How does Y14.5 call out through holes

[AmeristarQA]

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.

 

[Heckler]

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

 

[KENAT]

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.

 

[AmeristarQA]

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

 

[KENAT]

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.

 

[thundair]

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.

 

[fcsuper]

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

http://sw.fcsuper.com/index.php

 

[ctopher]

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
ctopher's home (updated 03-13-07)

 

[GDTGUY]

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

 

[powerhound]

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

 

[dingy2]

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.

http://www.qmsi.ca

 

[fcsuper]

dingy2,

I realize the process controls how the part is formed, but the ASME Y14.5M standard controls how it is documented. If the process intended does have such limitations, then the drafter can take this into account in the drawing, without getting into the detail specifying the process.

It seems from your statement that you have experience in this area. If you would, I highly suggest you address this issue with the ASME so that the standards can reflect the scenario you suggest. Are there ASME standards that cover the stamping process which could be used to back up any corrections needed to the Y14.5 standard?

Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA

http://sw.fcsuper.com/index.php

 

[powerhound]

As I said in my previous post. The 1982 standard was ANSI and it did not address the situation at hand. ASME has covered the base with it's addition of (m) to para 1.4 to the 1994 standard; so with respect to that standard, there is really no question. All the draftsman has to do is specify the hole size and tolerance without specifying the manufacturing method. The manufacturing method is up to the shop doing the work. They should use a method that produces the desired results. If stamping doesn't produce a hole that is in tolerance then the hole shouldn't be stamped. That being said; the issue you have is that the print is specifying the 1982 ANSI standard which made no provision for this situation. Did the print specify that the holes be punched? If so then we're into an entirely different discussion. If not then I would tend to lean towards your customer's contention that the parts be rejected...sorry.

Powerhound
Production Supervisor
Inventor 11
Mastercam X
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[fcsuper]

Powerhound,

Yup! This is ultimately correct. Besides that, the only criticism I have for the customer is to not use 1982 standards anymore. Vendor is responsible, but their out could be that the customer is using an outdated standard that doesn't address the issue...something like customer's fault for specifically employing a standard that doesn't address the issue.

Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA

http://sw.fcsuper.com/index.php

 

[KENAT]

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.

Apparantly it's not understood in the industry, or at least not all of it, or this post wouldn't have been made.

Even if it is "understood in the industry" there should still be some kind of reference to this on the drawing to make it clear. Otherwise the situation as in the OP occurs. This goes for things like welds, threads etc. While various