Bend Sheet
Makes the press brake bend sheet for each bent sheet metal part: the order to bend in and, for each bend, the angle, the way it goes, the inside radius, the K-factor used, the bend deduction, the flange lengths and the length of the bend line. A small picture of the flat pattern shows every bend by its step number.
What you get: a table of the bends, a table of the parts (flat size, number of bends, K-factor), a press brake check of every bend (the V die, the shortest flange it forms, the force, and whether your own dies and brake can make it), a list of short flanges to check before bending when no dies are set, and a flat pattern picture. Print it as a PDF, save it as Excel (paid plans) or as a CSV file. The same sheet is in Documents, as Bend sheet.
Step by Step
- Open the sheet metal part or assembly. Parts with no bends (plates) are left out and listed as such.
- Click Cut Files on the Fabrication tab, then Bend sheet... on its bar. You can also open Documents and choose Bend sheet.
- Pick All bent parts or one part, and the unit (inches by default).
- Read the table. Step 1 is the first bend to make. Press Print / PDF, Excel or Download CSV to take it to the brake.
What the Columns Mean
- Step is the order to bend in. It is a suggestion: the deepest bend first, bends that go the same way together, and the bend farthest from the middle of the part first. Check it against your tooling.
- Way is Up when the flange rises toward you as you look at the flat pattern, and Down when it goes away from you. It is read from the flat pattern drawn for that part.
- Inside radius and K-factor are the values used to unfold the part, so the flat size matches.
- Deduction is 2 x setback - bend allowance, with setback = (inside radius + thickness) x tan(angle / 2) and bend allowance = angle x (inside radius + K x thickness).
- Outside A and Outside B are the flat on each side of the bend plus the bend's setback. Flat A and Flat B are the flats alone. A is the side toward the lower left of the picture. A flat between two bends has the other bend's setback added too.
- Line length is the length of the bend line.
Press Brake Check
Below the bend table, each bend is checked for air bending on a press brake:
- V die is the opening to aim for: 6 times the thickness up to 12 gauge (0.105 in), 8 times up to 5/16 in, 10 times up to 1/2 in and 12 times above. Stainless steel is never less than 8 times, and soft aluminum never more than 6 times.
- Shortest flange is the shortest outside flange that die can form, 0.72 times the V opening.
- Force is the tons per foot of bend (tonnes per metre on a metric sheet) and for the whole bend line, for a 90 degree bend. Mild steel is the base, stainless takes 1.5 times and soft aluminum 0.5 times as much.
- Check says OK, or why the bend cannot be made.
With nothing set, the sheet shows the ideal V die for each bend. Open Your press brake in the Bend sheet window and type the V dies you own (in the unit shown), the brake's rating in tons and its bed length. They are kept with your account, like the machine rate. Each bend then uses the die nearest the ideal that its flange fits, and the sheet says which bends you cannot make: a flange too short for every die you have, no die between 5 and 19 times the thickness, a bend that needs more tons than the brake has, or a bend line longer than the bed. An AI assistant connected to your account can read and set your press brake and test any bend; ask it.
These are the usual rules of thumb for a 90 degree air bend, not a chart from your brake maker. A bend that comes out close to a limit should be checked against the chart for your brake and dies.
Check Before Bending
When no dies or brake are set, a flat shorter than 4 times the thickness is also listed here, because it may not seat in a normal V die. With dies set, the press brake check covers it.
Cut Files and Nest
Bend lines go in the cut files and on the nested sheets on their own layer, BEND. They are for marking: do not cut them. In the placements file each bend is a move marked as an etch, with cut set to false. A part with no bends gets no BEND layer.
Limits
- Only sheet metal parts that unfold have a bend sheet.
- The bend order is a suggestion. It does not look for collisions.
- The press brake check uses rules of thumb for air bending at 90 degrees. It is not your brake maker's chart.
- The K-factor and radius are the ones the part was unfolded with. Change them on the part, not here.