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!

*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.


implied % of thread.

implied % of thread.

It is fairly common on drawings to call out a tapped hole along these lines.
∅ 3/8-16 UNC-2B x.984 deep

Some folks prefer, or even insist, on including a tap drill size, and a tap drill depth.

My first concern comes from the fact some of our drawings call for a tap drill depth has been un-necessarily shallow, just 1 or 2 pitches deeper than the thread depth we want, even with the danger of "breaking through" is remote.

My 2nd concern with that is some threads are not necessarily made by tapping, but can be created by thread milling.
I would not insist that milled thread include a tap drill sized hole that extends beyond the usable threads.

But what the short version seems to leave open is the % of thread that will be created.
Specifying (the correct!) tap drill would keep the % thread to 75% or so.

A bunch of Googling, and a search of this forum, has not come up with much of anything about the % thread depth that is expected when the thread diameter and pitch and class are all that are specified.

Does anyone know a standard that addresses percent thread depth when tap drill size is omitted?

RE: implied % of thread.

All I know is that when I specify, say, 1/4-20 x 1.00, I expect 1.00" minimum of useable thread. Every machine shop I have ever sent work (and there's a lot of them) has understood this- I don't think I've ever been asked this question.

I also never specify tap drill depth unless there are very specific circumstances that require it. If I need to tell my machinist which drill size to use for M10 thread, I should focus my effort on finding another machinist.

RE: implied % of thread.

Hi jgKRI,

I share your opinions. pipe

It still leaves the percent of thread free to roam the range though.


Dan T

RE: implied % of thread.

yes, it does.

RE: implied % of thread.


Who cares what the percentage is? I specify the thread depth. I want at least that. If I need the hole to be blind, I will specify blind, and let the shop figure out how to do it.


RE: implied % of thread.

Quote (Tmoose)

It still leaves the percent of thread free to roam the range though.

I guess this is the source of confusion.

This callout:

∅ 3/8-16 UNC-2B x.984

does not leave the length of useable thread 'free to roam the range'. You are specifying nine hundred eighty four thousandths of useable thread. Period.

If there is no tolerance on that callout, than your thread depth is controlled by the general tolerance statement on your drawing.

RE: implied % of thread.

I believe Tmoose talking about the thread form, rather than the depth of a tapped hole. Most tap drill charts are based on 75% of theoretical thread profile i.e. crests are flattened.

Unfortunately I don't know the answer to the question.



The problem with sloppy work is that the supply FAR EXCEEDS the demand

RE: implied % of thread.

Quote (SnTMan (Mechanical) 2 Dec 16 00:24)

I believe Tmoose talking about the thread form, rather than the depth of a tapped hole. Most tap drill charts are based on 75% of theoretical thread profile i.e. crests are flattened.

Unfortunately I don't know the answer to the question.

A "perfect" cut thread using the a perfectly aligned and perfectly centered "perfect" tapped hole drillsize will still vary only slightly from the nominal tapped hole using a nominal tap drill size using a manually-aimed and centered drill and manual tap. The very slight "extra" margin of the usual tap drill size will make the tapping operation easier, faster, and more reliable (many fewer broken taps inside slightly-too-tight holes) while creating adequate thread strength in adequately aligned (manually-drilled) holes. Thus, a nominal tap drill hole may have 60% thread (instead of 75% thread depth) but will perform adequately in all real world circumstances.

Sure - USE the CORRECT tap hole drill from the charts. But the slight difference in theoretical thread engagement is not going to come from you (the engineer) writing that in the tapped hole definition on the dwg. It will come from the shop after you define what threads are needed where to what depoth with what bottoming specification of the hole. A too-short thread will NOT engage sufficiently and WILL break off lifting lugs if wrongly defined thread and drilled holes depth.

RE: implied % of thread.

"But the slight difference in theoretical thread engagement is not going to come from you (the engineer) writing that in the tapped hole definition on the dwg.........."

I agree sufficient length of thread engagement of the fastener is a mighty important strength factor. Note the .984/.375 = 2.6 diameters of engagement in the example thread callout.
∅ 3/8-16 UNC-2B x.984 deep


"Sure - USE the CORRECT tap hole drill from the charts."

My OP was regarding the tap drill size "assumption" behind the simple thread callout.
∅ 3/8-16 UNC-2B x.984 deep

The actual size hole a drill will make is widely recognized as being pretty variable, to the tune of about 5% less %thread than theoretical.
Some folks don't even consider the perfect situation.
They create tables and charts that include info about "probable" drilled hole sizes and resulting 5% or so loss of thread % when using tap drill sizes right from the standard tables.

I'm pretty sure a drill sharpened by me, by hand, is going to drill even more oversize. So in the extremely unlikely event I'm on the ragged edge of overall thread strength, and think I "need" 75% thread, a check of minor diameter of every tapped hole on incoming parts might be wise.

Or routinely check all tapped holes just to be sure somebody didn't inadvertently use a "Q" tap drill pulled from "O" drill drawer.
"Man, those new Harbor Freight taps are great, They cut like buttah".


" The minor diameter of GO and NOGO threaded plug gages are smaller than the smallest allowable
minor diameter of the nut thread. The GO and NOGO thread plug gage will never detect an oversized
nut minor diameter. "


An oversized tap drill hole nearly the size of the pitch diameter (.328 for a 3/8-16 thread) would go undetected with normal thread plug gages.

This claims ASME B1.1 says the maximum minor diameter for a 2B 3/8-16 is .321", which mighty close to the probable hole size for an O drill.


I'm starting to think a reference to ASME B1.1 needs to appear in the tolerance block on the drawing.

RE: implied % of thread.

No. You're working too hard. Unless the safety margin of this particular series of tapped holes is closer to 1.05 than 1.5, 1.75, or the more normal 2.5 to 3.5 (on each tapped hole), the fasteners will hold.

RE: implied % of thread.

I always specify tap drill diameter tolerance limits and a max depth of the hole cylinder, a full thread specification and min complete thread depth, and a countersink at the hole leading edge with angle and diameter tolerances. Always a good idea to make your drawing callouts as explicit as possible. It doesn't require much extra effort, and it will ensure you get exactly what you want. If your vendor has an issue with what you call out, he will always let you know about it.

RE: implied % of thread.

There is no need to specify a tap drill size in a thread callout and doing so will often drive the cost of your part up while making you look foolish. Every relevant dimension is already called out between size, thread form, thread class, and thread depth, calculating thread engagement from this is basic arithmetic. Dictating tap drill dimension/tolerance and thread class in the same callout therefore is similar to placing a reference dimension next to a standard dimension for the same feature, an obviously silly mistake most engineers learn in the required 1st year drafting/print reading. If you need to call out a nonstandard thread form for extreme engagement, proprietary, or other reasons then you need a fully dimensioned view of the thread itself.

One easy rule to remember is that engineering prints dictate design intent, manufacturing process sheets and work instructions dictate manufacturing methods and tool usage. In this case you only care about the finished thread, not the drill necessary to get there, so calling out the drill is effectively knee-capping your machinists and if not done properly is an easy way to get into excessive amounts of tool wear and failure.

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