Must profile be applied to a basic profile?

[Belanger]

Several things have popped up in various threads that always seem to leave this question lingering: When a profile tolerance is applied, is it required for the dimensions defining the shape to be basic?
We all agree that the dimensions defining the location of the feature do not have to be basic (often they are). So please realize that I'm talking about the shape -- such as the radius of a curve: I would say that the radius must be basic if you're going to apply a profile tolerance to such a curve.

See the attached picture for the specific question to be debated. Would you say the two drawings mean exactly the same thing? Or would you say the second drawing does not comply with Y14.5?

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

 

[Belanger]

drawoh -- your last scenario is totally different. I presume everyone on here would agree that a profile tolerance larger than the other dimension it's applied to would make no sense. My question was just the opposite: a profile tolerance smaller than the other tolerance which defines the very shape.

CH -- this part is directed at you also... Let's go back to drawoh's first statement... "Anything conforming to the 0.4 profile tolerance, easily conforms to the R42±0.5." But since we're dealing with curvature, what exact curve must that profile zone be built around? Drawoh would say 42.0. I think CH would say any radius between 41.5 and 42.5. Thoughts?

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

 

[djhurayt]

When you have directly toleranced size, profile doesn't control size anymore. It doesn't have as much power as if it was controlling basic dimensioned feature. That's what I meant.

I TOTALLY disagree. CH you and I both posted the parargraph directly from the spec.
Where used as a refinement of a size tolerance created by toleranced dimensions, the profile must be contained within the size limits

My interpretation of this is that it is exactly what it says it is "a refinement of a size tolerance". Meaning that if my dimensional tolerance allows the part to be ±0.5 (using OP's original example)
1) the part is never allowed to biggger or smaller than the an assumed nominal of 15 by 0.5
2) however the profile call out requires the largest and smallest diameter on the part to be within 0.2 of each other

 

[CheckerHater]

@ Belanger:

I already said it once and I will say it again - the way it's shown on your picture it simply makes no sense.

 

[CheckerHater]

@djhurayt:

This is how "refinement" works.

This is why both +/-0.1 and +/-0.05 are required in example of form.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[djhurayt]

CH, just an FYI, it is hard to tell who you are responding to, maybe you could add a name or initial of the poster you are referring to at the beginning of your statements

Belanger,
I think it depends on how the toleranced dimension is written.

42±0.5:
Is pretty straight forward that the target is for the radius to be 42 but is allowed to vary by ±0.5; however the profile callout makes the ±0.5 useless because (by definition) the profile is a refinement of the tolerance dimension. Therefore the ±0.5 might as well not be there at all and this could be a basic dimension with the profile allowing it to be as small as 41.8 or as big as 42.2 and meet the drawing requirements. Or one could just drop the profile call out and make the radius dimension 42±0.2 and have the same thing.

Now if the radius dimension was stated as 41.5-42.5:
This scenario if different and it would seem that the part could be as small as 41.5 or as large as 52.5, but the profile tolerance will require that whatever the largest and smallest diameters are (within the ±0.5) they must be within 0.4 of each other.

???

 

[djhurayt]

CH, I think I see our difference of opinion from you last attachment.

I was interpreting the par. 8.2 toleranced dimension referecne as still applying to the "true profile".
Your attachement indicates that you think this part of par. 8.2 applies the the "real (as manufactured)" part surface.

???, I'm not really sure what is correct at this point.

 

[CheckerHater]

@djhurayt:

Wow. How you apply toleranced dimension to "true profile"?

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[JNieman]

I was initially stumped as to why one would want a size tolerance on a feature that is further refined by a profile tolerance. However, one very good example would be if the profile was only applied to a portion of the feature. The whole radius, for example, may only need to be +/-0.5 but for this very critical area near top-dead-center, maybe the designer would require +/-0.01 profile. That's a logical (in my mind) situation where a size tolerance could be applied to a single feature, with a "refined" profile tolerance. That could make a significant difference in the manufacturing.

I have nothing else to add, though, I've just been reading along and appreciating the education, so far. Thank you

 

[djhurayt]

CH, I think that is where my confusion starts. And seem to be related to a point in this discussion about "nominal" values of toleranced dimension. I was under the assumption (right or wrong) that if the toleranced dimension is a +/- then the target is the nominal and would therefore be used in the true profile shape of the part. But when the toleranced dimension is a max/min the target is not clear. Now, what you seem to be saying is that in the case of a feature that is dimensioned with a toleranced dimension the profile applies to the actual lay of the surface as in your last attachement and not some sudo-true profile.

 

[JNieman]

That makes a lot more sense. I initially missed that image in CH's post. So in other words, it's exactly akin to a thickness being dimensioned with a tolerance, with a flatness applied to either side, greater than the size tolerance... it's just using profile so as to include non-flat features. I hope I understand that right.

 

[drawoh]

Belanger,

Profile tolerances control everything. As such, if there is a profile tolerance on something and one or more other controls, the other controls refine the profile tolerance. I don't see how you can apply a profile tolerance as a refinement of something. I understand the concept. I just don't think it applies to profile.

...

CH -- this part is directed at you also... Let's go back to drawoh's first statement... "Anything conforming to the 0.4 profile tolerance, easily conforms to the R42±0.5." But since we're dealing with curvature, what exact curve must that profile zone be built around? Drawoh would say 42.0. I think CH would say any radius between 41.5 and 42.5. Thoughts?

If you apply a profile tolerance to a radius, you must have a nominal radius. Given a dimension of R42[±]0.5, I would guess 42 as the nominal radius. A case can be made for R42.5!

--
JHG

 

[Belanger]

drawoh -- I think the key would be in paragraph 8.2, as CH highlighted. Maybe refinement isn't the ideal word, but profile can certainly be a smaller tolerance that resides inside a larger tolerance. For instance, see Fig. 8-27 of the standard. There is a toleranced location dimension (height) of 80±0.2. The profile tolerance then controls form and orientation (but not location/size) of the top surface. Thus, profile is a "refinement" of sorts: it controls orienatation within the already-existing location.

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

 

[CheckerHater]

@All:

Where exactly does it say that toleranced dimension implies "nominal" or "target" value?

As far As I can remember, all different ways to represent the tolerance (limits / bilateral / unilateral) have exactly the same meaning.

Could somebody quote the actual standard?

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[Belanger]

CH -- you said for my first graphic that they mean the same thing (because it's a FOS). But in the other graphic of just an arc you said the radius should be basic, because it's not a FOS. So to recap, I'll post one other graphic... see attached.

If I'm hearing you, the first picture (arc) is not allowed per Y14.5, but the second picture (circle) is allowed.

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

 

[CheckerHater]

@Belanger:

I'd say it would be interpreted the same way as cylindricity, but it won't provide any special benefits, which may be the reason you don't see it very often

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[JNieman]

FYI:
Reading 14.5-2009, Chapter 2 consistently refers to the stated dimension as the "nominal" value when using bilateral or unilateral tolerancing. The section on 'Limits' dimensioning has no mention of the word nominal.

 

[drawoh]

Belanger,

I am looking at Figure[ ]8.27 here, and I am finding it weird, although it makes sense. The 80[±]0.2 is a measurement with calipers across the faces. The second part of the figure does not account for the profile tolerance. The profile tolerance controls the top face with respect to datum[ ]A, datum[ ]A being whichever three points of the surface contact your flat granite block. That bottom face could be way out of flat.

Why would I do this? If I want some face to be profiled to 0.07mm with respect to the opposite face, I am going to pay attention to the opposite face. It is going to be very flat, or there will be three datum targets, or there will be some other unambiguous geometry to define the datum.

--
JHG

 

[CheckerHater]

@JNieman:

Yes, and ANSI B4.2 uses term "basic".

I guess I was unclear. Where does it say that "nominal" represents the "target" and limits dimension somehow have special meaning different from "-lateral" ones?

What disproves (or proves) that shown ways of dimensioning are not equal?

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[axym]

Hi All,

Wow, this has become quite a thread. The discussion is similar to previous discussions over the years in other forums, and in the standards committees ;^/. Sigh. I've also had to think about how plus/minus tolerances affect profile tolerances for committee work fairly recently, so this is unfortunately familiar ground. When plus/minus tolerances are involved, the discussion inevitably grinds down into opinion-based interpretation because plus/minus tolerances are ambiguous and don't have rules.

With regards to the original question, I would say that the two drawings comply with Y14.5 and would apply the same tolerance requirements. I wish that it were otherwise and I don't think that combining +/- with profile is a good practice, but Y14.5 does currently allow it. CH's references are correct, and there are figures showing examples.

There is a very mixed message in the standard. Profile is mainly described in terms of true profiles being defined using basic dimensions, and I would say that this is definitely the best practice. Nevertheless, there are figures showing profile tolerances combined with plus/minus size tolerances. In Y14.5-2009 see the following:

-Fig. 8-17 where profile controls "conicity" but not size. This can be extended to apply to JP's initial cylindricity/profile example, since a cylinder can be thought of as a cone with an included angle of zero.

-Fig. 8-18 where profile controls form, orientation, and location (but not size). I would say that the appropriate characteristic for this type of control would have been total runout, not profile. But Y14.5-2009 does not allow (or at least does not show examples of) total runout on conical features. Part of the reason for this is lack of agreement on how plus/minus tolerances would be interpreted (such as the 45 +/- 2 degree cone angle in Fig. 9-2 for circular runout). Some argued that the nominal angle represents the "true geometric shape" and would be different if the tolerance was unilateral (43 +4 -0), others argued that no true geometric shape is defined, others argued that the cone angle would have to be basic. This is a major example of how the ambiguities of old-school plus/minus tolerancing clash with geometric tolerancing.

-Fig. 8-27 where profile controls form and orientation, but not location. In this case the location is height, and is controlled by a directly toleranced size dimension. I've ranted about this example before, on this forum, probably more than once. The only "explanation" given is that "In this application, the datum references only orient the profile of a line tolerance". We are left to wonder exactly how this happens.

These figures are problematic for several reasons. One reason is that they are example-based and case-specific. Without a general description of what a directly toleranced dimension does to a profile tolerance zone, we are on our own with examples that are not shown. Another reason is that these figures undermine Y14.5's own directive of using geometric tolerances to locate features. The plus/minus tolerances introduce non-rigorous and ambiguous aspects such as the orientation relationship between the size dimension and the geometric tolerance zone and DRF (if present). Another problem I have with 8-17 and 8-18 is that the size dimension is on a surface in which the points are not fully opposed - this would introduce additional errors and uncertainty (especially if the included angle was significantly larger than the 15 degrees in the figure).

Regarding whether or not profile can be applied with a directly toleranced radius, who knows? There is no figure showing this, so we really can't say for sure.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[Belanger]

Thanks all. Yes Evan, that was the same dissonance I found in the standard, which is why I asked the initial question. They show a figure such as 8-18, which might not always square 100% with some of the other things we profess about profile. And yet, unless they come up with another symbol called conicity, it seems to be the only way to control form on a cone as separate from size.

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