Diametrical True Position with Zero Tolerance

Hello,

I have just ran across a drawing with a diametrical true position tolerance of "0" (zero), with an M with a circle around it right next to it (for MMC). In the rest of the feature control from, it has an "A", then a "B" with MMC, then "C" with MMC. Datum A is a face, Datum B & Datum C are holes that are the same as what is being toleranced (there are twelve holes). The diameter tolerance of the hole is 8.5mm +1mm/-0mm.

I'm not the greatest GD & T guy (hence, the post), soooo does this mean I would only get tolerance if I held the diameter larger than 8.5mm because of the MMC callout? I am trying to determine the machining process for this part and need to know how feasible this tolerance is to hold...or what tooling/size I should use/try to hold. If I held the diameter at 9.2mm, how far could I be off from the mean dimension? I've never seen a "0" for a true position tolerance....

Thanks for any help.

Welcome to the forum and this issue is not a strong suit for me but a couple of observations. A zero tolerance is impossible to achieve. That would depend on the measuring instruments involved. Are we talking a wooden rule, a micrometer, a MMC, a microscope, and scanning electron microscope, and Atom watching thingy that IBM used to write their initials in Atoms?

Soo if your customer has zero tolerance on the drawing I suggest you send it back to them with a "get real" kinda statement.

Next, as a young draftsman many years back it was hammered into me to always put "Never assume, if in doubt ask" on all drawings (before pre-printed drawing sheets, yes, I am, that old). I suggest you take this advice and ask the customer.

[QUOTE=cncguy;5978]soooo does this mean I would only get tolerance if I held the diameter larger than 8.5mm because of the MMC callout? [/QUOTE]

Yes, true... Also, you get additional tolerance for that feature when the datum's B & C are manufactured at some size larger than MMC.

For every feature of size specified with an MMC modifier, datum or principal feature you get additional tolerance when those feature diverge from the stated material condition.

If you actually manufacture the feature at Dia of 8.55 and the feature is a hole it has diverged 0.05 mm, - this is your maximum allowed positional tolerance assuming the datums are manufactured at MMC size.

If the datum features are as-manufactured at a size greater than thier MMC, you can add that size divergence to the allowed maximum positional tolerance of the feature of size. So, if datum B diverges by 0.01 mm and datum C is manufactured at MMC size, and the primary features diverge by 0.05 mm.

Total maximum allowed positional tolerance for the hole features are 0.01 + 0.05 = 0.06.

Thank you for the replies.

I just want to make sure I'm understanding this fully ...

I was planning on cutting these diameters to 9mm, so those diameters along with Datum B & C will be 9mm diameter, so the size divergence is 0.05 mm, does that calculate to 1.0 mm maximum allowed positional tolerance for the hole features? (0.50 (diameter over MMC) + 0.50 (Datum B & C divergence).

So the tolerance is zero at MMC, but due to the large diameter tolerance of the primary feature and datums, (the size is stated at 8.5mm +1mm/-0mm) if we hold the holes 0.5mm big from the called-out diameter (holding 0.5mm over the called-out 8.5mm is really the mean size in this case), we have a fairly open diameterical true position then? (1.0mm)

If the size was stated as 9mm +/- 0.5mm with the tolerances spelled-out the same way, then I'd have to drill the diameters to the absolute high side (9.5mm) in order to get the 1.0mm true position tolerance, correct?

Thanks.

[QUOTE=cncguy;5991]

I was planning on cutting these diameters to 9mm, so those diameters along with Datum B & C will be 9mm diameter, so the size divergence is 0.05 mm, does that calculate to 1.0 mm maximum allowed positional tolerance for the hole features? (0.50 (diameter over MMC) + 0.50 (Datum B & C divergence).[/QUOTE]

Yes, this is correct.

I'm a little wary of how you expressed the bonus tolerance achieved from the datum features.

If each Datum (B & C) diverge 0.025 each ---> .025 + .025 = 0.5 total bonus tolerance from MMC.

If each Datum (B & C) diverge 0.50 each ---> .5 + .5 = 1.0 total bonus tolerance from MMC.

I think we have to be careful, because if datum features B and C are larger than 8.5, those enlargements do not [U]both[/U] translate into direct additional tolerance for the hole in question. So unless I'm reading your post wrong, Kelly, I would disagree.

If datum feature B is enlarged but datum feature C stays at 8.5, then the position tolerance of the hole being measured does not grow in a circular fashion. Think about it: if one datum hole (B) is big but the other is not, then the looseness around B only allows the part to swivel in a rotational manner. And if both holes are enlarged to 9 mm, that doesn't mean the the extra half-millimeter of growth on each translates into 1 mm of extra position tolerance, because together there is only one movement of the part

FYI -- this extra slop around the datum is usually called "shift tolerance," to distinguish it from "bonus tolerance," which is only the slop taken from the first MMC modifier. Bonus tolerance is always OK to directly add into the position tolerance number. But shift tolerance can only be thought of as additive if there is one datum being modified, and if it acts in the same direction as the hole being positioned.

[QUOTE=Belanger;6013]I think we have to be careful, because if datum features B and C are larger than 8.5, those enlargements do not [U]both[/U] translate into direct additional tolerance for the hole in question. So unless I'm reading your post wrong, Kelly, I would disagree.[/QUOTE]

Well, you’re right to disagree with me John-Paul – as you’re correct. My answer to the op cuts a lot of corners and is functionally not “most correct” :grin: .

It can be challenging to describe the effects of size divergence from MMB for multiple datum features without a function gage.

Now, if the op had a single datum that was coaxial with the datum feature, my answer would be “more correct”.

Hopefully, the op has either a CMM or a qualified functional check gage to verify the as-built features and the effective datum shift.

Thank you for the replies! And yes we do have a CMM to check our parts but this is in the quoting stage and I never have seen a "0" (zero) tolerance expressed for a diametrical true position feature. So I was just making sure that if I drilled the hole larger than the called-out size for the diameter (8.5mm +1mm/-0mm), that I truly would have a tolerance I could live with. So, I believe now, after reading your replies, that if we plan on cutting these at 9mm with a solid carbide drill, we shouldn't have any problems holding the true position tolerance.

Thank you again for the helpful information!

- Paul