Press Brake Forming: Bend Radius, Tolerances and Design Rules

How air bending, die opening and material choice set bend radius and tolerance, plus the design rules that keep bent sheet and plate parts out of rework.

Updated October 2026 5 min read By the ASA team

On this page
  1. Air bending vs bottoming vs coining
  2. V-die opening and inside bend radius
  3. Design rules for bent parts
  4. Springback and angular tolerance
  5. Press brake tonnage basics
  6. Press brake forming at ASA

Press brake forming bends sheet and plate along a straight line by pressing it between a punch and a V-shaped die. Most parts today are air bent on CNC press brakes, where the bend angle is set by how far the punch travels into the die and the inside radius is set mainly by the die opening.

Good bent parts start at the drawing. Choosing a realistic inside radius, keeping flanges long enough and holding holes back from bend lines prevents cracking, distortion and expensive rework. The rules below are typical industry guidance; confirm critical values with your fabricator for the exact material and thickness.

Air bending vs bottoming vs coining

There are three basic ways to form a bend on a press brake. They differ in how much the punch forces the material into the die, which changes accuracy, tonnage and tooling needs.

MethodHow it worksTonnageTypical use
Air bendingPunch presses the sheet partway into the V; material touches only the punch tip and die shouldersLowestMost CNC work; one die set covers many angles
BottomingPunch presses the sheet against the die walls, so the die angle sets the bend angleConsiderably higher than air bendingTighter angle consistency on thinner sheet
CoiningPunch tip penetrates and thins the material at the bend, eliminating springbackOften five times air bending or moreVery tight radii and angles on thin gauge

Air bending dominates because it is flexible and gentle on the machine. Modern CNC back gauges, crowning and angle measurement systems have closed much of the accuracy gap that once made bottoming and coining necessary.

V-die opening and inside bend radius

The standard rule of thumb for mild steel is a V-die opening of about 6 to 8 times material thickness. Eight times thickness is the common starting point for sheet, and heavier plate usually moves to 10 times thickness or more to keep tonnage and cracking risk under control.

In air bending, the inside radius forms as a percentage of the die opening, not the punch radius. Approximate values:

  • Mild steel: inside radius of about 15 to 17% of the V opening
  • 304 stainless: about 20 to 22% of the V opening
  • 5052-H32 aluminum: about 13 to 15% of the V opening

For example, 0.125 in (3.2 mm) mild steel in a 1.00 in (25 mm) V die forms an inside radius of roughly 0.16 in (4 mm). If the drawing calls for a very different radius, the fabricator has to change tooling or method, so call out the radius you actually need and leave it open where it does not matter.

Minimum inside bend radius by material

Bending tighter than a material can tolerate cracks the outside of the bend. The table shows typical minimum inside radii for bends made across the rolling direction, expressed as multiples of thickness (T).

MaterialTypical minimum inside radius
Cold rolled carbon steel (C1008, C1010)0.5T to 1T
Hot rolled carbon steel and A36, up to 1/2 in (12.7 mm)1T to 1.5T
Carbon steel plate over 1/2 in (12.7 mm)1.5T to 2T or more
HSLA sheet1.5T to 2.5T, depending on grade
304, 316 and 430 stainless1T
3003-H14 aluminum0.5T to 1T
5052-H32 aluminum1T to 1.5T
5052-H34 aluminum1.5T to 2T

Higher carbon grades such as C1045 and C1050 are much less forgiving and usually need larger radii. Bending parallel to the rolling direction raises the minimum for every material, so orient tight bends across the grain when you can.

Design rules for bent parts

Minimum flange length

A flange has to span the die opening during the bend or it will slip into the V. A common shop guideline puts the minimum flange at about 0.7 times the V-die opening, which works out to roughly 4 times thickness with a 6T die and about 5.5 times thickness with the standard 8T die. Short flanges on thick material force a narrower die, a smaller radius and more tonnage, so lengthen them when the design allows.

Hole-to-bend distance

Holes and slots too close to a bend stretch into ovals. A typical guideline is to keep the edge of a hole at least 2.5 times thickness plus the inside bend radius away from the bend. Elongated slots parallel to the bend need more room, and features that must sit closer usually have to be cut after forming.

Bend relief and edge distance

Where a bend ends inside the part outline, add a relief cut at least as wide as the material thickness and deep enough to clear the bend radius. Without relief, the corner tears or bulges. Laser cutting makes reliefs and small features cheap to add, which is one reason flat blanks for forming are usually laser cut (see laser vs plasma cutting).

Flat pattern and K-factor

The flat blank has to account for the material that stretches through each bend. Fabricators use a K-factor, typically 0.3 to 0.5 for air bending, to locate the neutral axis. Let your fabricator develop the flat pattern from your formed dimensions so it matches their tooling.

Springback and angular tolerance

Every bent part springs back a little when the punch retracts. Mild steel commonly opens up about 1 to 2 degrees on a 90 degree air bend, while stainless and high-strength steels spring back noticeably more. CNC press brakes compensate by overbending, and angle measurement systems correct the stroke in real time.

Typical commercial tolerances for CNC air bending are about ±0.5 to ±1 degree on angle and roughly ±0.010 to ±0.020 in (±0.25 to ±0.5 mm) per bend on sheet. These are industry norms, not guarantees, and dimensional error stacks up across multiple bends. Dimension from one datum and tolerance only what affects fit or function.

Tip: Material variation drives most bend inconsistency. Specify the same alloy, temper and thickness tolerance for every lot of a repeat part, and consult a sheet metal gauge chart so gauge callouts match actual decimal thickness.

Press brake tonnage basics

The classic air bending formula for mild steel (about 60 ksi or 414 MPa tensile) is:

Tons per foot = 575 x T² / V, with thickness (T) and die opening (V) in inches.

Multiply by about 1.5 for 304 stainless and roughly 0.5 for 5052-H32 aluminum. A few worked examples, each using an 8T die opening, show how fast tonnage grows with thickness and length:

Material and thicknessV openingTons per footTotal at bend length
Mild steel, 0.25 in (6.4 mm)2 in (51 mm)About 18About 180 tons at 10 ft (3.0 m)
Mild steel, 0.50 in (12.7 mm)4 in (102 mm)About 36About 720 tons at 20 ft (6.1 m)
Mild steel, 0.75 in (19 mm)6 in (152 mm)About 54About 1,080 tons at 20 ft (6.1 m)

Bottoming and coining multiply these numbers. Fabricators also derate for off-center loads and keep a safety margin, so a part that calculates close to a machine’s rating may need a larger press brake.

Press brake forming at ASA

ASA forms carbon steel, stainless and aluminum on CNC press brakes, up to 385 tons at the Liverpool, NY facility, for prototype through production quantities. A 1,500-ton, 20-foot press brake is being added at the Saco, Maine facility in Q1 2027. Blanks can be cut, formed and welded under one company as part of ASA’s precision sheet metal manufacturing; see press brake forming for capabilities.

Frequently asked questions

What is the most common press brake forming method?

Air bending is the most common method on modern CNC press brakes. The punch pushes the sheet only partway into the V-die, so one set of tooling can produce many bend angles by changing stroke depth. It needs far less force than bottoming or coining, and machine controls compensate for springback to hold consistent angles.

How do I choose the right V-die opening?

For mild steel, start with a die opening of about 6 to 8 times the material thickness, with 8 times being the usual default for sheet. Thick plate often moves to 10 times thickness or more. A wider opening lowers tonnage and produces a larger inside radius, while a narrower one tightens the radius but demands more force.

Why do parts crack on the outside of a bend?

Cracking usually means the inside radius is too tight for the material, the bend runs parallel to the rolling direction, or the blank edge was hardened by thermal cutting. Increasing the radius, rotating the blank so bends cross the grain, choosing a softer temper or preparing the edge before forming typically solves the problem.

What angular tolerance can a press brake hold?

Typical commercial air bending on CNC press brakes holds about ±0.5 to ±1 degree, and machines with in-process angle measurement can do better. Actual results depend on material consistency, thickness, part length and tooling condition. Tolerance only the bends that affect fit or function, since tighter callouts add inspection time and cost.

How much tonnage does a press brake need?

For air bending mild steel, a common estimate is 575 times thickness squared divided by die opening, giving tons per foot of bend with dimensions in inches. Multiply by bend length, then adjust for material: about 1.5 times for 304 stainless and about half for 5052-H32 aluminum. Add a safety margin before choosing a machine.

Material, processing and fabrication from one supplier

Send a drawing or a material list and the ASA team will quote it from stock.