Quick Answer
GD&T vs plus/minus tolerance is not a contest between old and new practice. Plus/minus limits give each dimension its own band, so the permitted area is a rectangle on a two-axis feature and a box in three dimensions. A geometric control attaches one tolerance zone to a feature and ties it to datums, so the zone can be cylindrical, a pair of parallel planes, or a profile band. Use plus/minus where a dimension stands alone; use GD&T where a feature has to work relative to another.
Key Takeaways
- The zone shape decides usable tolerance: a ± pair builds a rectangle, a position callout with a diameter symbol builds a circle.
- ±0.1 mm on two axes permits 0.141 mm of radial error at the corner — wider than the printed number suggests.
- Geometric controls separate size from form, orientation and location, so a mating requirement holds without tightening the size band.
- MMC modifiers apply only to features of size and pay off when inspection can verify the departure.
- Neither system is tighter by definition; the tighter one is whichever matches the function and can be inspected at sensible cost.
GD&T vs Plus/Minus Tolerance: What Each System Controls
A plus/minus tolerance sets two limits around a nominal value, measured between opposing points or planes, so it describes size along one axis only. Two ± dimensions on a hole's X and Y do locate the axis, but as independent constraints that say nothing about assembly clearance.
A feature control frame states the characteristic, the shape and size of the zone, and the datums it is measured from. That block can control an axis, a median plane or a whole surface as one entity; the position tolerance guide for hole patterns covers the syntax.
Plus/minus answers how big a feature is; GD&T answers how well it is placed and oriented relative to other features. A ± chain from edge to edge also accumulates, while a datum-referenced positional control keeps each feature's error local — worth a tolerance stack-up analysis before release.
Why a Square Zone Costs More Than It Looks
Take a hole pattern with ±0.1 mm on both axes. The permitted zone is a 0.2 by 0.2 mm square, and a hole at the corner sits 0.141 mm from true position — 41% further out than either printed limit suggests. If the mating part needs the axis within 0.1 mm radially, the square has to shrink until its corners fall inside that circle: ±0.07 mm per axis. Nothing about the function moved, yet both axes now carry a band 30% tighter, paid for with an extra finishing pass, closer probing and more scrap risk.
The trade runs the other way too. A Ø0.2 mm position zone covers 0.0314 mm² against 0.0196 mm² for the inscribed ±0.07 square, roughly 60% more acceptable parts for the same function. That arithmetic is why a geometric control is often looser rather than tighter where the requirement is genuinely radial.
Where Plus/Minus Is Still the Right Call
Plus/minus is the right tool for dimensions with no relationship to protect. Overall length, wall thickness, step depth and chamfer size each describe one feature in isolation. A feature control frame on them adds inspection cost without changing one accept-or-reject decision.
Fits taken from a standard limits-and-fits table behave the same way. When a shaft and bore are chosen as a catalogued clearance or interference fit, the table already encodes the intent, and a symmetric ± on the nominal diameter is the conventional way to express it. Adding position on top creates conflict rather than clarity.
Blanket title-block tolerances are a third use: an "unless otherwise specified ±0.2 mm" line keeps the drawing readable. For asymmetric limits, see unilateral vs bilateral tolerance.
Where GD&T Earns the Extra Effort
Geometric controls pay for themselves when one feature's job is defined by another. Three cases cover most of it.
Mating hole patterns. A bracket bolts to a housing only if the pattern is located from the datums the assembly uses. Position at MMC, checked with a functional gauge, tests the assembly condition directly.
Coaxial bores. Two bores on opposite walls have to share an axis before a shaft seats. Neither diameter's ± limits say anything about that alignment; a position or runout control does.
What a process can hold depends on material, geometry, workholding, process route and inspection requirements, so a geometric callout is a requirement to review against the route. A functional control is usually easier to meet than a tightened ± band, as the profile tolerance callout article shows.
Common Mistakes When the Two Systems Collide
Double-dimensioning a pattern. A center-to-center ± chain plus a position callout puts two controls on one requirement. The tighter one governs, inspectors may report either, and the drawing invites argument at the dock.
Using MMC where it cannot apply. The modifier is legal only on a feature of size. Attaching it to a surface produces a callout that cannot be verified.
Choosing position for a surface. Position locates an axis or center plane; a surface that must lie within a band needs profile, and swapping the two changes what the report means.
Assuming GD&T costs more. A cylindrical zone often accepts more parts than the equivalent ± box, so the geometric version can lower scrap. The added cost is engineering and inspection time.
FAQ
Does GD&T mean tighter tolerances?
No. A cylindrical position zone carries about 60% more area than the equivalent ± square, so a geometric callout can accept parts a ± callout would reject. What changes is where the constraint sits.
Can plus/minus and GD&T share a drawing?
Yes, and most production drawings do exactly that. The rule is one control per requirement: dimensions that stand alone get ±, features that must relate get a control frame.
How is a position tolerance checked without a CMM?
A functional gauge built to the virtual condition boundary accepts any pattern that will assemble. Plates, height gauges and dial indicators cover simpler controls, provided the setup matches the datum scheme. That is the practical test of GD&T vs plus/minus tolerance: the method has to match the callout.