Depth of cross-hole

[cbrf23]

So I have this blind hole which runs into another through hole.
We are doing root-cause analysis on why a drill went too deep (into the back side of part, almost through) and it wasn't caught.
I observed there was nothing in the inspection plan that required any verification of the depth of the blind hole, to which I was challenged that there was nothing on the print that defined the depth of the hole.

This is interesting to me. We specify prints are to be interpreted per ASME Y14.5-2009, so I went back to that, and couldn't find anything that spoke directly to this situation.
The print calls the hole exactly like the simplified drawing below (i.e. 3.000±.015 typical).

Now, it's my interpretation that the 3.000±.015 dimension controls both the distance from the identified face to centerline of the cross hole and the depth of the blind hole (as marked up below).
However, our quality department seems to disagree with this. They interpret it as only controlling the distance to centerline (just "1" in the mark-up below), and say this dimension does not control the hole depth. When questioned about how they would like the part dimensioned differently to specify hole depth, they don't have an answer, as they agree there's no additional dimension to add (it would just be the same dimension a second time).

So my question is, how would the rest of you interpret it, and how to best define the two requirements? Would you add a hole depth callout?

 

[JNieman]

I would never have thought that 3.000 +/- .015 applied to the depth of that blind hole.

Which, btw, I wouldn't consider a blind hole at all. It's a "thru to bore" hole.

Your "typical" is exactly why it's sometimes unwise to use "typical" - I don't think it would apply like you say, at all. The dimension is locating the center-line of the cross hole. That in no way is related to the depth of the intersecting hole - especially when the intersecting boss remains undimensioned. To me, it's an incomplete print. I would never start applying "typical" dimensions as I saw fit until the part was fully defined.

I would call out "Thru to bore" as the hole depth, and possibly (if necessary) a depth-to-centerline dimension as a reference-only. The requirement is that the hole completely intersect the bore and no further. Not that the drill goes to a certain depth (118, 90 or 135 degree drill? Answer: not my problem )

 

[KENAT]

TYP isn't supported by ASME Y14.5 94 or 2009 edition to best of my knowledge. You should use explicit number of times e.g. 2X. I would not interpret it how you are.

Similar to JNieman I'd normally dimension as 'through to XX dia hole' or similar - or if showing the cross section there is an argument you don't even need a depth stated as it's clear from geometry.

Sometimes I'll put a depth with a loose tolerance that ensures a full intersection but I prefer just the above.

Posting guidelines faq731-376

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

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

 

[CheckerHater]

I'v seen quite a few drawings in my life, but I'd never interpret 3.000 as a depth of blind hole.

Your drawing has important advantage - the geometry is perfectly clear from the section. Just keep it this way. Also, adding vertical 3.000 dimension wouldn't hurt.

Also (as a splash of kerosene), my impression was that "thru to bore" is supported equally well as "typical". Am I wrong?

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[cbrf23]

Thank you gentlemen!
Reflecting upon my own intepretation I have to say, I think I was really considering the graphic depiction (section view) to imply the drill was to go to bore and not beyond. I think I was attributing this to the dimension when looking for a way to explain my intepretation, which was wrong, and may have served to further the consternation.

I think I'll suggest changing print to something like this:

 

[KENAT]

Is'nt it only 2X 1.500? Even though it gets interrupted on the top side?

The 3X 3.000 isn't very clear what features it applies to.

For features of size, you should normally use position tolerance (unless working in 2009 changed).

Posting guidelines faq731-376

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

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

 

[3DDave]

The problem with this design is that it requires the holes to intersect perfectly; there is no allowance for the amount the intersecting hole can be offset from the through hole. Worse, the diameter of the holes at the intersection is not defined as neither is a full diameter, which is aggravated when the intersecting hole is off-center.

At best you can specify the minimum depth a full diameter pin can be inserted in each direction and note that there not be any wall defect/ loss of wall thickness due to processing. It would also be much easier if the intersecting hole was smaller diameter and had a position tolerance smaller than the difference in diameters so that the worst case might be a shared tangency.

 

[cbrf23]

@3DDave - Good points. This is a legacy design we're working with, so not even sure what type of allowance they have for that. The manufacturing process just runs the same program, rotating the part orientation in fixture (so all three sides are machined same way). I know on some of the more modern elbow designs they surface the intersection with a ball mill - but I don't believe there is any blend step here.