© Tailmaker!! All rights reserved.


  • Max. thread length ~25-30mm (1-1.25") depending on threading bit shank length
  • Triangular threads can be made with diameter of threading bit plus 2* cutting depth. ACME threads typically with diameter > 5*threading bit.
  • Recommended gap/clearance between bolt and nut for accurate CNC machines is 0.25mm/0.01". This will allow for smooth operation given the fuzzy wood surface. Less accurate machines may need more clearance.
  • Make sure to enter or check EVERY yellow cell in the spreadsheet. 
  • Make sure to use EVERY green cell in the spread sheet in VcarvePro or Aspire. Changes in each yellow cell may affect all green cells
  • Use multi-start threads to get faster screw travel
  • Optional: add a guiding stub to the tip of the screw to get the screw centered in the mating part. Otherwise it may get fumbly to align and find the thread start


  • Before the thread is cut, pre-shape the bolt outer and nut inner surface with an end mill. The diameter of the vector for that is the bolt diameter with offset as calculated in the spreadsheet. The cutting depth should be same as the depth for the respective threading path.
  • Make sure the blank is secured including the parts that are cut loose
  • Remove the excess material before cutting the thread
  • Zero the tip of the threading bit on the surface of the blank
  • Use a sacrificial piece of spoil board, because the bit will penetrate by the width of one thread.
  • Suggestion: run the pre-shape and the threading tool path twice to remove fuzz from the surfaces
  • Sand off any burrs.

Create triangular threads (with threading bit e.g. Magnate #796) or ACME style threads (with keyhole bit e.g. Rockler #92035) and Vectric VcarvePro or Aspire, no gadget required.


  • Enter all required values into the spreadsheet, then transfer all output values to VcarvePro or Aspire
  • The spreadsheet tab for triangular threads accommodates a method with fluting tool path and spiral profile tool path. The latter requires manual g-code editing to move the bit away from the thread and avoid cutting a groove when retracting upward. The fluting tool path (recommended method) does not need that.
  • For fluting tool paths short "dog legs" (length equal thread cutting depth) must be added to the beginning and end of the thread arc to clear the thread when retracting. The spreadsheet adds this length to the total arc length to cacluate the proper flute depth. It is the reason why the flute cutting depth is slightly different for the male and female thread with the same pitch. Please transfer these values accordingly.
  • Drawing the thread arcs is easy in Aspire/VcarvePro when they are less than 360 degrees (draw a circle and cut out the required angle). It becomes more interesting to make an arc vector larger than 360 degrees. But even that is easy, example here an arc of 937 degrees: Divide 937 by 3 (or whatever is needed to get the result under 360) and draw the resulting arc of 312.333 degrees. Then use the circular copy function to make 3 of them also spaced 312.333 degrees apart, making the total angle 937 degrees again. Then join them together (Aspire does not care that it has several loops in one vector on top of each other). Identify the start point and the end point in Node Editing mode and add the above mentioned "dog legs".
  • Depending on which vector end is the start point it will become a left or right hand thread.
  • For multi-start threads, this complete vector can also be circular copied as many times a needed (180 degrees for 2-start, 90 degrees for 4-start etc.). 

Threads with Aspire