Brake Press Tolerance Guide

Angle Tolerance

Air bending on CNC: ±1° standard, ±0.5° with angle measurement feedback. Bottom bending: ±0.5° standard, ±0.25° achievable. Coining: ±0.25° or better. These tolerances assume consistent material — variation in sheet thickness, hardness, or grain direction will cause angle variation even with perfect machine setup. Material consistency matters more than machine capability.

Bend Location (Flange Dimension)

CNC back gauge accuracy: ±0.001"–0.002" positioning. Practical flange tolerance: ±0.010"–0.015" accounting for material placement, thickness variation, and operator handling. On automated gauge systems with front-loading: ±0.005" is achievable in production. Short flanges (under 0.500") are inherently less accurate because the back gauge has less material to reference against.

Flatness & Twist

Long parts (over 36") formed with multiple bends may develop twist — angular deviation along the length. CNC crowning systems compensate for beam deflection (the center of a long bend opens up more than the ends). On 10' bed lengths, crowning correction is essential. Twist tolerance: 0.5° per foot of length is production-realistic. Tighter requires manual shimming.

Springback

All metals spring back after bending. Mild steel at 90°: 1–3° springback. Stainless steel: 3–5°. Aluminum: 2–6° (varies wildly by alloy and temper). High-strength steel: 5–10°+. CNC systems compensate automatically, but the compensation is based on assumptions about material properties. Batch-to-batch material variation is the primary source of angle inconsistency.

Inside Bend Radius

Minimum inside bend radius is a function of material thickness, ductility, and grain direction. Rule of thumb: minimum IR = 1x material thickness for mild steel, 1.5x for stainless, 2x for aluminum (varies by alloy). Going below minimum radius causes cracking on the outside of the bend. Bend across the grain where possible — with-grain bends crack at larger radii.

Hole & Feature Distortion Near Bends

Features within 2x material thickness of a bend line will distort during forming. Holes elongate, slots warp, threads strip. The standard rule: keep all features at least 2.5x material thickness (or the die opening width, whichever is greater) away from any bend line. If features must be closer, they should be added after forming.