CNC Bending Basics: How a Press Brake Really Forms Your Part

• 1
  What Happens Inside a Bend
• 2
  Air Bending, Bottoming and Coining
• 3
  Springback and the Bends That Fail
• 4
  What to Put on the Drawing
• 5
  Bending Method Compared

A press brake does not fold sheet metal the way you fold paper. The punch pushes the sheet into a V die, and the material on the inside of the bend compresses while the outside stretches. Between them sits the neutral axis, a layer that keeps its original length. Everything else in bending follows from that split.

The position of the neutral axis is described by the K-factor, usually 0.33 to 0.50 for cold-rolled steel. It shifts outward as the inside radius grows relative to thickness. If you assume K = 0.5 in your flat pattern and the shop forms at K = 0.40, your blank comes up short and the flange lands off position.

Tonnage is the second control. Required force scales with thickness squared, so doubling 1.0 mm stock to 2.0 mm takes roughly four times the load. A 1,000 mm air bend in 2.0 mm mild steel needs about 40 to 50 tonnes per meter. Exceed the tooling limit and you crack the punch, not the part.

Bend allowance ties the two together. It is the arc length along the neutral axis and it decides how much flat stock you need. Shops calculate it from the radius, angle and K-factor, then add bend deduction for outside dimensions. Give us a 3D model and a drawing with the tolerance callout, and we check the flat pattern before cutting.

• 1
  Neutral axisThe layer that keeps its original length through the bend.
• 2
  K-factor0.33–0.50 for cold-rolled steel; rises with radius-to-thickness ratio.
• 3
  TonnageScales with thickness squared, not thickness.

Three methods cover almost every job, and they trade accuracy against force. Air bending sets the punch to a depth short of full contact. The sheet touches the die shoulders only, the angle is set by ram position, and a single tool set can produce 90°, 120° or 60° without a die change.

Bottoming drives the punch until the sheet contacts the die walls. The angle comes from the tooling geometry, so repeatability is tighter than air bending. The trade-off is force: bottoming needs roughly three to five times the tonnage of air bending, and the tool set is locked to one angle.

Coining presses the punch fully into the sheet, thinning the bend zone and forcing material to the die shape. It removes springback almost completely and holds angles to about ±0.25°. It also needs five to ten times the air-bend tonnage, which rules out thin tooling and most small press brakes.

Pick by quantity and angle range. Mixed angles in low volume go to air bending. A single angle at high volume goes to bottoming or coining, where setup cost disappears into the run and the angle stays put across thousands of strokes.

• 1
  Air bendingFlexible angle, low tonnage, springback must be compensated.
• 2
  BottomingTighter angle, 3–5× the tonnage, one angle per tool set.
• 3
  Coining±0.25° repeatability, 5–10× the tonnage, no springback correction.

Springback is elastic recovery after the ram releases. Every metal springs back a little; high-strength steel and 304 stainless spring back more than 1018 mild steel. The controller compensates by overbending, typically 1° to 3° for mild steel and 5° to 10° for 304 or 5052 aluminium.

Radius-to-thickness ratio decides whether the bend survives. Below about 1× thickness, the outer fibers strain past their limit and you get cracking on the outside, especially in 7075 aluminium or 440C stainless. Keep the inside radius at 1× thickness or larger for ductile alloys, higher for hard ones.

Grain direction matters too. Bending parallel to the rolling direction cracks sooner than bending across it. On a part with tight radii in 5052 or 304, rotate the blank 90° in the nest and the same bend forms clean.

Other failures show up as flange length and hole placement. A flange shorter than about 4× thickness cannot sit on both die shoulders, so the angle drifts. Holes within 2.5× thickness of the bend line distort into ovals. Move them or add a relief slot, and the problem disappears before the first part is cut.

• 1
  Springback1–3° mild steel, 5–10° for 304 and 5052.
• 2
  Minimum inside radiusAbout 1× thickness for ductile alloys, more for hard ones.
• 3
  Minimum flangeAround 4× thickness to seat on both die shoulders.
• 4
  Hole distanceKeep holes 2.5× thickness away from the bend line.

A STEP file alone does not tell the shop which surface is the datum. Send a drawing with the bend line, the inside radius, the angle and its tolerance, and the material temper. On a bracket with three bends, the sequence and the datum face decide whether the last flange closes to ±0.5 mm or drifts to ±1.5 mm.

Call out tolerances you can live with. Sheet metal angles usually hold ±1° air bent and ±0.5° bottomed. Linear dimensions across a formed part stack up from bend deduction, material thickness variation and springback, so ±0.2 mm across three bends is a machining job, not a forming job.

Material thickness tolerance drives more scrap than most designers expect. Hot-rolled A36 can vary ±0.3 mm on a nominal 3.0 mm sheet, which moves the neutral axis and the flat pattern. If thickness is critical, specify cold-rolled or pick a machined part instead.

For prototypes, one bend radius and one material keep the tooling simple. We quote from the model and the drawing together, run a DFM check inside 12 hours, and flag any bend that will not form before we cut metal. From one prototype to 10,000+ parts, the same rules apply; only the method changes.

• 1
  Always sendSTEP plus PDF or DWG with bend lines, radii and angle tolerances.
• 2
  Datum faceMark it. The bend sequence is built around it.
• 3
  ThicknessState the temper and the acceptable thickness range.