True position interpretation 2

[Dyskolos]

Hello,

I have a drawing that I am having trouble interpreting and was hoping that someone here would be willing to provide a sanity check for me.I have attached a drawing with the pertinent dimensions*. The drawing is intended to be interpreted per ASME Y14.5-2009. My concerns are as follows:

1. The 2x Ø0.375 holes call out a true position to A and B. This seems ok to me, except that there are no basic dimensions to go with this true position. Seems like the Ø8.500 B.C and 45° should be basic, correct?
2. The drawing calls out a true position for the Ø8.500 B.C. It seems like this is intended to locate the Ø0.375 holes, but those already have a true position called out. Am I looking at this wrong?
3. I am unclear if the Ø8.500 B.C. with the true position callout applies to the 1/2-13 tapped holes or not. The drawing would seem to indicate not, since the callout for the threads calls out a Ø8.500 B.C. on its own.
4. Anything y'all see?

*I cannot upload the actual print due to confidentiality agreements. The attached print also has modified dimensions and tolerances compared to the original, but should suffice as an example. This drawing does not include all dimensions, just the ones I thought pertinent. Please let me know if you believe that I failed to provide any necessary info.

 

[Belanger]

The position tolerance of .001 isn't following the rules of GD&T -- not only because the holes it's trying to position are already controlled for position, but simply because you can't position a bolt circle. (It's not a "feature of size.") So it's just plain wrong, even if the position of .0005 weren't there.

All the GD&T is applied in the section view, so nothing seems to be controlling the position of the threaded holes.

So basically your hunches are correct.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[pylfrm]

Dyskolos,

First, a clarification: The term true position refers to a theoretically exact location established by basic dimensions. The tolerance is called a position tolerance or positional tolerance.

Responding to your concerns:

1. The diameter 8.500 +/- 0.001 B.C. dimension should instead be diameter 8.500 BASIC. A center line should probably be shown along the axis of the part to imply symmetry. The 45° dimension does not affect the position tolerance at all because it is not involved in defining either the hole pattern itself or how the pattern relates to datums A and B.

2. The position tolerance on the diameter 8.500 +/- 0.001 B.C. dimension is invalid. Position tolerances can only be applied to features of size, which this is not.

3. I agree that the 8.500 +/- 0.001 B.C. dimension refers to the 2X diameter 0.375 holes only.

4. There's plenty more room for improvement on the drawing, but you just asked about interpretation so I'll leave it at that.


- pylfrm

 

[Dyskolos]

John-Paul,
Thank you for confirming my suspicions.

Pylfrm,
I appreciate the lesson in terminology. As I am sure is glaringly obvious, I am not formally schooled in GD&T.

Once again, thank you both. I will pursue this with our customer to find out what it is that they actually want.

 

[mkcski]

Dyskolos,

Besides agreeing with everything already stated, let me add my two-cents. The selection and precedence(sequence)of datums should be determined by functional and fit-up relationships of feature(s) on the part. Your drawing "smells" of something amiss. But the Forum "team" cannot expand on this unless you share how the part "works".

 

[drawoh]

Dyskolos,

Take a look at the ASME Y14.5 standard. There are several examples of pitch circles. The normal way of showing this now is to show the circle on the end view, with the diameter marked as a basic dimension. The 45[°][ ]angle also is a basic dimension. The true position tolerances are applied to the holes only, as noted above. This presentation is clear and simple, and nobody phones or emails to ask you what B.C. means.

--
JHG

 

[Dyskolos]

Mkski, I understand your comment, but it is not my (or my company's) design and I can only make educated guesses about the part's function. My inquiry was limited strictly to interpretation.
Please also note that this is a severely abbreviated drawing; I included only the dimensions and features I thought required scrutiny. It is possible that I am being overzealous with confidentiality here, but I prefer to err on the side of caution.

Drawoh, Yes, that is how I usually see it, and how I do it when I create a drawing. I merely wanted a sanity check, because I consider it important to never forget the possibility that I could be full of it.