Sheet Metal Tolerances:
Laser Cutting
and CNC Bending

Why Tolerance Selection Matters

Specifying tolerances tighter than necessary drives up cost in two ways: it increases setup and inspection time, and it raises the rejection rate. Most industrial sheet metal enclosures and brackets function correctly with standard tolerances. Tight tolerances should be applied only to features where assembly fit or function genuinely depends on them.

The rule of thumb: apply tight tolerances to interfaces, not to overall part dimensions. A cabinet door that must align within 1 mm of an opening, yes. The overall height of the cabinet panel, probably not.

Laser Cutting Tolerances

The following tolerances apply to fiber laser cutting of SPCC and SGCC on our AMADA EML-3510NT system. Values assume standard production conditions — clean material, calibrated beam, correct assist gas.

Feature	Standard Tolerance	Achievable (tight)	Notes
Linear dimension (≤500 mm)	± 0.2 mm	± 0.1 mm	Tight tolerance requires slower cut speed
Linear dimension (500–1500 mm)	± 0.3 mm	± 0.2 mm	Thermal expansion becomes a factor at longer spans
Hole diameter (circular)	± 0.15 mm	± 0.10 mm	Minimum hole diameter = 1.2× material thickness
Hole position	± 0.15 mm	± 0.10 mm	Relative to datum edge
Kerf width (0.6–1.5 mm material)	0.1–0.2 mm	—	Affects final dimension on narrow slots
Edge squareness (perpendicularity)	≤ 1° draft	≤ 0.5°	Increases with material thickness
Surface roughness (cut edge)	Ra 3.2–6.3 μm	Ra 1.6 μm	Finish cut pass required for Ra 1.6

Minimum Feature Sizes for Laser Cutting

These are not tolerance values but hard minimum limits that the laser cutting process can reliably produce:

Feature	Minimum Dimension
Hole diameter (round)	1.2× material thickness (min. 0.8 mm)
Slot width	1.0× material thickness (min. 0.8 mm)
Web between two holes	1.5× material thickness
Distance from hole to part edge	1.5× material thickness
Notch width	1.5× material thickness

CNC Bending (Press Brake) Tolerances

Bending tolerances are more variable than cutting tolerances because springback, material variation, and tooling condition all affect the result. The values below are for SPCC/SGCC at standard production conditions on our AMADA HFB series press brakes.

Feature	Standard Tolerance	Achievable (tight)	Notes
Bend angle	± 1°	± 0.5°	Tight requires first-piece verification and springback compensation
Flange length (inside dimension)	± 0.3 mm	± 0.15 mm	Tight requires precision back-gauge setup
Overall part length after bending	± 0.5 mm	± 0.3 mm	Cumulative error from multiple bends
Flatness (after forming)	≤ 1 mm / 300 mm	≤ 0.5 mm / 300 mm	Depends on part geometry and material temper
Parallelism (opposite flanges)	± 0.5 mm	± 0.3 mm	Across full part length

Springback and K-Factor

Springback is the elastic recovery of the material after the punch is withdrawn. Every bend in sheet metal springbacks by some amount — this is compensated in the CNC program using empirical K-factor values derived from material grade, thickness, and tooling geometry.

SPCC has lower springback than SGCC at equivalent thickness. For parts with tight angle tolerances and multiple bends, specifying SPCC simplifies springback compensation and improves repeatability.

Minimum Bend Radius

Bending below the minimum radius cracks the material on the outer face of the bend. Minimum values depend on material and thickness:

Material	Thickness	Minimum Inside Bend Radius
SPCC	0.6 – 1.0 mm	0.5× thickness (0.5t)
SPCC	1.0 – 2.0 mm	0.5t – 1.0t
SGCC	0.6 – 1.5 mm	1.0t (zinc coating cracks below this)
SGCC	1.5 – 2.3 mm	1.5t

How to Specify Tolerances on Drawings

The most efficient approach is to state a general tolerance in the title block that covers most features, then call out tighter tolerances only on critical dimensions. This is standard practice in ISO GPS (Geometrical Product Specifications).

Suggested title block tolerance note for general sheet metal:

ISO 2768 tolerance classes for reference:

Class	Linear (≤30 mm)	Linear (30–120 mm)	Angular
f (fine)	± 0.05 mm	± 0.1 mm	± 20'
m (medium)	± 0.1 mm	± 0.2 mm	± 30'
c (coarse)	± 0.2 mm	± 0.5 mm	± 1°
v (very coarse)	± 0.5 mm	± 1.0 mm	± 2°

For most sheet metal enclosures and structural brackets, ISO 2768-c (coarse) is appropriate. ISO 2768-m applies when assembly requires tighter fit. ISO 2768-f is rarely needed for sheet metal and carries a meaningful cost premium.