Key takeaways
- Leave the formed model at nominal 90°. Springback compensation belongs in the die face, the bend table or the control, not in the geometry your customer measures.
- Expect 1–2° on mild steel and CRCA, 2–3.5° on 304 stainless and 2–4° on 5052 aluminium at a 90° bend with an inside radius near one thickness.
- A 2.5° springback needs a bottom-dead-centre angle of 87.5°, and the resulting tip error on a 100 mm flange is 4.37 mm if the correction is missing.
- Springback also grows the inside radius, which changes the bend deduction: 2.0 mm to 2.2 mm on 2 mm CRCA shortens the flat by 0.09 mm per bend.
A designer bends a bracket to 90° in CAD, checks the flange heights, releases the drawing, and the first article comes back at 92.5°. The model was right and the part is right by the same logic — the material recovered after the punch lifted, and nothing in the model or the drawing anticipated it.
Springback in CAD is usually framed as a modelling problem. It is not. The finished part is 90°, the model should be 90°, and the 2.5° of recovery is a property of the grade, the tool and the bend, which the press has to absorb. Building the recovery into the model moves the error into the drawing, the flat pattern and the assembly, where it is harder to remove.
The useful questions are how much recovery to expect, where to put the correction, and which parts are the exception where the die face genuinely has to be cut 2–3° off nominal.
Should springback in CAD be compensated in the model?
No, for a formed part. Yes, for a die face.
A formed part model is the geometry the assembly needs. Holes, flanges and mounting faces are positioned against mating parts, so bending the model to 87.5° to anticipate recovery puts every downstream dimension 2.5° away from the design intent. The customer measures the model, the CMM program is written to the model, and the drawing dimension no longer matches either.
A stamping die is different. The die face is a tool, not a part, and it can be cut with the recovery already subtracted. That is where CAD-level compensation belongs: the tool geometry is generated off the nominal part, then adjusted by the predicted springback, then proved on tryout. The part model stays nominal and the tool carries the correction.
How much springback to expect, by grade
The ranges below are for a 90° air bend with an inside radius near one thickness and a die opening of about 8 × thickness. They are starting points for a bend table, not a guarantee: yield strength varies within a grade, and a high-yield coil of the same specification can recover half a degree more.
| Material | Springback at 90°, R ≈ t | What it does to the part | Ganesh note |
|---|---|---|---|
| CRCA / mild steel | 1.0–2.0° | Tip moves 1.7–3.5 mm on a 100 mm flange | 200 T, 5-axis brake to 10 mm |
| Galvanised mild steel | 1.0–2.0° | Coating adds scatter at the bend line | Zinc-rich surface marks; punch radius matters |
| 304 stainless | 2.0–3.5° | Higher yield and work hardening hold the angle open | Bend across the rolling direction where possible |
| 5052-H32 aluminium | 2.0–4.0° | Recovers more and scratches easily | Soft punch and polished die |
| HSLA / high yield | 3.0–5.0° | Needs overbend or a restrike | Check tonnage before choosing a narrow V |
| 6–10 mm plate | 1.5–3.0° | Absolute tip movement is large even at low angle | Bed limit 4,450 mm; angle corrected along the bed |
The Ganesh column is where the correction happens. The brake holds about ±0.5° per bend on repeat work when the bend table is set for the grade, and the 5-axis control adjusts the ram position and the back gauge during the stroke so a long part does not lose angle towards its ends.
The arithmetic: overbend angle, tip movement and radius growth
Three numbers turn springback from a complaint into a setting.
The first is the overbend. If the part recovers 2.5° after the ram releases, the ram has to reach 87.5° at bottom dead centre to leave 90°. That is a single number in the press program on a CNC brake, and it is the number a bend table stores per material and thickness.
The second is the tip movement, which is what the assembly sees. For a flange of length L recovering by θ, the tip moves L × tan θ. At 2.5° and 100 mm that is 4.37 mm; at 2.5° and 250 mm it is 10.9 mm. This is why a "small" angle error is a large fit problem on a long panel.
The third is the radius. Springback does not only open the angle; the inside radius grows as the material unloads. A 2.0 mm inside radius on 2 mm CRCA might come back at 2.2 mm. Run that through the bend allowance at K = 0.44:
- Nominal: BA = π × (2.0 + 0.88) / 2 = 4.52 mm, deduction = 8.00 − 4.52 = 3.48 mm.
- After recovery: BA = π × (2.2 + 0.88) / 2 = 4.84 mm, deduction = 8.40 − 4.84 = 3.56 mm.
The deduction grew by 0.09 mm, so the flat pattern is 0.09 mm short per bend. On a four-bend box that is 0.36 mm, which matters on a hole pattern that spans the part and does not matter on a cover panel. The K-factor guide explains why the factor itself moves with the radius-to-thickness ratio, and the bend allowance guide works the flat length through.
Why compensating the formed model breaks the assembly
A model bent to 87.5° is a model of the tool position, not the part. Three things break at once.
The drawing dimensions stop matching the model, so a first article measured against the drawing disagrees with a CMM program written against the model. The flat pattern changes, because the bend deduction is computed from a geometry that is not the finished angle. And every assembly constraint that references the formed face inherits the 2.5°, so a bracket that should sit flat against a rail arrives with a 2.5° wedge built into its nominal.
The exception is a part whose function is defined at the recovered angle and whose drawing is written that way — rare, and usually the sign of a drawing that was corrected after a failure rather than designed. If the part really is 87.5° as a finished condition, model 87.5°, state it on the drawing, and accept that the press must overbend to about 85° to leave it there.
Where model-level compensation is correct
Two cases justify putting springback into the geometry.
The first is a stamping die. Progressive and single-stage tools are cut from a die face that is developed off the part and adjusted for recovery. Presses run 20–300 T here, with an in-house tool room for press tools, progressive dies and checking fixtures, so the die face and the tryout loop are inside the same plant. A new die typically needs two or three tryout corrections before the angle settles, and each correction is a die-face change, not a part change.
The second is a forming simulation that drives a die design. Simulation predicts the recovered shape, the die is cut to the predicted shape, and the first-off measures the difference. The simulation is worth running where the part has a drawn feature or a high-strength grade, because the alternative is trial and error on a tool that costs more than the simulation.
Neither case moves the part model. The part model stays nominal; the tool model absorbs the prediction.
What the brake does instead
Air bending compensates by angle. The ram travels past 90°, the material yields, and the elastic recovery brings the flange back. The control stores the overbend per material and thickness, so the operator selects a program rather than dialling an angle by feel.
Bottoming removes most of the recovery by pressing the material against the die, and coining removes nearly all of it by yielding through the thickness. Both cost tonnage. Coining a 4 mm mild steel bend can need three to five times the air-bend force, and on a 200 T brake with a 4,450 mm bed that force limit arrives quickly on long parts. The press brake tool selection page covers when a sharper punch and a narrower die are worth the load.
There is a geometric lever too. A wider die opening raises the inside radius, which raises the springback; a narrower one lowers both, at the cost of force and die marking. That trade is the reason a bend table is tied to a die set, not just to a material. The same 2 mm CRCA part formed on a 16 mm V and a 12 mm V will need different overbend angles, and the flat patterns will differ by a few tenths.
Bend speed and dwell are smaller levers, and they are the ones to reach for when the angle wanders within a batch rather than sitting consistently wrong. A short dwell at bottom dead centre lets the material settle against the tool before the ram lifts, and it removes a few tenths of a degree of scatter on stainless and aluminium. It costs cycle time, so it belongs on the parts where the angle is functional.
Measurement has to match. Read the angle with a digital protractor against the flange face 30–50 mm from the bend, not at the tip, where a slight curl reads as an angle error. On a long part, take three readings along the length: the ends and the middle show whether the ram is compensating evenly, which is the failure the 5-axis control exists to prevent.
How Ganesh sets a bend for springback
A new part starts from the drawing and the model, and the bend table is built from the grade, the thickness and the die that will run. The first article is measured for included angle and flange length, the recovered angle is recorded, and the correction goes into the press program. That takes one setup and one part, and it is repeated whenever the die or the grade changes.
Forming runs on the 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, to 10 mm thickness, with the 5-axis compensating the ram across long parts. Press work for higher volumes runs on mechanical presses from 20 T to 300 T, with 250 T punching, and the tool room builds and maintains the dies, welding fixtures and checking fixtures in-house. Where the part is a drawn component rather than a bent one, how springback affects pressed components covers the draw-specific behaviour.
Custom parts run from 0.8 mm to 40 mm at ±0.5 mm typical tolerance, with tighter features by agreement. Manufacturing has run since 1992 across five units in Mumbai (Vasai) and Nagpur, under ISO 9001:2015 and ISO 14001:2015, with first article inspection standard and PPAP available.
What to put on the drawing
- The finished angle, at nominal, with a tolerance per bend. Do not draw the overbend.
- The inside radius, or a note that the radius follows the tool. A radius tighter than one thickness in mild steel will crack before it forms.
- The bend line position from a datum edge, so the flat length can be derived consistently.
- The grade and the thickness, because springback is a material property and the drawing is where the material lives.
- The measurement state for angle: on the formed part, after the ram releases, at a stated temperature.
- A note on which bends are cosmetic and which are functional, so the correction effort goes where the fit needs it.
Send the drawing with the first-article angle if you have one from a previous supplier; it is the fastest way to set the overbend. The design and CAD hub collects the related handover guides, and the bending capability page lists the brake, the bed and the thickness range.
When springback compensation is the wrong answer
Compensation cannot fix a bad bend geometry. A flange shorter than the die allows will drop into the opening and produce a random angle that no overbend setting can hold. A radius below one thickness in mild steel will crack on the outside, and compensating the angle makes the crack worse.
It also cannot fix a material problem. A coil at the top of its yield range behaves differently from one at the bottom, and if the drawing does not control the grade tightly, the bend table is only right for the coil it was set on. For a part where the angle is critical, control the grade and the thickness tolerance, not just the angle.
And it is the wrong answer when the part should not be bent at all. A 12 mm thick bracket with a tight angle is a machined or welded part, not a brake part, because the force needed to coin it exceeds what the tool can take. Above 10 mm the brake is outside its range here, and the route changes.
If the angle is drifting between batches, send the grade, the die set and the measured angle from three parts. Request a quote and the engineering team will say whether the fix is the bend table, the die opening or the drawing tolerance.
Frequently asked questions
Should I model springback in my sheet metal CAD part?
No. Model the finished nominal part and let the tool compensate. A model bent to 87.5° to allow for recovery produces a drawing dimension that nobody wants and a flat pattern that is wrong by the correction. Compensate the die face or the bend program instead.
How much springback does 2 mm CRCA have?
About 1–2° at a 90° air bend with an inside radius near 2 mm. The exact figure depends on the yield strength of the coil and the die opening: a wider V die increases the inside radius and usually increases the recovered angle.
Does springback change the flat pattern?
Yes, through the radius. If the inside radius grows from 2.0 mm to 2.2 mm on a 2 mm part, the bend allowance at K = 0.44 rises from 4.52 mm to 4.84 mm and the deduction rises by 0.09 mm, so the flat shortens by 0.09 mm per bend.
Can a press brake eliminate springback?
It can compensate for it, not eliminate it. Air bending overbends by the recovered angle; bottoming and coining remove most of it by yielding the material through the thickness, at several times the tonnage. A 200 T brake coining 4 mm steel across a full bed runs out of force before it runs out of angle.
Why does the same drawing spring back differently at two suppliers?
Different die openings, different punch radii, different coil yield strengths and different bend speeds all move the recovered angle. A 16 mm V die and a 12 mm V die on the same 2 mm part produce different inside radii, and therefore different springback, from the same material.
Sources and further reading
- ISO 6892-1:2019 — Metallic materials: tensile testing at room temperature, which is where the yield strength driving springback is measured · reviewed 3 Nov 2026
- IS 513 Part 1 — Cold reduced carbon steel sheets and strips, including the grades and mechanical properties of the coil · reviewed 3 Nov 2026
- ISO 2768-1 — General tolerances for linear and angular dimensions where the drawing gives no individual tolerance · reviewed 3 Nov 2026
Have a bend that will not hold its angle?
Send the drawing, the grade and the measured angle from the first article. We check the die opening, the punch radius and the bend table before changing the tool or the part.
Send a drawing