When is it better to use coordinate tolerances to locate a hole instead of true position?

[Raddy13]

I'm learning about GD&T out of a textbook somebody had at work and there are questions at the end of each chapter that I assume are meant to be discussions with the instructor. In the first chapter on position tolerance, one of the questions is, "When is it better to use coordinate tolerances to locate a hole instead of true position?" I can't find anything in the text that explains when it would be better and googling hasn't turned up anything, so I thought I would ask here.

 

[greenimi]

Short answer: never.
I know it is debatable.

 

[chez311]

I'll assume by "coordinate tolerances" you mean directly +/- tolerancing the (x,y) coordinates of the hole instead of basic dimensions. (FYI assuming you're going by Y14.5-1994+ "true position" refers to the theoretically exact location of a feature, defined with basic dimensions - the tolerance providing allowable deviation from said true position is simply called "position" or "positional tolerance". I'm not sure if the term was ever used otherwise in a previous Y14.5 version but this is a commonly misused term)

If your drawing is Y14.5 compliant? I would say never. I can't imagine a situation where you would rather use directly toleranced location instead of basic dimensions/position of a hole (note - Y14.5 does not support position tolerance in combination with directly +/- toleranced location).

If your drawing is not Y14.5 (or ISO for that matter) compliant? All bets are off,

 

[3DDave]

It's a trick question, though for most cases there is little difference. When the acceptable variation is large compared to the precision of fabrication is the move to positional tolerancing a clear winner. Put another way - when the tolerance allowed is very close to process limits it become necessary to more precisely define the way that those features are to be inspected to ensure the appropriate parts are rejected.

 

[Raddy13]

Make sense. Thank you for the replies!

 

[dgallup]

If your parts are going to be produced and checked in a 3rd world country without access to measurement systems more advanced than a dial caliper and you have fairly generous tolerances you might be better off with direct tolerancing. I know from experience in that case it doesn't matter what you put on the drawing, the inspection results will be linear +/- measurements.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[geesamand]

Gear meshes incur twice the transmission error when they are misaligned across their axes vs. when the shaft ends are misaligned in the plane. So when you tolerance premachined dowel holes and bearing bores across the halves of a gearbox housing, it's most realistic to have a different tolerance on those locations in-plane vs across the plane.

But that's the only example I've seen so far. It's the only case I'm aware of.

 

[chez311]

Geesamand,

Could you clarify what you mean by "across the plane" or "across their axes" vs in plane? Do you mean orientation error vs position error? Or do you mean different tolerances for two directions say x vs y in cartesian coordinates? Both can be accomplished with geometric tolerancing - the first through orientation refinement of position and the second through bidirectional position tolerance.

As long as one has the ability to evaluate the geometric tolerances as specified (per dgallup - some do not have that capability) geometric tolerancing will ALWAYS result in the less ambiguous specification over direct +/- tolerancing of position. I don't see whats to be gained, especially as your requirements get tighter and more precise and closer to your process limits as 3DDave mentioned.

 

[geesamand]

It was a bidirectional position tolerance situation. Expressing it in direct +/- tolerances was actually simpler. This was a case where adjoining bores only cared about their position relative to the next bore, so it required multiple datum structures.

 

[chez311]

More simple? Perhaps in appearance. In determination of a single unambiguous tolerance zone to which the feature(s) must conform? I would say not, especially when the requirements become tighter.

If you could have tightened up the positional tolerance in both directions to convert the bidirectional to a single tolerance, I would think one could creatively daisy-chain several single segment tolerances without specifying more than three datum features*. Though perhaps different tolerances in each direction reflects functional requirements, I would suspect that in fact it is the more restrictive of the two tolerances which would have the greatest impact on production/process limits - though of course function should drive specification I think theres something to be said of the unambiguous specification of requirements. If multiple interpretations are possible and/or the requirements for your inspection department are unclear, I would think that would have the possibility to be detrimental to function.

Bidirectional might still be possible with a similar method (I'd have to see the application), but certainly more cumbersome and with some slightly more complex results - though not nearly as complex and potentially problematic as trying to hold a tight tolerance with +/- directly toleranced position.


*though more could be utilized if necessary - actually increasing the potential stack up from the first bore to the last bore for an increase in complexity. This might be beneficial if one of the bores is held in position relative to the other - however if it is only "mutual position" which is of concern ie: position relative to each other without biasing DOF constraint to one or the other then the complexity of additional datum features is not necessary in my mind

 

[dingy2]

The original purpose of GD&T was to reflect the features function and relationship to its mating part. Over a period of time that seems to have fallen apart and many designers place GD&T on all features.

In your situation, I probably would use co-ordinate tolerances on holes that had no function and relationship with the mating part such as holes to lighten the product or just for cosmetic purposes.

Always a bit of debate here but hope my thought helps.

Dave D.
Retired GD&T Trainer