Press brake bending turns a flat laser-cut blank into a three-dimensional part by forcing it into a V-die with a punch — and three variables decide whether it fits: bend radius, springback, and tolerance stack-up. Get one wrong and a bracket that looked perfect in CAD arrives two degrees open or 1.5 mm short across a datum. On our shop floor in Satellite, Ahmedabad, we run a 160-tonne press brake with a 3200 mm bed, and most drawings we reject fail not on the machine but on geometry the designer never checked: an inside radius no die can form, a flange too short to clear the V-shoulder, or a hole inside the deformation zone. This guide explains how press-brake bending behaves in mild steel, stainless, and aluminium, what tolerances you can hold under DIN 6935 and ISO 2768, and how to draw bends that come off the tooling right the first time.
Key Takeaways
- Radius follows the die: in air bending the inside radius floats to about 16% of the V-die opening — the punch nose barely matters.
- Springback is material-driven: mild steel opens 1–3°, stainless 3–7°; you compensate by overbending, not by re-clamping.
- Flat patterns need a K-factor: get the neutral-axis shift right (K ≈ 0.38–0.45) or every downstream dimension drifts.
- Datum discipline holds tolerance: dimension every bend from one face to keep stack-up inside ±0.2 mm.
- Layer X capacity: 160-tonne brake, 3200 mm bed, CMM-verified first article, 3–5 day lead, no minimum order.
The three ways a press brake forms metal
Every bend on a press brake uses one of three methods, and the choice sets your tonnage, radius, and springback before the ram even moves.
- Air bending — the punch presses the sheet into the V without touching the die bottom, so the angle is set purely by ram depth. Lowest tonnage and most flexible (one tool set bends many angles), but the highest springback.
- Bottoming — the sheet is pressed hard against the die walls at the target angle. Springback drops and the radius repeats tightly, but you need a die per angle and two-to-four times the force.
- Coining — the punch is driven into the material until it plastically flows into the die nose. Near-zero springback and a radius equal to the punch tip, at five-to-eight times air-bend tonnage.
For the brackets, enclosures, and chassis we form in Ahmedabad, air bending is correct roughly 95% of the time: fast, tooling-light, and repeatable to ±0.5° once depth is dialled in. We reserve coining for thin, safety-critical tabs where the radius must be exact. Choosing the method early is the biggest single lever on cost — coining a 6 mm plate that only needed air bending can triple the required tonnage.
Bend radius is set by the die, not the punch
The drawing error we correct most often is a specified inside radius no standard tool can make. In air bending the inside radius is not the punch-tip radius — it is a floated radius the material forms naturally, close to 16% of the V-die opening (the "five-thirty-seconds rule"). Because the die opening runs 6–8× material thickness, the practical inside radius lands near one material thickness in mild steel.
Under the air-bending geometry codified in DIN 6935, the natural inside radius is roughly 0.16 × the die opening; specifying a radius tighter than one material thickness in steel risks outer-fibre cracking along the bend line.
| Thickness (mm) | V-die (mm) | Inside radius (mm) | Min flange (mm) | Air-bend force (t/m) |
|---|---|---|---|---|
| 1.0 | 8 | 1.3 | 5.5 | 5 |
| 2.0 | 12 | 2.0 | 8.5 | 13 |
| 3.0 | 20 | 3.3 | 14 | 18 |
| 6.0 | 40 | 6.6 | 28 | 40 |
| 10.0 | 80 | 13 | 56 | 57 |
So a 3 mm mild-steel part drawn with a 1 mm inside radius cannot be air-bent — the tool that gives 1 mm needs a ~6 mm V, which will not form 3 mm plate. Draw the radius the tooling actually produces. When a part reaches our CNC sheet-metal line we flag any radius the dies cannot hit before it ever gets to the brake.
Springback: why press-brake bending opens up
Steel remembers. When the ram retracts, the elastic part of the strain recovers and the angle opens — a 90° form relaxes to 91–93° in mild steel and as far as 97° in half-hard stainless. Springback grows with tensile strength and with the radius-to-thickness ratio, so a wide-radius bend in 316 fights you far harder than a tight bend in mild steel. You cannot clamp it out; you compensate for it.
- Overbend the ram depth so the part relaxes back to the target angle.
- Move toward bottoming to shrink the elastic recovery.
- Bend a coupon from the same coil and heat, then read the real angle.
- Bend perpendicular to the rolling direction to keep recovery even.
| Material | Tensile (MPa) | Springback (air bend) | Overbend strategy |
|---|---|---|---|
| Mild steel (IS 2062) | ~410 | 1–3° | Overbend 2–3°, IR ≈ T |
| 304 / 316 stainless | 515–690 | 3–7° | Overbend 5–8°, IR ≥ 1.5T |
| 5052 / 6061 aluminium | 210–310 | 3–6° | IR ≥ 1.5–2T, bend across grain |
On a recent DRDO-tier enclosure in 2 mm 304, the first coupons sprang back to 94°. We reprogrammed to overbend to 86°, re-ran the coupon, and locked the depth — all 40 parts then measured 90° ±0.4° on the CMM. That coupon-first discipline is why press-brake bending should be quoted with a first-article check, not trusted to a nominal springback table.
Flat-pattern math: K-factor and bend allowance
A bent part is laser-cut flat first, so the flat blank must already account for the material that wraps each bend. The neutral axis — the plane that neither stretches nor compresses — shifts toward the inside of the bend; its position as a fraction of thickness is the K-factor, typically 0.38–0.45 for air-bent steel. The material added by each bend is the bend allowance, BA = (π/180) × angle × (IR + K·T).
- Fix the inside radius and K-factor for the material and bending method.
- Compute the bend allowance for every bend angle on the part.
- Flat length = sum of the flat flanges plus the bend allowances.
- Nest, laser-cut the blank, then verify the first bend against the model.
A wrong K-factor is subtle but expensive: use 0.5 instead of 0.42 on a four-bend chassis and each bend adds ~0.15 mm, so the box arrives 0.6 mm oversize — enough to miss a mating hole pattern. Because we cut blanks on our own 3 kW fibre laser and bend them on the same floor, the flat pattern and the tooling data come from one model — the K-factor used to cut is the one used to bend.
Tolerances press-brake bending can actually hold
Press-brake tolerance is not a single number — it depends on how many bends stack between the feature and the datum. One bend to an edge is easy; four bends compounding from a floating datum is where parts drift out of print.
ISO 2768-1 "medium" allows ±0.3 mm on lengths of 30–120 mm as a general tolerance; well-controlled press-brake bending routinely beats this, but only when every bend is dimensioned from one datum face rather than chained bend-to-bend.
| Feature | Standard brake | Precision (coined / CMM-checked) |
|---|---|---|
| Bend angle | ±1° | ±0.5° |
| Bend-to-edge (single bend) | ±0.2 mm | ±0.1 mm |
| Bend-to-bend (multi-datum) | ±0.3 mm | ±0.15 mm |
| Hole-to-bend | ±0.2 mm | ±0.1 mm |
Two habits keep us inside these bands: dimension from a single datum, and check the first article on the CMM before the run. On a HAL-supplier bracket we held ±0.1 mm bend-to-edge across a three-bend part by machining the datum edge first and bending to it — the CMM report shipped with the parts as full material traceability. Chain the same dimensions bend-to-bend instead and you would need ±0.4 mm just to absorb the stack-up.
Design rules that keep press-brake bending manufacturable
Most bending problems are designed in, not machined in. A short checklist prevents the expensive ones:
- Minimum flange ≥ 0.7 × die opening — a shorter flange drops into the V and folds unevenly.
- Hole or slot ≥ 2.5·T + radius from the bend — closer and the hole pulls into an oval.
- Add bend relief notches (≥ T wide, ≥ radius deep) where a bend meets an edge, to stop tearing.
- Keep every bend one thickness and, where you can, one radius — fewer tool changes, faster, cheaper.
- Bend across the grain in aluminium and high-strength steel to avoid cracking.
The minimum-flange rule catches people most: on a 6 mm part in a 40 mm V, any flange under ~28 mm cannot be formed reliably — the metal has nothing to sit on. If your design needs a shorter leg, we switch to a narrower die (tighter radius, more tonnage) or add a machined step. Send the STEP file to our sheet-metal bending team and you get a 24-hour, engineer-reviewed quote that flags exactly these issues before you commit to tooling.
Frequently Asked Questions
What is the minimum bend radius for sheet metal?
For mild steel, keep the inside radius at or above one material thickness; stainless and high-strength alloys need 1.5–2× thickness to avoid outer-fibre cracking. In air bending you rarely choose the radius directly — it floats to about 16% of the die opening. Design to the radius your shop's tooling produces, not an arbitrary CAD default.
Why does my bent part open up after forming?
That is springback — elastic recovery when the ram releases. Mild steel opens 1–3°, stainless up to 7°. We compensate by overbending the ram depth and confirming on a test coupon from the same heat, so the part relaxes back to nominal.
How thick a plate can you bend?
Our 160-tonne brake air-bends up to ~8 mm mild steel across the full 3200 mm bed, or ~10 mm over a shorter length, because tonnage scales with bend length. Thicker or longer bends split into shorter forms or move to a higher-tonnage partner. We size this at quote time.
Do you provide inspection reports with bent parts?
Yes. First articles are CMM-verified and shipped with a dimensional report and full material traceability to the coil heat. That is standard on our AS9100 and ISO 13485 lines, at no minimum order quantity.
Press-brake bending only looks simple: the radius, springback, and stack-up are all decided before the first part forms, and fixing them on the shop floor costs far more than fixing them in CAD. Send us your STEP or DXF and our engineers will return a manufacturability review — flagging radii, flange lengths, and datums — inside one working day. Request a 24-hour quote.