Other Language:


Subscribe to our mailing list

* indicates required


Zinc alloys are readily tapped and form excellent quality threads. Cutting fluids are strongly recommended, especially where local metal removal rates are large and tool workpiece sliding contact involves large areas.

Cutting Tap Design

Spiral point taps are preferred for through holes. For blind holes, the standard tap geometry or special aluminum geometry (high hook and clearance angles) are recommended.

Surface Speeds

Tapping surface speeds to 60 m/min can be employed, with generous applications of emulsified cutting oils. In general, speeds should be reduced as the pitch of the thread decreases.

Form Tapping

Form tapping can be performed on the zinc alloys over a wide range of conditions. Form taps are fluteless and much stronger than fluted cutting taps, making them especially useful for small diameter holes where tap breakage is a potential problem. Form tapping also eliminates congestion of the small flutes. Form taps are more expensive, give poorer thread shape and require more accurate hole diameters than cut thread taps but they do have the considerable advantage of producing no swarf and the strength of the thread produced is equal if not better than a cut thread, (except in respect of torque relaxation). The recommended tapping speeds for form tapping are the same as for cut threads. Cutting fluids are especially important because the process generates high frictional forces. Water based emulsifiable oils or light mineral oils are suitable.

In most cases tapping is performed on cored holes in the diecasting without any drilling operation.

Recommended Hole Sizes Prior to Threading

Nominal Thread
Diameter mm
For Cut Threads For Rolled Threads
and Taptite Screws
Parallel Taper Parallel Taper
3 2.525 2.567-2.500 2.745 2.779-2.711
4 3.350 3.424-3.300 3.643 3.691-3.595
5 4.250 4.327-4.200 4.592 4.646-4.538
6 5.050 5.136-5.000 5.490 5.558-5.422
8 6.850 6.930-6.760 7.363 7.450-7.276
10 8.550 8.710-8.510 9.236 9.340-9.132
12 10.250 10.500-10.260 11.108 11.230-10.987
14 12.050 12.280-12.010 12.981 13.120-12.842
16 14.050 14.280-14.010 14.981 15.120-14.842
20 17.550 17.850-17.520 18.726 18.900-18.553
24 21.050 21.425-21.020 22.471 22.680-22.263

Core diameter for form tapping

= basic tap diameter – (0.772 x Thread Pitch x % thread required)

External Threading

In general, type “S” chasers having a curved rake face and a throat angle of 33° should be used. The back rake should be 25° with a 4° negative side rake and 12° clearance. The work zone should be well lubricated and a slow feed rate employed.