Guide
Dual dimensioning in inches and millimeters: which value governs, and what can go wrong?
Dual dimensioning is showing each dimension in two units, usually inches with millimeters in brackets, on the same drawing. Only one unit can govern: state the primary unit in a note, mark the other values as reference only, and inspect to the primary unit, because rounded conversions can quietly widen a tolerance.
By Saola Manufacturing engineering team · Published · Updated
A drawing sent abroad often picks up a second unit system along the way. That is a different problem from projection, which the first angle vs third angle guide covers, but it causes the same kind of argument at receiving inspection: two readings of one drawing.
On this page
Does ASME Y14.5 allow dual dimensioning?
ASME Y14.5 has given no rules for dual dimensioning since support was dropped in the 1982 edition, and the standard requires that dimensions not be open to more than one interpretation. So a dual-dimensioned drawing has to say, in a note, which unit governs.
A Dassault Systèmes SolidWorks blog summary of the history notes that the appendix of ANSI Y14.5M-1982 already said support for dual dimensioning no longer existed in the standard, that the 1994 and 2009 editions contain no dual-dimension rules, and that Y14.5M-1994 requires dimensions that shall not be subject to more than one interpretation; it also points out that ASME Y14.100 uses soft language to discourage converting inch drawings to metric (SolidWorks blog, Discussion about dual dimensions, 2012).
In practice, many CAD templates still offer dual display, and inch drawings sent to metric suppliers often carry bracketed millimeters added by someone trying to help. The help is real only if the drawing says which number is the requirement. Without that note, a supplier can choose the unit whose rounded limits are easier to meet, and both sides can claim to be right.
How can a converted tolerance accept a part the original rejects?
When converted limits are rounded to the nearest digit, one limit can move outward, so the secondary-unit tolerance becomes wider than the primary. A part measured in the secondary unit can then pass while being out of tolerance in the primary unit.
The inch is defined as exactly 25.4 mm; the NIST guide to the SI lists the factor 2.54 E-02 meter per inch as exact (NIST SP 811, Appendix B.8). The conversion itself is never the problem. The problem is rounding: NIST's guidance in Appendix B.7 is to round a converted value to a precision comparable with the original, not to keep every digit, and that rounding is where the tolerance moves (NIST SP 811, Appendix B).
| Primary limits (in) | Exact conversion (mm) | Rounded to nearest 0.01 mm | Rounded inward to 0.01 mm | Effect of nearest rounding |
|---|---|---|---|---|
| 0.2500 to 0.2510 | 6.3500 to 6.3754 | 6.35 to 6.38 | 6.35 to 6.37 | Upper limit 6.38 mm is 0.2512 in: wider than the drawing |
| 0.498 to 0.502 | 12.6492 to 12.7508 | 12.65 to 12.75 | 12.65 to 12.75 | Both limits move inward: tighter than the drawing |
| 1.000 to 1.004 | 25.4000 to 25.5016 | 25.40 to 25.50 | 25.40 to 25.50 | Upper limit moves inward slightly |
The first row is the dangerous case. A part measured at the bracketed upper limit passes in millimeters and fails in inches. The second row shows the opposite risk: the supplier works to a tighter band than you need and prices it accordingly. Rounding limits inward, so the converted band always sits inside the original, removes the first risk but keeps the second, which is why the governing unit has to be stated.
Which unit should govern?
The unit the part was designed in should govern, because that is where the tolerances were worked out. Put it in a general note and make every bracketed value reference only.
The SolidWorks summary suggests controlling dual dimensions with a note that they are for reference only, for example DUAL DIMENSIONS IN BRACKETS ARE FOR REFERENCE ONLY, while noting that overuse of reference dimensions is itself discouraged (SolidWorks blog, 2012). The reference dimensions guide explains why a reference value is never inspected.
| Situation | Recommended practice | Why |
|---|---|---|
| New inch design sent to a metric supplier | Inch only, or inch primary with bracketed mm marked reference | Tolerances were designed in inches; the supplier can convert for its own use |
| Supplier asks for metric values | Supplier converts on its own planning documents; drawing unchanged | Keeps one controlled requirement |
| Legacy dual drawing with no governing note | Query before quoting; add the note at the next revision | Avoids choosing the easier rounded limits |
| Metric drawing with inch stock or thread sizes | Mark the inch values with IN and keep thread callouts in their native form | A UNC or NPT callout is a designation, not a dimension to convert |
| GD&T tolerances and surface finish values | Give them in the primary unit only | Converted geometric and roughness values invite the same rounding errors |
How should the drawing and RFQ be worded?
Add a general note naming the primary unit and marking bracketed values as reference, and repeat it in the RFQ. Ask the supplier to plan, gauge and report in the primary unit.
Generic wording to adapt:
DIMENSIONS ARE IN INCHES. VALUES IN [BRACKETS] ARE MILLIMETERS FOR REFERENCE ONLY. INSPECTION AND REPORTING IN INCHES.
If the title block carries a decimal-place general tolerance, it applies to the primary unit. A general tolerance written for inch decimals, such as two- and three-place values, has no meaning for bracketed millimeters, so do not let the supplier apply it to them. For the default tolerances that apply when nothing is stated, see the standard machining tolerances guide.
On a metric drawing that must call an inch-sized item, such as a bar stock size or a fastener, common practice is to mark the inch value with IN so it is not read as millimeters. Thread designations stay as written; a 1/4-20 UNC thread is gauged to its own standard, not to a converted diameter.
How is a dual-dimensioned part inspected and accepted?
Inspect with instruments set or read in the primary unit, record results in that unit, and reject on the primary limits only. If a report lists both units, the primary column decides.
Most digital micrometers, calipers and vision systems switch units with a button, which is exactly how a lot gets measured in the wrong one. Ask that the inspection report header state the unit, and that the first-article report use the primary unit for every line. If a dispute arises, convert the measured value with the exact factor and compare it with the primary limits; never compare it with a rounded bracketed limit.
For fixed gauges, buy or make them to the primary unit. A metric plug gauge sized to a rounded conversion of an inch limit carries the same rounding error as the bracketed number on the drawing.
How does Saola handle a dual-dimensioned drawing?
A drawing without a governing-unit note is queried at drawing review, and the answer is recorded before quoting. Parts are then planned and inspected to the unit you confirm.
Turned and milled parts run on the lead plant's CNC turning and CNC milling lines from your drawing as released. The first-article report and the dimensional inspection record each lot, described on the quality page, are written in the governing unit you confirm.
Send the drawing for a quote, and if it is dual dimensioned, say in the RFQ which unit governs.
Frequently asked
Is soft conversion the same as dual dimensioning?
Soft conversion is restating an inch design in metric numbers without changing the part; dual dimensioning shows both on one drawing. Hard conversion changes the design to round metric sizes, which is a design change, not a drawing format.
Should bracketed values be rounded inward?
If you keep them, yes, rounding inward keeps the converted band inside the original. But marking them reference only and inspecting to the primary unit is the safer fix.
Can a supplier work in millimeters on an inch drawing?
Yes, on its own programs and planning sheets. What matters is that acceptance is judged against the primary limits, converted with the exact factor.
What about angles and threads?
Angles in degrees need no conversion. Thread designations such as UNC, UNF, NPT or metric M sizes are standard designations and should never be converted to the other unit system.
Sources
- NIST Special Publication 811, Guide for the Use of the International System of Units, Appendix B.8 (inch to meter factor, exact), National Institute of Standards and Technology, 2008 edition
- NIST Special Publication 811, Appendix B: Conversion Factors, section B.7 (rounding converted values), National Institute of Standards and Technology, 2008 edition
- Discussion about Dual Dimensions, Matt Lorono, Dassault Systèmes SolidWorks blog, August 2012