Old Time Dimensioning & Tolerancing

My understanding of GD&T as practiced on Army Ordnance blueprints for the M1911A1 pistol during the 1940 to 1980 period was that it was based on Maximum Material Condition (MMC) guidelines of...

• Nominal value was of the largest pin with a negative tolerance,
• Nominal value was of the smallest hole with a positive tolerance and
• Nominal value for the location of a hole was the average value with a ± tolerance.

...as seen for most dimensions on this section of an Army Ordnance blueprint:



But many I come into contact with feel the nominal values on this and other Ordnance blueprints are something special and represent the optimum/best/ideal/preferred/optimal/most desired value - and not merely the MMC. My attempts to argue against this with...

• "How can the best value of, say, 0.200 + 0.004 be 0.200 when that value is on the verge of being out of spec - and therefore difficult and costly to make?" or
• "If the in-tolerance range of sizes is 0.200 to 0.204, don't you think most of them would follow normal Gaussian distribution and be 0.202?"

...usually fall on deaf ears.

Q: Is my understanding of this essentially correct or is it flawed?

Best Regards

Your drawing is a bit hard to read, so I can't speak for the actual dimensions/features of your print.

I recently machined some parts for a mounted .50cal gun, similar era to your print (although there were no blocks around dimensions that were referenced to specific datums etc; no MMC or the like. Drawing was circa 1960). The print specified a point on the part, which was called out as ".200 +.002" to a hole.

The print specified that "all dimensions apply when the part is oriented in this position" or something to that effect. I don't remember the specific wording. In this case, the part was a pawl, and the feature that was specified at a distance away from the hole was not a wear point (I don't believe, anyway) but some other features that were specified from that feature were points that would wear. Part 1 in this image:



It was a weird way to call out the feature, but the fact that this part has one long "arm" and one short "arm" means any small error in the short arm will be multiplied a few times in the other arm. In a case like this, I guess they'd rather have you try to hold it to tolerance, as it is more a "best case" scenario in terms of part functionality, not manufacturability. Up to you whether or not you can successfully hold the tolerance to the low. Calling out a +-.001 wouldn't be any different.

Also, I think it would help future engineers who do revisions or review the design to understand function and troubleshoot possible problematic areas to focus on. Such tolerances stick out as a "hey! This should be held on the low side for xxx reason."

I replaced the original image in Post #1 with a section of it that's easier to read. I've got dozens of Ordnanace blueprints for the various parts and while there's an occasional dimension that doesn't seem to fit the MMC pattern, most do. My use of the term "nominal" applies to the first number in, say, "0.200 + 0.004", but I'm not sure if that's the correct term for it. Thanks for your response.

Regards

I'm sure someone will chime in stating the exact opposite, but from where I stand, that B/P was clearly drawn to indicate MMC conditions and not desired/preferred/best ... fit.
Why?
a: The hole location is the only bidirectional tolerance, tough when you think about it you really can't give it any other way
b: With tolerance stacking, some of your +/-.003 grooves can be as much as +.012 out of place from one another and still be within tolerance. Of course one would need to see the assy to know for sure, but that
is likely not the design intent
c: Even the loose dims ( +.015 ) are given as such, and when you combine ( tough I did not try to draw it up ) the 2.060 +.015, .018-.01, .025 -.01R and the 4D40m dims, one would likely need to fudge something
for all of them to work exactly right. Willing to bet that modern day CAD won't agree with those numbers at the MMC conditions.

So count me into your camp as one who agrees with you that:
a: Those numbers cannot possibly represent the best scenario
b: You should not expect that part be anywhere else but mid tolerance when supplied

Sidenote: In this day and age, if the customer supplies the solid model of that part with features drawn to MMC as shown, most of us would charge extra for individually adjusting or drawing them up again
from scratch to median values.

Those types of dimensions look exactly like the kind of dimensions on the part I described above, as well as a few others for the same .50 cal gun. I guess I wasn't understanding without the print staring back at me.

I guess after seeing that, and reading Seymour's post, I would agree with you. After doing the math on many of the dimensions of my parts, *everything* had to be programmed to the middle, else other features would be very close to out of tolerance due to stacking.

I think another argument against the nominal value being the ideal value (on these Ordnance prints) is when imaginary assemblies are made from two different parts, such as the hole (lower, right above) and the pin that goes in it. The hole spec is 0.154 + 0.001 and the pin spec is 0.1555 - 0.0010. If hole and pin were both at their nominal values, the pin would be 0.0015" larger than the hole. This amount of interference, I think, would make assembly much more difficult than necessary. But the average pin is only 0.0005" larger than the average hole. BTW, even the loose fit of the minimum pin in the maximum hole is OK because once the pistol is assembled the pin gets trapped in its hole by the frame of the pistol.

Thanks again for the replies.

Best Regards

A couple of years ago when drawing a print for a local sheetmetal shop to make some custom collet racks, I had rather generous tolerances on hole diameter, but the "fit" would be much nicer if they made the holes toward the low end of the acceptable range. The tolerance on position was so generous, I didn't bother to specify it! The final print ended up with a fully asymmetric tolerance, -0, +0.050 with the nominal dimension all the way at the low end.

And you know what? They didn't make holes that were +0.025 over nominal. They made them pretty damned close to nominal. I was happy because 1) I didn't pay for functionally unnecessary tight tolerances, and 2) I got a nicer than necessary fit. It was up to the shop to know their actual process tolerances and determine a target diameter that would meet my tolerances and approach the nominal diameter, and not mine.

If position had been critical, there probably would have been a LMC constraint in this application, to ensure max-sized holes had proper separation.

sfriedberg said:

They didn't make holes that were +0.025 over nominal. They made them pretty damned close to nominal.

Click to expand...

Did the holes end up being close to nominal because the sheet metal shop knew that size would work better, or maybe simply because their hole punches (or whatever they used) just happened to punch holes that were close to nominal?

sfriedberg said:

-0, +0.050 with the nominal dimension all the way at the low end.

And you know what? They didn't make holes that were +0.025 over nominal. They made them pretty damned close to nominal.

Click to expand...

Not exactly a fair comparison.
You give me a .260 -0/+.03 tolerance, I likely will drill with a 1/4" drill and follow up with a 17/64 EM as a reamer to straighten out the hole and make it pretty. Result will be .2656-ish, quite near your nominal.
OTOH you give me a .260 -0/+.003 tolerance, you can bet your behind I'll be drilling with a 1/4" drill and interpolate with a 1/4" EM to .2615 +/-.001. Even allows the guys another +/-.0005 to screw up.

niemi24s said:

Did the holes end up being close to nominal because the sheet metal shop knew that size would work better, or maybe simply because their hole punches (or whatever they used) just happened to punch holes that were close to nominal?

Click to expand...

I believe (but did not explicitly ask) they used a laser cutter on these small quantity parts. I did briefly discuss symmetric vs asymmetric tolerancing for this part with their sales guy before submitting the final print, so the "size would work better" was mentioned, but didn't make a big deal of it.

SeymourDumore said:

Not exactly a fair comparison.

Click to expand...

I agree it wasn't a perfect comparison, but it was the best real example I had handy. I don't disagree at all with your two examples. The two tolerances clearly call for different processes (to be economic). And when the appropriate process is still much more precise than the specified tolerance, there's room enough to aim for nominal. When the process is not much more precise, the only safe place to aim is the middle of the band. And if the margin is really tight, apply windage to allow for tool wear.

The main point I was trying to make is that aiming for the middle of the band is not always necessary, or appropriate.

The asymmetrical tolerances I have seen are typically used to communicate design intent, especially if different suppliers are used and associated drawings are not available. The ISO limits and fits system uses letters and numbers to in relation to a nominal size to establish a class of fit (for example; holes will have plus tolerances while shafts have minus to ensure clearance). From what I know of the 1911 barrel, the linear dimensions with a unilateral plus tolerance indicate features that meet a hard stop. A short dimension may not leave enough space when a round is chambered and leave the round partially exposed (just speculating - not exactly sure). The hole has a bilateral tolerance because it is a looser clearance fit and does not stop on a fixed surface but rather floats in place. I am a big believer in understanding design intent and determining where to hold dimensions based on what is communicated in the drawing rather than trying to translate everything into something symmetrical or determine a median number. I have seen quite a few operators/machinists scrap parts because they were so focused on using a median dimension they ignored the fact that it was missing one sign or the other.

Old Nubbins said:

From what I know of the 1911 barrel, the linear dimensions with a unilateral plus tolerance indicate features that meet a hard stop. A short dimension may not leave enough space when a round is chambered and leave the round partially exposed (just speculating - not exactly sure).

Click to expand...

The breech of the 1911A1 barrel pivots downward during recoil. The muzzle is held in position by a bushing at the front of the slide.

A pin through the hole below the breech is one pivot for a link whose other end pivots on a pin below it in the frame.
The link is vertical with the slide fully forward.

The slots (.176+.004) above the link on top of the breech engage lugs inside the slide, locking the two together.
During the first phase of recoil, the barrel and slide move backward together, maintaining the gas seal so the powder can burn.
After the breech drops low enough to disengage the lugs in the slide, the slide continues to the rear, ejecting the case.

The unilateral tolerances on the interlock guarantee that any barrel will function properly with any slide at any temperature.
If the slide doesn't move fully forward with a round chambered, the gun cannot fire. These dimensions are critical.

- Leigh

The real Leigh said:

The breech of the 1911A1 barrel .... These dimensions are critical.

- Leigh

Click to expand...

I used to have Kimber 1911, man I miss that thing. I always had a general idea of how it worked but never really thought of all the mechanics involved - thanks for the explanation.

One part of my job I have always enjoyed is working with customers on design issues and machinability. Some may know what they want, and communicate it well person-to-person but fail miserably with a print. On the other hand, we had a customer with a new locking differential design that went overboard with some angularity requirements that backfired and created an alignment problem with the mating part.

Old Nubbins said:

On the other hand, we had a customer with a new locking differential design that went overboard with some angularity requirements that backfired and created an alignment problem with the mating part.

Click to expand...

Yep.

Designing a product is very different from designing a part.

- Leigh

John Moses was a real designer. The same lock detail is more common than Fleas on a Dog. And it still works well..... over a hundred years later.

The real Leigh said:

Yep.

Designing a product is very different from designing a part.

- Leigh

Click to expand...

WHHJR said:

The same lock detail is more common than Fleas on a Dog. And it still works well..... over a hundred years later.

Click to expand...

Wow. You were doing custom work a hundred years ago???

- Leigh

No Mr obtuse I am referring to the original designer of the "Browning 1911", probably the greatest weapon designer we can identify by name...


to

The real Leigh said:

Wow. You were doing custom work a hundred years ago???

- Leigh

Click to expand...

[off-topic post deleted... belongs in the gunsmithing section... TRL]