×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Are you an
Engineering professional?
Join Eng-Tips Forums!
• Talk With Other Members
• Be Notified Of Responses
• Keyword Search
Favorite Forums
• Automated Signatures
• Best Of All, It's Free!

*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.

Size tolerances on drilled and punched holes2

Size tolerances on drilled and punched holes

(OP)
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

RE: Size tolerances on drilled and punched holes

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

RE: Size tolerances on drilled and punched holes

Hole size tolerances to my knowledge have not be published by a standards organization, however some companies have some sort of shop practice or engineering standards of holes.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.

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.

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:

• Talk To Other Members
• Notification Of Responses To Questions
• Favorite Forums One Click Access
• Keyword Search Of All Posts, And More...

Register now while it's still free!