Guide
How do you inspect a tapped hole with a go/no-go thread gage?
A go/no-go thread gage is a pair of fixed limit gages that tells an inspector whether a thread lies inside its tolerance, without measuring it. For a tapped hole the pair is a thread plug: the GO end must screw in, and the NOT GO end, which the inch standards call HI, must not.
By Saola Manufacturing engineering team · Published · Updated
This guide is for engineers and quality staff who receive tapped parts from a supplier, including one overseas. It explains what each gage member actually checks, how to apply it, which gages a complete check needs, why two gages can disagree on the same hole, how plating changes the answer, and what to write on the drawing or purchase order so the supplier and your receiving inspector use the same rule. The acceptance rules quoted here come from the published US screw-thread standards and the federal handbook that preceded them; they describe the standards, not any particular shop.
On this page
What does a go/no-go thread plug gage actually check?
The GO member checks the functional size of the tapped hole at the maximum-material limit, so a screw at its largest permitted size will assemble. The HI or NOT GO member checks the pitch diameter at the minimum-material limit, so the hole is not cut so large that the thread engagement is weak.
The difference between the two ends matters. The GO member is a full-form thread, ideally made to the smallest permitted size of the internal thread and as long as the length of engagement. Because it is a complete threaded counterpart, it reacts to everything that makes a hole tight: pitch diameter, lead error, flank angle, taper, out-of-round and burrs. The federal screw-thread handbook calls the GO plug “a cumulative check of all thread elements except the minor diameter” (NBS Handbook H28, 1969).
The HI member is deliberately different. Its crests are truncated and it is shorter, so it touches the flanks near the pitch line and checks one element, the pitch diameter, at the loose end of the tolerance. Per the same handbook, each element can only be checked singly at the minimum-material limit, which is why a thread plug alone does not finish the job.
Neither threaded member checks the minor diameter of the hole, because both are cleared at the root. The minor diameter is the tap drill size, and it controls how much thread depth the screw can bear on. It needs its own plain cylindrical GO and NOT GO plugs.
How do you use a GO and NOT GO thread plug gage correctly?
Turn the GO member in by hand, without force, and it must enter the full threaded length of the hole. Then try the HI member: the thread is acceptable if it does not enter, or if it enters but picks up a definite drag on or before the third turn.
The drag allowance surprises people who expect the NOT GO end to stop dead. The handbook explains why it exists: the first threads of a tapped hole are incomplete, the starting threads of the HI gage wear faster than the rest, and no one can control the torque an operator applies. So the rule accepts limited entry and tells the inspector not to force the gage once the drag is definite. Thin walls, soft or ductile material and very short threads may need the rule adjusted, and that adjustment belongs on the drawing.
A practical sequence for each hole:
- Clean first. Blow out chips and cutting fluid. A chip in a blind hole reads as a short thread, and a GO gage driven onto a chip is a damaged gage.
- GO member, full depth. It should run in with finger pressure to the required thread depth. On a blind hole, compare against the callout for full-thread depth, not the drilled depth.
- HI member, count turns. Stop at the definite drag. Entering past the third turn with no drag is a reject.
- Minor diameter plugs. The plain GO plug must enter completely and the plain NOT GO plug must not enter.
- Record and set aside. A reject goes to a hold area with the gage serial number noted, so the result can be rechecked with a second gage.
Holes cut on a CNC milling center are usually tapped or thread-milled in the same setup, so a gage failure can often be traced to one tool. A GO failure on every part points to a worn tap or a drill running small; an HI failure points to an oversize tap, a thread mill offset, or material that springs back after tapping.
Which gages does a complete tapped-hole check need?
A full attribute check of an internal thread uses three gage members: the GO thread plug, the HI thread plug, and a pair of plain plugs for the minor diameter. The table lists what each one represents and how it is read.
| Gage member | Limit it represents | Accept when | Marking example |
|---|---|---|---|
| GO thread plug | Maximum material (smallest hole); functional size | Enters the full threaded length freely | .250-20 UNC GO PD .2175 |
| HI thread plug | Minimum material (largest pitch diameter) | Does not enter, or definite drag on or before the third turn | .250-20 UNC-2B HI PD .2224 |
| GO plain plug, minor diameter | Smallest permitted minor diameter | Enters completely | .250-20 UNC GO .1960 |
| NOT GO plain plug, minor diameter | Largest permitted minor diameter | Does not enter | .250-20 UNC-3B NOT GO .2067 |
Notice what the markings say. The GO thread plug carries no class, because the smallest size of a Unified internal thread is the basic size for every class; one GO gage serves 1B, 2B and 3B. The HI plug and the NOT GO minor-diameter plug do carry a class, because the loose end of the tolerance differs from class to class. A receiving inspector who owns only a GO gage and a class 2B HI gage cannot accept a 3B hole.
Metric threads follow the same logic under ISO 1502, where the gage members are named GO and NOT GO and are made for a tolerance class such as 6H. The class designations themselves come from ISO 965-1 for metric threads and ASME B1.1 for Unified threads.
What gage tolerance class and calibration should you ask for?
Thread gages that check the product directly are normally made to X tolerance, and the setting plugs used to set ring gages to W tolerance. Plain plugs are ordered by tolerance class, from XX, the tightest, to ZZ, the loosest.
| Size range (in) | XX | X | Y | Z | ZZ |
|---|---|---|---|---|---|
| 0.029 to 0.825 | 0.00002 | 0.00004 | 0.00007 | 0.00010 | 0.00020 |
| over 0.825 to 1.510 | 0.00003 | 0.00006 | 0.00009 | 0.00012 | 0.00024 |
| over 1.510 to 2.510 | 0.00004 | 0.00008 | 0.00012 | 0.00016 | 0.00032 |
| over 2.510 to 4.510 | 0.00005 | 0.00010 | 0.00015 | 0.00020 | 0.00040 |
Gage tolerance eats into product tolerance. At the GO limit the gage is made inside the product limits, so a gage at the edge of its own tolerance rejects a few parts that were technically good. That is intended: the standards protect assembly first. Buying tighter gage classes narrows that band but costs more, and on most commercial tapped holes the standard X class for thread plugs is the sensible default.
Calibration is the other half. A gage is only as good as the last time someone measured it against a traceable reference. NIST defines traceability as a result related to a reference “through a documented unbroken chain of calibrations” and puts the burden of proof on whoever provides the result (NIST). In purchasing terms, ask the supplier for the calibration record of each gage used on your parts, and keep your own receiving gages on a recall schedule. Thread gages wear most on the starting threads, and a worn GO plug quietly starts passing undersize holes.
Why can two gages disagree on the same tapped hole?
Because every gage has its own tolerance and wear, two legitimate gages can sit at opposite ends of the permitted band, and a hole close to a limit can pass one and fail the other. The standards accept this and say the producer and the user should agree on the gaging method in advance.
This is the most common source of disputes between a buyer in the US or Europe and a supplier in Vietnam, China or Mexico. The supplier gages the lot on its own set and ships; receiving inspection gages it on a different set and rejects a handful of holes. Both inspectors did their job. The fix is to decide beforehand whose gage governs, or to have a borderline part referred to a measured result.
Three habits prevent most of these arguments:
- Name the gaging system. ASME B1.3 sets out numbered gaging systems for dimensional acceptability, from attribute checks with GO and HI or LO gages up to systems that add measured thread elements. Stating the system on the drawing removes the guesswork.
- Correlate the gages. For a new part, have both sides check the same few sample parts and compare results before production starts.
- Agree a referee method. Decide in writing that a disputed hole is settled by a calibrated gage from a named source, or by measurement of the pitch diameter.
How does plating or anodizing change a thread gage result?
A coating adds material to the thread flanks, so a tapped hole that passed GO before finishing can fail GO after it. The Unified standard asks that finished internal threads not be below basic size after coating, which means the hole has to be cut larger before plating if a coating thickness is specified.
The federal handbook notes that it is hard to build up much coating on the flanks of internal threads, and it recommends a rule of thumb when a thickness is required: open the minimum limits of the minor and pitch diameters by six times the minimum coating thickness, and the maximum limits by four times, so that a GO plug of basic size still enters after coating. Anodizing adds a further wrinkle, because part of an anodic layer grows outward from the surface and part grows into it, so the change in size is only a fraction of the coating thickness.
For purchasing, the point is to say when the gage applies. “Thread gages apply after finish” tells the supplier to cut the hole to allow for the coating. If the hole is masked or plugged during plating, say that instead. The finish comparison guide covers how each coating builds up, and the surface finishing page lists the finishes that can be quoted with the part.
What thread acceptance wording should go on a drawing or purchase order?
State the thread designation with its class, the full-thread depth, the gaging system or gage set, and whether gaging applies before or after finish. With those four items, the supplier and your receiving inspector are checking the same thing.
A workable note for a Unified tapped hole reads like this:
- Callout. 1/4-20 UNC-2B, with the minimum full-thread depth for a blind hole.
- Acceptance. Gage per ASME B1.2 with GO and HI thread plugs and minor-diameter plugs, System 21 of ASME B1.3 unless otherwise agreed.
- Timing. Thread gages apply after surface finish.
- Referee. Disputed parts are settled with a calibrated gage set agreed in writing.
For a metric hole the same structure works with a callout such as M6x1-6H and gaging per ISO 1502.
Your own incoming check can then be short and repeatable: sample each lot, gage the threaded features with your own set, record the gage serial numbers with the result, and escalate only after a second gage confirms a reject. Threads on turned parts, such as ports and external threads on fittings, follow the same logic with ring gages; the CNC turning page describes that work.
The RFQ package guide covers the rest of what to send with a drawing. When your thread requirements are written down, send the package for a quote; the reply confirms how each threaded feature will be gaged.
Frequently asked
Is a HI gage the same as a NOT GO gage?
For thread plugs, yes in purpose. Older US documents called the minimum-material thread gages “Not go”; later editions renamed them HI for internal threads and LO for external threads. ISO 1502 still uses GO and NOT GO. Plain plugs for the minor diameter are still called GO and NOT GO in both systems.
Can a screw or a tap be used instead of a thread gage?
Not for acceptance. A screw is a product part with its own tolerance, so it can pass a hole that a GO gage would reject or fail one that is good. A tap is sized to cut, not to check. Use them to troubleshoot, and a calibrated gage to decide.
The GO gage only goes partway into a blind hole. Is that a reject?
Compare against the full-thread depth on the drawing. If the gage stops short of that depth, the hole fails, whether the cause is a chip, a short tap stroke or a drill that did not go deep enough. If the drawing gives no depth, ask for one; without it the check has no limit.
Do thread gages check thread position or perpendicularity?
No. Go/no-go plugs check size only. Position of a threaded hole is checked separately, usually with a thread-locating plug or a pin in the thread and a measurement to datums.
Should I send my own gages to an overseas supplier?
It is a common way to remove disagreement: both sides then gage with one set, or with a matched set checked against the same masters. At minimum, agree the gage standard, tolerance class and referee method before the first lot ships.
Sources
- NBS Handbook H28, Screw-Thread Standards for Federal Services, Part I (Section 6, gages and gaging; Section 2, coated threads), National Bureau of Standards, 1969
- ASME B1.2, Gages and Gaging for Unified Inch Screw Threads, ASME, 2025 edition
- ASME B1.1, Unified Inch Screw Threads (UN, UNR and UNJ Thread Forms), ASME, 2024 edition
- ASME B1.3, Screw Thread Gaging Systems for Acceptability: Inch and Metric Screw Threads, ASME, 2007 edition
- ISO 1502, ISO general-purpose metric screw threads — Gauges and gauging, ISO, 1996
- ISO 965-1, ISO general purpose metric screw threads — Tolerances — Part 1: Principles and basic data, ISO, 2013
- Metrological traceability, NIST, accessed September 2026