Help with GD&T (setting datums) on Square Hole and Crowfoot 2

[HightechHillbilly]

Howdy,

I'm trying to lay out the drawing details for a crowfoot wrench head (see attachment). Because I've always been taught that when choosing one's datums, the decision is based off of part functionality. Since this is a part of a tool, it will interface via the square hole with a ratchet with a square tab. And it will also interface with the fastener via the fastener opening on the crowfoot (where the angular dimension is).

I've given my best "guess" as to how the GD&T should be presented, but I'm wanting to know if the approach I'm taking is on the right track, or if I'm totally off base? Also, I'm not sure if I need to assign the fastener opening to Datum "C."

Any help, advice, links, etc would be appreciated.

Thank you,
Rob

 

[HightechHillbilly]

P.S. I must have attached the old picture, the one without the points for the profile. See the new attached picture, as it has the points "x" and "y" for where to apply the profile tolerance along the fastener cutout.

 

[Belanger]

In general, it seems OK as it is. However, no need for labeling a datum C unless it will be referenced in a subsequent callout (and even if it is used subsequently, it wouldn't be referenced at the same time as B).

Minor stuff: the arrow for "between" points X and Y should be pointing in both directions. And in the right-hand view, the convention is to have the feature control frame be attached to the surface (or an extension line, or leader), and then hang the datum label for A off of the feature control frame.

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

 

[HightechHillbilly]

Belanger,

Thank you very much for your reply (and "whew" - it's good to know I wasn't that far off base)!! heh

Anyway, the reason I was debating about Datum "C" is that, if the hole (Datum "B") would have been a circular hole, I still would've needed a 3rd Datum to control the rotation. However, since the "hole" is a square hole, then this is a case where only 2 Datums are needed to control all the translations & rotations.

Another reason was that the fastener profile cutout (what I was attempting to call Datum "C") has a functional purpose (to mate w/ a fastener), which confused me, since, as I said previously, I've always been taught that one defines datums where there is a functional purpose for the part.

And thank you for the advice on the "cleaning" up of the symbology, I assure you when I check in the drawing & it gets visibility from the manager, all notations, symbology, typos, formatting, and general "shop keeping" will be correct & ready to get released.

Again, thank you!
Rob

 

[HightechHillbilly]

P.P.S. I was finalizing the drawing, and I realized that I also wasn't sure if the position dimensions for the square hole (the x & y dimensions to position it on the part) needed to be basic dimensions? Or, should they be set at some positional tolerance from something, and if so, then what, because there is no horizontal or vertical surface to position from?

Thanks in advance,
Rob

 

[Belanger]

You are not tolerancing the location of the square hole with GD&T (in fact, that square itself is the datum for the hex shape). So no basic dims are needed on the location of the square at this stage. Perhaps use another profile tolerance with a larger tolerance for the perimeter of the part -- the other portion of the x - y connection -- and reference it back to A and B. But of course it depends on function and other fit requirements.

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

 

[HightechHillbilly]

Belanger,

Again, thank you for responding - your knowledge has been very helpful, as this is the first time I've had to perform the dimensioning on a part with such irregular geometry, having no real horizontal or vertical features to dimension from.

Anyway, I'm not sure I fully understand your suggestion regardind using another profile because I don't know how that relates to the position / location of the square hole (see my position / location dimensions in RED). The previous dimensions for the square hole only set the height & width of the square, but did not position / locate it on the part.

I think, perhaps my confusion, is that I don't fully understand how (or if) the profile tolerance for the square, with respect to Datum "A" can set the position / location of the square. Please correct me if I'm wrong, but in my example, I have put in an actual value for the profile tolerance of the square (.005). Does that mean that the position / location of the square must be within .005 from the vertical & horizontal edges of the shape (the dimensions I have in RED)? Do I even need those dimensions on the drawing, or does having the profile tolerance render those RED dimensions unnecessary? If I do need those dimensions (in RED), are they correct as I have them, pointing to the center of the square, or should I point each one to the appropriate edge of the square?

And finally, how does your suggestion to profile the perimeter come into play?

So yeah, I think my main question is regarding my lack of fully understanding how profile tolerance controls location.

Thanks again!
Rob

 

[Belanger]

I think this is the main issue -- you asked, "I have put in an actual value for the profile tolerance of the square (.005). Does that mean that the position / location of the square must be within .005 from the vertical & horizontal edges of the shape (the dimensions I have in RED)?"

The answer is no, not really. It we turn that statement around it would be correct: The square will be wherever it will be. That is the "driver" for the tolerancing on this part. The position / location of the outer hex shape must be within .xxx from the vertical & horizontal edges of the square.
(The .005 is simply controlling the shape and size of the square itself, as well as perpendicularity to A.)

We are all so used to thinking of the edge of a part as a datum and then locating a hole from the edge. This is the opposite, where the hole is the datum and the edge of the part is located from the hole! It might sound like identical statements but they are not. There is a nuanced difference that could affect how the measurements are reported in the end.

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

 

[pmarc]

HightechHillbilly,
You do not need to locate the square relative to anything, because the square is secondary datum feature from which other features of the part are located. The only things that need to be controlled regarding the square are: 1) its size, 2) form, and 3) orientation to higher precedence datum A. All three characteristics are controlled by this all around profile .005 wrt A.

In other words, as J-P said, the square is the "driver" for tolerancing other features of the part.

 

[HightechHillbilly]

Belanger,

OK, so I understand what you are saying now re: "The square will be wherever it will be. That is the "driver" for the tolerancing on this part. The position / location of the outer hex shape must be within .xxx from the vertical & horizontal edges of the square."

That being said, however, what keeps the square from ending up too far up, down, left, or right? The part (in this case, the crowfoot wrench head) would NOT function properly, much less "look" right, if the square hole ended up in some weird location (see attachment).

So, I *think* I need some way to control the position / location of where the square should be in relation to the geometrical shape of the part.

Sorry for beating this to death, but as I said, dimensioning such an irregular shaped part is new to me.

Thanks,
Rob

 

[HightechHillbilly]

Going back & re-reading Belanger's comment, as well as Pmarc's comment, I think I'm getting it now.

If I understand it, then I would need the profile tolerance for the perimeter of the part (the 2nd "X-Y" profile tolerance with respect to Datums "A" and "B").

Reason being, the profile tolerance for the hex shape will be controlled with respect to the square & Datum "A" but the overall "shape" (ie, geometry of the part) had not yet been controlled. Once the profile tolerance for the perimeter is added, now the overall shape is controlled, again, with respect to the position of the square, as well as Datum "A"

Am I getting it now?? heh

Thanks,
Rob

 

[pmarc]

Yes, that is right.

Do you have access to the newest version of Y14.5 (from 2009)? If yes, take a look at fig. 4-5 for instance. It does not show secondary datum feature controlled by profile callout, but is nicely presents this whole logic. Notice that on this figure secondary datum feature B is not controlled for location too, and that is absolutely fine, because this is the feature from which other features (slot width, and 3 holes) are located.

 

[HightechHillbilly]

Pmarc,

Yes, I have access to Y14.5, 2009. Looking at Fig 4-5 helps drive the point home that you & Belanger were trying to make. One other clarification regarding Fig 4-5, just to make sure I understand - to provide enough information to manufacture that part, there would need to be a diameter dimension called out for the overall circular shape of the part, correct? It doesn't necessarily need to be "controlled" via a profile tolerance, it could just be a dimension with the default tolerance specified in the Title Block.

And to relate Fig 4-5 to my crowfoot, if I did not set a profile tolerance for the perimeter, I would have to provide a dimension for the diameter or radial dimension for the circular portion, as well as a radial dimension for the smaller round portion (the end curve closest to the square), then somehow dimension the to straight surfaces which connect the smaller round feature to the larger circular feature - correct? But, being as that might be complicated, it's best to just set a profile tolerance to the perimeter, and control that entire geometry to the position of wherever the square ends up.

Is what I said above correct? I hope so, otherwise I'm back to square one regarding my understanding. heh

Thanks,
Rob

 

[pmarc]

Yes, the overall shape, as well as bottom of slot C, part's thickness, and chamfer on the top of datum feature B, needs to be controlled to make the drawing complete (keep in mind that figures in the standard are intentionally incomplete). Yes, this does not have to be profile tolerance - simple directly toleranced dimension plus a positional callout applied to it will do the job too.

In your case I would still recommend profile tolerance wrt A|B and basic dimensions defining true profile of the perimeter. Collection of directly toleranced dimensions for radii/diameters will not make this drawing unambiguous.

Side question: What kind of fit between the square hole and the square tab is designed? If this is always a loose fit, perhaps it would make sense to call out B at MMB (that is to put modifier (M) after B) in both X<-->Y profile callouts.

 

[HightechHillbilly]

Pmarc,

OK, looks like it's finally starting to sink in now! I'm really appreciative of the information you & Belanger provided, as this type of "real life" scenario is something which most books & tutorials do not cover, and I feel that my task would be considered somewhat higher level GD&T (maybe not to you, perhaps, but it definitely was to me) ;-)

As far as the fit between the square hole in the part, and the square tab in the ratchet it attaches to, I do not have that information as of yet. However, just thinking of typical "ratchet-to-attachment" interfaces, I believe there will be a ball-type retention on the ratchet's square tab which will help hold the crowfoot on the ratchet.

At any rate, when I get to that point, I can reevaluate the requirements for fit, keeping in mind your suggestions, & make modifications to the GD&T, if necessary.

I feel much more confident in my finalization of this drawing now - so I cannot thank you & Belanger enough for helping me to overcome my "fear of GD&T" & provide me w/ valuable information! Thanks!!

 

[Belanger]

Glad to help! A lot of GD&T is about the philosophy of things rather than just symbols and numbers

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