Combining +/- tolerance & basic dimension to locate a hole. 2

[Madhu454]

Hi All,

One more basic question. Please see the attached drawing.

Only one face of the block is mates with its counter part (datum feature B). the other side is open and does not mates with any surafces. The hole needs to be located with closer tolerances with respect to datum faeture B, the location of the hole from the other free face which can have a wider tolerance. In such case can we combine the +/- tolerance and basic dimensions to locate the hole.

Is it a legal specification in ASME? I have seen few drawings of this kind.

 

[CheckerHater]

ASME Y14.5-2009 para. 7.2.1.1:

"Dimensions used to locate true position shall be basic and defined in accordance with para.2.1.1.2"

One of the very few places where standard actually sais "shall"

I hope this helped.

 

[Belanger]

The drawing is legal. The true position is being held with respect to datums A and B, and those dimensions are basic. The other dim shouldn't be basic since the GD&T has nothing to do with that east/west location.

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

 

[TheTick]

I have seen few drawings of this kind.

I once saw someone clean a part by boiling it in gasoline on a kitchen stove. I wouldn't advise anyone else to do it.

 

[CheckerHater]

Belanger,

Per ASME Y14.5-2009 para. 7.2:
"Position is the location of one or more features of size relative to one another or to one or more datums."

The way I see it, if it is not located to the datum (or another feature of size), then it's not a "positon".
Your opinion?

 

[Belanger]

RIght... if it's not located to a datum (or another feature in a pattern), then it's not a position tolerance. But it can still have a location tolerance, which need not be the GD&T-specific term of "position," but rather a ± tolerance.

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

 

[fsincox]

JP,
And the "legal" definition of what it means is given where? How is the hole center to be related to the surface, all points, one point?
Frank

 

[CheckerHater]

This is actually very interesting.

I am a big fan of mixing GD&T with +/- dimensions myself, but this particular example looks like the worst way of doing it.
The question is "how to measure / gauge it?" Let say dim 50 is taken from "implied" datum. Is implied datum secondary or tertiary? How the resulting tolerance zone looks like?

I am really interested in seeing more opinions on this topic.

 

[Belanger]

Frank, I'm not sure what you mean. The standard doesn't require a position tolerance to lock a hole in every direction of space. Maybe rephrase your question?

I should add that the FCF probably shouldn't be pointing to the hole with the leader at an arbitrary angle. Better to show it with dimension/extension lines, similar to Fig. 7-28 of the standard, which are more clear about the direction of control.

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

 

[MechNorth]

J-P, there is no support in the Y14.5 standard ('94 or '09) for how to establish the center of the hole for use with a +/- location tolerance. There may be "common practices" but it's not part of the standard. I agree with you that the callout is poorly done. The size callout should be separated. The "vertical" position control should be attached to a vertical dimension leader (top to bottom of the hole). The "horizontal" position needs to be similarly called out with an FCF and a Datum C referenced (and added to the drawing).


+/- dimensions are point-to-point. From what point on the left surface do you measure, and how do you establish the center of the hole horizontally?

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Belanger]

Good point, Jim. I guess I was focusing on the legality of the feature control frame; there is no requirement that a FCF control all directions.

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

 

[pmarc]

+/- dimension for controlling position is not a best choice - it creates ambiguity, adds no value in comparison to standard positional tolerance and is illegal because Y14.5 clearly says that basic dimensions shall be used to define true position.

Why not to add tertiary datum feature C, then use basic 20 and 50 dimensions and assign bi-directional position callouts with 0.2 value in y direction and 1.0 in x direction? Would it create something confusing? Would it make measurements more difficult?

 

[drstrole]

I agree with pmarc's suggestion. Possibly the hole is actually the tertiary datum feature and the right and left edge be profiled back A/B/C, with the hole being teriary, if that is how the part works.

Drstrole
GDTP - Senior Level

 

[fsincox]

Jim,
Thanks, I think you covered the point I was trying to get at.
Frank

 

[drawoh]

Madhu454,

Your drawing almost makes sense to me.

If a feature is controlled by two tolerance, both tolerances must be met. Your positional tolerance requires your hole to be within 0.1mm of true position. Anything that meets this, meets to ±0.5mm from the side.

Your drawing actually would make sense to me if you called up a sloppy positional tolerance, and then called up an accurate ± dimension on the 20mm dimension.

You can do this directly with GD&T, and leave the ±[ ]tolerance out. How about a composite tolerance frame in which your positional tolerances to datums[ ]ABC was Ø1mm, with a second frame from datum[ ]AB, calling up 0.2?

JHG

 

[pmarc]

drawoh,
Composite positional tolerance makes no sense unless there are two or more FOS. See 7.5 and 7.5.1 of Y14.5-2009.

 

[drawoh]

pmarc,

Why not?

I am not trying to do the same thing as section[ ]7.5. I am trying to create a rectangular (not square) tolerance zone, as opposed to the normal round zone.

I could apply ±[ ]tolerances to each coordinate to the hole. On a simple part, this would work. On a complex part, with several features controlled by the dimension line, it would be hopeless.

JHG

 

[TheTick]

Directional tolerance in GDT.

 

[pmarc]

drawoh,
If you were trying to create rectangular tolerance zone look at fig. 7-28 in Y14.5-2009 or 5-41 in Y14.5M-1994 standard for clear example.

 

[CheckerHater]

I am trying to put myself in Belanger's shoes.
Let say, operative word is "one or more datums", so as soon as we have just one datum the FCF becomes legit.
Please look at the picture.
In "A" case we only relate to one datum [A]. "Position" in this case will become Perpendicularity. We all agree that +/- tolerances will be ambiguous, but if they are larger than hypothetical "shop accuracy" we will probably get the good part (from hypothetical shop )
In "B" case we have some weird desire to control position in 2 directions separately and only use 2 datums for each direction. The picture looks, say, questionable, but not totally illegal.
Any ideas - are those better or worse than layout suggested (or questioned?) by Madhu?
Don't get me wrong - I think we already have a good solution, but trying to explore the possibilities.