Calculating tap drill size

[mklotz]

The suggested tap drills on most charts are the size needed for a 77% depth-of-thread (DOT). If you're working with hard to tap materials, you can significantly reduce the tapping effort and chance of tap breakage by using a smaller DOT with only a very small loss of joint strength. The DRILL program on my website will suggest DOTs and calculate the required tap drill but it's not hard to do it yourself with a desktop calculator.

The generalized formula for 60 degree threads is:

TD = MD - 0.013*DOT/P

where:

TD = tap drill size
MD = major diameter of thread
DOT = desired depth of thread expressed as a percentage
P = thread pitch expressed as TPI

As an example, for a 1/4-20 thread with 75% DOT we have

TD = 0.25 - 0.013*75/20 = 0.201"

which corresponds to a #7 drill.

Some of you may be familiar with the simpler formula

TD = MD - 1/P

Here the product 0.013*DOT has been taken equal to 1. If we solve for DOT, we have:

DOT = 1/0.013 = 76.9%

so the simpler formula will always produce a drill that will yield a 77% DOT which is a bit too much for many situations.

The suggested DOTs used in my program are...


MILD AND UNTREATED STEELS 60-65
HIGH CARBON STEEL 50
HIGH SPEED STEEL 55
STAINLESS STEEL 50
FREE CUTTING STAINLESS STEEL 60
CAST IRON 70-75
WROUGHT ALUMINUM 65
CAST ALUMINUM 75
WROUGHT COPPER 60
FREE CUTTING YELLOW BRASS 70
DRAWN BRASS 65
MANGANESE BRONZE 55
MONEL METAL 55-60
NICKEL SILVER (GERMAN SILVER) 50-60