Short answer: Use position tolerance (ASME Y14.5 or ISO 1101) whenever the location of a feature of size matters for function. Typical cases are hole patterns for bolts, pins and mating parts. ± coordinate tolerances give a square zone with no defined datums, so different inspectors can measure the same part differently. Position gives a cylindrical zone tied to an explicit datum reference frame, and with an MMC modifier it can add bonus tolerance as the hole departs from its smallest size.
The problem with ± location
Say a hole is located at 50 ± 0.1 in X and 30 ± 0.1 in Y.
- The zone is square (0.2 × 0.2). A hole at the corner of the square is about 0.14 from nominal along the diagonal, but a hole the same distance away along an axis is rejected. Function, such as a bolt fitting, depends on radial distance, so the square zone is arbitrary.
- The origin is ambiguous. The drawing doesn't say which surfaces to measure from, or in what order to contact them. Two inspectors can get different answers.
- Tolerances can stack up. Chained ± dimensions between holes add up in ways the designer may not intend.
What position does instead
A position callout has three parts:
1. Basic dimensions (shown boxed) give the exact theoretical location. They carry no tolerance of their own.
2. A feature control frame gives the position symbol, a diameter symbol (for a cylindrical zone), the tolerance value, an optional material condition modifier, and the datums.
3. A datum reference frame (for example A|B|C) tells everyone how to fix the part: primary, secondary and tertiary contact.
With MMC (Ⓜ), the stated tolerance applies when the hole is at its smallest size. As the hole gets larger, the extra size is added to the position tolerance as bonus. This matches the physics of assembly: a larger hole can be further off and still clear a bolt.
Steps to convert a ± hole pattern
1. Pick datums based on function. The primary datum is usually the mounting face. Secondary and tertiary are usually edges or features that locate the part in the assembly.
2. Replace the location dimensions with basic dimensions from the datums, or between holes in the pattern.
3. Choose a cylindrical zone (⌀) for the holes and select MMC if the function is clearance assembly.
4. Size the tolerance with the fixed or floating fastener formula. In the ASME Y14.5 appendix approach for floating fasteners, the position tolerance at MMC is T = H − F, where H is the hole MMC size and F is the fastener MMC size. For fixed fasteners (threaded holes), T is shared between the two parts.
5. Check how it will be inspected. CMM or a functional gauge at virtual condition both work naturally with MMC position.
Worked example
A cover plate has four clearance holes for M6 screws that thread into a base. (This is a floating fastener case for the cover only if both parts have clearance holes. Here, the base is tapped, so it is a fixed fastener case.)
- Clearance hole: ⌀6.4 to 6.6. The MMC is 6.4.
- The screw major diameter MMC is about 6.0. Use the actual value from your fastener standard.
- The total available at MMC is 6.4 − 6.0 = 0.4. For a fixed fastener, the designer splits it between the cover holes and the tapped holes, for example ⌀0.2 each. A projected tolerance zone on the tapped holes is worth considering.
- Cover callout: ⌀0.2 Ⓜ | A | B | C, where A is the mating face and B and C are two edges.
- If a cover hole is produced at ⌀6.55, the bonus is 6.55 − 6.4 = 0.15. The allowed position tolerance for that hole is therefore ⌀0.35.
Compare that with ±0.1 in X and Y, which gives a fixed square zone with no bonus. This rejects some parts that would assemble and accepts some corner cases that are borderline.
Common mistakes
- No datums, or datums that don't reflect how the part mounts.
- Tolerancing basic dimensions. They must be boxed and untoleranced. The tolerance lives in the frame.
- Leaving out ⌀ when a cylindrical zone is intended, which makes the zone two parallel planes instead.
- Using MMC on features where bonus would hurt function, for example a precision pin location that controls alignment, not clearance.
- Ignoring projected tolerance zones on threaded or press-fit holes, where perpendicularity error moves the mating part.
- Mixing ± and position for the same feature, which creates conflicting requirements.
FAQ
Is position the same in ASME and ISO?
The concept is the same. Default rules differ. For example, ASME Y14.5 Rule #1 (envelope) is not the ISO 8015 default. State which standard governs on the drawing.
Can I use position on a slot?
Yes. Use a non-diameter (width) zone, with the boundary concept described in Y14.5.
Does RFS still exist?
In current ASME Y14.5, regardless of feature size is the default when no modifier is shown.
Do I always need three datums?
Only as many as needed to constrain the degrees of freedom that matter for that feature.