How-to guide

The Treatment Steps for Multi-Thread CNC Towers That Hold Their Phase

This guide is for machinists and process engineers who need two- or three-start threads cut on a lathe without pulling the part. It covers lead and pitch math, the G32, G92 and G76 cycles, tool offset, index shift and inspection. Read it and you can judge whether a part suits multi-thread CNC towers or belongs on a mill instead.

Get Instant Quote Talk to an Engineer

Lead = pitch × startsG32 / G92 / G76Ø400 mm rotary table±0.005 mm

Multi-thread CNC towers setup on a CNC lathe with a multi-start threaded part

On this page

1
What matters before you cut
2
What multi-thread CNC towers actually cut
3
Read the callout before you program anything
4
Choosing between G32, G92 and G76
5
Workholding and tool setup that survive the second start
6
Step by step: cutting a two-start M30 × 3 thread
7
Which threading method fits the part
8
Lead, pitch and index shift for common multi-start threads

Key takeaways

What matters before you cut

Lead is the number that drives the cycleFor M30 × 3 / 2, pitch is 1.5 mm and lead is 3 mm. Program F to the lead, not the pitch.

Index shift is just lead divided by startsTwo starts on a 3 mm lead means a 1.5 mm axial shift between passes. No gear change needed.

The G76 cycle handles multi-start in one blockSet the number of starts and the cycle repeats the passes with the index shift applied automatically.

Verify with a thread micrometer and a go/no-go gaugePitch diameter, lead error and flank angle decide whether the assembly threads on by hand.

Never re-chuck between startsOne setup, one zero. Moving the part between passes is the fastest way to lose the index.

Basics

What multi-thread CNC towers actually cut

A multi-start thread is a single helix cut two, three or four times around the same cylinder. Each start is a separate groove, spaced evenly around the circumference. The pitch stays small, but the lead grows by the number of starts. That is the whole trick: a shallow, fast-moving thread that still has a fine pitch for clamping force.

You see this on optical adjusters, valve stems, grease nipples, camera lens mounts and quick-release pins. Anywhere the operator needs a large axial travel per turn without cutting a coarse, weak thread. A two-start M30 × 3 / 2 moves 3 mm per revolution while the thread depth stays at a 1.5 mm pitch. A single-start M30 × 3 would move the same 3 mm but cut a much deeper V.

The trade-off is phase control. On a manual lathe you finish the first groove, loosen the chuck, index the part with a dial indicator, then cut the second. That works for one part. It does not scale, and it does not survive a re-clamp. On a CNC lathe the index shift is a number in the program, so every part is identical and the operator never touches the part between starts.

Multi-thread CNC towers are the right call when starts are 2 to 4, lead is under about 12 mm, and the part has a shoulder or a feature you can hold in one setup. Above that, or on a part that must be re-fixtured, a mill with a rotary table is usually the cleaner route.

Math

Read the callout before you program anything

The drawing usually reads something like M30 × 3 / 2-5g6g. Decode it in this order. The first number after the M is the lead, 3 mm. The number after the slash is the number of starts, 2. Pitch equals lead divided by starts, so 1.5 mm. That is the value you look up in the thread table for depth and pitch diameter.

This is where most first attempts fail. Operators see M30 × 3 and program F3.0 with a single-start thread profile. The cycle runs, the part looks threaded, and the gauge will not go on. The thread depth is wrong because the profile was cut for a 1.5 mm pitch.

For a 60° metric thread, thread height H equals 0.866 × pitch. With a 1.5 mm pitch, H is 1.299 mm. External thread depth is about 0.613 × pitch, so roughly 0.92 mm per side. Use the pitch, never the lead, for the depth and the infeed.

Keep a small table at the machine. It saves more scrap than any feed-and-speed chart. The lead drives the feedrate and the index shift. The pitch drives the profile, the depth and the gauge.

1
LeadAxial travel per spindle revolution. Programmed as F.
2
PitchDistance between adjacent flanks of the same start. Drives depth.
3
Index shiftLead divided by starts. Applied as a Z offset between passes.
4
Pitch diameterThe gauge dimension. Check it with a thread micrometer or three-wire method.

Cycle choice

Choosing between G32, G92 and G76

G32 is one pass, one block. You write every pass yourself: rapid to start, G32 to the end point, retract, return, shift Z by the index, repeat. It gives you full control over infeed and lets you start each groove from a different Z so the tool does not wear one spot. It is also long and easy to mistype.

G92 is a threading cycle on most Fanuc-style controls. One block per pass, with the start point and end point given. It is shorter than G32 and still lets you set the depth per pass. Some controls let you add a Q value for the index shift, some do not. Check the manual before you trust it.

G76 is the two-block cycle. The first block sets the number of finish passes and the chamfer amount, the second sets depth of cut, first pass depth, thread height, pitch and the number of starts. On a control that supports the starts parameter, G76 handles the index shift for you and the code stays short.

For 2 to 4 starts and a lead under 12 mm, G76 is the practical default. Use G32 when the thread is unusual, when you need a specific infeed pattern, or when the control's G76 does not support a starts value. Do not mix the two in one program.

Fixturing

Workholding and tool setup that survive the second start

Everything depends on the part not moving between passes. Chuck on a turned diameter, not on the raw bar. Turn a clean clamping land first, then grip that land for the threading passes. If the part has a shoulder, seat it against soft jaws so the axial position repeats.

For thin-wall parts, use a collet or a split bushing. A three-jaw chuck at high clamping pressure will ovalize the bore, and the pitch diameter will measure differently after the part relaxes. If the wall is under about 2 mm, expect to take a light spring pass and check the gauge twice.

Set the tool on center. A threading insert even 0.05 mm high or low changes the flank angle and the effective pitch diameter. Use a center-height gauge, not a shim stack. For a 60° insert, a small height error shows up as a poor gauge fit long before it shows on the micrometer.

Lock the Z axis reference at the start of the run. Write the index shift as a positive Z offset from that single reference. Do not re-zero between starts and do not touch the tool offset after the first pass. If a pass has to be repeated, repeat the whole groove, not one pass.

Procedure

Step by step: cutting a two-start M30 × 3 thread

Example part: 45# round steel, thread length 25 mm, 2 × 45° chamfer at both ends, Ra 3.2 μm flank finish.

1
1. Decode the calloutRead M30 × 3 / 2-5g6g as lead 3 mm, starts 2, pitch 1.5 mm. Write pitch, lead and index shift (1.5 mm) on the setup sheet before touching the control.
2
2. Prepare the blankFace and center. Turn the major diameter to 29.7–29.8 mm for a 5g external thread, leaving 0.2–0.3 mm for the finishing pass. Cut the 2 × 45° chamfers now, not after threading.
3
3. Set the toolMount a 60° full-profile insert for 1.5 mm pitch. Set center height with a gauge. Touch off X on the turned diameter and Z on the face. Lock both offsets.
4
4. Set the cycleProgram G76 with pitch 1.5 mm, thread height about 0.92 mm, first pass depth 0.3 mm, minimum depth 0.08 mm, and 2 starts. Confirm the control applies the index shift.
5
5. Dry runRun the cycle with the tool 20 mm clear of the part. Watch the Z shift between the two starts. It must equal 1.5 mm. Any other value means the starts parameter is wrong.
6
6. Cut the first partRun at 400–700 rpm for steel, depending on the part stiffness. Keep spindle speed and feed locked. Do not override the feed mid-thread.
7
7. InspectCheck pitch diameter with a thread micrometer or three-wire method. Run the go gauge by hand. If the no-go enters more than two turns, the thread is oversize.
8
8. Lock the processRecord the offsets, the cycle values and the gauge result. Run the balance of the batch without touching offsets. Re-check the first part after any tool change.

Decision table

Which threading method fits the part

Use this to pick the process before you write code.

Method	Best for	Watch out for	Typical use
Single-start G76	Fine pitch, high clamp load	Slow axial travel per turn	Bolts, fittings, adjustment nuts
Two-start G76	Fast travel, fine pitch	Index must be exact	Valve stems, lens mounts
Three or four starts	Very fast travel, short length	Shallow flanks, gauge wear	Quick-release pins, adjusters
G32 hand-coded	Odd profiles, controlled infeed	Long code, typo risk	Prototypes, repairs
Mill with rotary table	Parts that must be re-fixtured	Cycle time, setup cost	Housings, interrupted threads
Thread milling	Large bores, thin walls	Tool cost, spindle time	Manifolds, aerospace bodies

Reference

Lead, pitch and index shift for common multi-start threads

Lead equals pitch times starts. Index shift equals lead divided by starts.

Callout	Pitch (mm)	Lead (mm)	Index shift (mm)
M20 × 2 / 2	1.0	2.0	1.0
M24 × 3 / 2	1.5	3.0	1.5
M30 × 3 / 2	1.5	3.0	1.5
M30 × 3 / 3	1.0	3.0	1.0
M36 × 4 / 2	2.0	4.0	2.0
M42 × 6 / 3	2.0	6.0	2.0

Pick the cycle from the drawing, not from habit

If the callout has a slash and a starts number, do the lead and pitch math first, then choose G76 for 2 to 4 starts and G32 for anything unusual. Get the index shift right on a dry run before the tool touches metal.

Get Instant Quote Talk to an Engineer

FAQs

Questions that come up on the floor

Why does my two-start thread gauge fit on one start but not the other?

The index shift is wrong or the part moved. Check that the Z offset between passes equals lead divided by starts, in this case 1.5 mm. Verify it on a dry run before cutting.

If the shift is correct, the part rotated in the chuck. Re-chuck on a turned land, seat against a shoulder, and re-cut the whole groove. Do not try to blend a partial second start.

Can I cut multi-start threads with G92 instead of G76?

Yes, if your control accepts a starts value or if you write a separate cycle for each start with a shifted Z start point. Write the shift into the start point, not into the tool offset.

Check the control manual first. Some Fanuc-style controls apply the shift automatically in G92, others ignore it. If the dry run shows no shift, switch to G32 with an explicit Z offset per pass.

What spindle speed should I use for a 3 mm lead thread?

On 45# steel with a full-profile insert, 400–700 rpm is a practical window. The limit is usually the control's feedrate and acceleration, not the insert.

At 700 rpm and a 3 mm lead, the Z axis moves 2,100 mm/min in a synchronised move. If the machine hesitates at the start or end of the thread, lower the speed rather than the lead.

How do I check pitch diameter on a multi-start thread?

Use a thread micrometer sized for the pitch, or the three-wire method with the correct wire diameter for a 1.5 mm pitch. Measure each start in the same axial position.

A go/no-go gauge is the fastest check on the floor. The go gauge should enter by hand. If the no-go enters more than two turns, the thread is oversize and the depth of cut is too shallow.

When should I move the job to a mill instead of a lathe?

When the thread is interrupted, when the part cannot be held in one setup, or when the thread is larger than the spindle through-bore allows. Also when starts exceed four.

Thread milling on a 5-axis or 4-axis mill handles large bores and thin walls with less cutting force. The trade-off is cycle time and tool cost, so it is usually a batch-size decision.

Does tool height really matter that much?

Yes. A 60° insert set 0.1 mm off center tilts the effective flank angle and changes the pitch diameter by more than the thread tolerance on a fine pitch.

Set center height with a gauge every time you change the insert. On a 1.5 mm pitch thread, the tolerance band is narrow and a shim stack will not hold it.