What's new
What's new

True position callout .000 M to datum A M

What do you make of this? Part requires 100% inspection.
Dealing with purchasing, military replacement part, no deviation allowed.

View attachment 276011

It is called out as 0.0 deviation at MMC (the M in a circle) = maximum material condition. I don't see datum A on the print, but am assuming it is centerline of the part? If so just be sure to turn both diameters in one chucking and you should be good to go.

As far as no deviation allowed, well that is a purchasing/quoting screw up IMO that it did not get flagged. I imagine even inspecting with a cmm and tenth indicator, you will see something (even if it is just a slight bit of bearing play or whatever in the equipment). Might want to turn that diameter .0005-.0007" undersize to give you the little bit of play you will need for inspection...?
 
That's my thought too. Use MMC (go undersized on diameter by half the tolerance) as runout tolerance. Other datum is another diameter with .001 total tolerance, so i could pick up some there too. I'll be turning both diameters at the same holding, so I'm not worried about run out, just how to document it on an inspection report. Going to see if I can get purchasing to clarify through engineering. Never seen it toleranced this way.
 
there's really nothing to clarify, it's done like this all the time. In fact, I remember a gd$t quiz a while back whera tp of zero was given as a trick question.
 
This is a very good way to define the needed relationships, where close tolerances are required. The "zero"tolerance on the diameter's true position is modified enough with the MMC callout to describe that the part needs to be dead-nuts concentric, with a few tenths of diametral clearance allowed. Seems perfectly sensible for functional callout; whether you can hit the tolerance may be an open question. DAMHIKT.
 
there's really nothing to clarify, it's done like this all the time. In fact, I remember a gd$t quiz a while back whera tp of zero was given as a trick question.

Doesn't make it correct, or a 'good' way. I agree, nothing to really say about it except you usually see something like this and sweat trying to make them to print, and fast, and repeatable... then come to find out it is a clearance fit for some other component that has .02" "slop" in it :toetap:
 
barbter is right, where is "A"?

Seems A should be a diameter or bore. What is the tolerance of A? Edit: saw your reply, it is another diameter with .001 tolerance.

My understanding of these .000 boxed dimensions (and I see them a lot) is you get your .001 bonus tolerance for the size of that diameter if you hold it to the minimum size, and you get some more bonus tolerance based on the tolerance of "A".

EX: If A is a diameter with .001 tolerance, and you manage to put both diameters at the low, you'd get up to .002" TIR there.
 
I see this all the time with our customers. It's especially common on clevis ends of bellcranks for the holes in the ears. In this example the tolerance is .000 + the bonus of this feature based on its actual size and whatever the bonus is of -A- based on its actual size. We record it on the AS9102 as .XXX (whatever the measurement is, that's within the bonus tolerance) with the circled "m" after it indicating it is using mmc bonus.

Sent from my SM-N960U using Tapatalk
 








 
Back
Top