× Datum target point
Datum target point · Datums y referencias · ISO 1101 + ASME Y14.5
Example in plan
How to interpret it
On the drawing, “⊙ A1 — point target ✕ located with basic dimensions” states a datum target point requirement. The point target is embodied by a spherical contact locator: it touches at a single point, so it does not impose orientation by itself and needs companions to lock degrees of freedom. The classic scheme is 3-2-1: three points define the primary datum (the seating plane), two the secondary (direction) and one the tertiary (the final stop). The farther apart the three primary points are, the more stable the part; if they are close together, the part rocks and the measurement does not repeat. Targets are always located with basic dimensions from the datum reference frame, never with toleranced dimensions..
What controls
Defines the datum by contact at a specific, dimensioned point on the surface rather than by the entire surface. It is drawn with an X on the face and a divided circular symbol carrying the datum letter and target number (A1, A2, A3), and its location is fixed with basic dimensions. It is used when the surface is too irregular or too large for full-surface contact to be repeatable: castings, forgings, sheet metal, weldments. What it does NOT mean is that only that area needs to be within tolerance, or that the rest of the face can do as it pleases: what it defines is where the part is supported for measuring and machining, that is, where everything else is measured from.
How to verify
The locator is embodied by a spherical or rounded-tip pin, mounted in the fixture at the target's basic coordinate and at a known height. On a CMM without a fixture, one point is probed at each target location and the datum is built from those points: three for the primary plane, two for the secondary, one for the tertiary. What must not be done is to probe the entire face and fit a least-squares plane, because that measures the whole surface and gives a different result. Before accepting the setup, check that the part seats on all three points and does not rock on two.
Datums and notes
The point target is embodied by a spherical contact locator: it touches at a single point, so it does not impose orientation by itself and needs companions to lock degrees of freedom. The classic scheme is 3-2-1: three points define the primary datum (the seating plane), two the secondary (direction) and one the tertiary (the final stop). The farther apart the three primary points are, the more stable the part; if they are close together, the part rocks and the measurement does not repeat. Targets are always located with basic dimensions from the datum reference frame, never with toleranced dimensions.
Common mistakes when interpreting it
- Resting the part on the entire face instead of the indicated points, so the datum is no longer the one on the drawing.
- Probing the complete surface on the CMM and fitting a plane: with targets the datum must be built only from the indicated points.
- Using one locating scheme in machining and a different one in inspection, which is the most frequent cause of discrepancies between the shop and metrology.
How to get it in the workshop / if it comes out of tolerance
It is shown with a cross in a circle and the area size where applicable. It simulates contact at a physical point. For the shop, the targets are the fixture drawing: they say where to put the locators, and the same scheme must be used on the machine and in inspection. If the machining fixture locates on some points and the inspection fixture on others, the part will give different results without anything having changed. Protect those areas: no burrs, no scale, no shot blasting that leaves them uneven.
If the part rocks, first check cleanliness and burrs at the contact areas and then the distribution of the points: too close together or poorly spread and the part never seats the same way twice. If measurements do not repeat between shifts, suspect the locator (wear or play in the pin) before the machine. And if a locating point falls on an area that is machined in a later operation, the datum disappears partway through the sequence: the order of operations must be rethought or design asked to relocate the target.
Related symbols
Other symbols in Datums and references
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.