Significant digits on tolerance

[drum88]

Hi to everyone,
This is my first post, so apologies if this has been covered elsewhere (I did search FAQ's, but could not find anything relevant), or on the wrong forum.
We have a customer who wants to reject a brass semi tubular rivet that had an internal diameter call out of .019 - .021
Customer claims part measure .02104 - .02120 on the ID, and that the .021 stated is an absolute maximum.
Manufacturer claims parts are correct to print, citing significant digits, and that customer should not be measuring out to five decimal points.
Our company is stuck in the middle of this issue.
Given the nature of the part, and the very small oversize...is there a standard we can utilize to posssibly settle this disagreement to everyone's satisfaction?
Any views, opinions or further information is truly appreciated.

 

[meintsi]

Find a new manufacturer because they either don't have a clue or are feeding a big line of bu**sh**.

Limit tolerances are that, absolute maximum and minimum limits. No buts.



Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[rhodie]

"Significant Figures" or "Significant Digits" is a bad reference in the mechanical engineering/part print world. This expression acknowledges room for uncertainty in the value as stated.

ANSI 14.5 describes as a Standard all the expectations of a three-decimal tolerance. If the customer was critical to five decimal places, then they should have specified that going in, according to ANSI 14.5...

From where I'm sitting, the important issue here is which Tolerance Standard was agreed up when specifying the work. If the customer/supplier have differing standards, then somebody has hell to pay.

The rest of the field may help more here...

 

[rhodie]

...and I tend the agree with meintsi. The manufacturer should know better than that, unless they are a foreign source, or something equally as uncomfortable.

 

[tripleZ]

From the manufacturing perspective, what was the agreed upon means for inspection? The limit tolerance is in fact correct. But the method of inspection leaves you some open ground potentially. For instance, Ø.019 / Ø.021 measured with a pin will give you some dimensional leeway for holes and slight out of roundness, but if you're using some form of air gauging or the like, not so much.

And then, with pins, you also have to factor in if they're plus/minus pins, gage fit vs. slip fit, etc.

If they're measuring with a microscope, the ends could be slightly blown out or flared and which might not affect manufacturability in any way. Beyond the first .015" or so of the entry way to the hole, it could be perfectly round, straight, and in tolerance.

Figure out how the part is being measured currently, and how it is being measured at the manufacturer's facility. If they're using two entirely different quality systems, then they have to discuss some things.

 

[PSE]

I would agree with the above replies. The customer specification for the part is .019-.021. The manufacturer should control their process to meet this. This would include knowing the uncertainty and capability of both the manufacturing equipment and their metrology for measurement.

For the customer, they also would need to know the capability of their QC equipment. Just because a device may be able to resolve out to 5 significant digits does not mean that the it is perfectly accurate there. Operators vary in technique and environment can easily be a factor. Agreement and measurement correlation needs to be reached between customer and supplier. This can be difficult to achieve.

I have been working for months with one of our suppliers on a part and we still are having discrepant results. This is even after having the same type/brand of test equipment returned to the manufacturer for recertification. We have then used a certified reference in both machines and get differing results.

Regards,

 

[meintsi]

rhodie ...

I'm not quite sure how to take your post. If you are giving creedence to the manufacturer's claim of significant digits ...

ASME Y14.5M-1994 Section 2.4 Interpretation of Limits

All limits are absolute. Dimensional limits regardless of the number of decimal places, are used as if they are continued with zeros.

Example:
12.01 means 12.010...0

To determine conformance within limits, the measured value is compared directly with the specified value and any deviation outside the specified limiting value signifies noncomformance with the limits.

Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[rhodie]

meintsi:

I see how that can be confusing.
The point I was attempting to make is that it is important to agree on a standard before starting the work.

If the machine shop sees 1.2100, then the cost of machining the part is significantly higher than if the machine shop sees 1.21, agreed?

 

[GrimesFrank]

I see things as pretty clear, limits are limits;

.02120 > .021(0000....) The manufacturer has not met the terms of the agreement (however the customer measured to 5 sig digs)

You have two options;

1) Remeasure, perhaps it is uncertainty error, etc.
2) Receive concession on the ID fromt he customer if it is technically possible. (i.e. I doubt tolerance fit is affected by .0002 difference)

Frank "Grimey" Grimes
You can only trust statistics 90% of the time.

 

[drum88]

Thank you all very much for taking the time to answer, and your informative and enlightening replies.
At this point, it looks like parts will simply need to be re-made as our customer refuses to even let them out of QC to try them in the application.

 

[kenvlach]

I agree with meintsi.
The specification was 0.02000..+0.00100...
A clear & reasonable manufacturing specification.

If spec. was 0.02000..+0.00010.., i.e., 10x tighter,
the job would have cost significantly more.

If +0.00001..., then decline the job.

 

[ajack1]

Surely the accuracy you measure to has to be greater than the limits?

For example if you have .019-.021 the third digit is rounded up or down so only a measurement of .020 would be acceptable as .021 could be anything from .0206 to .0215 and could possibly be out of limit, in fact by only measuring to three places you are cutting your limits down.

Having said that it is hard to see where .0002 matters on the ID of a rivet, but that is a different story.

 

[meintsi]

rhodie ...

Yes, more digits usually means a higher cost.


kenvlach ...

Be careful because technically, 0.020±.001 IS NOT the same as 0.021/0.019


Limit dimensions apply when there are absolute maximum and minimums to what size is allowed and calls for theoretically perfect form at maximum material condition. (also called the Taylor Principle)

Plus/minus tolerances do not have this extra constraint.



Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[JohnNabors]

Meintsi-

I agree with your position with one caveat: clause 1.1.3 of ASME Y-14.5M-1994 states, "Where drawings are based on this Standard, this fact shall be noted on the drawings or in a document referenced on the drawings. References to this Standard shall state ASME Y-1.45M-1994."

If the drawing supplied to Drum88's manufacturer includes that statement, the manufacturer doesn't have a leg to stand on. Otherwise, in my opinion there is definitely some wiggle room and Drum88's company and their customer may need to work it out between themselves.

John Nabors

Never try to teach a pig to sing. It wastes your time and annoys the pig.