Sheet Metal Tolerance Chart: Cutting, Bending & Welding

Important Before You Use This Chart

The values below are typical manufacturing references for custom sheet metal fabrication. They are not universal guarantees and should not replace part-specific tolerances on a production drawing.

Actual results depend on material grade, thickness, sheet flatness, part size, feature geometry, bend count, bend direction, tooling, weld sequence, coating thickness, inspection method, and datum strategy. Use general tolerances for non-critical dimensions, then apply specific tolerances only where fit, function, sealing, alignment, motion, grounding, or assembly depends on them.

Rule of thumb: If a dimension affects fit, alignment, sealing, motion, grounding, hardware engagement, or an external interface, call it out clearly on the drawing.

Typical Sheet Metal Fabrication Tolerances

Feature or Process	Typical Reference	Practical Design Note
Laser-cut profile / outside dimension	±0.10–0.30 mm	Depends on material, thickness, feature geometry, and overall part size
Laser-cut hole diameter	±0.10–0.20 mm	Use drilling, reaming, or machining for precision bores
Laser-cut feature position	±0.15–0.30 mm	Dimension critical features from common datums
CNC-punched hole or profile	±0.10–0.20 mm	Tool condition, material, and sheet movement affect results
CNC-punched feature position	±0.15–0.30 mm	Use datum-based dimensions for mating patterns
Press-brake bend angle	±1° typical	Springback, grain direction, tooling, and material affect results
Single flange length	±0.30–0.50 mm	State the measurement reference or tangent point
Bend-to-bend dimension	±0.50–1.00 mm	Variation accumulates with bend count, length, and geometry
Overall formed dimension	±0.50–1.50 mm	Review large, asymmetric, or multi-bend parts individually
Inside bend radius	Process-dependent	Depends on material, thickness, punch radius, die opening, and bending method
Self-clinching mounting hole	Per fastener datasheet	Use the exact selected fastener’s hole size and tolerance
Self-clinching hardware position	Controlled by mounting-hole position	Locate critical hardware holes from datums
Welded assembly dimensions	Part-specific	Define post-weld datums, fixtures, and critical interfaces
Flatness	Part-specific	Depends on material stress, cut pattern, forming, welding, and finishing
Powder-coat thickness	0.06–0.10 mm per surface	Confirm coating specification for critical fits

These values are engineering starting points, not blanket capability commitments. JIS B 0408 Class B reference values, for example, change by nominal size:

Punched features: Range from ±0.1 mm (at 6 mm and below) to ±0.5 mm (at 121–400 mm).
Formed dimensions: Range from ±0.3 mm to ±1.2 mm across the same size bands.

General Tolerances

When General Tolerances Are Enough

Use a general tolerance for dimensions that do not directly affect fit or function, such as:

Non-mating cover dimensions
Cosmetic edge locations
Vent patterns without mating requirements
Non-critical mounting features
General enclosure height, width, and depth
Decorative cutouts and labels

General tolerance classes provide a default framework for dimensions without individual callouts. The required tolerance class must be stated on the drawing and evaluated against the chosen manufacturing process; it should never be assumed automatically.intertekinform+1

When to Add a Specific Tolerance

Apply a specific tolerance only where it controls a functional requirement:

Hole patterns that mate with another part
Self-clinching nut, stud, standoff, and connector locations
Hinge, latch, and door alignment
Gasket and sealing interfaces
PCB, display, connector, and fan mounting features
Sliding, locating, or interlocking features
Cosmetic gaps and visible front-panel interfaces
Features located from a customer-supplied datum system

Cost rule: Tight tolerance on every dimension increases setup, inspection, scrap risk, lead time, and cost. Tighten only the features that control assembly performance.

Laser Cutting Tolerances

Typical Laser-Cutting Reference Ranges

Feature Condition	Typical Reference	Recommended Action
Thin sheet and short profile dimensions	±0.10–0.20 mm	Suitable for most non-mating cut features
Standard sheet-metal profiles	±0.10–0.30 mm	Identify critical dimensions and inspect from stated datums
Thick material, large parts, or complex cut paths	Review by part	Allow for kerf, taper, heat input, and part movement
Precision bores, dowel locations, or bearing fits	Secondary operation required	Drill, ream, or machine after cutting

Laser-cut hole quality and dimensional consistency depend on sheet thickness, material, feature diameter, kerf, heat input, assist gas, cut path, and part geometry. Do not use a laser-cut hole as a precision locating bore unless a secondary operation or part-specific validation is planned.

Laser-Cut Hole Rules

Dimension mating-hole patterns from common datums rather than chaining dimensions.
Allow for coating thickness where a pin, screw, connector, or mating component passes through a finished hole.
Use drilling, reaming, or machining when roundness, location, or fit requires more control than normal laser cutting provides.
Use the selected self-clinching hardware manufacturer’s specified mounting-hole size; do not substitute a generic hole tolerance.

Punching Tolerances

Typical CNC Punching Tolerances

Feature	Typical Reference	Design Consideration
Round or shaped hole	±0.10–0.20 mm	Tool clearance, material, and punch condition affect edge quality
Hole position	±0.15–0.30 mm	Use datums for mating patterns
Slot width	±0.10–0.20 mm	Narrow slots may require special tooling or laser cutting
Formed feature height	±0.25–0.50 mm	Depends on material, tooling, and feature geometry
Louver, emboss, lance, or extrude	±0.25–0.50 mm	Confirm tooling availability and feature-clearance requirements

Punching is highly repeatable in production, but feature spacing, tool wear, material properties, part handling, and formed geometry affect results. If a punched hole receives self-clinching hardware, specify the exact hardware family and manufacturer-required mounting-hole dimension.

Bending Tolerances

Typical Press-Brake Tolerances

Feature	Typical Reference	Notes
Bend angle	±1° typical	Depends on springback, material, grain direction, tool setup, and bend length
Single flange length	±0.30–0.50 mm	Define the inspection reference or tangent point
Bend-to-bend dimension	±0.50–1.00 mm	Variation grows with bend count, part length, and geometry
Overall formed dimension	±0.50–1.50 mm	Review large, thin, asymmetric, or multi-bend parts individually
Inside bend radius	Process-dependent	Actual radius is controlled by material and tooling, not a universal tolerance

JIS B 0408 Class B gives a useful general reference for formed sheet-metal dimensions:

Nominal Size	Tolerance
≤ 6 mm	±0.3 mm
7 – 30 mm	±0.5 mm
31 – 120 mm	±0.8 mm
121 – 400 mm	±1.2 mm

Note: Bend-angle reference is ±1°.

Bending DFM Rules

Dimension critical features from the same formed datum whenever possible.
Avoid tolerance chains across multiple bends.
Do not apply very tight tolerances to dimensions controlled by several consecutive bends.
Keep holes, slots, and self-clinching hardware outside bend deformation zones.
Specify an inside bend radius only when it affects function or assembly.
Request first-article inspection for tight formed assemblies and production-critical interfaces.

Welding Tolerances

Welded Assembly Control

Welded assemblies should be toleranced according to their geometry, joint design, weld length, material, thickness, fixture strategy, weld sequence, and post-weld finishing requirement. Do not apply a generic welded-assembly tolerance to every part.

Feature	Recommended Control Method	Design Note
Overall welded dimensions	Part-specific tolerance	Identify critical post-weld interfaces and inspection datums
Squareness and perpendicularity	Datum- and fixture-controlled	Apply only when needed for functional alignment
Flatness after welding	Part-specific requirement	Heat distortion depends on weld sequence, length, and geometry
Weld position	Drawing note or GD&T	Identify critical joint locations from datums
Cosmetic weld finish	Approved sample or visual standard	Define weld side, grinding, blending, and visible-surface requirements

When a welded enclosure must fit a frame, gasket, door, PCB, or external housing, call out critical post-weld dimensions and the measurement condition instead of applying a blanket tight tolerance to every feature.

Hardware Tolerances

Self-Clinching Hardware

Use the selected fastener manufacturer’s exact mounting-hole diameter and tolerance for self-clinching nuts, studs, and standoffs. Hardware position is governed by the position of the pre-cut mounting hole; locate critical holes from datums and consider press access, nearby bends, coating sequence, and local panel deformation.

Example: An M4 self-clinching nut and an M4 self-clinching stud can require different mounting-hole diameters because their clinching geometries are different.

PEM instructs users to provide the specified mounting-hole size, avoid secondary operations such as deburring, and apply installation force between parallel surfaces until the clinching feature seats correctly.pemnet+1

Threaded Holes and Tapped Features

Choose threaded holes according to panel thickness, required thread engagement, load, serviceability, corrosion protection, and assembly sequence. Thin sheet may require extruded holes, self-clinching hardware, weld nuts, or threaded inserts instead of direct tapping.

Surface Finish Allowance

Typical Design Allowances

Confirm final coating thickness against the specified finishing process, coating supplier data, and approved production sample.

Finish	Typical Thickness / Change	Design Impact
Powder coating	0.06–0.10 mm per surface	Holes become smaller and outside dimensions become larger
Wet paint	0.02–0.05 mm per surface	Allow clearance for fits, threads, and grounding points
Zinc plating	0.005–0.025 mm per surface	Can affect threads and tight clearances
Electroless nickel	0.010–0.050 mm per surface	Relatively uniform build affects both sides
Anodizing	Process-dependent	Confirm alloy, type, sealing, masking, and dimensional requirement

Finish thickness varies with geometry, edge effect, coating system, grounding, application method, cure process, and specification. Treat these values as early design allowances; specify required clearances, masking, and post-finish fit conditions whenever coating affects assembly.

Frequently Asked Questions

Quick answers to common questions regarding sheet metal tolerances, standard process limits, and design best practices

What is the standard tolerance for sheet metal fabrication?

There is no single tolerance for every sheet-metal feature. As a practical starting point, laser-cut profiles commonly fall around ±0.10–0.30 mm, press-brake bend angles around ±1°, and formed dimensions vary according to size and bend complexity.

What is ISO 2768-m?

ISO 2768-m is a medium general-tolerance class for dimensions without individually stated tolerances. State the class in the drawing title block and confirm it is appropriate for the intended manufacturing process and part function.

How accurate is laser-cut sheet metal?

Thin sheet and short features can commonly achieve about ±0.10–0.20 mm, while standard profiles often fall around ±0.10–0.30 mm. Thick material, large parts, complex paths, and precision bores require part-specific review or secondary operations.

What tolerance can a press brake hold?

A typical press-brake bend angle is around ±1°. A single flange may commonly be held around ±0.30–0.50 mm, while bend-to-bend and overall formed dimensions generally need more allowance as bend count and part size increase.

Does powder coating affect dimensions?

Yes. Powder coating builds on surfaces, reducing hole diameter and increasing outside dimensions. Include clearance, masking, and post-finish fit requirements for pins, threads, connectors, doors, and other tight mating features.

How do I reduce tolerance stack-up?

Locate critical features directly from common datums instead of dimensioning one feature from another in a chain. Apply tighter tolerances only to functional interfaces and define the measurement datum system.

Need a Tolerance Review Before Production?

Tolerances should support function without adding unnecessary fabrication cost. Upload your drawing and ShincoFab’s engineers can review critical dimensions, bend chains, hardware locations, finish allowances, and inspection requirements before quotation.

Capabilities

Fabrication

Value-Added

3D Printing

Material

Products

Sheet Metal Parts

Thermal & Electrical

Sheet Metal Enclosure

Energy & Infrastructure

Industries

Resource

Why Choose Us