Is there an implied runout/concentricity in the absence of GD&T? 3

[joay11]

(I will form my question using a hypothetical drawing):

Envision a simple drawing of a bushing. The only view is a cross section (with centerline) which has some length Dim, an outer diameter Dim of .500(+/-.005) and an inner diameter Dim of .250(+/-.005). The drawing is completely absent of any GD&T and the title block contains no information about concentricity (or roundness).

The bushing arrives; I measure the part and find the runout is as much as .060" from the OD with respect to the ID (way off). Is this bushing out of spec.?

(Please note: this is NOT a question on how to GD&T, but rather a question of what can be implied in the absence of GD&T)



Taking a stab at my own question:

The centerline in the view implies a theoretical perfect center axis for both the inner and outer diameter Dim's (I may be wrong about this). Therefore, a theoretical cylindrical tolerance band exists for both the ID and OD with respect to the same centerline; since the tolerance for both diameter's is +/-.005, the maximum implied allowable runout is .010".....so, I would say the part is out of spec. Am I wrong?

 

[dingy2]

No, it is not out of specification as long as it meets the tolerances & specifications shown on the drawing.

You used the OD as the datum and then took a circular runout of the ID with the result of .060" TIR (or FIM) but there was nothing on the drawing requiring this.

Dave D.

http://www.qmsi.ca

 

[joay11]

If this is the case, it's interesting to note that the drawing is essentially missing a specification.

Maybe we should address this by making a note within our standard title block.

 

[KENAT]

Per ASME stds no there is not an implied runout/concentricity in the absence of GD&T.

See ASME Y14.5M-1994 section 2.7.3. or equivalent section in other versions.

Per the standard one option is to add a note such as "PERFECT ORIENTATION (OR COAXIALITY OR LOCATION OF SYMMETRICAL FEATURES) AT MMC REQUIRED FOR RELATED FEATURES.

I suppose even here, you could fall foul of ambiguity in what counts as 'related features' so arguably you may be better explicitly specifying it with GD&T.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[lifttrucks]

The Y14.5 standard states: "The limits of size do not control the orientation or location relationship between individual features. Features shown perpendicular, coaxial, or symmetrical to each other must be toleranced for location or orientation to avoid incomplete drawing requirements."

I have seen drawings in the past with a note that was something like this: "PERFECT COAXIALITY REQUIRED AT MMC." This is not a good practice, in my opinion. It leaves too many open questions and does not identify datum features.

Why not take 15 seconds and specify a datum feature and a positional or runout tolerance?

 

[dingy2]

Lifttrucks - You said "Why not take 15 seconds and specify a datum feature and a positional or runout tolerance?"

The simple answer to that is that there appears to be less people trained in GD&T especially since 2008. Training is not on the high priority list for many manufacturers since most are concerned about survival.

If Designers have not taken a GD&T course of some sort, it may not be wise applying it. In other words, if you don't really understand GD&T, maybe you shouldn't use it. Go for the note.

Dave D.

http://www.qmsi.ca

 

[KENAT]

However, without training will they really understand the implications of the note?

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[joay11]

I agree with dingy here. The primary problem I find with GD&T is it requires a Designer/Drafter who can write/read it, a fabricator who can read it and an inspector/quality engineer who can read it.

GD&T seems to work best if you keep it simple; some of the extreme GD&T examples in the book are difficult for everyone in the process to comprehend, so the meaning tends to get lost (there are exceptions).


In this case, if a supplier sent me parts that were .060" TIR and I told him to fix them or send me new parts; and he refused because "it wasn't specified"; I'd be looking for another supplier.

 

[KENAT]

And if I were the supplier, who had parts rejected based on a requirement not specified on the drawing, then I might look for a new customer. Or at least, next time the customer wants a 'favor' of some kind, may be less accommodating.

Assuming it's a small part then yeah .06 is pretty far off nominally aligned, but if you didn't spec it then how was the vendor to know it wasn't acceptable?

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[pmarc]

joay11,

- Since only two diameter dimensions are shown and there is nothing else on a drawing that could somehow imply any relationship between the features, lifttrucks is correct saying that "The limits of size do not control the orientation or location relationship between individual features. Features shown perpendicular, coaxial, or symmetrical to each other must be toleranced for location or orientation to avoid incomplete drawing requirements". Such drawing shows that something probably should be coaxial, but actually it does not specify how much tolerance is allowed for this relationship.

- The drawing is not defining any datum feature so assigning inner diameter as such may or may not be correct. One could take ID as datum feature, but someone else could use OD and they both might be correct. Noone will be able to judge this as the drawing simply seems to be incomplete.

- It is not specified anywhere that runout tolerance is the geometrical characteristic you should measure. Again, the drawing does not give any directions on this. Even assuming that someone is aware that the mutual relationship between ID & OD is missing (like you are) two different persons could go for two different methods of checking it. Circular runout, total runout or maybe position tolerance?

- Runout tolerance value does not have to be equal or smaller than size tolerance. If the tolerance for diameter is +/.005, it does not mean that for instance maximum total runout value is .010. Since total runout is a composite tolerance of cylindricity, orientation and axis offset of a diameter its value can be greater than .010. So your assumption on maximum runout value is unfortunately wrong.

 

[lifttrucks]

"GD&T seems to work best if you keep it simple; some of the extreme GD&T examples in the book are difficult for everyone in the process to comprehend, so the meaning tends to get lost (there are exceptions)."

I would say having one datum feature symbol and a runout or position tolerance is as simple as you can get.

 

[lifttrucks]

"The primary problem I find with GD&T is it requires a Designer/Drafter who can write/read it, a fabricator who can read it and an inspector/quality engineer who can read it."

That's the primary problem with English, algebraic expressions, surface roughness requirements, heat treat requirements, weld symbols, etc.

 

[dingy2]

Lifttruck - You said "I would say having one datum feature symbol and a runout or position tolerance is as simple as you can get."

Should the Designer place a circular runout on the ID relative to the OD? This controls the off center and roundness of the ID but not bend of the ID along its length. There is still of possibility that a mating part would not fit completely along the length of the ID.

Maybe the Designer should place a total runout which includes the attributes of circular runout but also the bend of the feature along its length. Many shop floor people really don't know the meaning of total runout and how one should confirm it.

Then there is concentricity and now we have an argument on what it means and how one should confirm it.

Of course, positional with a diametrical tolerance zone could be applied but should it be at MMC or RFS. Now at MMC, it is applicable to a hard gauge or checking fixture while at RFS one must measure it in various positions along its length perpendicular to its axis if appropriate measuring equipment was available.

Should one place a diametrical tolerance zone as part of the tolerance or leave it out?

We could also reference the datum feature which is an OD in either RFS or MMC.

It all depends upon the actual relationship between the OD and ID during assembly or usage. I just don't think that it is quite a simple application and applying the wrong requirement may not help.

Dave D.

http://www.qmsi.ca

 

[lifttrucks]

Applying no requirement at all and assuming the part will function properly obviously did not help either...

How do you know the note is applying the correct requirement? What's the difference between applying the wrong requirement in note form or symbol form?

 

[pmarc]

It is great to have this discussion, because it is clearly showing that GD&T is indispensible whenever any relationship (geometrical and/or functional) between features exists.

This example with seemingly very simple bushing or something similar should be used in every GD&T training to visualize implications of no GD&T on a drawing and limitations of classical coordinate dimensioning. Simple part but so many issues, caused by incomplete drawing.

 

[dingy2]

I agree liftrucks that is why I think people need a little training in this subject before applying anything. Unfortunately, that is not happening today.

One could also note a minimum wall thickness which should, to a degree, would control the off centre condition and everyone understands its meaning. It still does not control the straightness of the ID.


Dave D.

http://www.qmsi.ca

 

[lifttrucks]

Dave, I think GDT trainers, such as yourself, are indispensable since many colleges do a poor job training engineers in technical drawing. They must think we still get our own draftsman to make the drawings for us.

I guess the point I'm trying to make is that at some point it becomes beyond impractical to try to spell everything out on a drawing because someone may not be able to read it.

Don Day says it better than I could:

http://www.tec-ease.com/gdt-tips-view.php?q=250

 

[dingy2]

A Designer should place all the requirements needed on a drawing and the tube with the ID off center to the OD is an example of all the needs not placed on the drawing. Which geometrical control to use is not so simple though.

Does that mean that all dimensions on a drawing should be covered by GD&T? I don't think so. I looked at the 2 drawings that you reference on the tec-ease web site and question the top drawing along with the bottom one. The 2009 standard still recognizes linear & angularity tolerances and, in my opinion, they should be used in conjunction with GD&T. We have had this discussion here before.


Dave D.

http://www.qmsi.ca

 

[lifttrucks]

I did not communicate that linear or angular tolerances have no place (nor did Tech-Ease).

We make drawings using line conventions, orthographic projections, title block information, bills of material/raw material specs, surface texture requirements, weld symbols, local and general notes, linear and angular tolerances, etc. and require engineers and manufacturing personnel to be able to read and understand these requirements. At some point in history I'm sure someone said: "the problem with surface texture symbols is..."

Good luck putting a geometric tolerance on a drawing in note form and making it clearer than the ASME Y14.5 standard.

From my experience, the vast majority of mechanical drawings cannot be fully or properly defined without GDT. That does not mean that every dimension has to be controlled with GDT - but many do. And if someone is making mechanical drawings and is not using GDT, then the vast majority of their drawings are under-defined.

My stance is that I will not make an incomplete drawing just because someone may not completely understand it.

 

[fcsuper]

There needs to be a lot more GD&T training in drafting/design programs and in Engineering curriculum too.

Matt Lorono, CSWP
Lorono's SolidWorks Resources & SolidWorks Legion
Follow me on Twitter