GD&T (geometric dimensioning and tolerancing) controls the shape, orientation and location of features rather than just their size. For most CNC parts five controls do almost all the work: flatness, perpendicularity, position, runout and profile, each referenced to datums that reflect how the part is assembled. Used well, GD&T allows wider tolerances than plus/minus dimensions while still guaranteeing fit.
The two systems in use are ASME Y14.5 (current edition 2018), common in North America, and ISO GPS (ISO 1101 for geometrical tolerancing, ISO 5459 for datums), common in Europe and Asia. The symbols look almost the same, but some defaults differ — which matters when a drawing crosses a border.
Why GD&T instead of plus/minus
Plus/minus tolerances on hole locations create square tolerance zones and stack up from one dimension to the next. A position tolerance gives a round zone around the true position, which is about 57 % larger in area than the square zone that fits inside it, and it is measured from datums instead of from other features. The result is usually more usable parts for the same function.
GD&T also makes inspection unambiguous: the datum reference frame tells the inspector how to fixture the part, which is often the source of disagreement when only plus/minus dimensions are used.
The controls you will use most
- Flatness: a form control for one surface, no datum. Use it on sealing and mounting faces. A milled face of moderate size typically achieves a few hundredths of a millimeter without special operations.
- Perpendicularity (and parallelism): orientation of a face or axis to a datum. Use it on mounting faces, bore axes and shoulders that locate other parts.
- Position: location of holes, pins, slots and bosses relative to datums. The workhorse control for bolt patterns, often with the MMC modifier so clearance holes gain bonus tolerance as they get larger.
- Circular and total runout: for turned parts, controlling a diameter or face relative to a datum axis as the part rotates. Easy to check with a dial indicator between centers or in a V-block.
- Profile of a surface or line: controls a contour, a chamfer or an entire surface’s size, form, orientation and location in one callout. Very useful for freeform or 3D-milled shapes.
Concentricity vs runout
Concentricity controls the median points of a feature relative to a datum axis. Measuring it requires many points around the feature and calculating median points, which is slow and needs dedicated metrology equipment. ASME Y14.5-2018 removed concentricity and symmetry altogether and points designers to runout, position or profile instead; ISO still has the concentricity/coaxiality symbol.
For most turned parts the real requirement is that a diameter does not wobble relative to the bearing journals. Total or circular runout says exactly that, includes form error, and can be checked quickly on the shop floor. If a feature needs a coaxial location for assembly, position at MMC is often the better choice.
Choosing datums
Datums should be the features that locate the part in its assembly — the face it bolts to, the bore it slides on, the pin holes that align it. When the datums match function, the tolerances on everything else can be as generous as the function allows.
- Primary datum: the largest, most stable contact surface or the main locating diameter.
- Secondary and tertiary: features that stop rotation and translation, for example a bore and a pin hole or slot.
- Avoid datums on cast, rough or plated surfaces unless the coating is controlled.
- Make datum features accessible for fixturing and measurement, and do not choose small features that cannot support the part.
Callouts that drive cost
Machining cost follows the tightest tolerance and the hardest-to-measure requirement, not the average. Watch for:
- Position tolerances below about 0.02–0.03 mm on holes in different setups; features cut in one setup hold relative position far better.
- Flatness or parallelism in single microns over large faces, which may push the part to grinding or lapping.
- Profile tolerances applied to an entire part “all around” when only a few surfaces matter.
- Datums on features that are machined last or in a different operation, forcing extra setups.
- Unnecessary concentricity or symmetry callouts where runout or position would do.
- Geometric tolerances tighter than the size tolerance of the same feature, which is often a sign of an error.
ASME vs ISO defaults that cause confusion
Under ASME Y14.5 Rule #1 (the envelope principle) applies by default: a feature of size may not exceed perfect form at maximum material size, so a size tolerance also limits form. Under ISO 8015 the independency principle is the default: size and form are separate, and the envelope requirement must be called up with the Ⓔ symbol. A drawing should state which standard it follows, including the year, in the title block or general notes.
For untoleranced geometric features, ISO 2768-2 (classes H, K, L) is still widely quoted on ISO drawings alongside ISO 2768-1 for linear dimensions, though it was withdrawn and replaced by ISO 22081:2021; ASME drawings usually use a title-block general tolerance.
Tips to avoid over-tolerancing
- Start with general tolerances, then add GD&T only to features that mate, seal, rotate or locate.
- Use MMC on clearance holes and pins so bonus tolerance is available.
- Ask which features must be reported in the inspection report; a full layout of every dimension adds cost.
- Check tolerance stacks before tightening everything: often one well-chosen datum removes the need for tight tolerances elsewhere.
GD&T at Chi Xin
Chi Xin Technology is a CNC machine shop in Nantun District, Taichung, Taiwan, founded in 2022. We run 5+ CNC machines — 4.5-axis CNC machining centers and CNC lathes — and mainly machine aluminum alloys and alloy steel, with a metal tolerance of 0.02 mm. We also offer wire EDM and surface finishing including anodizing, and we export to customers in Europe and North America.
Our 4.5-axis machining centers let many features be cut in one setup, which helps hold position and orientation between faces; mark the critical GD&T callouts and required report items in your RFQ and we confirm in the quotation how they will be inspected.
Frequently asked questions
Should I use runout or concentricity on a turned part?
In most cases runout. It is easy to measure, includes form error, and ASME Y14.5-2018 no longer includes concentricity. Use position if you need a coaxial location with bonus tolerance.
Does GD&T make parts more expensive?
Not by itself. Well-applied GD&T often allows larger tolerances than plus/minus dimensions. Cost goes up when geometric tolerances are tight, applied to every feature or tied to datums that do not match how the part is made.
My drawing has no standard noted. Which one applies?
That is ambiguous, especially between ASME and ISO defaults for form. Add “Dimensioning and tolerancing per ASME Y14.5-2018” or the ISO GPS reference in the notes.
What position tolerance is realistic for a bolt pattern?
It depends on the fastener clearance. For clearance holes the position tolerance is often derived from the hole and bolt sizes, typically a few tenths of a millimeter at MMC. Very tight values are usually only needed for dowel holes.
Can you provide an inspection report for GD&T features?
Tell us which features must be reported and in what format in the RFQ, and we confirm in the quotation what the report will include.



