Dual Dimensioning and ASME Y14.5M-1994

Dual dimensioning is the drafting practice of using multiple units of measure in a dimension in the same direction of a feature.  SolidWorks and many other CAD programs support dual dimensioning.  This support is usually a little quirky.  It’s actually not  the fault of the CAD application.  At one point, it was a surprize to me (and often is to others too) that no current drafting standard actually supports dual dimensioning.  In retrospect, this makes perfect sense.

My experience is with ASME Y14.5M-1994.  When invoking ASME Y14.5M-1994 (or even ANSI Y14.5M-1982), one will find that rules regarding dual dimensions do not exist.  ANSI Y14.5M-1982 does mention in its appendix that support for dual dimension no longer exists in the standard.  This is apparently because it was mentioned in a previous version.  That said, dual dimensioning has never really ever been allowed by any incarnation of Y14.5.  This is because of very specific wording under the standard’s Fundamental Rules.  The wording may vary between versions, but carries the same meaning in all versions.  In ASME Y14.5M, that wording is as such in 1.4(d), “Dimensions shall be selected and arranged to suit the function and mating relationship of a part and shall not be subject to more than one interpretation.”  (Support for dual dimensions in pre-1982 versions was a mistake that was likely political in nature.)

General practice in the use of dual dimensions is that they are of equal importance to the primary dimension.  This creates issues in that it allows for more than one interpretation of the dimension.  It is nearly impossible for nominals and tolerance ranges to be identical between units of measure.  This means that the dual dimension tolerance range is usually resized to fit within the tolerance range of the primary unit of measure.  This creates a situation where the dimension has more than one interpretation, which is specifically prohibited by 1.4(d).  The conclusion that can be drawn from this is that dual dimensions are actually not allowed by ASME Y14.5M-1994.  This is the hard argument against the use of dual dimensions.  I could end this article right here.  However, I will also explore the soft arguments against their use.

ASME Y14.100-2004 paragraph 4.32.3 uses soft language to discourage the practice of converting inch to metric and vise verse (“should not be used”).  This is known as soft conversion.  This is not an outright prohibition against dual dimensioning by itself. However, the practice of soft conversion is integral to using dual dimensions.  With this practice discouraged, dual dimensioning is also discouraged.

ASME Y14.5M-1994 defines a reference dimension as such,

“A dimension usually without tolerance, used for information purposes only. A reference dim is a repeat of a dimension or is derived from other values shown on the drawing or on related drawings. It is considered auxiliary information and does not govern production or inspection operations.”

By definition of reference dimensions, dual dimensions must be treated as reference dimensions. However, anyone who uses them knows this is generally not their intent. As generally intended, dual dimensions are disallowed unless they are considered reference only.

The final soft argument is gleamed in the wording of ASME Y14.5M-1994 paragraph 1.5.  This paragraph assumes dual dimensions are not in use.  For example it begins one paragraph as so, “Where some inch dimensions are shown on a millimeter-dimensioned drawing…”.  It never then says “Where many inch dims are used on a metric drawing….” This is not a specific exclusion, but should be noted for its wording. It does allow for the use of both inch and metric units on the same drawing, but not multiple values of dimensions for the same features.

With all of these arguments aside, CAD applications do attempt to accommodate users who feel they need this capability.  However, if used, caution must be exercised.  Handling of dual dimensions by CAD (and common practice) can create confusion on a drawing, particularly if the software assumes values for the dual dimensions and its tolerances.

In the effort to avoid issues and violations of the standards, it is my opinion that if dual dimensions are used, they should be noted as for reference only on the drawing.  This can be accomplished by adding a note similar to “DUAL DIMENSIONS IN BRACKETS ARE FOR REFERENCE ONLY.”  This avoids problems caused by multiple interpretations for dimensions.  Of course, over use of reference dimensions is also discouraged by ASME Y14.5M-1994. But hey, who’s it hurting?

For SolidWorks, dual dimensions on a drawing may be employed by going to Tools>Options>Document Properties>Detailing and checking Dual dimensions display.  Also at that location is the choice to display the dual dimension on top, bottom, left or right of the primary dimension.  These are SolidWorks 2007 instructions (other versions of SolidWorks should be similar).

I did make a sample SolidWorks macro that will turn on dual dimensions for a drawing and automatically set them to display on the bottom (default is top).  This example macro can be downloaded here.  It can be modified to use any settings as default.

For the record, this article was inspired by multiple posts on various SolidWorks related forums over the past few months such as these at SW Forums, eng-tips.com, and Pro/E discussion at eng-tips.com.

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