Threads on machined parts: callouts, depth and gauging

What a thread callout actually controls

A thread is a helical form defined by a basic profile. The callout does not describe that profile in detail. It points to a standard, then states the size, the pitch, the tolerance class and the length. The shop reads the standard for the profile and uses the callout for the rest.

The two features that decide fit are the pitch diameter and the flank angle. The major diameter on an external thread and the minor diameter on an internal thread matter for clearance and for the crest, but they do not control the fit on their own. A thread can pass a major diameter check and still bind because the pitch diameter is wrong.

That is why a thread callout that only says M6 is incomplete. M6 is the nominal major diameter and the coarse pitch is implied, but the tolerance class, the direction of the thread and the length are still open. On a drawing these details are usually in the note or in the thread table, and they are the first thing a supplier checks.

The parts of a complete callout

Take a callout such as M6 x 1 - 6H, depth 12. Each element has a job. Read it from left to right.

Coarse or fine pitch

Coarse pitch is the default for general fastening. It gives more thread engagement per turn, tolerates a damaged crest better and is cheaper to tap. Fine pitch gives a higher tensile area for the same nominal diameter, a shallower thread depth and better resistance to vibration loosening.

Fine pitch is common on thin-wall parts and on brass fittings where wall thickness is limited. It is also common where adjustment is needed, because a fine thread moves less per turn. The trade-off is that fine threads are more easily cross-threaded and more sensitive to pitch diameter error.

Do not change the pitch without checking the mating part. A 1/4-28 and a 1/4-20 look similar on a drawing and will not assemble. If the drawing is derived from a catalogue, copy the exact thread callout from the mating component rather than the nominal size.

Cut, rolled or milled

A cut thread is produced by a tap, a die head or a single-point tool. Material is removed, the grain flow is interrupted and the root is a machined surface. It is the most flexible method and the standard for small batches and for internal threads in most materials.

A rolled thread is formed by displacing material rather than removing it. The grain flow follows the thread contour, the root is in compression and the fatigue strength is usually higher than a cut thread. The blank diameter must be close to the pitch diameter, and the material must be ductile enough to flow. Hard or brittle alloys can crack at the crest.

A milled thread is cut with a rotating multi-tooth tool on a machining centre. It is slower per thread but it holds position accurately relative to other features, and it can cut a thread close to a shoulder. It is common on large diameters and on parts where the thread position matters more than the cycle time.

Blind holes, depth and relief

A blind tapped hole needs three depths: the drill depth, the full thread depth and the usable depth after the chamfer. The drawing usually states the full thread depth, and the drill has to go deeper to leave room for the tap lead-in and the chip.

As a working rule, the drill depth should exceed the full thread depth by at least three to five pitches, depending on the tap. A forming tap needs more room because it displaces material rather than cutting it. A blind hole that is drilled only to the thread depth will produce a thread that stops short and a tap that bottoms out.

A thread relief or undercut at the end of the thread lets the tool run out cleanly and gives the mating part a place to seat. Without a relief, the thread fades into the shoulder and the last thread is incomplete. If the mating part has a chamfer, the relief can be shallow. If it has a square end, the relief has to be deep enough to clear it.

On thin-wall parts, a blind hole reduces the wall section at the base. Check the remaining wall against the torque the fastener will apply, especially in brass and copper where the wall yields before the fastener does.

How a thread is gauged

The standard check is a go/no-go pair. For an internal thread, the go plug gauge must enter the full thread by hand. The no-go plug must not enter more than a specified number of turns, typically two. For an external thread, a go ring must pass over the full thread and a no-go ring must not.

The gauge checks the maximum and minimum material condition. It does not measure a number, so it does not tell you where in the tolerance band the part sits. If you need that, use a thread micrometer, a three-wire measurement or a thread scanning instrument. These are slower and need a trained operator, so they are usually reserved for first articles and for problem features.

Depth needs a separate check. A thread depth gauge or a depth micrometer against a datum face is normal. Position and squareness need a third check, usually on a coordinate measuring machine or with a dedicated fixture. A go gauge that enters freely says nothing about whether the hole is perpendicular to the face.

For small threads, gauge wear matters. A worn go plug can accept an undersize thread. Ask for the gauge calibration record if the feature is critical, and keep the gauges in a controlled set.

Position, projected tolerance and thin flanges

A tapped hole is usually controlled with a position tolerance. If the mating part is thick or the fastener is long, the error at the far end of the hole is larger than the error at the surface. A projected tolerance zone extends the control above the surface to account for that, and it is the correct call for a hole that receives a stud or a long screw.

On a thin flange, the thread itself may be fine and the assembly may still fail because the hole is not square to the face. Perpendicularity of the hole axis to the mounting face is often a better control than position alone, particularly where two parts are bolted face to face.

Think about the fastener stack. A hole that is positioned correctly at the surface but tilted by half a degree over a 20 mm stack moves the far end by about 0.17 mm. That is enough to bind a close-fit bolt. The projected zone is how the drawing captures that risk.

The callouts that cause rework

Most thread problems start on the drawing, not at the machine. These are the ones that come up most often.

• A nominal size with no tolerance class, which leaves the fit to the supplier.
• A depth given as the drill depth, so the usable thread is shorter than the mating screw.
• No thread relief at a shoulder, so the last thread is incomplete and the mating part does not seat.
• A position tolerance with no projected zone on a long fastener stack.
• A fine pitch chosen for wall thickness without checking the mating part.
• A thread callout on a plated part without a pre-plate allowance, so the go gauge fails after plating.
• Mixed metric and inch callouts on the same drawing, which invites a wrong tap.