⟺ Translation
Translation · Modificadores de zona · ISO 1101
Example in plan
How to interpret it
On the drawing, “⌖ ⌀ 0.1 ⟺ |A|B|” states a translation requirement with a cylindrical tolerance zone of ⌀ 0.1 mm, measured from datums A, B in that order of precedence.
What controls
A modifier placed next to a datum letter to indicate that the datum orients the part but does not locate it: the simulator that establishes it can slide, and the tolerance zone with it, instead of being fixed at its theoretical location. It is used when the datum feature is a feature of size (a hole, a slot, a boss) whose exact location is not functional but whose direction is. The practical effect is that one translational degree of freedom is released when building the datum reference frame, while the rest remain constrained. What it is NOT: it does not increase the tolerance value, it does not allow the zone to move in any direction, and it does not make the datum optional. Both ISO and ASME include this idea of a datum reference that does not fix location, so the first thing to do is check which standard the drawing cites before interpreting the symbol.
How to verify
On a CMM, the alignment must leave the affected translational degree of freedom free and fit the part by best fit in that direction, instead of locking it at the theoretical datum coordinate: almost all software packages require that option to be enabled manually on the datum feature. With physical fixtures, the element simulating the datum has to be mounted on a guide or slide, not bolted in a fixed position. If the result with and without translation is the same, suspect that the software ignored it: normally the criterion with translation is equal or more permissive, never stricter.
Common mistakes when interpreting it
- Confusing translation with extra tolerance: the zone does not grow; it just stops being anchored in one direction.
- Fitting a fixed pin in the fixture for a datum with translation, which imposes a location constraint the drawing does not require.
- Applying translation on your own because the parts don't pass, when the drawing does not specify it.
How to get it in the workshop / if it comes out of tolerance
For the person making the part, translating it is simple: that datum governs how the part is oriented, not where things sit relative to it, so don't chase the location dimension of the datum feature. For the person inspecting it, the setup changes: the locator or pin representing that datum must be able to slide in the fixture, not be fixed at its coordinate. If it is not indicated on the drawing, never assume it: without the modifier, the datum does fix location.
If parts are rejected for position and the frame carries the translation modifier, first check that the evaluation actually applied it; this is the most common failure and it gets fixed in the report, not on the machine. If the rejection is real, correct what that datum does control: orientation, meaning squareness of the setup, perpendicularity of the datum feature and repeatability of the fixturing. And don't waste time fine-tuning the location of the datum feature, because the drawing has expressly stated that location is not being controlled.
Related symbols
Other symbols in Zone modifiers
Related tools
ISO fits
Calculates indicative ISO 286 tolerances for shaft and hole, H7/g6, H7/h6, H7/k6 and H7/p6 fits with clearance, transition and interference graph.
Inspection Plans
Upload a plan, extract dimensions and GD&T with AI and export your inspection guideline in PDF or CSV.
Shop trigonometry
Workshop trigonometry: right triangle, C chamfer, Z countersink, sine bar, taper and polar→X/Y for CNC operators.