huangyhg

mmc on datums
the question i have about mmc and datums is as follows

setup example

an mmc tolerance is placed on datum b.
an mmc tolerance is applied to a pattern of holes and then mmc applied to datum b.

is this statement correct?

when a datum is referenced at mmc and it fails its size tolerance, any tolerance that references the datum is set to status fail and the tolerance is re-analyzed as if the tolerance references the datum at rfs.
in some cases, this will cause the tolerance referencing the failed datum to show a deviation within tolerance.
this indicates that the position of the tolerances features is actually ok, but the tolerances fails strictly based on the failures of the datums.
is this statement correct?
or should the pattern of holes pass even though the datum has failed?

what, if any differences will the standards make, as both iso and asme are used, (not on the same part thought!!)

check out our whitepaper library.
b's deviation does not condemn the pattern's feature control to failure... it is just that the pattern's feature control with all of it's limits and liberties cannot be fully determined until b is compliant to it's size and orientation requirements.
in iso if the envelope principle -(e), or "taylor principle" is designated then asme and iso are the similar. the pattern would be tested in relation to b's actual mating envelope (as oriented to the primary if b is a secondary datum feature).
if the principle is not invoked then they are not necessarily similar as the datum feature's form and orientation can change the limits and liberties that b's size contributes to the pattern location tolerance.
paul
ja500,
you can do two things with mmc. you can specify a tolerance at mmc. you can call up a datum at mmc, although the datum must be a feature of size. on any given feature control frame (fcf), you can do either, both or neither. it all makes sense.
if your datum feature fails its size tolerance, then your part fails. who cares where the holes are? otherwise, what is the point of specifying tolerances? if your design and drawings have been done competently, your datum is an important feature. the holes may be okay from the non-conforming datum, but that does not mean they will pass when the datum feature is fixed.
just as a design note -- i avoid using features of size as datums. if i do it, the feature of size usually is accurate enough that i do not care about mmc. dowels and dowel holes are good datums. sometimes, you have to do it, but usually, there is a better way.
jhg
the first question has a simple answer. as drawoh said, a hole pattern can have a position tolerance at mmc and be referenced as a datum feature at mmc (or rfs). any combination is legal and one could dream up applications for each.
the second question is a can of worms. i agree with drawoh that if the datum feature fails its size tolerance then the part fails. i wouldn't necessarily stop there though. it may be useful to know the relationship between the considered feature pattern and the datum feature(s).
the problem is that a nonconformance in a datum feature might result in a more forgiving condition that helps the considered feature tolerance to pass. or it might be less forgiving. or it might not have any effect at all. one example would be the size of the holes in the pattern that is referenced as a datum feature at mmc. if they are oversize, this is more forgiving. if they are undersize, the considered feature control isn't given its full "liberty" as paul mentioned. if the datum holes fail a tolerance that is there for cosmetic reasons (such as cylindricity or perpendicularity), this may have no effect on the position tolerance on the considered feature.
so should a nonconformance on a datum feature mean that all controls referencing it get labeled as a fail? i would say that the actual values of any controls referencing the nonconforming datum feature are "suspect".
another part of the question relates to whether you look at the considered feature(s) and datum feature(s) as separate entities, or as an overall system. this is a whole other discussion - perhaps another time.
evan janeshewski
axymetrix quality engineering inc.
axym,
please note that i referred to "competent" design and drawings. obviously, if we accept an oversized datum hole, we have more slop for our bolt holes. but, why are we accepting the oversized datum hole? we had a reason to apply the tolerance. the part is rejected, and it does not matter what else was done right.
consider how you go about reducing the size of a datum hole. your conforming bolt holes may not conform after the part is fixed. all sorts of conformance may not survive welding, for example.
if the design and drafting are incompetent, then perhaps we really did not mean it when we applied the tolerance on our datum feature. perhaps we did not mean the positional tolerances on our holes either. what is the point of doing inspection? accept the parts, cross your fingers, and hope you do not cause a recall.
jhg
drawoh,
easy, pardner. i have no argument with rejecting the part. i didn't mean to imply that we would be accepting the oversized datum hole.
my point was that it might still be useful to measure the location of the considered feature holes for process diagnosis reasons. i wasn't suggesting any sort of rework scenarios which i agree may not result in an acceptable part. but it can be useful to know whether or not the considered feature holes would have checked good if the datum holes had been produced at the proper size.
i'm not sure how to respond to your last paragraph. it sounds like you've had some bad experiences with your tolerance specifications being questioned, overridden or ignored.
evan janeshewski
axymetrix quality engineering inc.
drawoh,
this response doesn't relate directly to question asked by ja500 and i don't want to divert the discussion away from conformance reporting of dimensional tolerances but...
you said,
quote:
i avoid using features of size as datums. if i do it, the feature of size usually is accurate enough that i do not care about mmc. dowels and dowel holes are good datums. sometimes, you have to do it, but usually, there is a better way.
i agree with your apprehension in selecting "features-of-size" as datum features considering that they complicate the measurement and predictive design processes... but... the ultimate variation that is inherent in assembly and function is subject to that variation. if your design does not account for it via "trustworthy" alternate stack paths... then the design specifications will fail to predict the function.
my advice is to select the datum features characterize the function directly "if possible" to minimize the need for alternate stack predictions that may fail to define function. i.e. if a pair of solid dowels are have identical clearance allowances... designate them as a 2x pattern secondary datum feature (constraining the remaining three degrees-of-freedom simultaneously) rather than making one secondary and the other tertiary. if those dowels are designed to "expand" functionally as an interference fit such as roll-pins specify them rfs if not mmc.
paul
promoting, selling, recruiting and student posting
are not allowed in the forums.
(add stickiness to your site by linking to this professionally managed technical forum)
title: drafting standards,
description: drafting standards, gd&t & tolerance analysis technical support forum and mutual help system for engineering professionals. selling and recruiting forbidden.

__________________
借用达朗贝尔的名言：前进吧，你会得到信心!
[url="http://www.dimcax.com"]几何尺寸与公差标准[/url]