Engineers say "We want positional tolerance to be .010!"

[randy64]

I am a designer (not an engineer). A vocal portion of the engineers we support are saying they want to make the positional tolerance on "standard" clearance holes .010. If we follow the fixed fastener formula in ASME Y14.5-1994 with our standard part tolerances, it comes out as .014. This isn't a disagreement about what the formula gives us - everyone agrees it comes out as .014 - it's about engineers getting a "warm fuzzy."

The .014 tolerance gives a possible (at MMC) line-to-line condition. They say that if this happens (which is, I would think a statistically tiny chance) the fastener may have to be tapped in, versus just dropping in. The other argument is that the shops/vendors that make our tools can hit within .005 "all day long", so it doesn't make any difference if we put .014 or .010. To me, this is designing based on a shop's capabilities - a bad practice. Design should be based on worst case abilities/scenarios.

Bottom line is, for some reason the engineers are wanting to throw aside a formula that was created by minds much bigger than theirs. It has been explained to them that they are giving away .004 in tolerance that could result in rejected parts. This falls on deaf ears.

Anyway, I have been called upon to participate in a "meeting of the minds" between drafting and engineering to hash this out. I truly don't know what to say, other than "ASME came up with this formula based on math and that's the way it is." It's so self-evident, it's hard to explain. Like 1 + 1 = 2, whether your comfortable with it or not.

Any ideas on how to approach this with the engineers?

Thanks

 

[KENAT]

Where to start.

"the fastener may have to be tapped in, versus just dropping in." No, line fit means it touches as it goes in but doesn't interfere.

I'm assuming that you're properly addressing the perpendicularity aspect either by adding projected tolerance or using the formula in B5 of Asme Y14.5M-1994 - or perhaps is this their poorly worded concern?

Why not make your 'standard' clearance holes the next size drill to gain a few thou?

As to conservative, you're right assuming nominal worst case is already conservative so throwing in an extra .004 is even more conservative. If they don't even want the parts to theoretically touch on the walls then .001 would be plenty extra, why .004?

That said, even using pos dia .014 is pretty arbitrary, one could argue you should use the largest clearance hole allowable for each screw (head) size and work back from there.

Do they understand MMC? You could really have fun and propose 0 position with all the extra tolerance budget on the hole size - arguably a better way to use the available tolerance budget.

The argument of 'they hit +-x all day' is great as long as that machine/shop is available but when for some reason the operation gets moved to the tool with the wobbly chuck (or similar) you have a problem. Or until someone doesn't set the part up quite right initially and it drifts a little and all the other reasons something can go slightly wrong. I've seen both these happen, by having the loosest tolerance that meets functional requirements you minimize the number of parts that might have to be rejected.

Risk management isn't just about how likely something is but also how severe the impact of it happening can be. If you're in low volume high cost manufacturing then while the likelihood of it going wrong may be low, the impact of it happening say when you need to ship a high price product before the end of the financial quarter or peopele get laid off etc. can be massive.

Now I may well be missing something but as an engineer myself, your engineers seem to be misguided.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[ewh]

Even when dis-allowing for a possible line-line condition, the tolerance would only be reduced to .013. The best way that I can think of is to chart out the "bonus" tolerance that they would be missing out on, making your parts more costly to fabricate by throwing out the ones that don't meet the .010 tolerance while still being functionally adequate.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[CheckerHater]

First things first:

they want to make the positional tolerance on "standard" clearance holes .010

By tolerance .010 do they mean diametral tolerance at MMC, or plus or minus tolerance?

If we follow the fixed fastener formula in ASME Y14.5-1994 with our standard part tolerances, it comes out as .014

Just from the look of it you are probably assign really small clearance to your "clearance" holes. It will help greatly if you give an example of your calculation.

The .014 tolerance gives a possible (at MMC) line-to-line condition

Yes, the formula (any formula for that matter) result is THEORETICAL and it is up to you to interpret the result according to your cituation.
Also, you can possibly modify the formula by adding "guaranteed clearance" to it, so line-to-line condition never happens.
But this is exactly why I would like to see more of your problem, to make sure you start from the right place.

 

[randy64]

Details:

Our standard clearance holes for fasteners are .031 over fastener size. Out drawing tolerance block for these holes are +.012/-.003.

So, as an example, in the case of a 1/4" screw, our clearance hole will be dia .281, dia .278 at MMC.

.278 - .250 = .028

.028/2 = .014

Yes, we use projected tolerance.

CheckerHater, yes, diametrical tol at MMC (on clearance hole), not +/-.

KENAT, I agree that the engineers are misguided.

Thanks for the replies.

 

[drawoh]

randy64,

Usually, the relationship in GD&T, between .010" and .014" is the conversion from [±][ ]tolerances to positional tolerances. The .010" actually is [±].005". The positional tolerance is functionally equivalent and it allows your holes to occupy 50% more area, resulting, in theory, in fewer parts being rejected by inspection.

Is that what is happening here? There is a discussion we are not seeing.

Another possibility is that they are looking for a safety factor that will ensure that your holes will work, as specified. This is a standard warm and fuzzy procedure. I fudge things a but because I am usually too lazy to call up projected tolerances. If I am clamping something thick, I worry about it.

Perhaps somebody likes round numbers! My experience inspecting machined parts is that they can achieve Ø.010" easily. There is no cost difference between Ø.010" and Ø.014".

The concept that GD&T allows more functional parts, is rather limited. If your tapped holes and clearance holes are being called up at the ragged edge of your fabrication accuracy, GD&T positional tolerances are a strategy for reducing scrap. A better strategy would be to open up the clearance holes a bit.

--
JHG

 

[pmarc]

randy64,
I tested a vendor once. I sent them two almost identical drawings of a relatively simple part with a bunch of thru holes in it for a cost calculation. The only difference between the prints was that one was showing all holes located by position tolerances of 0.4 mm at MMC, while on the other the same callouts were intentionally tightened to 0.2 mm at MMC. Based on prior cooperation I knew that the vendor was easily capable of delivering the holes even within 0.05 mm for such kind of parts. But guess what happened... They replied that the estimated manufacturing cost for part #1 (with 0.4 pos. tol.) was lower than for part #2 (with 0.2 pos. tol.). So actually, there was a difference, even though according to the logic of your engineers there should not be any.

That being said, my advice is, assuming that tolerances are set based on thorough analysis (tolerance stackups, etc.) and not just on a blind guess, try to specify the loosest possible tolerance values wherever possible - benefits hidden behind this additional, seemingly irrelevant amount of tolerance may be really positively surprising.

 

[randy64]

"...they are looking for a safety factor that will ensure that your holes will work, as specified. This is a standard warm and fuzzy procedure."

"Perhaps somebody likes round numbers!"

I believe these to be the underlying truth.

pmarc, I have heard stories of shops quoting higher for looser tolerances expressed via GD&T, versus tighter tolerances that are expressed as +/-.

Fear of the unknown...

 

[TheTick]

If the process allows it, may as well give it to them.

The engineers may want to remind themselves of the bell-curvy nature of the tolerance band. For most processes in good control, a Ø.013 tolerance will place over 95% of the holes within Ø.005.

 

[geesamand]

"The other argument is that the shops/vendors that make our tools can hit within .005 "all day long", so it doesn't make any difference if we put .014 or .010."

Our R&D engineering team pulls that out sometimes. My proximity to incoming inspection gives me a different opinion. This is not a good argument, for two different reasons.

1) Most machine shops remember the tolerance they hit "all day" in the best case. Some shops confuse the repeatability of their machine tools with the actual accuracy of the final part. They also forget the fixturing error and setup error. Now if their CMM inspector says "We can hit tolerance xxxx" all day, I take that statement with much more weight. Usually the engineer is not getting their information from them though.

2) No two holes are created equal. If you blindly apply the "manufacturable" tolerance, you will still be left with cases where that tolerance is harder to hit. Worse still, the shop may invest in fancier fixtures and extra setup steps to produce the part that would be unnecessary if you had given them full tolerance.

I know the other side of the story too - if you have optimistic vendors who don't meet the tolerances, then Engineering gets the call "can we use them?" when a batch doesn't come out right and production really needs the parts. But if you've maxed out the tolerance, it's straightforward to say "sorry we gave them all of the tolerance we could" at that point.