A drawing is not a picture of the part.
It is the statement of what has to be true when the part is measured. Geometry tells us the shape. The dimension scheme tells us which of those shapes actually matter — and that is the part we build to.
Two drawings can describe the same formed bracket and produce different parts. Not because the model changed, but because the dimensions were taken from different places. One says this face must sit flat against the plate and these two holes must land on the bolt pattern. The other says every leg is 40 mm. Only the first one tells us what to protect when something has to give.
Something always has to give. Material arrives with a thickness range. Springback varies from coil to coil. The backgauge repositions between hits. A formed part is the accumulation of those effects, and the dimension scheme decides where they land.
Chained dimensions add their errors together.
If each dimension is measured from the previous feature rather than from a common origin, every band in the chain contributes to the last one. This is the single most common reason a part measures in-spec at every step and still does not fit.
Our published bands already show the effect. On sheet up to 3 mm, a single leg (A) is held to ±0.2 mm. The opposing flange (B) is ±0.4 mm. A span measured across two bends (C) is ±0.8 mm. The band roughly doubles each time the measurement crosses another bend, because each bend contributes its own angular and positional error.
Baseline dimensioning does not make the machine more accurate. It changes which errors are allowed to combine. The far leg still has its own band, but the hole no longer inherits it, because the hole is no longer measured through it.
The datum is the face the part is used from.
Not the corner of the flat pattern, and not whichever edge the CAD sketch happened to start on. The datum should be the surface that locates the part in the assembly, because that is the surface every other feature has to agree with.
For most formed parts the choice is obvious once the question is asked properly: which face touches something else? A bracket that bolts to a plate is located by its mounting face. An enclosure panel is located by the flange that meets the frame. Pick that face, mark it, and dimension the features that matter from it.
Where GD&T is appropriate, this is exactly what datum references formalise. If you are already using feature control frames, our GD&T guide covers the symbols. If you are not, plain baseline dimensioning from a labelled face achieves most of the benefit with none of the notation.
Tolerance the few things that matter. Release the rest.
A tight band is not free. It narrows the acceptable window, adds inspection, and can force an extra setting. Applying a blanket tight tolerance to every dimension on a drawing is the most reliable way to raise a price without improving a part.
The efficient drawing has a general tolerance block that covers everything ordinary, and a small number of specific callouts on the features that genuinely have to hold. That contrast is information: it tells us where to spend the attention.
An angle tolerance is a length tolerance at the other end.
±0.5° sounds small, and on a short flange it is. On a long one it is not. The angular band converts to a linear deviation at the flange tip, and it grows with every inch of flange.
This is the number most often missed at design time. The angle is held to the same ±0.5° in every row below — what changes is how far that translates once you measure at the free end.
| Flange length | Drift at the flange tip | Angle held |
|---|---|---|
1″25 mm | ±.009″±0.22 mm | ±0.5° |
2″51 mm | ±.017″±0.44 mm | ±0.5° |
4″102 mm | ±.035″±0.89 mm | ±0.5° |
6″152 mm | ±.052″±1.33 mm | ±0.5° |
8″203 mm | ±.070″±1.77 mm | ±0.5° |
The design consequence is direct: if a hole near the end of a long flange has to locate accurately, do not dimension it from the flange tip and do not rely on the angle to place it. Reference it from the datum face and let the flange tip float. If the tip itself has to be accurate, shorten the flange or say so explicitly, and we will look at whether the geometry supports a tighter setting.
The angle itself is measured rather than assumed. The ACB laser on our TruBend 5170 reads the flange during the stroke and compensates springback before the ram retracts, which is what makes ±0.5° a standard rather than a best case. Our ACB guide covers how that loop works.
Dimension the folded part. Let us develop the flat.
Send the formed model and dimension it in its finished state. The flat pattern is an output of our tooling, not an input from your CAD system, and the two only agree if the bend deduction agrees.
Every CAD package will happily unfold a part using whatever K-factor is set in the sheet metal template. That number is a default, not a measurement of our tooling. If you dimension the flat and we develop our own, the formed dimensions can land differently even though both files were internally consistent.
Dimensioning the folded part removes the question. The formed dimensions are what get inspected, so those are the ones worth stating. Our bending ontology guide covers bend deduction and allowance if you want the underlying math, and the Onshape export guide walks through producing a clean folded STEP.
A hole too close to a bend stops being round.
Material near a bend stretches. A hole inside that zone deforms into an oval and pulls out of position, and no dimensioning scheme recovers it after the fact.
Keep holes clear of the bend-affected zone, and where a hole must sit close, tell us — there are options, including piercing after forming or adding relief. Our bend-affected zone guide covers the distances involved.
When a hole near a bend does have to locate accurately, dimension it from the datum face rather than from the bend line. The bend line itself moves within the angular band, so a dimension referenced to it inherits that movement. A dimension referenced to the seating face does not.
Before you send the drawing.
None of this requires GD&T or a formal drafting standard. It requires deciding what the part is for and saying so on the page.
If a dimension on your drawing cannot be met, we would rather raise it during quoting than discover it during inspection. Send the folded STEP and the drawing together and the preflight will flag the conflicts before anything reaches the brake.