BIZOMAT MAKEOS · Manufacturing
Thread Milling Tool Path and Feed
What tool-centre path and programmed feed does this helical thread milling operation need?
Tool-centre path diameter, programmed centre-line feed for the required feed at the cutting edge, helical path length per revolution and cycle time for internal or external thread milling.
Open the calculatorRuns in your browser. No account needed.
How this tool works
Inputs, units and where to find them
| Input | Unit | Typical source |
|---|---|---|
| Thread | choice | Internal or external thread. |
| Thread major diameter (internal) or major diameter (external) | mm | Major diameter of the thread (the cutting edge reaches this diameter for internal threads). |
| Pitch | mm | Thread pitch. |
| Cutter diameter | mm | Thread mill cutting diameter. |
| Spindle speed | rpm | Spindle speed. |
| Feed per tooth at the cutting edge | mm | Feed per tooth wanted at the cutting edge (from the tool maker). |
| Cutter flutes | flutes | Number of flutes. |
| Thread length | mm | Length of thread to mill (single-form cutters). |
| Radial passes | passes | Number of radial passes. |
What each input means
Open an input to see what it is, its units, the worked example and the common mistakes, with a small diagram.
What this means: Thread
- What it is
- Whether the thread is cut inside a hole (internal) or on the outside of a stud or shaft (external). It decides whether the tool path is smaller or larger than the thread.
- Units and format
- Choose one of 2 options from the list: Internal; External.
- Example
- The form opens with “Internal” selected as a worked example. Choose the option that matches your case.
What this means: Thread major diameter (internal) or major diame…
- What it is
- The major (largest) diameter of the thread, which the cutting edge reaches on an internal thread and starts from on an external thread.
- Units and format
- Enter a number in mm: millimetres. The form accepts 0.000001 mm to 10000 mm. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 20 mm as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Get it right
- Use the major diameter, not the tap drill or pitch diameter.
What this means: Pitch
- What it is
- The axial distance from one thread crest to the next, which the tool advances along its helical path for each orbit.
- Units and format
- Enter a number in mm: millimetres. The form accepts 0.000001 mm to 50 mm. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 2.5 mm as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Effect on the result
- For a given thread length, a finer pitch needs more orbits and more time.
- Get it right
- For threads given in threads per inch, pitch = 25.4 ÷ TPI.
What this means: Cutter diameter
- What it is
- The cutting diameter of the thread mill across its teeth, from the tool marking or catalogue.
- Units and format
- Enter a number in mm: millimetres. The form accepts 0.000001 mm to 1000 mm. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 14 mm as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Get it right
- Use the cutting diameter, not the shank diameter.
What this means: Spindle speed
- What it is
- The rotational speed of the thread mill spindle, chosen from the cutting speed recommended by the tool maker.
- Units and format
- Enter a number in rpm: revolutions per minute. The form accepts 0.000001 rpm to 1000000 rpm. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 3000 rpm as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Effect on the result
- Edge and centre feeds rise in direct proportion; milling time falls in proportion.
What this means: Feed per tooth at the cutting edge
- What it is
- The feed each cutting tooth should take at the actual cutting edge, as recommended by the tool maker. The tool converts it to the feed at the tool centre that is programmed.
- Units and format
- Enter a number in mm: millimetres. The form accepts 0.000001 mm to 5 mm. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 0.08 mm as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Effect on the result
- Edge and centre feeds rise in direct proportion.
- Get it right
- This is per tooth at the edge, not the programmed centre feed; the control needs the centre feed.
What this means: Cutter flutes
- What it is
- The number of cutting flutes (teeth) around the thread mill.
- Units and format
- Enter a number in flutes: flutes. The form accepts 1 flutes to 50 flutes. Use a whole number. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 3 flutes as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Effect on the result
- Feeds rise in direct proportion to the number of flutes.
What this means: Thread length
- What it is
- The length of thread to be cut along its axis. With a single-form cutter the tool orbits once for each pitch over this length.
- Units and format
- Enter a number in mm: millimetres. The form accepts 0.000001 mm to 10000 mm. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 25 mm as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Effect on the result
- Milling time rises in direct proportion to thread length.
- Get it right
- For multi-form cutters that cut the full length in one orbit, this tool’s time will be too long.
What this means: Radial passes
- What it is
- How many radial passes the thread is cut in, each repeating the full helical path at a larger depth.
- Units and format
- Enter a number in passes: passes. The form accepts 1 passes to 20 passes. Use a whole number. Required: the tool does not calculate until every input is valid.
- Example
- The form opens with 1 passes as a worked example. It is an illustration, not a recommended value: replace it with your own figure.
- Effect on the result
- Milling time rises in direct proportion to the number of passes.
Method and formulas
- Path diameter = D − dc (internal) or D + dc (external).
- Edge feed = rpm × z × fz; centre feed = edge feed × (D − dc)/D internal or (D + dc)/D external.
- Revolutions = thread length ÷ pitch per pass; time = revolutions × π × path diameter ÷ centre feed (plus entry and exit).
- Example: M20 × 2.5 internal with a 14 mm cutter: program 216 mm/min on a 6 mm path.
Limitations
- Single-form (one-tooth-row) thread mill; multi-form tools cut the whole length in one revolution.
- Arc entry and exit moves are not included in the time.
- Example values are illustrations. Replace them with values for your actual task.
Typical uses
- Program thread milling without a CAM system
- Correct feed for the cutter path
- Estimate thread milling cycle time
Who it is for
- Machinists
- CNC programmers
- Manufacturing engineers
What you get
- Tool-centre path diameter
- Feed at the cutting edge and programmed centre feed
- Helical revolutions and cycle time
Interpreting the result
- Many controls apply the centre-feed correction automatically when cutter compensation is used; check your control’s behaviour.
References
- Machinery’s Handbook, 29th edition (Industrial Press, 2012), printed pp. 2063–2070, 1292–1300. Topic reference; no source tables or recommended settings are reproduced.
BIZOMAT tools are screening and decision-support utilities. Verify important financial, engineering, safety, legal or operational decisions using appropriate professional standards and your organisation’s approved data.