A List of Key Knowledge of Thread Treatment in CNC Machining

Thread treatment on a CNC lathe starts with four numbers. The first is the major size, the largest on an external thread and the smallest on an internal one. The second is the pitch size, which sits roughly halfway up the flank and is the value that actually governs fit. The third is the minor size at the root. The fourth is the lead, the axial distance the tool advances per full turn.

The profile is not a triangle but a truncated one. On a 60° metric or unified thread, the flanks meet the crest and root through small flats. Those flats are why thread height is not simply pitch × 0.866. A standard metric thread at M10 × 1.5 has a thread height near 0.92 mm, not the 1.3 mm a sharp triangle would give.

Nominal size on a drawing never tells the whole story. Class of fit does the rest. A 6g external thread and a 6H internal thread are the default pairing in most drawings, and both allow a tolerance band on the pitch value. If a drawing calls out 6e or 4h6h, the band tightens and the cutting insert, the pass count and the gaging plan all change.

Worn inserts cut a wider flank angle than the nominal 60°. On a 1.5 mm pitch thread over 20 mm of engagement, a 1° flank error shifts the pitch value by roughly 0.05 mm. That is ten times our normal ±0.005 mm machining tolerance, so thread gages, not calipers, decide acceptance.

• 1
  Major sizeGoverns clearance at the crest; check with a micrometer over the wire-free crest.
• 2
  Pitch sizeGoverns fit; measure with thread wires or a pitch gage, not a caliper.
• 3
  Minor sizeGoverns root strength; on internal threads it sets the tap drill.
• 4
  Lead and lead angleLead is fixed by pitch; lead angle changes with part size.

Lead angle is the helix angle of the thread, and it depends on pitch and on the size of the part. A fine thread on a large shaft has a shallow helix. A coarse thread on a small shaft has a steep one. The formula is simple: tan(lead angle) = lead ÷ (π × pitch size). For M10 × 1.5 that gives about 2.7°. For M6 × 1.0 it rises to about 3.0°, and for a 1/4-20 UNC it reaches about 3.6°.

The angle matters because a thread insert has a fixed clearance ground into its flank. The standard shim that ships in the holder tilts the insert by 1°. That is enough up to roughly 2° of lead angle. Past that the trailing flank rubs instead of cutting, and the thread tears on one side.

When the lead angle exceeds the built-in tilt, you change the shim, not the insert. Shims are available in 1°, 2°, 3°, 4° and 6° of on-board tilt in most turning systems. The choice is a function of the part, not the machine. On a 40 mm shaft with a 6 mm thread step, a 3° shim is the usual answer, and the standard 1° shim will not do.

The same logic applies to internal threads, but the geometry is inverted. The lead angle is measured on the minor size of the bore, so a small bore with a coarse pitch can need 4° or more. If the bore is shallow, there may be no room for the shim and insert combination, and the thread has to move to a mill with a thread mill.

• 1
  Shallow helixUnder 2°; the standard 1° shim works.
• 2
  Moderate helix2° to 4°; step up to a 2° or 3° shim.
• 3
  Steep helixOver 4°; check holder clearance before quoting the job.

A threading tool does not stop on a dime. At the end of the pass the insert has to clear the flank before the carriage reverses, or the tool drags and the last two threads are ruined. The distance needed depends on spindle speed and on how fast the control can decelerate. As a rule of thumb, allow 1.5 to 2 times the pitch as a minimum, and more if the thread runs into a shoulder.

A thread relief groove is the cleanest answer. Cut it to the minor size of the thread, at least one pitch wide, with a small radius at the bottom to avoid a stress riser. That groove also gives the tool a defined exit and makes gaging repeatable. On parts that will see fatigue loading, the relief is not optional.

Runout at the start of the thread matters just as much. A chamfer at the entry, roughly one pitch deep at 45°, guides the insert in and prevents the first thread from being undersized. Without it, the crest of the lead thread often fails the gage.

On internal threads the retraction distance is limited by the bore depth. If the drawing gives no relief groove and the bore is blind, a single-point tool may not be able to finish the thread at all. In that case we switch to a thread mill on a 3-axis or 5-axis machine, or we ask the designer to open up the relief. Thread milling also handles threads close to a shoulder, and one tool can cut several thread sizes.

• 1
  Minimum retraction1.5 to 2 × pitch, measured from the last full thread.
• 2
  Relief grooveCut to minor size, one pitch wide, with a root radius.
• 3
  Entry chamferAbout one pitch deep at 45° to protect the lead thread.

Thread turning is a light cut with a long contact length. Surface speed usually sits lower than for general turning, often 60 to 120 m/min in steel and 150 to 250 m/min in aluminum. Carbide grades with a thin PVD coating hold up well on stainless, where work hardening at the flank is the main enemy. On 304 and 316, keep the tool moving and avoid dwelling in the cut.

Infeed strategy changes the chip. Radial infeed is simple but loads both flanks at once. Flank infeed cuts on one side, which gives a better finish and longer insert life, at the cost of more passes. Modified flank infeed is the usual compromise and is what most CAM posts default to for a 60° thread.

Lubrication matters most in blind holes and in gummy materials. High-pressure coolant aimed at the flank clears chips and cools the insert. Aluminum and copper alloys can be cut dry or with mist, but stainless, titanium and Inconel need flood or through-tool coolant. On titanium, chlorine-free coolant is a hard requirement.

The failures we see most often are torn flanks from a wrong shim, chatter from too little support on a long part, and a gage that will not enter because the pitch value drifted during the last pass. A spring pass at the same depth, without additional infeed, cleans up the flanks and costs a few seconds. On parts held in a collet, check that the collet is not marking the crest of the thread.

• 1
  Torn flankCheck shim tilt and lead angle before blaming the insert grade.
• 2
  ChatterSupport the part with a steady rest or reduce spindle speed.
• 3
  Tight gageAdd a spring pass; re-check the pitch value, not the major size.
• 4
  Chipped crestToo little entry chamfer, or the tool is dragging on retraction.

Thread gaging is the only reliable acceptance test. A go gage must enter by hand over the full thread length. A no-go gage must not enter more than two turns on an external thread or three on an internal one, unless the drawing states otherwise. Calipers and micrometers measure the crest, not the flank, so they cannot confirm a class of fit.

For low-volume work we use thread wires with a micrometer to check the pitch value directly. On production runs, a thread comparator or a thread gage set gives faster results with less operator judgment. Reports are available on request, and every part gets a full inspection before it leaves the floor.

Thread milling is the better process when the part is thin-walled, when the thread sits close to a shoulder, or when the material is hard and a single-point tool would deflect. A thread mill cuts with a helical interpolation, so the load is spread over several teeth and the wall sees less force. It also lets one tool cover a range of sizes.

Roll forming is another option on ductile materials. The grain flows along the flank instead of being cut, which raises fatigue strength. It needs a slightly larger blank than a cut thread, and it will not work on cast iron or on any material that tears rather than flows.

• 1
  Go gageMust enter by hand over the full thread length.
• 2
  No-go gageTypical limit is two turns external, three internal.
• 3
  Thread wiresDirect pitch value check on low-volume and prototype parts.