Updated
Use a complete designation and keep the feature extent explicit. This guide decodes metric, Unified inch and NPT examples, then shows how to deal with blind holes, finishing and inspection without assuming that every thread follows the same acceptance rules.
Read thread callouts as a system, size, pitch and fit
Thread callouts identify the thread system, nominal size, pitch or threads per inch, and applicable tolerance designation. Add the feature count, thread extent and any special direction or finishing requirement. A correctly decoded size still leaves an incomplete manufacturing instruction when usable engagement or final-condition acceptance is unspecified.
Start by recognizing the prefix or series: M indicates a metric screw thread, UNC identifies a Unified coarse series, and NPT identifies a tapered pipe thread. The number after a metric multiplication sign is pitch in millimeters. In a Unified designation, the number after the diameter is threads per inch.
Keep the complete designation together so a supplier does not infer one field from a different note. Thread Check’s designation reference illustrates internal and external metric and Unified formats. A thread form rendered in CAD can help visualization, but the drawing designation remains essential when the model uses simplified or cosmetic threads.
Metric, UNC and NPT examples side by side
The examples below show different systems, not interchangeable names for similar-looking connections. Interpret the size in the system stated by the designation. Pipe nominal size is particularly easy to confuse with a measured outside diameter.
The extent notes are illustrative additions. They must be located and dimensioned on the actual drawing so the start face and required thread length are unambiguous.
| Example | Decoded fields | Feature type | Additional requirement to resolve |
|---|---|---|---|
| M6 × 1 – 6H | 6 mm nominal diameter; 1 mm pitch; 6H tolerance class | Internal metric thread | THRU or minimum full thread depth |
| M6 × 1 – 6g | Same nominal size and pitch; 6g external tolerance class | External metric thread | Threaded length, shoulder clearance and final finish |
| 1/4-20 UNC-2B | 1/4 in nominal size; 20 TPI; Unified coarse; class 2 internal | Internal Unified thread | Extent and required inspection condition |
| 1/4-20 UNC-2A | Same nominal size, pitch and series; class 2 external | External Unified thread | Length, runout region and finishing condition |
| 1/8-27 NPT | Nominal pipe size 1/8; 27 TPI; tapered pipe thread | Port or fitting, as shown | Applicable standard, gauge acceptance and sealing arrangement |
Twenty threads per inch corresponds to a pitch of 25.4 / 20 = 1.27 mm. This arithmetic conversion does not make a 1/4-20 thread compatible with a metric thread having a nearby pitch; diameter, profile and tolerances still belong to the named system.
Interpret 6H and 6g without mixing internal and external classes
In a simple metric designation, the number identifies a tolerance grade and the letter identifies the tolerance position. Capital letters are used for internal threads and lowercase letters for external threads. Thus 6H and 6g describe different members of the connection; they are not alternative labels for the same tapped hole.
Metric tolerancing can specify the pitch-diameter and crest-diameter tolerances separately when required. A short designation such as 6H is common, but a more detailed designation may contain multiple tolerance classes. Read it under the drawing’s stated standard rather than reducing every metric requirement to one number and letter.
ISO 965-1:2026 defines the general-purpose metric tolerance system. Its edition does not automatically change an existing contractual drawing. State which edition governs the part and check mating requirements before altering the designation. If the thread will be coated, address the pre-coating manufacturing allowance and final acceptance condition separately; the finish cannot be left to an inspector to interpret from 6H alone.
Decode Unified fit classes without promising joint performance
For Unified threads, A designates an external thread and B an internal thread. Class 2A and 2B are commonly used general-purpose designations. Classes describe dimensional limits and allowance; they do not specify bolt material, preload, fatigue strength or the torque needed for a particular joint.
Specify the series as well as diameter and TPI. UNC and UNF differ in pitch for a given nominal diameter, and special series can have other combinations. A similar measured diameter does not prove that a fastener matches the thread. Use the full designation to select the mating component and the gauge.
ASME B1.1-2024 covers Unified thread forms. Do not use a tighter class as a shortcut for higher joint strength. The joint still needs an engagement and load assessment. Fine pitches can be useful for particular adjustment or wall constraints, but there is no universal rule that a fine thread always holds better in a thin wall or that a coarse thread is always easier to manufacture.
Keep NPT pipe size and sealing separate from screw-thread fit
An NPT nominal size is a pipe designation, not the thread’s outside diameter. The 1/8 in in 1/8-27 NPT therefore does not describe a 1/8 in external thread diameter. Do not select a drill, fitting or wall thickness by that nominal fraction alone.
ASME B1.20.1 covers the dimensions and gauging of NPT and other listed inch pipe threads. Specify the relevant form explicitly. Not all pipe threads are tapered, and a parallel port may seal at an O-ring, gasket or another designed surface rather than on the threads.
Parker’s fitting installation manual distinguishes NPT, BSPP and BSPT connection arrangements. Similar nominal labels do not establish interchangeability. For NPT, use the fitting manufacturer’s assembly and sealant guidance appropriate to the fluid and service. A dimensional gauge result does not prove leak tightness, and overtightening to stop a leak can damage the port or fitting.
Separate full thread depth from the drilled blind-hole depth
A blind hole must accommodate usable threads, incomplete tool lead or runout, and the remaining tool clearance. The full thread depth is the length of complete threads available for engagement; the hole depth is a separate geometric requirement. Neither should be inferred from the other.
Use a clear note such as M6 × 1 – 6H, MIN FULL THREAD DEPTH 12 mm, together with a separately dimensioned drilled hole. This is an illustrative callout, not an engagement recommendation. The actual required engagement depends on the joint load, fastener, parent material and permitted failure mode.
Dimension hole depth to a defined feature: full cylindrical depth and drill-point depth are different references. Let the supplier propose the needed machining clearance when the design permits, then confirm that the remaining wall and neighboring passages are protected. For a deep blind port, consider chip removal and access for gauging. Do not demand full threads to a mathematically sharp bottom that the selected tool cannot produce.
Specify the finishing condition before the gauge is selected
A coating can change the effective thread dimensions and the assembly behavior. State whether acceptance applies after all specified finishing, and identify masking or another approved route where necessary. A pre-finish passing result is insufficient when the purchase requirement is a finished threaded component.
Review plating, anodizing, paint and other treatments through the surface finishing route. Their effects depend on the treatment and geometry; do not apply one universal thickness allowance to all processes. Cutting or chasing a thread after coating can expose substrate and change the corrosion protection, so it needs an approved process decision.
Protect the thread lead-in and contact surfaces during handling. Cosmetic residue or coating buildup can interfere with a gauge or assembly even when the underlying machined size is correct. Define cleaning before inspection and keep it consistent. A drawing note that merely says plated is incomplete without the treatment specification, coverage and acceptance condition relevant to the threaded feature.
Make thread inspection match the actual requirement
Use the appropriate gauge and acceptance procedure for the thread system and class. Internal screw threads generally require thread plug gauging, and external screw threads require suitable ring or other specified gauging. Tapered pipe-thread gauging uses its own reference and acceptance rules; it is not a UNC GO/NO-GO check with a different label.
ASME B1.3 addresses screw-thread gauging systems and the characteristics evaluated for dimensional acceptability. Agree on the governing system rather than assuming one functional gauge covers every drawing requirement. Apply the standard’s rules for gauge engagement instead of inventing a universal NO-GO turn count.
Full-thread depth, thread-axis location and leak performance may require separate checks. A gauge entering the hole does not prove the thread is correctly located relative to mounting faces. Use the drawing tolerance framework to define that relationship. Record gauge identity, acceptance condition and any additional depth or location measurement needed for the inspection report.
Release a drawing that leaves the tool choice flexible
Specify the functional result and leave the manufacturing method open where it does not affect the design. Tapping, thread milling and turning can produce different access and runout requirements. The supplier should identify which route can meet the drawing without forcing an unnecessary tool constraint into the design.
Review material and thin-wall limitations through the CNC machining process; rotating external features may also need a turning review. Make thread count, pitch, class, extent, direction and finish consistent between the drawing and CAD model. A leader should point to the actual threaded feature, not an adjacent clearance hole.
A complete callout prevents interpretation work at the machine and inspection bench. The important outcome is a matching mating thread with enough usable engagement, the intended final condition and a reproducible acceptance method. A longer note is justified when it removes a real ambiguity; adding every possible manufacturing detail is unnecessary when the standard already defines it.
Submit the model and annotated drawing through 6CProto’s quote request. Include thread standards, minimum full thread depths and final finishing requirements for the DFM review.
FAQ
How should a left-hand thread be shown?
Add the applicable LH designation under the governing thread standard and make the mating requirement consistent. Do not rely only on the helix direction drawn in a view, particularly when CAD uses a cosmetic thread. Check that the purchase specification, fastener description and gauge request all identify the left-hand feature. A normal right-hand gauge or mating screw is not an acceptable substitute just because the nominal size matches.
Can an insert replace a directly tapped hole without changing the drawing?
An insert changes the parent-hole preparation, installed thread and possibly the joint behavior. Specify the insert system and installation requirements when it is part of the design. If it is proposed as a repair, obtain the appropriate engineering disposition rather than treating it as an invisible manufacturing choice. Confirm the installed thread, available engagement, protrusion limits and any effects on neighboring features or corrosion protection.
Should repeated tapped holes be called out individually?
A common note can cover identical threaded features when its scope is clear and the hole count is correct. Separate any feature with a different depth, finish, direction or acceptance requirement. Check every view so a pattern note does not accidentally include a clearance hole or exclude a hidden tapped hole. Clarity matters more than repeating the same designation beside each hole on a crowded drawing.