yang686526

how does y14.5 call out through holes
i have a part i am working on that is .250 thk aluminum. the problem i have is that when i pierce the hole i am out of the general tolerance on the bottom due to the blowout. my customer wants to reject this, the print is interpreted using y14.5m-82. how would this be stated on a print that the hole size must be in tolerance all the way thru or is it assumed that the holesize must stay within the general tolerance block.
what is the holes size and tolerances? also, what is the manufacturing process used to create this part?
heckler
sr. mechanical engineer
swx 2007 sp 3.0 & pro/e 2001
xp pro sp2.0 p4 3.6 ghz, 1gb ram
nvidia quadro fx 1400
o
_`\(,_
(_)/ (_)
(in reference to david beckham) "he can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. apart from that, he's all right." -- george best
if i'm understanding the op correctly, by default the tolerance applies all the way through the hole.
unless there is some other drawing note or annotation that relaxes the tolerance over specific sections i'm inclined to think your customer is right. for example if there's a note ro remove burrs/sharp edges by chamfer or rad of certain size, and you fall in this limit, you may be ok.
if what you are actually producing is functionally acceptable, just doesn't meet drawing, then the drawing could perhaps be revised to allow it.
however, i haven't worked with y14.5m - 1982 only newer version and uk specs.
heckler
the hole is a .375 +/- .010 hole. through .250" inch aluminum. on other customer drawings i have seen it noted as a thru hole. the hole is being created by using a punch press
explicitly saying 'thru' makes no difference on your tolerances etc. it's just to clarrify that the hole goes all the way through, especially when it wouldn't otherwise be obvious.
the hole should be .375 +-.010 all the way through.
although you can accommodate the manufacturing process by applying tolerance in their favor, but manufacturing methods have nothing to do with gd&t.
they can hand carve it if it meets your requirements.

stick to your guns if that is the requirement and let them laser cut the hole or drill it.
he may have a 'punch to die' clearance problem that he is unwilling to fix.
cheers
i don't know anything but the people that do.
i would agree with the others. if the process being employed doesn't allow the part to met the spec, then the process needs to be changed, a different process used, or the custom can make adjustments to the spec. as far the parts already made, if they don't match the print and then they are rejectable.
matt
cad engineer/ecn analyst
silicon valley, ca
i agree.
it's up to manufacturing to follow specs and make the part per print.
chris
solidworks 07 3.0/pdmworks 07
autocad 06
asme y14.5m-1994, paragraph 1.4(m) states; "unless otherwise specified, all geometric tolerances apply for full depth, length, and width of the feature."
unless you've indicated an exception to this fundamental rule on your drawing, the tolerance applies to the entire length of the hole.
gdtguy
gdtguy,
the paragraph you specified was an addition to the standard between 1982 and 1994. it didn't exist in the 82 ansi standard. in ameristarqa's original post he said the standard specified was the 1982 which would have been the ansi standard as they were the ones controlling it back then. asme only took it over starting with the 1994 standard. the paragraph was added to clarify exactly this issue.
ameristarqa,
regardless of whether or not this exact situation is addressed in the 1982 standard. the implication has always been that the tolerance applies for the entire length of the feature. i think kenat had some good advice to suggest that if the part is still functional then try to get the drawing revised to reflect the looser tolerance. if it won't work as it is, then you should change your process to produce a hole that is in tolerance (i.e., drill the thing).
powerhound
production supervisor
inventor 11
mastercam x
smartcam 11.1
ssg, u.s. army
taji, iraq oif ii
hey guys:
stampings are different. it is understood in the industry that the tolerance is at the "cut" and not the "break" and this situation is not covered under the standard.
one should never see profile of a surface on trim but profile of a line at the "cut".
in a stamping industry when blanking or piercing, the "cut" is approximately 1/3 the thickness of the material and the other 2/3 breaks off. the break, by and large, is uncontrollable.
dave d.