Tap Drills and Tapping
Estimate a cutting-tap drill, distinguish thread percentage from engagement length, and plan tap geometry, alignment and depth.
Subtract the pitch to estimate a cutting-tap drill; Practice
Subtract the pitch to estimate a cutting-tap drill
A tap makes an internal thread in a prepared hole. Start by reading the full thread callout. For common straight Unified and metric cutting taps, a useful roughly 75% thread estimate is:
- Inch: drill diameter ≈ nominal major diameter − 1/TPI. Both diameters are in inches; TPI means threads per inch.
- Metric: drill diameter ≈ nominal major diameter − pitch. Both dimensions are in millimeters.
This is an estimate, not a final hole specification. Use the major diameter, not the minor or pitch diameter. Select the actual drill from the tap maker's chart for the material and required thread. Do not apply this cutting-tap estimate to forming taps, pipe threads or insert-installation taps.
| Thread | Estimate | Cutting-tap chart comparison |
|---|---|---|
| 1/4-20 | 0.250 − 1/20 = 0.200 in | No. 7, 0.2010 in |
| M6 × 1 | 6 − 1 = 5.00 mm | 5.00 mm |
| 3/8-16 | 0.375 − 1/16 = 0.3125 in | 5/16 in, 0.3125 in |
Chart basis and the approximation's limits
The three comparisons were checked against page 1, cutting-tap column, of North American Tool's Tap Drill Sizes — Inch & Metric with Drill Size Formulas, using the supplied four-page copy. Only these selected rows are used here; the chart is not reproduced. The estimate and a selected stock drill need not be identical. The chart's metric percentage formula gives about 77% when the entire pitch is subtracted, which is why “about 75%” must remain approximate.
Thread percentage is not percent of bolt strength; Practice
Thread percentage is not percent of bolt strength
Percent thread describes how much thread height the hole permits relative to a reference profile. With the same cutting tap, a larger prepared hole leaves less thread height; a smaller hole leaves more material for the tap to remove and generally increases tapping torque.
It does not describe how far the screw enters the hole. That is engagement length. Nor does 75% thread mean 75% joint strength. Material, engagement length, thread geometry and loading all affect the joint. More thread height is not automatically a better choice.
Keep percentage and fraction separate
For a metric cutting-tap estimate, the supplied chart gives hole diameter = major diameter − (percentage × pitch / 76.98), entering 75 for 75%. Equivalently, multiplying a reference thread depth by 75% requires the fraction 0.75. Mixing those conventions introduces a factor-of-100 error. This formula estimates geometry, not allowable joint load.
Taper, plug and bottoming describe the tap's lead-in
Taper, plug and bottoming describe the tap's lead-in
The chamfer is the gradual lead-in where the first teeth progressively cut the thread. A taper tap has a long lead-in that helps starting; a plug tap has a shorter lead-in; a bottoming tap has the shortest of the three and reaches full thread closer to the bottom of a blind hole.
A bottoming tap still has a lead-in. It cannot produce full thread all the way to the physical bottom. For hand tapping, start with a tap that can establish alignment, then use a bottoming tap when the required depth calls for it. Leave room for incomplete threads, chips and the drill point.
Chamfer style is separate from chip direction. A spiral-point cutting tap generally pushes chips ahead and needs exit space; a spiral-flute cutting tap can draw chips back toward the entrance. Select a tap intended for the material and through or blind hole.
Use a guide to start a hand tap square; Checklist
Use a guide to start a hand tap square
- Confirm thread size, tap type, drill size, actual hole size and required full-thread depth.
- Prepare the hole entrance as specified. Clamp the work or hold it in a vise rather than by hand; see Machine Hazards for why. Choose the tap maker's recommended lubricant for the material.
- Align the tap with a suitable tapping guide. With a spindle used as a guide, keep it unpowered and follow the approved hand-tapping setup.
- Turn with a suitable tap wrench while maintaining alignment. Follow the tap's chip-breaking instructions; do not force a tap whose resistance rises unexpectedly.
- Keep within the planned travel, withdraw appropriately, clean and inspect the thread with the specified gauge or inspection method.
To help prevent broken taps, use the correct tap drill, maintain alignment, clear chips as the tap's instructions specify, use the recommended lubricant and do not force the tap. Reverse-to-break-chip routines depend on tap design; do not apply one hand-tapping rhythm to every tap.
For injury hazards, operating rules and chip handling, see Machine Hazards and Housekeeping, Personal Protective Equipment and Metal Chips and Swarf.
Power tapping needs a machine and holder designed for it
Power tapping needs a machine and holder designed for it
Machine tapping coordinates spindle rotation with axial travel at the thread's lead. Depending on the machine, that may use synchronized rigid tapping or a suitable tapping attachment. The machine, holder, tap, reversal and depth control must work together. An ordinary drill-press setup is not automatically a power-tapping setup.
A cutting tap removes chips. A forming tap displaces suitable ductile material to make the thread without cutting chips. Forming taps require their own, generally larger, prepared-hole sizes and suitable lubrication. A cutting-tap drill can be much too small for a forming tap of the same thread size.
Use the machine's instructions and the approved shop procedure for tapping equipment.
Why the local setup decides what is permitted
Recognizing a production process does not authorize it on a particular machine. Spindle speed, tapping attachment and power-tapping procedure depend on the particular machine and setup.