GD&T is it a philosophy 5

[fsincox]

I am interested in hearing the different points of view on your philosophy to GD&T.
As new draftsman we had always been told “you can’t use bolt circles, only co-ordinates” and “don’t dimension from centerlines, only edges” I suspect these are a lot like the caliper guys of today. When I was first trained in Y14.5-1982 in 1987 I found it a very liberating. The philosophy I was told was if it did not violate the basic rules or is not prohibited by the standard it was OK, Notes on drawings were not desired because of language barriers, but in extreme cases, you may need to supplement with a note to explain what you intend. The sense I got was it was a tool kit to be used and the simplistic examples in the text were just that, period. The book certainly did not explore the limits of what can be done it was more of a universal language that would be built upon as languages do. English, for example, has had words like computer and geometric dimensioning and tolerancing added to it (my MS word still thinks tolerancing is not a word or is misspelled). We all know it is a word.
In my first job AGDT (After GD&T Training) I worked with a lot of machines and a lot of dowels patterns that people always wanted located to unimportant edges (“the from the edge guys”, always 2 dowels in case some don’t know), I said: “fine, we have this new tool called composite position tolerancing that was perfect for that”. Eventually, the question was asked: “now, can we put an orientation on the centerline between the dowels to refine for orientation”. “Not in the ANSI world”, I said, “this is explicitly prohibited”, if we were ISO well life would have been easy. I was told the committee was working on just that issue, and, the restatement of secondary datums in a composite position tolerance would do just that. We were also instructed that since the standard did not actually show it we may want to add a flagnote to explain what we meant. This practice is part of the standard now and since Y14.5-1994 an accepted practice, some apparently argued it was implied before in the 82, but, it was not explicitly shown.
Out here in the real world we do not always have time to wait for the politicians to make decisions, the job has a deadline and we need tools to do the job. MMC and LMC (also a new concept at the time) are good valid tools, adding it to profile tolerances to get the job done foe the heavy hitters is great, but why take it away from the poor little radius, Is it really because it is hard to measure? Life isn’t always easy.
There’s lots I want to get into with guys who are interested in exploring ideas.
Like:
To circle “E” or to circle “I”, that is the question?
Why not true position of a surface instead of profile?
Why perpendicular and parallel, not just orientation?
Is a feature defined by a radius really different than the same one defined as diameter?
Doesn’t anyone out there use the dreaded ISO and like it?
How can rule #1 not be a violation of all the logic all we are trained in as engineers and assume the worst case, as ISO does, by the way. Must we cling to our calipers in one hand and our concept that we will someday actually produced that perfect feature at MMC in the other? (When I am asked by the shop to accept an oversize shaft is it more perfect, then?)
Anyway thanks, if you bothered to read this far, I guess I will get off my soapbox for now to give someone else a chance.

 

[ewh]

The standard "allows" for a +/- linear dimension, but it would be bad practice.

Please, please, please show me where it is stated that ± dimensioning is bad practice. Personal opinion is not quite as valid a documented standard. ;-)

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

 

[NormCrawford]

Dave,

I have yet to ever find a person in a fundamentals class that can explain a so called "simple" +/- linear dimension intended to locate one feature to another, particulary a surface to another surface. And I teach a lot of classes.

To completely answer you on this forum can be a bit much and so you are welcome to track my information down and call or e-mail me. (see our website for that info)

But the short of it is that very few people understand where and how big the tolerance zoneS are when a +/- linear dimension is used and therefore misunderstand the inherent form control and often invoke rule #1 where rule #1 is not functional in the design of a particular feature.

The fundamental reason that profile more explicitly defines the functional need and inspection process is that it truly establishes the functional relationship to other features as functional datum features. A +/- linear dimension has nothing to do with a datum feature and therefore nothing to do with a functional datum reference frame.

The composite profile control that you seem to be referring to is an excellent method of control but again way too much to discuss here. Perhaps a new thread will be more appropriate and/or track my info down and contact me.
(I'd provide it here but I think it is against the rules.)

As my own humble personal opinion, a +/- dimension should only be used for a feature of size. That's it! When someone sometimes responds to me; "But what if the feature(s) is/are not important?", I usually respond with; "Then what is it doing there?"

Norm Crawford
GDTP-S
Applied Geometrics, Inc.

http://www.GDandT.com

 

[dingy2]

Norm:

I come from the Quality field and at one time in my life, I measured automotive parts using CMM equipment. We had to develop the datum sructure in the same manner that Designers today reflect them on the drawing. All dimensions were +/- and the practical use of GD&T certainly would have been of value rather than having all those notes for flatness, straightness, concentricity, etc. on the drawing.

In Quality, Process and Manufacturing management today, there are pre-production meetings where we decide what features are important to its function and relationship so that we might address them from a process and quality perspective. Should we control and confirm surfaces on an regular basis that have no meaning to the part's function? No! Should be make checking fixtures for holes that are only to lighten the product? NO!

The practical use of GD&T should reflect the functional needs of the features on a part as per the 2009 edition and, thus, all the personnel involved in the producing of the part would be on the same page. The 2009 standard does not state that only +/- dimensions must be on features of size only. It does not state that profile of a surface is mandatory on all surfaces.

It doesn't take much thought to figure out the datum structure when some dimensions come from the datum as a basic dimension while another dimension is reflected in a +/-.

I remember one automotive supplier where I was training. They had a drawing where their customer told them that they must have a default profile of a surface of 0.5 mm in notes for all surfaces. I noticed on the drawing a profile of a surface of 0.5 on a particular surface was noted in a FCF. Why I asked since it was also a default tolerance? They said that the particular surface had a function requirement and the default profiles had no functional importance. Is this the intent of the standard??

Maybe a good blend of +/- with GD&T as applicable could best reflect the function needs of the part.








Dave D.

http://www.qmsi.ca

 

[axym]

Since Norm has already stirred the pot, I'll stir it some more. Dave, do you think it would be a good practice to put a plus/minus dimension on the height of the part in Fig. 6-4? It's really no different than putting one on the width. In each case, there is partial opposition and one surface extends past the other.

I agree with Norm that putting a directly toleranced dimension on the width would be a bad practice. To state the obvious, the merit of a design practice shouldn't be based purely on its legality. Of course the standard doesn't make statements about what constitutes a good or bad practice. The standard is a dimensioning and tolerancing tool kit, not an engineering design manual.

A designer could change datum feature A in Fig. 6-4 to that narrow flat on the top of the left leg of the part. The standard doesn't say they can't. Would that feature provide a good stable datum plane for the orientation tolerance? Probably not, and the argument could be made that it's a bad practice. Should the standard somehow forbid the practice then? Should the standard impose rules for a minimum aspect ratio for datum feature extent to tolerance zone extent?

The standard gives designers more than enough rope to hang themselves, and specify bad practices that are perfectly legal.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[Belanger]

My two cents...

Plus/minus should not be used for location or orientation. It's only really good for size, chamfer, and radius. That is, for features of size, and also for chamfers and radii, which aren't features of size

Norm, I got confused because you seemed to imply that plus/minus shouldn't be used even to control the width of the part in Fig. 6-4. It's perfectly fine to do that. I see now that the issue is how to tie all the relationships together (since A is primary).

But I agree that the perp control in that figure is off base. The surface in question is certainly not perpendicular relationship to B.

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[dingy2]

Evan:

RE: figure 6-4 in the standard

I don't know if placing a +/- tolerance on the height is applicable since I don't know the function of the height. If it has no function and is in space, then yes, I would suggest a +/- tolerance.

As far a placing a +/- on the width, there is nothing in the standard that states that I could not do that - nothing! Personally, I don't like any of the angles whether to a surface or a hole. If the feature HAS a functional importance, I would suggest using profile of a surface on a surface or positional in case of a hole rather than angularity, perpendicularity or parallelism.

The point that I was making was not about fig. 6-4 but Norm's contention that it is "bad practice" to place a +/- tolerance on a surface.

Dave D.

http://www.qmsi.ca

 

[NormCrawford]

Your right! The standard does not state that +/- shall only be used for features of size. But it's not my fault. I wasn't on the committee. And the standard does not require or recommend using profile on all surfaces; nor do I.
However, there are some clear indications that +/- is not the best choice for tolerance of location. Such as 'dimensions shall not have more than one interpretation' and paragraph 2.6.1 defines the origin symbol to help prevent such incorrect interpretation using +/-, and in the 2009 standard the note in paragraph 2.6 "Tolerance Accumulation" even goes on to make the recommendation that 'locating features using directly toleranced dimensions is not recommended'.
When you say it doesn't take much thought to figure out the datum structure when a +/- dimension comes off of a datum feature that basic dimensions are related to, I have to disagree. Companies and industries can make whatever "policy" for "assumption" they want but the fact of the matter is that a +/- dimension for locating one feature to another has no datum structure and therein lies the problem.
What if the designer does not want a location relationship to be measured from a datum feature simulator? For example a direct thickness requirement. How can that be stated? The general practice is that that is exactly what +/- linear dimensions of location do. It is in many "opinions", including mine, that it is incorrect to measure the location of a feature from a datum feature simulator unless the use of said simulator is explicitly noted on the drawing which is what feature control frames do and +/- linear dimension of location do not do.
And so here we are. Two different interpretations which violates a fundamental rule in both the 1994 and the 2009 editions.
I think it would do the standard well to make the statement that +/- linear dimensions of location shall not be measured from a datum feature simulator.
I too think there can be the right blend of +/- linear dimensions and GD&T, but I just think that is accomplished when the +/- dimensioning is left to limits of size only and I wish the standard would make that statement too!
With regard to the automotive general profile note example, I haven't a clue either what they mean by the default not having any functional importance.

Norm Crawford
GDTP-S
Applied Geometrics, Inc.

http://www.GDandT.com

 

[NormCrawford]

John-Paul - putting a +/- dimension to control the width is perfectly fine. I didn't say it wasn't. But in reality, why would I control the one face of a functional feature of size with the angularity? I suppose someone will somehow come up with some theoretical need, but it just doesn't seem practical to me and my hand would certainly go up during a design review. And if the width is a functional feature of size, there are form control tools available without the datum reference example shown in Fig 6-4 that I would certainly prefer to use to refine or release the Rule #1 control on form. And if the width is a "functional" feature of size, would it not be more common to use that functional feature as a datum feature rather then one surface of the total width FOS?
The perpendicular control is in fact valid per the standard. I don't like it, but it is valid inb both the 1994 and 2009 versions.

Dave & Evan --- I would not put a +/- dimension on the height again, unless the height acts like a feature of size. That is that it has a mating feature of size. If in fact the "non-functional" feature is only making contact with air, I would definitely not use a +/- dimension and would use profile. The so called height is some sort of requirement even if it only makes contact with air; no mating surface. I would want that requirement measured consistently any where in the world and so how to inspect that feature is clear to everyone. Clear, consice, valid communication. If you use a +/- dimension one can easily argue that it is a feature of size and thus subject to rule #1 requirements. So, I prefer using a tool that clearly states that rule#1 is not in play, is not part of the design intent, and will not be checked for that feature.

Norm Crawford
GDTP-S
Applied Geometrics, Inc.

http://www.GDandT.com

 

[axym]

Here's why putting directly toleranced dimensions on predominantly non-opposed features can be risky and therefore considered a bad practice. Even if the feature "acts like a feature of size", Norm.

A size tolerance provides control in terms of requiring that the entire feature conforms to an MMC boundary and that all actual local sizes be within a certain range. This provides inadeqate control when applied to features that have unopposed sections where the actual local size cannot be defined.

Please see the attached diagram of what could happen if the height of the part in Fig. 6-4 was toleranced with a +/- size dimension. Even though the form error of the lower surface is huge, the feature conforms to the MMC boundary and all the local sizes are within the proper range.

If Rule #1 was waived, then the boundary requirement would go away leaving only the local size requirement. Then the lower surface could be almost any shape at all and still pass the size tolerance.

One might argue that other tolerances on the part would prevent my inane scenarios from actually occurring. Maybe, but this doesn't change the fact that a directly toleranced dimension only provides meaningful control of the feature in the areas where there is opposition.

That's why I think it's a bad practice.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

 

[Belanger]

Norm --

I like your comments, but I need you to clarify a few things. Mainly your statement that "it would do the standard well to make the statement that +/- linear dimensions of location shall not be measured from a datum feature simulator."

I don't even see how it's possible to use a +/- dimension from a datum feature simulator. Datum feature simulators only exist for callouts that invoke one or more datums, and +/- dimensions never invoke a datum, unless a local note specifically says so, per the note at the bottom of p. 52 in the 1994 standard (and even this seems to have been dropped in 2009, unless I am missing it).

So are you just saying that the standard should spell out that what's not possible is not possible? If folks are using Y14.5, this should already be understood. Or am I missing something?

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[fsincox]

First, I want to thank you all for your wonderful insights, this has really gotten interesting.
I must say, the last few posts, seem to me to provide some possible insight to other reasons the ISO does not use rule #1 as it’s default. For all the benefits people seem to think it brings, it seems from some discussion here, like it caused this whole feature of size problem that I have had such an issue with.
When I worked in machine tool we had these 1.5 inch X 6.0 inch X 8.0 FOOT steel transfer beams I had to deal with. Along the beams were various hole patterns that were really only important functionally and practical to relate locally as patterns and somewhat less important over all (I did NOT say NOT important at all). These beams were tied together at the ends with dowels and bolts, forming long chains across a long transfer line say 60 feet.
I knew rule number #1 was really working against me, I knew the beams would not be perfect form and allowed for straightness errors. The datum concept used in the book was impractical, also. I struggled with locally defined datums, individually, and decided on defining all features only in a restrained condition explaining to all that once the part was released from the fixture the holes and the local surface would move together so they could just measure locally.
This is when I first saw the ISO standards. The ISO definition of dimensions meant measured locally not from some datum if there was no one is given, that is what I really wanted all along.
So the little blocks in the book are fine, for what they are, some of us have different parts.

 

[dingy2]

Norm:

When an angularity (perpendicularity, parallelism or angularity) is the only requirement, the location of the feature cannot be shown as a basic dimension since the angularity of the feature and its location are somewhat independent.

If the feature was a surface and profile of a surface is the requirement, then basic dimensions to the feature must be shown.

Now back to fig. 6-4.

There is no doubt that the dimension from datum B to the surface feature MUST be shown as a +/- tolerance. There just isn't any other way since we cannot use a basic dimension.

Let's say we have a hole and the only geometric requirement (besides rule #1) is angularity. How would one show its location besides a +/- tolerance?? Any takers on this question??



Dave D.

http://www.qmsi.ca

 

[Belanger]

Yes Dave,

The problem with using a +/- dimension to locate a hole is this: to locate the hole requires dimensioning in at least two directions of space. Yet with +/- dimensioning, we don't know which edge takes precedence. This requires datums, which mandates GD&T, not a +/- tolerance.


John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[dingy2]

John-Paul:

You did not answer the question about how one should tolerance the location of a hole that had only angularity (which is GD&T). How would you do that?

Dave D.

http://www.qmsi.ca

 

[Belanger]

My point was that +/- dims should only be used for size, chamfer, or radius callouts. Not location!

I guess that does bring up an interesting question -- if I say that +/- dimensions can't be used to locate a hole that has angularity on it, what's the point of the angularity? But it's still valid: I would say that a position tolerance should be given (with a larger value than the angularity).

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[dingy2]

John-Paul:

I might agree with you about positional rather than angularity but the question was how would a Designer reflect a location of a hole where there was only a angularity requirement. They cannot use a basic dimension.

You stated that +/- dims should not be used for location. What left to use then????



Dave D.

http://www.qmsi.ca

 

[Belanger]

Not sure what you're asking. You want to give a location tolerance, but you say that angularity is the only requirement. So why mention a location tolerance?

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[dingy2]

John-Paul:

We have a hole that has only a angularity requirement in the FCF. We know that angularity is relatively independent of its location so one cannot use a basic dimension.

How would the Designer show the location of this hole?

Dave D.

http://www.qmsi.ca

 

[Belanger]

If the hole needs to be controlled for location, use basic dimensions and give it a position tolerance. If the hole's location is not terribly important, use a generous tolerance in the position FCF. Either way, plus/minus tolerancing should not be used at all except for tolerancing the size of the hole.

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[dingy2]

John-Paul:

You seem to say that angularity tolerance on a hole is not a valid requirement by itself and cannot be used. It needs a positional tolerance where the angularity is a refinement?? Is that correct?

Using your philosophy, perpendicularity, angularity and parallelism should never be utilized without either a positional or profile of a surface since the only way to tolerance the feature location is with a +/-. Is this your understanding?

I certainly didn't read any of this in the standard. I have both the 94 and 2009 standards here and would like to know where to find this information?

Dave D.

http://www.qmsi.ca