Guide
What is a reference dimension on a drawing, and do inspectors check REF values?
A reference dimension is a value shown on a drawing for information only: it repeats a size already defined elsewhere, or can be calculated from other dimensions, so it carries no tolerance and does not decide whether a part is accepted or rejected. Current ASME practice shows it in parentheses, older drawings add the letters REF, and ISO drawings call the same thing an auxiliary dimension.
By Saola Manufacturing engineering team · Published · Updated
Engineers search this term for one practical reason: they want to know whether a supplier is bound by a value in parentheses, and whether an inspector can reject a part because of it. The short answer is no on both counts, but only if the drawing is built so that the reference value really is redundant. This guide covers the decision of when to add one, the arithmetic that makes a REF value safe or dangerous, the mistakes that turn it into a dispute, and the exact wording to put on the drawing, RFQ and purchase order.
On this page
What does a reference dimension mean under ASME Y14.5 and ISO 129-1?
Under ASME Y14.5 a reference dimension is a dimension, usually without tolerance, used for information purposes only, which does not govern production or inspection operations. It is either a repeat of a dimension or a value derived from other values on the same drawing or a related drawing.
The ASME
Y14.5 standard identifies a reference dimension by enclosing it in parentheses, for example
(42.0). Drawings made to editions from before the parentheses convention, and many drawings made
by habit since, write 42.0 REF instead; both mean the same thing, and a modern checker will ask
you to use the parentheses. The same standard sets the fundamental rule that every dimension needed to define
the part must be shown, that no more dimensions than necessary should be given, and that the use of reference
dimensions should be minimized. That last clause is the important one: a reference dimension is tolerated
redundancy, not a design tool.
On ISO drawings the equivalent is the auxiliary dimension in ISO 129-1:2018, also shown in parentheses and also never toleranced. The ISO term is helpful because it describes the job well: the value assists the reader but adds no requirement. If your organization works to both systems, the ASME Y14.5 vs ISO GPS guide covers the wider differences.
Do not confuse a reference dimension with a drawing stamped “FOR REFERENCE ONLY”. That stamp marks an uncontrolled copy of a whole document, and a supplier should never build production parts from it. A REF value on a controlled, released drawing is a different thing entirely.
How do inspectors treat a REF dimension compared with other dimension types?
An inspector does not accept or reject a part on a reference dimension, and the title-block general tolerance does not apply to it. At most, the value is recorded and marked as reference only.
The confusion usually comes from mixing up four kinds of value that all look like plain numbers on a print. A basic dimension sits in a box and is theoretically exact; its tolerance lives in a feature control frame, which is what gets inspected (the GD&T symbols chart explains those frames). A plain dimension with no tolerance of its own is still a requirement, because it inherits the general tolerance block. A reference dimension inherits nothing. The table below sets them side by side.
| Dimension type | How it appears on the print | Governs acceptance? | Typical inspection report entry |
|---|---|---|---|
| Directly toleranced | Limits 24.95–25.05 mm, or a plus/minus tolerance | Yes | Measured value, accept or reject |
| Untoleranced, covered by general tolerance | 25 mm plus a title-block note such as ISO 2768-m | Yes, to the general tolerance | Measured value against the general-tolerance limits |
| Basic | 25 mm in a rectangle | Only through the feature control frame it locates | Frame result recorded; basic value not measured on its own |
| Single limit | R0.5 MAX, 3.0 MIN | Yes, one side only | Measured value against the one limit |
| Reference (ASME) / auxiliary (ISO) | (25) or 25 REF | No | Not listed, or value recorded and marked REF with no accept column |
When should you put a reference dimension on a drawing?
Use one only when a reader genuinely needs a value that is already fully defined by other dimensions, and when you are certain you never need it controlled. If you would be unhappy to receive a part where that value drifted, it is not a reference dimension.
Legitimate uses fall into a short list:
- The closing link of a chain. When three steps on a shaft are each toleranced, the overall
length is already decided by them. Showing the overall as
(60)saves the machinist, the packaging engineer and the buyer from adding it up. - A value owned by another drawing. A machining drawing for a casting often repeats a cast-in size from the casting drawing as reference, so the operator knows what to expect at the fixture without the machining print taking ownership of it. The casting vs machining drawing guide explains why the requirement must live on only one of the two.
- A derived value that helps setup. A chord, a developed length, a radius that results from two tangent lines, or a hole-to-edge distance that follows from a toleranced pattern.
- Envelope or weight for logistics. Overall size for packaging and handling, where nobody will measure it for acceptance.
Equally clear are the places where a reference dimension does not belong. A fit size, a sealing face location, a thread length that must engage a mating part, or anything a downstream assembly relies on must be toleranced or controlled with GD&T. A stock size that matters, such as the across-flats of an unmachined hex, should be called out with the material specification so that the mill standard’s tolerance applies, rather than shown as a bare REF value. And a dimension before coating that the shop has to hit is a requirement; state it as a BEFORE COATING limit, as the threads after anodizing and plating guide shows for threads.
What happens when a REF dimension disagrees with the toleranced dimensions?
The toleranced dimensions win, because the reference value carries no requirement. A part that meets every toleranced dimension conforms, even if the measured reference value differs from the number in parentheses.
The worked example below shows why the reference value can legitimately differ. In version A the three steps are toleranced and the overall is reference; the overall then varies by the sum of the three step tolerances, worst case. In version B the designer wanted the overall controlled, so the overall carries the tolerance and step C becomes the reference value; now step C absorbs the variation instead. Neither drawing is wrong. What is wrong is drawing version A when the assembly actually needs the overall held tightly, which is the most common way a reference dimension causes a field failure.
| Feature | Version A: overall as reference | Version B: step C as reference |
|---|---|---|
| Step A length | 19.9–20.1 mm | 19.9–20.1 mm |
| Step B length | 24.9–25.1 mm | 24.9–25.1 mm |
| Step C length | 14.9–15.1 mm | (15.0) REF |
| Overall length | (60.0) REF | 59.9–60.1 mm |
| Resulting range of the REF value | 59.7 to 60.3 mm | 14.7 to 15.3 mm |
The inspection consequence follows directly. An inspector who measures the version A overall at the top of its range has found nothing to report against the part. If the drawing was meant to control the overall, the fix is a drawing revision, not a rejection. Before release, run the same check on every chain: pick the one link whose variation you can live with, make that the reference value, and confirm the accumulated range still assembles. Where a press fit or clearance depends on the result, the clearance, transition and interference fits guide shows how to size the limits that matter.
Which reference dimension mistakes cause disputes with a supplier?
Almost every REF dispute traces back to one of five drawing habits. Each is cheap to fix before release and expensive to argue about after a lot has shipped.
- A functional value marked REF to avoid a tight tolerance. It removes the requirement, so the supplier has no obligation to hold it. If the value matters, tolerance it and accept what that does to the price; the cost of tight tolerances guide helps decide how tight.
- Inspectors applying the title-block tolerance to a REF value. The general tolerance applies to untoleranced dimensions, not reference ones. A receiving inspector who rejects a part on a parenthesized value has created a nonconformance that does not exist.
- REF values that no longer match after a revision. Change a toleranced step and forget the reference overall, and the print now contradicts itself. The supplier will raise a question, and the job stops until it is answered.
- Reference values that disagree with the CAD model. When the model is supplied with the drawing, state which governs. In model-based definition, where the annotations live in the model as product and manufacturing information (PMI), the nominal geometry is carried by the model itself, so a reference annotation that disagrees with it adds confusion without adding a requirement.
- A REF value with no parentheses or label. A number that is meant as reference but drawn as a plain dimension becomes a requirement under the general tolerance, which is the opposite of what the designer intended.
One further trap is over-dimensioning without any REF marking at all: a fully toleranced chain plus a fully toleranced overall. The links can no longer all use their full tolerance at the same time, so the real tolerances are tighter than drawn and the print does not say which dimension governs. Mark one link as reference, or delete it.
How should reference dimensions be handled on the RFQ, purchase order and inspection report?
Say in writing whether reference values are to be measured and recorded, because the standard alone tells the supplier only that they are not acceptance criteria. Whatever you want reported must be on the RFQ, so it is priced in.
First-article practice varies by industry. Aerospace first-article reports built on SAE AS9102 account for every design characteristic on the drawing; supplier instructions that apply AS9102C typically allow the measured result for a reference dimension to be omitted, and customer instructions differ on whether the line is listed and marked as reference or left off. Automotive PPAP under the AIAG PPAP manual asks for dimensional results against the design record, and the same question applies. The ballooned drawing guide shows how to mark a reference line on the report if you want one. Useful wording for an industrial part:
- On the drawing:
DIMENSIONS IN PARENTHESES ARE REFERENCE ONLY AND ARE NOT INSPECTION CRITERIA.ASME Y14.100 covers how general notes like this are laid out on an engineering drawing. - On the RFQ or PO, if you want data:
REFERENCE DIMENSIONS TO BE MEASURED AND RECORDED ON THE FIRST ARTICLE REPORT FOR INFORMATION; NOT GROUNDS FOR REJECTION. - If you want a reference value watched in production, it is no longer a reference value. Revise the drawing to tolerance it, or issue a written deviation that says what limit applies.
For the rest of the package that keeps an overseas quote accurate, see how to prepare a machining RFQ and first article inspection for an overseas supplier.
How does Saola treat reference dimensions on your drawing?
Saola reads every tolerance, callout and note during drawing review and sends back a marked-up copy of your own drawing, so a reference value that conflicts with the toleranced dimensions is raised at drawing review, before the first article is made, rather than at inspection. The first-article report covers every toleranced dimension on your drawing.
Because a reference value is not toleranced, tell us in the RFQ if you want it measured and recorded on the first article or on the dimensional record that goes with each lot. If a value matters enough to watch through the run, mark it on the drawing as a process-capability control point; the quality page explains that marked dimensions are checked more often than the rest of the print. Turned parts run on CNC turning, and machined castings and blanks on CNC milling. To have a drawing reviewed this way, send it for a quote.
Frequently asked
Can a supplier reject or rework a part because a REF dimension is off?
No. A reference value is not a requirement, so it cannot make a part nonconforming. If a supplier sees a reference value that cannot be reached while every toleranced dimension is met, the right step is a written question to the buyer, because it means the drawing contradicts itself.
Does the general tolerance block apply to dimensions in parentheses?
No. Per ASME Y14.5 the general tolerance covers untoleranced dimensions that are requirements; a reference dimension is informational and carries no tolerance at all. The same logic applies to auxiliary dimensions under ISO 129-1, and to the default classes described in the ISO 2768 and NADCA tolerance guide.
Is “REF” still acceptable, or must I use parentheses?
Parentheses are the current method in both ASME Y14.5 and ISO 129-1. A legacy drawing that uses REF is still understood and keeps its meaning; there is no need to revise it only for notation, but new drawings should use parentheses so the convention is consistent across the print.
What is the difference between a reference dimension and a basic dimension?
A basic dimension, shown in a box, is a theoretically exact value that locates or defines a tolerance zone given in a feature control frame, so it is part of a requirement. A reference dimension, shown in parentheses, is redundant information and part of no requirement. Swapping one for the other changes what the inspector has to verify.
Should reference dimensions be ballooned?
Normally not. If your system balloons everything or your customer asks for it, give the line a balloon, record the value if requested, and mark the accept column as reference only so nobody treats it as a pass or fail result.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ISO 129-1:2018, Technical product documentation — Presentation of dimensions and tolerances — Part 1: General principles, ISO, 2018
- ASME Y14.100, Engineering Drawing Practices, ASME, accessed October 2026
- SAE AS9102C, Aerospace Series – First Article Inspection Requirements, SAE International, 2023
- Production Part Approval Process (PPAP), 4th edition, AIAG, 2006
- MBE PMI Validation and Conformance Testing Project, test models and results, NIST, accessed October 2026