| Fundamental rule (a) | Each dimension shall have a tolerance | Each feature shall be toleranced; basic features take feature control frames | Flag features left with no control in the frame or the general block |
| Plus-and-minus location | Shown in some figures | Moved to an appendix and discouraged; profile emphasized for surfaces | Ask for the origin of any plus-and-minus location on a 2018 print |
| Profile in the general tolerance block | A feature control frame could sit in a note or the general tolerance block | Stated as a way to apply profile all over the part | Treat the block profile as the default for every untoleranced surface |
| Nominal value as a target | Not stated | The as-designed value is not a manufacturing target unless a note says so | Aim for the middle of the zone unless the drawing names a target |
| Surface flaws | Not stated | Surface elements include texture and flaws such as burrs and scratches | Deburr and finish so no flaw breaks a tolerance boundary |
| Radius with a located center | Not addressed directly | When the center is located by dimensions, the zone is bounded by arcs about that center, giving a uniform width | Inspect against concentric arcs, not a zone tapering to the tangents |
| Rule #1 exception | Note: perfect form at MMC not required | Independency symbol, a circled I, next to the size | Check size only; control form through the separate form tolerance |
| Translation modifier, movable datum target, continuous feature | Introduced in 2009 | Retained; two defined types, continuous feature and continuous feature of size, so CF can apply to surfaces | No change in practice; confirm the edition before reading a CF callout on a surface |
Why were concentricity and symmetry removed, and what replaces them?
They were removed because other characteristics give more direct control and because the symbols were widely misapplied; coaxial features now take position, runout or profile, and symmetrical features take position or profile. A 2018 drawing that still shows either symbol cites a characteristic the edition no longer defines.
In the 2009 edition, concentricity did not control an axis. It controlled the median points of diametrically opposed surface elements, which a supplier can only evaluate by sampling many cross-sections, usually on a CMM, and computing median points one by one. As the Mitutoyo Institute of Metrology presentation on the 2018 edition points out, many organizations had already banned both symbols, and the 2018 standard removed the term, the symbol and the concept, citing the confusion around their misapplication. The same presentation notes that many CMM software packages use ISO 1101 terms and evaluate a callout labeled concentricity much like a position tolerance, which is how the same print can pass at one shop and fail at another.
The replacement depends on the function. If a bearing bore must sit on the axis of a shaft for assembly, position at MMC on the bore relative to the shaft axis lets the supplier use a functional gauge and gives bonus tolerance as the bore departs from its smallest size. If the requirement is dynamic balance or a seal running true, circular or total runout is quicker to check and also limits form. If the feature is not a simple cylinder, such as a cam or a lobed bore, profile of a surface relative to the datum axis does the job. The concentricity, runout and position guide compares the three in more detail, and our drawing reviewers suggest the replacement when a 2018 print still carries the old symbol.
What do the dynamic profile modifier and the other profile changes do?
The dynamic profile modifier, a small triangle after the profile tolerance value, lets a profile zone control the shape of a feature without controlling its size, so the zone may expand or contract while its width stays fixed. The 2018 edition also added a from-to symbol for zones that vary along a feature and made the circled U the only way to show an unequally disposed zone.
A normal profile of a surface on a closed shape controls size and form together, because both boundaries are offsets from a true profile defined by basic dimensions. That is often stricter than the function needs. The dynamic modifier is typically used as a refinement in a composite or two-segment profile: the upper segment locates and sizes the contour against the datums, and the lower segment, with the triangle, holds a tighter shape tolerance while the contour is free to be slightly larger or smaller. For a supplier, the inspection changes in one way: the CMM fit for the refinement must allow the offset of the nominal to float, not just translate and rotate.
The from-to symbol gives a symbolic way to state a non-uniform zone that the 2009 edition could only show with sketched boundaries, which remain permitted. Two values in the frame set the zone width at each end, and the width changes gradually between the named points, so the result is a pass or fail along the feature rather than a single deviation number. The circled U had already been introduced in the 2009 edition, which also accepted a phantom-line sketch of the offset zone as an alternative; the 2018 edition dropped the sketch method. A buyer who revises an older print that used the sketch should convert it to the U modifier when moving the print to the 2018 edition. The GD&T symbols chart shows the current symbol set.
How did datum and general rules change in the 2018 edition?
The largest datum change is a single default for an unstable datum feature: the part is adjusted to the one solution that minimizes separation from the true geometric counterpart, replacing the earlier candidate datum set. The general rules shifted from tolerancing every dimension to tolerancing every feature, and added defaults on nominal targets and surface flaws.
On a rocking face, the 2009 edition allowed several valid seatings, so two inspectors could each be right and still disagree. The 2018 default gives one answer, which a CMM can reproduce and which the companion mathematical standard, ASME Y14.5.1, describes as a constrained least-squares fit. When a drawing needs another method, such as a three-point seat for a cast face, it should say so with datum targets or a note. Two terms also changed: datum features used together, such as A-B, are now called common datum features, and the theoretical perfect counterpart is again called the true geometric counterpart. The datum reference frame guide covers datum selection itself.
Among the general rules, three have direct effects on a machined part. First, each feature shall be toleranced, either by limits of size or by a feature control frame on a basic definition, which is why a general profile in the tolerance block is now a stated method of covering every surface. Second, unless a note says otherwise, the as-designed value is not a manufacturing target, so a supplier aims for the middle of the zone. Third, surface elements include texture and flaws such as burrs and scratches, so a burr that breaks a boundary is a nonconformance, not a cosmetic issue. For milled housings and plates, our CNC milling reviewers read the general tolerance block first for exactly this reason, since it sets the default for every surface without a callout.
Which edition of ASME Y14.5 should a drawing cite?
A new drawing should cite ASME Y14.5-2018, the edition ASME lists as current, by full number and year in the title block or general notes. A drawing revised from an older release should either keep its original edition for the whole sheet or be moved to 2018 completely, never partly.
Use of Y14.5 is voluntary, and an organization can keep working to an older edition, so the edition on the drawing decides how the print is read. A note that says only “per ASME Y14.5” with no year leaves the supplier to guess, and the guess usually defaults to the edition the inspection software was set up for. Use the rule below on the drawing or the RFQ.
| Situation | Cite on the drawing | Before release |
|---|---|---|
| New part, new drawing | ASME Y14.5-2018 | Remove concentricity and symmetry from the CAD template; use the U modifier for offset profile |
| Existing 2009 print, minor revision | Keep ASME Y14.5-2009 | Add no 2018-only symbols such as dynamic profile, from-to or the circled I |
| Existing 2009 print, major revision | Move to ASME Y14.5-2018 | Replace retired symbols, convert sketched profile zones, re-check datum features that rock |
| Customer contract names an edition | The contract edition | State it in the title block so the supplier does not rely on the contract alone |
| Edition missing from the drawing | Add the edition before the RFQ goes out | Confirm in writing which edition governs, part number by part number |
What should a supplier do when an old print and a new print mix editions?
Read each drawing under the edition it cites, and settle any conflict in writing before cutting metal. When two prints in one assembly disagree, the mating requirement has to be confirmed by the design owner, not resolved by the supplier’s choice.
Mixed packages are normal. A housing released years ago may cite the 2009 edition while a new cover cites 2018, and both are valid as written. The supplier keeps a separate interpretation for each sheet: a concentricity callout on the 2009 housing is inspected as defined in 2009, while the same symbol on the 2018 cover is queried. The risks sit at the interfaces. A datum feature that rocks may be seated by a candidate datum set on one part and by the 2018 default on its mate, and a location given with plus-and-minus tolerances on the old print may not stack cleanly with a profile on the new one. The ASME vs ISO GPS guide covers the related case of a package that mixes ASME and ISO drawings.
When we review a mixed package, we list each drawing with its cited edition, flag retired or not-yet-defined symbols for the edition named, and ask the buyer to confirm the governing edition for every interface feature. The same list goes into the inspection plan, so the CMM program for each part uses the right datum rules. Sending that list with the drawings to a quote request means questions about editions come back feature by feature with the quote, not after first-article inspection. The RFQ package guide lists the rest of what to send.
Frequently asked
Is ASME Y14.5-2018 the latest edition?
Yes. ASME lists Y14.5-2018 (R2024) as the current edition and states that it replaces Y14.5-2009. Although dated 2018, it was released in early 2019. The R2024 mark means it was reviewed and reaffirmed in 2024, with the content kept rather than revised.
Is a drawing made to ASME Y14.5-2009 still valid?
Yes. The edition cited on the drawing governs how it is read, and nothing in the 2018 edition voids an older drawing. The supplier should inspect a 2009 print to 2009 rules, including concentricity or symmetry if it carries them.
Did Rule #1 change in the 2018 edition?
No. Rule #1, the envelope principle, still applies by default to regular features of size. What changed is the way to waive it: where the 2009 edition used a note, the 2018 edition adds the independency symbol, a circled I placed next to the size.
Can I keep using concentricity if I cite the 2009 edition?
You can, because the 2009 edition still defines it. It remains hard to inspect, so position, runout or profile usually gives the same functional control at a lower inspection cost, whichever edition the drawing cites.
Does ASME Y14.5-2018 cover 3D models without drawings?
It covers annotated models as well as drawings, and many figures now include model views. The foreword notes that the methods for applying annotation in model views are defined in the companion standard ASME Y14.41, while Y14.5 defines what the tolerances mean.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 edition published 2019 (reaffirmed 2024), accessed October 2026
- GD&T and the new ASME Y14.5-2018, Mitutoyo Institute of Metrology, Mitutoyo America Corporation, 2019
- ISO 1101:2017, GPS — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017 (for the ISO terms used by CMM software)
- Quick Guide to the Latest GD&T Standard: ASME Y14.5-2018, GeoTol, Inc., updated 2025 (from-to symbol, free state on datum references, continuous feature types, profile in the general tolerance block)