Cons of zero tolerancing at MMC

[Ivan Silva]

Hello!

Today I was presented to the concept of zero tolerancing at MMC on postion tolerance. I quite understood how it works but couldn't understood why it's not so used in industry. For me, it ALWAYS has more benefit than using the MMC plus any tolerance since the virtual condition doesn't change as well the LMC and beside it the inspector could use a fixed gage with size at virtual condition and just be sure the part pass trought the gage and don't waste time checking if it's meeting the MMC. Do anyone knows an situation where zero tolerancing at MMC may not be the right choice?

 

[Belanger]

One reason might be to control weight. In the aviation industry, every fraction of an ounce is important. Thus, they might need a hole to have an MMC size that's slightly bigger than it functionally could be (resulting in a slightly lighter rib/spar/panel/bracket).
The only other reason might be psychological: A designer who throws a zero MMC on a drawing knows that there might be a bunch of questions from people downstream. That's not a good reason, but it's sometimes the thinking in the real world.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[Ivan Silva]

A good example Belanger. Thank you!

Another good example that just come into my mind is when you have maybe three mating parts, a flat piece with hole where an pin must fit and then an small ring which fits the pin. Maybe for the pin manufacturing process the usage of zero tolerancing at MMC on perpendicularity tolerancing could easy the turning process and the assembly with the flat piece. The usage of zero toleracing would make the pin LMC even smaller which could not be good when thinking about the small ring assembly because it would increase the looseness between pin and ring.

 

[3DDave]

They still need to check the hole/feature size no matter the position tolerance to ensure the hole is not too large. The gage will have the Maximum Material Condition Boundary built in regardless, so there is no advantage there; it's not a no-go gage for the hole size.

The typical reason for non-zero position tolerance on holes is that drills are made slightly larger than the fastener and that increment in diameter is partly or totally used for position tolerance. In doing so it saves the machinist from having to calculate how much the hole location can vary without having to also choose a hole size to match; the fewer calculations on the shop floor the better.

Finally, suppose one decides on an amount of clearance and set that as the MMC size with zero position tolerance - but that number isn't one that matches conventional drills? Sure, they can pick the next larger size drill and then calculate their own position tolerance from that - but again, the fewer calculations on the shop floor the better.

 

[powerhound]

The only time I can think when 0@MMC wouldn’t be appropriate is if ANY value at MMC is not appropriate, such as a hole that is meant to receive a press fit pin or bearing race. Otherwise, I use 0@MMC every chance I get.

To JPs point, there are countless suppliers out there who are clueless about this and all they see is a 0 and think that you’re requiring a perfect part.

John Acosta, GDTP Senior Level

 

[drawoh]

Ivan Silva,

I like zero tolerancing because it is a precise description of what I want. It does scare vendors, and if they know what they are doing, they know they cannot fabricate to MMC.

--
JHG

 

[TheTick]

The biggest con is processes and their respective precision. You are basing the resulting tolerance of downstream features 100% on the ability to precisely create datum features as close to MMC as possible.

The math works. I'll give you that. In some cases, the processes may have the necessary precision to pull it off. But it puts a lot of overhead on adjusting dimensions that are not usually simple to adjust in-process.

Part of my own on-the-fly DFM-while-designing is to not make things unnecessarily onerous for the good people who get to actually make the parts. Parts turn out better when you respect the processes. All processes--not just machining, but quoting, programming, fixturing, and inspection. If you make your vendors sweat more, they will make you pay more.

 

[engAlright]

In some applications you may require a very close fit with a pin, but the location of the pin is not critical (or at least less critical). In that case for ease of manufacture you may apply a loose positional tolerance with tight control on the hole diameter. It doesn't make sense to impose tight control of the hole location as part of the size variation, since that's not a driving requirement. This is common for quick-release pins since they require a tight tolerance on the hole diameter to ensure the ball detents engage properly.

More often though as others have mentioned I think it's an "optics" problem - if it's not well understood suppliers or customers get nervous when they see a zero tolerance.

 

[drawoh]

TheTick,

Let's say I am calling up a solid PEM nut in a piece of sheet metal. I call up M6X1 and I specify [box][⌖][/box][box][⌀]0.8[/box][box]A[/box][box]B[/box][box]C[/box] to locate it. My keep[‑]out is [⌀]6.9mm, which is the screw diameter plus its positional tolerance plus 0.1 for good luck. In sheet metal, I don't worry about projection. This is also MMC at zero positional error of the clearance hole. If I call out a clearance hole[ ][⌀]8.5/6.9, I have allowed for positional tolerance and variability in hole punching. There is no way a smart fabricator is punching [⌀]6.9mm[ ]holes. I could just as easily call up [⌀]8.5/7.7 at [box][⌖][/box][box][⌀]0.8[Ⓜ][/box][box]A[/box][box]B[/box][box]C[/box].

There is no precision here, just math, and optics.

Edit: I added MMC to my clearance hole specification. Zero positional tolerances must be called up at MMC.

--
JHG

 

[TheTick]

That assumes the precision of the location is tighter than the tolerance gained from the hole diameter. If you rely on luck to maintain precision, hope that works. I usually consult with the operator.

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

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[mfgenggear]

I believe some of the issues here is what is the fit form and function. and what is required to maintain all three. over tightening of tolerances is just foolish.
one can do it , but the cost of doing business goes up. believe me the vendor will cover his or her cost.