A press brake bending calculator answers four questions before any steel is cut: how much force the bend needs, how much material it consumes, what the flat blank must measure, and how short a flange the die can still grip. Three are arithmetic. The fourth — the K-factor — is measured, not calculated, and it decides whether a multi-bend enclosure closes. This guide works through each output with one worked example and lists the numbers a calculator never gives you, because they live on the shop floor.
Key takeaways
- A bending calculator is four outputs sharing one set of inputs — bend force, bend allowance, bend deduction and minimum flange. Change the V-die opening and all four move, so pick the die first.
- Air-bend force scales with thickness squared and inversely with die opening. For 2 mm cold-rolled steel at a 16 mm die the estimate is about 13 t per metre; size the machine with 20–30% margin.
- Bend allowance and bend deduction are not the same number. On a 90° bend in 2 mm steel they differ by about 1 mm per bend, and entering the wrong one is the most common cause of a short flange.
- The K-factor is a measured value, not a material constant. Start at 0.44 for mild steel, then correct it with a test bend on the tooling that will actually run the job.
- SanJun runs the calculation, then proves it with a test bend. We are a sheet metal fabricator: we hold the measured dimensions and the first-article record, and we do not issue listings or certificates of compliance, and we do not run UL 9540A.
What does a press brake bending calculator actually compute?
Despite the name, a press brake bending calculator is not one calculation. It is four outputs sharing the same inputs, and they are not independent — change the die opening and all four move.
- Bend force — the load the ram must deliver to form the bend in the chosen die; it decides whether the job can run at all.
- Natural inside radius — the radius the material actually takes in air bending, set by the die opening rather than the punch tip.
- Bend allowance (BA) — material the bend consumes along the neutral axis, added to the straight legs to get the flat blank.
- Bend deduction (BD) — what you subtract from the sum of the outside flange dimensions. Same destination, different route.
- Minimum flange — the shortest leg the die can grip before the part slips.
The first two are mechanics and can be derived. The third and fourth depend on the K-factor, which comes from measurement, not a formula — which is why a calculator can be exactly right and still produce a part that does not fit. For the physics inside the bend see our sheet metal bending guide.
Which inputs does it need, and which one is most often wrong?
Seven inputs feed every bending calculation. Six are numbers read off the drawing or the tooling rack; the seventh is how the bend will be formed.
- Material and its actual tensile strength. Not the alloy name — the number. Tensile strength sits in the force formula as a direct multiplier.
- Thickness, measured. A coil ordered at 2.00 mm that arrives at 1.94 mm bends as 1.94 mm — and force scales with thickness squared.
- Bend angle — the interior angle. 90° is the default; 30°, 45° and 60° are common on enclosures; 135° appears on hems.
- Inside radius — the radius you call out, or the natural radius the die produces if you do not.
- V-die opening — the width of the lower tool. This is the input that quietly drives the other three.
- Bend length — scales force linearly; unrelated to flat-pattern length.
- Forming method — air bending, bottom bending or coining. The three differ by a factor of three or more in required force.
The input wrong most often is tensile strength, because nobody writes it down. A drawing says "CRS" or "304" and the calculator gets a generic handbook value. Use the number from the mill certificate instead — ask for an EN 10204 3.1 certificate, as set out in our RFQ checklist.
One customer sent a 1.5 mm 304 door that our first article measured at 1.42 mm — nobody had checked the coil. The angles were fine, but every flange came out 0.6 mm short, because the blank was calculated at 1.5 mm and the material was not there. Two hours of setup and 60 parts went to scrap before the micrometer came out. Measured thickness, measured tensile strength, then calculate.
How do you calculate bend force (tonnage)?
For air bending — the default on every CNC press brake we run — the standard estimate is:
P (kN) = 1.42 × Rm × L × t² ÷ (V × 1000)
where Rm is tensile strength in MPa, L is bend length in mm, t is material thickness in mm and V is the die opening in mm. Divide kN by 9.81 for metric tonnes.
Two things follow directly. Force rises with the square of thickness, so doubling thickness quadruples the load. And force falls as the die opening widens — which is why a die change is the cheapest way to bring an overloaded job back inside capacity.
Worked example: 2 mm cold-rolled steel, Rm = 370 MPa, 90° bend, 1,000 mm bend line, 16 mm die. P = 1.42 × 370 × 1000 × 4 ÷ (16 × 1000) = 131 kN ≈ 13.4 t per metre. That is the theoretical figure; in production we size the machine 20–30% above it and treat it as a floor, not a forecast — tool wear, thickness variation and tensile strength at the top of the band all push it up.
| Thickness | Die opening (V = 8t) | Cold-rolled steel (370 MPa) | 304 stainless (515 MPa) | 5052-H32 aluminium (228 MPa) |
|---|---|---|---|---|
| 1.0 mm | 8 mm | 6.7 t/m | 9.3 t/m | 4.1 t/m |
| 1.5 mm | 12 mm | 10.0 t/m | 14.0 t/m | 6.2 t/m |
| 2.0 mm | 16 mm | 13.4 t/m | 18.6 t/m | 8.3 t/m |
| 3.0 mm | 24 mm | 20.1 t/m | 28.0 t/m | 12.4 t/m |
| 4.0 mm | 32 mm | 26.8 t/m | 37.3 t/m | 16.5 t/m |
Two caveats separate a useful number from a dangerous one:
- These are air-bending numbers. Bottom bending needs roughly three to five times the force, coining more again.
- The figures are per metre of bend. A 300 mm bend needs 30% of the load, delivered across the full ram.
Method matters as much as the formula. Air bending touches the die on two edges and the punch at the tip, so one tool set covers every angle. Bottom bending presses the sheet into the die — better angle, more force. Coining holds angle best, at several times the force. For most enclosure work air bending is right.
How do you choose the V-die opening?
The die opening is the input people treat as a constant, and it quietly decides the radius, the force and the minimum flange. In air bending the sheet does not take the punch tip radius — it takes a natural radius set by how far it must span the die, roughly 0.15 to 0.17 × V for mild steel. That is why an 8t die lands near 1.2× material thickness.
The practical bands we use:
- V = 8t — the default for cold-rolled steel; balances force, radius and flange length.
- V = 6t to 8t — aluminium, to keep the outer surface from stretching.
- V = 8t to 10t — stainless. It work-hardens and springs back more; a wider opening keeps the force manageable and reduces cracking at tight radii.
- V below 6t — possible, but force climbs steeply and the punch tip marks the material.
| Material & thickness | Recommended V | Natural inside radius | Minimum flange | Note |
|---|---|---|---|---|
| CRS 1.0 mm | 8 mm | ≈ 1.3 mm | 5.5 mm | Standard tooling |
| CRS 1.5 mm | 12 mm | ≈ 1.9 mm | 8.0 mm | Standard tooling |
| CRS 2.0 mm | 16 mm | ≈ 2.6 mm | 10.6 mm | 10 mm if the radius is held at 2 mm |
| CRS 3.0 mm | 24 mm | ≈ 3.8 mm | 15.8 mm | Check ram capacity |
| 304 2.0 mm | 16–20 mm | ≈ 2.6–3.2 mm | 11–12 mm | Springback compensation needed |
| 5052-H32 2.0 mm | 12–16 mm | ≈ 2.0–2.6 mm | 10 mm | Mind grain direction on tight bends |
Where the drawing calls out an inside radius, the die has to be chosen to produce it — and that is where a radius that is not on the tooling rack costs money: a tool change, or an operator who quietly uses a different die. The radii we hold as standard are in our DFM guide.
How do you calculate bend allowance?
Bend allowance is the arc length of the neutral axis through the bend — the length of material the bend consumes, which the flat blank has to include.
BA = (π ÷ 180) × A × (R + K × t)
where A is the bend angle in degrees, R is the inside radius, K is the K-factor and t is thickness.
Using the same example — 90° bend, 2 mm cold-rolled steel, 2 mm radius, K = 0.44:
BA = 1.5708 × (2 + 0.44 × 2) = 1.5708 × 2.88 = 4.52 mm
That is the whole bend. Everything else on the flat pattern is straight leg, measured to the bend tangent.
| Output | Value for the worked example | How it is derived |
|---|---|---|
| Bend force | 131 kN ≈ 13.4 t per metre | 1.42 × 370 × t² ÷ V, V = 16 mm |
| Inside radius | 2.0 mm (as called out) | Punch tip / die selection |
| Bend allowance (BA) | 4.52 mm | (π ÷ 180) × 90 × (R + K·t), K = 0.44 |
| Outside setback (OSSB) | 4.00 mm | (R + t) × tan(A ÷ 2) = 4 × tan 45° |
| Bend deduction (BD) | 3.48 mm | 2 × OSSB − BA |
| Minimum flange | 10 mm at R = 2 mm; 10.6 mm at the natural radius | 4 × t + R |
| Flat length | Leg 1 + Leg 2 − 3.48 mm | Using outside dimensions |
Bend allowance or bend deduction — which one does your CAD want?
These two numbers answer the same question by different routes, and mixing them up is the most common flat-pattern error we see on incoming drawings.
- Bend allowance (BA) is what you add: flat length = leg 1 + leg 2 + BA, where the legs are measured to the bend tangent.
- Bend deduction (BD) is what you subtract: flat length = leg 1 + leg 2 − BD, where the legs are measured to the outside faces.
On the worked example the two differ by 1.04 mm. That sounds small until the part has six bends, at which point the wrong convention has moved the finished part by roughly 6 mm — enough that a door will not latch. Most CAD systems compute both once you supply a K-factor, so the discipline is knowing which convention your software and supplier both use, and writing it on the drawing.
There is a second convention to watch: some systems ask for a Y-factor, where Y = K × π ÷ 2. Enter a K-factor into a Y-factor field and the flat pattern comes out wrong in a way that looks plausible enough to ship. Check which one your CAD template expects.
What K-factor should you enter, and where does a real one come from?
The K-factor is the position of the neutral axis as a fraction of material thickness. K = 0.5 means the neutral axis sits mid-sheet; in reality it shifts inward, because the inside surface compresses more than the outside stretches.
| Material | Starting K-factor | Typical springback | Comment |
|---|---|---|---|
| Cold-rolled steel | 0.40–0.45 (use 0.44) | ≈ 1° | Most predictable; the reference case |
| Galvanized sheet | 0.42–0.46 | ≈ 1° | Coating adds thickness at the bend |
| 304 / 316 stainless | 0.45–0.50 | ≈ 2° | Work-hardens; wider die recommended |
| 5052-H32 aluminium | 0.40–0.45 | ≈ 3° | Mind grain direction on tight radii |
| 6061-T6 aluminium | 0.45–0.50 | ≈ 3° | Cracks below about 1.5× thickness |
Two things make the K-factor awkward: it is not a constant for a material — it rises as the radius-to-thickness ratio falls — and it depends on the method, the tooling and the machine. A table value is a starting point, nothing more.
A real K-factor comes from a test bend, about ten minutes. Bend a coupon on the tooling that will run the job, measure the flange lengths, back-calculate the actual bend allowance and solve for K:
K = (BA ÷ ((π ÷ 180) × A) − R) ÷ t
Do it once per material, thickness, radius and tooling combination, record the result, and the next job with the same combination starts from a proven number instead of an assumption. That record is why first articles fit.
How does springback change the answer?
Sheet metal is elastic: the punch drives past the target angle, the load comes off, and the part relaxes back. The compensation is overbend, and the amount is measured, not calculated.
The rough figures in the table above are starting points for setup, not drawing tolerances. Four things move them:
- Yield-to-tensile ratio — higher-strength material recovers more.
- Radius-to-thickness ratio — a generous radius springs back more than a tight one.
- Forming method — bottom bending and coining set the material under pressure and recover far less.
- Batch variation — two coils of the same specification can need different compensation.
CNC controllers handle this with an angle measurement system or a stored correction per program; manual brakes need an operator who has done it before. Either way, the gap between the calculated angle and the angle off the machine is closed by a measured first article.
What is the minimum flange, and what happens below it?
A flange has to reach far enough into the die to be supported before the bend starts. The rule used on our floor is minimum flange = 4 × material thickness + inside radius — for 2 mm material with a 2 mm radius that is 10 mm, and about 10.6 mm at the natural radius from a 16 mm die.
Below that, three things happen and none of them are recoverable:
- The part slips into the die opening — the bend line lands in the wrong place and the flange never measures true.
- The flange deforms — the short leg is dragged and rolled instead of folded, and the outside corner goes rounded.
- The operator improvises — a narrower die, a shim, hand pressure: a part that passes once and drifts on the next hundred.
A telecom customer sent a 1.5 mm aluminium tray with a 6 mm return on two sides; the die needed 8 mm. The first article came off the brake with the short leg rolled into a curve, and the lid that sat on it rocked by 3 mm. The fix was a drawing change to 9 mm — no cost, no tooling, two days sooner than forming it as drawn. The related edge forms are covered in our hem, relief and corner joint guide.
If the design cannot give the length, the options are a narrower die, a hem or return flange to give the tooling something to hold, or a change to how the part is assembled.
What does the calculator not tell you?
A calculator is honest about what it computes and silent about everything else. Five things consistently decide whether a bent part ships on schedule, and none appear in the output:
| Not in the output | Why it matters | Where it is handled |
|---|---|---|
| Whether the tooling is on the rack | A correct radius that needs a tool nobody owns means a change or a delay | Check at quotation, before programming |
| Hole, slot and cutout clearance from the bend | Features inside the forming zone get dragged oval; it is the largest single source of bend rework | Drawing — see the bending guide |
| Grain direction | Bending parallel to the rolling direction cracks on hard alloys and tight radii | Nesting and blank orientation |
| Coating build-up | Powder coat adds 60–120 µm per surface, which is enough to bind a door that fitted bare | Finishing spec — see the surface finishing guide |
| Tolerance stack across many bends | Each bend carries its own variation; eight bends accumulate it | Tolerance analysis — see the tolerance guide |
Two deserve emphasis. Hole-to-bend clearance is measured to the tangent of the bend, not the centreline — which is why a clearance that looks fine on paper produces an oval hole on the floor. And coating build-up surprises people at final assembly: a door that closes beautifully bare can bind after powder coat, because two mating flanges each gained 0.1 mm.
Frequently Asked Questions
What is the difference between bend allowance and bend deduction?
Bend allowance is the arc length of the neutral axis through the bend, added to the legs measured to the bend tangent. Bend deduction is subtracted from the sum of the outside flange dimensions. Both give the same flat length; on a 90° bend in 2 mm steel they differ by about 1 mm per bend. Check which convention your CAD expects.
What K-factor should I use for cold-rolled steel?
Start at 0.44 for air bending, and treat it as a starting point only — the real value depends on radius-to-thickness ratio, tooling, method and batch. The reliable number comes from a test bend on the tooling that will run the job.
How much tonnage does bending 2 mm steel need?
About 13 t per metre for cold-rolled steel in a 16 mm die: 1.42 × 370 × t² ÷ V. Size the machine 20–30% above that. The figure is for air bending — bottom bending needs roughly three to five times as much, and stainless at the same thickness and die needs about 18.6 t per metre.
What V-die opening should I specify?
V = 8 × material thickness is the default for cold-rolled steel; use 6–8t for aluminium and 8–10t for stainless. The opening sets the natural inside radius at roughly 0.15–0.17 × V, so it also sets the minimum flange. Choose the die first.
Why does my flat pattern come out short?
Three causes cover almost every case: the wrong convention (bend deduction where bend allowance was expected), a K-factor taken from a table instead of measured, or thickness assumed nominal when the coil came in thinner. Measure the material, confirm the convention, then correct the K-factor with a test bend.
Do I need to allow for springback in the drawing?
No — call out the finished angle and the tolerance, and let the fabricator compensate. Compensation starts from roughly 1° for cold-rolled steel, 2° for stainless and 3° for aluminium, but the value is measured on the actual material and tooling. What belongs on the drawing is the angle the finished part must hold.
Can the same K-factor be reused on the next job?
Yes, if material, thickness, inside radius, tooling and forming method are all the same. We measure the first article, record the K-factor and compensation, and hold that record so the next run does not repeat the setup. Change any one of the five and it has to be re-measured.
Does SanJun verify calculator output before running a batch?
Yes. We run the calculation for force, bend allowance and minimum flange, confirm the tooling is on the rack, then bend and measure a first article before locking the program. We hold the measured dimensions and the first-article record. We do not issue listings or certificates of compliance, and we do not run UL 9540A; where a project needs a witnessed third-party test or a certificate naming a standard, that is agreed at RFQ and run by the named laboratory.
From calculator output to a first article
The calculator begins the loop rather than ends it:
- Choose the die first — radius, force and minimum flange all follow from the V-opening.
- Enter measured inputs — thickness off the micrometer, tensile strength off the mill certificate.
- Run the four outputs against machine capacity and the tooling rack.
- Confirm the flat-pattern convention — bend allowance or bend deduction, K-factor or Y-factor.
- Bend one piece, measure it, correct the K-factor, lock the program, then sample and log the result.
Step five is what separates a calculator result from a part that fits: most setups settle in two test pieces and ten minutes, and it is the cheapest ten minutes in the job.
Send us the drawing and we will run the calculation, flag what the calculator cannot tell you — tooling availability, hole clearance, coating build-up — and return a quotation with a bend sequence and a first-article plan. For the wider workflow see our sheet metal fabrication process.
Need CNC-bent sheet metal parts? Send your drawings for a free DFM review and a quotation within 24 hours.