The formula, and what the 575 is doing there
Air bending tonnage per foot of bend is approximately 575 times the thickness squared, divided by the die opening, with everything in inches. That constant is calibrated to mild steel of around 60,000 psi tensile strength. Every other material is handled by scaling: stainless roughly one and a half times, aluminum roughly half, high strength low alloy somewhere between mild steel and stainless. If you know the actual tensile strength of the heat you are bending, put it in and the calculator scales against 60 ksi directly rather than using a family average.
Two things in that expression deserve attention. Thickness is squared, so going from 14 gauge to 10 gauge is not a small change: it roughly doubles the thickness and quadruples the force. And the die opening divides, so the die selection is as powerful a lever as the material. A bend that will not fit a 60 ton machine in a 1 inch vee fits comfortably in a 2 inch one, at the cost of a larger inside radius.
Choosing the vee
The convention is a die opening of eight times material thickness. It is a convention rather than a law, and shops that bend one product all day settle on their own ratios, but it is the right default when nothing else is driving the choice. From that ratio two other numbers follow.
| Thickness | Conventional vee (8 x t) | Air bend tons/ft, mild steel | Inside radius |
|---|---|---|---|
| 0.048 in (18 ga) | 0.394 in | 3.4 | 0.061 in |
| 0.060 in (16 ga) | 0.478 in | 4.3 | 0.075 in |
| 0.075 in (14 ga) | 0.598 in | 5.4 | 0.093 in |
| 0.105 in (12 ga) | 0.837 in | 7.6 | 0.131 in |
| 0.125 in (1/8) | 1.000 in | 9.0 | 0.156 in |
| 0.187 in (3/16) | 1.500 in | 13.4 | 0.234 in |
| 0.250 in (1/4) | 2.000 in | 18.0 | 0.312 in |
The inside radius column is the reason air bending confuses people at first. You do not set the radius with the punch. In air bending the punch tip never touches the bottom of the vee, the material bridges the opening, and the radius that forms is set almost entirely by how wide that opening is, at roughly 0.156 times the die width. Change the die and the radius changes whether you wanted it to or not, which is why the flat pattern has to be recalculated when the tooling changes. The bend allowance calculator handles that side of it.
Air, bottoming and coining
Air bending leaves the punch short of the die bottom, so the angle is set by how deep the ram travels. It takes the least force, it is the most flexible because one set of tooling makes any angle, and it springs back the most, so the ram overbends to land on the angle you want. Nearly all production bending is air bending.
Bottoming closes the punch into the vee so the material takes the shape of the die. It costs roughly four times the force, gives a more repeatable angle and a tighter radius, and needs a die matched to the angle you want. Coining goes further and squeezes the material until the inside radius conforms to the punch nose, which takes something like eight times the air bending force and essentially eliminates springback. Those multipliers are approximate and vary with tooling geometry; treat them as the right order of magnitude rather than a precise figure, and check the tonnage rating of the tooling itself before assuming the machine is the limit.
What the number does not cover
Rated capacity is quoted over the full bed length. A short bend concentrated near one end of the bed loads the ram unevenly and most machines derate substantially for it, sometimes by half. The manufacturer publishes a load distribution chart and it is worth finding before you assume a 20 ton bend fits a 60 ton machine because it is only a third of the rating.
Nor does the tonnage say anything about whether the part will crack. That is a question of the inside radius against the material thickness, the alloy and temper, and the direction of the bend relative to the rolling grain. Aluminum in particular will pass a tonnage check comfortably and split on the outside of the bend anyway. When a part cracks, the answer is almost always a wider die rather than more force.
A press brake closes with enough force to remove fingers without the operator noticing resistance, and the part swings up as it forms. Guarding, foot control discipline and where you stand are training questions, not calculation ones.
Questions people ask
How many tons do I need to bend 1/8 inch mild steel?
About 9 tons per foot of bend, in the conventional 1 inch vee. A 4 foot bend is therefore around 36 tons. Move to a 1/2 inch vee and it doubles to 18 tons per foot, or 72 tons for the same part, because the die opening divides. Move to a 2 inch vee and it halves. The single most useful habit in press brake work is checking the die before checking the machine, because the die is the variable you can actually change.
Why does the die opening matter more than I expected?
Because bending over a wide vee is mechanically a longer lever. The material spans the opening and the punch pushes at the middle; the wider the span, the less force it takes to produce the same bend, exactly as a longer wrench loosens a bolt more easily. The trade is that the resulting inside radius grows with the opening, at roughly 0.156 times the die width, so you cannot widen the die indefinitely without changing the part. Every press brake decision is a negotiation between the tonnage you have and the radius you can accept.
Does the punch radius set the inside bend radius?
Not in air bending, which is what most shops do most of the time. The punch tip never reaches the bottom of the vee, so the material forms a radius set by the die opening rather than by the punch. A sharp punch and a blunt one in the same die produce a similar radius, within limits. It only becomes the punch's job in bottoming and coining, where the material is pressed into contact with the tool. This surprises people who expect the punch to stamp its shape into the part, and it is why swapping to a wider die quietly changes every flat pattern in the job.
What is the minimum flange length I can bend?
Roughly 0.77 times the die opening, which for a conventional 8t vee works out near six times material thickness. Shorter than that and the flange does not reach across the vee, so it drops into the opening instead of forming, and the result is a bend that is out of angle and a part that is scrap. Treat that figure as a rule of thumb that varies with tooling: some special dies and hemming tools do better, and a gooseneck punch changes the clearance situation without changing the flange arithmetic. If a part needs a shorter flange than the vee allows, the fix is a narrower die and the higher tonnage that comes with it.
Can I bend stainless on a machine rated for mild steel?
It depends entirely on the thickness and length, because stainless takes roughly one and a half times the force of mild steel at the same thickness and die opening. A machine that comfortably bends a 4 foot length of 1/8 inch mild steel at 36 tons needs about 54 tons for the same part in 304. That may or may not be within the rating. Stainless also springs back further and marks more visibly in the die, so shops often use a wider vee or urethane die protection, which changes the tonnage again. Work out the actual figure rather than assuming the machine that has always coped will keep coping.