To specify threads on a drawing, give the nominal size, threads per inch or pitch, thread series, class of fit, and internal or external designation, followed by the full thread depth. A complete callout such as 1/4-20 UNC-2B, 0.50 deep, or M6x1-6H, 12 deep, tells the machine shop exactly how to cut and gage the thread.
Incomplete thread callouts are one of the most common reasons a machine shop sends questions on a quote. This guide covers unified inch threads, metric threads, thread classes, and depth callouts so your drawing can be quoted and gaged without ambiguity.
Anatomy of a unified inch thread callout
A unified thread callout under ASME B1.1 reads left to right:
- Nominal size: 1/4, or a number size such as #10.
- Threads per inch: 20.
- Series: UNC coarse, UNF fine, UNEF extra fine, or UN constant pitch.
- Class: 1, 2, or 3.
- Designation: A for external, B for internal.
- Depth: full thread depth for internal threads, and length for external threads if needed.
Example: 1/4-20 UNC-2B, 0.50 full thread depth. Add LH for left-hand threads.
Thread classes explained
| Class | External / internal | Fit | Typical use |
|---|---|---|---|
| 1A / 1B | External / internal | Loose, generous allowance | Quick assembly, dirty environments; uncommon today |
| 2A / 2B | External / internal | Standard commercial fit | Most fasteners and machined parts |
| 3A / 3B | External / internal | Tight, no allowance on 3A | Precision assemblies, aerospace-style hardware |
| 6g / 6H | Metric external / internal | Standard metric fit | Default for most metric threads |
| 4g6g / 5H | Metric external / internal | Closer metric fit | Precision metric assemblies |
Class 3 threads cost more to produce and gage than Class 2. Specify Class 3 only where the fit requires it.
Metric thread callouts
A metric callout under ISO standards gives M, nominal diameter, pitch, and tolerance class: M8x1.25-6H for an internal thread. Coarse pitch is sometimes omitted, but stating it removes any doubt. For fine pitch, the pitch must always be shown, such as M8x1-6g.
Specifying thread depth correctly
For tapped holes, give the full thread depth and the drill depth if it matters. Taps have a chamfered lead, so the drilled hole must be deeper than the full thread depth. In blind holes, a full thread depth of about 1.5 times the nominal diameter is usually enough for steel, and about 2 times diameter in aluminum. Deeper threads add cycle time and tap breakage risk without much strength gain.
Other thread details to state
- Countersink or chamfer at the thread entrance.
- Thread relief or undercut on external threads that run to a shoulder.
- Whether threads are to be gaged before or after plating.
- Pipe threads: NPT or NPTF, with size, such as 1/4-18 NPT.
- Thread inserts: specify the insert and the tapped hole for it, such as the STI tap size.
Common thread callout mistakes
- Omitting the class, which leaves the fit undefined.
- Calling only the tap drill depth, not the full thread depth.
- Specifying full thread to the bottom of a blind hole, which a standard tap cannot produce.
- Mixing inch and metric threads on one part without clear notes.
- Calling Class 3B on every hole when only a few need a precision fit.
- Leaving out the pitch on fine metric threads.
- Specifying deep threads in a thin wall without checking that the wall supports them.
Each of these produces a question from the shop or, worse, parts that pass the shop's interpretation but fail your assembly. Thread forming, as opposed to cutting, is an option in ductile materials such as aluminum and some steels; if the drawing does not allow formed threads, say so.
How machine shops cut and inspect threads
On CNC lathes, external and internal threads are single-point cut or formed with taps and dies. Live tooling allows tapping and thread milling of off-axis holes. On machining centers, threads are tapped or thread milled. Threads are inspected with go and no-go gages, and measured further when required. Wexmar cuts threads on its CNC lathes, Swiss-type machines, and horizontal machining centers. See CNC turning and inspection and quality.
Thread callout checklist
- Size, pitch, and series stated.
- Class and A or B designation stated.
- Full thread depth given for tapped holes.
- Chamfer, relief, and left-hand requirements noted.
- Gaging before or after plating noted.
Getting a quote
Wexmar reviews thread callouts during quoting and will flag incomplete or conflicting callouts. You can upload a drawing for an instant estimate or call (315) 400-2654.