Metal Stamping and Sheet Metal Tolerances: Charts and Standards

Published: February 14, 2024

Metal stamping and sheet metal tolerances reference chart

This article pulls the key points from GB/T13914-2002 (Dimensional Tolerances for Stamping Parts) and applies them to real shop-floor conditions. Meeting tolerance specs is non-negotiable, but you also have to weigh feasibility and cost—so we flag where you can relax tolerances without compromising function.

Tolerance for precision metal stamping parts depends on both the part's physical size and the tolerance grade you pick. If the part meets its functional requirements, choosing a more economical grade makes it easier to manufacture and keeps tooling costs down.

Dimensional Tolerances for Flat Stamping Parts

Flat stamping parts are classified into 11 grades, labeled ST1 through ST11. ST stands for the dimensional tolerance of flat stamping parts, and the number indicates the grade. Accuracy drops sequentially from ST1 (tightest) to ST11 (loosest).

Dimensional Tolerances for Formed Stamping Parts

Formed stamping parts are classified into 10 precision grades, labeled FT1 through FT10. FT stands for the dimensional tolerance of formed stamping parts, and accuracy drops sequentially from FT1 (tightest) to FT10 (loosest).

Limit Deviations

For hole dimensions, the lower deviation is typically zero, with the upper deviation set to the full tolerance. For shaft dimensions, it's the reverse: the upper deviation is zero, and the lower deviation is the negative tolerance. For hole-center distances, edge distances, bend lines, draw lengths, and heights, we commonly use equal bilateral deviations—plus or minus half the tolerance.

Key Production Points to Control

Bend angles and punch angles.
Punched fillet radii.
Forming dimensions from bending or drawing operations.
Punching and blanking dimensions.
Material thickness, die clearance, and measurement method.

Keeping these parameters in check lets us hold the required precision, hit your design specs, and turn out consistent stamped-part quality run after run.

Blog

Extrusion with Sharp Corners in Deep Drawn Stamping

Ironing in Deep Drawn Stamping

Balford Employees Participate in the Zhuji Marathon

Balford Trademark and ISO9001:2015 Certified

Balford's Metal Components Expertise

Deep Drawing Sheet Metal: Precision Components

What is metal stamping?

Design Guide: Double-Sided Chamfered Circular Washer

Design Guide: Stamping Washers

Automotive Motor Housing Manufacturing via Deep Drawing

Reference Tolerances for Stamped and Deep-Drawn Parts

The values below are general industry references for sheet-metal stamping and deep drawing. They are what the process family typically holds — not a promise for a specific part. The tolerance Balford quotes for your part is confirmed from your drawing during DFM review, because material, thickness, feature type and tooling all move the number.

Blanking and piercing

Feature	Dimension range	Typical tolerance
Blank / outer profile	up to 25 mm	±0.05 – 0.10 mm
Blank / outer profile	25 – 100 mm	±0.10 – 0.20 mm
Blank / outer profile	over 100 mm	±0.20 – 0.40 mm
Pierced hole diameter	up to 10 mm	±0.05 mm
Hole position (hole to hole)	up to 100 mm	±0.10 mm

Forming and bending

Feature	Typical tolerance
Bend angle	±0.5° – 1°
Bend dimension (flange length)	±0.10 – 0.25 mm
Formed height	±0.10 – 0.30 mm
Flatness / perpendicularity	per drawing, commonly 0.1 mm per 100 mm

Deep drawing (cylindrical parts)

Feature	Dimension range	Typical tolerance
Outside diameter	up to 25 mm	±0.05 – 0.10 mm
Outside diameter	25 – 100 mm	±0.10 – 0.20 mm
Outside diameter	over 100 mm	±0.25 – 0.50 mm
Wall thickness (after ironing)	—	approximately ±10% of nominal
Overall height	—	±0.15 – 0.40 mm
Concentricity	—	0.05 – 0.15 mm TIR

What actually decides the number

Material and temper — harder and stronger grades spring back more and hold less of the formed geometry.
Thickness — the thinner the strip, the smaller the absolute tolerance the process can hold.
Feature type — a pierced hole, a bend and a drawn wall are three different processes with three different capabilities.
Relation to the datum — tolerances measured from the same tooling station are tighter than tolerances measured across several stations.
Whether the feature is cut or formed — cut features come off the tool; formed features carry springback and material-flow variation.

If your drawing carries a tolerance the process cannot hold at volume, the DFM review says so before tooling — which is much cheaper than finding out at first article.

Frequently asked

What tolerance can Balford hold on a stamped part?

It is confirmed per part from your drawing, not from a single headline number. Send the drawing with material, thickness and annual quantity and the DFM review returns the achievable tolerance per feature, plus which features need a secondary operation or a tolerance relaxation.

Can tighter tolerances be achieved with a secondary operation?

Often yes. A pierced or drawn feature can be brought into tolerance afterwards by coining/calibration in the die, or by CNC turning, milling or grinding where the geometry allows. The trade-off is cost per part, and the review will show both options.

Do these reference values apply to stainless steel and aluminium too?

The ranges shift with the material. Stainless steels work-harden and spring back more than mild steel; aluminium forms easily but marks and scratches easily and needs more care in handling. The reference table above is a starting point — your drawing decides the real number.

Sheet metal tolerances: the reference chart

Engineers looking for sheet metal tolerances usually want one thing first: a starting number per feature, before a supplier has been chosen. The table below is the band a well-maintained press tool holds in serial production on 0.5–3.0 mm mild steel. Stainless steel, aluminium and pure iron shift these numbers — the last column says which way.

Feature	Typical holdable tolerance	What moves it
Blanked profile, overall size	±0.10 – ±0.25 mm	Die clearance, strip position and burr allowance. Below ±0.10 mm expect a shaved or ground edge rather than a sheared one.
Pierced hole diameter, Ø under 10 mm	±0.05 – ±0.12 mm	Punch clearance and punch wear. A hole smaller than the material thickness needs a stepped punch.
Hole-to-hole position, one station	±0.05 – ±0.15 mm	Every punch in a station moves with the same tool, so position repeats far better than absolute size.
Hole-to-hole position, across stations	±0.15 – ±0.30 mm	Strip feed pitch error accumulates; pilot pins recover most of it.
Bend angle	±0.5° – ±1.5°	Springback. Stainless needs over-bending, or a coining/bottoming station.
Bend-to-hole distance	±0.15 – ±0.30 mm	Material flowing into the bend. Keep holes at least 2×t plus the bend radius from the bend line.
Drawn outside diameter, Ø 20–80 mm	±0.05 – ±0.15 mm	Die ring wear and ironing. An ironed wall holds the diameter; a wall that is only drawn does not.
Drawn wall thickness	±5–10 % of nominal, or ±0.01 mm when ironed	Thinning is a process choice: drawing thins unevenly, ironing controls the wall on purpose.
Drawn height or depth	±0.15 – ±0.30 mm	Blank-size variation and the number of draw stages.
Concentricity of a drawn body	0.05 – 0.15 mm	Punch-to-die alignment carried across stages — set on the tool, not on the part.
Flatness of a formed part	0.10 – 0.30 mm	Residual stress from forming, plus any later heat treatment.

These are process references, not a contractual promise. The number Balford quotes for a specific part is confirmed from the drawing during DFM analysis, because material, thickness, feature type and tooling all move it.

How this compares with the standard printed on your drawing

General-tolerance standards such as ISO 2768-1 (classes f, m, c, v), DIN 6930-2 for cold-rolled steel pressings and GB/T 1804 exist so that a drawing does not have to dimension every feature. They are a floor, not a capability statement:

ISO 2768-m is roughly ±0.2 mm in the 6–30 mm band — comfortably inside what a normal press tool holds, which is why so many drawings carry it.
ISO 2768-f (±0.1 mm in the same band) is where a stamped part needs a deliberate decision: shaved edges, in-die gauging, or a lower Cpk accepted in writing.
DIN 6930-2 was written specifically for pressings and separates cut features from formed features — useful when a customer asks why the hole is held but the bend is not.
The detail that catches buyers: ISO 2768 applies unless the drawing says otherwise, so an undimensioned feature is not "whatever comes out" — it is class m, and the tool has to hold it.

Which tolerances actually drive the price

Tolerance costs money in three places, and only the first one is obvious:

Tooling. Going from ISO 2768-m to ±0.05 mm on a pierced hole usually adds a station (pilot plus shave), not just a tighter punch.
Tool life. A punch running at half the normal clearance wears faster, and the consumable cost lands in the piece price at volume.
Inspection. A feature that cannot be checked with a plug gauge or a simple fixture needs CMM time per batch, which is a cost per lot rather than per piece.

That is why the cheapest answer to "make it tighter" is often a design change: move a datum, open a non-functional tolerance, or let one surface be machined after forming. Ironing is the good example — it tightens wall and diameter tolerances enough to remove a turning operation.

Frequently asked about sheet metal tolerances

What is the standard tolerance for sheet metal parts?

There is no single number, because it depends on the feature. For a normal press tool the practical working figure is ±0.1–0.2 mm on cut features and ±0.5–1° on bend angles, with general-tolerance standards such as ISO 2768-m or DIN 6930-2 used where the drawing does not call out a value.

Can I get a tolerance check on my own drawing?

Yes. Upload it to the DFM pre-screen: it lists the tolerance callouts it read, flags the ones tighter than the process normally holds, and names the feature that drives them.

Are deep drawing tolerances different from stamping tolerances?

Yes. Cutting operations reproduce the tool, so they hold sizes directly. Drawing depends on material flow, so wall thickness, roundness and height vary with the draw ratio, the number of stages and whether the wall is ironed. A drawn diameter holds well; the drawn wall is the feature to watch. See tolerances on deep drawn housings.

Does a tighter tolerance always cost more?

Not always, but usually. If the feature is already formed in a station that exists, tightening may cost nothing. If it needs an extra station, a shave, a coining pad or 100 % gauging, it does — and the cost lands either in the tooling or in the piece price.

How do I know what my part can actually hold?

Send the drawing with material, thickness and annual quantity. The DFM review returns the achievable tolerance per feature and the cost of tightening the ones that matter, before tooling starts. The instant estimate gives a first price indication in the same session.