Positional Tolerance 2

[Seco1]

We have a discrepancy between options about the positional tolerance of a drilled hole in a cast part. I would appreciate anothers opinion. The drawing calls out the following tolerance (as closely as I can imitate the actual call outs, I wish I could attach a drawing):

4 HOLES (diameter symbol)9.0 +-0.2
(control frame)|(position symbol)|(diameter symbol)0.3|A|B|E (end of control frame)
CHAMFER (diameter)10.2 +-0.2 * 45

The horizontal and vertical linear dimensions (for one hole for example) are marked as 29 (horizontal from center) and 50.23 (vertical from center). There is no specific tolerance called out on these dimensions. The title block also has a note about unspecified tolerance on linear dimensions equal +-.2.

What linear tolerances apply to this 9mm hole?

Thanks in advance,

Steve

 

[ringman]

No Standard being specified.... The whole thing is anyone's guess.

This is not necessarily an uncommon occurence, sadly.

 

[kbro151]

Seco1, the lack of a specified standard on the drawing does not mean that you can't apply a standard. Either the customer specifies a standard or you do. If your company consistently works to a standard, that should be on your bids/contracts. If the customer wanted a standard, that should be on their documents.

Heckler had it right; positional tolerance trumps title block tolerance. Positional callouts are basic dimensions, and the title block tolerance only applies if no other tolerance is specified. The positional tolerance called out is tighter than the title block tolerance, not looser. danap's post on the location of the hole is a good explanation. However, you don't need a note saying that the positional dimensions are basic. They are always basic. The tolerancing comes from the positional callout.

 

[ewh]

kbro151,
In this situation, I agree. However, it is not a good idea to use a blanket statement like "you don't need a note saying that the positional dimensions are basic. They are always basic." Wrong. It may be acceptable to interpret this drawing in this manner, but it is still a drawing mistake. For a correct drawing, you DO need either a note or a block around basic dimensions. Without those, there is ambiguity regarding the dimensions.

 

[tank627]

the "untoleranced dimnesions are basic" clause may be buried in some other spec.

 

[kbro151]

We aren't discussing new drawings. For new drawings, I don't believe a note qualifying basic dimensions meets either ISO or ANSI specifications. A block meets ANSI. Not using a block does not meet ANSI.

A dimension locating the position of a feature is a basic dimension. That is part of the definition of position. If the dimension is not basic, then it does not give you the position of the feature.

 

[ewh]

See ASME Y14.5 para 5.2.2.1(b) regarding untoleranced dimensions (untoleranced dimensions locating true position are basic).

 

[MechNorth]

A few things here;

1) You need to have a note on the drawing, or in documentation referenced on the drawing, which clearly states what standard the drawing adheres to. Without that, there is no way to interpret a drawing that mixes linear and geometric tolerancing. In this case, if the drawing is from Europe, it's probably ISO, so assuming ASME/ANSI interpretation could be incorrect.

2) A positional tolerance can only be used on a Feature of Size, which this hole is (it has linear size tolerances).

3) A positional tolerance requires basic dimensions to locate the feature wrt the datums. There must be (i)a BASIC box around the dimension, or (ii) a note on the drawing to the effect of "NON-TOLERANCED DIMENSIONS ARE BASIC" (which disallows the use of a linear general tolerance block), or such similar statement must be contained in a document referenced on the drawing. As neither of these are indicated on the drawing, those dimensions cannot be interpreted as BASIC (I know it seems logical to assume they're BASIC because of the positional tolerance, but that's not a path of logic that a court is likely to take).

4) Linear general tolerances in the title block need a statement such as "UNLESS OTHERWISE SPECIFIED", or else they are meaningless, and inapplicable on the drawing.

5) Absent any statement or reference to those locational dimensions being basic, and since they do not have a linear tolerance on them, you would be compelled to use the general tolerances in the title block (providing the "UNLESS OTHERWISE SPECIFIED" note from #4 is invoked)

Intuition is a great thing, but the courts don't tend to buy it as an acceptable reason for doing something. Where the work doesn't follow the rules, courts will tend to follow a line of logic that best follows the rules.

Now the reality; your client wants you to make parts. Period. If they're not willing/able to correct the drawings, your next best solution is to ask which interpretation they want, and then send them an e-mail with detailed minutes of your conversation. If you have the time, YOU should create a drawing with the correct GD&T on it and send it to them.

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca

 

[ewh]

Bravo Jim!