linear dimensions on geometricly toleranced print 3

[mack52]

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.

 

[drawoh]

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

 

[SteveMartin]

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.

 

[Belanger]

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

 

[dingy2]

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.

http://www.qmsi.ca

 

[MechNorth]

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

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.

http://www.qmsi.ca

 

[caseynick]

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

 

[MechNorth]

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

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.

http://www.qmsi.ca

 

[Belanger]

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

 

[caseynick]

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"?

 

[dingy2]

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.

http://www.qmsi.ca

 

[Belanger]

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

 

[axym]

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.

http://www.axymetrix.ca

 

[Belanger]

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

 

[MechNorth]

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

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.

http://www.qmsi.ca

 

[caseynick]

"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.

 

[axym]

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.

http://www.axymetrix.ca