Guide
What stamped part tolerances are realistic, and which standard sets them?
Stamped part tolerances are the permitted variations on a part that is blanked, pierced and formed from flat strip or sheet: hole sizes and positions, outline dimensions, bend angles, flatness, burr height and thickness. No single US standard covers all of them, so each one comes from a different place, and the drawing has to say which.
By Saola Manufacturing engineering team · Published · Updated
The practical consequence is that a stamping drawing written like a machining drawing tends to get quoted badly. In a die, some features are fixed by hardened tool steel and repeat closely from part to part, while others depend on springback, coil thickness and the stress rolled into the strip at the mill. This guide takes each feature type in turn: what governs it and how to call it out.
On this page
Which standard sets general tolerances for stamped parts?
In Europe the dedicated standard is DIN 6930-2, the general tolerance standard for stamped steel parts; internationally, ISO 2768-1 also applies, since its scope explicitly includes parts formed from sheet. US drawings usually rely on a company tolerance block in the title block instead, under ASME Y14.5 dimensioning rules.
DIN 6930-2:2011 was written for cold- and warm-formed stamped parts made of flat steel products. It sets general tolerances for linear and angular dimensions, concentricity and symmetry in four accuracy levels: f (fine), m (medium), g (coarse) and sg (very coarse). Unlike ISO 2768-1, its tolerance values depend on material thickness as well as nominal size, which reflects how a stamping actually behaves: a thicker blank shears, bends and springs back differently from a thin one. The 2011 revision widened the nominal size ranges and added tolerances for thickness ranges and for angles on flat stamped parts. Its companion, DIN 6930-1:2011, covers the technical delivery conditions.
Two points are easy to miss. First, per DIN 6930-2, its general tolerances apply only when the drawing or the delivery terms refer to it, so a stamping with no note is not automatically held to it. Second, its scope is steel. For brass, copper or aluminum stampings, either state the tolerances directly or agree in writing that the DIN levels will be applied by analogy.
ISO 2768-1:1989 is the other common reference. Its abstract says it applies to workpieces produced by metal removal or formed from sheet, so an “ISO 2768-m” note on a stamping drawing is valid. It does not scale with material thickness, though, so for thick blanks or tight outlines it can be stricter or looser than the process naturally delivers. The ISO 2768 and NADCA guide reproduces its linear tolerance table.
Where does each stamped-part tolerance come from?
Each feature type has its own governing document: the general tolerance standard for outline and hole dimensions, a bending standard for bent features, GD&T for flatness and position, and the mill specification for thickness.
| Feature | Governing document | What to write on the drawing |
|---|---|---|
| Outline and hole sizes on one flat | DIN 6930-2 level, ISO 2768-1 class, or the title-block tolerance block | One general tolerance note, named once |
| Dimensions across a bend | DIN 6930-2 (by thickness range); bend geometry per DIN 6935 | A wider tolerance than on the flat, or a datum on the formed flange |
| Bend angle | DIN 6930-2 angular tolerances or ISO 2768-1 angular table | Angle tolerance only where the flange locates something |
| Hole position | ASME Y14.5 position tolerance | Position to datums on the same flat as the hole |
| Flatness | ASME Y14.5 flatness; raw stock per ASTM A568 or A480 | Flatness on the functional face, with any restrained condition stated |
| Burr | Drawing note; edge conditions per ISO 13715 | Maximum burr height and which side it may be on |
| Thickness | Material specification (ASTM A568, A480 or the named alloy standard) | The material spec, not a separate thickness tolerance |
Why do features across a bend get a looser tolerance than features on one flat?
Features on one flat are cut by punches fixed in the same die, so their relationship is set by the tool; a dimension that crosses a bend adds the variation of the bend angle, the bend-line location, springback and the stock thickness on top of that.
Picture a bracket with two holes in the base and one hole in a formed flange. The two base holes are pierced in the same station, and the distance between them repeats as closely as the die was built. The flange hole was pierced while the strip was flat, and its final position depends on where the bend line fell, how far the flange sprang back after forming and how thick that particular coil was. Each adds to the stack.
Three drawing habits keep this under control:
- Datum on the flat that matters. Put the primary datum on the face that locates the part in the assembly, and dimension critical holes from that same face.
- Loosen what crosses a bend. If a flange hole only takes a clearance fastener, give it a wider position tolerance than the base holes, or make it a slot.
- Flag holes that must align after forming. If a flange hole has to line up tightly with a feature on another flat, say so in the RFQ. The supplier may pierce it after forming, which is a different die design and a different cost, so it should be priced on purpose.
For the bend itself, DIN 6935:2011 covers cold bending of flat rolled steel, including minimum bend radii. Give the inside radius as a reference or as a range rather than a tight value, and let the die designer choose within it.
How should punched holes be toleranced?
Tolerance a punched hole for its function: a clearance hole can take the general tolerance, while a hole that locates a pin, takes a bearing or must seal needs a stated size, a stated measuring side, and often a secondary operation.
A punched hole is not a straight cylinder. On the punch side the wall is smooth and burnished, where the metal was sheared; further through the thickness it breaks away in a rougher fracture zone, and the hole opens slightly toward the die side. A plug gauge finds the smallest section while a probe may touch elsewhere, so state where the hole is measured.
For holes that do real locating work, the usual choices are to ream or machine the hole after stamping, to shave it in an extra die station, or to extrude it so it has a longer wall. Hole size is also limited by thickness: as a common design rule, a pierced hole should not be smaller in diameter than the material is thick, and hole-to-edge spacing should be at least one material thickness, or the web tears instead of shearing cleanly. The stamping capability page explains more of the design choices that drive die cost.
Remember plating. Zinc or other coatings applied after stamping build up inside holes as well as on faces, so a hole toleranced tightly before plating can gauge undersize afterward. Say whether the hole tolerance applies before or after finishing; the finishing comparison guide covers how each coating adds material.
How flat is a stamped part after blanking?
A blanked part is never flatter than the coil it came from, and blanking itself adds a slight dish near the cut edge, so flatness should be specified only on the faces where it is functional, with a flatness tolerance per ASME Y14.5.
Flatness problems start at the mill. Coil carries residual stress, which shows up as coil set along the length and crossbow across the width, and the stock’s own flatness allowance is set by its material specification: ASTM A568/A568M-25a sets thickness, width, length and flatness tolerances for carbon and HSLA steel sheet, and ASTM A480/A480M-24 does the same for flat-rolled stainless. When the blank is cut out, some of that stress is released and the part moves. The shearing action also rolls the edge over on the punch side and pushes a burr out on the die side, which lifts the part slightly around its outline.
A flattening station, precision-leveled strip or a straightening step can improve it, but none is free, so put the flatness callout on the mounting or sealing face only.
Thin stampings are also flexible, which makes “how flat” depend on how the part is held. ASME Y14.5 allows a restrained condition note, which states how the part is clamped for inspection, and a free-state modifier for requirements that apply unrestrained. If the part will be bolted flat in service, inspecting it restrained the way it is assembled is usually the honest requirement.
How should burrs and edge condition be specified?
Give a maximum burr height and say which side of the part the burr may be on; a note that says only “remove all burrs” cannot be inspected and gets interpreted differently by every supplier.
Every sheared edge has a burr on the die side. Its height grows as the cutting edges wear and as die clearance drifts from the ideal for that material and thickness, so burr height is a maintenance question as much as a design one. A stated burr limit gives the supplier a trigger for sharpening the die and gives inspection something to measure.
Burr direction matters just as much. On a part that slides against another component, or is handled by people, the burr should face away from the contact side; mark that side on the drawing. ISO 13715 is the ISO convention for indicating edge conditions such as burr allowed or sharp edge required, if your drawings follow ISO practice. Where edges must be smooth, tumbling or vibratory deburring is the usual secondary step, and it is typically quoted together with plating on the surface finishing side of the job.
How does sheet thickness tolerance affect a stamped part?
A stamped part is only as consistent in thickness as the coil it is cut from, so its thickness tolerance is the mill tolerance of the material specification, not something the stamping process controls.
First, do not add a thickness tolerance tighter than the material specification allows unless you mean to buy premium-tolerance strip, because that is what the note requires. Name the specification instead, for example cold-rolled carbon steel sheet to ASTM A1008/A1008M-24, which takes its general dimensional requirements from A568. Second, remember that thickness variation feeds every bent dimension, so a part with tight across-the-bend tolerances may need tighter stock even if the thickness itself is not critical.
Coined features are the exception. Coining squeezes the metal locally and does set thickness in that spot, so a coined boss or embossed rib can carry its own dimension.
What should a stamped-part drawing sent to a Vietnam supplier include?
Name one general tolerance source, the material by its full specification, the datum faces, the burr side and limit, and any feature that must be held after forming or after plating. With those five items stated, a supplier in Vietnam or anywhere else can quote the part as drawn instead of sending questions first.
- One general tolerance. A DIN 6930-2 level, an ISO 2768-1 class or your title-block block, not a mix.
- Material by specification. Mills in Asia often supply to JIS or GB grades; if an equivalent to your ASTM or EN grade is acceptable, say so, and if it is not, say that too.
- Units stated. DIN and ISO tables are metric, so an inch drawing that cites them forces a conversion on every dimension.
- Critical features listed in the RFQ. Across-the-bend holes, flatness faces and post-plating hole sizes should be named in the request, not discovered at first-article inspection.
Sourcing a stamping from Vietnam rather than China also raises country-of-origin questions if the coil or the blank comes from elsewhere; that belongs in the commercial conversation, separate from the tolerance review. The RFQ package guide lists what else to send. When the package is ready, send it for a quote, and tolerances that need a conversation are answered feature by feature.
Frequently asked
Does ISO 2768 apply to stamped parts?
Yes. The ISO abstract for ISO 2768-1 states that it applies to workpieces formed from sheet as well as machined ones. It does not scale with material thickness, which is the main reason European stamping drawings often cite DIN 6930-2 instead.
Can DIN 6930-2 be used for aluminum or brass stampings?
Its scope is stamped parts made of flat steel products. Many buyers apply its levels to other metals by agreement, but that should be written into the drawing or the purchase terms rather than assumed.
Why does a punched hole measure differently on each side?
The punch side is sheared and burnished; the die side breaks away in a fracture zone and opens up slightly. State where the hole is measured, or specify a reamed or shaved hole where size really matters.
Should I put a tolerance on the bend radius?
Usually no. Give the inside radius as a reference or a range, and control the features the bend positions instead. DIN 6935 gives guidance on bend radii for cold-bent steel.
Can a stamped part hold machining-level tolerances?
Individual features can, if they are machined after stamping. A stamping with a few reamed or milled features is often cheaper than machining the whole part from plate; the CNC milling page covers the secondary-machining side.
Sources
- DIN 6930-2:2011-10, Stamped steel parts — Part 2: General tolerances, DIN, 2011
- DIN 6930-1:2011-10, Stamped steel parts — Part 1: Technical delivery conditions, DIN, 2011
- DIN 6935:2011-10, Cold bending of flat rolled steel, DIN, 2011
- ISO 2768-1:1989, General tolerances — Part 1: Tolerances for linear and angular dimensions without individual tolerance indications, ISO, 1989
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ASTM A568/A568M-25a, Steel, Sheet, Carbon, Structural, and High-Strength Low-Alloy, Hot-Rolled and Cold-Rolled, General Requirements for, ASTM, 2025
- ASTM A480/A480M-24, General Requirements for Flat-Rolled Stainless and Heat-Resisting Steel Plate, Sheet, and Strip, ASTM, 2024
- ASTM A1008/A1008M-24, Steel, Sheet, Cold-Rolled, Carbon, Structural, High-Strength Low-Alloy, ASTM, 2024
- ISO 13715:2019, Technical product documentation — Edges of undefined shape — Indication and dimensioning, ISO, 2019