Position is the most used geometric control. It says where a feature is: how far a hole’s axis may stray from its exact, theoretical location, measured from the datums. It replaces coordinate tolerances (the ± on x and y) with a true, usually round, tolerance zone, and it is the control that makes bolt patterns, dowel holes and bearing bores interchangeable. This page covers zone shapes, bonus tolerance, patterns, composite position, coaxial features, slots, projected zones, the fixed and floating fastener formulas, and worked examples. It is part of the GD&T guide and follows ASME Y14.5-2018.
What position controls
A position tolerance locates the axis (or center plane) of a feature of size, such as a hole, a pin, a slot or a tab, relative to a datum reference frame, by means of basic dimensions. The location is exact on the drawing (a boxed value with no tolerance of its own) and the permitted variation is stated entirely in the feature control frame.
- Basic dimensions give the true position from the datums, for example 25 and 40 in boxes. There are no ± values on them.
- The frame gives the symbol, the zone shape and size (⌀0.3), an optional material condition (Ⓜ), and the datums in order. Position without datums makes no sense: there would be nothing to locate from.
- Position controls orientation and form too, in a limited way. The zone has a fixed angle to the datums, so the axis cannot tilt more than the zone allows over the feature’s length. The feature’s size is still limited by its own size tolerance.
- It is a three-dimensional control. A cylindrical zone has a length (the length of the feature, or the projected height), so a hole must be in position along its whole depth, not just at the surface.
Zone shapes
| Zone | Written as | Used for |
|---|---|---|
| Cylinder ⌀t | One frame with ⌀ before the tolerance | Holes, pins, bosses: the axis can be off in any direction by the same amount |
| Two parallel planes t apart | One frame, no ⌀ | Slots, tabs, the center plane of a width; or a hole where only one direction matters |
| Rectangle (bi-directional) | Two frames, each with its own value and its own direction of datums | A feature that is critical in one direction (a pin that must align across a joint) and loose in the other |
| Sphere S⌀t | S⌀ before the tolerance | A point in three dimensions: a spherical joint center, a probe point |
| Cylinder around a datum axis | ⌀ with the datum axis only | Coaxial features (see below) |
A round zone is more generous than the old ± square: a ±0.05 square zone has a worst-case corner at 0.0707 from the center, and a round position tolerance of ⌀0.141 includes the whole square while allowing 57% more area. Parts that sit in the corners of the square zone but are within the round zone still work, and the round zone is what a gage pin, which is round, actually checks.
Actual position (⌀) = 2 × √( Δx² + Δy² )
RFS, MMC and LMC
The tolerance applies regardless of feature size (RFS) unless a modifier says otherwise. With Ⓜ the tolerance grows as the feature departs from its maximum material condition; with Ⓛ it grows as the feature departs from its least material condition. The extra amount is the bonus tolerance. The full treatment, with virtual and resultant condition and the zone charts for all three, is on the Modifiers and Material Conditions page. In short:
Total tolerance at MMC = stated tolerance + (actual size − MMC size) for a hole; + (MMC size − actual size) for a pin
- Ⓜ for clearance fits that only need to assemble: bolt holes, locating pins with clearance, anything that is gaged with a fixed pin.
- RFS for features that must be precisely located at every size: press fits, bearing seats, features that guide motion.
- Ⓛ to protect a minimum wall or edge distance (see the modifiers page).
Patterns of features
A group of identical features is toleranced together: 4 × ⌀8.4–8.6 above one position frame. The frame applies to all four holes as a pattern: their zones are fixed in position relative to each other and to the datums, so the holes can be inspected by a single gage plate with four pins.
- One frame, one pattern. The zones keep their exact spacing (given by basic dimensions); each hole has to lie in its own zone.
- Several patterns with the same datums in the same order and with the same modifiers are treated as a single pattern (a simultaneous requirement) in ASME Y14.5, unless the drawing says SEP REQT (separate requirements). This keeps related patterns, for example the holes on two faces, in step with each other when measured from the same datums.
- Different datums or modifiers make them separate requirements, and each is checked in its own set-up.
- The ‘X’ note. “4X” in front of the size says the requirement applies to four features; the frame itself is written once.
Composite position
Sometimes the location of a pattern on a part does not need to be exact, but the holes within the pattern must line up very precisely with each other and with what they mate to. A composite position frame has two rows that share one symbol and gives two requirements:
| Row | Name | What it controls | Datums |
|---|---|---|---|
| Upper | Pattern-locating tolerance zone framework (PLTZF) | Where the pattern is on the part, relative to the datum reference frame; also its orientation. This is the large tolerance. | Full datum reference frame: location and orientation |
| Lower | Feature-relating tolerance zone framework (FRTZF) | How the features relate to each other (spacing) and their orientation to the datums named. A much smaller tolerance. | Usually only the primary (and sometimes secondary) datum: orientation only, not location |
- The lower value must be smaller than the upper. Each lower zone framework may float inside the upper zones (shifting and, if the lower row has only datum A, rotating about it).
- Composite is not the same as two stacked frames. In two separate single-segment frames (one directly above the other, each with its own symbol), both rows locate the pattern from the datums, so the lower row is a refinement of location. In a composite frame, the lower row does not locate the pattern; it only relates the holes to each other and to the orientation datums.
- Use it for hole patterns on a mounting face where the part may be positioned loosely on the machine but the holes must still fit a mating pattern precisely, for example a pump flange or a motor mount.
Coaxial features
To make two diameters share an axis, give one of them as a datum feature and position the other to its axis. The zone is a cylinder ⌀t coaxial with the datum axis, and the controlled feature’s own axis must lie in it:
- Position of a coaxial feature: | | ⌀0.05 | A | where A is the datum axis (a bearing journal or a bore). The position can use RFS (precision seats) or Ⓜ (clearance fits).
- Versus runout. A runout tolerance also works from the same axis, but reads the surface and so includes the surface’s own out-of-roundness; position controls the axis. Runout is easier to inspect (a dial indicator), position is more precise about what matters (the axis). See Profile and Runout.
- Position replaces concentricity. ASME Y14.5-2018 removed concentricity and symmetry (below). A coaxial position tolerance, a runout tolerance or a profile tolerance covers every use of them.
- A common datum such as A-B (two journals) makes the best reference for a shaft: the axis through both bearings.
Slots, tabs and widths
For a width feature (a slot or tab) there is no single axis, so position controls the center plane. The zone is two parallel planes t apart, symmetric about the true center plane, and the frame has no ⌀. The frame is attached to the size dimension of the width.
- Slot 10 +0.2/0, position 0.3 Ⓜ to A and B: the center plane may be off by 0.15 each way at MMC (the narrowest slot, 10.0), and by 0.25 each way when the slot is at its widest (10.2), because the bonus is 0.2.
- A key and keyway use the same approach: the keyway’s center plane is positioned to the shaft’s axis.
- Each direction needs its own control. A square or rectangular pocket usually needs position in both directions, with a frame for each.
Projected tolerance zones
A position zone normally runs along the length of the feature. For a tapped hole or a press-fit pin, what matters is where the bolt or pin is above the surface, in the mating part, not where the thread is inside. The projected tolerance zone modifier Ⓟ moves the zone to start at the surface and extend upward by a stated height P (the thickness of the mating part, or the length of the pin that sticks out).
- Written as Ⓟ after the tolerance, with the projection height under the frame: Ⓟ 12.
- The effect of a tilt: a tilt of angle θ moves the axis by P × tan θ at the projected height. For θ = 1° and P = 12 mm that is 12 × 0.01746 = 0.21 mm, even though inside a 2 mm thread the same tilt moves the axis by only 0.035.
- The rule of thumb: use Ⓟ on threaded holes, press-fit holes and locating pins whenever the part that is attached stands off the surface.
- Projected zones and Ⓜ go together: for a clearance bolt pattern use the fixed-fastener formula below with Ⓟ on the threaded part.
Fixed and floating fasteners
The position tolerances of a bolted joint can be calculated so that the parts always assemble, with every hole at its worst case. Two cases:
| Case | Meaning | Formula |
|---|---|---|
| Floating fastener | Bolts pass through clearance holes in both parts and are held by nuts. Each hole has its own clearance, so each part gets the full tolerance. | T = H − F (per part) |
| Fixed fastener | The fastener is fixed in one part (a tapped hole, a press-fit stud). Both parts share the clearance. | T₁ + T₂ = H − F (equal split: T = (H − F) ÷ 2) |
H is the clearance hole at MMC (its smallest size), F the fastener at MMC (its largest size), and T the position tolerance (diameter, at MMC). The table gives values for metric screws with the ISO 273 close and medium clearance holes (taking the listed size as the smallest hole):
| Screw | F (max) | Close hole H | Floating T | Fixed, each | Medium hole H | Floating T | Fixed, each |
|---|---|---|---|---|---|---|---|
| M3 | 3.0 | 3.2 | 0.2 | 0.10 | 3.4 | 0.4 | 0.20 |
| M4 | 4.0 | 4.3 | 0.3 | 0.15 | 4.5 | 0.5 | 0.25 |
| M5 | 5.0 | 5.3 | 0.3 | 0.15 | 5.5 | 0.5 | 0.25 |
| M6 | 6.0 | 6.4 | 0.4 | 0.20 | 6.6 | 0.6 | 0.30 |
| M8 | 8.0 | 8.4 | 0.4 | 0.20 | 9.0 | 1.0 | 0.50 |
| M10 | 10.0 | 10.5 | 0.5 | 0.25 | 11.0 | 1.0 | 0.50 |
| M12 | 12.0 | 13.0 | 1.0 | 0.50 | 13.5 | 1.5 | 0.75 |
These are the largest tolerances that still guarantee assembly. Use smaller values where the process can hold them, and always add Ⓜ on the holes, so the bonus is available. For the threaded part of a fixed joint add Ⓟ, otherwise the tilt of the thread eats into the clearance above the surface.
Concentricity and symmetry
Concentricity controlled how far the median points of a feature’s cross-sections strayed from a datum axis, and symmetry did the same for the median points of two opposite surfaces from a datum center plane. Both were removed in ASME Y14.5-2018 because the median points are almost impossible to measure directly, so the controls were costly and hard to verify. ISO 1101 still has them.
| Instead of… | Use | Why |
|---|---|---|
| Concentricity of a diameter to an axis | Position (⌀t to the datum axis), or runout if the surface is round | Position controls the axis; runout is easy to inspect and includes the surface form |
| Symmetry of a width about a plane | Position (two planes) or profile | The center plane is derived from the whole feature, which a CMM can fit |
| Balancing a rotating part | Total runout or a balancing specification | Runout controls the actual wobble that causes imbalance |
Worked examples
Example 1: a hole position with bonus tolerance
A hole is drawn ⌀8.4 to 8.6 with a position of ⌀0.2 Ⓜ to A, B and C. Inspection finds the hole at ⌀8.55, with its axis 0.07 off in x and 0.10 off in y.
- Actual position = 2 × √(0.07² + -0.10²) = ⌀0.244.
- MMC of a hole is its smallest size, 8.4. Bonus = 8.55 − 8.4 = 0.15.
- Allowed position = 0.2 + 0.15 = ⌀0.35.
- 0.244 is less than 0.35: the hole passes. Without Ⓜ the limit would have been a fixed ⌀0.2 and the same hole would have been rejected, although a bolt goes through it easily.
Example 2: the functional gage for a bolt pattern
Four holes ⌀8.4 to 8.6 are located by a position of ⌀0.3 Ⓜ to A and B on a 50 × 50 square. A fixed gage plate is made with four pins at the exact basic positions.
- Virtual condition of each hole = MMC − tolerance = 8.4 − 0.3 = ⌀8.1.
- So the gage pins are ⌀8.1 (made a little larger or smaller within the gage tolerance, in the direction that never accepts a bad part) and stand at 50 × 50 basic, square to the datum surface.
- The part passes if it sits on datum A, is pushed against B, and drops over all four pins. That one test proves every hole is in position at its actual size, automatically including the bonus.
- A hole at ⌀8.6 (the biggest) has a total tolerance of 0.3 + 0.2 = ⌀0.5, and the pin test accepts exactly that.
Example 3: composite position of a flange pattern
Four holes ⌀6.4 to 6.6 on a mounting plate have a composite position: upper ⌀0.5 Ⓜ to A, B, C; lower ⌀0.1 Ⓜ to A.
- Upper segment. The hole pattern as a whole may be up to ⌀0.5 from where the datums say (0.25 off-center in any direction), at MMC (6.4), plus bonus at larger hole sizes.
- Lower segment. The holes must hold their spacing to each other, and stand square to A, within ⌀0.1 at MMC.
- A reading: the pattern is found shifted 0.18 in x and 0.12 in y (radially 0.216, a ⌀0.43 position error), and the holes’ spacing from the average pattern is within ⌀0.07. Both are inside their segments: ⌀0.43 < ⌀0.5 and ⌀0.07 < ⌀0.1, so the part passes.
- Had it been a single ⌀0.5 for everything, the holes could have drifted 0.5 apart from each other. The lower row is what makes the pattern fit the mating pattern.
Example 4: coaxial position, and the equivalent runout
A bearing seat ⌀35 must be coaxial with datum axis A (the shaft’s main journal) to ⌀0.04 RFS. An axis offset of e in any direction makes the surface’s indicator reading change by 2e per turn, so on a perfectly round surface the position tolerance corresponds to a circular runout of the same value: position ⌀0.04 ≈ circular runout 0.04. A real surface that is slightly out of round adds to the runout reading, so the runout is the stricter test.
Example 5: bolts for a bracket
M6 screws go through a bracket (clearance holes) into a threaded base (fixed fastener). The bracket holes are ⌀6.6 at MMC (medium fit).
- H − F = 6.6 − 6.0 = 0.6 to share between the two parts.
- Equal split: ⌀0.3 Ⓜ position on the bracket holes, ⌀0.3 Ⓜ Ⓟ on the tapped holes.
- If the bracket is made by laser cutting and is accurate to ⌀0.1, give the threaded part more: T₂ = 0.6 − 0.1 = ⌀0.5.
- Check: the bracket hole’s virtual condition is 6.6 − 0.3 = 6.3, and the screw’s worst-case boundary above the threaded part is 6.0 + 0.3 = 6.3. They are equal, so the worst parts only just assemble, which is exactly what the formula guarantees.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Parts assemble but fail position inspection | Ⓜ is missing on a clearance fit, so no bonus is allowed | Add Ⓜ where more clearance really is available; check the drawing’s intent |
| Bolts will not go in although every hole is “in position” | Tolerances exceed the fastener formula, or Ⓟ is missing on the threaded part | Recalculate T from H − F; add Ⓟ to tapped holes |
| Pattern fits the gage but not the mating part | The mating part is located from different datums than the gage | Use the datums the assembly really uses; consider a composite frame |
| Inspection results differ between labs | Datum feature simulators or fitting algorithms differ on the CMM | Agree the alignment; simulate datums as the standard describes |
| A tight position tolerance is costly | The tolerance is tighter than the function needs | Apply the fastener formula; use Ⓜ; use composite position to relax the overall location |
| Slot passes but its walls are not parallel | Position of the center plane does not limit each wall | Add parallelism or profile to the walls, or control the width with a size tolerance |
Related
- GD&T: the overview and quick reference.
- Datums and Datum Reference Frames: the references that position is measured from.
- Orientation Tolerances: controls that limit tilt only.
- Modifiers and Material Conditions: MMC, LMC, virtual and resultant condition and projected zones in full.
- Inspection and Tolerance Stack-up: gages, CMMs and stack-ups using position.
- Tap Drill Size and Thread Pitch Lookup and Bolt Torque and Thread Engagement Tool.
FAQ
Why is the position zone usually round?
The axis of a hole can be off in any direction, and a part works just as well whichever way it is off, so the natural zone is a circle (a cylinder in 3D). Use a rectangular or two-plane zone only when the function really differs by direction.
What is the difference between position and coordinate (±) tolerancing?
Coordinates give a square zone and a different result depending on which dimensions you chain, and they cannot use bonus tolerance. Position gives a circular zone, measured from the datums in one step, and can use bonus tolerance, so parts that work are not rejected for being in a corner of a square.
Does position control size?
No. The feature’s size is controlled by its size tolerance. With Ⓜ or Ⓛ the position tolerance changes with the size, but the size limits still apply.
Can I put position on a surface?
No. Position applies to features of size (axes and center planes). For a surface use profile, and for a feature’s surface relative to a datum axis use runout or profile.
When should I use a composite frame instead of two single frames?
Use composite when the pattern’s location on the part is loose but its internal geometry is tight. Use two single frames when both rows have to locate the pattern from the full datum reference frame, with the lower row a tighter refinement of location.
What does “4X” mean?
It says the requirement applies to four features of the same kind. It repeats size and position for all of them without drawing four separate frames.
What is the bonus tolerance if I use Ⓜ on a pin and the pin is small?
For a pin, MMC is the largest size, so the bonus is MMC size − actual size: a pin made smaller than its largest size gets extra position tolerance equal to the amount it is undersize.
References
- ASME Y14.5-2018, Dimensioning and Tolerancing (position, composite position, projected tolerance zone and the fixed and floating fastener formulas in the non-mandatory appendix).
- ASME Y14.5.1M, Mathematical Definition of Dimensioning and Tolerancing Principles.
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures.
- ISO 1101 (position, concentricity and symmetry) and ISO 2692 (maximum and least material requirements, MMR and LMR).
- ISO 273, Fasteners: Clearance holes for bolts and screws.
- Krulikowski, A., Fundamentals of Geometric Dimensioning and Tolerancing, Cengage.
Last reviewed: October 2026. Formulas guarantee assembly only for the cases stated; check the standard your drawing names.