CNC / machinist calculator
Thread Milling Feed Compensation Calculator
A thread mill orbits the hole, so the feed the cutting edge sees is not the feed the control commands at the tool center. Program the edge feed straight and an internal thread comes out coarse and an external one fine. Enter the cutting-edge feed, the thread major diameter and the cutter diameter, and this calculator gives the adjusted center feed to put in the program for an internal or external thread.
How it works
When a thread mill interpolates around a circle, the center of the tool travels a smaller circle than the cutting edge for an internal thread, and a larger circle for an external thread. Feed is set at the tool center by the control, but the chip load happens at the edge, so the two differ by the ratio of their radii.
For an internal thread the programmed center feed is the edge feed times the thread major diameter minus the cutter diameter, divided by the major diameter. For an external thread it is the edge feed times the major plus the cutter, divided by the major. The cutting-edge feed itself is the usual feed per tooth times the number of teeth times the spindle RPM, which you can get from the feeds and speeds tools.
The effect is large. A small cutter in a small hole can need an internal feed only a quarter of the edge feed, while the same setup externally needs well over the edge feed. Skipping this adjustment is a common reason thread mills produce the wrong surface finish or chip load.
Worked example
A 0.370 in cutter milling a 9/16-18 internal thread (major 0.562) at an 8.3 in/min edge feed: 8.3 x (0.562 - 0.370) / 0.562 = 2.8 in/min programmed. Externally the same setup needs about 13.8 in/min.
Frequently asked questions
Why does thread milling need a feed adjustment?
Because the tool orbits the hole, the cutting edge and the tool center travel different size circles. The control sets feed at the center, but the chip load is at the edge, so the programmed feed must be scaled by the radius ratio.
How do I calculate the internal thread milling feed?
Multiply the cutting-edge feed by the thread major diameter minus the cutter diameter, then divide by the major diameter. The center moves slower than the edge inside a hole, so the programmed feed is less than the edge feed.
Is the external adjustment different?
Yes. For an external thread the center travels a larger circle than the edge, so the programmed feed is the edge feed times the major plus the cutter, divided by the major. The programmed feed comes out larger than the edge feed.
How do I get the cutting-edge feed to start with?
It is the standard milling feed: feed per tooth times the number of teeth times the spindle RPM. Use the feeds and speeds or chip load tools to set a sound chip load and RPM for the material, then adjust it here for the orbit.
Does the helix or pitch change the feed much?
The axial helix adds a tiny correction, far less than one percent for normal pitches, so mainstream practice and this calculator ignore it. The dominant adjustment is the planar orbit radius captured by the formula above.
Related calculators
Sources
- Harvey Performance - thread milling speeds and feeds (worked example)
- Modern Machine Shop - get the feed rate right when thread milling
Every formula on this page is shown and sourced. See how we verify.
These calculators are for planning and as a starting point. Recommended speeds and feeds are published starting values that vary with your specific tool, coating, machine rigidity, workholding and coolant. Always start conservative, listen to the cut, and follow your tool maker data sheet.