CNC Thread Milling Feed Rate Calculator
A thread mill runs along a circular path, so the feed at the cutting edge is not the feed the control sees at the tool centre. This calculator gives both, and an estimate of how long the thread takes.
Your numbers
Nominal diameter of the thread, for example 20 for M20.
Must be smaller than the thread diameter for an internal thread.
Your results
The centreline correction uses the nominal thread diameter as the contact diameter, which is the common shop approximation. Follow your tool maker's catalogue for exact feed and for the radial passes needed.
Internal centreline feed vs cutter diameter
Sweeps Thread mill cutter diameter from 4 to 16, holding your other inputs fixed.
Link CNC cycle times to ERP routings
Optional: a short review of how to keep routing times in step with real programs.
Optional. The tool and every export work without this. No spam.
How to use it
Enter the thread major diameter, the cutter diameter, spindle speed, number of teeth and the feed per tooth recommended for the material. The first result is the feed at the cutting edge, which is rpm x teeth x fz. The second is the feed to program on the centreline when the cutter moves in a helix with G02 or G03 and cutter radius compensation is not applied to the path. Use the internal value for holes and the external value for threads cut on a boss or shaft.
Why the feed must be corrected
On an internal thread the cutter edge travels a larger circle than the tool centre. If you program the edge feed on the centre path, the cutter ends up with a much higher feed per tooth than intended because the tool centre moves slower for the same angular speed. The correction is vf_centre = vf_edge x (D - d) / D for internal threads. On an external thread the centre path is larger than the edge path, so the factor is (D + d) / D. For a 20 mm thread with a 12 mm cutter the internal centreline feed is only 40 percent of the edge feed.
- Internal: factor below 1, so the programmed feed is lower.
- External: factor above 1, so the programmed feed is higher.
- A control with cutter compensation on the path may need the edge feed instead.
Cycle time and passes
A single helical turn advances the tool by one pitch. The number of turns is the thread length divided by pitch, plus about one extra for the entry. Multiply by the circumference of the centre path to get the cutting length, then divide by the centreline feed for minutes. Hard materials and deep or fine threads often need two or three radial passes at progressively larger radii, so multiply the time accordingly. Add approach, arc lead-in and retract time from your program.
Common mistakes
Programming the edge feed on the centre path is the classic error and leads to broken thread mills. Others are running a cutter whose diameter is too close to the minor diameter, which leaves no clearance for chips, and using full-depth single passes in stainless or titanium. Always check cutter reach and the minimum pre-drilled hole size in the tool catalogue.
Frequently Asked Questions
Should I program the edge feed or the centreline feed?
If you program the tool centre path without cutter compensation, program the corrected centreline feed. If your control applies radius compensation on the path and interprets the feed at the cutter edge, use the edge feed. Check your control manual, because this differs between controls and cycles.
What feed per tooth should I use?
Take it from the thread mill manufacturer's table for your material. Typical values are 0.03 to 0.08 mm per tooth for steels in small thread mills, with lower values for stainless and titanium. This calculator does not guess the value for you.
Does this work for tapered pipe threads?
It gives a good first value, but NPT and similar tapered threads change diameter along the helix, so the correction factor varies. Use the average diameter for a rough estimate and follow the tool maker's cycle for production.
Why is the internal feed so much slower than the edge feed?
Because the tool centre travels a smaller circle than the cutting edge in a bore. The control moves the centre, and the edge speed is the centre speed scaled up by the ratio of the diameters. Without the correction the teeth would take heavy chips.
If you want these feeds and cycle times to flow into your routing and costing in the ERP, we can show you how. The calculator works fully without it.
Related Tools
CNC Spindle Power and Torque Required Calculator
Check whether your machine has enough power and torque for a milling cut before you run it, using specific cutting force kc and drive efficiency.
MES & Shop FloorCNC Drilling Cycle Time Calculator
Calculate spindle speed, feed rate and total time for a drilling job with peck cycles, and see how peck depth affects time.
Discrete ManufacturingCNC Radial Chip Thinning Feed Compensation Calculator
When radial depth is less than half the cutter diameter the chip is thinner than the feed per tooth. Find the feed that restores the chip thickness you want.
Discrete ManufacturingCNC End Mill Deflection Calculator
Predict how far a cutter bends under load, and see why shorter stickout and a larger diameter matter so much for accuracy.
More Discrete Manufacturing tools
See all- Ball End Mill Scallop Height and Stepover Calculator
- CNC Turning Surface Roughness and Feed Calculator
- OEE Calculator (Overall Equipment Effectiveness)
- Scrap Rate Cost Calculator
- Takt Time Calculator
- Cycle Time & Capacity Calculator
- Inventory Carrying Cost Calculator
- Economic Order Quantity (EOQ) Calculator
- MRP Nervousness Assessment