Tolerances for Basic dimensions, continued... 2

[ewh]

israelkk,

Don't think of it as a debate. The standard is a complex one, and I'd say that most of the people who use it don't understand it fully. I definitely don't, but I do have a basic working knowledge of it and turn to the standard often to improve my understanding of it. The worst thing we can do if we don't understand why something is toleranced the way it is is to blindly accept that because it's been used that way before, it must be correct.

You are correct in that you can use basic dimensions without establishing features, by using other dimensional tolerances. Examples are angularity and taper. I have gotten into the habit of establishing datums before I dimension, thus my erroneous comment.

However, to properly use a geometric tolerance on a hole, you must establish what that tolerance is relative to, which would be datum(s). It can't be relative to itself.
For true position, per Y14.5M-1994, para 5.2.1.3, "It is necessary to identify features on a part to establish datums for dimensions locating true positions." For your example to be correct, one of the holes would have to be a datum, and the others located relative to that.

I am definitely open to correction on this, to better understand the standard myself. I won't accept "because that's how it's done" as a valid reason, but will gladly accept any argument documented by the standard.

Eric

 

[btrueblood]

The bolt pattern (or more specifically, the pattern of bolt centerlines) can form its own implied datum, as in bolt circles or basic dimensions.

 

[ewh]

btrueblood,

Could you direct me to where in ASME Y14.5M-1994 that implied datums are referred to, defined or used? My copy of the standard is missing the index. Thanks!

Eric

 

[btrueblood]

(blush) Y'know, I was worried I'd get called out on that one! I don't have a copy of the 1994 standard, but base my knowledge on years of using the 1982 version.

Take a look at examples of position tolerancing of bolt holes in a circular pattern. The TP tolerance is applied with no specification of a datum (i.e. there is no "A" or "B1" etc. called out in the gdt block), and instead is taken as meaning (essentially) the TP of the bolt holes relative to one another. I may be wrong, and the new standard may have abolished the practise -- if so, they've nullified the specifications of a lot of other standards, wherein the datum is "any and all the bolt holes in aggregate" in order for the wheely thing to fit onto the axle-thing.

 

[btrueblood]

By the way, on all our prints, we still specifically call out ANSI-Y14.5M-1982 as our standard.

 

[drawoh]

ewh,

You can apply geometric tolerances without specifying datums if you confine yourself to self contained qualities such as flatness. When you control qualities like location or profile, you need reference datum.

ASME Y14.5M-1994 specifically describes a dual location tolerance where you specify a location of 1mm diameter with respect to datums A, B and C, and a 0.1mm diameter with respect to datum A. This means that the pattern must be accurate, but you do not care where it is located. A positional tolerance without a datum does not mean anything to me, at least as per ASME Y14.5M-1994. The 1982 standard is not close at hand at the momemt.

There is no taper tolerance. My copy of the standard uses a profile tolerance to control this. Both angularity and profile require datums.

JHG

 

[ewh]

drawoh,

I agree with what you have posted, but need to clarify my statement regarding angularity and taper. While a datum is required when specifying angularity in the geometric tolerance block, you can also control it using a basic dimension and a toleranced dimension (no geometric control block or datums involved)(Fig. 2-14 of the current standard).

There is no geometric control symbol for taper, but again, it can be controlled by the use of a taper symbol, basic and toleranced dimensions (no geometric control block or datums involved)(Fig. 2-15).

Profile is a handy and powerful control. It lets you control the form without multiple geometric control blocks, and is the simplist way I know of to control non-standard shapes, such as splines and lofted surfaces. In the new standard ASME 14.41-2003 DIGITAL PRODUCT DEFINITION DATA PRACTICES, the profile tolerance has been updated so that a unilateral tolerance no longer has to be specified in a true view using phantom lines, but is specified using a modifier in the geometric control block.

 

[drawoh]

ewh,

You might have me on this one. I once did a drawing of a 45 degree elliptical mirror in which I specified the angle as a basic dimension. The mirror was a piece of round glass bar cut at 45 degrees on both sides, and I did specify datums. I need to specify one surface as parallel to the other.

I put a tolerance on the diameter. The mirror would have been inspected, admittedly with some difficulty, by jigging it on a 45 degree surface and testing the diameter. There was no need for an angle tolerance.

If I had not cared about parallelism, I could have done without a datum.

JHG

 

[btrueblood]

Well, now...I have a copy of ASME Y14.5M 1994 standard in my lap, fresh from the printers...

There is nothing in the standard that REQUIRES a t.p. tolerance to have specified datums. In fact, the definition of true position (1.3.36) is the position of a feature related established by basic dimensions, not datums. Furthermore, basic dimensions are defined (1.3.9) so that they may or may not reference a datum. My case regarding bolt circles stands - you can dimension the bolt circle without a datum (provided you as a designer don't care about the position of the bolt circle relative to other features). The spacing can also be defined by basic dimensions if necessary. At t.p. tolerance frame can then control the location of the holes relative to the basic dimensions, without reference to any datums required. In such a case an "implied datum" or whatever you want to call it, is formed from the features themselves, and the basic dimensions used.

 

[ewh]

btrueblood,

Read a little further on.
Para 5.2 states "Basic dimensions establish the true position from specified datum features and between interrelated features." "A positional tolerance is indicated by the position symbol, a tolerance value, applicable condition modifiers, and appropriate datum references..."
Para 5.2.1.3 states "It is necessary to identify features on a part to establish datums for dimensions locating true positions." In other words, when using true position, you need to establish what the true position is relative to.
I still have not found where "implied datums" are referred to in the standard.
I am glad to see that you have the standard and are attempting to understand it. Keep at it and let me know when I misinterpret it.

 

[btrueblood]

ewh,

I have read the whole section. I know this is confusing, since most of the time (possibly "all the time" for some of you) the t.p. tolerance based on datums is exactly the type of control required to establish fits and alignments on a simultaneous basis between mating parts. My point applies to a special case, and I'm trying to make sure I know how to handle this case (since it occurs occasionally in the work I do), in a manner which results in the least confusion to people here, and thus hopefully to the least confusion to shops that are going to use the resulting drawing.

First, to counter-argue your points:

5.2 does not require a basic dimension to reference a feature, it can also apply between features.

The verbage "appropriate datum references" holds only when such datum references have been defined.

5.2.1.3 is troublesome, I agree - but what do you do when you DON'T want the pattern controlled tightly relative to other features, or at least not as tightly as you want it controlled for the features relative to the other features in the pattern (i.e. I don't care about the alignment of a pipe flange blank o.d. relative to the bolt pattern to better than 1/4", but the bolt holes must line up to the other part within .03"). I would maintain that 5.2.1.3 simply states that "if you are going to establish a datum, it must be related to features on a part" - i.e. you can't identify a centerline as a datum, but should show the feature(s) that the centerline is to be gauged from.

The definition of t.p at 1.3.36 takes precedence over the statement in 5.2.1.3; at 5.2.1.3 the example is given where the bolt circle is to be controlled (concentric to) an inside diameter as the datum - critical when alignment of some mating part at the i.d. is required, but not always required for all parts.

That said, I know what I'd do now (to avoid the confusion that most of you express in this forum on this topic), is to define the bolt circle as a datum. Would this get the point across to most shops, and avoid confusion regarding the position tolerance requirements as the apply between bolt holes?

I'd worry that the result of the above is an over-dimensioned print (since the bolt circle also needs a basic dimension).

 

[ewh]

btrueblood,

I agree with most of what you have posted. I disagree that the definition of t.p at 1.3.36 takes precedence over the statement in 5.2.1.3; 1.3.36 is only a "basic" definition, while 5.2.1.3 expands on the definition and it's application. In the example fig. 5.2, I don't see where the bolt circle is controlled; rather the holes are controlled with ordinate dimensions, and the bolt circle is a reference dimension.

As for 5.2, I stand by my statement, as it was taken directly from the standard. It can be between interrelated features, but is a basic dimension.
It is my understanding that "appropriate datum references" refers to datums that can directly affect the feature, as opposed to datums refered to only by unrelated features.

As for your situation, I have approached similar cases by loosely locating only one of the holes in the pattern to the center bore datum, establishing that hole as a separate datum, and locating the other holes in the pattern more tightly to that datum.

You could define the bolt circle as a datum, but only as a reference for some separate feature. You cannot locate it relative to itself. That would be circular logic. The hole locations would be dependant on the bolt circle location, which itself would be dependant on the hole locations.

Good discussion!

 

[israelkk]

btrueblood

I think a better example will be a square thin plate with 4 holes. Let's assume a 100+/-0.5mm x 100+/-0.5mm square 1 mm thick having 4 "equally spaced" 10mm dia holes. Each hole is on the diagonal and is 10 mm apart from the closest two adjacent sides. Now, for the first any two hole two basic dimensions are given from the closest adjacent sides to the hole center. Adding four 80 mm basic dimensions between the center holes completely defines the basic hole locations.

I too agree with you that it is irrelevant to assign the plate sides where the 10mm basic dimension are taken from as a datum feature.

 

[drawoh]

btrueblood,

There is nothing in the standard that requires a datum for TP dimensions. To be pedantic about this, there is nothing in the standard that requires the TP to mean anything. Your hole must be positioned with respect to something for your dimension to be useful.

Do not think rigidly in terms of GD&T. Think in terms of somehow controlling the geometry of each feature you call up on your drawings. The basic dimension states that your dimension is exact and nominal. The geometry control is elsewhere, probably in a feature box.

If you do not do a basic dimension, the feature is controlled by your tolerance notes, and by rules elsewhere in ASME Y14.5M-1994.

If you do not have tolerance notes, basic dimension boxes or explicit tolerances, than you have an incomplete drawing.

JHG

 

[ewh]

drawoh, israelkk,

Why is it that there are no examples of true position callouts without datum references or basic dimensions in the standard? How difficult is it to label a surface as a datum?

What would be the point in using true position without basic dimensions? Wouldn't you control the feature better without the true position, defaulting to block tolerances?

Why would the standard include true position if it doesn't have to mean anything?

I still struggle to understand the validity of your points relative to the standard. I agree that many people use GD&T in various ways, and it may work for them, but are those methods legitimate per ASME Y14.5M-1994?

I guess I am getting confused by your comments. Apparently using the standard causes more confusion and misunderstandings than not using it (for geometric control). No wonder it costs more to fabricate a part defined with GD&T than it does without.

Is there anyone reading this forum that has had formal training on this standard?

 

[btrueblood]

Israelkk,

I think I'm following your logic - two bolt holes and the line between their centers defines one datum? According to the logic by ewh, and in 5.2.1.3, you would "have to" define the part edge as a datum, since your basic dimensions reference that edge.

My problem comes here - ewh says: "You could define the bolt circle as a datum, but only as a reference for some separate feature. You cannot locate it relative to itself. That would be circular logic."

I would agree with that statement, thus my conclusion that in the case given, no datum is required: just the basic dimensions (the diameter of the bolt circle and the spacing between the bolts) are sufficient to locate the bolts in the desired pattern. To inspect the part, a gage plate would be built, with the pins at LMC located on the bolt circle and spaced at the appropriate spacing. The gage plate does not need to engage any other feature than the bolt holes in the pattern, the inspection criteria being "do the pins go into the holes without interference?" No datum needed or wanted, none used.

By locating a single hole, ewh, you effectively constrained my problem - the other bolt holes are now located using one hole as a datum. I can see how this would work, but wonder why I can't just locate the bolt circle using standard dimensioning, and then control the positions of the holes relative to each other with a tp tolerance block...

drawoh says: "There is nothing in the standard that requires a datum for TP dimensions. To be pedantic about this, there is nothing in the standard that requires the TP to mean anything. Your hole must be positioned with respect to something for your dimension to be useful."

Um, I hope I'm not being pedantic. Maybe I am. If I am, say so and I'll shut up and go away.

But to reply to your last sentence, I'm not talking about a single hole but a collection of holes (a bolt pattern). The point I'm trying to make is: the basic dimensions control the location of the bolt holes relative to each other. No datums are required for the definition of these relative positions (see figure 5-1 of the standard). As long as I know and understand that the position of the bolt holes (the pattern), _relative to other features_, is not controlled by this, I can draw the feature control frame without reference to a datum. Is what I'm trying to define understandable, or does it make inspection impossible or difficult?

 

[drawoh]

ewh,

I have taken an official course on GD&T, based on ASME Y14.5M-1994.

I regard the relationship between basic dimensions and datums to be very simple. I think much of our problem here is getting people to think through GD&T from first principles. I think that the fundamental problem is that people are thinking of basic dimensions as having +/- tolerances. The whole beauty of GD&T is that it defines the actual geometry.

If Israelkk,'s plate were my drawing and I were to systematically use GD&T, the drawing would work ss follows...

- Datum A would be the bottom of the plate. Datums B and C would be adjacent edges of the plate.

- The rectangular plate would be dimensioned 100mm by 100mm, basic dimenions.

- There would be a profile tolerance around the outside of 0.25mm with respect to A, B and C.

- The 10mm diameter holes would be in a pattern 80mm by 80mm centre to centre. I do not see the logic of dimensioning from the outside edges.

- I would apply two positional tolerances to the holes. There would be a 1mm tolerance with respect to A, B and C. There would be a 0.5mm tolerance with respect to A.

These positional tolerances control the pattern so that the holes will fit accurately to four mating holes. The outside edges of the plate are located less accurately.

If I did the same plate using +/- tolerances, I would take all the dimensions from two adjacent edges. Two sets of holes would be 10mm from the edge +/-0.15mm and two sets would be 90mm from the same edge +/-0.15mm. The length and width would both be 100mm +/-1mm.

In both cases, I have solved the problem of locating the holes accurately enough to put screws through. The linear drawing of a machined part probably required less thought on my part. The GD&T drawing allows more error without impairing the functionality of the part.

You have to think differently to use GD&T.

JHG

 

[ewh]

drawoh,

Thanks for the clarification. I agree with your entire post. I have not taken any "official: GD&T courses, but when I worked with an excellent (IMO) company, MOOG, the entire engineering department was given a full two week course on the subject. They approached it much as you do; establish the primary, secondary and tertiary datums as well as any incidental datums, determine the accuracy required and relative to which datums, and apply the principles of the standard. At the time, I had a firm grasp on the reasoning behind the practices. Tolerance the part as it is to be inspected, and eliminate any assumptions.
Since then I have spent many years as a contract worker, and have been exposed to some atrocious practices in regards to the standard. I have to frequently read up on it to determine what is legit and what is not. And I am still looking for those slippery "implied datums".

 

[btrueblood]

ewh,

If you want to find implied datums, look at the 1973 version of the standard. Implied datums were eliminated in the 1982 standard.

In regard to the 1982 standard, however, there is a clearly labelled chart in the "Drawing Requirements Manual" by J. H. Lieblich, which explains where and when datums and basic dimensions are REQUIRED. Position tolerances clearly (in 1982) did not require datums; they did require basic dimensions.

I agree with your reading of the standard, in that it appears that position tolerances now appear to require datums. I wonder why, and have given you an example, but in no way do I mean to imply that I would not use basic dimensions to define a bolt pattern. Just that the basic dimensions would apply between the features of the bolt pattern, and not refer to datums. In MY example, I don't give a damn about the boundaries of the part - just the locations of the bolt holes relative to each other.

By the way, to make sure we are talking about the same thing, when I say "bolt circle" I am referring to a circle, shown as a centerline, defined by a basic dimension that includes a diameter (or radius) symbol. The bolt circle, and a "equal spacing" callout, or a basic angular dimension, shown drawn through the centers of a group of bolt holes, is sufficient to define what I call a bolt pattern. My questions are in regards to the location of said holes, relative to each other, within the pattern.

For what it's worth, I have copies of, and have read through, and have received formal training to the following:

ASME Y14.5 - 1973, received formal training from an aerospace company (for which, by the way, we purchased parts from MOOG, and I have my own opinions about that company, mostly good) for this standard, which training had been updated for the 1982 revision.

ASME Y14.5 - 1982

ASME Y14.5-1994 (recently purchased, and no, I'm no expert in this version, thus my questions).

 

[ewh]

btrueblood,

Thanks for the explanation. As I stated in my first post, I was refering ONLY to the 1994 version. Your points are valid for the previous versions.

I'm sure not looking forward to the next release!

Eric