Guide
How should you set position tolerance on threaded holes, and when do you need a projected tolerance zone?
Position tolerance is the geometric control that limits how far the axis of a feature may sit from its true, theoretically exact location relative to a datum reference frame. On a tapped hole the controlled axis is, by default, the axis of the thread’s pitch cylinder, and the question engineers usually get wrong is not how big the tolerance should be but where along that axis it is checked.
By Saola Manufacturing engineering team · Published · Updated
A tapped hole is unusual: the screw it holds continues upward through a mating part with only a plain clearance hole, so any tilt of the thread grows with distance. This guide covers how the fixed-fastener relationship splits tolerance between the two parts, why a projected tolerance zone solves the tilt problem, a worked example, and how inspectors measure the result.
On this page
What axis does a position tolerance on a threaded hole actually control?
Unless the drawing says otherwise, it controls the axis of the pitch cylinder, the imaginary cylinder that passes through the thread where ridge and groove are equally wide. ASME Y14.5 lets you override that default with the note MAJOR DIA or MINOR DIA, and ISO drawings use the modifiers MD or LD for the same purpose.
The pitch cylinder is where the flanks of screw and hole bear, so it is the axis the fastener follows. The federal screw-thread handbook defines the thread axis this way and, in the same passage, admits the catch: locating that axis accurately is relatively difficult, which is why gage makers often reference the minor diameter of an internal thread instead, provided it is round and concentric with the pitch cylinder (see NBS Handbook H28, paragraphs 5.2 and 7.2).
For a drawing, leave the default alone unless you have a reason, and expect inspection to approximate the pitch axis rather than probe it. A probe on the crests of a tapped hole reads the minor diameter, which on a cut thread in cast aluminum can be torn or offset; the practical answer, covered below, is to thread something into the hole and measure that.
How do you split position tolerance between a tapped hole and its clearance hole?
Use the fixed-fastener relationship from the nonmandatory appendix of ASME Y14.5: the positional tolerances of the tapped hole and the clearance hole, both at maximum material condition, may add up to no more than the clearance hole’s smallest size minus the fastener’s largest size. Split equally, each part gets half of that difference.
The reasoning is geometric. At maximum material condition the clearance hole is as small as it can be and the screw is as large as it can be, so the gap between them is the whole allowance for error. The screw is locked to the tapped hole, so any error in the tapped hole moves the screw; any error in the clearance hole moves the hole around the screw. Written as a relationship, H − F = T1 + T2, where H is the clearance hole at its smallest, F the fastener at its largest, T1 the clearance-hole tolerance and T2 the tapped-hole tolerance. That is the “fixed fastener” case. When both parts have clearance holes and a loose bolt and nut pass through them, the “floating fastener” case applies instead, and each part may use the full difference because neither hole drags the bolt with it.
An equal split is not compulsory. If a clearance hole in a stamped cover is harder to hold than a tapped hole machined in a housing, give more of the allowance to the stamping. What matters is that the sum stays within H − F and that both drawings apply the tolerance at MMC. The formula also assumes the tapped hole’s zone reaches as far as the fastener does, which by default it does not.
What is a projected tolerance zone, and why do tapped holes need one?
A projected tolerance zone moves the position tolerance zone out of the part and into the space the fastener will occupy, above the surface, for a height you specify. It is needed on tapped holes and press-fit holes because a small tilt inside the part becomes a large offset where the fastener passes through the mating part.
Without the projection, the zone is a cylinder the depth of the thread, and an axis may lean from one side of it to the other and still pass while the screw drifts further off at the lid. With the projection, the same cylinder is lifted to start at the mating surface and extend upward for the projected height, so the part is judged at the place where interference would actually happen. ISO set out the method as its own standard in ISO 10578:1992 (since withdrawn; the projected zone is now covered by ISO 1101:2017), whose introduction described the purpose as limiting extreme variation in the perpendicularity of threaded features and interference-fit holes. Cite ISO 1101 on new drawings, not ISO 10578.
On the drawing, the projected zone is shown by the letter P in a circle placed after the tolerance value in the feature control frame. Under ASME Y14.5-2018 the projected height may be written directly after that symbol, or shown with a chain line drawn beside the view and dimensioned. Either way, the zone starts at the surface the mating part sits on unless the drawing places it somewhere else.
How high should it be? Set it to the greatest thickness of whatever the fastener must pass through: the mating part at its maximum thickness, plus any washer, gasket or spacer in the stack. For a stud or a dowel, use the maximum length it stands above the surface.
How much tolerance do you lose if you leave the projection off?
You lose the more the thicker the mating part is compared with the thread engagement. When the mating part is as thick as the engagement is deep, the tapped hole’s allowable tolerance falls to about one third of the value the projected zone permits.
The loss can be worked out from the lean described above. If the tapped-hole axis may cross its zone from one side to the other over the engagement depth D, then at height P above the surface it can sit further off by a factor of 2P/D. An unprojected tolerance T2 therefore behaves, at the top of the mating part, like a projected tolerance of T2(1 + 2P/D). To keep the fastener clear, the relationship becomes H − F = T1 + T2(1 + 2P/D). The table applies both versions to a common inch case, a socket head cap screw in a tapped hole holding down a flat cover.
| Item | With projected zone | Without projected zone |
|---|---|---|
| Fastener, largest size F | 1/4-20 UNC, 0.250 in | 1/4-20 UNC, 0.250 in |
| Clearance hole, smallest size H | 0.281 in | 0.281 in |
| Total allowance H − F | 0.031 in | 0.031 in |
| Cover thickness P (maximum) | 0.375 in, used as projected height | 0.375 in |
| Thread engagement D (minimum) | 0.375 in | 0.375 in |
| Relationship used | H − F = T1 + T2 | H − F = T1 + T2(1 + 2P/D) = T1 + 3 T2 |
| Equal split, T1 = T2 | ⌀0.015 in each at MMC | ⌀0.007 in each at MMC (0.031 / 4, rounded down) |
| Tapped hole only, T1 fixed at ⌀0.015 | ⌀0.016 in (T2 = 0.031 − 0.015) | ⌀0.005 in (T2 = 0.016 / 3, rounded down) |
The last row is the one that matters on a real print. If the cover is already released, leaving the projection off forces the tapped hole down to about a third of the projected value. That is the argument for projecting every tapped hole that holds a mating part.
The ratio 2P/D grows quickly, so a short engagement in a soft casting under a thick plate is worse than the table shows. If cover and housing are drawn by different teams, record the projected height and both tolerances on the assembly drawing so the allowance is not spent twice.
How is a projected tolerance zone inspected on a CMM?
The usual method is to screw a thread pin, a close-fitting threaded gage pin with a precise plain shank, into each tapped hole and measure the shank rather than the thread. The CMM builds the pin’s axis from the shank and evaluates it only over the projected height above the datum surface.
A typical routine aligns the part to its datum reference frame, with the mating face as primary datum, runs a thread pin in until it seats on its flanks, probes circles on the shank near the surface and near the top of the projection, and reports the fitted axis within that band, not inside the hole.
Measurement error comes mostly from the pin’s fit in the thread. A standard tapped hole carries clearance on the pitch diameter, so a loose pin can rock and add apparent tilt. Inspectors reduce that by using pins with minimal pitch clearance, expanding or tapered thread pins that center on the flanks, or by snugging the pin against the surface in a consistent way. The method should be agreed before production, because two labs using different pins can report different numbers on the same hole. Gage requirements for the thread itself (go and no-go plugs) are set separately in ASME B1.2 for Unified inch threads and do not check location at all.
For volume work, a functional gage with pins or bushings at true position, sized to the virtual condition of the projected zone, gives a fast accept or reject answer once a CMM study has shown the process is stable.
What should the drawing tell an overseas supplier about tapped-hole position?
State the standard and edition, put the projected zone and its height in every relevant feature control frame, and say how you want the result reported. With those on the print, a shop in Vietnam or anywhere else can plan the inspection before it prices the part.
- Edition. “Dimensioning and tolerancing per ASME Y14.5-2018” or “per ISO 1101”. The symbol reads the same, but the default rules around it do not.
- Projection. The circled P and the height after it, sized to the thickest stack the fastener passes through. A bare position callout on a tapped hole is read as unprojected.
- Material condition. MMC if you used the fixed-fastener relationship; it is the assumption behind the subtraction.
- Datums. Make the mating face the primary datum, because that is the surface the projection starts from and the one the cover will sit on.
- Report format. Say whether you want CMM values for each hole at the projected height, a functional-gage result, or both, and at what sampling. It changes inspection time per part.
- Cast bosses. On a die casting, tapped holes are usually drilled and tapped in a secondary CNC milling setup located from machined datums, not from the as-cast surface. If the drawing locates the holes to cast features, say so and expect that question back.
For die-cast housings in particular, pair this with the die casting process notes and the tolerance standards guide, since the cast-to-machined relationship drives where the datums can sit. The RFQ package guide lists everything else to send. When the drawing is ready, send it for a quote; any position callout that needs a conversation is raised in the reply.
Frequently asked
Do through tapped holes need a projected zone too?
Yes, if a screw or stud from them passes through a mating part. The zone is projected from the face where the mating part sits, which may be either side of a through hole, so show which side on the drawing.
Can I use RFS instead of MMC on a tapped hole?
You can, but the fixed-fastener subtraction assumes MMC, and a tapped hole has a narrow pitch-diameter tolerance, so any bonus tolerance from MMC is small anyway. RFS mainly makes functional gaging impossible, since the gage cannot represent a fixed size.
Is a projected zone the same as a perpendicularity callout?
No. Perpendicularity limits tilt but not location. The projected position zone limits both at once, where they matter, which is why it usually replaces a separate perpendicularity callout on tapped holes.
Why not just tighten the tapped-hole tolerance instead?
Because it costs more and still leaves the requirement unstated. A tighter unprojected tolerance guards against tilt indirectly; a projected zone checks the condition that causes assembly trouble and usually allows a larger number.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024); source of the projected tolerance zone symbol, the pitch-diameter default for screw threads and the fixed-fastener appendix
- ISO 10578:1992, Technical drawings — Tolerancing of orientation and location — Projected tolerance zone, ISO, 1992 (withdrawn; now covered by ISO 1101:2017; public preview: introduction and scope)
- ISO 1101:2017, Geometrical product specifications (GPS) — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017
- Screw Thread Standards for Federal Services, Handbook H28, Part I, National Bureau of Standards, 1969 (paragraphs 5.2, 5.7 and 7.2)
- ASME B1.2, Gages and Gaging for Unified Inch Screw Threads, ASME, 2025 edition