What Tolerances to Expect on Cut and Formed Parts

Tolerance everything tightly and you pay for precision you do not need. Tolerance nothing and you gamble on fit. The middle path is knowing the standard tolerances the shop already holds, so you can call out only the few features that truly matter and leave the rest at standard. Here are the numbers to design around.

For parts up to 24″ × 24″, outside profiles and large internal cutouts hold ±0.010″, and holes hold ±0.005″. Those two numbers cover the great majority of flat and formed hardware, so most drawings never need anything tighter.

Larger parts open up a little, and the rule is simple. For every additional 12″ beyond 24″ in the largest part dimension, add ±0.002″ to the profile and large cutout tolerance. The hole tolerance stays at ±0.005″ unless thickness, geometry, or process conditions require an adjustment. So a longer part gives up a couple of thousandths on its overall profile while its holes stay right where they were.

One number you do not control is the thickness of the stock itself. Sheet and plate thickness is nominal and follows mill tolerance, which means the material arrives close to its stated thickness but not exactly on it. A nominal 0.250″ plate can run slightly over or under, and that is normal material, not a defect.

Design so that a few thousandths of thickness variation does not break a fit or a stack. If a slot has to accept a tab, or a set of plates has to add up to a target height, give the fit a little room rather than sizing it to the nominal thickness and hoping. For how the same gauge is a different thickness in each material, see the gauge chart, and call out thickness in decimals to avoid confusion.

Once a part gets bent, a second set of numbers applies. Standard flange dimensions hold ±0.030″ and standard bend angles hold ±1°. Those are the numbers to design around for a normal formed part, and they are looser than the cutting numbers on purpose, because forming introduces spring back and material behavior that a flat cut never sees. See Sheet Metal Bending and press brake bending for the process behind these.

This is the point that catches people. On a multi bend part, each individual flange and each angle holds its own standard tolerance. That is fine on its own. The trouble starts when an overall dimension crosses several bends at once, because it adds up the variation of every bend it passes through. Stack three bends between two features and the tolerances stack with them.

• Dimension from a single datum. Where you can, measure critical features from one reference edge rather than chaining dimensions bend to bend.
• Avoid crossing a critical dimension over many bends. A hole to hole distance that spans three flanges will carry the combined variation of all three.
• Put critical holes on one face. Features cut into the same flat face hold the tight cutting tolerance between them, before any bend variation enters.

The finished inside bend radius comes from the closest available tooling for your material and thickness, so it can differ from the nominal radius in your model. The bend is formed with real tooling, and the shop picks the closest match rather than grinding custom tooling for one job. In practice the radius is close, but it is not a number you should assume to the thousandth.

If a radius is functionally critical, say a part has to nest against another or clear a mating feature at the bend, identify it before ordering so it can be reviewed. See bend radius and minimum flange and what is K factor for how radius drives the flat pattern.

Standard forming tolerances assume the part sits inside the normal forming envelope. On the press brake that means a maximum bend length of 96″, a minimum part size of 1″ × 1″, and a thickness range of 0.020″ to 0.500″. Parts that live comfortably inside that window form predictably at the standard numbers. Parts that push the edges, very small, very long, or very thick, are where you should expect a closer look and possibly a custom quote.

Tighter than standard is available, but it is not automatic. Call it out clearly on the drawing and expect the part to route to a custom quote so an estimator can confirm it is achievable on your geometry, material, and thickness. A tolerance the shop cannot see is a tolerance the shop cannot hold, so put the number where it will be read.

The cheapest path to a good part is to tolerance the few features that are functional and leave everything else at standard. Every tight tolerance you add is precision someone has to hold and verify, and precision you do not need is money you did not have to spend. Ask of each dimension whether it actually controls fit, function, or assembly. If it does, tolerance it. If it does not, let it ride at standard and let the shop work efficiently.