Significant Figures On Dimensioned Drawing When Converting Units 7

[JonnyK]

Hello,

The mechanical drawings that my company generates are in standard units (inches) and typically to the one-thousandths place (i.e. .001).

However, we have some drawings that require (for European customers) that dimensions be called out in both inches and millimeter.

Standard practice is to call out the millimeters to the one-hundredths place.

So a length of 4.125” would be dimensioned as “104.78 [4.125]”.

Does this make sense to have the SI units with five significant digits while the Standard Units only have four significant digits?

The conversion is being done by the CAD system so maybe significant figures are unimportant, and it is usually clear what the drawing dimensions imply.

I was just wondering how other people have/would address this issue. Or maybe it is not an issue and just anal-retentiveness.

Any feedback would be appreciated.

TIA

 

[KENAT]

Take a look over in GD&T, this or similar came up a while back. Someone thought they'd read that it was standard practice to add a sig fig when doing this conversion.

If in doubt look at function:

In your case the exact conversion is 4.125" = 104.775mm.

104.8-104.775 = .025mm or about .001".

Depending what you're dimensioning adding or losing a thou here or there could definitely cause problems.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[drawoh]

JonnyK,

It is not significant figures in the sense of doing scientific calculations. It is the number of decimal points. Typically, most people use one less decimal when showing metric dimensions.

How accurate are your actual parts? There is no point quibbling over .001" or .01mm increments on a weldment that is accurate to ±1/16" (±1.5mm). Note how sloppy my tolerance conversions are.

JHG

 

[IRstuff]

"Does this make sense to have the SI units with five significant digits while the Standard Units only have four significant digits?"

Yes, because in your original units, a 1 mil change is about 0.025%. If you leave off the 5 significant figure in the new units, a 0.1 mm delta represents 0.095%, a substantial change.

TTFN

FAQ731-376

 

[katmar]

I'm with IRstuff on this one - use the extra significant digit. Presumably the components have not been redesigned and the tolerances have not been set in terms of the actual dimensions in SI units, so you need to play safe. I would also cover myself by adding a note on the drawing along the lines of "In case of doubt or conflict imperial units take priority".

Katmar Software
Engineering & Risk Analysis Software

http://katmarsoftware.com

 

[JonnyK]

KENAT

I think this is the post you are referring to:

http://www.eng-tips.com/viewthread.cfm?qid=206463&page=1

I found it today when searching for ‘GD&T’. Although the post is referring to tolerances it answers my question indirectly. Since we have a similar tolerance conversion note our drawing, I would have inadvertently changed the tolerance of the dimension in question.

drawoh

“ It is not significant figures in the sense of doing scientific calculations. It is the number of decimal points.”

This is the answer to the questions I was asking in a round-about way. I was trying to treat the dimensions as I would a scientific calculation (i.e. 1.000 in * 25.4 mm/inch), and it appears that this is not the right way to handle dimensions on a drawing.

IRstuff

“Yes, because in your original units, a 1 mil change is about 0.025%. If you leave off the 5 significant figure in the new units, a 0.1 mm delta represents 0.095%, a substantial change.”

I agree, it did give me heartburn but at the time it seemed technically correct so I was conflicted.

katmar

“I would also cover myself by adding a note on the drawing along the lines of "In case of doubt or conflict imperial units take priority".

I like this idea, not sure if our drafting department will like it, but it seems like it is worth a try.

Thanks again.

 

[TVP45]

The question is already answered, but I'd like to add a comment on why it's important to always use good judgement and have an awareness of actual manufacturing tolerances (By the way, many packages allow you to keep the "exact" dimension hidden and that's a really good idea). I recently worked with a set of drawings that had been moved from US standard units to metric years ago and were now being moved back to US standard. Both times, a conversion program had been run. The problem was that I found sheet metal dimensions with 5 decimal places! And, because of the huge cost involved in doing stacking analysis, nobody was willing to truncate. I can only wonder at the huge extra cost this must involve (although I suspect the sheet metal shops really come as close to 3 places as they can and then just charge for the other two).

 

[TheTick]

Is there a standard for this? I was taught that the dual-unit portion was reference only, and that the primary units were the governing value.

 

[KENAT]

Maybe I'm imagining it, I swear there was a thread discussing decimal and/or sig figs on conversions and/or dual dimensions. I thought it was started by ringman or ringster but can't find it, I may have been confused & thinking of the one you found or one of those below, neither of which fully answer your point.

thread1103-225708 thread1103-120758

This is addressed in the standards:

1.6.4 Conversion and Rounding of Linear Units. For information on conversion and rounding of U.S. customary linear units, see ANSI/IEEE 268

http://ieeexplore.ieee.org/Xplore/login.jsp?url=/iel1/2881/5489/00210930.pdf?temp=x

Genium Manual has a section on conversion in 6.9

http://www.draftingzone.com/shoppingzone/DM_TopicList.pdf

They say a lot about it, too much to really try and put here but one simplification they give is use one less decimal place for mm than for inches so...

.365 inches becomes 9.27 mm

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[ProfDon]

Don't forget the limits of the dimension due to tolerance. You are not allowed to increase the tolerance as a result of rounding. The safest way to convert is to determine the limits, perform the conversion and round in. Attached is a page on Conversions from the Tec-Ease, Inc. GD&T Hierarchy Pocket Guide copied with their permission.

 

[miner00]

Do yourself a favor, put reference markers around the metric units and make it VERY clear that the english units are the driving ones.

I am in the process of removing the secondary tolerance block from a big bunch of drawings (inherited from a swedish company). A small slip on a decimal point in a secondary unit can trash your parts.

Good Luck!

 

[eromlignod]

The concept of significant figures as an implied tolerance based on how many digits are shown after the decimal point is used mainly in scientific calculations, not engineering drawings.

I have been in industry for 22 years and virtually all the drawings I have dealt with included an explicit table in the title block declaring what the default tolerance is for each number of decimal digits (if not superseded by a tolerance on the dimension itself). And they are almost never one figure of accuracy (e.g. +/-.001 for three decimal places). Usually three decimals is something like +/-.005, two is +/-.015, etc.

Metric units are usually bracketed [] in an English-based system, and while it is customary to use fewer digits after the point, they are for reference only and un-bracketed primary dimensions always drive the tolerancing.

Don
Kansas City

 

[4grand]

The following is an excerpt from NASA Document GSFC-X-673-64-1F, ENGINEERING DRAWING STANDARDS MANUAL, which answers your question....

"Generally, the accuracy of the number of significant digits to which a value is to be rounded must be known before a conversion factor is used. If this is not known, then the best rule of thumb is to round the final value to the number of significant digits corresponding to the least number of significant digits of the original, unconverted numbers. For example, to convert 11.4 feet (ft) to meters (m): 11.4 x 0.3048 = 3.47472, which rounds to 3.47 meters. Neither the conversion factor nor the quantity shall be rounded before performing the multiplication, because accuracy would be reduced. For converting inches (in) to millimeters (mm), which would generally be the case in drawings, the rule of thumb is to round to one less decimal place than the original inch dimension. When converting from millimeters to inches, the rule is to round to two more decimal places than the original value.

Example: Convert 3.5748 inches to millimeters.
3.5748 x 25.4 = 90.79992 Answer: 90.800 mm
Example: Convert 1.625 inches to millimeters.
1.625 x 25.4 = 41.275 Answer: 41.28 mm
Example: Convert 101.83 millimeters to inches.
101.83/25.4 = 4.009055118 Answer: 4.0091 inches"

I hope this is helpful.

 

[juergenwt]

JonnyK - You can use a Box like this:

http://www.ams-prototipi.it/webfiles/iso.pdf

In general it is best to have a person fluent in both systems look at your print. Converter programs can be a pain in the neck when used to convert prints for someone in the rest of the world. Common sense should be used. First have a knowledgeable person look at it and determine what is important.
3/4" could be 19mm and 5/8" could be 16mm etc.
Depending of the kind of work you do overall dim's should be rounded to the nearest solid metric dim..
In most places of the metal industry unless otherwise noted it would be +/-0.1mm. That would be where we would use +/-1/64th". Let's take a 1/4" hole - if we would use 1/4 you could use 6.4mm but if it was .250 +/- 0.0002 you would have to use The ISO system of fits found here:

http://www.engineersedge.com/iso_tolerance.htm

Now keep in mind if you had a screw hole for a 1/4" screw and your print says 1/4 + 1/64th or 17/64th that nobody but the US uses 1/4" screws. You would most likely end up with a 6mm screw and your hole would be way to big ( 6.35 +0.4mm). So you would have to change that to 6.3mm. See what i mean with having someone familiar with both systems look at it?
You would almost never use three decimals on a metric print.
If you have a tol. that is that close it would almost always have a fit involved and you would use the ISO system of fits and tolerances as per DIN ISO 286 part 1 and 2.
I urge you to study the ISO system and use it on all your print conversions. That is how the rest of the world operates. Look on the internet for DIN ISO 286.
I am adding a drawing explaining the ISO 286. It is from an old school book and in German with added translations but it will help you to understand the system. Clk. here:

Post if you need more info.

 

[ProfDon]

juergenwt brought up a good point regarding fits. Where the fit is size on size you can refer to the American National Standards for both metric and inch in:
B4.1 Preferred Limits And Fits For Cylindrical Parts
B4.2 Preferred Metric Limits And Fits
B4.3 General Tolerances For Metric Dimensioned Product
If the location and/or orientation of the feature will affect the assembly you need to turn to ASME Y14.5. The ISO 2768 standard is ± tolerances which is not recommended to control location or orientation. The ASME Y14.41 Digital Product Definition Data Practices standard allows embedding tolerances in solid models. This standard recommends that ± tolerances be used for size because locating features with ± is open to interpretation. Geometric tolerances should be used for location and orientation.

 

[zekeman]

Look, if the call in mm units is to .01 mm, then the equivalent accuracy in inch units is .01mm*.04in/mm =.0004" which says the call is twice as tight as the .001" ; but if the mm call is only to .1 mm, the equivalent inch call would be to .004" , which would be a factor of 4 too high.
So the mm call has to be to the .01mm for at least the accuracy of the .001".
Hope this jumble makes sense?