GD&T Angular conflict?

[Ecomm1]

Seeking clarity on an angular check. We have a tight tolerance on an angular surface. ( 35 degrees )

1.0000”/1.0002” from the angular surface to .250” gage pin. ( On a sine bar )

Angular callout is .002”. Assuming the hypotenuse is 1.000”.


1. Without a 1.0001” basic dimension using 1.0000”/1.0002” tolerance, is the .002” angular callout excessive as the .002” band is greater than the .0002” tolerance on the gage point length?

2. Would providing a surface profile callout of .0002” and a basic dimension of 1.0001” override the .002” angular callout or should the angular callout be tightened?

See attached hand sketch.

Thanks,

Ron

 

[75sv1]

I think you need to know the diameter of the gage pin. The 1.000-1.0002 is a distance. So, is the 1.000 degrees tolerance less than the .0002 over the length of the feature. If so, then valid. If not, then not. It would be better if stated as a profile of a surface.

 

[guythatbrews]

I don't think the drawing is in error, though it is curious.

"C" in the feature control frame is not needed. The feature must lie within two parallel planes .002" apart centered on 35* basic dim. That sets the angle, not the position.

The 1.0000-1.0002 positions the surface. So the position of the surface is much closer than the angle. Pretty darn close considering all the measuring tools also have a tolerance to take into account.

I'm sure you just omitted the pin size. The dashed lines are called extension lines and should be solid, thin lines. A dashed line means the line is hidden.

Good luck. It looks like a handful!

 

[implmex]

Hi Ecomm1:
I don't think you can have a toleranced dimension to describe where the surface is, if you are going to use a GD&T angularity callout for the same surface.
If the angular tolerance is open, the surface can be all over the map, and the dimension you actually measure depends on where along the surface you happen to interrogate it.
Calling a dimension with any tolerance to that surface doesn't make any sense to me.

On the other hand, if it were a basic dimension, then the angular tolerance would control where the surface could lie and together with a separate flatness callout would define the part unambiguously.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[guythatbrews]

Hi Ecomm1:
I don't think you can have a toleranced dimension to describe where the surface is, if you are going to use a GD&T angularity callout for the same surface.
If the angular tolerance is open, the surface can be all over the map, and the dimension you actually measure depends on where along the surface you happen to interrogate it.
Calling a dimension with any tolerance to that surface doesn't make any sense to me.

On the other hand, if it were a basic dimension, then the angular tolerance would control where the surface could lie and together with a separate flatness callout would define the part unambiguously.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

It seems to me this is unambiguous. Both conditions may and must be met. The angled surface can deviate within the .010 band, and the surface is located over the pin.

Granted, the angled surface must be very flat, as the 1.0000/1.0002 implies, and all the angled surface must meet the 1.0000/1.0002 requirement. Maybe my word "implies" adds the ambiguity? If I had the skill (and measuring tools) to even come close to meeting the distance requirement, I'd level the angled surface and confirm all the surface met the distance requirement. Quite a tedious check.

It does seem there is a better way to GD&T tolerance the position of the surface, but I'm not sure what it is. Maybe the designer wasn't sure either. Hence the hybrid dimensioning. Probably all of us have seen some crazy dimensioning.

Any way you slice it, it is a very close requirement, with very special inspection methods required. Considering the precision of the measuring method required, is there really any way to check this feature reliably?

 

[John Garner]

I'm no GD&T guru, but I would understand a tolerance to have the same unit as the quantity it controls. On that basis, the permissible angle error would be 0.002 degree, or 7.2 arcsecond.

 

[implmex]

Hi guythatbrews:
Be aware, first of all, that I have only a machinist's knowledge of GD&T, so I cannot claim to know what I'm talking about with any authority.
Having said that, the place where ideal geometry and "real" geometry intersect is where I and seemingly many others get stuck, and in this example, the fact that the GD&T angularity tolerance leaves a comparatively large deviation from ideal geometry possible, makes it difficult for me to understand how a tight position tolerance can be called out for the same surface.

As you describe it, I could set the part up on a sine bar at the nominal angle.
I could interrogate the top of the gauge pin to find the tangent plane that's parallel to the ideal surface of the ideal part.
I could then traverse up to the real surface of the real part and compare real to ideal.
If I confine my distance measurement from the tangent plane of the pin (that's parallel to the ideal surface) to the line on the real surface parallel to the axis of the pin and closest to the pin axis, I would be "theoretically good" and could take my measurement.
But if that surface is deviant across its width as well as along its length, by the amount the tolerance band allows, I do not know where along the imaginary line across that surface to take my measurement.

I suppose I could take the midpoint of that line I've imagined across the surface, but I don't think the GD&T (as expressed), captures that intent, so that toleranced distance dimension remains problematic to me.

I know this all sounds terribly convoluted: does it make any sense to you at all?
It hurts my head a bit even reading it, and I just wrote it.

Cheers

Marcus
www.implant-mechanix.com
www.vancouvewireedm.com

 

[implmex]

Hi John Garner:
Yeah, you'd think so, but GD&T sadly doesn't work that way.
An angularity tolerance callout doesn't describe a minimum and maximum angle, it describes two parallel tolerance zone limits (planes) centered about the theoretically perfect surface of the ideal part, into which the entire real surface of the real part must fall.
So no bits of the real surface may protrude beyond either the upper limit plane or the lower limit plane anywhere.
Within that tolerance zone it can be any shape...wavy as hell if the limit is liberal.
It can also be at any angle in three dimensions provided it doesn't violate those limit planes.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[guythatbrews]

Marcus I have done a lot of studying in the 1982 GD&T spec, but it has been long ago. So I'm no guru either. Heck there may be another revision by now.

I understand what you are getting at. It is an interesting problem.

How about this. Put the part on the sine plate with -C- resting on the stop that satisfies the secondary datum. The only way to check this distance is to assume the primary datum is the bottom of the part. Not talking in GD&T terms here but practical terms. The pin is on the same plate against the same stop. By trial and error the plate is raised until the entire surface meets the 1.0000/1.0002 requirement, as tedious and impossible as that might be. The plane checked would then be normal to the sketch. This satisfies the much tighter distance requirement. Some assumptions have been made, but they are arguably all reasonable.

Can't we now switch to -A- and -C-, check the angle requirement and be good?

 

[implmex]

Hi again guythatbrews:
The latest ASME Y14.5 GD&T manual that I'm aware of is 2018, and from what I understand it differs in detail but not really in principle from the standard you're used to working with.
Some callouts have been eliminated as redundant (symmetry and concentricity I think...maybe some others too).
There used to be a material condition modifier for "Regardless of Feature Size" too, and I think it's also officially gone now.
Don't quote me on any of this!

Moving on to the OP's part.
I think you and I can agree the drawing is woefully incomplete and you could never make or inspect a part from the sketch alone.
I can see, even in the few callouts that there are problems.
For instance, the angular callout references two datum surfaces, each of which could be appropriately used as a datum for a basic callout for the angle.
So which is it...surface A or surface C?
The sketch clearly shows it as Datum surface A but the feature control frame shows it as A and C.
I don't believe C is necessary in that feature control frame.

So we could debate all day about what this sketch means.
The OP did describe using an alternative way to tolerance the part, with basic dimensions and a very tight surface profile tolerance for the angled face, referenced to a Datum Reference Frame that's unambiguous and straightforward: A, B, and C where A is the top or bottom of the part instead of one edge.(assuming the part is not as thick as it is tall and wide)

I think that's a better way to go, and may well capture the designer's intent better too.
As you commented in post #5, I also cannot envision needing a super tight distance tolerance to a sloppy, rough surface...there's kinda no point.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[Ecomm1]

Fascinating and insightful replies! I agree that datum -C- should not be considered. My concern was how could such a large angular window be considered with such a tight tolerance. If I trig the 35 degree angle with a 1.000 hypotenuse the side opposite is .5736". Adding .0001" on SO increases the angle to 35.0086 degrees, and Subtracting .0001" on SO decreases the angle to 34.9947 degrees. Although not an exact band, the difference here is .0139 degrees which I believe should contain the .0002" for this surface. The .002 angular callout seems to be useless. I'll discuss with engineers in hopes of getting a basic dimension, profile of a surface and perhaps a reasonable angular callout. Perhaps the profile of the surface would refine the angular callout?

Thanks for all the replies,
Ron

 

[John Garner]

A couple of thoughts:

1. Tolerancing the angled face to Datums (American English plural, not Latin plural, for Datum) A and C might be an around-the-block way of establishing a tolerance on the angle between A and C. Or it could be an erroneous citation of Datum C, with the intent to tolerance a "compound angle" error having both in-drawing-plane and out-of-drawing-plane components.

2. The reference line for the 1.0000 - 1.0002 inch dimension is not defined. As shown, it either a) awkwardly specifies the required distance between the angled face and and the center of the pin hole without including the hole radius, or 2) absurdly requires that the angle face should be parallel to one of its own parallels.

 

[gbent]

I believe C is referenced to give a vector to the intersection between A and the angled surface.

 

[75sv1]

I can see that the linear dimensioning and the GD&T conflict. It is hard to 'dimension' this without knowing the design content or function of the part. Not sure what the design content of the pin is, and its function. Yes, the ASME docs would have examples. I didn't have time to look at them. The pin look like the classic math problem of the wheel against the wall. No, I didn't figure it out back in HS. It come up from time to time. Don't get me started. I have had to use variations of it at work.
So, first, I question the Datums. Since the pin is referenced, then why isn't the bottom plane DTM A? Then make DTM C , to DTM B. DTM C is one of the sides.
Either dimension one of the angle intersection to A and B. Or, make a gage point on the angle dimensioned to A and B. Then Profile of a Surface, XXX, ABC.

 

[75sv1]

Edit: also, in a linear dimension, as like a GD&T zone, the surface can do what it wants within that zone. So, if you need a parallelism or a flatness, than that need to be called out. Remove datums from the Profile of a surface callout to achieve this. A flatness or from will have no datum. These would be added below the initial profile of a surface call out. There are examples in the AMSE. I think page 70.

 

[implmex]

Hi again Ecomm1:
If you have a complete Datum Reference Frame, and you call out the angle (with a basic dimension) and call out the distance from a datum to an edge of the angled surface (with another basic dimension), you can describe the whole tolerance zone (2 parallel planes) with a single profile (of a surface) callout.
You then no longer need a flatness callout, or an angularity callout; the profile callout fully describes where the real surface of the real part must lie relative to the ideal part shown on the drawing.
If your datums are A on a surface parallel to the paper, B on the long edge of the part where the gauge pin is currently depicted, and C as either end of the part, you can lay your part on the granite of a (really really good) CMM, set your B and C datums with the CMM and then just probe your angled surface to know immediately whether all of it sits within your profile tolerance zone.
No sine bar, no gauge pin, no screwing around to try to validate that nutso ambitious tolerance on that 1" dimension.

But you do need a really good CMM to interrogate reliably within a tenth.
I wonder actually, if that tenth is a misprint or a typo...wouldn't be the first time!

Cheers

Marcus

 

[75sv1]

I did look at ASME. It does show the angle call out as in the print. It does not show dimensions, though. I'd think a dimension from dtm C to the intersect to A, would be good.

 

[jccaclimber]

Is the drawing viable? Yes. Is Datum [C] used as shown? No.
Ignoring the other issues with measuring this, I hope that 0.25" gage pin is perfect. If you're using a common Class Z pin, the diameter tolerance on the pin alone might make one shop measure it as in spec and the next disagree.
The 1.0002"/1.0000" callout defines the position of the face, but does nothing to define the angle.
The angularity of 0.002" limits the angle, but does nothing to define the position, which is why it doesn't need [C]. Had Profile been used then position would have been defined, though I suppose you could still use the other to tighten the requirements. You're getting pretty close to double dimensioning at that point though.
As drawn, and assuming that you intend to follow envelope principle the 1.0002"/1.0000" spec also effectively adds a tight flatness callout within the region allowed by the angle.
Give this the angle callout might as well have a +/- tolerance on it. Not *quite* the same, but very close.
Just for fun, if you wanted to allow a bit looser flatness and are just locating a larger plane you could make the sloped surface [D], then specify datum [D] as having the angularity control. Then you'd only be holding the highest two points in place.
If one of my engineers showed me this on a drawing in a vacuum I'd ask them if this design was really the best way to get what they wanted, but I don't know enough about the rest of your project to say either way.