← Back to All Guides
// Press Brake Reference

Bending Ontology

Every term, value, and constraint that defines a sheet metal bend — explained in one place, then mapped to live tooling data for every material we run on our TRUMPF press brake.

Xeon NC Bending Ontology — part, tooling and formed bracket

An "ontology" is simply the shared vocabulary that lets a designer and a machine agree on exactly what a bend is. Get the words right and the geometry follows — get them wrong and you ship a flat pattern that folds into the wrong part.

This guide defines the core bending terms the same way you'll see them in our instant quoting platform and on a press brake controller, then connects each one to the actual K-factor, radius, tooling, and bend deduction values we use in production. Use the material lookup tool below to pull the exact numbers for the material and thickness you're designing in.

The Bending Vocabulary

These are the building blocks of every formed part. Each card explains the term, its common abbreviation, and how it affects your design.

Bend Angle deg
The angle the flange is formed through. We quote the included angle (90° = a right-angle bend). Air bending on our brake covers 30° to 135°.
Inside Bend Radius IR
The radius left on the inner surface of the bend. Driven by the V-die width (roughly 0.16 × die opening), not the punch tip. A larger radius is gentler on the material.
Bend Deduction BD
The length removed from the sum of the outside flange dimensions to get the correct flat blank. Flat = A + B − BD. Listed per angle in the tool below.
Bend Allowance BA
The arc length of the neutral axis travelling through the bend. It's the material consumed by the curve itself and is the basis from which bend deduction is derived.
K-Factor K
The ratio that locates the neutral axis inside the thickness: K = t / MT. It's the single most important constant for accurate flats. Each material/temper has its own — see the tool.
Neutral Axis
The plane through the thickness that is neither stretched nor compressed during forming. Under load it shifts inward toward the punch — which is exactly why the K-factor is never simply 0.5.
Setback / Mold Line
The distance from the bend tangent line to the apex where the two outside flange planes would intersect. Setback plus bend allowance is what reconciles "dimension to the corner" with the real flat.
Minimum Formed Flange
The shortest leg the V-die can fully support and form without slipping into the die gap. Roughly 0.63 × die opening. Designing below it risks a malformed or unsafe bend.
Bend Relief
A small slot cut where a bend ends mid-sheet. At least 1× material thickness wide, it stops the metal tearing or buckling at the transition between bent and flat regions.
Springback
The elastic recovery that opens the angle slightly after the punch retracts. Harder tempers (6061-T6, 7075) spring back more; our ACB laser measures and compensates in real time.
V-Die Opening V
The width of the lower die's V. It sets the inside radius, the minimum flange, and the tonnage. We select V ≈ 8 × thickness from a 5-die TRUMPF set.
Tonnage / Grain
Tonnage is the force needed to form the bend (scales with length, thickness and die). Grain direction is the rolling direction — bend perpendicular to it to avoid outer-fiber cracking.

What Is Bend Deduction?

Bend deduction is the bridge between the part you model in 3D and the flat blank our laser actually cuts. When sheet metal bends, the outer surface stretches and the inner surface compresses, so the developed (flat) length is shorter than the sum of the outside leg dimensions. Bend deduction is exactly how much shorter.

Bend deduction illustration — formed bracket beside its flat pattern
The formed part (solid) vs. its developed flat pattern (outline). Bend deduction accounts for the difference.
Flat Length Formula ───────────────────────────────────────── Flat Length = Flange A + Flange B − Bend Deduction Where: Flange A, B = outside dimensions to the bend apex Bend Deduction depends on: • Material & temper (K-factor) • Material thickness • Inside bend radius • Bend angle Example — 0.060″ (16 ga) 304 stainless, 90°: BD ≈ 0.120″ per bend (from the table below)
Why it changes per angle: a 30° bend removes far less material than a 135° bend, so bend deduction is listed for every angle from 30° to 135° in the lookup tool — pick the angle you're actually forming.

Minimum Formed Flange

The minimum formed flange (or minimum leg length) is the shortest flange the press brake can reliably form. The flange has to bridge the V-die opening with enough material on both shoulders for the die to support it. Go shorter and the part slips into the die, producing a rolled, malformed, or dangerously launched bend.

Minimum formed flange shown in the Xeon NC quoting platform with a warning flag
Our quoting platform flags flanges below the minimum formable length before you order.

Because it scales with the die — and the die scales with thickness — the minimum flange grows as material gets thicker:

  • Rule of thumb: minimum flange ≈ 0.63 × V-die opening, where the V-die is about 8× the material thickness.
  • Thin sheet (24–16 ga): minimum flange around 0.20″–0.30″.
  • Heavier plate (3/16″–1/4″): minimum flange climbs past 0.74″–1.24″.

The exact minimum flange for your chosen material and thickness is shown in the lookup tool below.

Bending Specifications Per Material

Select a material and thickness to pull its TRUMPF tooling assignment, K-factor, inside radius, minimum formed flange, and air-bend deduction at every angle. These are the same reference figures we form to in production — verify on a test bend before committing critical flats.

Choose a material above to view its technical bend data.

K-source family indicates the calibrated material whose K-factor was applied. Alloys without direct data (6061, 7075, 1100, Corten, AR500, spring steel) are proxied to the closest family — see the flag on each card. Tooling: 5-die TRUMPF set, V-die ≈ 8× thickness, air bend, dimensions in inches.

Bend Deduction & Allowance Charts

The full reference tables, the way you'd pin them up next to the brake. Pick a material, then read bend deduction (or bend allowance) straight off the row for your thickness and the column for your angle. These are computed from our actual TRUMPF tooling — the same numbers behind the lookup tool above.

Material
Value
Angles
Highlighted columns are the common press-brake angles (30 / 45 / 60 / 90 / 120 / 135°).
Reading the chart: bend deduction is subtracted from the summed outside flange dimensions to get your flat length — Flat = A + B − BD. Bend allowance is the developed length of the bend itself. Both assume air bending at the inside radius and K-factor shown for that gauge.

Designing Your Flat With This Data

Putting the vocabulary and the numbers together, here's the order of operations for a clean first-article part:

  • 1. Pick material & thickness — this fixes your V-die, inside radius, K-factor, and minimum flange in one move. Look them up above.
  • 2. Check every flange against the minimum formed flange. Lengthen any leg that falls short, or plan a secondary operation.
  • 3. Apply bend deduction per bend at the actual angle you're forming to develop the flat pattern. Multiply by the number of bends.
  • 4. Keep features clear of the bend — hold holes and slots back at least 2× MT + IR from the tangent line (see our Bend Affected Zone guide).
  • 5. Add bend reliefs wherever a bend terminates mid-sheet, at least 1× thickness wide.
  • 6. Specify the inside radius on your drawing — don't leave it to chance. The tool gives you the radius our tooling actually produces.
Let us do the math: upload a STEP file to our instant quote and the platform applies all of these values automatically — flagging short flanges and over-range thicknesses before you ever place the order.

Ready to form your part?

Upload your flat pattern or 3D model and our press brake programmers will confirm tooling, K-factor, and bend deduction for your exact material — free of charge.

Upload Your Design