# Metric dimensions in ( ) or [ ]

What is the proper way of showing on the drawing metric dimensions (dual dimensions). Is it with square parenthesis, just like solid works does it?
Does anybody know what ANSI standard # it is?
I got someone here that keep saying that metric dimensions should be in ( ) not [ ]
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I don't know what the standards say, but I've NEVER seen anything other than square brackets [xxx] for dual dims. Regular parenthese (xxx) are for reference dims.
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That70sTick wrote:

I'll second that notion, (n.nn) is reference dims, [n.nn] is for dual dims. not necessarily metric dims, just the opposite dimension of what the drawing is.
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On Feb 20, 6:13 am, "mr.T" <mr.T@Somewhere Far away from the rainbow.com> wrote:

Can this person provide a reference for this?
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According to the following reference:
Modern Drafting Practices and Standards Manual originally Published by The General Electric Company my copy is published by Genium Publishing Corporation 1988 currently available at http://www.draftingzone.com/faq /
DUAL DIMENSIONING IDENTIFICATION OF METRIC EQUIVALENTS
The inch and millimeter dimensions must be identified, one from the other by square brackets [ ] surrounding the millimeter dimensions and placed adjacent to the inch dimension. Position is optional, selecting the method which best fits into the available space.
~George
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I also checked my ANSI Y14.5M - 1982 ( I know this is old )
latest rev is: ANSI/ASME Y14.5.1M-1994 (R1999)
This standard states... Two methods were recommended to distinguish the U. S. customary unit from from the SI unit - either the position method or the bracket method...
Then there is a diagram that shows both methods and the brackets are indeed, square brackets [ ].
However, at the end of this paragraph it says... Dual Dimensioning is no longer featured in this Standard.
~ George
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mr. T,
I have ASME Y14.5M-1994. There is no mention of dual dimensioning in the standard whatsoever. This surprised me cuz I just assumed it was in there. The only suggestion is that if dimensions of one unit appear on a drawing that is drawn in the other unit, then it should be followed by the appropriate unit symbol.
This makes sense since having dual dimensions can create confusion in how to convert units, and allows for two interpretations of the drawing (which is not allowed by the standard).
If you wish to use dual dimensioning, you could either invoke an older ASME version (1970's edition), or add a note to the drawing that explains how they apply.
However, do not use parenthesis for dual dimensioning. This will be confused with any ASME Y14.5M revision for reference dimension.
Personally, I would suggest just not using them. If you need metric, make it a metric drawing. If you need inch, then make it inch.
Matt Lorono http://sw.fcsuper.com http://www.fcsuper.com/swblog
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wrote:

mr. T,
I have ASME Y14.5M-1994. There is no mention of dual dimensioning in the standard whatsoever. This surprised me cuz I just assumed it was in there. The only suggestion is that if dimensions of one unit appear on a drawing that is drawn in the other unit, then it should be followed by the appropriate unit symbol.
This makes sense since having dual dimensions can create confusion in how to convert units, and allows for two interpretations of the drawing (which is not allowed by the standard).
If you wish to use dual dimensioning, you could either invoke an older ASME version (1970's edition), or add a note to the drawing that explains how they apply.
However, do not use parenthesis for dual dimensioning. This will be confused with any ASME Y14.5M revision for reference dimension.
Personally, I would suggest just not using them. If you need metric, make it a metric drawing. If you need inch, then make it inch.
Matt Lorono
Just to chime in on that last note, Matt...while I'd had loved to do so while I was at my last place, it was not possible. When a part was quoted (or made) in both China, India, Korea and U.S., dual dims were needed. I will also say that it also created problems, as a 3 place decimal (inch dim) was usually provided as a 1 or 2 place metric dim. It took twice as long to create prints because almost every dim had to have tolerances on it (as opposed to a generic tolerance box in the title block) to make certain that the metric dim would fall within the inch tolerance with the rounding up or down with metric: dwg states: .500±.005 [12.70±0.13] if made using metric, part could be: .5051 max / .4948 min. Both of which fall out of the intended min/max of the inch design, but are within the metric tolerance. So you would have to tighten either the inch or metric tolerance. And depending on how tight your part is, tolerance stack-ups would need to be verified in both inch and metric. A real PITA especially if you had to make sure if fit with a part manufactured using inches. My current company uses all inches. But I do wish that all the world used the same damn system...(actually, they do, the US won't, which is the dumbest thing... Wish they'd get their act together and get it right....which is to get the world back on the inch system!! lol ;)
Sorry for the rant...
IYM
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So it is not just me...
Thanks guys
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