Drilling depths for easy tapping

A major challenge when creating threads is to avoid breaking the tap. A tap breaks when the drilled hole is not deep enough. Broken taps cause lost time, broken tools, and scrapped parts. With some foresight and a few simple calculations we can reduce the risk of breaking taps.

Take a look at this example. The full drill depth is 1.4" and the full tap thread depth is 1.0". The difference between the two is only 0.400".

The limited amount of space means there is little room for error. If the tap depth exceeds the drill depth, the hole will not be deep enough and the tap breaks.

Drill depth

Program the drill deep enough to allow for the tap's point. The example shows the full drill depth. To calculate the programmed value, determine the drill point allowance and add it to the full drill depth.

The point allowance depends on the type of drill and its diameter. Each drill type has a rule for calculating the drill point:

Rules for drill point allowance:
• For HSS drills with a 118 deg included angle the formula is: drill dia x 0.3 = drill point allowance
• For Cobalt drills with a 135 deg included angle the formula is: drill dia x 0.2 = drill point allowance

When programming the hole (5/8 - 11 TPI), consult a tap drill chart and use a 17/32 dia HSS drill (0.531''). Calculate the point allowance: 0.531x 0.3 = 0.159.

Add the point allowance to the required drill depth to achieve the programmed depth. 1.4 + 0.159 = 1.559 (Z-1.559) Tap chamfer clearance The hole requires 1.0'' of full threads. You must allow for the chamfer on the lead of the tap when programming. The programmed depth of the tap must be larger than the 1.0'' listed on the print; the difference is the tap chamfer. To calculate the length of the chamfer, use the appropriate formula. Tap chamfers are identified by the terms, taper (longest lead chamfer), plug (medium lead chamfer), and bottoming (shortest lead chamfer).

Rules for tap chamfers:
• taper tap chamfer = thread pitch x 9
• plug tap chamfer = thread pitch x 4
• bottoming tap chamfer = thread pitch x 1.5

On the above Add the chamfer length to the required full thread depth from the print: 1.0 + 0.3636 = 1.3636 (Z-1.3636)

Making these simple calculations alters the depths to allow for actual tool lengths, reducing the chance of the tap breaking. Drilling and tapping are everyday procedures, but breaking taps and making scrap don't have to be part of this process. Keeping these few simple rules handy can make this frustrating process easier. For a chart of these calculations, visit our web site at http://www.cnc-training.com