Holemaking and tapping
What are the tapping formulas for tap drill size, percent of thread and feed?
Technical review pending. Formulas and values are cited. This notice comes down after a machinist review.
Tap drill = major diameter minus pitch: D - 1/TPI in inch, D - P in metric. That rule of thumb gives about 77% thread by the Handbook formula; for 5/16-18 it is 0.3125 - 0.0556 = 0.2569 in, so an F drill (0.257 in). Tapping feed is one pitch per revolution: IPM (inches per minute) = RPM / TPI.
Source: Machinery's Handbook (tap drill sizes; percentage of full thread); ASME B1.1 (Unified inch screw threads)
| Quantity | Inch | Metric |
|---|---|---|
| Tap drill (rule of thumb, cut taps) | drill = D - 1 / TPI | drill = D - P |
| Percent of thread for a given drill | % thread = 76.98 x TPI x (D - d) | % thread = (76.98 / P) x (D - d) |
| Drill for a target percent of thread | d = D - % thread / (76.98 x TPI) | d = D - (% thread x P) / 76.98 |
| Tapping feed rate | IPM = RPM / TPI | vf = RPM x P (mm/min) |
| Tapping feed per revolution | IPR = 1 / TPI | fn = P (mm/rev) |
| Tapping spindle speed | RPM = (SFM x 12) / (pi x D) | RPM = (Vc x 1000) / (pi x D) |
The tap drill rule applies to cut taps on Unified and ISO metric 60° threads. It is a rule of thumb; the percent-of-thread formula is the check.
| Symbol | Meaning | Inch unit | Metric unit |
|---|---|---|---|
| D | Major (nominal) diameter of the thread | in | mm |
| TPI | Threads per inch | 1/in | none |
| P | Pitch: 1 / TPI in inch, the number after the x in metric | in | mm |
| d | Drill diameter | in | mm |
| % thread | Percent of full thread height, per the Handbook formula | % | % |
| 76.98 | Constant: 1 / 0.01299, from a double thread depth of 1.299 x P | none | none |
| RPM | Spindle speed | rev/min | rev/min |
| IPM, vf | Feed rate | in/min | mm/min |
| SFM, Vc | Tapping speed from the tap maker's data | ft/min | m/min |
Calculators
Tap drill (D - P rule of thumb)
Tap drill
in
drill = D - 1 / TPI = 0.3125 - 1 / 18 = 0.2569 in
0.2569 in (6.53 mm). About 77% thread. Rule of thumb for cut taps; pick the nearest drill you have and check it below.
Percent of thread for a given drill
Thread engagement
%
% thread = 76.98 x TPI x (D - d) = 76.98 x 18 x (0.3125 - 0.257) = 76.9%
Tapping feed rate
Feed rate
IPM
IPM = RPM / TPI = 400 / 18 = 22.22 IPM
Feed per revolution: 0.0556 in (1 / 18).
Worked example: 5/16-18
A 5/16-18 UNC cut tap in steel, tapped at 400 RPM.
- Find the major diameter and pitch. For 5/16-18: D = 0.3125 in and P = 1 / 18 = 0.0556 in.
- Subtract the pitch from the major diameter: 0.3125 - 0.0556 = 0.2569 in. The nearest standard drill is an F, 0.257 in.
- Check the percent of thread for the F drill: 76.98 x 18 x (0.3125 - 0.257) = 76.98 x 18 x 0.0555 = 76.9, about 77%.
- Compare the next size up, a G drill (0.261 in): 76.98 x 18 x 0.0515 = 71.4, about 71%.
- Set the tapping feed. At 400 RPM: 400 / 18 = 22.22 IPM, which is 0.0556 in per revolution.
Result: F drill (0.257 in, 6.53 mm), about 77% thread, 22.22 IPM feed. Starting points; check the tap maker's data.
Worked example: M8 x 1.25
An M8 x 1.25 cut tap, tapped at 500 RPM.
- Subtract the pitch from the major diameter: 8 - 1.25 = 6.75 mm.
- Take the nearest common drill, 6.8 mm, and check it: (76.98 / 1.25) x (8 - 6.8) = 61.58 x 1.2 = 73.9, about 74%.
- Set the feed: 500 x 1.25 = 625 mm/min.
Result: 6.8 mm drill, about 74% thread, 625 mm/min.
Tapping speed
Tapping RPM comes from the same formula as any other cutting tool, with D as the tap's major diameter: RPM = (SFM x 12) / (pi x D). Take the tapping speed from the tap maker's data for the material and coating; the spindle speed calculator does the arithmetic in inch or metric.
Common mistakes
- Using the D - P rule for a form tap. Form taps need a larger drill from the tap maker's chart.
- Plugging the TPI in where the pitch goes. 18 TPI is a pitch of 0.0556 in, not 18.
- Programming a rigid tapping feed that does not match RPM x pitch. The tap pulls or pushes the thread and the hole gauges oversize or the tap breaks.
- Chasing a higher percent of thread. It raises tapping torque and tap breakage for little gain in strength.
Shop notes
- By hand or on a light drill press, the torque you can feel is the limit. A drill that gives a lower percent of thread cuts tapping torque; check it with the percent calculator above.
- On a rigid CNC with rigid tapping, the feed has to equal RPM x pitch. Many controls take the feed per revolution directly (pitch), which removes the arithmetic.
- A tension-compression tapping holder forgives a small feed mismatch; a solid holder does not.
- Blind holes: drill deeper than the full-thread depth the drawing asks for, so the tap chamfer and the chips have room.
- Percent of thread is a shop check on the drill. An internal thread is inspected against the class 2B minor diameter limits in ASME B1.1 (or 6H in ISO 965 for metric), not against a percentage.
FAQ
What size drill for a 5/16-18 tap?
An F drill (0.257 in). By the percent-of-thread formula it gives about 77% thread. A G drill (0.261 in) gives about 71%.
What percent of thread is right for steel or aluminum?
This is a forum rule of thumb, not a standard: about 60 to 65% in hard steel, about 70% in steel, and 75 to 80% in aluminum. Check the tap maker's recommendation for your tap and material.
Does the D - P rule work for form (roll) taps?
No. Form taps displace metal instead of cutting it and need a larger drill. Use the tap maker's drill chart for form taps; the D - P rule of thumb is for cut taps.
What is the tapping feed rate for 5/16-18?
Feed per revolution equals the pitch, so IPM = RPM / TPI. At 400 RPM that is 400 / 18 = 22.22 IPM. In metric, feed = RPM x pitch; an M8 x 1.25 tap at 500 RPM feeds 625 mm/min.
How deep should a tapped hole be?
Shop rule of thumb, not from a standard: thread engagement beyond about 1.5 x the major diameter adds little strength in most materials. For a calculated length of engagement, use the Machinery's Handbook formulas or the fastener maker's data, and follow the drawing when it calls out a depth.
Last updated