Hole Position Usage 2

[lecuyero]

I have been following this forum for a few months now and thought I had a basic understanding of GD&T. I have a book as well and have read it cover to cover. We had a drawing review session last week and one of my drawings came up for question. The other drafters picked out my GD&T and marked it up.

There are 2 issues that I need clarification about. I thought you could declare positional tolerances with 1, 2, or 3 datums (or 0 but bad things can happen). In my drawing the relationship of the holes to the edges of the surface is not important. To save manufacture cost I did not call out the other datums. My book says this is OK to do but my colleagues do not. Which is correct?

Second issue is regarding projected tolerance. Am I missing something or is this correct usage of projected tolerance? The part that mates up to this part is 1" thick and the holes are .266+.003 and have a positional tolerance of 0.005

http://files.engineering.com/getfil...eb0-4f54-8c83-4411e80c95c6&file=gdt_usage.JPG

 

[powerhound]

If the hole pattern MUST be a datum then attach the B datum identifier to the FCF and position the holes relative to A only. The only problem is that if you are identifying a B datum then you should probably locate something relative to it. The only thing I see is the outside profile, in which case you will need to use "Profile".

Is there a problem with making the long edge B and the short edge C, then positioning the holes (using basic dimensions) to A, B, and C? I You can use a composite tolerance with .020 in the top section located WRT A, B, and C and then in the lower frame put .008 WRT to A only. That will more tightly control the perp AND the distance between the holes but leave the pattern itself to be free to wander within the .020 tolerance zone.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[SeasonLee]

Happy New Year to all who loves GD&T.

Lecuyero

On your latest post, the 1st drawing is incorrect. If you are using pattern as a datum feature, be sure attach the base of the datum feature symbol to the FCF (hanging from the FCF) as shown on your 2nd drawing, you can’t just directly adhere to a hole feature. Besides, secondary datum B should be removed from FCF.

The 2nd drawing is correct except the secondary datum B should be removed from FCF, the 2 threaded hole is a pattern and used as secondary datum, so can’t use itself as a reference datum. However, you need this datum if there are other features relative to the secondary datum (pattern). Fig. B on my attachment is a good example for your reference---when to use a pattern as a datum.

Fig. A is the recommended callout for your case, of course you may choose composite tolerance as an alternative method, but I prefer to the projected tolerance zone since it is an easy way to meet your design intend, a simple case. Do not complicate a simple issue.

SeasonLee

 

[dtmbiz]

PowerHound,
What you have posted in reference to requirements regarding positional tolerancing is in complete agreement with what I had posted. I believe because there are no basic dimensions or datum references relating the edge surfaces to the holes, then this cannot be a correct positional tolerance accoding to the standard. I believe yourself and others then go further to say the original drawing is incorrect.
There’s where we part paths.

You say logic cannot be used to eliminate the true position possibility and consider the edges being located from the hole(s) center. It is true that the hole FCF is legal to control the holes perpendicularity and distance to each other. It is true that features of size can be dimensioned legally according to the standard without using positional tolerancing. Dingy2 says that the holes are being positioned from the edge as a pattern. I disagree with that opinion because there would be a mix of a rectangular tolerance zone and a cylindrical tolerance zone. I see this as problematic.

I have never said that the original drawing was the best way to define the drawing as shown. I simply say that it is NOT illegal according to the standard and go on to give examples from the standard to support my position. SeasonLee’s last post simply claims the drawing is incorrect with nothing that I see supports that opinion based on the standard. If it’s there, then please show me.

The following examples from the 1994 standard illustrate dimensioning to holes without the use of “positional tolerancing”. Without the use of the “origin symbol” whether or not the dimension starts from the edge or hole is a matter of interpretation. There is nowhere in the standard that states positional tolerancing with a cylindrical tolerance zone is mandatory. BTW I personally believe the positional tolerancing “is” the best way to go.
pg 6 fig 1-4; pg 7 fig 1-6; pg 9 fig 1-14; pg 10 fig 1-18
Rectangular Coordinate, Baseline, Polar Coordinate dimensioning
pg 19 fig 1-48, 1-49; pg 20 fig 1-50, fig 1-51

 

[powerhound]

dtmbiz,

Your examples are completely out of context of our discussion. We are discussing tolerances of postion and your examples are specifically about what dimensions and leader lines are supposed to look like and how they are placed. The standard provides examples to illustrate the point being made and some are incomplete by intent. I'm not even sure what point you were trying to make by providing them. I know how dimension lines are supposed to look and how they are placed.

That being said, I think I had the wrong impression of what your position was on our topic. I've been under the impression that you thought it was okay to use +/- dimensions to position a feature using a true position callout and FCF. From reading your last post I don't think that's what you were trying to say. Were you?

I do see what you're saying regarding the edge being located from the holes instead of vice-versa and this is why this print is technically illegal because it violates 1.4(d) of the standard. It can be interpreted in more than one way.

Regarding the logic, nothing can be left open in GD&T. I know of a legal case where logic was pitted against what the standard said and the standard won in court. It was the reason that "Spotface" got its own symbol in the 2009 standard.


Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dtmbiz]

PowerHound, Seriously? Figs are out of context?

Quote;
"If these words aren't enough to convince you then there's really nothing left...maybe you can show me a place in the standard where it says features can be positioned using non-basic dimensions, and maybe I'll become a believer"

These are references to dimensioning "without using basic dimensions". Or maybe this is one of those "logical" times to ask for your definition / context as to what you mean by "positioned"? Maybe I'm not understanding you?

Rectangular and Polar Coordinate, Baseline dims. If you read the corresponding paragraphs it clearly states that these types of dimensions can be basic or non-basic. Is your opinion that if a standard uses a fig to focus on let’s say broken extension lines; that the rest of the fig is erroneous; not to standard, even though it may not be complete? If you place the ASME Y14.5 reference on a drawing format, you can dimension the entire drawing without basic dimensions nor FCF's of any kind and still comply with the standard.

Quote:
"That being said, I think I had the wrong impression of what your position was on our topic. I've been under the impression that you thought it was okay to use +/- dimensions to position a feature using a true position callout and FCF. From reading your last post I don't think that's what you were trying to say. Were you?

I was not suggesting in any way to use +/- dimensions for a proper "positional tolerance" call out. You are correct that we are in agreement to use basic dimensions.

As far as 1.4(d)..... good luck.... just re-read this thread and how many others with all the various interpretations. I am not saying this is wrong, however for those that oppose using the standard, this is one of the standard's fundamentals that is used to advocate not using the standard. In light of this I have been thinking about what the intent of this paragraph is. It is obvious that in many cases using coordinate dimensioning and not using the origin symbol, many dimensioning schemes would be subject to more than one interpretation. I wonder if this paragraph is aimed more at the interpretation of what feature is being dimensioned. For instance that a feature be clearly dimensioned to an intersection, tangency, or center point (axis). Or maybe "one interpretation" as to what datums are being defined. I'm not really convinced myself on this one, however if 1.4(d)were applicable to all callouts "in the real world", then I don’t think this forum would exist.

I would be getting off topic to write more about my point of view on logic. Where is the standard for subtraction and addition to calculate virtual conditions for example? Or any other math calculation for that matter. Where is it in the standard that we use for instance the word "parallel" in the context of geometry and not "a parallel conversation"? Where in the standard does it mandate the formula to choose a profile callout let’s say, other than a positional callout? Where in the standard does it state exactly what order of precedent the DRF datums should be in? I'm fairly certain that you won’t see that these are relevant examples either. That's Ok with me, hopefully, we'll just agree to disagree.

As for the case you sight, where can I read about this spot face controversy? I do not think the standard(s) are flawless.[\b] Humanoids are involved.

Back to the OP and my assertion that the original drawing is legal. Since you bring up a court of law in the US, then I shouldn’t have to remind you that unless one is proved to be found guilty according to a particular law; then I will continue to assert that this callout is legal until I see a convincing argument that sites the standard proving it is not legal.

That's my story and I am sticking to it...

 

[axym]

Very interesting discussion. I haven't had time to jump into this but I will now. Here are some thoughts:

I would say that the original drawing is compliant with Y14.5. The Position FCF obeys the rules - the relationships between the considered features and the datum features are all basic. There are explicit basic dimensions for the hole spacings, and implied basic 90 degree angles for their orientation relative to datum A.

Fundamental Rule 1.4(d) is a very big can of worms, and worded in such a way that it cannot be meaningfully applied. It's difficult to say what the original intent of this rule was - I think that dtmbiz is right that it was probably something to do with clearly defining which feature(s) a dimension applies to. If one goes beyond that and looks at how dimensions can be defined on a real (i.e. imperfect) part, then 99.9% of drawings violate Rule 1.4(d). Other than size tolerances on regular features of size (cylinders, spheres, slots), directly toleranced dimensions (a.k.a. plus/minus tolerances or coordinate tolerances) are ambiguous on real part geometry. There are no rules on how to define directly toleranced dimensions on a real part, so they are fundamentally subject to more than one interpretation. Yet Y14.5 allows them, describes them, and provides many examples of their use.

So the directly toleranced dimensions on the original drawing are legal, but not without problems. Their meaning is clear on a drawing or model, but ambiguous on a real part in which the holes are not perfectly round and the edges are not perfectly flat and square. Which is every real part, so there is always some ambiguity. This used to drive me crazy, and I was an advocate of limiting the legal use of directly toleranced dimensions to simple sizes only.

But I eventually realized that directly toleranced dimensions have their place, because there are many applications in which they are used successfully. Directly toleranced dimensions go along with a simplified approximation of the part geometry, in which the features are assumed to have perfect form and perfect orientation. In situations where the form and orientation error of the features is small in comparison to the size and location tolerances, directly toleranced dimensions can be the lowest cost option. The overall savings gained from simple dimensioning and simple inspection can outweigh the costs of multiple interpretations. Geometric tolerancing is the tool of choice if you need things to be fully defined, but sometimes the quick-and-dirty approach ends up being cheaper.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[dingy2]

Evan:

You certainly have changed your original thinking.

I absolutely agree with you that one could apply directly toleranced dimensions on a drawing where there is no function and mating relation while the geometrical applications could be applied to fully describe the design intent where there is a need.

I realize that you, MechNorh and I have had some "intense" discussions in this area in the past but the standard reflects origins without the application of GD&T.

Dave D.

http://www.qmsi.ca

 

[axym]

Dave,

I may have softened my stance on directly toleranced dimensions, but I'm not ready to admit that I agree with you yet ;^).

I still don't agree with the rule of thumb that directly toleranced dimensions should be used when there is no functional or mating relationship between the features, and geometric tolerancing when there is. All features on the part have a function and dimensional requirements that go along with it, otherwise the feature wouldn't have to exist. The requirements may be very loose but they are there, and geometric tolerancing would always be capable of giving the largest tolerance for manufacturing while meeting the functional requirements. But in many manufacturing situations the extra tolerance cannot be taken advantage of, and does not result in a significant cost saving. In these situations, the complexity of GD&T ends up not being worth it. The simplicity of directly toleranced dimensions wins out, even though it gives away some tolerance and makes borderline parts very difficult to evaluate. Many companies are willing to live with these headaches, or avoid them by not making parts that approach the limits. Simple inspection can definitely be bought by making parts with very good form.

I do agree with you that the standard has its roots in directly toleranced dimensions and gradually added geometric controls to the tool set. Users have found that there are many applications where directly toleranced dimensions are "good enough" and other applications where they are not.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca