Smart questions
Smart answers
Smart people
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

Join Eng-Tips
*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

ozzkoz (Mechanical) (OP)
21 Jan 10 19:31
Hi, I am dimensioning an o-ring grove and parkers catalog says the max eccentricity is .002 and states this is TIR between the groove and adjacent diameter.  I think TIR is total indicator reading, but is this total runout (two arrows) or circular runout (one arrow)?  

Thanks
Helpful Member!  dingy2 (Mechanical)
21 Jan 10 19:56
Eccentricity is the amount of non-roundness and will result in a TIR value (total indicator reading).

The relationship between a diameter and another diameter sharing the same centre is called "circular runout" and combines roundness and off centre in one value which is also reported in a TIR.

I don't think total runout (2 arrow heads) is applicable here so I won't get into its meaning.

So, what do you want? Roundness of the feature or its circular runout to another diameter sharing the same centre that will become a datum?

Dave D.
www.qmsi.ca

Belanger (Automotive)
21 Jan 10 22:28
I'm with Dave -- total runout is not what's wanted here. Circular runout (single arrow) with a specification of .002 (and the correct datum reference) will probably equate to this TIR callout.

But there's one other catch that Dave is getting at:  circular runout error is caused by two main factors: eccentricity (coaxiality) and circularity (roundness). So in reality, you could have a groove that is perfectly centered to the adjacent diameter (so there is no eccentricity), but if this groove is slightly egg-shaped it could be rejected by circular runout.

To truly isolate "eccentricity" is rather difficult (pretty much "concentricity" in GD&T lingo), so I would stick with circular runout.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

ozzkoz (Mechanical) (OP)
22 Jan 10 7:44
Thanks, I think circular runout is what I need.  The TIR is used to control the minimum amount of squeeze on the o-ring so I think I would want to control both eccentricity if it is perfectly circular and form if it is more egg shaped.

Thanks all
fsincox (Aerospace)
22 Jan 10 8:03
Dave,
Was that a misquote? roundness and excentricity are not the same, they are separate contributors to runout. This is why I am not a fan of them. It leaves me to ask: "well which is it", it does not answer the question. Circular runout is traditional for this application, done many in the day.
Frank
dingy2 (Mechanical)
22 Jan 10 8:44
Frank:

I now agree with JP on this one. Eccentricity is not roundness but non-coaxial.

Circular runout is a combination of roundness and off centre.

Dave D.
www.qmsi.ca

axym (Industrial)
22 Jan 10 10:10
The TIR mentioned in the catalog could be circular runout or total runout.  For the geometry of an o-ring groove, the difference between the two would typically be very small.

The word "eccentricity" is a bit confusing.  On the one hand, "eccentric" generally means "not concentric".

On the other hand, "eccentricity" is also used to describe the proportions of an ellipse, or egg shape.  An ellipse with zero eccentricity is perfectly circular.

On the third hand, an "eccentric" can also be "a person with an unusual or odd personality".  This term has probably been applied to several of us on this forum.

Perhaps we could describe how centered an egg-shaped feature is with the term "egg-centricity".  ;^)

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

MechNorth (Mechanical)
22 Jan 10 10:56
For an o-ring groove on a shaft (as opposed to a face), I'd go with total runout as the interpretation rather than circular.  Circular just covers one individual segment at a time, whereas total covers the entire surface as a single entity.  The o-ring gets deformed to take up pretty much all of the bottom surface of the groove, not just the initial circumferential ring contact at the tangent of the toroid.

Evan ... most of us are third-hands.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

Belanger (Automotive)
22 Jan 10 11:08
Interesting, Jim...
Your suggestion will also include a straightness tolerance and a parallelism tolerance of .002.  Do we really care if the bottom of the groove is that good as it goes across longitudinally?

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

dingy2 (Mechanical)
22 Jan 10 11:56
I certainly would use a total runout if the groove width was, say, 4 inches wide, but in most cases, it would be rather small in the .060 - .100 or so range.

I agree with JP on this one - circular runout.

Dave D.
www.qmsi.ca

MechNorth (Mechanical)
22 Jan 10 14:36
JP, yes, you'd get the roundness, cylindricity, longitudinal straightness and position from the total runout.  I suppose that in a sense you'd also get the line-segment longitudinal parallelism to the axis as well; interesting thought.  As for how good the bottom of the groove needs to be, that's dependant on a number of factors including load magnitude & type, seal compound & deformability/durability.  I had to work with some o-rings and custom seals that were made from some interesting polymers that were highly susceptible to abbrasion wear and seatng form; those required even better control of the surface.  But to turn your question around, why go for a lesser, and more difficult to validate, control than one that gives you extras for free.  If you buy a base-model car these days, it probably has a lot of "extras" like power locks & windows, CD player, etc ... would you tell them to strip the extras out because it doesn't add value to you personally?  By more difficult, I mean that you have to verify each segment independently rather than as an entire surface; decision criteria must then be set for how many locations along the surface, etc.  As Dave points out, it's a very short surface typically (1.5-2.5mm), so where is the economy and value of using the lesser control?  

Personally ... wait for it, Dave ... I prefer a surface profile that goes from the tangency point on the major diameter to the other tangency point on the major diameter.  It controls size, location, runout, form, orientation.  I've gone thru the work of checking the difference vs traditional linear tolerances & runout ... less time to inspect the profile & well within the tolerances required.  Considering that most such grooves are now done by form tools, it's even more likely that the same tolerance can be held on all aspects.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

Belanger (Automotive)
22 Jan 10 15:04
I mentioned parallelism because total runout certainly detects taper, so I wondered if that along with straightness is really necessary.  As you mentioned, it of course depends on the application.

As for why I voted for a "lesser" tolerance when there's another that gives you more for free, I hold to the philosophy that tolerances should not be constraining something that has no bearing on manufacturability or function (i.e., make the tolerances as large as possible while still making sure the thing works).

Total runout is easier to check, but it's also going to reject a part that otherwise might be passed by circular runout.  So when buying a car, I love getting more for free, but when tolerancing a part, I would disagree with you.  :)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

fsincox (Aerospace)
22 Jan 10 22:04
Dave,
I apologize, I did not realize that eccentric was a word also used for egg shaped. I sometimes forget that communication is not just about what "you" read but also about what was really meant.
Sorry :)
Frank
MechNorth (Mechanical)
23 Jan 10 15:23
Gotcha, JP.  On such a small surface, I doubt there would be much of a difference on results either way.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

fsincox (Aerospace)
5 May 10 9:20
MechNorth,
Total runout? Please have a dicussion with the Tec-Ease people (very nice site) about inspecting the perpendicularity of short length-large diameter pilots then, if you are willing to inspect TR on an o-ring groove.
To the OP,
SAE specifications AS4395 & AS5202 based on the earlier MS33649 & MS33656 referenced in the Parker book itself use circular runout to define the faces, Parker's acctual catalog page states it as concentricity.
Frank
MechNorth (Mechanical)
5 May 10 10:15
Fsincox,
Indeed, perpendicularity of a short-length, large-diameter hole is not usually useful, however sometimes it IS necessary and IS done.  I am used to working with tolerances down to 0.005mm on pilot diameters, and on occasion it does matter; usually it doesn't.  And yes, I have had o-ring grooves inspected for Total Runout on a shaft when seals were failing.  I prefer surface profile for o-ring grooves though.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

fsincox (Aerospace)
5 May 10 22:13
Jim,
I am really curious, how do you teach students to calculate the correct VC for checking the bolt holes and to create the gauge, if you do not give the perpendicularity value of the pilot diameter to the face? (say: Fig. D-4, pg 216 ASME Y14.5M-1994). Do you really tell them it is not important?
Frank
 
MechNorth (Mechanical)
6 May 10 10:28
Frank,
In that particular case, you're reading too much into the figure.  The purpose of that particular figure is to illustrate former datum feature symbol applications, not to give a comprehensive GD&T application for all features.  

Section 1.1.4:  The figures in this Standard are indended only as illustrations to aid the user in understanding the principles and methods of dimensioning and tolerancing described in the text.  The absence of a figure illustrating the desired application is neither reason to assume inapplicability, nor basis for drawing rejection.  In some instances, figures show added detail for emphasis.  In other instances, figures are incomplete by intent.

The example you cite is clearly missing the relationship between datum feature-B and datum-A.  No argument there, but it's not relevant to the point of that illustration.  Now, let's say pilot diameter was only .020" high; would perpendicularity wrt datum-A actually be relevant in "most" situations?  Likely not, and it would be outside of the ability of most shops to verify it; in that particular situation, the perpendicularity back to datum-A would be omitted from the drawing without jeopardizing the intent or quality.

Jim

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

KENAT (Mechanical)
6 May 10 10:34
Come on MechNorth, you don't actually expect people to take "Section 1.1.4:" into account do you, rather than monkey see, monkey do off of an incomplete figure that may be illustrating a different point entirely.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

MechNorth (Mechanical)
6 May 10 10:47
Play nice now.  Besides, I'm a "naive Canuck".

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

Belanger (Automotive)
6 May 10 10:50
Ha ha  Kenat!!  That's true!

But this all brings up a good reminder to designers: the relationship of a datum to a prior datum on the drawing should be established.  For example, when a pilot hole is called out as a datum for others to be positioned from, that pilot hole should still be tied back to the primary datum surface.

In the figure mentioned (D-4) the intent was to show the old datum symbol, but if really pressed for an answer, we could say that the perpendicularity of that boss comes from the title block (perhaps ±1º) and that should be factored into any functional gage...

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

MechNorth (Mechanical)
6 May 10 11:03
Or, JP, we could say that the perpendicularity is per gage-maker's tolerances as the a +/- angular tolerance (if provided in the title block) arguably only applies to surfaces (please, measure the inclination of that axis?!).  Honestly, people leave way too much up to subjective and selective interpretation.  One of the reasons that I advocate using a note that NON-TOLERANCED DIMENSIONS ARE BASIC, and putting a decent general surface profile; it takes another level of ambiguity away.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

Belanger (Automotive)
6 May 10 12:05
Hi again Jim--
I agree with your comment about removing ambiguity, and profile is a handy way to do that.  

Regarding title block ± tolerancing on angles, I always presumed that it applies to any angle not directly toleranced in the field of the drawing. And the old drafting rule tells us that anything that looks like 90º is implied as 90º, so why wouldn't a center line or axis fall under that rule?

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

MechNorth (Mechanical)
6 May 10 13:10
Yes, but ... the old way (typically) doesn't provide a datum reference, so it's just +/- degrees to the related feature (i.e. actual face) as opposed to the datum ... potentially a substantial difference.  If there's a catch-all note tying back to a datum reference frame it would help, but then would you be checking a secondary datum feature wrt an entire datum reference frame?   Ambiguity.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

fsincox (Aerospace)
6 May 10 13:46
Jim,
Thanks all for your replies. I was certainly only intending this example as a picture to represent the concept (the smallest length pilot I could find in the whole book). I you think about it you will realize that, I myself, was also hoping that you would take section 1.1.4 into account. Otherwise all you would have to do is say: "see, the ASME standard did not do it either". I suspect we all know what that is like.
Frank
MechNorth (Mechanical)
6 May 10 13:51
BTDT ... been there, done that

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

dingy2 (Mechanical)
7 May 10 9:19
Frank:

You asked Jim "how do you teach students to calculate the correct VC for checking the bolt holes and to create the gauge, if you do not give the perpendicularity value of the pilot diameter to the face? (say: Fig. D-4, pg 216 ASME Y14.5M-1994). Do you really tell them it is not important?"

I really didn't see an answer to that question. The gauge for this part would be such that the part would mount on datum A with the 25.4/25.6 mm OD dropping in a hole of 25.6 ID (MMC) that is perpendicular to datum A. There is not a qualifier for datum B since there just isn't any depth to the feature.  The only possible qualifier is perpendicularity - not positional.

There would be a clocking or tertiary datum C simulator of 18 mm for anti-rotation and then we would then have 4 pins of 6.4 mm (virtual condition size) for the positional of the four (4) holes.

JP stated "that pilot hole should still be tied back to the primary datum surface". I do agree and it is understood that since no other angle was shown, the feature is perpendicular per 2.1.1.4 of the 2009 edition..

Jim - you stated "we could say that the perpendicularity is per gage-maker's tolerances as the a +/- angular tolerance". What does that mean? Over the years I have had only a few people from gauge shops take GD&T with me and each one has a different shop tolerance on gauges. In each case, the tolerance is larger than expressed in ASME Y14.43-2003.

You also suggested that "NON-TOLERANCED DIMENSIONS ARE BASIC, and putting a decent general surface profile; it takes another level of ambiguity away." So we apply GD&T without any consideration to the function of the feature? The 1994 or 2009 standard does not mandate this and actually gives examples where surfaces and features of size are shown without GD&T. Figure 3-30 Page 47 of the 2009 edition is just one example.

I have been watching this thread and just had to put in my 2 cents worth.  

Dave D.
www.qmsi.ca

Belanger (Automotive)
7 May 10 10:14
Not to be nitpicky -- but like Frank, I maintain that the boss in Fig. D-4 of the 1994 standard must have a tolerance for its angle, and since none is given directly then we must appeal to the title block.  As Jim points out, that has its own perils, but somehow that angle must be accounted for when designing a functional gage.

Dave, I'm 95% on board with your comments.  But I don't think we can just make the functional gage hole 25.6, because that is saying that perfect orientation is required at MMC.  (Perfect form is required at MMC, but not orientation.) Paragraph 2.7.4(a) or (c) of the 2009 standard would be the only way to safely say that the functional gage is 25.6.

I think that para. 2.1.1.4 is meant only for basic angles, meaning that there is a perpendicularity feature control frame involved. So while the dimension of the angle is implied 90º, we still need to know a tolerance on that angle.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

MechNorth (Mechanical)
7 May 10 10:26
Dave,,
Each gage-maker shop has rights & responsibilities to use an appropriate tolerance, typically not exceeding 5% of the overall tolerance applied to the feature being inspected.  If I'm making a granite mill grinding wheel then the tolerances would be fairly loose and any gages made for checking it would be looser than if it was for a precision bearing.  When people tell you things like "my tolerances are looser than that", you have to maintain a view to the source and their market base; you can't make a blanket statement then that nobody uses the published gage-maker tolerances ... as implied by your comment.

Your reference to 3-30 seems irrelevant; tabulated values of tolerances for feature control frames applied directly to a feature on a drawing seems misplaced in this conversation.  As for Fig. 3-29 in '09, which I suspect you meant to reference, please also read section 1.1.4 regarding incompleteness of figures when they are showing a specific concept.  This figure is specifically intended to show FCF placement.

As for a general surface profile not considering the function of the part ... well, "decent" does not automatically mean "gross" or "excessive".  ISO has traditionally mandated that the general tolerance be the shop's poorest capability.  To me, that is rarely known and irrelevant ... I'm not going to put a +/-5mm tolerance on a chamfer just because some supplier in Asia uses a hand-file to break edges.  My advice to clients is to use the most common (i.e. frequently occurring) tolerance on their drawing as the default surface profile tolerance; this significantly reduces the drafting time and communicates the exact same design intent as putting individual controls on every feature ... plus, it ensures that every feature IS in fact controlled ... the old +/- system never truly achieved that.  The issue that a few people have with using the "most common value" method is making the mental leap; it's just a mental switch that needs to be toggled.  
As a participant in a number of Y14.5 meetings, I can assure you that the intent of the standard IS to ensure that the entire part is defined.  That means that every feature of size (excepting primary datum fos and secondary datum fos under certain conditions) must be toleranced for location.  Junk features such as fillets, rounds, chamfers, etc. are still permitted to have +/- tolerancing, but it adds no overriding benefit to the product definition.  

As for supporting the general surface profile philosophy, it is shown well in the '09 edition.  Start with 2.1.1.2(b) Basic Dimensions.  Check out 3.3.35 All-Over Symbol.  8.2.3 Profile Tolerances as General Requirements.  Maybe look at 2.1.1 (e) and 2.1.1.1 also.

The argument about "well, the standard doesn't tell me that I HAVE to do it that way" always arises.  In a grossly simplified interpretation, "shall, must, will" are directives rather than suggestions.  These are mostly avoided to cut off legal issues except where safety is at risk.  "Preferably" is about as strongly worded a recommendation as can be made; i.e. do it another way at your own peril ... not recommended...Danger Will Robinson.  "May" is typically a guidance word and probably sends you in the right direction for best practices.

Jim





 

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

dingy2 (Mechanical)
7 May 10 12:35
Jim:

You stated "As for Fig. 3-29 in '09, which I suspect you meant to reference, please also read section 1.1.4 regarding incompleteness of figures when they are showing a specific concept.  This figure is specifically intended to show FCF placement."

One might use this argument on all the figures shown in the standard since 1.14 appears to be a disclaimer. Does that mean that all other non-pertinent information on each figure can be incorrect? These figures are our examples and we must assume that the examples in the standard are correct.

Section 1.14 states "Numerical value of dimensions and tolerances are illustrative only" which makes sense. It also states about the lack of GD&T application is "neither reason to assume inapplicablity, nor basis for drawing rejection". That also makes sense. It does not state that the applied information in the figures can be incorrect.   

So, Jim, are the linear tolerances to surfaces shown in Figure 3-29 wrong? Must all surfaces shown in figure 3-30, page 47 of the 09 edition be reflected as profiles? Is it wrong to have a feature of size with its location shown with a +/-??

Dave D.
www.qmsi.ca

fsincox (Aerospace)
7 May 10 13:45
Dave,
I really owe you one here; I want to thank you for getting an answer to my apparently uncomfortable question. Your 2-cents is worth a whole lot more to me, today.
Thanks,
Frank
MechNorth (Mechanical)
7 May 10 13:52
Dave, as a trainer, do your training sample drawings 100% complete?  I suspect not, because otherwise you would never get people to focus on the relevant material rather than the irrelevant items.  I have worked on standards for over a decade, and continue to do so today.  I know from experience and legal advice that "how to" standards cannot be nailed down to everyone's satisfaction, and the most effective avenue is to use illustrative examples.  With the exception of a simple basic shape and one or two simple features, it would be impossible to meaningfully illustrate any GD&T concept within the standard while fully annotating everything.  

As for linearly-toleranced stepped geometries, which I believe is what you're referring to, while strictly legal  it's typically a bad practice except on junk features.  My rationale is that there are no opposing points and no indication where to measure to or from ... and you and I both know that THAT subtlety can make a huge difference.  For the 35.5/36 dia recess of 9.4-9.6mm depth, where would you inspect it?  From any single point on the "A" surface to any single point on the bottom of the recess technically is all that you need ... vice-versa is equally legal.  You may think it's irrelevant or not critical in this situation, but let's say that you're inspecting using a CMM.  As programmer (offline for the sake of argument) you set several points on each face and run the program.  You have point-sample data which may or may not be indicative of the rest of the feature(s).  You could have hit a couple of pits or pockets and been out of spec, or maybe those pits & pockets are the only areas in-spec...no way of knowing from inspection data alone.  If a profile tolerance wrt datum-A had been applied to the depth, you would have had a clear tolerance zone within which the entire surface must be contained.

It is impossible to appease everyone on the standards committees, never mind the wider population.  I've caused hours of debate over whether an illustration that has been in use for over 20 years means what most people have thought for just as long.  As a result, information has been stripped from some drawings because it was superfluous to the concept and confused rather than clarified.  Such is standards work.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

MechNorth (Mechanical)
7 May 10 13:57
Frank, I thought your question was rhetorical, not uncomfortable.  Sorry.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

dingy2 (Mechanical)
7 May 10 14:14
Jim:

You asked "For the 35.5/36 dia recess of 9.4-9.6mm depth, where would you inspect it?  From any single point on the "A" surface to any single point on the bottom of the recess technically is all that you need ... vice-versa is equally legal."

Now you are into my area - quality and measuring. I was taught so many years ago that we would come from the plane (not a single point) shown here as datum A and use a 3 point set-up 120 degrees apart located towards the circumference. Zero off the dial indicator on the created plane.

Now, I would sweep the feature with a dial indicator and all surfaces contacted must be not less than 9.4 and no greater than 9.6. I would then record the range of readings such as 9.48 - 9.54, as an example.

I am not doing anything that any CMM Operator would not perform. Of course, when I was measuring parts, the CMMs were not computerized as they are today.

The standard does not get into measuring at all and I am wondering where it states that a 1 point contact is sufficient. I have not read that but maybe you have. Where in the standard is this reflected?

Dave D.
www.qmsi.ca

fsincox (Aerospace)
7 May 10 14:30
Jim,
I do come on too strong here, it is my personallity. I can imagine that J-P is relieved he did not end up training here, now he can realize how lucky he really was. I assure you all this is do more to my enthusiasm for the subject than some attempt to really disrupt. I have just finished reading through all of the posts on this site and earlier on the yahoo site to glean any knowledge I may have missed. It has made me aware of the fact that, as Ken likes to always remind us, we have already discussed many of these issues before. I really do not see where that is all so wrong but suffice to say there certainly is repetition.  I have to admit once I got to my own posts I am frankly embarrassed by some of them. I am sorry if I push you or others the wrong way, I am not sorry I have, and ask, questions and like to explore ideas.
Frank

"Some like to look at the standard and say why, I prefer to think of how it could be and say why not" (pharaphrase RK)
MechNorth (Mechanical)
7 May 10 14:33
That's great, Dave, that you measure things that way but the ASME standards, indeed no standard that anyone's ever been able to reference for me, says to measure a +/- toleranced dimension from a plane.  Please clarify where you get that from.  You could successfully argue that it has been a "common practice", but so is avoiding stepping on sidewalk cracks so you don't break your momma's back ... equally irrelevant to valid metrology.  Supported by Taylor's Principle, +/- tolerance dimensions only need a 2-point check at LMC.  If I recall correctly, the '82 standard and/or predecessors referenced the caliper-rule, which cannot be considered anythying but a 2-point check.  

If you are going to advocate measuring +/- tolerances from a defacto datum plane, please provide standards-based justification.  Doing something because it's "common practice" doesn't make it safe or legal.  It's common for people to race thru yellow traffic lights, but is it safe or legal?  No.  And I'd be surprised to hear any instructor actually advocate such a practice to someone who doesn't know any better.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

MechNorth (Mechanical)
7 May 10 14:40
No offense taken, Frank.  We all like to challenge each other, and I don't get upset about recurring questions ... it's how I learned too, and it still gives me alternative perspectives to consider in contrast to and in support of my own understanding.  

I realized after posting my reply that "rhetorical" could be taken different ways.  It was not intended to denegrate your question.  I thought of your question as more illustrative of question re the underlying topic than an actual question in search of response.

Dave and I tend to spar in these forums because we hold differing backgrounds and therefore philosophies about some of this.  I don't take offense at his comments and I don't intend mine to be offensive either.  It's all good.  Engineers like to "debate".
Jim

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

dingy2 (Mechanical)
7 May 10 15:12
Jim:

You answered my question on 2 point measurement with a question. With that answer, I must assume that there is nothing in the 94 and 09 standard on the subject.

When one gets into measuring, there is levels of confidence in the outcome. I reflected how I was taught how to measure at General Motors so many years ago and we did use planes, axis, etc. A shop floor person may only use a depth micrometer but the CMM result superseded the shop floor result.  

CMMs came into existence before the wide spread use of GD&T. Yes, we tried to simulate the function of the part just as the datum structure used today. If the +/- dimensions extensively used at that time were only 2 point contacts as you claim, the layout room would only have verniers and micrometers.

Unfortunately, there doesn't seem to any intensive metrology training available or, at least, in our area. This is an area that does need standardization.

Haven't had one of these discussion with you in quite a while.

Have a good weekend.

  

Dave D.
www.qmsi.ca

MechNorth (Mechanical)
7 May 10 15:28
Figured citing '82 without mentioning '94 or '09 was a clear indication, but ok ... no, I don't recall any specific reference to 2-point checks in the '94 or '09 standard ... I'm not ready to write an '09 cert exam yet as I'm still working my way thru the book.

I haven't found a decent metrology training program anywhere; MCC (Monroe Community College) apparently used to have one, but I understand it's not as effective as it once was.  The topic of a metrologist accreditation or certification program pops up every few years but the big companies won't endorse and drive it so far.  Another of those things that we need, but business seems to be scared of doing properly ... no problem, keep shipping everything to Asia and India...another topic for another day.

Enjoy your weekend too, Dave.  Almost gave you a shout a few weeks back when I was in your area, but it was rather rushed. Maybe next time.

Jim

 

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

axym (Industrial)
7 May 10 16:03
Dave,

You asked Jim whether the linear tolerances to surfaces shown in Fig 3-29 are wrong.

Fundamental Rule 1.4 (d) on page 8 of '09 states the following:

"Dimensions shall be selected and arranged to suit the function and mating relationship of a part and shall not be subject to more than one interpretation."

One could argue that the linear tolerances to surfaces shown in Fig 3-29 are subject to more than one interpretation when applied to real part geometry.  When applied to the perfectly flat and parallel features of the drawing, the meaning is clear.  But when applied to real features that are not perfectly flat and/or not perfectly parallel, the meaning is not clear.  Does this make the linear tolerances wrong?  It depends on your interpretation of "shall not be subject to more than one interpretation". ;^)

The considered feature is not a feature of size - there are no opposed points, no local sizes, no Rule #1 boundary, no rules of any kind.  I understand that as an inspector you can't just throw up your hands and say that the requirement is ambiguous.  You have to do something, so you come up with practices like the 3-point setup you described.  But as Jim said, there is nothing in the standard supporting it.  A different inspector might use his caliper as a step gauge  and get different numbers.  They're all equally (in)valid because the specification itself contains uncertainty.

If the surfaces are produced very flat and parallel, the effects of this uncertainty are minimized.  Measurements taken using the 3-point setup and the caliper would closely agree.  This is often the case, and so the uncertainty and risk that the linear tolerances introduce often presents no symptoms.  If the assumption of perfect form and orientation is close to valid, then the linear tolerances provide a useful approximation.  But let's not pretend that it's fully rigorous.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

MechNorth (Mechanical)
7 May 10 16:09
Evan, don't forget about the new "irregular" features of size.

Have a good weekend on the coast.

Jim

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

axym (Industrial)
7 May 10 16:19
Jim,

Irregular features of size?  You mean those features that don't necessarily have opposed points, that we can't apply size tolerances to, that really aren't features of size?  Don't get me started on those!

Have a good weekend as well.  I'll be watching the Canucks and Black Hawks game tonight while the barbecue is going!

EJ

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

MechNorth (Mechanical)
7 May 10 16:23
Salmon?  I glaze with real maple syrup infused with coarse dijon, garlic and maybe some white wine if the spirit moves me.  Now I'm getting hungry again.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

fsincox (Aerospace)
7 May 10 16:25
I believe the caliper rule is one of those cultural myths. it is in no standard I have. (MIL-STD-8, 66,73,82,94,09) Anyone else find it in the standards?
Frank
axym (Industrial)
7 May 10 17:00
Jim,

I'm not really a fish guy, I think it's going to be some good old Alberta beef sirloins.

I'm the only customer in the butcher shop who specifies a profile tolerance for steaks instead of a thickness.  I wouldn't want them to use calipers for the measurement, would I? ;^)

EJ

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

MechNorth (Mechanical)
7 May 10 19:24
It's hard to get Alberta beef here without paying dearly with body parts.  There's just such a pleasant difference between grazed beef & the feed lot beef we get here.  Of course, if you did specify a thickness tolerance you'd still have perfect form @ MMC & a 2-point check to see they're not too thin.  Enjoy one with a shot o' rye for me.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

fsincox (Aerospace)
8 May 10 0:27
Thanks guys, there was a lot of valuable insights here in this last discussion for me, I hope you all have a good weekend.
Frank

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close