Key Knowledge of Thread Processing: How a Thread Is Really Cut

• 1
  Key Knowledge of Thread Processing: What a Thread Is, in Numbers
• 2
  Four Ways to Make a Thread and What Each One Costs You
• 3
  Class of Fit and Why the Gauge Decides the Part
• 4
  Material Behavior Decides the Speeds You Can Use
• 5
  Common Thread Defects and What Causes Them
• 6
  Choosing a Thread Method by Part and Volume

A thread is a ramp wound around a cylinder. Pitch is the axial distance from one crest to the next. Lead is how far the nut travels in one full turn. On a single-start thread those two numbers are the same, which is why most callouts list only pitch. On a two-start thread the lead is twice the pitch.

The 60° included angle is the default for metric and unified threads. It spreads load across the flanks and leaves a flat or rounded root that resists cracking. A 55° Whitworth or a 29° Acme form changes the load direction, so never mix them into one assembly.

Three diameters matter. Major is the outside. Minor is the root. Pitch diameter is where the flanks actually touch, and it is the number a thread gauge checks. If a print gives only major diameter and pitch, the pitch diameter comes from the class of fit table, not from the drawing.

• 1
  PitchAxial distance between crests, in mm or threads per inch
• 2
  LeadTravel per revolution; equals pitch on single-start threads
• 3
  Pitch diameterThe controlling dimension for fit and gauge checks

Single-point turning uses a shaped insert fed along the axis while the spindle rotates. The tool follows the lead, so the lathe must be able to synchronize spindle and carriage. It cuts any pitch, left or right hand, internal or external. It is slow per part but needs no special tool, so it suits one-offs, large diameters and threads that must be concentric to a turned bore.

Thread milling interpolates a helical path with a smaller cutter. The tool can be smaller than the hole, so a single mill makes several thread sizes. Chips clear easily and the thread can be cut after heat treatment. It is the practical answer for large internal threads, thin walls and parts that would distort under tapping torque.

Tapping drives a shaped tool straight into a drilled hole. It is fast and cheap per hole on a mill or lathe. The catch is torque. A tap in 17-4PH or titanium can snap, and a broken tap in a finished part is often a scrap decision. Form taps displace metal instead of cutting it, giving stronger threads in aluminium and ductile steel.

Thread rolling squeezes a blank between dies or rolls. No material is removed, so the grain flows along the thread and fatigue strength rises. It needs a ductile material and a diameter close to the finished pitch diameter. It is the method for high-volume studs and fasteners, not for a one-off housing.

• 1
  TurningAny pitch, one-offs, large diameters, tight concentricity
• 2
  MillingLarge internal threads, thin walls, hardened parts
• 3
  TappingFast small holes; risk of breakage in tough alloys
• 4
  RollingHigh volume, ductile metal, stronger thread

A class of fit is an allowance on the pitch diameter. A 1/4-20 UNC 2B internal thread is looser than a 3B, and a 6H metric internal thread is looser than a 6G. Loose fits assemble fast and tolerate plating. Tight fits locate better and resist vibration. The drawing should name the class; if it does not, ask before cutting.

Plating changes the pitch diameter. Electroless nickel at 25 μm adds roughly 50 μm to the major and pitch diameters of an external thread. A 6g external thread that gauged before plating may not gauge after. The fix is to cut undersize before plating or to mask the thread, and that decision belongs on the traveler, not at the machine.

Gauging is where the argument usually ends. A go gauge must enter by hand, and a no-go gauge must not. For critical parts we check pitch diameter with a thread micrometer or optical comparator and record the number. A thread that looks right under a light and fails a no-go gauge is scrap.

• 1
  External6g, 6h, 4g6g; plating allowance matters
• 2
  Internal6H, 6G, 2B, 3B; go / no-go gauges
• 3
  CoatingMask or undersize when the plate is thicker than 10 μm

Aluminium 6061 and 7075 cut freely. Use form taps where you can, because displaced metal gives a stronger thread than a cut one. Watch built-up edge on the flanks of a turned thread; a light spring pass at the same lead clears it.

Stainless 304 and 316L work-harden the moment the tool rubs. Feed must stay above the rubbing threshold, so a tap that is fed too slowly will dull and then snap. 316L also galls, so a sulfurized or coated tap helps. For 17-4PH in the H900 condition, thread milling usually beats tapping.

Titanium Ti-6Al-4V and Inconel 718 are the hard cases. Heat stays at the edge, so use slow surface speed, generous feed and plenty of coolant. Rolled threads are preferred on titanium fasteners because the compressive stress at the root improves fatigue life. On Inconel, thread milling with a coated carbide cutter is the safer route.

• 1
  AluminiumForm tap; beware built-up edge on flanks
• 2
  StainlessKeep feed up; galling is the main failure
• 3
  TitaniumRoll when possible; slow speed, heavy feed
• 4
  InconelThread mill; tapping is a breakage risk

A torn or rough flank usually means the tool rubbed instead of cut. Raise the feed per pass or reduce the number of passes. On a turned thread, a chip caught under the insert leaves a mark that repeats every revolution.

A drunken thread, where the helix wanders, comes from a loose setup or a lathe that cannot hold spindle synchronization. Check the chuck, the tailstock and the program before blaming the insert.

A bell-mouthed internal thread is wider at the entry. The tap or mill pushed the wall out. Reduce cutting force, add a chamfer, or thread mill the hole instead of tapping it. On thin-wall parts, support the outside during the operation.

• 1
  Torn flankTool rubbing; increase feed per pass
• 2
  Drunken threadLoose setup or lost spindle sync
• 3
  Bell mouthWall deflection; lower force or thread mill