Cut Taps vs. Form Taps: Drill Sizes, Materials, Pros and Cons

Quick answer: A cutting tap removes metal and makes chips. A forming tap (also called a roll tap or fluteless tap) pushes metal aside to form the thread and makes no chips. Because the displaced metal has to flow into the thread crests, form taps need a larger drill than cut taps. For a 1/4-20, that’s a #1 (0.228 in) instead of a #7 (0.201 in). Form taps work in ductile metals such as aluminum, copper, brass, mild steel, and many stainless steels. They don’t suit brittle materials like gray cast iron.

How each tap makes a thread

A cutting tap has flutes and sharp cutting edges on its chamfer. Each tooth shaves a little metal from the hole wall, and the chips curl into the flutes or get pushed ahead of the tap. The drilled hole becomes the thread’s minor diameter.

A forming tap has no cutting edges. Its threads have lobes that press into the hole wall, and the metal flows up into the gaps between the tap’s threads. Nothing is removed. The hole actually gets smaller as the thread forms, because displaced metal rises toward the center to make the crests.

That one difference drives everything else: drill size, materials, torque, and the finished thread’s look.

Why form taps need a bigger hole

With a cut tap, a smaller hole just means more metal to cut. With a form tap, a smaller hole means more metal that has to go somewhere. Too much, and torque climbs until the tap breaks or the thread overfills.

The two formulas we use:

• Cut tap: drill = major diameter − 0.01299 × % thread × pitch
• Form tap: drill = major diameter − 0.0068 × % thread × pitch

Our form tap drill chart targets 65% thread with the second formula, the figure Komet recommends for rolled threads (it suggests 60–65%). For a 1/4-20 that gives 0.250 − 0.0068 × 65 × 0.05 = 0.2279 in, and the nearest drill is a #1 at 0.228 in.

Cut vs. form drill sizes, side by side

Check the tap maker’s chart

Treat the form tap column as a starting point. Each maker uses its own formula. OSG, for example, factors in the tap’s pitch-diameter limit and target thread percentage, and tells users to go slightly larger than the calculated value in less ductile or harder material, then adjust after checking the thread. Komet notes the usable hole range for a form tap is very narrow. For a 1/2-13 it gives 0.466–0.469 in, which is why production shops sometimes buy special-size drills. Our 15/32” (0.4688 in) choice lands inside that window.

Which materials suit form tapping

Form tapping needs metal that will flow without cracking. Emuge’s guidance:

• Tensile strength up to about 1,200 N/mm² (roughly 174,000 psi).
• Hardness below about 35–40 HRC.
• Simple test: if the material makes a continuous chip when you drill it, it’s probably a good candidate.

Emuge’s list of suitable materials includes wrought and cast aluminum, copper, brass, stainless steels, carbon steels, and zinc die-casting alloys. OSG’s form tap tables cover steels under 35 HRC, mild and free-cutting steel, stainless, aluminum and its alloys, zinc alloys, copper, and brass.

Poor candidates:

• Gray cast iron and other brittle, short-chipping materials, which crumble instead of flowing.
• High-silicon cast aluminum. Sandvik’s Jim Nielsen says form taps are a good choice below about 10–12% silicon, because higher-silicon castings get brittle and can fracture.
• Hardened steel above the 35–40 HRC range.
• Thin walls. Forming pushes outward. Thin bosses can bulge or crack.

Pros and cons

Form tap advantages

• No chips. Nothing to pack into a blind hole, which makes form taps popular for blind holes.
• Stronger threads. Emuge and OSG both say formed threads are generally stronger because the metal is cold worked along the thread profile.
• Tough tool. No flutes means a solid core. OSG describes form taps as highly resistant to breakage.
• Accurate size. OSG reports form taps oversize the thread much less than cutting taps.
• Speed. OSG says form taps can often run at about double the standard speed in suitable materials.
• Smooth, burnished flanks.

Form tap drawbacks

• More torque. OSG measured form tap torque at up to about twice that of a cutting tap. A machine near its limit with a cut tap may stall with a form tap.
• Exact hole size matters. Too small overloads the tap; too large leaves a weak thread.
• Lubrication is mandatory. Emuge, OSG, and Tapmatic all stress good lubrication. OSG recommends high-lubricity oils with sulfur or chlorine additives.
• Split crest. The formed crest has a small seam at the minor diameter, and Tapmatic notes the minor diameter looks rough. OSG says this is cosmetic, but if it matters for your part, use a cutting tap.
• Burrs at the entrance. Metal rises at the hole edge. OSG recommends chamfering the hole with a 60–70° countersink.
• Limited materials, as listed above.

Cutting tap advantages

• Works in almost any machinable material, including cast iron and brittle alloys.
• Uses the standard chart drill.
• Lower torque, so it’s easier by hand and in light machines.
• Cheap and available everywhere.

Cutting tap drawbacks

• Chips have to go somewhere, which is the main cause of broken taps in blind holes. See broken tap removal if it’s already too late.
• More sensitive to dull edges and the wrong flute style.

Which should you use?

If you do switch to form taps, change the drill. Using a cut-tap drill with a form tap is one of the most common ways to snap one. Our thread pages list both drills, and the form tap drill chart covers every size in one place. For more on how thread height affects strength, see percent of thread.

Sources: Emuge-Franken, “Cold-Forming Taps” (emuge-franken.se); OSG Tap Technical Guide Vol. 1, Part 9 and Tables 8 and 26; Tapmatic, “Tap Recommendations for Specific Materials”; Cullen Morrison (Komet), Canadian Metalworking, 2014; Jim Lorincz, “Gummy, Stringy Material Meets its Match,” SME Manufacturing Engineering, 2022.