Smart questions
Smart answers
Smart people
Join Eng-Tips Forums
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Member Login




Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • 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!

Join Eng-Tips
*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.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

tunalover (Mechanical) (OP)
1 Oct 04 12:51
Guys-
I'm a design engineer and am looking for an authoritative source for run-of-the-mill size tolerances on drilled and punched holes.  I've spoken to three machinists and each have given me different ideas on what "the standard" is.

One source, Engineers Edge(www.engineersedge.com/drill_sizes.htm) gives the following diameter ranges and tolerances:
.0135-/125:  +.004/-.001
.126-.250:  +.005/-.001
.251-.500:  +.006/-.001
.501-.750:  +.008/-.001
.751-1.000: +.010/-.001
1.001-2.000:  +.012/-.001
but they provide no rationale or data to substantiate the tolerances!

Thanks!



Tunalover

Helpful Member!  mrainey (Industrial)
1 Oct 04 16:29
From my Machinery's Handbook, Twentieth Ed, p.1668

"The following formulas give the amount of hole oversize to be expected in normal drilling operations within .001 inch for drills of 1/8 to 1 inch diameter:

Maximum Oversize = .005 + .005D
Minimum Oversize = .001 + .003D

where D is the nominal drill diameter in inches."


I don't see this as being a standard, just a helpful rule of thumb.

Manufacturing Freeware and Shareware
http://mrainey.freeservers.com

Helpful Member!  BillPSU (Industrial)
2 Oct 04 9:08
Hole size tolerances to my knowledge have not be published by a standards organization, however some companies have some sort of shop practice or engineering standards of holes. I have old Allis-Chalmers and an old Catepillar guides. Cat groups them by class of holes A-F. The classes really means what method is used to produced the hole such as drilling, punching, or flamecutting. Punched holes in both guides show some sort of breakout tolerance for punched holes and is based on the thickness of the material.

The rationale behind the tolerances is based on experience. A normally sharpened drill will produce the hole sizes listed from some sort of study or they were plagarized from someone else's standards book. The Allis Chalmer shop practice guide shows the following tolerances for drilled or the top of punched holes:

0 to .125        -.002/+.005
.125 to .250     -.002/+.006
.250 to .500     -.002/+.008
.500 to .750     -.002/+.009
.750 to 1.000    -.002/+.010
1.000 to 2.000   -.002/+.016
2.000 to 3.500   -.005/+.025

Breakout for Allis Chalmers follows:

Thickness           Oversize at bottom
0 to .015               .006
.015 to .040            .008
.040 to .125            .02
.125 to .250            .03
.250 to .500            .04
.500 to .750            .05

I won't publish the Cat standards as they are still in business and may show releasing this info as a violation of their copyright.

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!

Back To Forum

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