How to use this calculator
- Pick the thread type. Choose internal or external — it sets whether the centre runs inside or outside the contour.
- Enter the diameters. Enter the thread major diameter and the thread-mill diameter.
- Enter the cutting-edge feed. Enter the desired feed at the cutting edge from your tooling chart.
- Read the tool-centre feed. Read the compensated tool-centre feed to program, plus the radius-ratio factor.
How it works
A thread mill cuts a thread by helical (circular) interpolation: the
tool orbits the thread axis while feeding one pitch per revolution. The CNC commands
a feed at the tool centre, but the feed your tooling chart specifies is at the
cutting edge — on the thread contour. Those two paths are circles of different
radius, so the same edge feed needs a different centre feed:
Vfcenter = Vfedge × (D ∓ d) / D
For an internal thread the centre orbits inside the contour, so
it travels a smaller circle and the centre feed is reduced:
Vf_center = Vf_edge × (D − d) / D. For an external thread the
centre orbits outside, a larger circle, so the centre feed is increased:
Vf_center = Vf_edge × (D + d) / D. D is the thread major diameter and d the
thread-mill diameter.
The compensation factor is simply the radius ratio of the centre path to the contour. Skipping it is the single most-missed thread-milling setting: program the edge feed straight into the centre move on an internal thread and the part cuts too fast at the edge — because the centre runs slower than the edge, the real edge feed ends up higher than you intended, overloading each tooth.
Worked example
Verified against the live calculator
An M20 internal thread cut with a 12 mm thread mill, charted at 300 mm/min at the edge:
factor = (20 − 12) / 20 = 0.4, so the feed to program at the tool centre is
300 × 0.4 = 120 mm/min. The same tool on an external M20
thread gives factor = (20 + 12) / 20 = 1.6 → 300 × 1.6 = 480 mm/min.
Those are the numbers the calculator returns for these inputs.
Frequently asked questions
Why is the tool-centre feed different from the cutting-edge feed in thread milling?
A thread mill cuts the thread by helical (circular) interpolation, so the tool centre orbits on a different radius than the cutting edge. The CNC programs a feed at the tool centre, but the feed you actually want is at the cutting edge (the thread contour). Because the two circles have different radii, the centre feed must be scaled by the radius ratio.
How do I compensate thread-mill feed for an internal thread?
Multiply the cutting-edge feed by (D − d) / D, where D is the thread major diameter and d is the thread-mill diameter. The tool centre orbits a smaller circle than the edge, so the centre feed is lower. Example: D = 20 mm, d = 12 mm, edge feed 300 mm/min → factor 0.4 → program 120 mm/min.
How do I compensate thread-mill feed for an external thread?
Multiply the cutting-edge feed by (D + d) / D. The tool centre orbits a larger circle than the edge, so the centre feed is higher. Example: D = 20 mm, d = 12 mm, edge feed 300 mm/min → factor 1.6 → program 480 mm/min.
What happens if I ignore the compensation?
If you program the cutting-edge feed straight into the centre move, an internal thread cuts too fast at the edge — the tool centre runs slower than the edge, so the real edge feed is higher than intended. That overloads each tooth, hurts finish and shortens tool life. It is the single most-missed thread-milling setting.
Which diameter do I enter — major or pitch?
Use the nominal (major) thread diameter for D. It is the diameter the manufacturers quote and is what most CAM systems base the interpolation circle on. Enter the thread mill cutting diameter for d.
Does it work in metric and imperial?
Yes — enter diameters in mm or inches and feeds in mm/min or in/min. Toggle SI/Imperial in the header; the compensation factor is dimensionless and unchanged.
Method & assumptions
- Compensation is a pure geometric radius ratio between the tool-centre path and the thread contour — it assumes the CAM/control programs the move at the tool centre (the usual case).
- Vfedge is the feed you want on the contour (the value from your tooling maker's chart); the result is the feed to enter in the program.
- For an internal thread the cutter must be smaller than the bore — a cutter at or above the thread diameter cannot fit, so the result is undefined.
- It compensates feed only; the helical interpolation radius, lead per pass and climb/conventional direction are set up separately.