×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • 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!
  • Students Click Here

*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.

Students Click Here

Jobs

linear dimensions on geometricly toleranced print
3

linear dimensions on geometricly toleranced print

linear dimensions on geometricly toleranced print

(OP)
If a print has a section view with a linear dimension
describing a feature, does the view need to be set up for measurement purposes according to the geometric datum scheme or can I just measure it as a independent feature
because of the linear dimension callout?
This print has a combination of both linear dimensions and geometric callouts on the print.  

RE: linear dimensions on geometricly toleranced print

mack52,

   If the drawing shows a toleranced linear dimension, I would inspect the dimension.  

   Is this dimension a location of something, or a feature of size?

               JHG

RE: linear dimensions on geometricly toleranced print

I would say the dimension can be inspected without a specific setup, unless there's something on the element dimensioned that references one.

As always, the safest way would be to ask whomever created the drawing, if possible.


 

RE: linear dimensions on geometricly toleranced print

GD&T datums (such as "A" or "B" or other letters) are ONLY used for measuring items specifically calling out those datums.  So you can have a part labeled with A, B, C for some GD&T feature control frames, but the regular linear dimensions such as length or width that have plus/minus tolerances will not be measured with those datums in mind.

 

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

RE: linear dimensions on geometricly toleranced print

I have personally measured products without GD&T so many years ago at GM and we had to create a datum structure. We ended up looking at the part's function and how it assembled and then, accordingly, created the primary, secondary and tertiary datums for set up.

Today I would use a datum structure shown on the drawing as much as possible. Figure 3-29 in ASME Y14.5-2009 reflects linear dimensions coming from datum A which is the face of the part. It doesn't take much thought to figure out that one should measure the linear dimensions from datum A. Notice that this figure also has a combination of both linear and geometrical tolerances which provides a clear understanding of its function and mating relationship.

If there is no datum structure shown on the surface and there is a dimension from that surface to the other surface, one can  mark the original surface as an origin using the origin symbol. If one is using base line dimensioning, the origin symbol is not needed.

On a surface to a surface, we would set up the origin surface as a plane using a 3 points and then would sweep the other surface confirming that the full surface is not exceeding the requirement of the linear tolerance. This sure looks a lot like profile of a surface with the exception that we would probably not confirm this dimension on an ongoing basis. If the dimension had a function or mating relationship, I would utilize profile of a surface and then a variable checking fixture would be created and this feature would be confirmed on an ongoing basis.

Hope this helps.   

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

Referring to Fig 3-29 ('09), for the 41.3/41.1 linear-toleranced dimension, measuring from datum-A is not acceptable.  It's intended as a point-to-point measure, otherwise a profile tolerance wrt datum-A would have been specified.  Calipers are all that's required to verify this toleranced dimension.  Rule #1 doesn't apply because it's not a FOS because the boss is not directly opposite to the flange.

When done properly, and interpreted properly, GD&T (including linear tolerances) communicates the design intent; the tolerance values indicate criticallity, not the presence of a geometric control.

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

RE: linear dimensions on geometricly toleranced print

Jim:

As discussed before, there is nothing stating a point to point measurement requirement when a linear tolerance is applied. I don't know where you came up with that thought but I know we discussed this before.

Fig. 2-5 of ASME Y14.5-2009, page 27, reflects 2 parallel planes with a 12 +/- 0.4 dimension from the bottom to the top surface. Nothing on the top surface can be below 11.6 mm nor above 12.4 mm.

Please explain your concept of point to point measurement on this example and how one should take measurements?  

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

2 cents
    I believe that the example in question meets the definition of a Irregular Feature of Size as defined by 1.3.32.2. But Rule #1 still would not apply because 2.7.1 refers solely to Regular Features of Size. Why Irregular Features of Size are not included in 2.7.1 I can't figure out.
    Also. I think the idea of a pt-pt measurement derives from the FOS definition and concept of opposed elements. If you can't theoretically measure it with a ball mic or inside mics i.e. pt-pt, it does not meet the definition of a FoS (1994), of Regular FoS (2009).

caseynick

RE: linear dimensions on geometricly toleranced print

Quite right, CaseyNick.  As to why Irregular FOS are not included, consider a kidney shaped feature as an irregular FOS, or a CF as an irregular FOS; because of the reversals of geometry and discontinuities, it would be difficult(?!) to validate the perfect form at MMC and 2-point check at LMC (Taylor Principle).

Dave, picture the same article if it had been allowed to warp after injection moulding; opposed points could still be in +/- spec, but clearly your use of a defacto datum would be inappropriate.  If the the intent was that the indirectly opposed faces remain parallel, then some sort of geometric control would be needed (profile or parallelism); profile would locate the entire upper surface wrt datum-A (i.e. the simulator as apposed to the actual surface) and constrain parallelism and flatness as well.  Please, Dave, tell me where (in any ASME or other standard), it indicates that you get to pick a defacto datum at will?  Same question, as always, which you refuse to actually answer in this forum.  "Common practice" is not a standard.

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

RE: linear dimensions on geometricly toleranced print

Jim:

Reviewing Fig. 2-5, page 27 of AMSE Y14.5-2009 (also in 94 standard on page 26), where there are 2 planes that appear parallel but are not opposing. One might think of a stretched out "Z". There is an origin (where to measurements are take from) and a linear tolerance to the other surface of 12 +/- 0.4. Would this catch a warped surface? Can one apply your point to point contact in the fig. 2-5?

It is not my use of a defacto datum, it is reflected in the newest ASME standard. It states in 2.6.1 "The high points of the surface indicated as the origin define a plane for measurement." Is this inappropriate as you stated? In your opinion, is the 2.6.1 incorrect?

One certainly cannot measure the other plane with a micrometer or vernier and must set up on the plane as described. One would now sweep the other plane with an indicator and the use of height gauge and confirm that the surface is not below 11.6 nor above 12.4.

Where in the standard does it state "the tolerance values indicate criticallity, not the presence of a geometric control?" What section of the standard is that statement shown?

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

Dave, I think all this stuff you are talking about is only true when the "dimension origin" symbol is imposed.   In essence, that little circle calls out a datum (just like a GD&T datum: high points form the plane).  But all the other situations being discussed are of examples that lack that "dimension origin" symbol.

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

RE: linear dimensions on geometricly toleranced print

I agree with JP re: the dimension origin symbol.

Jim, I get your point re: irregular features of size and a normal rule 1 check in a case such as you suggest. In this case it would be convenient if IFoS were included in 2.7.1. Then the dimension in question could be checked as Dave describes for a valid perfect form at mmc check.

 Jim, What do you mean by "cf"?

RE: linear dimensions on geometricly toleranced print

JP:

That is not entirely true. It states in 2.6.1 the following: "Without such indication (meaning origin symbol), the longer surface could have been selected as the origin, thus permitting a greater angular variation between surfaces."

I believe that there are places on the drawing where a linear tolerance is applicable while in other areas, geometrical tolerances are better utilized. It depends upon the function and mating relationship of the feature.

 

  

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

CaseyNick -- I don't think Jim will mind if I jump in there...   The "CF" is a new modifier in the 2009 standard meaning "continuous feature."  See pages 29-30 of the new standard.

 

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

RE: linear dimensions on geometricly toleranced print

2.6.1 is a bit of an unfortunate section to cite, as Dimension Origin is kind of an oddball tolerancing tool that has more in common with geometric tolerances than with conventional plus/minus tolerances.  Section 2.6.1 also contains some misleading (and arguably incorrect) statements.

Dave is right that 2.6.1 says that the other surface could have been selected as the origin.  But it shouldn't say that!  There's nothing else in the standard that supports the idea of arbitrarily selecting one of the features controlled by a plus/minus tolerance as any kind of origin.  The statement just pops up out of nowhere and never comes up again.

This reference to selecting the origin unfortunately opens the door to "create your own datum structure" inspection practices that Dave (and countless others) have used over the years.  On the one hand I can sympathize with inspectors who are faced with plus/minus tolerances on non-opposed features, who must come up with some way of getting numbers from ill-defined and ambiguous specifications.  On the other hand, I can't sympathize with Dave's defense of plus/minus as the preferred method for features that don't have a "function and mating relationship".  An ambiguous spec is an ambiguous spec, regardless of the feature's function.

2.6.1 also states that the dimension origin concept does not result in the same kind of datum reference frame defined in Section 4.  This is also misleading, because the Dimension Origin tool defines a geometric control that is functionally equivalent to a Surface Profile control.  Both define a plane derived from the datum feature's high points, and an oriented and located tolerance zone for the other feature.  

I must also comment on Dave's comment that if baseline dimensioning is used then the origin symbol is not needed.  The Dimension Origin symbol defines something completely different from the implied origin defined by baseline dimensioning!  Let's be careful not get those two things confused.  There is already enough confusion between GD&T datum reference frames and drafting coordinate systems.  The two are not connected.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: linear dimensions on geometricly toleranced print

Good stuff, Evan.  I too felt that something wasn't right about 2.6.1, but wasn't quite sure how to say it.

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

RE: linear dimensions on geometricly toleranced print

Sorry for dropping out for a bit; tidying up some projects before leaving for vacation.

Dave, the use of tolerance value as an indication of criticallity is based in engineering and common sense.  If I have a workpiece that has tolerances of +/-1" & +/-.005", which do YOU think is more critical?  It really shouldn't have to be spec'd in Y14.5; it's not an engineering instruction book.  Now, that's not to say that all engineers & designers use common sense ... all the time ... maybe ever, but it is how I was taught and how I believe most of the engineering world was taught.  I believe that the comments re dimension origin answer the rest of your question.  By the way, if memory serves me, Evan works on the Y14 committee(s) responsible for the gd&t math standard, data reporting and maybe measuring standards.  I've found he is a good resource to ask questions about what is intended as far as metrology and mathematical definitions are concerned.  See y'all at the end of the month!

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

RE: linear dimensions on geometricly toleranced print

Evan:

I appreciate the fact that you would agree that the linear tolerance used in fig. 2-5 is comparable to profile of a surface. The linear tolerances shown in fig. 3-29 also are comparable to profile of a surface. So, why would one use a linear tolerance over a profile of a surface tolerance??? Conversely, why would one use profile of a surface over a linear tolerance?

There does appear to be a certainly amount of confusion over linear tolerances and how they can be applied and if they can be mixed with geometrical tolerances. Here is a statement from a forum contributor on the fig. 3-29 with the use of linear and geometrical tolerances on the same drawing - "Fig 3-29, yup, I think this is a good mix for this part's functionality."

The fact that you stated that sections of 2.6.1 are wrong would be your opinion. It is still in the standard and should be respected. It doesn't make any difference whether or not one is on the Y14.5 committee, 2.6.1 is valid to the 2009 standard.

Jim has stated that it is not the geometrical tolerance applied but its tolerance value that would reflect the importance to its function or mating relationship.

Using that thought, I am going to use a hypothetical example here. Let's say we reviewed a drawing where we have 4 flatness requirements on 4 surfaces with 3 having a tolerance of .010" while 1 has a tolerance of .005". Are we to assume that the 3 flatness requirements with a .010 have no bearing on it function while 1 with a .005" tolerance does? How does one know that fact when reviewing a drawing? I would suggest that one may not require 4 flatness tolerance in this situation but only 1. Why would a Designer place a requirement on a drawing that is not needed? So, is it the tolerance or the application of GD&T?

I have been arguing on behalf of all the Manufacturing and Quality personnel out there that review drawings. I hope that the features that have a bearing on its function and mating relationship are reflected so that we can concentrate on those features. Other features would only be confirmed at initial sample or on a infrequent basis.
    

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

"Why would one use profile of a surface tolerance over a linear tolerance?" Because it more clearly defines the drawing. If there was a datum surface designated and a profile of a surface tolerance on the dimension in question if fig 2-5 this whole discussion/debate would not have happened.

RE: linear dimensions on geometricly toleranced print

Dave,

You say that the linear tolerances shown in Figure 3-29 are comparable to profile of the surface, in the same way as the one in Figure 2-5.  Does that mean that you would use the Datum A surface as the origin when inspecting them, and measure to the other surfaces?

Regarding how frequently a characteristic should be inspected, I'm not sure that I agree with either you or Jim.  Geometric controls and small tolerance values are often associated with critical and functionally important features, but there is more to it than that.  The capability of the process to produce the feature within the required tolerance also has a major influence how frequently inspection is required.   

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: linear dimensions on geometricly toleranced print

axym, the more I think about this issue the more I feel like you that perhaps the more important thing when deciding which dimensions to heavily sample is process capability.

Of course, for this to make sense one has to assume that the person creating the drawing paid attention to the tolerances and that effectively they've done it in a way where they are all important.

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"?

RE: linear dimensions on geometricly toleranced print

Tolerance values should be as large as possible while still allowing the part/assembly to work.  Thus, a smaller tolerance value should be driven by the function.  I've seen crazy things like 0.5 mm on the contour of a foam cushion -- gaaaawww!!
 

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

RE: linear dimensions on geometricly toleranced print

Quote (Belanger):

Tolerance values should be as large as possible while still allowing the part/assembly to work. Thus, a smaller tolerance value should be driven by the function. ...

   This discussion about critical dimensions bothers me.  To me, as I prepare drawings, you are absolutely correct.  

   The fabricator is supposed to meet all the tolerances on the drawing.   The sloppy dimensions can be just as critical as the tight ones.  

   I used to work with a guy who left notes on his drawings telling fabricators to pay particular attention to certain dimensions on the drawing.  The obvious implication is that the other dimensions and tolerances do not matter, and there is no need to meet them.  How does our inspector reject shoddy work?

   I have run up against sort of an interesting drafting problem.  I was dimensioning some holes tapped in a machined plate, for cable ties.  I actually do not care where cable ties are located.  A positional tolerance of Ø5mm would be adequate for me.  On the other hand, there is no way for a machinist to take advange of this.  There is the significant possibility that someone will look at the the holes, and use them for a fabricated bracket, thus imposing a requirement for accurate tolerances, not met by my drawing.  I called up a tolerance of Ø0.2mm.

               JHG

RE: linear dimensions on geometricly toleranced print

drawoh, I tend to agree with you on the 'critical dimensions' issue.

The problem in your last paragraph is also familiar.  I tend to pick a fairly loose figure well within anticipated process capability, even if functionally it could be looser.

This 'future proofs' it so some extent, for later modifications.

It also shouldn't increase cost as it's 'well within' process capability.

Now the gray area is that if they happened to slip up, and exceed your already generous tolerance, you probably wouldn't reject the part, which generally one might say suggests the drawing should change.

I've got the process selection wrong before too.  I'd set it at something like +-.030", which for most machining processes I anticipated to be ample.  Well they had a capacity issue and decided they wanted to rough the outline dimensions on the bandsaw (or maybe it was a round part and they flame cut it - my memory fades).  For this the relatively loose tolerance wasn't loose enough so we had to do a drawing change.

I'm a bit more generous with such tolerances now.

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"?

RE: linear dimensions on geometricly toleranced print

drawoh:

All dimensions must meet the criteria on the drawing but ones that have a function or mating relationship should be monitored (controlled) more often. No manufacturing company will confirm each dimension on each product and that is a fact. How one dimensions the part provides the information needed to control functionally important dimensions.

Your example of only requiring a diametrical tolerance zone of 5 mm but placing a tolerance of 0.2 mm is a typical example of the kind of drawings floating the shop floor today. If you had placed a MMC with the positional tolerance, then manufacturing may end up considering it a functionally important feature and have a checking fixture made for the location of the holes. What a waste of time and $$. If you left the extremely tight positional tolerances in RFS, then I know it would only be checked using variable measuring methods on a limited basis.

Has the application of positional tolerances on these holes assisted in making the drawing clearer or has it added to the confusion?  

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

Yes, some dimensions require monitoring more than others, but I disagree that the drawing defining the part is the best place to note which is which.  QA often makes their own documents to control part quality, such as ballooned inspection drawings, based on the original part drawing.  There is nothing to prevent them from doing the same defining what dimensions get monitored how often.
This comes back to the purpose of the original drawing; to completely define a part without ambiguity.  Part definition, not manufacturing process definition.  Adding notations of any kind that do not aid in part definition are superfluous and should be documented elsewhere.

"Good to know you got shoes to wear when you find the floor." - Robert Hunter
 

RE: linear dimensions on geometricly toleranced print

ewh:

You are absolutely correct about QA developing a Control Plan. We would get together with the Customer QA and ask such questions as "How does the part fit and function?" since the drawing did not always reflect the function and mating relationship of the part.

I would never ask about adding notations but would suggest that design intent including applicable GD&T is reflected on the drawing.  

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

dingy2,

   We subcontract fabrication, but we inspect in-house.  I can tell our inspector all sorts of things I would never tell the machine shop.  My assumption is that Ø0.2mm positional tolerances are easily achieved.  The cost of unneeded accuracy in my situation, is tiny.

   In your environment, I would make the tolerance sloppy.

   The holes are tapped, so MMC does not help me.   

               JHG

RE: linear dimensions on geometricly toleranced print

We got a bit sidetracked with the discussion of inspection frequency, which is a very important but separate issue.  We didn't really answer the "plus/minus versus GD&T" questions from the discussion of Figure 3-29.

Dave, you said that the linear tolerances in Figure 3-29 are comparable to profile of a surface tolerances and posed the question of why one would pick one method over the other.  Caseynick replied that profile of a surface more clearly defines the drawing.  I agree, but what are the details?  

Surface profile tolerances would each designate one feature as the datum feature and create a well-defined tolerance zone for the considered feature.  This tolerance zone would control the form, orientation and location of the considered feature but the datum feature would not be controlled in any way.  The meaning of surface profile is well defined in the Y14.5 standard.

If linear tolerances were specified, as they are in Fig 3-29, exactly what do we get in terms of control of the features?  This is where it gets interesting.  These features are not well-behaved features of size, because the surfaces are not fully opposed:

The 35 36 and 25.4 25.5 dimensions are between surfaces that directly oppose each other in some areas but not everywhere.

The 41.1 41.3 dimension is between surfaces that point in opposing directions but do not directly oppose each other anywhere.

The 9.4 9.6 dimensions are between surfaces that point in the same direction and are therefore not opposed anywhere.

The 6.1 6.6 dimension is between a surface and a cone-cylinder intersection line.

So exactly what do these linear tolerances define in terms of control of the features?  Can any of these dimensions be considered "size dimensions" to which the Rule #1 perfect-form boundary would apply?  Can the actual local size requirement be applied to any of them?  If the answer to these questions is no, then what does apply?

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: linear dimensions on geometricly toleranced print

Evan:

I would set up a plane on the bottom surface which is datum A and then sweep any plane that has a linear dimension from that surface just as one would using profile of a surface. This concept is shown in fig. 2-5.

Dimension 9.4-9.6 is shown from the other end so I would create a plane on the smaller end and the check around the shoulder in various areas confirming that they do, indeed, are not outside the 9.4-9.6 criteria.

That fact that these dimensions are not profiles indicate that they may not have anything to do with the part's function and relationship and would be confirmed infrequently. All dimensions shown in the feature control frames must have an influence on its function and mating relationship and would be confirmed on a regular basis.  

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

Dave,
Once again, if you're going to keep posting your recommendation to use a defacto datum, please justify it based on a standard.  You keep challenging others to prove their case, and we either provide the proof or retract, but you have yet to prove your case on this matter.  This is a recurring theme and scenario.  It concerns me because there are comparatively inexperienced people using this forum to up their game based on the Y14.5 standard, not a personal opinion.  As you are a GDTP, your voice carries extra credibility but pulling in your own opinions, uncorrelated to the standard.

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

RE: linear dimensions on geometricly toleranced print

Hi Jim:

Each time I respond, I reference a figure or figures as I have in the last post but I do not align myself with the philosophy of "every dimension must be covered by GD&T". I did mention figures 2-5 and 3-29. As a matter of fact, you mentioned that the following "Fig 3-29, yup, I think this is a good mix for this part's functionality".

In the foreword of the standard it states "it is even more important that the design more precisely state the functional requirements". I am attempting to follow that concept.

I was asked how I would measure that linear dimensions shown in figure 3-29 and I answered based on both the standard and my years measuring parts using a CMM.

So, Jim, how would you measure that linear dimensions shown in figure 3-29? The 9.4-9.6 dimension would be most interesting.


 

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

The closest measurement to the intended point-to-point would be using a set of calipers across the top and bottom.  Not truly a point-to-point, but the closest you'll get that I've come across.  Measuring from a defacto datum is not indicated in the standard.  To advocate that method is not valid to the standard.

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

RE: linear dimensions on geometricly toleranced print

Dave,

Jim is right, your last post contained several statements that represent your personal opinion.  The connection you make between geometric tolerances, function and mating relationship, and inspection frequency does not have any basis in the standards.

I still challenge your use of Figure 2-5 to justify choosing a de facto datum for linear tolerances.  The Dimension Origin tool shown in Fig 2-5, with the circle at one end of the dimension, is not interchangeable with baseline dimensioning.  We don't see the Dimension Origin circle symbol on the linear tolerances in Fig 3-29, so the high-point-plane origin described in 2.6.1 does not apply to them.

So what does that leave us with?

There is a note on Page 27 of Y14.5-2009, right underneath Fig 2-5.  The final sentence in the note is:

"Locating features using directly toleranced dimensions is not recommended."

Why would that statement be there?  I think it's because directly toleranced dimensions like the ones in Fig 3-29 don't provide a clear definition of what the control over the features is.  There is specification uncertainty.  There are no rules in the standards to clarify what the considered feature is, what the tolerance zone is, or what the origin of measurement is.  The inspector must invent something based on other knowledge of the part, "tribal knowledge", assumptions, or guesswork, as Dave and countless others have over the years.

So how are non-rigorous specifications like these still workable in industry?  Any thoughts?

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: linear dimensions on geometricly toleranced print

Jim & Evan:

Figure 2-5 reflects the surface using the origin symbol where the 12 +/- 0.4 dimension. The bottom line of 2.6.1 states "Without such indication, the longer surface could have been selected as the origin, thus permitting a greater angular variation between surfaces." Please note that the feature is not a feature of size in any stretch but a distance between 2 planes.

Using that concept, I wonder which surface I should take my readings from on fig. 3-29? Obviously, I would take them from datum A. I really don't know where this point to point measuring concept is derived but I see a surface (origin plane) to a surface (plane).

Evan:

You should have stated that complete note where the statement "Locating features using directly toleranced dimensions is not recommended." was taken out of context.

Bottom on page 26 it states:

Note: When basic dimensions are used, the is no accumulation of tolerances. A geometrical tolerances is required to create the tolerance zone. In this case, the style of dimension (chain, baseline, direct) is up to the user. Locating features using directly toleranced dimensions is not recommended.

The full statement was discussing geometrical tolerances using basic dimension in which certainly makes sense. Certainly, one would not use directly tolerances dimensions in this situation.

8.2.3 Profile Tolerance as General Requirements

This covers your default profile tolerances but  8.2.1 states "A profile tolerance may be applied to an entire part, multiple features, individual surfaces or to individual profiles taken at various cross section through part." So, there is an option to place a general profile tolerance but it is not mandatory. If you use a general profile tolerance, is the datum structure valid for all the features??

I have read (was implied) where if one does not place a default positional and profile tolerances, your company may not be modern (with it). It appeared to be blasphemy that I would actually question this concept since I am a GDTP and have been training in this subject since 1988. Possibly, I might be just old fashion or out of step but I am one of the few that offer live online GD&T training. I don't think that is old fashion.

Does your drawing truly reflect the design intent? Are the part's function & mating relationship clearly shown using GD&T in FCFs or are they all part of the default tolerances?

This, thankfully, is my last input on this subject so beat away guys.       

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

Dave, again, you avoid answering the question directly.  Where do you find your position of using defacto datums in any standard?

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

RE: linear dimensions on geometricly toleranced print

Gentlemen:

I am now going to eat dirt.

In the forward on page vi, I have noted "design more precisely state the function requirements." but there is more that I should have stated.

It states below the above statement "To accomplish this it is becoming increasingly important that the use of geometric and dimensioning (GD&T) replace the former limit dimensioning for form, orientation, location, and profile of part features. This revision contains paragraphs that give a stronger admonition that in the past that the fully defined drawing should be dimensioned using GD&T with limit dimensioning reserved primarily for the size dimensions for features of size."

This the concept that my fellow colleagues were arguing but could not find anything in the standard to support their claims but it is here.

For that, I will give both Jim and Evan a star.  

Dave D.
www.qmsi.ca

RE: linear dimensions on geometricly toleranced print

Tks Dave.  Very gracious, and appreciated.
Jim

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

RE: linear dimensions on geometricly toleranced print

Dave,

That is very gracious of you, and you don't need to eat dirt.  I'm not sure that Jim and I deserve a star though - obviously neither of us stated our case well enough to convince you.

Y14.5-2009 does admonish the use of limit dimensioning for purposes other than size dimensions, but that use is still illustrated in the standard.  The infamous Figure 3-29 uses limit dimensioning for the location of part features.

That is why we need to examine for ourselves what the consequences are when plus/minus or limit dimensions are used on features that are not features of size.  It's case-specific.  There are consequences, such as the drawing not being "fully defined" in terms of bulletproof definition of what is controlled.  In some cases we can live with these consequences and in other cases we can't.  

That's why plus/minus tolerances are used extensively and are not going to go away.  The pros outweigh the cons in many situations.  Opinions?

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

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!


Resources