Ordinate dimensioning, baseline or chain: which scheme keeps tolerance buildup off your part?

How much tolerance buildup does each dimensioning scheme create?

Between two features, chain dimensioning allows the sum of every link tolerance in between, baseline and ordinate dimensioning allow the sum of just two tolerances, and a direct dimension allows only its own tolerance. Which scheme is “tighter” depends entirely on which pair of features you care about.

ASME Y14.5 states the rule plainly in its section on tolerance accumulation: chain dimensioning gives the greatest accumulation between the end features, baseline dimensioning reduces the maximum variation between two features to the sum of the tolerances on the two dimensions from the origin, and direct dimensioning gives the least variation, equal to the tolerance on that one dimension. The table runs that rule on a simple part: a row of five holes on a common pitch, measured from a machined edge called datum A, with every untoleranced dimension taking the general tolerance from a title block note citing ISO 2768-m.

Three things stand out. First, the chain drawing is the best of the plus/minus layouts for the adjacent pair and the worst for everything else; the distance from the edge to the last hole carries five link tolerances. Second, baseline and ordinate are identical in tolerance meaning. Ordinate is a drafting convenience, not a tighter scheme, and the adjacent pair is actually looser than under chain because it inherits two origin tolerances. Third, general tolerance tables are size-banded, so in an ordinate layout the features far from zero automatically pick up the looser band per ISO 2768-1, while a chain of short links stays in the tighter band but adds them up. The fourth row shows the price of a direct dimension: hole 1 to hole 5 tightens to one tolerance, but hole 5 is now located through hole 1, so its distance from the edge loosens to the sum of two.

None of this is visible on the print. Nobody wrote a stack-up; the scheme made one. Once you know which distance is functional, you can either draw that distance directly or move the pattern onto basic dimensions, which is the last row and the subject of a later section.

Why do CNC shops find ordinate drawings easier, and where can that go wrong?

A CNC program positions every feature as an absolute coordinate from a work zero, so an ordinate or baseline drawing maps directly onto the program and onto the inspection report. A chain drawing has to be converted to coordinates first, and that conversion is where the drawing’s tolerance intent can be lost.

When a programmer turns a chain of links into coordinates, the machine positions each hole from the work zero, not from the previous hole, so on the machine the errors do not actually accumulate the way the drawing allows. That sounds like a free gain, but it cuts both ways. The part is now made to an ordinate logic and inspected, if the report follows the drawing, to a chain logic. Each link is measured from the feature before it, and a small offset in one hole shows up twice: once making its upstream link long and once making its downstream link short. A part can pass in reality and fail on paper, or the other way round, depending on which method the inspector picks.

The second risk is the choice of zero. The programmer will put the work zero on whatever surface is convenient to pick up on the machine. If the drawing’s ordinate zero is a different surface, say a centerline or the opposite edge, every coordinate is re-referenced through one more measured distance, and that distance adds its own error to every feature. The fix is on the drawing: make the ordinate zero a real, accessible datum feature, label it, and use the same datum on every view.

The third risk shows up on cast and stamped blanks. A chain that starts from an as-cast face carries the casting’s variation into the first link and, through it, into the whole chain. Start machined dimensions from a machined datum, and tie that datum back to the casting with only one dimension. The guides on setting datums on cast parts and on separate casting and machining drawings cover how to choose it.

Which dimensioning mistakes create hidden stack-ups on a drawing?

Most hidden stacks come from mixing schemes without meaning to, and from origins that are not the functional datum. They are cheap to fix at the drawing stage and expensive to argue about after the first article.

• Two origins in one view. Half the holes dimensioned from the left edge, half from the right edge, and the critical pair split across the two groups. That pair now carries two tolerances plus the overall length tolerance between the edges.
• Ordinate zero on a centerline. A centerline cannot be touched by a probe or a height gauge; it is derived from two measured surfaces. Use it as an origin only if it is a defined datum (for example a datum axis from a bore) and say so.
• Closed loops. A chain with an overall dimension, or an ordinate layout where someone also added a direct dimension between two ordinates with its own tolerance. Each distance must be controlled by exactly one dimension; the others become reference.
• The functional distance is never drawn. The bearing bores that set gear center distance are each located from the edge, so the center distance is a derived result. Draw the center distance directly, or put both bores under one position tolerance.
• Chain across a second setup. On a turned or milled part, a chain that crosses from one setup to the next picks up the re-clamping error at the link that crosses over. Start each setup’s dimensions from a feature made in that setup, or control the relationship with a geometric tolerance to a datum.
• Unit conversion in a chain. Each converted and rounded link carries a little rounding error, and in a chain those errors add up just like tolerances do. Convert from the origin, not link by link.

If the part goes through an inspection report keyed to balloon numbers, every one of these shows up as a row that is hard to measure the way it is drawn. Walking the drawing as an inspector would, balloon by balloon, is a good final check; the ballooned drawing guide shows the method.