Full or Partial GD&T 1

[MechNorth]

A long time ago, in a thread started before I joined Eng-Tips, someone initiated the debate over whether a drawing needs to be completely GD&T'd or not. Clearly each supporter of the rival factions has their own reasons for their assertions, but I'd like to see them listed, defended & debated in a logical & hopefully standards-based manner. I'm not naive enough to believe that this will launch everyone over to one side, but it should give us all some perspective as to what the other side of the wall is thinking and why.

So here goes ... I'm for an essentially complete product definition using geometric controls tied back to datums where possible. The exceptions where conventional tolerances would be used as listed in Y14.41 Table 8-1 are:
1) Fillets, Rounds & Chamfers
2) Reliefs, Step Surfaces (I don't particularly support this one; surface profile is more concise)
3) Countersinks
4) Oblique Surfaces
5) Entry Depth and Spotface
6) Remaining Thickness
7) Notches, Flats, and Pin Heights.
Now, if you look at the Note in Section 8.2 of Y14.41, it indicates that the list is not exhaustive, but rather indicative to similar and other valid applications. While it doesn't explicitly preclude the applicability to position dimensions, such application would be contrary to the indicated application methods of such controls which are restricted to attachment to size callouts, directed leader to the feature (surface), or on an extension line from the feature.

Also, from an engineering perspective, I want to remove ambiguity from my documentation, so that many featues such as weight-reduction holes, non-functional outer geometries, etc. are at least related loosely back to my DRF. Ambiguous documentation cannot be defended in court, and that is a growing reality in industry today as margins & survival dwindle.

Et tu?

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[powerhound]

I'm with Jim on this. I think applying GD&T to some features and not to others only perpetuates the myth that GD&T is only for critical features which in turn strengthens the belief of the uneducated that if GD&T is on a print then the part must be really critical and thus needs to cost more.

There will come a day when GD&T will be fully accepted as the "old schoolers" and "fence straddlers" retire and the new generation is fully on the GD&T side of the fence. This will be when people that hold the ASME GDTP certification will be more the rule than the exception as it is today. But that day will not come as long as there are the those out there that preach "tolerance"...



Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

The more I learn the more I tilt toward the viewpoint you give above.

For features of size ASME Y14.5M-1994 arguably dictates the use of Position or Profile in paragraph 2.1.1.1. It doesn’t differentiate between “critical functional features” and “non critical” features or similar.

However, I do think that +- dims can be usefully used for overall/outline dimensions in many, even most, cases. This is fully compliant with my understanding of 14.5. In fact many illustrations in the standard show this although one must bear in mind what paragraph 1.1.4 says about the figures in the standard.

Problems come when you have a supply chain, or even your own staff, that don't adequately understand the GD&T.

The widespread perception(s) that "you only use GD&T when it's important" or "they used GD&T it must be tight so we'll charge more" and similar is one of the biggest obstacles I see to more widespread acceptance/use.

At the end of the day we/our employers are in business to make money. How far do you take having a fully standard compliant drawing that follows all the best practices etc., just in case it ends up in court, despite the fact that in reality it causes parts to cost more. Not everyone has the ability to force their vendors to get trained etc. and it can be time consuming to shop around and change vendors just to find someone standards compliant etc. It’s a case of balancing risk/reward/consequence etc.

Sorry if that’s not quite as standards based as you intended Mech North.


KENAT, probably the least qualified checker you'll ever meet...

 

[drawoh]

MechNorth,

I do not think this discussion is meaningful. The really important thing a standard like ASME Y14.5M-1994 does is provide a consistent interpretation of whatever is on your drawing. Even if you apply no GD&T, your drawing is unambiguous.

There is no guarantee of course that it means what you think it does.

GD&T is a tool, and I use it a lot because it expresses what I want to tell my fabricators. I want to make my drawings as simple and clear as possible, and GD&T provides resources for this.

Most of the time, I apply a profile tolerance to my outlines. This is simple and clear, and it gets me around the angle tolerance on my nominal 90[°] angles.

Most of the time, I apply sloppy ± tolerances to my chamfers. This is because the chamfer usually is just a modification to an edge, and I cannot be bothered to relate it to a datum anywhere. If it matters, then I think through what I am doing.

I love positional tolerances because the tolerance is part of the hole specification. Applying the tolerance to the X and the Y[ ]coordinate is not very logical, especially if there is more than one hole at that position, and the holes do not have the same requirement.

I still apply ± tolerances to a lot of linear dimensions. A positional tolerance would work, but often the drawing is more cluttered as a result. A lot of linear dimensions do not rely on implied perpendularity.

JHG

 

[fcsuper]

I personally try to avoid using profile unless necessary for linear dims. In my mind, profile still needs some refinement before it can be generally applied. For example, it takes more space and time to set up a profile tol than just a linear over all with +/- right now.

I'm trying to use positional more often these days.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[swertel]

I would use GD&T more, but I much prefer +/- tolerances for the reason that they are typically easier and cheaper to inspect. I can pull out a drop mic, calipers, or other desktop instrument to check most +/- tolerances. Positional tolerances require the above, plus some mathematics to determine tolerance especially when the tolerance is based on MMC or LMC of not only the feature being checked for position, but of datum references as well.

Most certainly, feature control frames - when properly applied - can actually save money by relaxing tolerances, the mere sight of them just screams of increased inspection cost that often exceeds the manufacturing savings of loose tolerance. And the screams are not just screams of inexperience. They are often justified screams because the determination of acceptance/rejection to the tolerance requires more than a pair of calipers.

--Scott

http://wertel.eng.pro

 

[drstrole]

I have to agree with MechNorth on this one also.

The part is dimensioned by how it mates, assembles or functions in the assembly. The features in the part need to be dimensioned by the function / role that they play in the part. If the correct geometric characteristic is not selected to locate or orient that feature back to the correct datum features, then how do you ensure that the feature is going to serve its purpose? If it is a hole to shed weight maybe a profile tolerance or possibly size tolerance and position at LMC apply. My point is the designer needs to make sure that every feature does what it needs to do and does not adversely affect other features. Just because a feature may be able to have a large tolerance does not imply that you use an incorrect method to tolerance it.

Drstrole

 

[MechNorth]

Thanks everyone for the replies so far. As I said originally, I'm not naive enough to believe that this would sway anyone's thinking, but I do like to get people thinking about their beliefs & convictions.

I'm a notorious Devil's Advocate, and was one even before I started calling myself such. We all have developed instinctive "gut" feelings, biases, etc. What I've long ago discovered and repeatedly confirmed is that people rarely challenge their own knowlege base that is the basis of their instinct and intuition, and therefore have difficulty considering other points of view even when presented with empirical and scientific support.

As a GD&T virgin, I had some bad experiences with a mish-mash of modified standards and didn't see any value in the technology; we were highly profitable and our scrap rate was reasonably low, and we had a strong base of tribal knowledge developed internally and with external suppliers. I was forced (kicking & screaming) into leading a GD&T implementation in which I had no faith. As my knowledge of the technology evolved, so too did my scope of knowledge for our internal & external fabrication practices. I started to see the cost of developing & re-developing tribal knowledge, and that GD&T could allow greater flexibility in fabrication sources. I saw, too, that engineering had to start challenging their basic assumptions and core beliefs. We were doing many things for archaic and invalid reasons when evaluated based on modern design & manufacturing technologies. So I started to believe, but not completely.

I still allowed a mixture of GD&T and conventional tolerances despite being coached not to by new trainers. After all, what did they know about our product lines, right? Turned out that the conflicts that they anticipated between the two methods being applied on the same drawing came to be, and we had unanticipated problems as a result.

After that, I lead a functional rethink of our basic product right down to the component level. By playing Devil's Advocate, we peeled away our founding assumptions to recognize the true functionality of each component, resulting in changes to our design that would reduce fabrication costs significantly and improve tool life.

Of course, the immediate reaction from our purchasing department was that the cost would double, and that's generally what happened when the quotes came back in. I questioned a few of those suppliers and found that they made an assumption that the requirements were tighter because of the GD&T application. In other cases, however, suppliers took the initiative to study the prints and recognized that the requirements were significantly looser than before, and reflected that in their quotes. Some suppliers, however, understood a bit of GD&T and came in significantly below the others. The difference was just a couple hours of training.

We went through the exercise of offering non-mandatory training which most suppliers didn't bother with, but those that did were able to reduce their costs, our costs, and open themselves to a broader market. Those shops are the ones that now have a competetive advantage in the global industrial war that is waged between western nations and the cheap labor markets of the east.

GD&T is a tool. Any tool is intended to make your work easier and more effective. Hopefully you use the tool to your greatest advantage and greatest value.



Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

Please share with us your experience where a drawing containing positional on all holes and profile of a surface on all surface(feature control frames shown in notes) assisted the Designer with design intent.

Thanks

Dave D.

http://www.qmsi.ca

 

[MechNorth]

Interesting question Dave. If I'm understanding you correctly, included in the "Unless Otherwise Specified" notes, you have a general surface profile tolerance and a general positional control which is labeled as exclusively applicable to holes.

If you are questioning which to use, consider the following:

First, a surface profile is not used to control the location of a feature of size (FOS) (criteria: directly opposed points and applied size tolerance). 6.5 PROFILE CONTROL ... With profile tolerancing, the true profile may be defined by basic radii, basic angular dimensions, basic coordinate dimensions, basic size dimensions, undimensioned drawings, or formulas. So, in the case of a hole with a conventionally toleranced size dimension (a FOS), the general positional control for holes is applicable.

Next, a position tolerance can only be used to locate the center planes/axes/points of features of size (5.2 POSITIONAL TOLERANCE, A positional tolerance defines: a. a zone within which the center, axis, or center plane of a feature of size ... or b. ...a boundary, defined ast he virtual condition...), or to locate the boundary of an irregular enclosed feature (6.5.5.1 Boundary Control for a Non-Cylindrical Feature)

So, in the case where you have a non-toleranced size dimension for a hole, and there is no indication that UNTOLERANCED DIMENSIONS ARE BASIC, then it is not known whether or not the hole is to be considered a feature of size, and you have no resolution, and the designer needs to be flogged.

If the size dimension has a directly applied tolerance, the hole is a FOS and position is applicable, profile is not.

If, on the other hand, you have a non-toleranced size dimension for a hole, and there is a note equivalent to UNTOLERANCED DIMENSIONS ARE BASIC, then the hole cannot be considered a feature of size which means that the position control is not applicable and the surface profile is applicable.

As for my experience with this, unfortunately I have made the error of releasing drawings (early on) that had both the general surface profile and general hole position controls in the notes, but without the note "UNTOLERANCED DIMENSIONS ARE BASIC". At first it wasn't an issue because the shop had no idea what it meant either way, but as they evolved their understanding of GD&T, they started to recognize the conflict and addressed it with me. By that time, I understood the difference (subtle as it may be), and added the note to our templates.

The reason that I followed that approach was that initially the majority of our holes were held to a standard positional tolerance, regardless of size or function, so we could reduce drafting time. We removed the general positional tolerance on holes when we started to actually do fixed & floating fastener calculations. I still include a general positional tolerance for tapped holes in my notes under "UNLESS OTHERWISE SPECIFIED" to reduce detailing. Where a different positional tolerance is needed on individual features or patterns, whether more or less restrictive, I apply it directly to the appropriate features.

The design intent for the features is indicated by a combination of the size controls and location controls, and the relationship to the datum reference frame. Without datum references, I would be free to verify the dimension pretty much any way that I wanted to. For example, if the center of a DIA 5+/-2mm hole is dimensioned as 50+/-5mm from an edge of a plate, I could do a two-point check from the tangent point on the hole to the edge of the plate; if the value is in the range of 47.5 +/- 7mm, the part could legitimately pass the spec. But what if the edge of the plate has a significant deformation at that location? The use of conventional tolerances doesn't require the use of the entire plate edge to establish an origin of measurement, just the closest point to the opposed measurement point. By invoking the edge face of the plate as a datum feature, and referencing the center of the hole back to that datum, I eliminate the bias of that localized deformity along the edge. In that way, my design intent is communicated to the drawing users.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

You gave an example where you had in the notes section a general positional tolerance and a general profile tolerance that applies to all holes and all surfaces. Your error was to also place a tolerance on the location rather than have them in basic dimensions. You were new at this at that time and was a clear error.

I realize that design time is reduced if all dimensions are basic and the GD&T in notes covers everything. Shouldn't a design give the user a clear understanding of the design intent? There are so many features that could be out of specification and the part will still function while others are important to its function.

Here is the question again.

You have a drawing that states in notes "Complies with ASME Y14.5M-94" and all three datums are shown on the drawing. Please explain why having the default GD&T in notes assists design intent rather than isolating important features from a design perspective and applying GD&T on those features only.



Dave D.

http://www.qmsi.ca

 

[MechNorth]

I guess that I don't see your real question, Dave. Having datums on the drawing does not automatically mean that you measure from their respective simulators. Conventionally-toleranced features aren't measured from a datum simulator, and only require 2-point measurements, so they are dependent on local irregularities in the surface(s). Having any geometric control is more indicative of whatever design intent than leaving the inspection setup as indeterminate. With geometric controls, you pretty much eliminate tolerance stackups, which again emphasizes the design intent and inter-feature relationships via principle of simultaneous requirements and other patterning methods.

Some users unquestioningly maintain the mindset that "GD&T equals CRITICAL" and "Conventional Tolerancing equals irrelevant". I'm curious what imbedded this belief and where it is supported in the ASME standards? I understand that this was a popular convention for a long time, but the GD&T standards (Y14.5, Y14.41, etc.), their use, and the supporting technologies no longer hold it valid or useful. The tolerance value included in the geometric control determines the criticality of the feature, not whether there is a geometric control or not. That remains consistent with conventional thinking re criticality as reflected by the limits placed on the feature's geometries and location.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

As I have stated before, one would come from the datums to measure a surface or hole. On a surface, one measures in various locations and report either the values from the lowest to highest readings or the worst reading. On holes, one would measure exactly the same as bi-directional in positional tolerances in RFS. I have actually measured product like this in the past.

The present standard really does not get into application. It certainly does not state that one's note section must contain default positional and profile feature control frames.

Let's get back to my original question again.

Let's say that we have a pattern of holes that will receive fasteners on fixed locations. We also have another pattern of holes to lighten the product while there is another threaded hole where a machine screw will attach a wire. You now know the design intent of the holes.

How does having a default positional tolerances on all holes in the notes section enhance the design intent in this situation?

Dave D.

http://www.qmsi.ca

 

[MechNorth]

Dave, you are making an assumption that you measure from a datum for a conventionally toleranced hole location. That is not defined in the Y14.5 standard, and in fact, is not defined anywhere. This may have been your personal convention (and likely a good one at that, though not accurate to the standard) that you learned by rote, but it is not supported in the standard, and therefore cannot be used as the basis of your argument. Conventional tolerances only require a two-point measurement, and even then you can alter your inspection setup to help the part pass spec ... so how are you finding the center of that hole in a repeatable manner? If the assumed relation to the datum reference frame is the underlying foundation of your conjecture, then it's time for you to either validate it based on a standard, or step away from it. Again, my standard-supported position is that by invoking a general surface profile, all features on the workpiece are tied back to the datum structure, and that is design intent. I have repeatedly defended my position based on the Y14.5M-1994 and associated standards such as Y14.41-2003.

In addition, if you look at Chapter 5: Tolerances of Location, Section 5.1 General - This Section establishes the principles of tolerances of location. Included are position, concentricity, and symmetry used to control the following relationships: ...". Notice that there is no indication whatsoever of using conventional tolerances to locate features.

Where is your supporting documentation? By repeatedly asking the same question in the same way, you are just establishing that you don't have any basis to substantiate your position. So now the ball is back in your court; I challenge you to prove your case based on recognized standards.

I look forward to seeing your results.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

I am not trying to prove a case nor am I arguing a point, I just asked a question. You answered the question the best you could.

Thanks

Dave D.

http://www.qmsi.ca

 

[dingy2]

How does it assist users of a drawing having in notes a default positional and profile of a surface tolerances? Does this make the drawing clearer, more concise reflecting the design intent of the product and features? It certainly does reduce design time though.

Default Positional Tolerances

2.1.1.1 Positional Tolerance Method (ASME Y14.5M-94) "Preferably, tolerance on dimensions that locate features of size are specified by positional tolerancing method described in Section 5." That statement does not say "must" only "preferable" so co-ordinate tolerancing of features of size is acceptable in today's standard.

Having positional tolerances with a diametrical tolerance zone as a default could actually reduce tolerances if the Designer does not convert the tolerances correctly. If one had a +/- 0.25 mm co-ordinate tolerance, it does not convert to a diametrical tolerance zone of 0.5 mm. It converts to a diametrical tolerance zone of 0.7 mm.

Having default positional tolerances on a variety of hole patterns at MMC referencing the same secondary and tertiary datums in RFS or in MMC is extremely restrictive. One must assume a single pattern for all holes (5.3.6.1 or 5.3.6.2) and are best confirmed with a checking fixture. That's tough.

If one still wants to place a default positional tolerance, I would suggest using RFS in both the tolerance and reference datums and convert the co-ordinate tolerances correctly.

If we have holes or bosses where there is a function and relationship, then that pattern should be shown with a positional tolerance in MMC referencing the secondary and tertiary datums in MMC. The drawing now becomes clearer and Manufacturing Engineering, Production and Quality will concentrate on that pattern on a continuous basis building a checking fixture.

Profile of a Surface

Most surfaces are not important to its design function but having a default profile tolerance is easy for the Designer reducing design time. There is absolutely nothing in the standard dictating default profile tolerances.

Some surfaces are vital to its function and relationship and a profile tolerance is required.

I guess if the Designer wants to reduce design time and use a default profile tolerance rather than co-ordinate tolerances, make sure the actual tolerance is huge. Then the Designer could define surfaces that really require a profile tolerance much tighter.

Frankly, default co-ordinate tolerancing on surfaces is still clearer.

I think that we keep forgetting that the end result of a Designer's product is a drawing that reflects the design intent of the features. Having default positional and profile tolerances in notes does not appear to make the end result clearer and could actually confuse the end users.

Jim - you have the last kick at this.

Dave D.

http://www.qmsi.ca

 

[KENAT]

dingy2, read all of 2.1.1.1 and you'll see, that to my understanding the recomended alternative to position, is profile.

2.1.1.1 Positional Tolerance Method. Preferably, tolerance on dimensions that locate features of size are specified by positional tolerancing method described in Section 5. In certain cases, such as locating irregular-shaped features, the profile tolerancing method described in Section 6 may be used.

It could be argued that the above is telling you to use position, unless profile is better suited. The 'Preferably' is arguably to allow use of profile, not +- dimensioning.

Of course, like most users I at times use the 'preferably' to allow me to use +-, but I'm no longer convinced that was the intent of the above paragraph.

Having positional tolerances with a diametrical tolerance zone as a default could actually reduce tolerances if the Designer does not convert the tolerances correctly

Well the same goes for any kind of general or block tolerance etc. If you don't use it/allow for it the same way you would individual tolerances then it can cause problems.

As I recall you have previously stated concerns over the use of general/block tolerances as people tend then to not think about the tolerances, and may have even proposed that they should be done away with. I share your concerns, but used properly block/general tolerances can help create a cleaner, easier to read drawing.

I'm not sure having general position or profile controls is any worse than general/block +- tolerances but I must agree with you and say I don't like the idea, except maybe on some MBD applications.

KENAT,

Have you reminded yourself of faq731-376 recently?

 

[MechNorth]

As always, you bring up some good arguments, Dave.

First, there is no support anywhere in the Y14.5 standard, whether textual or graphical, which supports the use of +/- tolerances of locations for features of size. Along with that, the standard says how to check the size & location based on evaluating the true geometric counterpart which best represents the feature in relation to the datum reference frame. How do you repeatably find the center of a hole or boss otherwise, particularly when you must consider the full depth of the feature and not just one end or cross-sectional location? What reference point do you use as your measurement origin when checking conventionally-toleranced locations? Do you use the entire surface or just the closest local point on the surface? This is ambiguity. One can, of course, take the lazy-man approach and put a note "ALL POSITIONS TO BE INSPECTED WRT DATUM REFERENCE FRAME A/B/C" or equivalent, which at least tells you where to measure from, but still doesn't help you on repeatably finding the 3-D center of the feature.

The argument that a designer may mis-convert the tolerance is valid, and unfortunately does happen ... so, let's do away with all position tolerances because the uneducated / undertrained can't be trusted to use them correctly? If it's ok on "critical" features, then it's ok on "non-critical" features too, isn't it?

Excellent point re the restrictiveness of a general positional control as it invokes simultaneous requirement. If that is the intent, then yes MMC is needed. I'll be adding SEP REQT to my title block. Tks. In my title block, I don't use a general position tolerance for simple cylindrical holes, just for tapped holes, and then at RFS. I need to add "MINOR DIA" as well now that I think of it. general clearance / non-critical holes, I typically use a basic size dimension and control with a surface profile (direct or general) which is easier to inspect anyway.

Now, all the above is relevant to the current revision of Y14.5 (1994), but does not consider Y14.41. Will you be able to continue with that conventional tolerancing methodology for position within that standard?

Again, you are correct that there is nothing dictating (in Y14.5) the use of a general surface profile tolerance, though it is supported, and it is the way to control all aspects of a workpiece not directly controlled.

Dave, our definitions of "clearer" and "easier" are different, and understandably so. We both initially learned under different standards, different manufacturing and metrology technologies, and from different perspectives (engineering vs inspection). While many businesses will be able to continue with the old methodologies for a while longer, my concern is what will happen when they get forced into a CAD-model-based environment where they will have to comply with Y14.41? Will the conventional tolerances on location hold up? I have a lot more studying to do on that standard before I understand the full ramifications. I think I'll ask that next week at the Y14.41 meeting if I get a chance.

In the interim, if you have the time, pls let me know (by forum or e-mail) how you are measuring the position under the coordinate tolerancing scenario. That's not to continue the debate, but so that I can appreciate the steps, simplifications and assumptions that go into this conventional measurement method; I am genuinely interested, and this is how I broaden my understanding and knowledge base. Tks again. I'm enjoying the challenges.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[ewh]

I want to thank you, Jim, for a good, condensed lesson on =/- vs positional/profile tolerancing. While I have attempted to follow the standard as written (and as you have explained), it is sometimes an uphill battle when those with the final approval authority resist. Your posts may help me help them to actually see the light.

When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - [small]Thomas Jefferson [/small]

 

[MechNorth]

Thanks to everyone who participated. As I've said, I like to play devil's advocate to try to figure out not just the what, but also the why of a belief system. For those that gained some insight or alternative perspectives, I'm glad our debate helped.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com