Of late, we have been machining numerous prototype designs that have come through our online instant quote system that require threaded holes. Much of this prototype work comes from entrepreneurs or students who, in some cases, are unfamiliar with machining and the requirements for specifying threaded holes.
Although there are multiple methods for creating threaded holes, the most economical and fastest is using a drill followed by a tap. Many of the drawings or sketches we receive do not consider the requirements for specifying a tapped hole, especially blind tapped holes.
We hope the following information will be helpful to those who are new to mechanical drawings and specifications.
Background on Taps:
There are two basic types of taps: cutting tabs and thread-forming taps. A cutting tap creates the thread by cutting into the wall of the drilled hole to make the thread form. Thread-forming taps, as the name implies, form the thread by deforming the material in the wall of the drilled hole.
Whichever type of tap is used, all require the drilled hole to be deeper than the threaded hole depth. This is because the thread form on the tap does not begin at the tip. All taps have some initial threads which partially form the thread. These lead-in sections are different lengths depending on the size and type of tap selected.
With cutting-style taps, there are three basic types: taper, plug, and bottom. Taper taps have the longest lead-in length, followed by plug and bottom taps. Thread form taps typically have a short lead-in section, equivalent to a bottom tap in most cases.
Different types of thread fits can also be specified for a tapped hole. We won’t outline the different types here, but if you want to learn more about taps and thread fits, the Machinery’s Handbook is a great reference. This book is invaluable when designing mechanical components.
A pdf version of the 29th edition can be downloaded from our downloads page or by selecting the following link: (machinerys-handbook-29th-edition)
We have also posted a pdf Imperial and metric drill and tap chart on our downloads page.
Drawing Specifications for Threaded Holes:
Different tap manufacturers have different amounts of lead-in. However, as a general rule, the depth of the drilled hole should be, at a minimum, three times the thread pitch deeper than the required thread depth. As an example, a ¼-20 threaded hole with a ½” thread depth requirement should have a minimum hole depth specification of .650” (one pitch (1/20) is .05” and 3 x .05” + .5” = .650”)
A full specification on a drawing or sketch would be as follows for a ¼-20 UNC class 2B cut tap blind hole:
Ø .201 x .650 DP
¼-20 UNC 2B x .5 DP
If you have a CAD package, the symbols (downward arrows) are used to indicate depth.
However, a simpler method is to only provide the type of thread and depth as follows:
¼-20 UNC 2B x .5 DP
In most cases, the drilled hole diameter and depth are unnecessary.
If there is concern about breaking through a wall with the drilled hole, a limitation can be added to the specification as follows:
¼-20 UNC 2B x .5 DP, NO BREAK THRU
Renovo CNC