Threading technology choice
How to use the calculator
Specify diameter, pitch (or TPI for inch), profile percentage, ISO material, hole type (through or blind), thread standard, and length. Additionally, set the conditions: overhang, presence of chamfer, machine type, batch size and priority. The calculator will determine the optimal technology (tap/former/thread mill), calculate the diameter of the pre-drill, estimate the torque and chip control, show the clamping strategy and risk focus.
Why technology choice is critical
Threading is one of the last operations on a part. A broken tap in a blind hole on a nearly finished part isn't just a lost tool, it's a lost part and hours of downtime. The correct choice of technology (cutting tap, rolling machine or thread mill) determines not only the quality of the thread, but also the likelihood of an accident.
There is no universal "best" method: a tap is fast and cheap, but fragile in blind holes and on heat-resistant materials. The rolling machine does not produce chips, but requires a plastic material and a high torque. A thread mill is the safest of all (if it breaks, it does not get stuck in the hole), but it is slower and more expensive. The calculator weighs all factors and makes an informed recommendation.
What influences the choice
Workpiece material. Steel (P) and aluminum (N) - the area of taps and rolling tools. Stainless steel (M) is prone to work hardening and sticking - the tap works, but requires sharp geometry and stable coolant. Heat-resistant (S) and hardened (H) - almost always thread milling cutters: the torque and heat are too high for the tap. Cast iron (K) is a tap, but a rolling tool is not suitable (the brittle material does not form).
Hole type. Through - spiral point (gun) tap: chips go down, minimal risk. Deaf - spiral flute: chips go up along the grooves. With a depth > 3D in a blind hole, the risk of chip clogging increases sharply - the calculator recommends a thread mill.
Pre-drill diameter. Calculated using the formula: Ø = D − K × P × (% profile / 100), where K ≈ 1.227 for 60° profile (ISO). For the rolling machine, the hole is made larger (by 15–30% of the pitch), because the metal is not cut off, but displaced. Error in pre-drilling is the main cause of tap failure.
Profile percentage. Standard - 75%, but for difficult conditions (heat-resistant, blind, long reach) a reduction to 60-65% reduces the moment by 25-35% and sharply reduces the risk of failure. Thread strength at 60% is still sufficient for most applications.
Machine and clamp. CNC with rigid tapping - optimal for tappers: the spindle is precisely synchronized with the feed. Without rigid tapping, a floating cartridge (compensator) is needed, otherwise the tap breaks due to axial misalignment. The thread mill works on any machine with interpolation.
Entry chamfer. The absence of a chamfer increases the impact load on the first turn of the tap and the risk of chipping. A chamfer of 0.5–1.0P is a must, especially for blind holes and hard materials.
Frequently Asked Questions
When is a rolling tool better than a tap? On plastic materials (aluminum, mild steel) with through or shallow blind holes. The rolling machine does not produce shavings (there is nothing to clog the hole), forms a stronger thread (the fibers are not cut) and lasts longer. Disadvantages: higher torque, requires good lubrication, does not work on brittle materials (cast iron, hardened steel).
In what cases is a thread mill the only option? For hardened steels (H) > 45 HRC, heat-resistant (S), blind holes with depth > 3D, for single production (one tool for all diameters of one pitch), and when tap breakage is critical (expensive part at the last operation).
How to calculate the pre-drill diameter for M12×1.75 with 75% profile?Ø = 12 − 1.227 × 1.75 × 0.75 = 12 − 1.610 = 10.39 mm. Standard drill Ø 10.4 mm. The calculator calculates this automatically. For a rolling machine, 0.25–0.30 × P (≈ 0.44–0.53 mm) is added to this value, that is, Ø ≈ 10.8–10.9 mm.
Why does the tap break in blind holes? Three reasons: 1) Chips clog the grooves - the torque increases sharply. 2) The tap rests on the bottom - there is not a sufficient reserve of drilling depth. 3) There is no chamfer at the entrance - the first turn is overloaded. Solution: spiral flute (chips up), drill margin ≥ 2P, chamfer, profile reduction to 60–65% and stable coolant.
What is rigid tapping and why is it needed? Rigid tapping - synchronization of spindle rotation with axial feed. The spindle rotates exactly 1 thread pitch per 1 revolution. Without this (on machines without rigid), the axial feed “floats” and the tap experiences additional loads. On such machines, a floating holder is required, which compensates for misalignment.
Do you need help selecting a tap, rolling tool or thread cutter? Contact our specialists - we will select a tool, pre-drilling and modes for your material and machine.