Guide
What is a basic dimension in GD&T, and why do suppliers flag boxed dimensions on a drawing?
A basic dimension is a theoretically exact value, drawn inside a box, that sets the true size, location, orientation or profile a geometric tolerance is measured from; it carries no tolerance of its own, so in basic dimension GD&T practice every boxed value must lead to a feature control frame or datum target that supplies the tolerance.
By Saola Manufacturing engineering team · Published · Updated
Boxed dimensions are a frequent reason a drawing comes back from a supplier with questions before a price. The usual pattern is simple: someone boxed a set of hole locations or a contour, but the feature control frame that should give those boxes a tolerance is missing, points at the wrong datums, or controls a different feature. This guide explains what a basic dimension does and does not do under ASME Y14.5-2018 and its ISO counterpart, how to trace each box to its tolerance, how to repair an orphaned box before the RFQ goes out, and what to put on the drawing so an overseas shop quotes the part you meant.
On this page
What does a basic dimension in GD&T actually tell the machinist?
It tells the machinist where the perfect feature would be, not how far the real feature may stray. The allowed variation lives somewhere else on the drawing, almost always in a position or profile feature control frame.
ASME Y14.5 defines a basic dimension as a theoretically exact size, profile, orientation or location of a feature or datum target. Read that definition literally and the consequences follow. A boxed 2.500 is not 2.500 plus or minus anything; it is the exact center of a tolerance zone whose size and shape come from a frame. Two boxed values in a chain do not stack up, because neither of them varies. The number of decimal places shown in the box does not make the value more or less exact: a box reading 40 is as exact as one reading 40.000, and the precision you need is set by the tolerance in the frame.
The ISO system uses the same idea under a different name. ISO 1101 calls it a theoretically exact dimension, or TED, and draws it in the same rectangular frame. If you work across both systems, the comparison in ASME Y14.5 vs ISO GPS covers the defaults that do differ; the meaning of the box is not one of them.
Three things a basic dimension never does on its own: it never sets size limits on a hole, pin or slot (unless a profile frame is deliberately used to control that size); it never inherits the title block tolerance; and it never tells the inspector which datum to measure from. Each of those has to be stated elsewhere, and each one is a separate drawing mistake when it is not.
Where does the tolerance on a basic dimension come from?
From whichever control the boxed value feeds: a position or profile frame, an angularity frame for a boxed angle, a datum target for a boxed target location, or a gauge tolerance when the box sizes a fixture element. If you cannot point to one of those for every box, the drawing has a gap.
The table maps each legitimate use of a boxed value to the control that turns it into an inspectable requirement. Use it as a checklist: walk every box on the sheet and write down which row it belongs to. A box that fits no row is the one a supplier will flag. The datum letters in the frame matter as much as the frame itself, because the boxed values have to start from the datum features named there; a hole pattern boxed from an edge that is not one of the referenced datums has an exact location relative to nothing anyone will inspect. For how datum features should be picked on a cast part before the machining datums take over, see setting datums on castings for machining.
| The boxed value defines | Tolerance comes from | Example callout (illustrative) |
|---|---|---|
| Location of a hole, pin, slot or tab | Position frame on that feature of size | 4X Ø6.6–6.8 mm with position Ø0.25 M | A | B | C; holes boxed from B and C |
| Shape or location of a surface, edge or contour | Profile of a surface or profile of a line frame | Boxed radii and points on a contour, profile 0.4 mm | A | B |
| Angle of an inclined face or hole axis | Angularity frame (or profile) | Boxed 30° with angularity 0.1 mm | A |
| Spacing within a pattern only | Lower segment of a composite position or profile frame | Upper segment to A | B | C, lower segment to A only |
| Location and size of a datum target | Gauge and fixture tolerances (per ASME Y14.43) | Boxed target point locations on a casting, datum targets A1, A2, A3 |
| Size of a hole or pin | None: size must carry its own tolerance, unless a profile frame deliberately controls it | Boxed Ø10 on a hole with no limits and no profile frame is a drawing error |
Why do suppliers flag basic dimensions that have no feature control frame?
Because an orphaned box leaves the feature with no tolerance at all, and a shop cannot price or inspect a feature it cannot accept or reject. The flag is a request to complete the drawing, not a complaint about GD&T.
Orphans usually appear in one of four ways. A designer boxes every location dimension by default in the CAD template and never adds the frames. A drawing is revised from coordinate tolerancing to GD&T halfway, so the boxes were added but the position frame landed on only one of two hole patterns. A frame exists but references datums that the boxes do not originate from. Or a general note such as “UNTOLERANCED DIMENSIONS ARE BASIC” quietly turns every dimension without limits into a box, including some that were meant to fall under the title block tolerance.
That last case causes the most trouble. Under ASME Y14.5, a general note may designate untoleranced dimensions as basic, but then every one of those dimensions needs a geometric control somewhere. A buyer who expects the block tolerance to cover a non-critical chamfer location is reading the drawing differently from the supplier, who sees an exact value with no zone. Per ISO 2768-1, general tolerances likewise do not apply to theoretically exact dimensions in frames, so the same gap exists on ISO drawings that rely on a general tolerance class; the ISO 2768 and NADCA tolerance guide covers how those general notes are meant to work.
A supplier that quotes an orphaned drawing without asking has to guess. Guess loose and the part may not assemble; guess tight and you pay for inspection and scrap you never asked for. Either way, the dispute surfaces at first article, after tooling and fixtures already exist.
How do you fix an orphaned basic dimension before the RFQ goes out?
For each orphaned box, decide whether the feature is functional: if it is, add the position or profile frame with the right datums; if it is not, remove the box and give the dimension a plus-minus tolerance or let the general tolerance cover it.
Work through it in this order. First, list every boxed value and the feature it locates or defines. Second, for features of size such as holes, pins, bosses and slots that mate with something, add a position frame and size the zone from the fastener or pin clearance; the method is in how MMC bonus tolerance works and, for tapped holes, position tolerance on threaded holes. Third, for surfaces, edges and cast contours, use profile; profile tolerance on castings explains bilateral and unilateral zones. Fourth, for anything that does not mate, seal or locate, unbox it. A non-functional feature carried as a basic dimension forces a geometric check where a caliper reading would have done.
If the original drawing used coordinate tolerances and you are converting, do not simply copy the plus-minus value into the position frame. A square zone of plus-minus t on each axis has a diagonal of about 2.83 times t, so the circle that just contains the old square is roughly 2.83 times t in diameter; a zone that size accepts every part the old square accepted. Copying the numbers across shrinks the zone instead: a position diameter equal to the old total band (2 times t) is the circle inscribed in the old square, so parts that sat in the old square's corners, and used to pass, now fail, and a diameter equal to t is tighter still. The values below are that calculation, not a recommendation for any specific part.
| Old coordinate tolerance (plus or minus, each axis) | Equivalent position zone that contains the square | Position zone equal to the old total band, 2t (tighter) |
|---|---|---|
| 0.002 in each way | Ø0.0057 in | Ø0.004 in |
| 0.005 in each way | Ø0.0141 in | Ø0.010 in |
| 0.010 in each way | Ø0.0283 in | Ø0.020 in |
| 0.05 mm each way | Ø0.141 mm | Ø0.10 mm |
| 0.1 mm each way | Ø0.283 mm | Ø0.20 mm |
Which basic dimension mistakes show up most on drawings sent for quotes?
Beyond the orphaned box, the repeat offenders are boxed sizes, double-dimensioned locations, boxes that do not start at the referenced datums, and boxed values that disagree with the CAD model. Each one is quick to fix on the drawing and slow to fix after first article.
- Boxed size of a feature of size. A hole diameter in a box has no size limits. Size needs its own tolerance or limits; position then locates the axis. The exception is a contour where profile deliberately controls size, such as a boxed radius on a profiled outline.
- Plus-minus and position on the same location. A hole located by a toleranced dimension and also controlled by position has two conflicting requirements. Pick one. If the frame stays, the location dimensions must be basic.
- Boxes that start from a non-datum edge. The frame says the zone is located from datums A, B and C, but the boxed dimensions run from an unlabeled side or a center mark. The inspector cannot reconcile the two, and the supplier will ask which one governs.
- Boxed angle with a plus-minus angle beside it. A boxed angle needs angularity or profile; an angle with limits needs no box. Showing both on one feature is the angular version of double dimensioning.
- Rounded display versus model value. A box shows two decimals while the model carries a different exact value. Because the box has no tolerance, the supplier needs to know which number is the true location. State on the drawing whether the model or the sheet governs.
- Boxing the obvious. Per ASME Y14.5, right angles and zero offsets are implied basic where geometric tolerances control features related to a datum reference frame, so boxing every 90° adds clutter rather than information.
None of these is exotic. The GD&T symbols chart lists the frame-level mistakes that sit alongside them, such as missing datum references and the wrong material condition modifier.
How are basic dimensions inspected, and what should the report show?
A basic dimension is not inspected by itself; the feature is measured in the datum reference frame and the result is reported against the frame it supports. A report line that says a boxed location was “measured” with no position or profile result has not proved anything.
In practice the inspector sets up on the datum features named in the frame, measures the actual location or surface, compares it with the true location defined by the boxed values, and reports the deviation as a position diameter or profile value against the allowed zone. Functional gauges do the same job physically: pins or gauge elements sit at the basic locations, sized from the virtual condition, with gauge tolerances set per ASME Y14.43. Either way, the boxed value is an input to the measurement, not an output.
This has a direct effect on how a first-article report reads. Balloon the feature control frame and let it carry the result, and only balloon the boxed values if your customer's PPAP or first-article instructions require it; the reasoning and numbering approach are in ballooned drawings and inspection reports. If the reporting format matters for your approval, say so in the RFQ, alongside which datum setup you expect.
What should the drawing and RFQ say about basic dimensions?
The drawing should let a stranger trace every box to a frame and every frame to its datums without asking a question. The RFQ should name the standard and edition, say whether the model or the sheet governs, and point out the frames that actually matter for function.
Before release, check these points on the sheet: the governing standard and edition in the title block, for example ASME Y14.5-2018; every boxed value tied to a frame, a datum target or a gauge; no general “untoleranced dimensions are basic” note unless every such dimension is controlled; sizes toleranced separately from locations; and boxes that originate from the datum features named in the frame. In the RFQ, list the critical frames, state the inspection report format you expect, and attach the model if it carries the exact basic values. The wider RFQ checklist is in how to prepare a machining RFQ, and the cost side of tight frames is in the cost of tight tolerances.
At Saola, the first step for a new part is a drawing review in which every tolerance, callout and note is read, and the buyer receives a marked-up copy of their own drawing; orphaned boxes, conflicting locations and unclear datum origins are the kind of item that review is meant to catch before tooling. Datum faces, bores, pockets and tapped holes on castings are machined to geometric tolerance on our CNC milling line, and its page lists the limits we hold; if a frame on your drawing is tighter than that table, say so before tooling, not after first samples. The first piece off new tooling is measured against every toleranced dimension on your drawing and you receive that report, as described on the quality and inspection page. Turned features follow the same review on the CNC turning side.
Frequently asked
Does the title block tolerance apply to a basic dimension?
No. Under ASME Y14.5 a basic dimension is exact and is excluded from general tolerances, and ISO 2768-1 likewise excludes theoretically exact dimensions in frames. The only tolerance that applies is the one in the frame or datum target the box supports.
Is a basic dimension the same as a reference dimension?
No. A reference dimension, shown in parentheses, is for information only and does not govern production or inspection. A basic dimension is a requirement: it fixes the true location or shape that the geometric tolerance is measured from. Turning a reference dimension into a box changes what gets inspected.
Can basic dimensions live only in the CAD model?
They can when the drawing or model states that model values are basic and names the governing standard, which is how model-based definition works; NIST publishes test models showing GD&T carried this way. Say so explicitly on the sheet and send the native or STEP model with the RFQ, or the supplier will only see whatever values the PDF happens to display.
Do I need a box on every 90-degree angle?
Usually not. ASME Y14.5 treats right angles and zero offsets as implied basic where geometric tolerances control features related to a datum reference frame. Box an angle when it is not a right angle and is controlled by angularity or profile.
Can a boxed dimension be used without any datums?
Yes, for relationships inside a feature or pattern: hole-to-hole spacing controlled by a position frame with no datum references, or the shape of a contour controlled by a profile frame with no datum references. Locating that pattern or contour on the part still needs a frame with datums.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures, ASME, 2011 (reaffirmed 2020)
- ISO 1101:2017, GPS — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017 (reviewed and confirmed 2022)
- ISO 2768-1:1989, General tolerances — Part 1: Tolerances for linear and angular dimensions without individual tolerance indications, ISO, 1989
- MBE PMI validation and conformance testing: CAD models and PMI test cases (ASME Y14 GD&T), NIST, 2016 (updated 2025)