When applying tolerances using MBD, is it valid to define a plus/minus tolerance on a feature of size, say a hole, and allow the general tolerance to control its position? The general tolerance is a profile tolerance that is listed in the notes as applying to all features and surfaces unless otherwise specified. I have been unable to find information in 14.5 or 14.41 related to this. Can a profile tolerance just control position of a feature if it's size tolerance is already defined?
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Default Position Tolerance for Features of Size
- Thread starter goz304
- Start date
CheckerHater
Mechanical
@belanger:
I agree with you on more positions then you may think.
For example, I don't like the idea of the same feature having toleranced and basic dimensions at the same time.
I believe profile should be used only where profile can do.
But unfortunately today profile is used to control form, orientation, acts as a substitute for runout (some time
)
Just like in ISO position is used to control flat surface where profile can do, in ASME profile is used where flatness or straightness can do.
As long as it stays this way, we have to be aware of it and put it to best use (just an opinion)
@greenimi:
I believe G. Henzold understands GD&T better then both of us. Sorry to be rude.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
I agree with you on more positions then you may think.
For example, I don't like the idea of the same feature having toleranced and basic dimensions at the same time.
I believe profile should be used only where profile can do.
But unfortunately today profile is used to control form, orientation, acts as a substitute for runout (some time
)Just like in ISO position is used to control flat surface where profile can do, in ASME profile is used where flatness or straightness can do.
As long as it stays this way, we have to be aware of it and put it to best use (just an opinion)
@greenimi:
I believe G. Henzold understands GD&T better then both of us. Sorry to be rude.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
The default profile contains a tolerance and is UOS; the hole callout has an explicit tolerance, and therefore is "otherwise specified". Given that any queried dimensions are considered basic, a positional control would have to be applied to the hole callout, or an additional default positional tolerance UOS would need to be provided.
"Know the rules well, so you can break them effectively."
-Dalai Lama XIV
"Know the rules well, so you can break them effectively."
-Dalai Lama XIV
CheckerHater
Mechanical
@greenimi: Could you point out EXACTLY what is wrong with G. Henzold’s illustrations?
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
CH,
What you are asking is to hijack the discussion. The OP won't be happy
Anyway, I am not sure the first two pictures (form and orientation) are the best practice and in agreement with Y14.5
(Yes, I know the orientation is "almost" the same as the one in the standard, with a big difference of profile of a line instead of a profile of a surface)
As you already know, there are many many discussions posted in this forum about the idea of combining ± with profile. Again, the issue is with the first two figures: form and orientation.
Disappointing to see it in a book from a subject mater expert, regardless of his name.
I know, I keep those SME's to a higher standard, specially when a public (published) document is released to the world and consequently money are made from that process.
What you are asking is to hijack the discussion. The OP won't be happy
Anyway, I am not sure the first two pictures (form and orientation) are the best practice and in agreement with Y14.5
(Yes, I know the orientation is "almost" the same as the one in the standard, with a big difference of profile of a line instead of a profile of a surface)
As you already know, there are many many discussions posted in this forum about the idea of combining ± with profile. Again, the issue is with the first two figures: form and orientation.
Disappointing to see it in a book from a subject mater expert, regardless of his name.
I know, I keep those SME's to a higher standard, specially when a public (published) document is released to the world and consequently money are made from that process.
I don't have a +/- tolerance applied to a basic dimension. I have a toleranced size dimension applied to a cylindrical surface that also happens to have its basic geometry defined by a 3D model. The equivalent non-MBD scheme would have two dimensions, one of them basic and one of them toleranced, applied to a cylindrical surface.
Whatever you want to call this, why do you see it as a problem for drawing interpretation? Why shouldn't the toleranced dimension be considered independently from the profile tolerance and basic 3D model?
The toleranced size dimension is essentially two independent requirements: UAME size must be 8.3 or more, and all actual local sizes must be 8.9 or less. The profile tolerance requires that all surfaces fall between two boundaries, each with a uniform offset of 0.6 from the true profile defined by the 3D model. For the hole, those boundaries are cylinders of diameter 7.4 and 9.8.
These requirements are controlling different aspects of the geometry. The limiting values are also different. Most importantly, it's possible to satisfy them all simultaneously. Why do you call this a conflict?
It's hard to be specific without a proposed implementation to discuss. I think the most likely difficulty would be unambiguously identifying which features the tolerance applies to.
pylfrm
pylfrm said:
You have a toleranced dimension applied to a cylindrical surface that also happens be be defined as a basic geometry. How is that not what it says it is?
Are you thinking that a basic geometry is different than a basic dimension?
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
Burunduk
Mechanical
- May 2, 2019
- 2,563
Pylfrm and others,
I don't get what the controversy is about. If it was a fully defined drawing and not MBD, would it be OK to have +- dimension AND basic diameter AND Profile referencing datum features on a hole? The answer is no as the Profile fully defines the feature including the size of it. That is unless you want to consider the profile as some odd "refinement" of size that also controls location and orientation - but that probably makes the size dimension redundant.
Same for MBD.
The OP should either skip the size limits and leave everything including size and location to be controlled by the general Profile, or add the +- dimension + Position and consider size, location and orientation of the hole "otherwise specified".
I don't get what the controversy is about. If it was a fully defined drawing and not MBD, would it be OK to have +- dimension AND basic diameter AND Profile referencing datum features on a hole? The answer is no as the Profile fully defines the feature including the size of it. That is unless you want to consider the profile as some odd "refinement" of size that also controls location and orientation - but that probably makes the size dimension redundant.
Same for MBD.
The OP should either skip the size limits and leave everything including size and location to be controlled by the general Profile, or add the +- dimension + Position and consider size, location and orientation of the hole "otherwise specified".
tim_member
Aerospace
True MBD (with all tolerances digitally consumed downstream) shouldn't be defining tolerances in general notes in first place.
To me, a basic dimension is a number*, often with a box drawn around it, which is attached to some geometry (surfaces, axes, etc.) with dimension lines and extension lines or a leader line. A "dumb" CAD model** generally does not contain any dimensions in this sense.
*Actually not a pure number, but a quantity with a numerical value and a unit, the latter often defined in a separate note.
**Formats such as STL or (more commonly) STEP AP203 Edition 1.
**Formats such as STL or (more commonly) STEP AP203 Edition 1.
I'm using "basic geometry" as a catch-all term for true profile, true position, etc.; essentially any geometry that is defined by a CAD model that has been identified as basic or by basic dimensions on a drawing.
Sorry about the terminology nitpicking. When I first read your statement partially quoted in my previous post, I assumed "it" referred to "basic dim", but I now realize you may have been referring to "true profile" in your preceding sentence (excluded from the quote). Applying a tolerance to a basic dimension is generally contrary to the definition, and I want to be clear that I am not suggesting that here.
What I am suggesting is that it's acceptable to apply a toleranced dimension to a portion of a true profile (regardless of whether a profile tolerance is also applied), and that it's acceptable to apply a profile tolerance to a portion of a true profile (regardless of whether a toleranced dimension is also applied). The two tolerances seem completely independent to me. I don't see how a conflict is possible unless the tolerance values are chosen poorly.
You apparently disagree with some portion of this, but it's not yet clear to me what that might be. Are you saying there's a conflict between the toleranced dimension and the basic dimension, or between the toleranced dimension and the profile tolerance? And are you saying it's just bad practice, or actually prohibited by the standard? If the latter, where?
I regret involving MBD in my earlier example. Here's one which is much simpler and hopefully better:
Imagine a drawing that shows a steel ball with the following specifications:
spherical diameter 5.5 +/- 0.3 (call this "tolerance A")
spherical diameter 5.5 BASIC
[box]profile[/box][box]0.4[/box] (call this "tolerance B")
spherical diameter 5.5 BASIC
[box]profile[/box][box]0.4[/box] (call this "tolerance B")
If you like, imagine the basic dimension and profile tolerance are applied in one view, and the toleranced dimension is applied in a different view.
Perhaps "customer A" only cares about "tolerance A" and "customer B" only cares about "tolerance B". It's possible for a part to meet both tolerances simultaneously, so I want a single product that I can sell to both customers and simplify my inventory. It's also possible for a part to meet "tolerance A" and not "tolerance B", or to meet "tolerance B" and not "tolerance A", so neither tolerance is redundant. Perhaps my manufacturing process results in balls with profile error of approximately 0.35, making it impractical to reduce the profile tolerance to 0.3 and eliminate the toleranced dimension (even though I might prefer to simplify the drawing by doing exactly that).
I think we'd all agree that each tolerance would be fine by itself on its own drawing. It would also be possible to inspect a part against two different drawings. So why would combining them on one drawing be an issue?
pylfrm
Between the toleranced dimension and the profile tolerance.pylfrm said:
There is a conflict when a profile tolerance is applied in the manner you describe: to a geometry that is also defined by a plus/minus tolerance. Notice (CH) that I'm referring to the profiled shape itself having a plus/minus, not the relationship of that profiled shape to any datum references.
As an example, take Figure 8-6 of the 2009 standard. Suppose the R12 defining the curved portion on the left were changed from a basic R12 to a non-basic R12 +/- 0.5. (Keep the existing profile tolerance of 0.12.)
That would be OK to you?
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
No. Eliminating the basic dimension (by changing it to a toleranced dimension) would leave the true profile undefined.
I am suggesting that the following would be acceptable:
[ul][li]Leave the R12 BASIC dimension unchanged.[/li]
[li]Apply a second dimension to the same surface: R12 +/- 0.5.[/li][/ul]
I don't know how else to say this.
pylfrm
Double dimensioning? (Sharp intake of breath!) Gasp!
I think it runs afoul of the one-interpretation requirement; otherwise it's two different allowable sets of outcomes for one designated item. The sets may overlap, but they aren't identical.
I think it runs afoul of the one-interpretation requirement; otherwise it's two different allowable sets of outcomes for one designated item. The sets may overlap, but they aren't identical.
pylfrm -- so with your modification made upon Fig. 8-6, the result is that the radius of that curve is allowed to be as much as 12.5, but at the same time the radius of that curve is only allowed to be as much as 12.06.
Sounds like an internal conflict within that drawing.
If I gather what you're trying to achieve, though, then it might be a good candidate for the new dynamic profile modifier (refining form alone). But in the 2009 standard, it's just, well, a conflict.
Sounds like an internal conflict within that drawing.
If I gather what you're trying to achieve, though, then it might be a good candidate for the new dynamic profile modifier (refining form alone). But in the 2009 standard, it's just, well, a conflict.
Burunduk,
A perfect sphere of diameter 5.89:
A perfect sphere of diameter 5.79 except with a single flat spot bringing the local size down to 5.21:
3DDave,
Gasp indeed.
Each tolerance does have a different set of allowable outcomes, and that is exactly the point. Compliant parts are in the intersection of those sets. Just like every other drawing with multiple requirements, they must all be met simultaneously.
The interpretation of each tolerance is not affected by the presence or absence of the other. If each tolerance has only one interpretation when used independently, then that should remain true when they are both applied on the same drawing and to the same surface. And if each tolerance has only one interpretation, then so does the drawing as a whole.
Belanger,
I only described the modification to Fig. 8-6 to emphasize that the basic dimension should not be eliminated if the profile tolerance is to remain valid. The specific tolerance values used in Fig. 8-6 make it an unreasonable example because any part that satisfies the profile tolerance will also satisfy the dimension tolerance.
In the examples I presented, the tolerance values were intentionally chosen such that it's possible to satisfy only the profile tolerance, only the dimension tolerance, both, or neither. The second example with the spherical part should make this somewhat more clear.
To me, two tolerances conflict only if it's impossible to simultaneously satisfy both. I guess you are using a different meaning of "conflict".
pylfrm
A perfect sphere of diameter 5.89:
- meets the profile requirement (in by 0.01)
- does not meet the 5.5 +/- 0.3 requirement (out by 0.09)
- does not meet the 5.5 +/- 0.3 requirement (out by 0.09)
A perfect sphere of diameter 5.79 except with a single flat spot bringing the local size down to 5.21:
- meets the 5.5 +/- 0.3 requirement (in by 0.01)
- does not meet the profile requirement (out by 0.15 or so)
- does not meet the profile requirement (out by 0.15 or so)
3DDave,
Gasp indeed.
Each tolerance does have a different set of allowable outcomes, and that is exactly the point. Compliant parts are in the intersection of those sets. Just like every other drawing with multiple requirements, they must all be met simultaneously.
The interpretation of each tolerance is not affected by the presence or absence of the other. If each tolerance has only one interpretation when used independently, then that should remain true when they are both applied on the same drawing and to the same surface. And if each tolerance has only one interpretation, then so does the drawing as a whole.
Belanger,
I only described the modification to Fig. 8-6 to emphasize that the basic dimension should not be eliminated if the profile tolerance is to remain valid. The specific tolerance values used in Fig. 8-6 make it an unreasonable example because any part that satisfies the profile tolerance will also satisfy the dimension tolerance.
In the examples I presented, the tolerance values were intentionally chosen such that it's possible to satisfy only the profile tolerance, only the dimension tolerance, both, or neither. The second example with the spherical part should make this somewhat more clear.
To me, two tolerances conflict only if it's impossible to simultaneously satisfy both. I guess you are using a different meaning of "conflict".
pylfrm
Burunduk
Mechanical
- May 2, 2019
- 2,563
pylfrm, I now get it about the sphere example, thanks. A part can conform to both requirements or rejected by just one (any) of them.
With that said I think that what would bother most people is that both requirements control the same characteristics of the samepart feature; form and size. Yes, when both defined the result in terms of acceptance/rejection might differ from using just one of the tools, but I don't think this is a very practical scheme. You don't see many (if any) drawings having the same diameter appearing both basic controlled by Profile and non-basic controlled by +/- tolerance. Probably for a good reason.
With that said I think that what would bother most people is that both requirements control the same characteristics of the same
Burunduk,
I generally agree. It would be a rare case where I'd support using this scheme over all the various alternatives. I do see it used though, and I don't think interpreting it is particularly problematic.
Part of the reason I mentioned this is the connection to default tolerances. If you have a basic CAD model and a "profile all over unless otherwise specified" tolerance, I think there is a strong case to be made that a toleranced size dimension should not count as "otherwise specified". It would actually be something more like "additionally specified". I realize many will disagree though, so I recommend avoiding the issue by omitting the "unless otherwise specified" exception. If exceptions are still desired, they can be identified much more clearly using flag notes or other methods.
pylfrm
I generally agree. It would be a rare case where I'd support using this scheme over all the various alternatives. I do see it used though, and I don't think interpreting it is particularly problematic.
Part of the reason I mentioned this is the connection to default tolerances. If you have a basic CAD model and a "profile all over unless otherwise specified" tolerance, I think there is a strong case to be made that a toleranced size dimension should not count as "otherwise specified". It would actually be something more like "additionally specified". I realize many will disagree though, so I recommend avoiding the issue by omitting the "unless otherwise specified" exception. If exceptions are still desired, they can be identified much more clearly using flag notes or other methods.
pylfrm
- Status
Similar threads
- Question
- Question
- Locked
- Solved
- Question