Why tapping feed is arithmetic rather than judgement
In every other machining operation feed is something you select. In tapping it is not. The tap is cutting a helix of a fixed lead, and it has to travel along that helix at exactly the rate the helix demands: one pitch per revolution. Feed faster and you are pulling the tap through material it has not cut; feed slower and you are compressing it. Either way the thread tears and often the tap breaks.
So the only real decision is spindle speed, and feed follows from it. For an imperial tap the pitch is one divided by the threads per inch, so feed in inches per minute is simply rpm divided by TPI. For a metric tap the pitch is given directly in millimetres, so feed in millimetres per minute is rpm multiplied by the pitch.
That relationship is why a tapping cycle on a CNC is either rigid, with the spindle encoder and the Z axis synchronised so the ratio is held exactly, or done through a tension-compression holder that lets the tap float axially and correct the mismatch itself.
Choosing the surface speed
Tapping runs far slower than drilling the same hole, and for a reason worth understanding: a drill cuts at its periphery with two lips, while a tap is cutting on every flute along several threads of engagement at once, in a hole with nowhere for the chips to go, and then has to reverse back out through the thread it just cut.
As a starting point, cut taps run about 20 to 50 SFM in steel, 60 to 100 in aluminium, and toward the low end of those ranges in stainless and the high-temperature alloys. Form taps, which displace metal rather than cutting it, run considerably faster — often double — because there are no chips to clear at all, though they need a larger pre-drill and only suit ductile materials.
The other constraint is the machine. Above roughly 3000 rpm most spindles cannot decelerate, reverse and accelerate cleanly enough to hold synchronisation at the bottom of the hole. Small taps hit that ceiling quickly — an M3 at 40 SFM already wants over 1200 rpm.
Worked example: 1/4-20 in mild steel
A 1/4-20 cut tap, mild steel, 40 SFM, half an inch deep in a through hole.
- Spindle speed. rpm = 40 × 12 ÷ (π × 0.250) = 480 ÷ 0.7854 = 611 rpm.
- Pitch. 20 threads per inch means 1 ÷ 20 = 0.050 inch per thread.
- Feed rate. 611 × 0.050 = 30.6 in/min, which is 776 mm/min.
- Time in the hole. 0.5 ÷ 30.6 = 0.98 seconds in, and the same coming back out, so about two seconds per hole excluding rapids.
The metric equivalent is instructive. An M6×1.0 tap is 0.2362 inch in diameter, so at the same 40 SFM it turns 647 rpm — faster, because it is smaller — and its feed is 647 × 1.0 = 647 mm/min. Same surface speed, different numbers, because both rpm and feed track the diameter and the pitch.
Thread engagement is where taps actually break
The pre-drill size decides how much material the tap has to remove, expressed as a percentage of the full thread form. It is the single biggest influence on tapping torque, and the place most tap breakage originates.
Going from 65% to 75% engagement raises torque substantially. Going to 100% roughly doubles it against 75%, and buys almost nothing: a 75% thread carries the great majority of the strength of a full one, because the failure mode in a properly designed joint is the bolt stretching rather than the thread stripping. Most shops tap 65% to 75%, and in tough materials or deep holes the lower end is normal practice.
Depth matters the same way. Torque rises with the number of threads engaged, so a hole tapped two diameters deep is far harder on the tap than one tapped one diameter deep, for no practical gain in joint strength. Threading deeper than about one and a half diameters is usually wasted effort.
Starting surface speeds for cut taps
| Material | Surface speed (SFM) | 1/4-20 rpm | 1/4-20 feed (in/min) |
|---|---|---|---|
| Aluminium alloys | 60–100 | 917–1528 | 46–76 |
| Brass and bronze | 50–80 | 764–1222 | 38–61 |
| Grey cast iron | 40–60 | 611–917 | 31–46 |
| Mild steel | 30–50 | 458–764 | 23–38 |
| Alloy steel | 20–35 | 306–535 | 15–27 |
| Austenitic stainless | 15–30 | 229–458 | 11–23 |
Form taps in ductile materials run roughly double these speeds, because they displace material rather than cutting chips.
Match the tap style to the hole, not just the material
A spiral point (gun) tap pushes chips forward, which is ideal in a through hole and wrong in a blind one, where the chips pile up at the bottom and jam the tap. A spiral flute tap pulls chips back out of the hole, which is what a blind hole needs. A form tap makes no chips at all, so it suits either, but only in ductile materials and with a noticeably larger pre-drill.
Why taps break
- Feed and speed out of sync. If the ratio is not exactly one pitch per revolution, the tap is being pushed or pulled against the thread. This is the failure rigid tapping exists to prevent.
- Too much thread engagement. Tapping 100% instead of 75% roughly doubles the torque for almost no gain in strength.
- Chips in a blind hole. A spiral point tap in a blind hole packs the bottom with chips and then tries to bottom out into them.
- Tapping too deep. Torque scales with engaged length. Past about one and a half diameters you are adding risk without adding strength.
- The wrong pre-drill. A drill running oversize is forgiving; one running undersize raises engagement above what you calculated and is the quiet cause of a lot of broken taps.
Before and after the tap
The tapping operation starts with the hole, and the hole size is what sets the engagement percentage this page warns about. Work it out with the tap drill size calculator rather than from a chart, because the chart usually assumes 75% and the right answer for tough material is often lower. Drilling that hole has its own speeds and feeds — the drilling calculator covers it, and note how much faster the drill runs than the tap that follows it.
If the tap is large, the hole is deep, or the material is difficult, thread milling is worth considering instead: a single-point thread mill removes far less material per pass, cannot break in the hole in the same catastrophic way, and cuts any pitch of the same form. The trade is cycle time. For torque on the finished fastener rather than on the tap, see the bolt torque calculator.
Terms used here
- Pitch
- The distance a thread advances per turn. Quoted directly in millimetres on metric taps, and as its reciprocal — threads per inch — on imperial ones.
- Rigid tapping
- A cycle where the control synchronises spindle rotation with Z-axis feed so the pitch is held exactly, with no floating holder.
- Thread engagement
- The percentage of the full thread form actually cut, set by the pre-drill diameter. The dominant influence on tapping torque.
- Form tap
- A fluteless tap that displaces metal into the thread shape rather than cutting it. No chips, higher speeds, larger pre-drill, ductile materials only.