CNC Knowledge

How to Use the Internal Thread Knife Percentage Table

This guide explains how the internal thread knife percentage table converts thread height into a radial offset you can dial into the control. It is written for machinists and process engineers cutting internal threads on a lathe or mill-turn center. Read it and you can size an internal thread bore, calculate the infeed, and know when the table stops being useful.

Get Instant Quote Talk to an Engineer

Thread height mathBore sizingOffset incrementsThread inspection

Using the internal thread knife percentage table on a CNC lathe

On this page

1
Key takeaways
2
What the Internal Thread Knife Percentage Table Actually Tells You
3
How Bore Diameter Affects the Percentage You Can Hold
4
Converting a Table Percentage into a Radial Offset
5
Where the Percentage Table Stops Being Useful
6
Step by Step: Using the Table at the Machine
7
Percentage Table Values and What They Mean in Practice

Quick answer

Key takeaways

The table is a ratio, not a depthEach row gives thread height as a percentage of pitch. Multiply by pitch to get radial depth.

Percentages above 80 need a reasonHigh engagement raises cutting force and the risk of a torn or oversized thread.

Bore diameter drives the resultA few hundredths of a millimeter change in the pre-drilled bore moves the finished pitch diameter.

Measure pitch diameter, not the ODA three-wire or thread micrometer check is the only reliable pass/fail on an internal thread.

The basics

What the Internal Thread Knife Percentage Table Actually Tells You

An internal thread knife is a single-point boring bar with a triangular insert ground to the thread form. You feed it radially into a pre-bored hole while the spindle turns, and the tool traces the helix. The depth of that radial infeed decides how much of the thread form is engaged, and that is the number the percentage table gives you.

The table is a lookup between thread height and pitch. For a 60° unified or metric thread, the theoretical height H equals 0.866 × pitch. A row that reads 65% means you cut 0.65 × H, which is 0.563 × pitch of radial depth. Nothing more complicated than that, but the arithmetic has to be done once per thread size, not guessed at the machine.

Most published tables run from about 55% to 95% in 5% steps. Lower percentages cut an easier thread with more clearance at the crest. Higher percentages fill the form and raise the load on the insert. The internal thread knife percentage table does not decide which you need. Your drawing, the class of fit, and the material do.

Bore sizing

How Bore Diameter Affects the Percentage You Can Hold

The pre-drill or pre-bore diameter sets the crest of the internal thread. If the bore is too large, the crest falls away and the thread looks sharp but measures undersize on pitch diameter. If the bore is too small, the insert has to remove more material, cutting force climbs, and you get chatter on a long bar.

A practical starting bore for a 60° thread is nominal minor diameter plus 0.05 to 0.10 mm for coarse pitches under M12, and 0.10 to 0.15 mm for finer pitches where the tool has less room. This is not a tolerance; it is a starting point you adjust after the first part measures.

On stainless 304 or 316L, add 0.02 to 0.05 mm to that bore. The material work-hardens ahead of the edge, and a tighter bore pushes the insert into the hardened skin. On 6061-T6 or C36000 brass, stay at the low end and let the thread height do the work.

1
Bore too largeCrest flats out, pitch diameter reads undersize, thread fails a functional gage.
2
Bore too smallHigher radial load, chatter on bars over 4 × diameter, poor flank finish.
3
Bore on sizePercentage table values apply as written, with a small allowance for tool wear.

Offset math

Converting a Table Percentage into a Radial Offset

Suppose you are cutting an M10 × 1.5 internal thread and want 70% engagement. The table tells you thread height is 70% of H. With H = 0.866 × 1.5 = 1.299 mm, the radial depth is 0.70 × 1.299 = 0.909 mm. That is the distance from the thread crest to the root, measured radially.

Your control usually wants the minor diameter or an X offset, not the radial depth. Minor diameter equals nominal major diameter minus 2 × radial depth. For M10 × 1.5 at 70%: 10 − 2 × 0.909 = 8.182 mm. Program that as the X end point for the threading pass.

If the first part measures oversize on pitch diameter by 0.03 mm, do not reach for the table again. Change the X offset by 0.06 mm, because pitch diameter moves at twice the radial rate. Half the error is on each flank, so the diameter change is double the offset change. This is the single most common mistake when operators use the table without understanding the geometry.

When not to use it

Where the Percentage Table Stops Being Useful

The table assumes a sharp, correctly ground insert with the standard 60° form. A worn insert has a rounded crest, so the effective thread height is lower than the table says and your pitch diameter drifts. Check the insert under a loupe every few hundred parts, not once a shift.

It also assumes a rigid setup. On a boring bar with a length-to-diameter ratio beyond about 4:1, deflection adds to the cut, and the radial depth you dial in is not the radial depth you get. Reduce the percentage by 5 to 10 points on those bars, or use a carbide shank, and verify with a gage rather than trusting the number.

Finally, the table does not apply to pipe threads, buttress threads, or any form that is not the standard 60° V. Those forms have their own height factors. Using a 60° table on an NPT thread is a reliable way to scrap a part.

Procedure

Step by Step: Using the Table at the Machine

1
1. Identify thread size, pitch, and classRead the drawing. Note whether it is 6H, 6G, or a custom class, because that sets your pitch diameter limits before you touch the table.
2
2. Pick a target percentageStart at 65–70% for most internal threads. Go to 75–80% only when the drawing calls for full engagement or the thread carries a sealing load.
3
3. Calculate radial depthMultiply H (0.866 × pitch) by the percentage. Keep three decimal places. Example: M10 × 1.5 at 70% gives 0.909 mm.
4
4. Convert to minor diameterSubtract twice the radial depth from the nominal major diameter. That number goes into the threading block as the X end point.
5
5. Cut the pre-boreBore to minor diameter plus 0.05–0.15 mm depending on pitch and material, then deburr the entry chamfer to 1.5 × pitch.
6
6. Cut one test thread and measureUse a thread micrometer or three-wire check on pitch diameter. Do not judge by eye or by how the nut feels on the first turn.
7
7. Adjust by half the errorIf pitch diameter is off by 0.03 mm, move the X offset by 0.06 mm. Re-cut and re-measure. Two iterations should land inside tolerance.
8
8. Log the setting and lock the offsetRecord the percentage, offset, and insert grade on the setup sheet. The next operator should not have to repeat the whole exercise.

Reference

Percentage Table Values and What They Mean in Practice

Values are for a standard 60° form. Radial depth = percentage × 0.866 × pitch.

Engagement	Radial depth factor	Typical use	Risk
55–60%	0.476–0.520 × pitch	Free-running fasteners, soft brass	Loose fit, low strip torque
65–70%	0.563–0.606 × pitch	General internal threads, most materials	Low risk, good balance
75–80%	0.650–0.693 × pitch	Sealing threads, high load joints	Higher cutting force, insert wear
85–90%	0.736–0.779 × pitch	Special applications only	Chatter, torn flanks, gage rejection
95%	0.823 × pitch	Not practical on an internal knife	Thread likely to fail inspection

FAQs

Internal Thread Knife Percentage Table: Common Questions

What percentage should I start with for a general internal thread?

Start at 65–70% for most work. It gives a clean thread, keeps cutting force reasonable, and leaves room for the pitch diameter to land inside a 6H tolerance band.

Move up only when the drawing asks for full engagement or the thread seals against pressure. Above 80%, check the insert after every few parts.

Why does my thread measure undersize when the table says it should be on size?

The usual cause is a pre-bore that is too large, which flattens the crest and pulls the pitch diameter down. Check the bore before you change the offset.

A worn insert does the same thing. The rounded crest cuts less material than the sharp form the table assumes.

How much do I move the offset when pitch diameter is out of tolerance?

Move the X offset by twice the pitch diameter error. Pitch diameter changes at twice the radial rate because both flanks move.

If pitch diameter is 0.02 mm oversize, reduce the offset by 0.04 mm. Re-cut and measure again.

Can I use the same table for NPT or buttress threads?

No. Those forms have different height factors and different crest geometry. A 60° table gives the wrong radial depth.

Use the height factor listed in the thread standard, or the tooling supplier's chart for that specific form.

Does the material change the percentage I should use?

It changes the bore allowance more than the percentage. Stainless and titanium need a slightly larger pre-bore to avoid work-hardening at the crest.

For aluminium and brass, stay at the low end of the bore range and keep the percentage at 65–70%.

How do I inspect an internal thread without a thread gage?

Use a thread micrometer with the correct anvil set, or a three-wire check on a cast of the thread if the part is small.