Press-Brake Simulation
When a sheet-metal part is shown on a 3D page, it is also bent on a simulated press brake: bend by bend in the bending order, each bend on its own punch and die, and the flanges already made are checked against the punch, the die and the machine's upper and lower beams as the bend goes from flat to its angle. What runs into the machine is said in the message bar, with the bends the part runs into each other on (see Collisions and the bending order).
How the part sits in the press brake
For each bend the part is placed as the operator puts it in: the bend line under the punch's tip, the inside of the bend against the tip, the flanges resting on the die's shoulders either side of its V, rising evenly as the punch goes down. The bends made before it stay made; the bending order is the bend table's (or the better one the collision check finds). The check looks at the part in section, square to the bend: the punch and die are taken to be as long as the bend (sectional tooling, as a box's sides are bent on), so a flange standing at the bend's end doesn't hit them. It takes the sheet as its middle layer: a face closer than almost half the thickness to the tooling hits it. Bends of more than 150° (hems, which are flattened rather than bent in a
- are not checked.
The tooling library
| Tool | What it is |
|---|---|
| Straight punch 88° | A straight punch with an 88° tip: for most bends. |
| Gooseneck punch 88° | Its neck curves back, leaving room for a return flange (a channel's or a pan's). |
| Acute punch 30° | A narrow 30° punch for bends past 90°, such as a hem's first bend. |
| V-die 8, 12, 16, 24, 35 mm 88° | V-dies for bends up to 92°. |
| V-die 12, 16 mm 30° | Acute dies for bends past 90°. |
Choosing the tools for each bend
Unless its bend line says otherwise, each bend gets the die whose V opening is nearest eight times the thickness (of those that make its angle) and the straight punch. When a flange hits the straight punch, the other punches are tried, and the first that clears it is used (and said: Bend 2: the Gooseneck punch 88° clears the part).
To bend a line on tools of your choice, give it PUNCH and DIE settings:
LINE P4,P5,1
RULE PUNCH="Gooseneck punch 88°",DIE="V-die 16 mm 88°"
A named punch that is hit is still used, and a punch that would clear the part is suggested.
Your own tools
Add your own punches and dies in JSON files in the PressBrake folder of your Extensions folder: each file a list of
tools, each with its name, its kind (Punch or Die), its angle (a punch's tip, a die's V), a die's v
opening, and its profile: its outline in section, in millimetres, as points [x, y] - a punch's tip at [0, 0]
and its body upwards; a die's V centred on x = 0 with its top at y = 0 and its body downwards. A tool of yours replaces
the app's of the same name.
{ "tools": [ { "name": "Sash punch 85°", "kind": "Punch", "angle": 85,
"profile": [[0,0],[9,10],[9,60],[-25,60],[-25,40],[-9,10]] } ] }
What is said
- On the press brake, flange 1 hits the punch (Straight punch 88°) while bend 2 is made (at 68°). A flange runs into the tooling or the machine in this order: bend in another order, choose another punch (a gooseneck), or change the part.
- Bend 2: the Gooseneck punch 88° clears the part (name it on the bend line: …). The punch named on the bend line is hit; this one isn't.
See also: Sheet metal and living hinges in 3D, Sheet Metal, K-Factor Tables.