Sheet Metal Bending Guide: Radii, K-Factors & DFM Rules

This guide presents the Design for Manufacturing (DFM) rules to follow when designing bent sheet metal parts fabricated by Laseo. Following these rules ensures part feasibility, minimizes lead times, and guarantees dimensional quality. Our app automatically checks most of these rules at design time — this guide helps you get it right the first time.

Process: air bending on a CNC press brake. The bend radius is determined by the material, the thickness and the tooling. Custom radii are not offered. The bending service is presented in detail on the bending service page.

In this guide

Bending terminology
Bend radius
Minimum flange length
Hole-to-bend distance
Distance between bends
Angles and angular tolerances
Bend relief
Bend allowance & flat pattern
Tolerances
Part size constraints
U-channels
Master table per material
Common mistakes
Quick reference

1. Sheet metal bending terminology

Before designing a bent part, it's essential to understand the fundamental terms: inside radius (R), thickness (T) and angle (θ) define the anatomy of every bend.

Term	Definition
Bend angle (θ)	Angle between the two faces after bending
Inside radius (R)	Radius of curvature of the inside surface of the bend
Thickness (T)	Sheet metal thickness
K-factor (K)	Neutral axis position through the thickness: K = t/T
Flange	Flat portion between the part edge and the start of the bend
Bend allowance (BA)	Arc length of the neutral axis in the bend zone
Bend deduction (BD)	Reduction applied to the flat pattern for each bend
Bend line	Line on the flat pattern where the bend occurs
Die	Bottom V-shaped tool — its width drives several constraints
Bend relief	Cutout at the ends of a bend line to prevent tearing

2. What is the bend radius?

The inside bend radius is fixed for each material/thickness combination. It depends on the tooling (punch and die) and cannot be customized. Check the "Inside radius" column in the master table for your material's exact radius.

In practice, radii range from 0.024″ for thin sheet to 0.346″ for 1/4″ stainless. Design your 3D models with these radii so the computed flat pattern matches the manufactured part.

3. What is the minimum flange length?

The flange length is the distance between the part edge and the start of the bend zone. If the flange is too short, the sheet slips in the die and the bend won't form correctly — the flange deforms instead of bending.

Minimum flange ≈ max(2 × T, T + R)

Exact values per material and thickness (0.200″ to 1.155″) are in the "Min flange" column of the master table. The app automatically blocks any bend whose flange would be too short.

4. How far from a bend should holes and cutouts be?

Holes, slots, engravings and any other cut feature must be far enough from the bend line. A feature that is too close sits in the die contact zone and will be distorted during bending.

Minimum distance = die width ÷ 2

Die width	Minimum distance	Metric
0.472″	0.236″	6.0 mm
0.630″	0.315″	8.0 mm
0.984″	0.492″	12.5 mm
1.575″	0.788″	20.0 mm

Tapping and hardware insertion are done before bending. A distorted hole renders threads unusable — respect this distance for any tapped hole or hardware location.

5. What is the minimum distance between two bends?

For two parallel bends, the minimum distance between bend lines depends on the bend angle. Bends that are too close make the die contact zones overlap, which causes metal puckering.

Parallel bends

Bend angle	Minimum distance
5°–45°	Material joggle spec (see below)
46°–90°	2 × minimum flange
91°–130°	Acute angle spec — checked case by case by the app

Joggles (close Z-bends, opposite directions)

Die width	Minimum joggle distance
0.472″	0.700″
0.630″	0.900″
0.984″	1.200″
1.575″	1.500″

6. What bend angles are possible?

Parameter	Value
Minimum angle	5°
Maximum angle (standard)	130°
Thick stock (≥ 3/16″)	90° max

The exact range per material/thickness is shown in the app when you add the bend.

Angular tolerances

Condition	Tolerance
Sheet metal, bend ≤ 24″	±1°
Sheet metal, bend > 24″	±2°

7. When is a bend relief needed?

A bend relief is a small cutout at each end of a bend line that prevents the sheet from tearing or deforming when the bend runs into solid material.

Recommended for thicknesses ≥ 3/16″ (0.187″)
Recommended wherever a bend line meets an inside edge

Minimum dimensions per material are in the "Relief" column of the master table. When in doubt, this conservative rule works in all cases:

Depth ≥ R + T + 0.020″ · Width ≥ 50% × T

8. How do I calculate bend allowance and the flat pattern?

During bending, the sheet stretches in the bend zone. The flat pattern must account for that deformation through the bend allowance (BA) or the bend deduction (BD). If you upload a 3D STEP file, this calculation is done automatically with our real parameters.

BA = θ × (R + K × T) // θ in radians

BD = 2 × (R + T) × tan(θ/2) − BA

OSSB = (R + T) × tan(θ/2)

L_flat = L_{flange 1} + L_{flange 2} + BA

Example — Aluminum 5052-H32 14G, 90° bend

T = 0.064″ R = 0.047″ K = 0.459 θ = 90° = π/2 rad

BA = (π/2) × (0.047 + 0.459 × 0.064) = 0.120″

BD = 2 × (0.047 + 0.064) × tan(45°) − 0.120 = 0.102″

The "BD @ 90°" column in the master table gives the precomputed deduction for each material/thickness — the value to subtract per 90° bend if you're building your flat pattern by hand.

9. What tolerances should I expect?

Bending — ±0.015″ per bend, cumulative

Number of bends	Tolerance
1	±0.015″
2	±0.030″
3	±0.045″
4	±0.060″
5+	±0.015″ × n

Cutting

±0.005″ (±0.13 mm) on laser-cut profiles.

Design tip: dimension critical features from the same bend rather than chaining across several bends — bending tolerances stack up.

10. Part size constraints

Parameter	Value	Metric
Minimum part size	0.375″ × 1.500″	9.5 × 38 mm
Maximum part size	30″ × 44″	762 × 1118 mm
Maximum bend length	16″ to 44″ depending on material	406 to 1118 mm
Maximum bends	12 per part	—

11. U-channels: what base-to-flange ratio?

For a U-profile, the base (the panel between the two bends) must be wide enough relative to the flange height, otherwise the part collides with the tooling and cannot be air-bent.

Condition	Minimum ratio
Standard	Base ≥ 2 × flange height
Thin sheet (≤ 0.135″)	1:1 accepted if flanges ≤ 3.00″ and base ≥ 1.00″

12. Bending specifications per material

The master table below gives, for every bendable material and thickness at Laseo: the V-die, the inside radius, the K-factor, the minimum flange, the relief depth and the 90° bend deduction. All values in inches.

Material	T (in)	V-die	Inside radius	K-factor	Min flange	Relief depth	BD @ 90°
Aluminum
3003-H14 — 22G	0.025	—	0.039	0.380	0.200	0.038	0.064
5052-H32 — 18G	0.040	0.315	0.039	0.330	0.200	0.060	0.076
5052-H32 — 14G	0.064	0.472	0.047	0.459	0.285	0.096	0.102
5052-H32 — 12G	0.081	0.630	0.047	0.371	0.382	0.122	0.135
5052-H32 — 11G	0.091	0.630	0.047	0.400	0.382	0.137	0.145
5052-H32 — 10G	0.102	0.945	0.063	0.425	0.568	0.153	0.163
5052-H32 — 8G	0.129	0.945	0.157	0.420	0.568	0.194	0.242
5052-H32 — 3/16″	0.188	1.575	0.157	0.418	1.000	0.282	0.320
5052-H32 — 1/4″	0.250	1.969	0.312	0.392	1.155	0.375	0.480
Mild steel (hot rolled)
HR steel — 22G	0.030	0.315	0.055	0.289	0.200	0.045	0.070
HR steel — 18G	0.048	0.394	0.067	0.262	0.245	0.072	0.105
HR steel — 16G	0.060	0.472	0.075	0.288	0.285	0.090	0.125
HR steel — 14G	0.075	0.630	0.102	0.236	0.382	0.113	0.166
HR steel — 12G	0.105	0.945	0.146	0.295	0.568	0.158	0.224
HR steel — 11G	0.120	0.945	0.125	0.385	0.568	0.180	0.221
HR steel — 10G	0.135	0.945	0.125	0.418	0.568	0.203	0.235
HR steel — 3/16″	0.188	1.575	0.217	0.431	1.000	0.282	0.342
HR steel — 1/4″	0.250	1.969	0.272	0.379	1.155	0.375	0.468
Galvanized steel G90
G90 — 24G	0.028	0.315	0.055	0.218	0.200	0.042	0.070
G90 — 22G	0.034	0.315	0.055	0.330	0.200	0.051	0.070
G90 — 18G	0.052	0.394	0.067	0.340	0.245	0.078	0.105
G90 — 16G	0.064	0.472	0.075	0.350	0.285	0.096	0.125
G90 — 14G	0.079	0.630	0.102	0.288	0.382	0.119	0.166
G90 — 12G	0.108	0.945	0.146	0.322	0.568	0.162	0.224
Stainless steel 304
304 #2B — 22G	0.031	0.394	0.085	0.277	0.245	0.047	0.085
304 #2B — 18G	0.050	0.472	0.094	0.437	0.285	0.075	0.106
304 #2B — 16G / 1/16″	0.063	0.630	0.141	0.480	0.382	0.095	0.139
304 #2B — 14G	0.078	0.630	0.117	0.361	0.382	0.117	0.162
304 #2B — 12G	0.109	0.945	0.203	0.445	0.568	0.164	0.229
304 #2B — 11G	0.125	0.945	0.188	0.462	0.568	0.188	0.240
304 #2B — 7G	0.188	1.575	0.250	0.357	1.000	0.282	0.378
304 #1 — 1/4″	0.250	1.969	0.346	0.365	1.155	0.375	0.505
Stainless steel 316
316 #2B — 1/16″	0.063	0.630	0.141	0.480	0.382	0.095	0.139
316 #2B — 1/8″	0.125	0.945	0.188	0.462	0.568	0.188	0.240
316 #1 — 3/16″	0.188	1.575	0.250	0.357	1.000	0.282	0.378
316 #1 — 1/4″	0.250	1.969	0.346	0.365	1.155	0.375	0.505
Brass 260 (cartridge)
Brass 260 — 18G	0.040	0.320	0.039	0.370	0.200	0.060	0.076
Brass 260 — 14G	0.064	0.512	0.047	0.330	0.285	0.096	0.102
Brass 260 — 8G	0.129	1.032	0.157	0.300	0.568	0.194	0.242
Brass 260 — 3/16″	0.188	1.504	0.157	0.380	1.000	0.282	0.320
Brass 260 — 1/4″	0.250	2.000	0.312	0.330	1.155	0.375	0.480
Copper 110 ETP (half hard)
Copper 110 — 19G	0.043	0.344	0.039	0.390	0.200	0.065	0.064
Copper 110 — 16G	0.062	0.496	0.047	0.330	0.285	0.093	0.102
Copper 110 — 10G	0.134	1.072	0.063	0.340	0.568	0.201	0.163

13. The 6 most common design mistakes

1. Holes too close to the bend

Respect the minimum distance Die ÷ 2. Holes inside the die zone will be distorted.

2. Flange too short

The sheet slips in the die and the bend deforms. Meet the minimum flange from the material table.

3. No bend relief on thick material

Tearing risk at the ends of the bend. Add reliefs of depth R + T + 0.020″.

4. Bends too close together

Die zones overlap and pucker the metal. Keep 2 × minimum flange between parallel bends.

5. Channel too narrow

The base-to-flange ratio must be ≥ 2:1, or the part hits the tooling.

6. Forgetting the bend deduction

Without BD, the finished part will be larger than expected. Use the section 8 formulas or upload a STEP.

14. Quick reference

Rule	Value / formula
Feature-to-bend distance	≥ Die ÷ 2
Minimum flange length	See material table (≈ max(2T, T+R))
Distance between bends (46°–90°)	≥ 2 × minimum flange
Angles	5°–130° (standard), 90° max from 3/16″
Per-bend tolerance	±0.015″ cumulative
Cutting tolerance	±0.005″
Bend relief — depth	R + T + 0.020″
Bend relief — width	≥ 50% × T
Channel base-to-flange ratio	Base ≥ 2 × flange
Maximum bends per part	12
Part size	0.375″ × 1.500″ to 30″ × 44″

Question about a specific part? Write to info@laseo.ca or see the bending service page.

Design Guide — Sheet Metal Bending