Turn Threads with a Single-Point Tool

Difficulty: 2 Moderate
Time required: 15 minutes to 1 hour
Tools needed:
 - CNC Prototrak lathe
 - Threading tool, internal or external, sized appropriately for your objective


Use the CNC lathe to turn any thread configuration, including fine, coarse, metric, multi-start, and tapered.

This guide is provisional

It should be used as a general note by experienced lathe operators, in conjunction with the manual. Please ask a lathe mentor or staff if it’s the first time you need to turn threads.

This guide is written for external threads.

Step 1 Set Up Tool Table

  • Threading is a CNC operation, and works best if you have set up at least the right-hand turn/face tool, threading tool, and cutoff tool in the tool table.
  • Ask a Lathe Mentor or Staff to help the first time you are setting up a tool table. It’s very easy to get wrong, which leads to damaged parts or machine crashes.
  • Load Tool #1 in the machine and in the DRO. Destructively set the DRO by facing and turning and measuring a piece of stock.
  • Press Setup | Set Tool | New and set tool 6 and 7 using the air gap method, following the onscreen diagrams. X readouts are on the diameter, so double the size of your dowel rod.

Step 2 Turn a Boss to Receive the Thread

  • Part diameter should be equal to the major diameter of the thread. Typically this is smaller than the nominal diameter.
  • Major diameter tolerance bands can be found from charts such as https://www.engineersedge.com/screw_thre…
  • Thread relief is optional with the CNC lathe, but should be provided if you want the nut to thread all the way to the end.
  • The thread tool path must stop .070″ away from any shoulder on the part. This is based on the width of our threading insert.
  • Check clearances carefully if approaching the left side of a shoulder – our threading tool is optimized for right hand approach and needs much more clearance for left hand approach.

Step 3 Program Threading Operation

  • For semi-manual operation, you can use a single-step program to cut a thread.
  • X Begin and X End should be the nominal diameter of the thread.
  • Z Begin is the more positive end of the thread (for right hand threads)
  • Z End is the more negative end of the thread. At least .070″ away from shoulders.
  • Pitch is the thread pitch in inches or mm. Inch threads are typically specified in threads per inch, which is the reciprocal of pitch
  • Pass Depth .020″ for big threads in soft materials; .010″ for small threads or hard materials
  • Spring passes: 0 or 1 is usually enough. These are extra cuts at the full depth to remove material left behind by part deflection.
  • Plunge angle – accept the default 29.5
  • Side – select inside or outside. This guide is written for outside threads. We have a thread boring bar, but question every setting when using it.
  • # of starts: typically 1
  • RPM: 200 – 700 usually works well. The machine has to coordinate spindle and carriage movement, so it can’t necessarily go full speed.
  • Tool # – the threading tool in the tool table, usually 7

Step 5 Preview

  • View the toolpath using Setup | Tool Path
  • Look for where the threading operation is relative to the origin
  • Note where the home position is relative to the origin and cutting. Make sure the lathe will not attempt to jog into the headstock or tailstock.
  • Setup | Verify
  • Look for a plausible simulation

Step 6 Cautiously Do the First Cut

  • Mode | Run | Start
  • Read, understand, and follow each line of instruction in a Green Box. Do not click through mindlessly.
  • Press Go – machine will move to home position for tool change
  • Install tool 7, threading tool, if not already installed
  • Start Spindle
  • Press Tracking
  • Turn handwheels to approach part
  • Stop and check Distance-to-Go
  • When the machine reaches the threading position, it will take over under CNC control to coordinate threading movements
  • At the end of the thread. press GO twice to continue in CNC run

Step 8 Test Fit, Adjust

  • Use a nut to test the thread fit. If you don’t have a nut, you would need thread gages and thread wires.
  • Do Not Unchuck the part. If you do, you’ll lose registration and no further adjustments will be possible, except perhaps using the ‘thread repair’ routine
  • If the fit is tight – decrease X begin and X end in small increments (.005 or so) and repeat the cut until the fit is good
  • If you need to make multiple parts, you have now now found the best X Begin and X End to use for your thread.

Step 9 Advanced: qualifying thread tool for multiple sizes

  • If you want to set up multiple thread sizes without trial and error for each size, it is possible by precision qualifying the thread tool. It’s usually not worth it.
  • After setting the thread tool in the tool table, set up a threading program that will cut deep enough to leave sharp points at the major diameter. There should be no flats on the outside of the thread form. Measure this OD with calipers / micrometer.
  • Take (XBegin - Measured diameter) / 2 + X Modifier (if any) and enter this as X Modifier for the thread tool in the tool table.
  • Repeat this procedure until the measured diameter is equal to XBegin

Related Articles


This site uses Akismet to reduce spam. Learn how your comment data is processed.