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


Determining Position Tolerance Value

Determining Position Tolerance Value

Determining Position Tolerance Value


I understand most GD&T and how to interpret a position callout, however, I'm still a little confused on how to actually determine the correct value for diametrical position callouts.

Please let me know if my below method is correct:

1. Two parts are to be bolted together via a pattern of 4 .25-28 UNF-2B bolts.
2. From online tables, I have determined the correct close-fit clearance hole to be .266 +.006/-.001 (.265 to .272).
3. From this, subtract the bolt major diameter from the smallest hole: .265 - .250 = .015
4. Therefore, I have .015 tolerance to split between the two 4-bolt patterns (.010 and .005 or .007 and .008 for example)

I feel like this is too simple. Does the threaded hole not come into play at all?
What book and or website do you guys use/recommend as a good resource for GD&T?

Any help is much appreciated.

RE: Determining Position Tolerance Value

Retsied, ASME Y14.5M-1994 has the equations in appendix B4 and I've posted an excel sheet* before that has the most basic 'fixed' fastener version that you invoke above in it.

It also gives guidance on projected tolerance or over-sizing the hole in lieu.

I suggest you take a look at the proverbial 'horses mouth'.

BTW, I'd think twice putting much less than a .010 tolerance on a threaded hole - it's often better to split the tolerance allowance with a bit more going to the threaded hole than the clearance hole due to typical process capabilities for threaded V plain holes.

The typical 'close fit' holes may be more applicable for floating fastener than fixed fastener so take them with a pinch of salt as they can lead to unnecessarily tight position tolerances.

(*Be careful there's a bit of an error on a tab relating to converting +- dims to pos tol.)

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Determining Position Tolerance Value

If you have Y14.5 2009 std, pls look at page 191~193 Appendix B.


RE: Determining Position Tolerance Value

Thanks for the replies and reference to Y14.5-2009. After looking over this, it appears I have done it right. Just seemed too simple to me. Thanks guys!

RE: Determining Position Tolerance Value

Not sure if this discussion is still active or not, but I think it is worth to mention that what OP said in initial post (that there is 0.15 to split between the clearance holes and threaded holes) is true only if projected tolerance zone concept is used in conjuction with position tolerance applied to the pattern of threaed holes.

If the projected tolerance zone concept is not used, possible orientation error of the threaded holes relative to mating face needs to be taken into account - and this is where additional threaded hole parameter, that is ,the minimum depth of engagement of threaded member comes into play. The formula in Appendix B.5 of Y14.5-2009 shows how it is done.

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!


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close