Very Basic GD&T Question

[ozzkoz]

Hi, I am a young engineer still trying to get a good handle on GD&T. I have a basic understanding of it and can interpret just fine, but have a question regarding basic dimensions. Every example I have seen for true position gives the basic dimension of a hole location from the referenced datums and this makes it very easy to understand in this case. Suppose the basic dimensions don't refer back to the datums though?

For example, consider a square part with a hole and each side of the square have a dim and tol. Datum A is the face the hole is drilled into, datum B is the right face, and datum C is the top face. The hole has a basic dimension from the right face and from the bottom face and the TP of the hole is called out wrt ABC. Can this dimensioning be done or is it nonsense because the location of the hole is not specified relative to datum C (top face) via basic dimensions only. Not saying I would do this, but could I?

Put another way, must a feature be located relative to the referenced datums using basic dimensions only? When we use the FCF we are saying that the position is to be checked relative to the datums, but do the basic dimensions need to specify the location relative to the datums as well?

 

[ctopher]

If using datums for feature size of the hole, use basic dim for location of the hole.

http://www.tec-ease.com/tips/may-00.htm

http://www.draftingzone.com/shoppingzone/dmpgd.pdf

http://www.draftingzone.com/shoppingzone/dmpgt.pdf

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[PaulJackson]

Ozzkoz,

The basic dimensions do not have to dimension directly to the datum features specified in the feature control frame for the specification to be legitimate... but there must be a basic path to the FCF for it to be legitimate.

It is poor drawing practice however, to detail indirect basic paths between the toleranced feature and the FCF since everyone beyond the designer has to figure the direct relationship to do their job with the design.

Paul

 

[ozzkoz]

Ok Thanks, So it needs to be at least possible to calculate the position relative to the referenced data using only basic dimensions. I know this is not preferable but if I had to I'll know to use only basic dimensions.

 

[fsincox]

Paul,
Sorry, I must at least dissent. While I agree that dimensions from datums, directly are certainly OK, and also, there must be a basic chain back to the stated datums. The standard does not require, and shows examples of, dimensions chained "so to speak". What you are stating is what I believe is an understandable old engineering/manufacturing preference not a real requirement of the standard. In my opinion, this is the kind of thing the adoption of the standard "allows us the flexibility of doing" since tolerances no longer accumulate, otherwise what would be the point of them showing it that way.

 

[PaulJackson]

fsincox,

Dissention acknowledged. I assume it was directed at my "poor design practice" comment. That is however what I have experienced causes unnecessary problems with "customers" of the designers detailing choices “the processors, inspectors, analysts and documentation police.”

Ctopher's linked tip from tec-ease is an example where there are competing practical choices for the basic dimension’s direct orientation and reference from the FCF. You see the 30 basic @ (90º understood) is tidy for reporting ’s error to [A]… likewise 21.21 basic @ 45º is tidy for reporting that feature’s error to [A|B]. Which to choose? In this case it is not as clear as in many others and personally, I would question whether the angled hole should be positioned functionally as [B|A|C] rather than [A|B|C] which would actually eliminate the need for the 21.21 basic. If not, I might suggest that both the 30 (on the left) and the 21.21 (moved to the right) be shown if I suspected that the feature’s displacement @ 45º [A] was more likely to be misinterpreted as central to ’s axis without it.

Tec-ease’s example here is not so clean cut as are most others in terms of how basic dimensions can be specified so that “customers” need not transform the specification basics into those required for measurement and subsequent comparison to the detailed specification.

paul

 

[fsincox]

Paul, thanks.
Ctopher's Tec-Ease example is a good one for the case I would like to make that the 30 dimensioned version likely preserves design intent most directly for posterity, so to speak, as I assume 21.21 is rounded. While I understand that at some point the difference is so small as some may question it’s relevance. That is why I apreciated the standard’s approval, in my opinion, of using bolt circles to define some circular hole patterns. I doen't say you must, but it kind of made it OK again.
I agree with your suspicion of the frameworks but only the design condition will tell us.

 

[KENAT]

PaulJackson, I'll also dissent. When checking, having the hole patterns explicitly dimensioned, rather than all directly back to the datums, is a a bit easier. So, having dimensions back to the datums isn't easier for every other user of the drawing. In fact I'm tempted to say, for what little it's worth, the standard shows dimensioning of the 'pattern' more often than directly back to the datums.

Posting guidelines faq731-376

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

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

 

[fsincox]

Before my work in aerospace, I worked in the machine tool industry specifically as a vendor for the auto industry. We were fighting a battle we ultimately lost with vendors from Germany and Japan. To compete we had to look more for non-American work, I assume it should be obvious to all as to why.
The customer demanded metric based designs as, I believe, they should it is their standard, they are the customer. We worked in inch, the shop required it from us, and beside we used inch stock. Our drawings either had to be dual dimensioned or we would provide 2 sets of drawings, one for the customer and one for the shop.
My point here is that in real world applications if you do not stick to the design dimensions, start rounding for convenience and are looking at it later with out knowing the nominal, it can get difficult to determine whether the nominal design is a metric number or an inch number. This is one way I learned the value of documenting and maintaining the true design intent and that rounding to obtain 1 place, 2 place or 3 sometimes only shoots us in the foot.

 

[PaulJackson]

There are patterns and there are patterns...
Some are created solely for the sake of collectively limiting DRF mobility to a common magnitude and direction via the simultaneous requirements rules. Some, on the other hand, are designated explicitly (as you stated) for mating pattern purposes and for distinguishing differences in functional constraints and liberties for pattern fit and location.

I agree with both of you that it is tidy to define those explicit patterns among the pattern members as it is often illustrated in the standard. My point is that when basics are applied to features on the drawing respective of down-stream customers it saves the customers unnecessary time and work transforming specifications and "confusion with documentation police". It shows the depth of understanding the designer has in other disciplines... like limiting unique process orientations to as few as possible, providing room for spindle collets to minimize tool lengths, limiting bore depths, yada, yada, yada.

As far as rounding goes... someone has to do it if it must be done. You are correct though that 21.21 is actually 21.213203435596425732025330863145. I suppose you could express the basic as an equation like figure 5-43 of ASME Y14.5M-1994. In this case the basic would be [30 / SQRT 2] or [sin 45º * 30] or you could leave it as an irrational value as it is on your CAD model and show as many digits as you choose on the detail layer or as many digits as will appear when the model distance is queried.

Paul

 

[MechNorth]

Paul, designating a new datum reference framework from A/B/C to B/A/C is arbitrary! The designer decides the relationship, not the drawing user. Plus, the purpose of the Tec-Ease example IS to show that regardless of how you lay out the BASIC dimensions on the drawing, the absolute IDEAL location in space is the same (ignoring the question of round-off error which can be addressed by more sig figs). If you are reporting actual GD&T position inspection results, it's a deviation from BASIC location, not from the datum origins. I understand that many (most?) customers don't have the knowledge required to understand the properly-described GD&T deviations, but that's a separate issue distinctly apart from product definition.

As for which way to lay out BASIC dimensions on the drawing, I tell my students to make friends with key people in programming, the shop and inspection, and find out which works best for them. NC programmers often want the chained dimensions because that's how they program their machines. Inspectors often want dimensions from the datums features because they will verify directly from the datum feature simulators ... it's a crap shoot, so figure out who downstream is most likely to bring you a free coffee every now and then, and focus on their needs!

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[NormCrawford]

Works for me Jim!

Norm Crawford
GDTP-S
Applied Geometrics, Inc.

http://www.GDandT.com

 

[MechNorth]

Tks Norm. I dropped off the grid for a while too, just returned a couple days ago myself. Welcome back.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[PaulJackson]

Paul, designating a new datum reference framework from A/B/C to B/A/C is arbitrary!

Jim, designating the datum reference framework from A/B/C to B/A/C is never arbitrary to function. See attachment.

The designer decides the relationship, not the drawing user.

The designer should reflect the functional relationships in his design… all of the users “the downstream customers” are punished when the design fails to communicate that function.

Plus, the purpose of the Tec-Ease example IS to show that regardless of how you lay out the BASIC dimensions on the drawing, the absolute IDEAL location in space is the same (ignoring the question of round-off error which can be addressed by more sig figs). If you are reporting actual GD&T position inspection results, it's a deviation from BASIC location, not from the datum origins.

Agreed but to inspect the deviation one has to orient the measurement system to the basic feature orientation and compare its point, axis, surface or opposed surface element displacements relative to DRF specified… if the basics are not specified directly then the inspector/programmer has to figure them.

I understand that many (most?) customers don't have the knowledge required to understand the properly-described GD&T deviations, but that's a separate issue distinctly apart from product definition.

The customers of the design are the ones that are charged with (and have always been charged with) reporting the properly-described GD&T deviation. It is just bothersome when a designer snaps X,Y, Z coordinates on an axis / surface intersection where the hole’s axis is not square with the datum features. In order for the inspector to communicate with others who only have the specified design in front of them he has to transform the worst measured axis deviation into X,Y,Z coordinates where the axis would intersect the “nominal” surface contour. It is a royal pain in the but and it is totally preventable if designers could adopt a more user friendly strategy.

As for which way to lay out BASIC dimensions on the drawing, I tell my students to make friends with key people in programming, the shop and inspection, and find out which works best for them. NC programmers often want the chained dimensions because that's how they program their machines. Inspectors often want dimensions from the datums features because they will verify directly from the datum feature simulators ... it's a crap shoot, so figure out who downstream is most likely to bring you a free coffee every now and then, and focus on their needs!

Good for you for pointing that out, however It is not “a crap shoot”! I would suggest that you consider first the needs of measurement/inspection – they have to report their findings relative to the specification. Manufacturing is free to process as they see fit to accomplish the task… they often adopt surrogate coordinate references and rotations respective of fixturing and tooling.

Paul

 

[MechNorth]

I understand your point, Paul, but your comment that you'd have done "B/A/C" rather than "A/B/C" is still arbitrary because you don't know the function of the part. So, while you may be right, it still puts a doubt in the mind of other readers and may promote their own deviation from what is on a drawing they receive...because it would make more sense to them.

Agree on the punishment of the downstream users; too common, and we were all purpetrators in our early days.

I empathize that your focus may be on facilitating the inspector's job, but my experiences more often reflect a higher mathematical capability in the inspection area than in the machine shop as a result of the degradation of skills in a button-pusher environment. Even within the inspection area, the dimensional layout needs can vary significantly. Open setup, sure, dimensions from the datums is probably easier for some, but no value for others. Manually programmed CMM, chained dimensions are fine because the program itself assumes basic dimensions. CMM from CAD, doesn't matter. CMMs don't go back and re-generate datums between every measurement point, so tying them back to the origins doesn't necessarily help there either. Hence, it's a crap-shoot. As I often point out to students, "play nice" because those downstream are making and checking your parts, and they can make life very difficult. Of course, inevitably, you will tick someone off as you are making someone else very happy.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com