Holemaking and tapping
Tapping calculator
Tapping feed equals pitch per revolution: IPM (inches per minute) = RPM / TPI, or mm/min = RPM x P.
Technical review pending. Formulas and values are cited. This notice comes down after a machinist review.
Tapping feed
IPM
IPM = RPM / TPI = 500 / 20 = 25.0 IPM
Feed per revolution: 0.0500 in (the pitch). Fanuc-style mill G84: F25.0 in feed per minute (G94), F0.0500 in feed per revolution (G95).
Tap drill
(0.2010 in)
drill = D - (0.01299 x %thread / TPI) = 0.25 - (0.01299 x 75 / 20) = 0.2013 in
Nearest drill: #7 (0.2010 in, 5.11 mm), 75% thread. Check: %thread = 76.98 x TPI x (D - drill) = 76.98 x 20 x (0.25 - 0.201) = 75.4%.
Source: Machinery's Handbook (tapping); ASME B1.1; ISO 261; control programming manuals for G84 and G74 (Fanuc-style mill controls).
How it works
A tap advances one pitch per revolution, so the feed is fixed by the thread: the only choice is the spindle speed. IPM (inches per minute) = RPM / TPI. The tap drill comes from the percent of thread you want.
Tapping feed
IPM = RPM / TPI; vf = RPM x P
| Symbol | Meaning | Unit |
|---|---|---|
| IPM | Feed rate, inches per minute | in/min |
| vf | Feed rate, metric | mm/min |
| RPM | Spindle speed | rev/min |
| TPI | Threads per inch; feed per revolution (IPR) = 1 / TPI | 1/in |
| P | Pitch, the number after the x in a metric callout | mm |
Spindle speed from tapping speed
RPM = (SFM x 12) / (pi x D)
| Symbol | Meaning | Unit |
|---|---|---|
| SFM | Surface feet per minute, the tapping speed from the tap maker's data | ft/min |
| D | Tap major diameter | in |
| pi | 3.1416 | none |
Metric: RPM = (Vc x 1000) / (pi x D), with Vc in m/min and D in mm.
Tap drill for a percent of thread
drill = D - (0.01299 x %thread / TPI)
| Symbol | Meaning | Unit |
|---|---|---|
| drill | Drill diameter for the target percent | in |
| D | Basic major diameter | in |
| %thread | Target percent of thread as a whole number (75, not 0.75) | % |
| TPI | Threads per inch | 1/in |
Metric: drill = D - (%thread x P / 76.98). The nearest drill is then checked with %thread = 76.98 x TPI x (D - drill) (inch) or %thread = 76.98 x (D - drill) / P (metric).
Worked example: 1/4-20 at 500 RPM
A 1/4-20 tap, rigid tapping at 500 RPM on a Fanuc-style mill.
- Feed: 500 / 20 = 25.0 IPM.
- Feed per revolution: 1 / 20 = 0.0500 in.
- Tapping block in feed per minute (G94): G84 Z-0.500 R0.100 F25.0. Depth and R plane are examples.
Result: 25.0 IPM. The rigid tapping command that goes before G84 varies by control; check the programming manual.
Worked example: M8 x 1.25 at 600 RPM
An M8 x 1.25 tap at 600 RPM.
- Feed: 600 x 1.25 = 750 mm/min.
- Feed per revolution: 1.25 mm, the pitch.
Result: 750 mm/min.
Worked example: 1/4-20 from tapping speed
A 1/4-20 tap at 20 SFM (an illustrative tap maker value; use your tap maker's number).
- RPM = 20 x 12 / (3.1416 x 0.250) = 240 / 0.7854 = 305.6 RPM; use 306 RPM.
- Feed: 306 / 20 = 15.3 IPM.
Result: 306 RPM, 15.3 IPM.
Worked example: 1/4-20 at 65% thread
A 1/4-20 hole in hard steel, 65% thread target.
- Target drill: 0.250 - 0.01299 x 65 / 20 = 0.250 - 0.0422 = 0.2078 in.
- Nearest drill: #4 (0.2090 in).
- Check: 76.98 x 20 x (0.250 - 0.209) = 76.98 x 20 x 0.041 = 63.1%.
Result: #4 drill, about 63% thread.
Shop notes
- No tapping speed table here: take the SFM for your tap, coating and material from the tap maker's data.
- Rigid tapping needs the feed to equal RPM x pitch. A floating (tension-compression) holder tolerates a small feed mismatch; a solid holder does not.
- Percent of thread by material, forum rule of thumb (not a standard): 60 to 65% in hard steel, about 70% in steel, 75 to 80% in aluminum.
- Form (roll) taps need a larger drill than the cut-tap formula gives. Use the tap maker's chart.
- Rule of thumb: thread engagement past about 1.5 x diameter adds little strength in most materials.
- By hand or on a light drill press, a lower percent of thread cuts tapping torque and tap breakage.
FAQ
What feed for rigid tapping 1/4-20 at 500 RPM?
25.0 IPM (500 / 20). Feed per revolution is the pitch, 0.0500 in.
What feed for M8 x 1.25 at 600 RPM?
750 mm/min (600 x 1.25).
What does G84 do on a Fanuc mill?
G84 is the right-hand tapping cycle on a Fanuc-style mill control; G74 taps left hand. In feed per minute mode (G94) F = RPM x pitch; in feed per revolution mode (G95) F = pitch.
What drill for 1/4-20 at 65% thread?
The formula gives 0.2078 in. The nearest drill is a #4 (0.2090 in), which gives 63% thread.
How deep should threads go?
Rule of thumb: past about 1.5 x diameter of engagement, extra depth adds little strength in most materials. Follow the drawing when it calls out a depth.
Last updated