Press Brake Basics Explains How CNC Bending Actually Works

• 1
  Key takeaways
• 2
  What a press brake does to the metal
• 3
  V-opening, inside radius and flange length
• 4
  Why the angle springs back and how to compensate
• 5
  Tonnage, bend length and the limits of the machine
• 6
  Design rules that keep a bend manufacturable
• 7
  How a CNC press brake job runs, step by step
• 8
  Air bending vs bottoming vs coining
• 9
  What bending can and cannot hold

A press brake is a machine that applies a vertical load to a sheet metal blank sitting on a die. The punch comes down, contacts the sheet, and pushes it into the V-opening. The material yields, then plastically deforms around the punch nose. The angle it reaches depends on how far the ram travels, not on how hard the machine pushes.

That distinction matters. On a manual brake, the operator sets ram depth by feel and by a mechanical stop. On a CNC press brake, the controller positions the ram and the back gauge from a stored program, so the same bend repeats within a few hundredths of a degree without re-setting. The forming mechanics are the same. The repeatability is not.

Three families cover most work. Air bending leaves a gap between punch and die; the angle is set by depth. Bottoming drives the punch until the material touches the die walls, which fixes the angle more tightly and needs more tonnage. Coining presses the punch fully into the material and forces the angle to match the tool exactly, but requires several times the tonnage and leaves a thinner bend line.

Air bending is what we use for most production parts. It tolerates material thickness variation better than bottoming, needs the least force, and lets one punch and die set produce many angles. When a drawing calls for an angle held to ±0.5° or better on thin material, bottoming is the more honest choice.

• 1
  Punch nose radiusOften sets the inside corner radius when it is larger than the natural radius.
• 2
  V-opening widthControls the bending force and the achievable minimum flange.
• 3
  Back gaugePositions the blank along the bend line; its stop face defines the flange length.

The V-die opening is the single most useful number on a bending job. For air bending, the inside radius follows the die, not the punch. On mild steel the rule of thumb is inside radius ≈ V-opening ÷ 6. An 8 mm V-die gives roughly a 1.3 mm inside radius regardless of the punch nose.

This rule shifts with material. Aluminum 5052 and 6061 need a slightly larger radius for the same opening because they crack at tighter bends. Stainless 304 work-hardens quickly, so a generous radius reduces the risk of surface tearing at the outside of the bend.

Flange length is the other constraint. If the flange is too short, it will not span the V-opening and the part can drop into the die. A practical floor is four times the material thickness plus the inside radius. Below that, use a narrower die or a different process.

The minimum die opening is also bounded by force. Force rises as the V-opening narrows. Halving the opening roughly doubles the tonnage per meter. Thin dies on a small machine quickly run out of capacity, so the die is chosen against both geometry and the press tonnage chart.

Metal does not stop moving when the punch lifts. Elastic recovery pulls the bend open. On 1.5 mm mild steel the springback is typically 1–3°. On 304 stainless or 7075 aluminum it can run higher because the yield strength is higher relative to the elastic modulus.

Two things reduce it. The first is overbending: program a shallower ram depth so the material is pushed past the target angle and then relaxes back onto it. This is how air bending hits a nominal 90° without touching the die walls.

The second is die geometry. A narrower V-opening increases the plastic strain at the bend and reduces the elastic share. That is why a tight die holds angle better, at the cost of higher tonnage and a smaller inside radius.

For parts that must hold ±0.25° across a batch, temperature and material lot still move the number. The controller compensates from its stored table, but the first article is always measured on a protractor or an optical angle gauge before the run is released.

• 1
  Measure the first partCheck angle at both ends and the middle of the bend line.
• 2
  Log the material lotA different heat of stainless can shift springback by a degree.
• 3
  Check grain directionBending across the rolling direction behaves differently than with it.

Tonnage is not a constant. It scales with material thickness squared, with bend length, and inversely with the V-opening. A 1 m bend in 3 mm mild steel on an 24 mm V-die needs far less force than the same bend in 6 mm steel, which needs roughly four times as much.

The press brake rating is the maximum force at mid-span. On a long bed, the ram and bed deflect under load. A 3 m part bent near the center will open up in the middle unless the machine has crowning or the tooling is shimmed. This is the most common cause of a part that measures 90° at the ends and 92° in the middle.

Bend length also drives tooling choice. Punches and dies are supplied in segments so a short bend can be made without loading the full bed. Segmented tooling lets us bend a 200 mm flange on a 4 m machine without the tonnage penalty of a full-length tool.

We treat the tonnage chart as a limit, not a target. Running a brake at 90% of rated capacity shortens tool life and makes the angle less stable. If a job needs more force, the answer is usually a wider die, a different tool, or a different process.

Most bending problems are created at the drawing stage. A flange that is 3 mm on 2 mm steel cannot be formed reliably; the material will not span the die. Move the bend line or thicken the flange.

Holes and slots near a bend line distort. Keep them at least 2.5 times the material thickness plus the inside radius away from the bend, or the hole will pull oval as the material stretches.

Bends that collide with each other are the next issue. Two bends 5 mm apart on a 90° part can leave no room for the punch body. Check the tool clearance, not just the finished geometry.

Finally, consider the bend sequence. A box with four flanges cannot be formed in one pass. The order matters, and a part designed without that order in mind may need a special tool or a different corner relief. A quick DFM review catches this before the tooling is set.