Dimensioning for Interchangeability 1

Would like to start a long overdue discussion of the significance of the ASME Y14.5, paragraph 2.7.1(a) statement: “The surface or surfaces of a feature shall not extend beyond a boundary (envelope) of perfect form at MMC. This boundary is the true geometric form represented by the drawing” (para. 2.7.1.(a)). From my perspective, based upon this statement, designing and dimensioning at MMC should be a design goal. See attachment.

No attachment. You have to copy/paste the attachment link into the message.

I would rather see designers and engineers exercise awareness of the state of their designs. But the pro-competence faction doesn't attract many rabid or even casual followers.

Paul,

Of course adding the missing attachment would possibly help determine what you mean, but I'm not clear on what about the bolded statement you take issue with or want to discuss. Could you clarify a bit?

It also always helps to state the version in question, in your case Y14.5-2009.

I tried the attachment button again. Hope this time it goes through.

Oop. The attachment function doesn't like files with the ampersand or I think other symbols (ie: GD&T is a common error around here), I tried to guess at the file name to try and pull up the link but no luck, I would try to reattach without any symbols.

Also, can you expand on more specifically what you want to discuss about Rule#1, "true geometric form" and/or drawing practices? Your OP is pretty general.

I had hoped that my PDF file would have explained everything. It says that upload was successful.

Replace the offending "&" with "%26" (not the quotes, just the contents) in the download url that shows up when clicking on the link.

Paul Finch,

Interchangeability is the whole point behind GD&T! All this stuff about drafting standards kicked in after World War[ ]II. To give you an excellent example, Rolls Royce made their Merlin engines in factories in Derby (32377), Crewe (26065) and Glasgow (23647). Ford of England made 30428 in Manchester, and Packard in the USA made another 55523. Forget the American fasteners versus British Standard Whitworth. How many of the components were interchangeable?

The ASME Y14.5 standard accomplishes something actually more important than interchangeability. It creates a precise interpretation of all the stuff we apply to drawings. The text you have quoted is Rule[ ]#1. A rectangular feature with plus/minus dimensions is surprisingly ambiguous, until Rule[ ]#1 is applied.

--
JHG

Paul Finch,

I am reading your attachment. I hope it is not a slide show. You are almost certainly violating most of the rules for a good slide presentation.

In your section Throwing Away Good Parts [—] Accepting Bad Parts, you discuss throwing away good parts and accepting bad parts. This has nothing to do with MMC[ ]tolerances, and everything to do with bad drafting. As drafters, we need to do our tolerance stacks, and understand how our parts must work. Too many companies leave drafting to CAD[ ]monkeys. MMC[ ]tolerances will not fix that problem. Your notes mention "at least 50% more functionally good parts". This problem shows a lack of comprehension of geometry by your drafters. All of the tolerancing approaches can be made to work if the drafter is competent.

A conventional claim about GD&T is that positional tolerances provide 50% more allowance than plus/minus. All of this allowance is functional. I looked into this and it is only sort of true.

My notes on Positional Tolerances.

--
JHG

Paul,

Admittedly I haven't had a chance to finish reading your dense presentation yet, but here are a few of my initial thoughts.

1) It seems the concepts of size/MMC size, bilateral/unilateral tolerancing, and the envelope principle/rule#1 are conflated with geometric tolerances applied at MMC and the virtual condition generated from such a tolerance. These are separate, but not mutually exclusive, concepts and being precise about which one is being referred to or utilized is important.

2) I'm not sure I agree that "Product Development has lost sight of [interchangeable parts] as a design objective." Every Engineer and Designer wants parts to fit and assemble reliably and this is usually one of the top considerations, and if you're making more than one part thats design for interchangeability. I'd argue that this is one of the top considerations in creating and maintaining standards like Y14.5. In fact, I'd say the focus on ergonomics, ease of assembly, and throughput has only increased as the years go on - especially as factories turn to automation where high assembly forces don't just result in a complaint from assembly line workers but a rejection by a robot which is programmed to not exceed a certain maximum force, or damage by an indiscriminate robot with installation/applied forces that are too high.

3) The presentation seems to be focuses on MMC as the only way to achieve design goals. There are plenty of situations where RFS might be desirable or even required. Press fits come to mind where RFS actually best represents design intent, and certain controls like profile require RFS. MMC is often the most robust way to ensure assembly/design requirements and interchangeability, but its certainly not the only one. GD&T standards are often compared to toolboxes, they provide the tools to use and aren't necessarily there to tell you which ones to use.

4) You said ISO "doesn't have the tools for dimensioning for interchangeability" because the envelope requirement is not default? I'm no ISO expert, but can certainly be enforced with the Envelope symbol. Additionally the claim in ISO is that default enforcement actually can cause good parts to be rejected which is also true in ASME unless zero (insert geometric tolerance - typically position) @ MMC is utilized. There are also some nuances there due to the difference in the way size is evaluated in ISO vs ASME.

5) There is the claim that "there is no getting around the fact that there can be no tolerances added beyond that [rule#1 envelope of perfect form at MMC] or there becomes a conflict with this rock solid requirement." There are several exceptions to this rule even without the Independency symbol (I) which are right there in 2.7.1 after the portion you quoted - namely straightness, flatness, bars/stock, parts subject to free state variation (or more precisely when the free state modifier is used in Y14.5-2018), and one that it omits but it mentioned elsewhere (but is again mentioned in 2018) as when average diameter is used. I'm not sure how you can reconcile this with your claim.

6) Your definition of the MMC part as the ideal or "strongest" part ignores something as simple as assembly requirements - it would stand to reason that in most cases your "MMC part" would result in the highest installation forces and most difficult assembly (as well as highest imparted stresses due to press fit if that is the design condition). So on each end you have a less desirable condition depending on what you are considering, taking both into account a bias toward nominal could be considered most "desirable".

7) There are several references to the verbiage "true geometric form" contained in the standard. To my knowledge this isn't directly defined other than the context it is used in the quoted section, I haven't given it much thought till now but I would probably consider this in the same vein as True Profile. Not something that suggests "ideal" meaning "best" form, but that defines the "ideal" as in "theoretical" geometry of the feature.

Paul Finch,

Most of my design experience has been machined and sheet metal parts. In CAD, I prefer to model to what I call nominal size.

Eg. I want to slide a [⌀]40mm shaft accurately through a hole. Let's use an RC5[ ]fit as per ANSI B4.1[‑]1967[ ](R1987). This means that the shaft is [⌀]40e7, and the hole is [⌀]40H8. I am working from the 26th edition of Machinery's Handbook.

[pre]
Dimensions: Hole Shaft
Nominal 40 40
Maximum 40.041 39.949 [Ⓜ]
Median 30.0205 39.9365
Minimum 40 [Ⓜ] 39.924
[/pre]

In SolidWorks, if I model at nominal size, I can call up the ISO tolerances in the dimension box. Now, I can change the nominal size, and be confident that my tolerance specifications continue to be correct. I can make sure the final drawing at the shop has the actual inspection numbers. The drawing's primary purpose is to tell everyone what we want from the fabricator. I care about the fabricators and inspectors, and I will make sure my drawings are clear to them. I don't care much about anyone else.

I have since sent parts out for rapid prototyping. Nominal size modelling is a mistake. If I want something rapid prototyped, or other process directly from the 3D[ ]model, median size modelling is the right way. If my 3D[ ]model is at MMC, half of the rapid prototyped variation will be outside MMC, and wrong. Median modelling gives me maximum allowance.

I am sure other people here can add to this.

--
JHG

How would a casting be treated, with tool shops cutting the tool to the 3D model, at this point how does this work? If the tool shop cuts to MMC per the model, that will be bad situation for the tool, especially with die tolerances. Now if the die tolerances are out above MMC from your model, the tool will need to be welded on to get it back to tolerance that is less than your MMC. Interesting presentation.

Fit calculations should be considered pre-product manufacturing data. Those calculations don't work by the way with purchased pins. End product verification is only concerned with MMC of the pin in relation to the datum reference frame of the assembly.

With castings you are normally only concerned with machined surfaces that mate and fit with other parts within an assembly. Some companies do not even dimension cast surfaces and default to the model STP with a general note specifying a loose profile tolerance per ASME Y14.5-2009, para. 8.3.1.1 to what is termed the "true profile" --- an undefined term which is generally taken to mean "nominal"---another undefined term within the standard.

Casting patterns aren't often made to nominals anyway, which is why shrink rulers exist (aside from slipping one to an unwary newbie for hilarious results.)

If they can do that they can look at the rest of the process variation for similar parts and, because they have experience with the amount of shrink and sink, know where to put vents, gates, riser, and otherwise manage the process to make the dies and patterns that turn out compliant parts.

FDM parts should probably use a path along the LMC surface as the squeeze-out will add part volume and, unless that is very well dialed in, will add in. Unless the part will be machined after, and then the MMC boundary with the CNC path on the median surface path. Same with SLS (selective laser sintering.)

SDETERS said:

How would a casting be treated...

Click to expand...

A foundry would be similar to a rapid prototyping shop. A model at median size allows maximum variation of functional parts. On the other hand, a batch of castings is expensive. I would expect my foundry to read my drawings carefully. The 3D Prototyping shop I dealt with did not. Also, I would make a point of talking to the foundry to see how we need to communicate. I would expect all sorts of drafting tips, most or all of which, I would follow.

--
JHG

3DDave said:

FDM parts should probably use a path along the LMC surface as the squeeze-out will add part volume and, unless that is very well dialed in, will add in...

Click to expand...

Are you sure about that? Is there any reason people designing[ ]FDM machines cannot make them account for their nozzle diameter when they construct their model? And of course, is any reason why other people making FDM[ ]machines won't bother to do this? This is why we need to prepare drawings with tolerances.


--
JHG

I haven't read every page and bullet of this. I have read some though so here are my thoughts:

Paul Finch said:

The American standard ASME Y14.5 nowhere uses the terms “ideal” nor “nominal”.

Click to expand...

Have a look at 1.3.56 and 1.6 in the 2009 version.

If ASME Y14.5, paragraph 2.7.2(1) states that the MMC boundary is the “true geometric
form represented by the drawing,” then there is no getting around the fact that there can...

Click to expand...

It doesn't say that.

Therefore, this statement can only mean one thing all tolerances must be applied in
the direction from the boundary at MMC to LMC.

Click to expand...

Why do you think it means that? I certainly don't glean that from that statement that is actually in 2.7.1(a), not 2.7.2(1).

Are you saying that there's a real difference between
.500+/-.005
.495-.505
.505 +.000/-.010
.495 +.010/-.000
?
The last question is regarding page 13. What's the difference between your scenario and specifying a mean dimension and equally disposing the tolerance zone? 1.000 +.000/-.010 is the exact same thing as .995 +/-.005. Is this what your argument is, that all dimensions should be at the MMC limit of size and the tolerance be unilateral?


John Acosta, GDTP Senior Level
Manufacturing Engineering Tech

Paul,

You have posted a very dense (and honestly, potentially conflicted) document with the intent of sparking discussion and when several members myself included provide multiple responses to many aspects of said "presentation" you chose only those tiny portions to respond to? I'm trying to keep an open mind but if my frustration is palpable in my ensuing replies, I apologize.

Coupled with my previous bullet points (1) about the intermixing/conflated terminology and (5) stating rule #1 cannot be broken it is somewhat concerning that you claim "true profile" is an undefined term however its right there in the introduction to profile para 8.2 as "A true profile is a profile defined by basic radii, basic angular dimensions, basic coordinate dimensions, basic size dimensions, undimensioned drawings, formulas, or mathematical data, including design models." Y14.5-2018 goes on to add this directly to the definitions section. Despite this dubious claim about true profile being undefined (probably one of the least ambiguous ideas in Y14.5, at least until you dig into borderline cases and extension of concept) your entire presentation centers around a term mentioned once in the standard without any sort of actual definition for "true geometric form." We can of course deduce meaning from context so I'm not suggesting there is much ambiguity but your insistence on undefined terms is somewhat....ironic.

While we're at it, despite what you stated nominal is actually also defined (albeit not well, but a definition is provided) in Y14.5-2009 para 1.3.56 as "the designation used for purposes of general identification." I wouldn't consider that lack of specific definition as terribly consequential, as nominal is relatively subjective and could refer to whatever the designer deems as appropriate for the "purposes of general identification" including a value not actually contained within the tolerance bounds, common on press fits and threads among others. If one wanted to refer to the middle of the tolerance zone, one might utilize "median" as drawoh pointed out as the mathematically precise term.