Thru hole dimensioning in deep part 15

[Out0fSquare]

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?

 

[ringman]

Without the benefit of a specific standard, such as Y14.5, there is no clear cut definition of the allowables.

IMHO.

 

[MadMango]

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."

Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[fcsuper]

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
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[powerhound]

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

 

[MikeHalloran]

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

 

[ctopher]

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
ctopher's home (updated 10-07-07)
ctopher's blog

 

[Out0fSquare]

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.

 

[Heckler]

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.

 

[TheTick]

Carelessness on multiple fronts:
[ol][li]As mentioned, no standard, no perpendicularity, etc.[/li]
[li]What manufacturing genius ignored the fact that the holes were so deep as to almost guarantee that the drill would wander?[/li]
[li]If exit location is that important, why not spell it out?[/li][/ol]

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[KENAT]

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...

 

[MouseTrap]

With all due respect to everyone here, I don't think anyone of the respondees has this right.

ANSI 14.5 may not have been specified on the drawing, and whilst ANSI Y14.5 could have been invoked to enable less rigid manufacturing methods, that doesn't mean that the specification for the hole and its location is incomplete.

Outofsquare tells us the hole was specified as a THRU hole...a THRU hole...in case you haven't got it by now it was specified as a THRU hole.

That THRU hole (according to the drawing) is to be located a certain distance from two surfaces of the part. The hole location has been measured in reference to the two surfaces of the block and has been found to be out of spec.

 

[PaulJackson]

Mousetrap,

You are right! The drawing is as it is. The problems only surfaces when one tries to compare the part to it!!! Everyone that must deal with the contract... those that "designed function" engineering, "specified fit" CAD, "measured result" inspection, "predicted conformance" quality, "speculated cost" manufacturer or "expected performance" customer.... trust that apples are being compared to apples. Without constraints on the scrutiny the expected and actual conclusions tend to diverge.

Paul

 

[ctopher]

Has been located a certain distance from which two surfaces of the part? If not specified, how can it be out of spec?

Chris
SolidWorks 08 0.0/PDMWorks 08
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[desertfox]

Hi OutOfSquare

If the hole centres on one face are given and the tol is +/-0.01" then I would expect the entry and exit holes to fall within that.
If the hole needed to be tighter controlled then a squareness or position tol should have been specified from the appropriate face.
The parts should be rejected.
I would however make reference here to the unpractical situation of trying to drill a hole a 1/4" dia through a 8"
block.
From memory a rule of thumb about drilling hole depths is
8*drill dia.
I think that the holes were drilled from both sides which makes it a very difficult job to get the holes to meet without error.

regards

desertfox

 

[ringman]

Mousetrap,

Do you know of a standard that imposes the conditions that you state should be applied to the holes?

At one time I worked for a company that had its Standard of Acceptable Workmanship, which I think would have covered the hole positioning, even before Y14.5. But without some applicable standard, I think there is a definite problem.

 

[powerhound]

I see your point mousetrap, you are saying that the use of the word "THRU" makes the hole a 3D object instead of the 2D object shown on the print, and thus the tolerance applies to the entire object, top to bottom. The problem is that it is still an "interpretation" with nothing but good reasoning backing it up. What is good reasoning to you and me may not be good reasoning to others. Simply stating ASME Y14.5M-1994 on the drawing would have invoked the fundamental rules of GD&T and we wouldn't even be having this discussion.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dingy2]

I agree with DesertFox on this one. I would check the holes on both sides for the coordinate tolerance shown but would not check to see if the holes were straight, size and location only.

Using the word "THRU" may be more precise but if I did not see a depth of the holes somewhere, I would assume it would be thru.

Stating on the drawing "complies with ASME Y14.5M-94" does mean that GD&T rules apply including rule #1 but how many out there in industry really know the rules. There are only about 300 - 400 ASME GD&T Professional - Seniors and a similar number of Technologist and we still argue (discuss) GD&T in this forum.

Dave D.

http://www.qmsi.ca

 

[Out0fSquare]

My question was not whether it's practical to drill a 1/4" hole, 8.00 deep, to +/-.010, or whether feature control frames, positional tolerances and datums would make for a better design.

My real world question was: Using the drawing described, what's the permissible deviation for exit hole locations and how is this determined from a technical perspective? What I was looking for is, what STANDARDS can be relied upon in making any determination about how the part may be built? As pointed out above, the question begs another question: Deviation from what?

I appreciate Mousetrap's contrary argument because it forced me to re-evaluate my position. I needed some way to demonstrate the lack of enforceability of the "assumption standard". This has given me even greater confidence in my original conclusion.

Using Mousetrap's argument, the strictest interpretation is that: "The part is presumed symmetrical, and every feature must fall within +/-.010 of every other feature (point, edge or surface)."

Another, equally valid interpretation howerver is that: "The stated tolerance applies to every dimensioned feature through the thickness of the part relative to the respective feature's reference point, edge or surface (datum)."

The design has three views: Top, Side 1, and Side 2. Overall dimensions are shown on all three views. The design width, height and depth is 8.000. Hole locations are shown only on the Top View and are referenced from only the "sides" or "edges" (depending on interpretation). Drawing tolerance is +/-.010, with no angular tolerance given.

Let's look at this part from the side view. In this instance, the top surface is "Datum A". The right-most top edge (TE) is "Datum B". The dimension to the centerline of the first hole is 2.500 from Datum B. Distance to the second hole is 3.000 from the first hole. (right or wrong, it's the way it's drawn.)

Here's one way the part could be built (measurements shown represent possible tolerance extremes):


TE

|<------------------8.000----------------->

|<--2.480-->|<---3.010--->|<--2.510-->|
__________________________________ ___TOP___
|\ /| /| /|\ [A]

|<------------7.990~8.010------------>


(TE = Top Edge opposite Datum B. The solid horizontal line represents the top surface which is Datum A. The vertical and angled lines represent sides and hole centerline locations. At the bottom, shown are three possible locations for Datum B. The opening at the bottom of the triangles each represent .010.)

The sides may be out-of-square, relative to "Datum A," top-to-bottom, by +/-.010. Right?

From Datum B, the centerline of the first hole has +/-.010, left-to-right, and +/-.010, top-to-bottom. If Datum B slanted out at the bottom and the first hole slanted away from Datum B, this first hole could be up to .020 greater from its nearest bottom edge than it is at the top.

The next hole likewise has +/-.010, measured from the first hole, and also +/-.010, top-to-bottom (through the part).

The exit hole on the bottom left could be as much as .050 closer to its nearest edge than is the first hole from Datum B!

Some seem to want to argue that the right-most surface is the reference surface for the hole pattern, in which case it would effectively be "Datum A". If this is "Datum A", then how about the hole at the top-left which is .020 closer to its nearest edge. Out of tolerance? Would the part have to be made .010 smaller in order to hold both the overall AND hole-to-side tolerances?

What if the part tapers out on both sides at the bottom by .005, to 8.010. The overall dimension would be in tolerance, but you'd effectively reduce the exit hole tolerance to ".005" (I think I figured that right) relative to the two sides -- contrary to the stated tolerance!

If I'm seeing this wrong I'm still open to constructive, technical opinions, backed up with some empirical standard beyond assumptions.

 

[Out0fSquare]

In the third from last paragraph, I should have asked, would the part have to be made .010 larger in order to make the second hole fall within tolerance. And to reiterate, the drawings sets out no standard.