Fully Employing Positional Tolerancing Over Rectangular Tolerancing?..

[Peterup]

I am in the process of updating my activities’ in-house drawing standards and I would like to hear your opinions on the full use of employing geometric positional tolerancing.

ASME Y 14.5 allows either rectangular coordinate system or geometric positional tolerancing method.
Per ASME Y 14.5, para. 2.1.1.1 it use the term “Preferably” in regard to the use of positional tolerancing for the location of features. Some of my engineers and draftsman feel that they have a choice (which they do) whether to use rectangular coordinates dimensioning/tolerances or geometric positional tolerancing. Some feel that since geometric positional tolerancing is more “accurate” ( not me) one should only employ geometric positional tolerancing to critical features. Also some feel it will add to cost, but I only see that if one over tolerance compared to tolerancing/controlling without GD&T ( the old way).

The way I understand geometric positional tolerancing in a nut shell is that it opens up the tolerance region ( plus the bonus tolerance) which will result in not rejecting acceptable parts when compared to the rectangular "square" tolerance zone method . With positional tolerancing, one can say that the actual center could be less “accurate” from true center ( since you have a large tolerance zone) but who cares if the part is still acceptable.

With this reasoning, I do not see why one wouldn’t want to fully employ positional tolerancing thought out all drawings.

 

[ajack1]

It depends largely on what you are trying to dimension, the more complicated the part the stronger the argument for geometric. It gives far more control to specific items, if required and avoids stack up or tightly tolerance things that do not need it.

However for simpler parts it is possibly more work to achieve the same results.

 

[TheTick]

Another great benefit to positional tolerancing is that it works much better for check gages. If you have parts that you want to check with go/no go gages, then positioinal tolerancing is the best way to go.

Also, positional tolerance opens up a larger tolerance zone in up to three ways:
[ol][li]Uses a circular region larger than the rectangular region defined by traditional tolerancing[/li]
[li]Allows bonus tolerance by using MMC on features[/li]
[li]Allows bonus tolerance by use of MMC on datums[/li][/ol]

In mass production scenarios, increase of tolerance band can save much money over the life of a part.

 

[wgchere]

It is also easier to design mating parts with GD&T. Instead of intuiting the proper sizes of holes or applying the complicated algebraic formula for toleranceing mating holes and stackups, GD&T uses simple arithmatic.

I worked at a Navy base for awhile and the policy was only GD&T. It was nice. But we also had our own fabrication shops. The claim that it will raise the cost is only true if using shops that don't understand GD&T. Those shops usually put a "GD&T surcharge" on parts just because they don't understand it.

One caveat for full implimentation of GD&T: Thin sheet metal only needs a datum A surface. The added stability of Datums B & C doesn't add much when your feature is only .062 thick! Saves some time.

 

[dingy2]

Only use positional tolerances when you have features of size (pins or holes) and there are mating features that are used for assembly.

Positional tolerances are applicable for a pattern of holes when we have a pattern of threaded studs on fixed centers that are inserted in the holes. This is just one example.

Whenever one uses positional tolerances, use MMC on both the tolerance and also the datum if the datum is also a feature of size.

One can then develop a gauges which is, essentially, the mating part made in the worst case. If the manufactured part fits the gauge, then it will assemble and the part is acceptable.

If the feature of size is a ROUND, then use diametrical tolerance zone while holes, pins or other featurs of size that are not round should not use this.

Designers use positional tolerances a bit too much. If we have holes to lighten the part, use coordinate tolerancing. There also may be a threaded hole that a wire attaches. Use coordinate tolerancing in this situation.

Hope this helps

DD

 

[ctopher]

All good responses. wgchere made a good point about sheetmetal. We always made it a standard not to have for than one datum for under .094 thick.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[Peterup]

Question For Dingy2

In regard to your comment of holes to lighten the part, use coordinate tolerancing.

If one uses coordinate tolerancing, the plus/minus tolerance still would be required. What ever plus/minus tolerance one chose , say + .125 , you could still use GD&T tolerance method , just place .125 RFS in the positional control box.

I do not see why coordinate tolerancing is any cheaper or easier to use.

 

[ewh]

While it is not a GOOD reason, coordinate tolerancing tends to be cheaper for the simple reason that when a shop sees GD&T, the price automatically goes up. Find a good shop and there should be no problem.

 

[dingy2]

Designers should realize that GD & T is applied when there is a function and relationship between features and mating parts. This also applies to positonal tolerances mentioned.

The proper useage of GD & T will help everyone in manufacturing and quality apply efforts where needed but if we have a drawing with everything in GD & T, then we have defeated the purpose.

I really wish Designer would ask themselves when applying GD & T on a drawing "what is the function and relationship of this feature"?

Apply positional tolerances on features of size when there is a function and relationship only. Applying positional on all holes irrespective of their function does not help anyone. It causes confusion on the shop floor with gauges made to check a pattern of holes (to lighten the product in this example)that have no meaning. A waist of time and $$.

No function or relationship of the feature to mating parts - no GD & T.

I do know that one could apply positional tolerances in RFS but it does defeat it's purpose.

DD

 

[ctopher]

You will find a lot of people do not understand GD&T and will fake their way through it. I see drafter's, designers & engineers take older dwgs and copy GD&T stuff over to new dwgs to make it look good! IMO, all engineering, drafting & designers positions should have manditory training in it. So should inspection and machining.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[KENAT]

I think some of you have nailed it. Whilst in theory in most situations appropriate GD&T should open effective tolerances and hence make a cheaper part in practice most people (Designers, engineers, machinists, inspectors, estimators, me etc) don't know it as well as we should.

Hence you may end up being charged more for what should be a cheaper part. Also as mentioned above for something simple with low value/production you need to consider if the effort of doing the GD&T is worth it.

Also you only mention positional which mainly applies to holes and some slots. Use of profile expands this principle to other shape features but even less people will immediately understand it.

That said we've made it policy at my place to use GD&T to as much as possible, it’s introduction hasn’t been entirely painless.

We have a training software to help but I haven’t used it yet so am not sure just how good it is.

 

[MechNorth]

GD&T is an engineering language to communicate design intent...how you use it makes the difference between quality & scrap, economy & costly waste. GD&T by itself doesn't "open" or "tighten" tolerances, it just provides a better way to communicate the tolerances you need on each feature.

All features must have a locational tolerance; Features of Size are typically located with a positional tolerance, and surfaces are typically (and best) located by a Surface Profile. In fact, you can use Surface Profile to locate most Features of Size except threaded holes, which makes it an ideal "General Tolerance" method. Rounds (i.e. a curved feature which does not have a MINIMUM 180-degrees of rotation) CANNOT be located by the positional tolerance, and MUST be located by the Surface Profile. The tolerance of the positional or surface profile determines the accuracy and cost, not the generic use of these controls. For those that think Surface Profile is an expensive control to inspect...it's time to study this control, because it typically is much less costly and much easier to verify because the feature needs to be "in the zone" and nothing more (i.e. "actual" dimensions don't matter).

Ctopher nailed the problem in his comment above...too many people fake it. It's not because they don't want to do it correctly, it's typically that they don't have enough training (and yes, it takes a lot!), which is the responsibility of the designer, the machinist, the inspector and the company.

Incorrectly applied GD&T can only produce bad parts. Machinists who don't understand GD&T can't create the specified parts. Metrologists who incorrectly inspect GD&T can't prove that the finished part meets the design intent.

It is true that "bad" shops will crank up the price as soon as they see GD&T. I had a standardized part that had cost about $180 to produce (for almost 6 years of production); using GD&T, we opened the tolerances on the sizes and hole positions, removed a couple of "history" holes, decreased the surface finish quality, and submitted the parts for quotation. The range was $500 to almost $1k. These were shops in Europe, USA and Canada; some claimed GD&T expertise and others accepted their GD&T ignorance. The $500 quote was from a small shop untrained in GD&T who bothered to open Machinery's Handbook and look things up. The highest quotes were from "aerospace" manufacturers who claimed GD&T expertise. When I communicated the "translation" to the shops, the lowest quote came in around $80, and it wasn't an "aerospace" shop.

Applying GD&T is never a "waste of $$" unless it isn't taken seriously. The designer needs to rationalize (and hopefully analyze?) the controls and tolerances being applied. The shop needs to correctly read the controls and understand their meaning, and inspection needs to be able to validate it all. As designers, we need to start the ball rolling and hold everyone's hand as they come up to speed. If we don't, then we've wasted $$.




Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

 

[KENAT]

MechNorth, You're right.

I think when I put "Also as mentioned above for something simple with low value/production you need to consider if the effort of doing the GD&T is worth it." I was allowing my frustration over many of the issues you put get the better of me.

We've got a very complex part (with high scrap rate) which previously had minimal, fairly poorly applied GD & T on it redrawn with extensive GD & T to take advantage of areas we can "relax" the tolerances (done by some of my more senior coleagues who have the experience and training to really know what they are doing). We also incorporated a number of DFMA ideas into it, such as making some of the small blind tapped holes less deep etc, mostly in response to requests from the machine shop.

If I remember correctly the price doubled! This despite it being easier to make.

I stand corrected,

Ken

 

[zissou]

Well, let's take some time to educate ourselves about GD&T... we can all break out our copies of Y14.5 and break it down one step at a time. Some sort of hive-learning. We'd need to find ourselves some sort of leader - Lord Of The Flies-style. Anyone else think this is a good idea?