How do you measure a non-feature of size 1

[MartinSr00]

I've read through both the ASME Y14.5M-1994 and Y14.5-2009 standards. They are very clear about how to measure features of size. For example: The minimum dimension on an external feature of size is the unrelated actual mating envelope. The maximum is the largest local size. Clear enough.

But what of measurements that are not features of size. For example, the length of a step in a shaft, where the surfaces to be measured are unopposed.

Look at the attached drawing. What is the min and max dimension for Dimension "A"?

 

[SeasonLee]

The step is not a feature of size, you can’t think it as what shown on your print, I will recommend you to think this way:

The overall length is a FOS, let’s assign it X
Max A = Max X – Min of 1.00
Min A = Min X – Max of 1.00

SeasonLee

 

[NomLaser]

E. None of the above.

Using a measuring bar (sorry can't think of the proper name), you would measure down from the surface on the right to get the correct depth of A. How many measurements depends on how tight the parallel or perpendicular tolerance is.

 

[MartinSr00]

Thanks NomLaser and SeasonLee for your reasoned responses.

How do we know these things? Is there a paragraph in the 14.5 Standard that supports these interpretations?

If I understand it, NomLaser says that we measure everything from the high side of right hand vertical feature. Why not from the high sides of the left hand vertical feature (at the right end of the 1.00 dimension)?

SeasonLee says that we would essentially measure from both the highs and lows of the right hand vertical feature. Remember, I haven't dimensioned the overall in my picture. I've dimensioned one feature of size 1.00 with a tolerance of plus/minus something, and a non-feature of size "A". Whether or not this is recommended practice, it is allowable. I see similar examples in the Standard.

I find either one of these answers quite plausible. I could make a persuasive argument for either case.

But what does the 14.5 Standard say? Where? I have trouble reaching a definitive conclusion that one can hang their hat on.

They give a bit of a clue on origin dimensions in one of the Figures in the 14.5 Standard. But the example they show is a feature of size.

For me, the standard is so crystal clear in every respect for geometric tolerances, and limit or plus/minus tolerances for features of size. I see a hole in their definition for non-features of size.

Did I miss a paragraph in the 14.5 Standard? I've read them both a couple of times.

I have copies of both the 1994 Standard and the 2009 Standard. If anyone can nail this down, I'm very interested.

Once again guys, thanks much for your posts!

 

[KENAT]

I believe one of the references at the start of 14.5 is to an inspection spec or something. Would this have any answers?

Posting guidelines faq731-376

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

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[MartinSr00]

One that might have something to do with it could be ASME Y14.5.1M-1994(2004) "Mathematical Definition of Dimensioning and Tolerancing Principles". in Section 1.2.1 "Cited Standards".

In Section 2.6 "Tolerance Accumulation", they show some non-feature-of-size dimensions. In 2.6(c) "Direct Dimensioning", they state "The maximum variation between two features is controlled by the tolerance on the dimension between the features. This results in the least tolerance"

This may agree with my original post.

I'm thinking this way: with a feature of size, Rule number 2 holds. So, on an external feature, the maximum size is the unrelated actual mating envelope. This is so a 2.00 dia. pin will fit in a 2.00 dia hole.

But the minimum size is the min local size.

Well, for a non-feature-of-size, some projection needs to be made because the features are not opposed. That's why I proposed the method in my original post. But there's no way I can pound my fist on the table and say categorically, "This is the correct way".

As for measuring it first from one side, then the other, I can point to Figure 2-5 covering origin dimensions. But in this example, the origin feature shown is a feature of size, and is interpreted such -- the only difference is that one opposed plane forms the basis for measurement rather than either.

Again, let me know your thoughts. Thanks.

 

[powerhound]

Wow, this really seems to be a simple situation that has really been overthought and overcomplicated. You're not going to get what you're after without some datum structure. A primary datum will use the three high spots from one surface and create a plane from which to measure your other surface.
See Fig 4-10 for how the standard tells you how to derive a datum. While you are correct that this is not a feature of size, it has absolutely nothing to do with what you're asking about. A non-feature of size of this nature should still be set up with datum structure to avoid the issues you are addressing right now

Powerhound, GDTP T-0419
Production Manager
Inventor 2010
Mastercam X3
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MartinSr00]

Datums are applied via geometric controls and are not operative in this example. With Rule #2 for features of size you have a quasi-datum construct. The "A" dimension in my original post is not a feature of size.

If I've overcomplicated it, just simply give me the answer. Mark it on the drawing. And using the 14.5 Standard or one of it's referenced documents, tell where it says so.

Fig 4-10 in the 2009 Standard refers to datum plane establishment. This is not a datum plane.

Look at Fig 2-4(a), it shows non features of size and chain dimensioning -- all legal under the standard. My question is very simple -- if you have a part, from where-to-where do you measure to confirm the part is "in-tolerance". Is it from projected high spot to high spot? Total projected variation? High spot to low? Left to right? Right to left?

Because if you claim "A" is true, and another claims "B" is true -- absent a rule book, all we have is an argument.

If you were to tell a new inspector how to measure the part that I showed. What would you tell him/her? And how would you defend it using the standard?

So far, on the forum, I have three answers. (1) It means "A", (2) It means "B". (3) that's a dumb question and you've over-complicated it.

My question remains -- how do I properly inspect the part to see that its "in-tolerance".

The question is not "how do I change the drawing so it would be clearer?". The dimensioning is legal under the standard. What does it mean? Is the answer buried in a referenced document somewhere?

 

[dingy2]

Powerhound is correct but he has experience measuring as I have had. Nothing is written in the ASME standard on how to measure but we do have datum structure shown and how one theoretically would come from a datum or the use of datum targets.

Some people would argue that if the part is not shown with GD&T, then the dimension is strictly 2 dimensional. That is the reason many GD&T trainers love to push profile of a surface and positional in notes.

Many years ago, in my youth, I measured V-8 blocks, and other parts, using coordinate measuring equipment and there was no GD&T at that time. Yes, I did set up a datum structure using a 3 point for the primary, 2 point for the secondary and 1 point for the tertiary. It was the very same as today.

If there was a dimension to a surface, I would come from the datum structure to sweep the full surface and report its highest and lowest value.

In your case, I would use a height gauge and come from a developed datum structure and measure the 1.00 inch dimension and report my highest and lowest value. As an example it could be .997 - 1.002. Then I would measure the top of the stepped area but since you did not place a value on it, lets say the actual readings were from 1.498 - 1.505.

Step "A" is .496 (highest to lowest) - .508 (lowest to highest).

Dave D.

http://www.qmsi.ca

 

[MartinSr00]

Thanks Dave for your response. It sounds reasonable and highly defendable. What you're saying is, "derive this non feature of size (unclear) from clear and known adjacent features of size.

Typically, I wouldn't dimensions a production part like that shown in my example from the original post. It doesn't telegraph engineering intent. Normally, I would dimension the entire part basic, do an all-around profile tolerance with the plate surface being the only datum and lock in the part definition precisely.

But if someone were to ask you about a feature of size and how to measure it -- exactly -- you could find many examples in the 14.5 standard telling you how to do it. If you had applied geometric controls (say location or profile), it would be crystal, crystal clear how to tell if the part was OK. The standard's examples in these area are profuse -- maybe sometimes complex, but not unclear.

You see, I wish to teach others about interpreting the standard. I would tell them that "drawings must be subject to one interpretation" (from the fundamental rules). And looking in the Standard, I didn't find that interpretation for non features of size.

I know of many work-arounds to make everything perfectly clear. Build a datum structure and apply geometric controls and you have instant clarity. But if someone asks "what does this mean?" I find myself resorting to personal opinion.

One definition I would consider using is (1) the largest dimension is the smallest pair of parallel lines (or planes) that will just enclose the two features. (2) the smallest dimension is the largest pair of parallel lines (or planes) that will inscribe the features. I undertand that the orientation of the two sets of lines (planes) could be very different.

Thanks again for your reasoned response.

 

[axym]

I'll acknowledge the elephant in the room that MartinSr00 is pointing out. There is no definition of where to measure a real part to confirm that the dimension is within tolerance. It's not "A", it's not "B", and it's not a dumb or overcomplicated question. The answer is not defined anywhere.

The "A" dimension in Martin's diagram is an example of a "directly toleranced dimension". Y14.5 does a good job of explaining how to specify these on a drawing, but doesn't explain what they actually mean on a real part. The Y14.5.1 "math standard", which defines conformance and actual values for geometric characteristics, doesn't deal with directly toleranced dimensions. For good reason - they don't stand up to rigorous mathematical analysis.

I agree with the assertions that datums have nothing to do with this. Any attempt to superimpose a datum scheme on direct tolerancing is purely arbitrary. The scheme Dave suggests would greatly improve the repeatability of measurement, but other schemes giving different numbers would be equally valid.

To me, directly toleranced dimensions are a carry-over from traditional drafting. They offer a simplified (and sometimes oversimplified) view of the world, which causes specification uncertainty. The implicit assumption is that the form and orientation error of the surfaces is small compared to the location tolerance. In cases where this is a valid assumption, direct tolerancing is workable. This is why many designers still cling to it - because the errors it causes are insignificant in their particular applications. In other cases where form and orientation errors are significant, direct tolerancing falls apart completely. The effects shown in Martin's diagram are always present to some degree, but that degree depends on the magnitude of the tolerance and the geometric variation in the real parts.

If you want something with a well-defined meaning that you can hang your hat on, then you have to go to geometric tolerancing.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[dingy2]

Hold on now. I defy anyone here to show me in the standard a measuring method. The standard reflects the meaning but not how to measure?? Do I use a CMM? How about a height gauge? Maybe a attribute gauge is best? I know how to measure but I didn't gain that knowledge from the standard.

Where, as an example, does the standard show how one should measure a cylinder which is a feature of size? Most people know rule #1. Should I use a vernier? That will not check straightness would it and we cannot go beyond the outer boundary at MMC? Now where does the standard reflect any kind of measuring methods? Page 27 of the 94 standard certainly doesn't.

I do feel for other people who are also in GD&T training and they don't know how a feature is measured. What would one say when asked the best method to measure a feature of size? How about positional at MMC referencing datums at MMC?? One cannot say "carefully" and bluff your way through.

ASME Y14.5M-94 & also 2009 standard do not show measuring methods only the meaning of the geometrical criteria using dotted lines.

Dave D.

http://www.qmsi.ca

 

[MartinSr00]

Wow! Well reasoned. As I searched in vain for a "correct" answers, I couldn't find it. It's nice to know that I'm not sitting alone in a dark room wearing a tin-foil hat trying to read everyone else's thoughts. Ha Ha.

So I have my answer, Evan. You confirmed what I was thinking. OK, direct tolerancing does fix size when applied to features of size. But only size. Not orientation or location.

What I would now tell any students would be, "if you do this, you'll be on uncharted territory -- for the cost of a line or a few symbols, you can switch from a poor definition to a solid definition of your part."

Thanks Evan

Martin Smith
Metropolitan Water District of Southern California

 

[ewh]

It's nice to know that I'm not sitting alone in a dark room wearing a tin-foil hat trying to read everyone else's thoughts.

Silly, you have to take the hat off to be able to do that!

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[MartinSr00]

Dave D

Sure, the 14.5 standard doesn't describe the measurement means and methods, but it specifies the quantity to be measured. For a feature of size, the specifiecation is the envelope rule for the MMC side, and local size on the LMC side. (with a built-in exeption if the geometric tolerance is expressed LMC)

For the origin dimension, it's from the high spots on the origin to high/low spots on the other dimension (note how figure 2-5 has been updated for the 2009 standard).

But for non features of side, there's no spec I can find. So you can take all the cmm machines or calipers, etc., but in the end, the standard won't guide you on what to measure. You can accurately measure anything you choose. You just don't know what to choose.

The standard is not about means and methods. So it won't tell you how. But it better tell you what if you mean to control your geometry so your parts will reliably fit.

 

[dingy2]

MarinSr00:

I agree that the standard does not show the meaning of +/- tolerances with dotted lines where if one had a profile of a surface, the meaning is shown.

Of course, it there were no tolerances shown on the drawing with only a 10 mm dimension, I would ask Engineering to define the tolerance.

Having a background in the Quality field, I just know that if there was a dimension of 10 mm +/- 0.25, it would mean that we have an upper limit of 10.25 and lower of 9.75 and nothing on the surface can be above 10.25 or below 9.75.


Dave D.

http://www.qmsi.ca

 

[dingy2]

MartinSR00:

I just came across this in ASME Y14.5 -2009 on page 27 figure 2-5. I shows a 12 +/- 0.4 dimension to a surface from another surface with an origin symbol.

It does reflect that the surface in question can go up to 12.4 and down to 11.6.

I believe that this is the example from the standard that you were searching.

Dave D.

http://www.qmsi.ca

 

[MartinSr00]

Dave D

Thanks for your post. These are all helpful in scoping out this problem. The issue isn't purely academic -- I came across the problem while doing some research for a possible book.

You're absolutely correct with if you use a dimension origin. The 14.5 Standard is quite specific in this area. I recommend to others that if they use limit and plus/minus dimensions without a datum structure, they should use dimension origins. This was one of the first things I looked at before sending my first post.

Note with dimensions relative to origins, it's high spots on the origin, to all spots on the other end. Note also that the 2009 standard changed this diagram to make it clearer.

My current prejudice is to favor Evan's explanation from October 9.

But if there's no origin then what? Is it the minimum of the minimums when measured from both possible origins and the maximum from maximums when measured from both possible origins? Is it pick either for best effect? What exactly is it? It would be easy enough for the Y14.5 Commitee to say, but they didn't. I suspect it has to do with that any strict rule may not be very workable in all situations. I'm almost certain that it isn't because the Y14.5 Committee forgot or didn't recognize the problem.

The 14.5 Standard is very specific in exhaustive detail in nearly every other area of measurement. I've seen all these posts with differing versions about how they would do it given their experience. They all seem valid to me even when they don't agree. The problem is, with the 14.5 standard silent, they're all just opinions.

After researching it, I think the best practice is to use dimension origins when you must dimension non-features of size. Then it's clear.

Again, thanks Dave for weighing in on this.

 

[fsincox]

I am a little perplexed with the responces here, the 1.00 dimension on the drawing I see, IS a dimension of size. Opposing sides do not have to be the same length. If this is in an envelope principle referenced drawing, perfect form should apply.

 

[fsincox]

Are you sure you guys are not referencing rule number #1, perfect form a MMC (also refered to as the envelope principle), not #2.