INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Remember Me

Are you an
Engineering professional?
Join Eng-Tips Forums!
• Talk With Other Members
• Be Notified Of Responses
• Keyword Search
Favorite Forums
• Automated Signatures
• Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

#### Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Just copy and paste the

# ISO GD&T vs. ASME GD&T8

Share

## ISO GD&T vs. ASME GD&T

(OP)
What do you think about discussing more in details about differences between ISO and ASME GD&T? What are the most important discrepancies between the two in your opinion?

### RE: ISO GD&T vs. ASME GD&T

While others may be able to articulate it more fluently, one trend seems to be that ASME is about defining the functional design requirements and what will be accepted, while ISO seems to lean more toward minimizing rejections/maximizing 'good parts' with less regard to function.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

### RE: ISO GD&T vs. ASME GD&T

(OP)
Kenat,
Here is a content of paragraph 4.1 from ISO 1101:2004 - one of the most important standards from the group of ISO standards:

"Geometrical tolerances shall be specified in accordance with functional requirements. Manufacturing and inspection requirements can also influence geometrical tolerancing. NOTE Indicating geometrical tolerances on a drawing does not necessarily imply the use of any particular method of production, measurement or gauging."

Doesn't this look similar to Y14.5's fundamental rules 1.4(d) & (e)?

Isn't a general purpose of GD&T (regardless whether it is ISO or ASME) to minimize rejections / maximize "good parts"?

### RE: ISO GD&T vs. ASME GD&T

(OP)
'Elsewhere' means where?

### RE: ISO GD&T vs. ASME GD&T

How 'bout the fact that the ASME standard is one volume with a cost of US$170, but for ISO you have to buy scads of separate standards where the total cost gets into several hundred dollars! John-Paul Belanger Certified Sr. GD&T Professional Geometric Learning Systems ### RE: ISO GD&T vs. ASME GD&T Well, you could checkout some of the infamous last paragraphs of ISO2768 (I think part 1 but it may be in part 2 as well, just thinking about that damn standard makes me want to punch whoever wrote it so I'm not going to go look it up). Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you) What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"? ### RE: ISO GD&T vs. ASME GD&T 2 I recently stumbled upon the following quote: "All features on component parts always have a size and a geometrical shape. For the deviation of size and for the deviation of the geometrical characteristic (form, orientation and location) the function of the part requires limitations which, when exceeded, impair this function. The tolerancing on the drawing should be complete to ensure that the elements of size and geometry of all features are controlled, I.e. nothing shall be implied or left to judgment in the workshop or in the inspection department." Could somebody identify if it comes from ISO or ANSI/ASME standard, or somewhere else? ### RE: ISO GD&T vs. ASME GD&T 2 Kenat, Are you refering to ISO2768-Part 1 section 6 (and clause A4) along with ISO2768-Part 2 section 7 (and A4 again) "Workpieces may be whatever shape the manufacturer decides, the designer has no say in the matter unless it's totally fubar" Has to be my favourite part of any standard Apologies if you punch anyone as a result of me looking it up for you. Designer of machine tools - user of modified screws ### RE: ISO GD&T vs. ASME GD&T Checker, as it's on my desk, your quote is also ISO2768, its the introduction to parts 1 and 2. Designer of machine tools - user of modified screws ### RE: ISO GD&T vs. ASME GD&T Finally someone in the possession of actual book! Ninja, could you back me on the fact that 2768 is very limited in scope, as it only applies to dimensions without tolerances usually typical for "non-critical" features? And in fact, it doesn't apply to "invisible dimensions", such as hidden inside of 3D-model? And also it doesn't apply to reference dimensions and basic dimensions? And also it doesn't cover cylindricity, profile of any line, profile of any surface, angularity, coaxiality, positional tolerances and total run-out? And it still your right (and responsibility) as a design engineer to: Explicitly indicate smaller tolerances than 2768 on the drawing when required for proper function?. Explicitly indicate larger tolerances than 2768 on the drawing when permissible for economical manufacturing? Explicitly indicate that your favorite (sorry, favourite) section 6 (and clause A4) do not apply? ### RE: ISO GD&T vs. ASME GD&T Within ISO, Rule #1 does not apply (unless specifically invoked) therefore size does NOT control form of a FOS. In other words, within the ISO system you typically control form separately from size. ISO 2768 deals with the size of a feature, and by extension of the preceding, not its form. I've heard arguments to the contrary, but nobody's backed it up from the ISO 2768 standard. Now, to be specific, the general tolerance classes in 2768 apply to non-toleranced dimensions which are NOT reference and which are NOT basic. Reference dimensions don't have any meaning as far as part definition is concerned. Features established with Basic dimensions typically are controlled with feature control frames. A notable exception for basic dimensions occurs when they are used to locate and/or size a datum area target in which case a basic dimension has gage-maker tolerances applied. Another difference between ISO and ASME is that ASME tolerances are nested, or inclusive. As you work down a stack of controls on a feature, each subsequent control must be a refinement of the preceding control (i.e. a smaller tolerance zone). With ISO, each control is considered separately and therefore you could for example have a parallelism of 0.1 with a flatness of 0.5. In other words, in ISO the tolerances are cumulative. As an extension, within ASME the surface finish/roughness is considered a refinement of the surface form; within ISO, the surface roughness is cumulative, so it can actually exceed the flatness. Overall, ISO seems to be moving to a metrology-based standard. The definitions of the various controls indicate means of checking the control rather than focusing on the functionality of the control. ASME has always been functionality based and with 2009 moved even further from including any instructions on verification. The differences between the standards is a big topic. Jim Sykes, P.Eng, GDTP-S Profile Services www.profileservices.ca TecEase, Inc. www.tec-ease.com ### RE: ISO GD&T vs. ASME GD&T JIm, I've seen that mentioned before (about ISO thinking of tolerances separately, rather than refinements). But I'm having trouble picturing your example: if I verify a surface parallelism of 0.1, how the heck could it's flatness error be more than 0.1? The logic just doesn't connect. (Unless ISO's parallelism is something like tangent plane or each element.) Also, I don't think ASME sees surface roughness as a refinement of form. You could have a crowned surface that fails flatness, yet its surface roughness could be as smooth as glass. John-Paul Belanger Certified Sr. GD&T Professional Geometric Learning Systems ### RE: ISO GD&T vs. ASME GD&T (OP) Jim, It is interesting what you are saying about relationship between values for parallelism vs. flatness tolerance (0.1 vs. 0.5). I know you used this as an example only, however I am really tempted to not agree with you. Paragraph 5.2.2 of ISO 2768-2:1989 "General Tolerances for Parallelism" states that: "The general tolerance on parallelism is equal to the numerical value of the size tolerance or the flatness/straightness tolerance, whichever is the greater." Doesn't this mean that parallelism value must be at least equal to flatness value? ### RE: ISO GD&T vs. ASME GD&T (OP) J-P, #### Quote: Also, I don't think ASME sees surface roughness as a refinement of form. You could have a crowned surface that fails flatness, yet its surface roughness could be as smooth as glass. This is because actual surface roughness is a refinement of actual flatness error. But the opposite situation can't happen, and this is, I believe, what Jim meant. ### RE: ISO GD&T vs. ASME GD&T No, the opposite situation is what I meant. In fact, both cases are possible: A surface can pass surface finish and fail flatness. Also, a surface can fail surface finish and yet pass flatness. I guess the confusion is because the parameters for surface finish are localized (the cutoff width), but flatness spans the entire surface all at once. So in this regard, both ASME and ISO see flatness and surface finish as separate requirements, which was my intent in replying to Jim. John-Paul Belanger Certified Sr. GD&T Professional Geometric Learning Systems ### RE: ISO GD&T vs. ASME GD&T Jim, Allow me to disagree. "Within ISO, Rule #1 does not apply (unless specifically invoked)" All you need to invoke Rule 1 in 2768 is to add (E) symbol to the call-out, just once on the entire drawing sheet. ISO is well aware of Envelope principle and puts it to good use. "ISO 2768 deals with the size of a feature, not its form. I've heard arguments to the contrary, but nobody's backed it up from the ISO 2768 standard" ISO 2768 covers Flatness, Straightness add Circularity which ARE form controls. Nobody will "back" it for you, open the book and see for yourself. "With ISO, each control is considered separately and therefore you could for example have a parallelism of 0.1 with a flatness of 0.5" Entirely not true. In ISO location and orientation tolerances also control form characteristics. In your case flatness may be indirectly controlled by the Envelope requirement, Perpendicularity, Parallelism, Angularity, surface Profile, Position, Total run-out, and general tolerances, like ISO 2768. "As an extension, within ASME the surface finish/roughness is considered a refinement of the surface form; within ISO, the surface roughness is cumulative, so it can actually exceed the flatness" Wrong again, flatness specification could limit surface waviness or roughness, it's just no one cares because form tolerances are much larger that surface texture specs. ### RE: ISO GD&T vs. ASME GD&T I should refresh the page before posting ### RE: ISO GD&T vs. ASME GD&T ISO2769 should only be used to save the designer the hassle of tolerancing every feature on the drawing. That is its only purpose. It's a more useful version of "all dimensions +/- 0,25mm" no more Doesnt mention dimensions in a 3d model (the standard is from 1987, its likely this concept didnt exist at the time). Doesnt apply to reference (auxiliary in the standard) or basic dims. Doesnt cover cylindricity but implies cylinders are controlled by circularity and paralelism, which the standard does cover. Profile of a line and surface are covered lightly by straightness, flatness and paralelism. Angularity no but it covers tolerances on angular dims. Coaxiality is not covered but coaxiality may be limited by circular runout which is covered. Positional tolerance and total runout are not included. The last three are correct, what use is a designer who doesnt control tolerances which improve the design. The last bit of the standard is right when interprited correctly and common sense applied, it needs re-phrasing badly. Designer of machine tools - user of modified screws ### RE: ISO GD&T vs. ASME GD&T I possess the 2768 standard thanks CheckerHater, both parts 1 & 2 and spent plenty of time looking at them in the past, just not going to bother now. Next you'll be saying the bit ninja paraphrases is only in there to allow deviations/waivers etc. Plus 2768 gets misused the same way block tols and the like do - though arguably that's not the fault of the standard itself. Almost nothing is being said above that hasn't been said before in earlier threads on the topic. Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you) What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"? ### RE: ISO GD&T vs. ASME GD&T The current revision of the ISO surface finish standard is totally FUBAR. I don't have it in front of me so I may not have this exactly right, but it says something like "only 86% of the surface has to meet the requirement"! That is so stupid. If I'm trying to specify a surface for an o-ring to seal on and only 86% of the surface meats the requirement it is going to leak like a sieve. 100% of the surface has to meet the requirement. The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows. ### RE: ISO GD&T vs. ASME GD&T So, JP, are you saying that you can have a surface roughness callout (i.e. tolerance) that is greater than the flatness tolerance on the surface? In otherwords, 0.1mm on flatness and 0.5mm on roughness? I don't think so. I understand that the two controls are generally orders of magnitude different, but the extreme is possible in some cases (cast surface for example). I'm not saying that it can't pass roughness and fail flatness; it's not uncommon for a lower-order control to pass when a higher-order control fails. Specifically what I mean is that the control tolerance must be a refinement of any higher-order control tolerance. PMarc, the citation from 2768 is a good example of ISO double-speak. ISO (1101?) indicates that size and form must be controlled separately (as a default method), yet here they are implying that size also controls orientation? Orientation wrt what? ISO 2768's not valid for orientation control because it doesn't require the definition of a datum reference frame. I have seen people work around this by putting a generic note such as "GENERAL TOLERANCES WRT DRF /A/B/C" In 2768, does ISO treat parallelism as a localized thickness control? I've never been able to have an ISO-trained person answer that question and support a datum reference requirement per elsewhere in ISO GD&T standards. I retract my earlier statement about ISO controls being cumulative. Per ISO 1101:2004(E), Section 17 Interrelationship of geometric tolerances; "For functional reasons, one or more characteristics can be toleranced to define the geometrical deviations of a feature. Certain types of tolerances, which limit the geometrical deviations of a feature, can also limit other types of deviations for the same feature. ... Orientation tolerances of a feature control orientation and form deviations of this feature and not vice-versa. Form tolerances of a feature control only form deviations of this feature." Looking at the '83 version, this was covered in less detail in 13.2. Interestingly in '83, figures 36, 37, 44 & 45 show parallelism to a surface without a datum reference, but rather with a datum triangle anchored to the "reference' surface. Jim Sykes, P.Eng, GDTP-S Profile Services www.profileservices.ca TecEase, Inc. www.tec-ease.com ### RE: ISO GD&T vs. ASME GD&T Fully agree that engineers/designers/draftspeoples shouldn't abdicate their responsibility for clear documentation by invoking ISO 2768 on the drawing. It increases the risk of improper interpretation when the machinist, inspector read the drawing. Jim Sykes, P.Eng, GDTP-S Profile Services www.profileservices.ca TecEase, Inc. www.tec-ease.com ### RE: ISO GD&T vs. ASME GD&T Gotcha, Jim. I might say that it's pretty much a moot point to even compare surface finish and flatness, because their intents are totally different (thus the order-of-magnitude difference). But I now agree that if someone were to create a roughness callout of 0.5 microns (with the cutoff width being the same as the full length of the surface) and a flatness tolerance of 0.0000006 mm, then we have a problem (both in terms of mathematics and practicality). John-Paul Belanger Certified Sr. GD&T Professional Geometric Learning Systems ### RE: ISO GD&T vs. ASME GD&T 2 I agree the no-rule #1 is a bigger difference than people realize at a casual glance. Remember, you can still invoke it, though. As most here know I am not a big believer in the problems created by the definition and the associated restrictions created to define a "FOS". The ASME standard seems to be backing farther and farther away from the certainty it seemed to provide in 1982. I believe this is good as it was a myth anyway. Many tolerances no longer cover a FOS anyway but an AME, and we talk about them defining by abstract concepts. We do not use a lot of gauges here at my company all CMMs. As far as ISO 2768-1's paragraph I believe that is a bunch of fuss about nothing, we accept parts out of spec every day, all this says is we can and will if it occurs on features covered ONLY by the general tolerances, it does not use "fubar" that is an incorrect quote added to put something in a bad light. I really wish some of these ISO people would come on here and defend it themselves I supose we would need to be able to read German. As far as the thickness of the ASME book well I have seen discussions here wanting to through out examples that have been in the book since 1973. After everyone here throws out the parts they don't like, the ASME standard might not be as thick and may even look like the ISO standard just showing general concepts and letting it go at that. Frank ### RE: ISO GD&T vs. ASME GD&T Sorry Jim, "ISO 2768's not valid for orientation control because it doesn't require the definition of a datum reference frame" Wrong once again. Parallelism requires one and only one datum – have you ever heard of being "parallel to A, B, and C"? And for this datum 2768 picks the largest of two features – smart and simple. So, yes indeed, THERE IS datum reference frame – just enough of it. Note that 2768 is carefully avoiding controls that require more than 1 datum – position, profile, etc. One should agree that 2768 is too smart for what essentially is glorified tolerance sticker. And "double-speak" is a harsh word. One day your company may have more ISO clients than ANSI/ASME clients. Just a thought. ### RE: ISO GD&T vs. ASME GD&T Jim, As I recall it does attempt to define how to apply the form type tolerances. if it is not perfect well niether is ASME I reference the disagreements here on Fig 6-18 or 6-52 and as far the comments on taloring a tolerance to an inspection method, who can look at runout, Yes I know it doesnot have to be checked that way. Checker Hater, I like you more and more. I have a feeling we have had a similar experience somewhere, First, I want to say, I learned a lot from checkers and consider some were my friends. However, when I was trying to convert our system to GD&T (1982 standard) they were the ones most against change, as they liked the old way, it made them powerful. "my" GD&T threatened all that. The entrenched buracracy won that battle, company went out of buisness soon after I left. Frank ### RE: ISO GD&T vs. ASME GD&T Sorry, I may have technically misspoke, they filed for bankruptcy, closed and are now reopened as a division of a Chinese Company (new owners). I believe that is more correct. Frank ### RE: ISO GD&T vs. ASME GD&T Interesting points on 2768. Quite true about parallelism also, but what of perpendicularity? 2768 covers it wrt one surface only. That's adequate for most uses. There is no datum reference frame, but there is a reference surface invoked by the leaders of the callout in those cases. And angularity? So 2768 covers the comparatively easy items. I don't have an issue, in reality, with 2768; I've used it as a design tool many times and it is excellent for general purpose design. Overall, what I've seen is a cleaning-up of many of the outstanding issues in ISO's GD&T standards collection. That's a sentiment shared by many in the ISO user community as well. And, I've used stronger language in comments about ASME's GD&T standards. Jim Sykes, P.Eng, GDTP-S Profile Services www.profileservices.ca TecEase, Inc. www.tec-ease.com ### RE: ISO GD&T vs. ASME GD&T Maybe, ASME put's the drawing originator in the driving seat. If a vendor or whoever wants me to accept a part that doesn't explicitly meet drawing then I get to decide if I want to spend the time and effort ($) looking into the defects and how they affect function (above and beyond that already defined on the drawing) and if they can be recovered...  They can't force me to do so.

However, the ISO 2768 way, the drawing originator has to justify why it can't be recovered.  I have to justify why I won't accept parts that don't meet my stated requirements.  Whether I want to or not I have to spend the time to justify not taking them.  Am I meant to have some other document besides the drawing that captures this?  In the end who decides if my justification is adequate?

The ISO 2768 sure makes it easier to ask forgiveness than ask permission - forgiveness is the default state and not forgiving has to be justified.  Though I suppose in a way that almost makes it Christ like.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

### RE: ISO GD&T vs. ASME GD&T

My suspicion is that what Kenat brought up from 2768 was developed as a catch-all for a poorly-documented design.  I.e. If it works, use it unless you have a really good reason not to.  ASME does tend to favor the designer over the manufacturer in this way.
On the plus side for ISO, I think that they're way ahead of some of the metrology and math-definition aspects compared with ASME.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

Ken,
Sorry,

"Workpieces may be whatever shape the manufacturer decides, the designer has no say in the matter unless it's totally fubar"

I believe you, and maybe some others around, may feel that this statement captures, in your opinion, the essince of the referenced statement, but, it is NOT a "TECHNICALLY" corect ISO statement. Any representation as such is incorrect. I would expect more persnicityness (is that the word I want?) from a real technical discussion, particularly from a checker (sorry, I had to say it).

I feel it my duty to any of the "uninformed" here to call it out as such. Understand, I believe the ISO standard is not perfect either, but I will say the more I learn the more I like it.
Frank

### RE: ISO GD&T vs. ASME GD&T

The ISO standard is not stopping you from specifying any tolerance you wish and if you have a valid reason for the tolerance it supports that it is still not an acceptable part, is that really too much to ask. The truth be told we should have a reason for a tolerance or it just should not be, it is the way it is, folks, isn't that our job?
The ISO standard just recognizes that too many GENERAL tolerances are not based on practical absolute requirements. The basic supposition that they spell out is that it is not practical to control every dimension to the absolute extremes when process will GENERALLY hold them much tighter, did you read that part too?  If you make millions of the same thing it may be worth the time to check, but in many cases it is not justified. Why don't your inspectors check EVERY point of EVERY feature? I suppose there are some that actually think they do?
So if I am not going to check every single dimension to it's absolute extremes, it is only a rational buisness decision to say don't throw the part away unless it will not work. I believe this is a rational position to take give the premise they have laid out
There are some here that will say "they" have checked all of theirs, well good for you, yours are fine then. I am here to tell you most do not. I have been around too long and worked at too many places to believe it. I have even seen some admit it here.
As we have stated here, before, in this area the ISO is covering areas not covered by ASME and when they have attempted they just basically adopted the ISO's work (ref: ANSI B4.3).
Frank

### RE: ISO GD&T vs. ASME GD&T

I am guessing, but 2768 is likely based on an old DIN standard; the Germans did amazing work documenting "norms" for manufacturing processes.  Other ISO-contributory countries would have verified the applicability of the general tolerances.  From my understanding, the information is based on typical machine shop capabilities at the time of publication; 1989 being the release date of the copy I have, which supersedes the '73 release.  Given the different tolerance classes, the selection thereof by the designer SHOULD be based on their own shop's or suppliers' capabilities.  The problem is, I haven't seen too many companies that have the slightest idea of what those actual capabilities are (Europe, N.America, Japanese), and most of the 2768 users (designers/engineers) that I've encountered just select a tolerance class based on "desired" outcomes and go from there.  In addition to that, even fewer shops understand the 2768 process (at least in N.America) and just "do their best".  To me, that makes 2768 an inappropriate choice for those users.  I have seen it used correctly, though surprisingly it was in N.America rather than in Europe.  Note that this is not a criticism if the standard, it's a commentary on the state of engineering in business today.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

(OP)
As the initiator of the thread, I'd like to say that although I was rather thinking the discussion will focus more on differences between ISO and ASME GD&T, I'm really glad it went into ISO 2768 direction - after all "general tolerances" concept is nicely showing how ASME's and ISO's approaches to dimensioning and tolerancing differ in general.

I believe the approach difference is a key to everything here. And I wouldn't even try to judge which one is correct and which is not. In fact, in my opinion, there are strong and weak points in each of them. And what we shouldn't do for sure is to arbitrarily assume that ISO standards (in this case 2768) are bunch of useless junk without any logic behind - they have been created by people with tremendous amount of experience and practical knowledge.

Here are some of my other thoughts:
I still do believe that ISO standards in general are oriented for 'functional design' even if some paragraphs may sound otherwise. The point is that ISO additionally pays a lot of attention to how the part is manufactured and even more to how it should be inspected. But is it wrong? I wouldn't say so. For me the functionality is not only a question whether something will assemble with something else. It is a matter of manufacturing abilities and economy too. One can have perfectly 'functional' assembly but the effort put on manufacturing and on the inspection will generate such a high price that at the end nobody will think of this product well. As usual, the compromise has to be found, and this is one of the purposes of 2768 standard - it is trying to tell that with this kind of tolerances a design can be economically optimized, adjusted to manufacturing and inspection abilities of a workshop.

But unfortunately this is a noble theory, nicely described in the annex A of both parts of 2768. The reality shows that 'general tolerances' concept is so general and broad that it had to be boiled down to some relatively simple cases and even with that it gets quite unclear. Example: take the general symmetry tolerance for instance - ISO 2768-2 is saying that: " The longer of the two features shall be taken as the datum; if the features are of equal nominal length, either may be taken as the datum."  That is clear, but what if there were 3 features of different length shown nominally symmetrical? Which one should be chosen as the datum? Figure (b) in annex B5 is showing such a situation but not explaining how the third feature should be controlled. Should the two shorter features be controlled wrt the longest one or should there be two different datums for two positional callouts?

This was an example only - all I am just trying to say is that the standard is not perfect and leaves plenty room for assumption, but that is life. For some of us it can be useful, for some can't. I saw drawings of really complex parts with almost no geometrical tolerances shown but stating that general tolerances are according to ISO 2768. You would not even imagine how much time a product engineer spent on explaining to inspector which geometrical characteristics should be measured relative to which features. They finally found an agreement but only because they were working in the same plant and were speaking the same language, so they sat together with their bosses and clarified all the issues. Can you imagine what would happen if one was speaking American English, the second one Chinese English and they were located thousands miles apart?

And just for the end, despite of all shortcomings of ISO standards (not only 2768), I agree that they have one big advantage over Y14.5 and associated documents - they are way ahead in mathematical definition of inspection routines for geometrical tolerances. I fully respect and admire Y14.5 for its versatility in describing so different dimensioning and tolerancing schemes within one document, but the fact that those concepts are not fully supported by mathematical definitions is one of its biggest weaknesses.

### RE: ISO GD&T vs. ASME GD&T

Pmarc, check out Y14.5.1 for mathematical definitions of Y14.5.  I believe that the sub-committee is working on the next revision now.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

(OP)
Jim, I am well aware of Y14.5.1, but in my opinion 1994 revision is not doing a proper job. Very small percentage of concepts presented in Y14.5 is thoroughly covered by Y14.5.1. I hope the newest edition will be much more specific.

### RE: ISO GD&T vs. ASME GD&T

Guys,

This thread was created to COMPARE ISO with ANSI/ASME.
Did anyone notice that there is no general tolerance ASME standard AT ALL?
So, there in nothing to compare. There is a "bad" standard vs. no standard.

"The outcome being that the drawing no longer defines what is an acceptable part"
No, drawings don't define it, engineers do. If due to laziness or lack of professionalism someone forgets to attach tolerance and/or geometry requirement to critical feature, 2768 will come back and bite him in the leg. I have no problem with that.

Sorry for all the bitterness, it's a bad case of Mondays.

And on the lighter note:

### RE: ISO GD&T vs. ASME GD&T

(OP)
Why would somebody like to invoke ISO or any other "foreign" GD&T standards on ASME prints? I do not see a reason. If you are thinking specifically about invoking independency rule into ASME drawings, I do not think there is something incorrect in placing a general note like: "UNLESS OTHERWISE SPECIFIED PERFECT FORM AT MMC NOT REQUIRED". This would be a switch between default tolerancing principles, wouldn't it?

### RE: ISO GD&T vs. ASME GD&T

Or of course, use the new "I" modifier.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

### RE: ISO GD&T vs. ASME GD&T

So, first off fsincox, as I've already said I have a copy of 2768 and back when I had my first run in with it spent a bunch of time studying it thank you very much.  As an idea of a standard to suggest what are realistic manufacturing tolerances or similar it arguably has some merit.  However, as a complete and comprehensive solution to the never ending problem of most designer not being willing/able to spend enough time & effort to properly tolerance drawings/do so most efficiently I'd say it's a miss.

Say whatever you want about checkers, our place 'saw the light' a couple of years ago and I no longer get that miserable task, except when someones drawings are so bad that even management can't divert the blame.  Now I even get to do some project management so I could play the other side of the fence if I really wanted.

I believe there was an ASME equivalent to 2768, which was indeed a din originally.  I think it's been brought up before, or maybe I'm imagining it.

I've already said that using 2768 incorrectly is comparable to using the typical inch block tols incorrectly.  Though, one might incorrectly think they were doing a better job simply by referencing a 'standard' than relying on some fairly arbitrary numbers on a drawing template or similar.

The first few years of my career were in the UK to iso standards, so any implications of nationalism are questionable.

Finally, the implications that using 2768 is analogous to the whole 'critical dimension' debacle is scary stuff - enough to make me like it even less.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

### RE: ISO GD&T vs. ASME GD&T

Ken, Frank,

"complete and comprehensive solution to the never ending problem of most designer not being willing/able to spend enough time & effort to properly tolerance drawings" is to fire the bastards and replace them with knowledgeable skilled professionals.

Bad drawings cannot be improved by magically applying some "fairy dust" to them, be it genius-written Standard to invoke, or Tolerance sticker made by Elves.

At the end of the day everything is made by imperfect people. And guess what? I spent number of years in a machine shop. We were producing new part every day (or night), so I had literally hundreds of prints going thru my hands. In all those years one single drawing made by some government sub-sub-contractor would qualify as "standard-compliant". The rest was Creative drafting, or complete fubar which is fashionable word on the forum today. There was never one unsatisfied customer. Period.

The truth is: One can make a living by producing good parts from the bad prints, and at the end of the day its all that counts.
Don't try to save the world by application of general tolerances.

I am old and I am tired. Next time let me offer Ken my help - I will be holding people that he will be punching.

### RE: ISO GD&T vs. ASME GD&T

Ken,
You should know the above statement is not correct as written in the ISO standard. It is an exaggeration for dynamic effect.
You are quite correct: ANSI B4.3 General Tolerances for Metric Dimensioned Produts.
The German reference was not in reference to you and your heritage, but from the fact that, we both know, this standard is basically derived from the DIN (German standards) version.

Jim,
The problems you see in the general application of the ISO standard are in my opinion related to the same problems I see with the ASME standard. While ASME does not cover general tolerances like ISO in the same way, they do try to cover the meaning of how to interpret implied general tolerances. We seem to see a progression of statements in the standard over the years to less certainty of intent of the old implied tolerance dimensions. They basically are recommending using the "new GD&T" system for better coverage in stronger and stronger language but refusing to pull out the rug completely. So I think the real problem is they are retroactively trying to give a clear definition to what is an already an acknowledged imperfect system.
Frank

### RE: ISO GD&T vs. ASME GD&T

Interesting, Frank.  There are many conversations about withdrawing some older standards, or significantly overhauling them to remove some historically less-useful bits.  There tends to be an erring on the side of caution by generally diluting things and redirecting.  C'est la vie.  There is gross imperfection in both systems and it really comes down to which one you were initially trained in for most people.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

Jim,
I agree, again we are really working in an imperfect world. I am not suprised at all about the caution, either. I believe it would only cause more resistance to adopting the standards than there already is currently. We still live in 1982.
Frank

### RE: ISO GD&T vs. ASME GD&T

I'm in the next generation, Frank.  '94.  So, will it be the kids in diapers today that will be the '09 generation?

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

No Jim,

It will be fools like me who think latest and greatest stuff will get them somewhere.

### RE: ISO GD&T vs. ASME GD&T

CH,
I am all for keeping up, myself, I have been pushing for it. In my years of experiance change does not come easy to bureaucracies. I would venture to say it even scares them.
Are you the boss?
Frank

### RE: ISO GD&T vs. ASME GD&T

I am the guy lucky enough to have the boss who is listening.

Given current state of economy no-one will retire at 65, so there is metric ton of time ahead.

### RE: ISO GD&T vs. ASME GD&T

So I've been thinking about this issue a bit, especially as regards a drawing defining an acceptable part (based on function) per ASME, and Iso 2768 para 6/7 about function not the drawing defining it.

Maybe part of my concern is that much of early GD&T as I understand it came out of the need/desire to ensure interchangeability, any part 'A' would assemble to any part 'B' and this is still a major factor to me today.  This is still what ASME with it's emphasis on worst case & drawing defining an acceptable part seems to lean towards.

The thing with not relying on the functional needs as summarized in an ASME drawing is what happens if it's a spare part for instance.  If function is defined as being able to be assembled, well because you aren't assembling it straight away how can you tell if it's a good part?

If function is based on some strength requirement, then you potentially end up having to run some calculations, doing FEA, or maybe even proof tests...  Now I'm sure many of us have been involved with approving deviations/waivers/concessions etc. which required some of the above, however the iso 2768 para 6/7 forces you to do it as I see it.

Of course, then there's the statistcal tolerancing approach which is already a deviation from true interchangeability but widely practiced and accepted.

Just some incoherent musings, sorry.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

### RE: ISO GD&T vs. ASME GD&T

The simultaneous requirement is not treated the same, either.
Frank

### RE: ISO GD&T vs. ASME GD&T

Kenat, you just have to let it go.
All the parts have Fit, Form and Function requirements, but every feature is "biased" towards one of them.
If you are in America you probably have a car. Think of the wheel.
The interchangeability is achieved thru fit and form requirement.
Wheel has mounting holes that have to "fit" over the studs (by diameter), there is a position requirement for wheel to fit on certain model hub. The cone countersinks on the holes probably controlled by really crazy GD&T (everybody hates cones, right?)
And then there are vent holes with the sole "function" to let the air to the brake rotors. There is no fitting part.
The dreadful clause only applies to vent holes. In fact, there are many wheels that look different, but are actually interchangeable.
Disclaimer: not a wheel designer. Things are probably more complicated (balance, etc.) Just trying to make a distinction between things that have and don't have to physically "fit", but both have a "function".

### RE: ISO GD&T vs. ASME GD&T

#### Quote (Kenat):

...and Iso 2768 para 6/7 about function not the drawing defining it

I believe that is incorrect.  The drawing per 1011, 5459, & 8015 defines an acceptable part; not the "tolerance unless otherwise specified."  I think you are taking that part of 2768 way out of context.

Joe
Dell T3500 Xeon W3505 2.4Ghz
6.0GB  Win7 Pro x64
ATI FirePro V5800

### RE: ISO GD&T vs. ASME GD&T

#### Quote (CheckerHater):

ISO 1101 declares Independence principle by default
CheckerHater,
a bit incorrect, it is ISO 8015

### RE: ISO GD&T vs. ASME GD&T

CH,
Not everygody hates cones ... they are actually a specialty of mine due to my mold-design origins.  I actually had one instructor tell me that it was impossible to use cones as datum features and that we would have to redesign our molds to use flats & cylinders ... don't think so.  Cones can be a challenge for those that don't know/like/understand profile of a surface, but they're easy once you go that way.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

AK,

Jim,

There are heated discussions happening about what cones are good for.
Will be glad to see more of you on this forum

### RE: ISO GD&T vs. ASME GD&T

CH, let me know when & where if I miss the posts.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

### RE: ISO GD&T vs. ASME GD&T

OK, where does it say that clause only applies to vent holes?  (Plus vent holes are an over used example for features that don't matter in my opinion - my vent holes always seem to be close enough to each other or to other features that their size & location matters more than one might initially expect)

Iso 2768-1 6. Unless otherwise stated, workpieces exceeding the general tolerance shall not lead to automatic rejection provided that the ability of the workpiece to function is not impaired (see clause A.4).

Iso 2768-1 A.4  The tolerance the function allows is often greater than the general tolerance.  The function of the part is, therefore, not always impaired when the general tolerance is (occasionally) exceeded at any feature of the workpiece.  Exceeding the general tolerance should lead to a rejection of the workpiece only if the function is impaired.

I get the idea that the general idea is that the 'general tols' are meant to be so 'loose' that they should easily be met.  However, I don't fully buy into what it says in A.3 about reducing the need to do detailed tolerance calculations.  I don't see how it helps guarantee parts will fit or similar which is when you do detailed tol calcs typically.

Perhaps, if you're using the spec properly, any directly functional dimensions are actually fully specified on the drawings, while only those that are effectively in 'free space' or similar fall under the 2768.

However, I've never really seen it used this way - though as I've conceded before, in this extent it's comparable to block tols being misused.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

### RE: ISO GD&T vs. ASME GD&T

OK, where does it say that "any part 'A' would assemble to any part 'B'" based on general tolerances all alone?

Close Box

# Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

• Talk To Other Members
• Notification Of Responses To Questions
• Favorite Forums One Click Access
• Keyword Search Of All Posts, And More...

Register now while it's still free!