huangyhg

thru hole dimensioning in deep part
really need help with this.
i have a cube that is eight inches square. there are four holes to be drilled through the entire depth of the part and the centerline of the holes are dimensioned only on the top view. the holes are 1/4" diameter. there is a drawing tolerance of +/- .010.
the hole pattern dimensioning uses no control boxes, neither does it have any requirement for perpendicularity, celindricity, parrellism, etc. all that is shown is the distance to the first hole from the part edges and the center-to-center location for the hole pattern.
the part was manufactured by a outside shop. where the holes exit the part on the "bottom" they do not fall within the drawing tolerance as measured from the edges at the bottom of the cube.
i contend that the drawing does not control the exit hole locations and so our inspection department should not flag this as discrepant.
my question is this: what controls the exit hole tolerance for thru holes drilled through thick parts when the holes are dimensioned on a drawing only on the "entrance" view of the hole?
without the benefit of a specific standard, such as y14.5, there is no clear cut definition of the allowables.
imho.
to me, the use of "thru" would indicate that the entry hole positions and the exit hole positions are required to have the same tolerance. but as noted above, if there was no use of gd&t, the tolerances are open to interpretation.
a good shop would have drilled 4" and rotated the parts for the other 50%.
"art without engineering is dreaming; engineering without art is calculating."
the tolerance of its size is for the whole length of the hole. asme y14.5m 2.7.1.1 states "the actual local size of an individual feature at each cross section shall be within the specified tolerance of size."
to fix this, it might be useful to use geotol's to actually loosen the specifications.
matt lorono
cad engineer/ecn analyst
silicon valley, ca
i disagree with that blanket statement mango. that would be the correct course of action if the holes were for alignment like a coupler or something where 2 coaxial sets of blind holes would have worked, but if the purpose was to run a single .250 shaft all the way through the hole then that method would not work because there would be a mismatch in the middle that would prohibit it.
the drawing is definitely open to interpretation in the absence of any specified standards. in my opinion, a good shop would have known that a drill bit over 8" long was going to walk and they would have either asked about the importance of the exit hole or they would have taken measures to prevent the hole from walking such as center drilling, then drilling with a jobber length bit, then a standard length, then maybe go back through with the full length drill bit. this shop very well may have done all this but it still didn't work out.
powerhound, gdtp t-0419
production supervisor
inventor 2008
mastercam x2
smartcam 11.1
ssg, u.s. army
taji, iraq oif ii
if i were actually intending to put a shaft through the hole, and the location at both ends was important, i'd specify the hole location tolerance at both entry and exit, and i'd probably draw the holes with a 'bottle bore'.
bottle bore: the central 3/4 or more of the length of the hole is drawn enlarged, i.e. with a diameter larger than the diameter of either end of the hole, with a tolerance loose enough to allow drilling from both ends with a little mismatch at the intersection. actually making a bottle bore is possible, but probably not easy at that size, so i might add a note that gundrilling the entire hole to size would also be acceptable... and i'd expect most machinists to just use a stock gundrill.
in the extant case, it sounds like you're obligated to buy the parts even if the distal ends of the holes come out of the corners, since you didn't specify otherwise.
mike halloran
pembroke pines, fl, usa
being a cube, how do you know which 4 holes are exit holes?
depending what the part is used for and if it mates with others, i would use gd&t (projected tol on the holes or...?)
for a length of eight inches, call out the hole size needed per it's max depth on both sides, another size between the two holes.
i can't say for sure without knowing the part.
chris
solidworks 08 0.0/pdmworks 08
autocad 06
thanks to everyone for the quick replies.
it sounds like, as ringman said above, "without the benefit of a specific standard, such as y14.5, there is no clear cut definition of the allowables." the drawing does not call out any standard.
the drawing is not very old, and came from a well-known entity. our inspection department flagged the exit holes as non-conforming (though the deviation is minimal even by their interpretation of the design requirements). my position was that the drawing fails to control the exit hole locations (and now i'll add, fails to state any controlling standard), and consequently there is no criteria against which the exit locations can be checked.
this part bolts to another part with a matching threaded hole pattern. i know the "intent" of the designer was that the exit locations match what is shown for the entrance. and i feel confident the part will work as intended, as is. but, whereas this is a technical issue, subject to interpretation, i still must convince inspection that the part conforms to the drawing. the points made here are very helpful. thanks again for all the help.
i would have to agree with ringman, if their is no callout on the drawing such as "interpret all dimensions and tolerances per asme y14.5m-1994" then you really get what the machinist decides to give you.
heckler
sr. mechanical engineer
swx 2007 sp 4.0 & pro/e 2001
o
_`\(,_
(_)/ (_)
this post contains no political overtones or undertones for that matter and in no way represents the poster's political agenda.
carelessness on multiple fronts:
as mentioned, no standard, no perpendicularity, etc.
what manufacturing genius ignored the fact that the holes were so deep as to almost guarantee that the drill would wander?
if exit location is that important, why not spell it out?
honesty may be the best policy, but insanity is a better defense.
ringman pretty much covers it, the drawing is effectively incomplete.
if 14.5 were invoked it would be as fcsuper points out.
i don't think rejecting the part can be justified as the drawing is incomplete, unless there is some workmanship standard etc. invoked on the contract somehow.
kenat, probably the least qualified checker you'll ever meet...

__________________
借用达朗贝尔的名言：前进吧，你会得到信心!
[url="http://www.dimcax.com"]几何尺寸与公差标准[/url]