GD&T question
GD&T question
(OP)
Hi,
So hoping some experts can help me put a question to bed. I work in the electronics industry, so really don't need to use GD&T at all. However, our data sheet drawing has this call out, and it's been the source of much debate with some customers. I've attached a picture of how I understand it, but some customers are taking it to mean that the 0.1 profile zone encompasses the B & C edges of the part. But those are datums, so shouldn't be included, right? In general, I think it's just a poorly done, but that's another issue.
So hoping some experts can help me put a question to bed. I work in the electronics industry, so really don't need to use GD&T at all. However, our data sheet drawing has this call out, and it's been the source of much debate with some customers. I've attached a picture of how I understand it, but some customers are taking it to mean that the 0.1 profile zone encompasses the B & C edges of the part. But those are datums, so shouldn't be included, right? In general, I think it's just a poorly done, but that's another issue.





RE: GD&T question
"Know the rules well, so you can break them effectively."
-Dalai Lama XIV
RE: GD&T question
RE: GD&T question
0.8 MAX is not a tolerance, because it is one-sided. Flatness of 0.1 controls the surface of datum feature A.
Unless something else is controlled wrt A|B|C, you may be able to drop B and C altogether.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
RE: GD&T question
"Know the rules well, so you can break them effectively."
-Dalai Lama XIV
RE: GD&T question
lightweight, cheap, strong... pick 2
RE: GD&T question
RE: GD&T question
RE: GD&T question
Sorry to complicate this, but your drawing happens to include a couple of subtleties (oddities?) of the Y14.5 standard.
First, I would say that B and C are not centerplane datums. Datum feature B is just the right-hand surface and datum feature C is just the top surface. The 4.9 and 8.2 widths are not considered features of size, because the dimensions are basic. If the 4.9 and 8.2 were not basic and had direct plus/minus tolerances, then the widths would be considered features of size and the B and C datums would be centerplanes.
Second, I would agree that the profile tolerance includes all 4 sides. But there is a quirk because the datum features are included. Because datum planes B and C are derived from the high points of the B and C features, the effect is that only half of the profile zone is usable. So the B and C surfaces must be flat within 0.05. Something like this:
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: GD&T question
ASME Y14.5-2009 para. 4.11.4 (Specifying Datum Features RMB) does not mention features of size. Where is this requirement for centerplane datums?
- pylfrm
RE: GD&T question
Not only there is no requirement for feature of size, the dimension line itself doesn't even have to contain actual dimension.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
RE: GD&T question
RE: GD&T question
What we ended up doing was leaving datums in place for BGA location, but changing the package size dimensions to 4.9 +/-0.05 and 8.2+/-0.05.
RE: GD&T question
the result of the OPs drawing is a 0.1 profile of all 4 sides.
lightweight, cheap, strong... pick 2
RE: GD&T question
I guess you eliminated the profile tolerance? This leaves the orientation of sides to ends at the mercy of the default angle tolerance, if there is one.
RE: GD&T question
I expected some disagreement regarding the centerplane datums for the basic widths.
pylfrm - I agree that 4.11.4 does not specifically mention features of size. But it makes no mention of a basic size either. In the figures that show a dimension for a width datum feature, the dimension is always directly toleranced. I was not able to find an example that uses a basic width (or a basic diameter, for a cylindrical datum feature).
CH - There are some figures in section 4 on width datum features, that only show a datum feature symbol and a dimension line (no dimension is shown). Does this mean that this is a legitimate way of specifying a datum feature? I would say no, because these figures are intentionally incomplete.
Tenkan - I agree that the placement of the datum feature symbol and dimension line makes a difference with width datum features of size. But because basic dimensions were used, I would argue that the 4.9 and 8.2 widths are not features of size. The definition of a regular feature of size in 1.3.32.2 contains the statement "associated with a directly toleranced dimension". I would say that a basic width controlled by a profile tolerance is not a directly toleranced dimension - you (and others) may disagree.
So at the end of the day, Y14.5 does not give a clear indication of whether or not a basic width results in a centerplane datum. It makes no indication that you can do this, but doesn't say that you can't. So we have to decide whether this is a valid extension of principle. Overall, I would say that it is not.
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: GD&T question
If it's true that only half the tolerance zone is usable on that side, then I'd like your views on what the tolerance zones would look like for each part in my attached graphic. (I'm not interested in whether we all like the second picture; but interested in how folks would envision the tolerance zone if that's what the drawing showed.)
PS: (a corrected graphic is given in a subsequent post)
John-Paul Belanger
Certified Sr. GD&T Professional
RE: GD&T question
Hopefully I can offer an opinion here as well. In the first picture I would envision a tolerance zone that extends from the high points of the surface, up 1mm, just like shown in the standard (I think). As for the second picture, I think it would be sheer guesswork. What is datum feature A exactly? According to the print it's the surface on the left only, but then both surfaces are referenced WRT to datum A so that makes it kind of a self referencing datum which is no good. I can't imagine a valid, or at least supported, tolerance zone setup for this.
John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
RE: GD&T question
See one version of a corrected graphic (attached). But you might see where I'm going with this: Most of us acknowledge that the first picture places the tolerance zone all on the "up" side. I wonder if people would think the same on the second picture I give?
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: GD&T question
You may want to take a look at fig. 4-33. This figure does not seem to support your standpoint.
Besides, if we really want to analyze the paragraphs in the standard, para. 3.3.2(b) states that datum is a center plane if the datum feature symbol is placed on the dimension line or an extension of the dimension line of a feature of size. It does not say 'regular feature of size'. The widths in question are features of size, just not regular, but irregular, as defined in para. 1.3.32.2(a).
J-P,
On your first picture the maximum possible offset between both surfaces can be 1. On the second picture only 0.5, because half of the tolerance zone width is unsable as it lies inside the material of datum feature A-B simulator, and the datum A-B is established by the high points of surfaces A and B simultenously.
This concept has not been explicitly pictured and described in the Y14.5-2009, but most likely will be covered in the future version of the Y14.5. From existing standards the closest is fig. 4-16 from Y14.8-2009. It shows datum target application, but the basic tenet is the same - profile tolerance zone applied to datum features from which datum plane is derived is equally disposed about that datum plane. This means that in case of datum targets the entire profile tolerance zone is usable, but in case of datum feature being entire surface only half of the profile tolerance zone is usable.
3DDave,
With that being said, in the OP example there would be a difference between having and not having datum feature reference B and C in the profile callout. Since only half of the profile tolerance zones are usable for each pair of opposed surfaces when B and C are referenced, the maximum allowed angular error between surfaces in each pair (expressed in linear units) is twice as small as in case of profile callout with no datum references or reference to A only. I am not saying that presence of B and C makes sense from functional point of view, just trying to describe difference.
Hope this helps.
RE: GD&T question
What I think it would do is reject a certain number of parts that are as usable as parts that are accepted.
RE: GD&T question
I don't perceive any difference in interpretation between your first picture and your second.
John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
RE: GD&T question
Okay, you got me on this one. You're absolutely right, I hadn't thought of irregular features of size at all. Basic widths and profile are used with those, the examples clearly show it. I'm not a big fan of the irregular features of size section - I don't think the definitions are very clear. Perhaps this is why I didn't think of it - it never entered my mind to apply the "irregular" concept to a feature that has "regular" geometry (two opposed parallel planes). This does not seem very intuitive to me at all, and must be very confusing to those who don't obsess over the Y14.5 standard like we do.
But I would disagree with the interpretation of the zone availability. If B and C are treated as features of size with centerplane datums, then I would say that the entire zone thickness is available for the B and C surfaces. Like this:
So the form of the B and C surfaces, and maximum angular error between them, is the same as it would be if only A was referenced (or no datum features).
I would agree that specifying the B and C datum features does make a difference. Aligning the profile zone to the two B surfaces will be different than best-fitting it to the four surfaces together. This will need a different figure though.
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: GD&T question
And everyone should keep in mind that the OP's question was about the datums being derived from a FOS. My sketch was about a surface datum. (Sorry if that introduced any confusion, but my sketch is related to a real design I'm working on, and I figured they are somewhat related topics.)
I think the bottom line is that good practice deems that a profile tolerance shouldn't reference a datum that is derived from a surface lying within the profile coverage.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: GD&T question
John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
RE: GD&T question
I got you on one, you and 3DDave got me on the other. I was too hasty with my reply to Dave. Thank you for being cautious and critical.
RE: GD&T question
John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
RE: GD&T question
Here is how I would envision the situation for the coplanar surfaces:
I've shown the same as-produced surface geometry for both cases. When no datum feature is referenced, the surfaces can occupy any part of the zones and the control is equivalent to coplanarity. When the A-B datum feature is referenced, the surfaces must have high-point contact on simulators located at the basic surfaces.
I believe that this is fully consistent with pmarc's description.
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: GD&T question
I keep telling them about it, and suggesting that they "qualify" A, B, and C (flatness on A, perp on B, etc.) so that those surfaces are exempted from the general profile note. We'll see if it goes anywhere.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: GD&T question
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
RE: GD&T question
The "profile of a surface all over unless otherwise specified" usage brings up another question in my mind though. Does flatness, perpendicularity, angularity, or anything other than profile of a surface count as "otherwise specified", or is a different profile of a surface tolerance with an identical DRF required? I'd lean towards the latter, because anything else could be intended as a refinement or supplement to the general profile of a surface all over. Other opinions on this?
- pylfrm
RE: GD&T question
John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
RE: GD&T question
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: GD&T question
RE: GD&T question
If you use hard gage to establish "highest points" datum, then only half of the tolerance is usable on the datum features.
If you "average" your CMM measurements, the entire tolerance is available.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
RE: GD&T question
In case of a rectangle specified with profile, as a general note, to A, B and C:
If the datum feature is the center plane (B and C) of the part then the full profile tolerance is available.
If the datum feature is the surface (right vertical surface OR left vertical surface for datum feature B; top horizontal surface OR bottom horizontal surface for datum feature C) then only half tolerance is available.
Please kindly advise.
RE: GD&T question
Could you explain what you mean by:
"If you use hard gage to establish "highest points" datum, then only half of the tolerance is usable on the datum features.
If you "average" your CMM measurements, the entire tolerance is available"
Why if you are using LSQ method on CMM then the entire tolerance is available?
RE: GD&T question
That's a good question. I would think that the general tolerance would apply to everything, and then other tolerances would be refinements that would apply in addition to it.
powerhound,
It sounds like there is still a difference in our points of view. I'm saying that the tolerance zone is centered about the true profile in both cases. I don't see the zone extending from the high points inwards in either case. Please see the additional example below. Here is the logic:
1. The tolerance zones have basic location (centered about the true profile).
2a. If no datum feature is referenced, the toleranced features can be simultaneously fitted (rotated and translated) relative to the zones to get the best result.
2b. If datum features are referenced, the datum feature surfaces must contact the datum feature simulators at their high points. The datum feature simulators are coincident with the true profile.
3DDave,
Yes, if the profile tolerance was SPF|1(U)0|A-B| then there would be no usable tolerance. Interesting.
CH,
You're correct, but the method used to establish the datum is not open to interpretation. The default is high-point contact with a perfect simulator. If an averaged plane (such as least squares) is used, then the rules are not being followed. This is a big issue with CMM's.
greenimi,
I believe that you're correct. If the B and C datum features are width features with centerplane datums, then the entire profile tolerance is available for the B and C surfaces. If the B and C datum features are each single planar surfaces, then only half the profile tolerance is available for the B and C surfaces. Strange, isn't it?
Here's another example:
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: GD&T question
Evan, I think you meant SPF|1(U)1|A-B|.
RE: GD&T question
From the Y14.41-2012 "Digital Product Definition Data Practices" (future version of the Y14.5 will have very similar paragraph):
"1.3.10 Unless Otherwise Specified (UOS)
The phrase “unless otherwise specified” or UOS is used to indicate a default requirement. The phrase is used when the default is a generally applied requirement and the exception can be clarified by providing a reference to another document or requirement."
To me 'the exception' means that anything other than the general profile tolerance overrides that general profile tolerance.
RE: GD&T question
Yes, good catch. I think I got my material direction turned around because it's the bottom surface. The number after the (U) is the amount in the direction that adds material, and the datum plane sits on the high points of the surface. So you are given a tolerance for how much material is higher than the high points ;^). Odd, isn't it?
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: GD&T question
RE: GD&T question
With that in mind, I would say that the middle paragraph within your original graphic gives the wrong numbers. Just based on that given GD&T, the dimensions of the part can be translated to 4.9 ± 0.1 by 8.2 ± 0.1. (You lose control of perpendicularity on the corners by translating it back to coordinate tolerances, but the individual dims would work out that way.)
Now, if that was not the intent, then the GD&T should be altered. But those are the results based on wrapping the profile all around.
The other side discussion was about a case where the datums are taken from those two surfaces only. (To designate that you'd have to move the datum symbols to be offset from the width and height dims.) If that were the case then you'd get only half of the 0.1 on those two surfaces, but the full 0.1 on the other two sides.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: GD&T question
This is why I suggested to the committee they use something like +.010/-.005 to indicate material added and removed about the nominal profile, but someone had already committed to (U) and that decision was -done- and could never be revisited.
RE: GD&T question
Your reply to greenimi...
Why would you say that the full tolerance is useable on all identified profile controlled surfaces with the datum center planes, when those dattum center planes are established by contact on "both" surfaces for each datum center plane ?
Wouldnt all identified profile controlled surfaces be contacted to establish the B|C datum center planes which would give half useable tolerance zones for all 4 surfaces?
RE: GD&T question
It's true that all of the profile-controlled surfaces would be contacted to establish the B|C centerplanes. But the "halving" effect only occurs when one individual plane is used to establish a datum. See the figures from my Mar 4 and Mar 6 posts.
The halving is not any kind of rule or condition that's being imposed - it's a consequence the "self-referencing" feature control frame. If the toleranced feature also establishes a datum plane, and the tolerance zone must be centered on the datum plane, then half of the tolerance zone is below the feature's high points (and therefore usable) and the other half is above the high points (and therefore not usable). In other words, the high points of the surface are perfect (coincident with the true profile). This doesn't occur when the datum feature is two opposed planar surfaces, because the high points of the two surfaces are not necessarily coincident with the true profile. This is very hard to explain in words - the pictures do a much better job.
The moral of the story is that in Y14.5 datum features are not all treated equally, with the same amount of tolerance. There are the halves and the halve-nots ;^).
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca