×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Positional Tolerance
2

Positional Tolerance

Positional Tolerance

(OP)
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

RE: Positional Tolerance

What good is a positional tolerance on a +/- located feature?  The positional dimensioning should somehow relate back to your datums, and should be basic.

RE: Positional Tolerance

The locating dimensions must be basic.  You can calculate what the linear tolerances would be if you were not using the true position callout....remember the square inscribed in the circle

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

RE: Positional Tolerance

(OP)
I'm sorry I did not make myself clear ... these are not my drawings or can I change them in any way.  I'm simply trying to interpret what is already there.  I'm just not sure how to.  Well, I'm pretty sure I get what the drawing is getting at, but them someone says your wrong, doubts creep in and you post on message boards :).  The main discrepency is the linear tolerancing of the hole position.  Is it a priority issue (.3 in the control block or .2 in the title block)?

RE: Positional Tolerance

You could play it safe and ASSUME the locating dimensions are basic, or you could assume that the geometric control is in error.  I would play it safe and consider the dimensions basic (provided they do link back to the referred datums).

RE: Positional Tolerance

Since the True Position is taken at RFS (regardless of feature size) you get no bonus tolerance from the feature tolerance.  The title block tolerances should only apply is no other tolerances are specified.  Their should be a note somewhere in the title block that states "Unless Otherwise Specified"

Have you had any formal training in the area of GD&T?

RE: Positional Tolerance

I actually don't think this one is that confusing.  Before the days of CAD, a lot of effort went into ensuring that drawings were as simple as possible, with the minimum of data required.  It took a long time to add dimensions, notes, callouts, etc.  I know times have changed, and it is now quite easy to overdimension or put notes in everywhere.  If I had a drawing like Seco1, I would assume:

1) title block doesn't apply whenever someone goes to the trouble of specifying a tolerance, and

2) no one 'accidentally' adds a positinoal tolerance callout.

I know, never say never, but this would be my starting point.

Things that supoprt it are heckler's points about rfs and the usual notes in a tolerance block that qualify when the block is applied, and the fact that the positional callout is tighter than the tolerance block.

RE: Positional Tolerance

(OP)
Thank you for your replies.  Personally, no I wouldn't say I have formal training in GD&T, but many years of practical experience.  In a nutshell, we are a manufacturing plant and I disagree with the customers interpretation of the tolerancing on this old drawing.  I too have been assuming basic location tolerancing.  Of course the customer is always right, but if I could show the purchasing agent (who does know anything about GD&T) something concrete it would make my life considerably less complicated.  I spent sometime checking ASME today, but have not yet found anything.  I was hoping to be able to craft (or find one) a simple explanation of standards, not that they necessarily have to follow standards.

RE: Positional Tolerance

Is the chamfer dia suppose to be part of the FCF?
I would make it a separate callout.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

RE: Positional Tolerance

Sounds like they just forgot to put the box around the basic dimension.  I'd treat the 29 and 50.23 as basic.

RE: Positional Tolerance

I told you an explaination, according to you original post it's true position regardless of feature size of DIA 0.3 mm.....so in practical terms regardless of what size the feature comes in between 8.8 - 9.2 mm it's location must be within a 0.3 mm diameter tolerance zone.  This translates into +/- 0.21 mm linear tolerance if you do the math....remember the diameter with the inscribed square I was talking about earlier...... the diagonal of the square is 0.3mm so the leg is Cos 45 = leg/0.3 = 0.21

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

RE: Positional Tolerance

kbro151,
If you are drawing to ASME Y14.5, nothing has changed in regard to simple drawings.  It is still standard practice to include the minimum number of dimensions needed to make the part.  A good drawing is a concise drawing.  Be it a board drawing or a CAD drawing, this still applies.

RE: Positional Tolerance

Seco1,
If the purchasing agent knows something about GD&T, just showing him the situation should be enough without having to provide concrete evidence for your position.

RE: Positional Tolerance

Seco1, Machinery's Handbook has a table in the inspection section that is simple enough for even a purchasing agent to understand.  It clearly says position callouts use basic dimensions and RFS is implied unless MMC or LMC is stated.

ewh, of course drawings should still be simple and concise.  My point was that it is incredibly easy these days to overdo it.  It takes 10 seconds to add a dimension.  It used to take a few minutes, more if you had removed the drawing from your desk.  In the time it now takes to dimension and add callouts, you used to have plenty of time to consider the necessity of a note, callout, or dimension.  That time and incentive to think was built in.  Now, it isn't.  Usd to be learning to draft took a big time investment.  Now the time to produce working drawings is much, much shorter.  This is one reason why, in my experience at least, we have a lot of drawings being dranked out for production by a bunch of folks with a less than perfect understanding of drawing, never mind GD&T.

RE: Positional Tolerance

Which is why I miss good drawing checkers...

RE: Positional Tolerance

lol....

are you saying that you still have checkers?  Never mind good ones...

I have to badger ppl to check my drawings around here.

RE: Positional Tolerance

Checker is one of the hats that I wear around here.  Problem is that I create many of the drawings, and it is hard to get someone to check my drawings as critically as I do theirs.
hairpull

RE: Positional Tolerance

From ASME Y14.5M-1994

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

The center of the hole (9.0) has to be inside a circle of 0.3 where the center of that circle is located at 29 (horizontal from center) and 50.23 (vertical from center) - This assumes the 29 & 50.23 are BASIC(read as "theoretically exact, ideal, nominal"), there should be a note somewhere that states UNTOLERANCED DIMENSIONS LOCATING TRUE POSITION ARE BASIC.

If you want to use plus minus dimensions you would divide the tolerance by 2 and multiply by 0.707: (0.3/2)* 0.707 = 0.11 so the tolerance is now +/-0.11

Doing this would not violate the customer specification of being within 0.15 of the BASIC or nominal hole location.

RE: Positional Tolerance

Does the drawing make reference to Y14.5 as being applicable?  Do you have any insight as to the mating condition of the holes?
These are some factors tneed to be taken into account when specifing the tolerances for the holes. with that being said.......

If Y14.5 is referenced.the 0.3 in the callout will be the diametric tolerance.  

RE: Positional Tolerance

(OP)
Thanks again, this is great help.  The drawing does not reference any standard, but it was originally from a source in europe.  If the date is accurate it is from '92.  There are no notes about basic tolerancing, only the note about unspecified tolerances.  If I had to guess, this drawing may have been converted at some point in the past, maybe from hand drawn to digital or from one company to another because of a buyout.  That's just a guess though based on several inaccuracies.

RE: Positional Tolerance

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

This is not necessarily an uncommon occurence, sadly.

RE: Positional Tolerance

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.

RE: Positional Tolerance

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.

RE: Positional Tolerance

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

RE: Positional Tolerance

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.

RE: Positional Tolerance

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

RE: Positional Tolerance

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
www.profileservices.ca

RE: Positional Tolerance

Bravo Jim!

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources