Press brake tool selection for repeat parts

A repeat part with an 18 mm return flange is a tooling problem before it is a price problem. On 3 mm CRCA, a 25 mm V-die leaves a minimum flange of 15.5 mm, so the flange forms but the punch body meets the wall on the next bend and the part has to be re-clamped or the sequence rebuilt. The tool set decides how many operations that takes, and on a 20,000-part release one extra operation at 30 seconds a part is 167 hours of press time.

Press brake tool selection for repeat parts is mostly about removing decisions. Pick the die opening from thickness, pick the punch tip from the required inside radius, pick the segment stack from the part envelope, then leave that set together for the life of the part number so the bend table stays true.

Press brake tool selection starts with the die opening

The V-opening sets the tonnage, the minimum flange, the natural inside radius and the sensitivity to thickness variation. For sheet below 3 mm, use 8 × t. From 3 mm to 8 mm, use 10 × t. Above that, 12 × t, subject to a tonnage check.

A narrower opening looks attractive because it holds a tighter radius and a shorter flange. It also raises the force per metre roughly in inverse proportion to the opening, and it increases die marking on the outside face. On a repeat part the marking is usually the complaint that arrives first, and it arrives because the die was chosen for a flange rather than for the bend.

The tonnage number, worked

Air-bending force per metre is 1.42 × σb × t² / V, with tensile strength in MPa, thickness and V-opening in millimetres, and the result in kN/m. Divide by 9.81 for tonnes per metre.

• 2 mm CRCA at 450 MPa in a 16 mm V-die: 1.42 × 450 × 4 / 16 = 160 kN/m, or 16.3 t/m.
• 3 mm CRCA at 450 MPa in a 25 mm V-die: 1.42 × 450 × 9 / 25 = 230 kN/m, or 23.5 t/m.
• 6 mm CRCA at 450 MPa in a 50 mm V-die: 1.42 × 450 × 36 / 50 = 460 kN/m, or 46.9 t/m.

Multiply by the bend length in metres to get the machine load. A 4,450 mm bend in 3 mm CRCA needs 1,023 kN, which sits comfortably inside the 200 T rating of the brake. The same bend in 6 mm needs 2,047 kN, which does not: the 200 T press is 1,963 kN, so the longest full-thickness bend it can make in 6 mm is about 4,268 mm. That 4% gap is the sort of arithmetic that turns a quotation into a rework order, and it is why the tonnage check belongs in the tool selection, not after it.

Punch tip radius and the natural radius

With a sharp punch in an 8 × t die, the inside radius of an air bend settles at about 0.16 × V, which is roughly 1.3 × t. That is fine for a general part and wrong for one drawn at 1.0 × t.

To hold a specific radius, the punch tip has to be that radius, and the die opening still has to be wide enough for the flange and the tonnage. The two constraints pull in opposite directions on thin sheet: a 1.0 mm tip on 1.0 mm sheet gives a genuinely tight bend but concentrates load on a small area, and the punch is the first thing to wear.

An 88° punch used for a 90° air bend is normal, because the material springs back before it reaches the punch angle. The amount of springback is grade-specific, so an 88° tool that produces 90° in CRCA produces 88° in 304 without a bend table correction.

The three tools a repeat family usually needs

Most repeat parts are covered by a straight punch and die for the long bends, a gooseneck punch for return flanges, and a sectional stack for box corners and inner walls. Buying all three for every part is waste; keeping the right three on the machine for the family is not.

The segment stack is the least glamorous and most valuable decision on the list. A part 2,400 mm long with bends at 300 mm and 1,900 mm does not need a 4,450 mm tool; it needs a stack that reaches the bend without fouling the rest of the part. Two segments of the right length held together with a locating key give a repeatable shoulder position, and the operator stops hunting for a shim.

Clearance: gooseneck, box bends and the tools that get in the way

A straight punch has a body that sits directly behind the tip. Form a 90° flange and then try to form a parallel flange 60 mm away, and the body meets the first flange. A gooseneck punch moves the body back, which buys the clearance to form the second flange in the same setup.

Gooseneck tools are less stiff than straight tools, so they are used for the short return flanges and not for the 2,500 mm bend. Mixing the two in one setup is normal; mixing them without re-proving the angle is not, because the deflection differs.

For a box or a channel with an inner wall, sectional tooling is the only way to form a bend that the punch body would otherwise block. The segment length has to be shorter than the inner wall, and the stack has to be arranged so the shoulder height is the same across every segment.

Bend sequence follows the same logic. Longest flange first while the part is still flat, then the return flanges from the outside in, then the closing flange that needs the punch to enter a channel. A part formed in the wrong order often cannot be formed at all, and the fix is a new tool, not a new operator.

What a dedicated tool set buys on a repeat part

Three things, none of them dramatic on their own.

Setup time falls from 30–45 minutes to under 10, because the stack is assembled, keyed and labelled rather than rebuilt. On a part that runs every three weeks, that is an hour a year of machine time and a much larger saving in the first-off scrap that follows a rebuild.

The bend table stays valid. The ram depth, the die opening and the tip radius are the inputs to the correction values the control stores, and changing any one of them invalidates the table. A shared tool set means a new table for every run; a dedicated set means the table proved at first article is still correct at part 5,000.

Angle variation between operators falls. Two operators setting the same part with the same dedicated stack and the same programme produce the same angle. The variation that remains comes from material, not from setup.

Wear, regrind and the 0.2 mm that moves the angle

A punch tip wears on its radius. After 50,000–100,000 bends in 3 mm CRCA, a 1.0 mm tip can measure 1.2 mm, which raises the inside radius by about 0.2 mm and changes the developed length by roughly 0.1 mm per bend. On a part with six bends, that is 0.6 mm of accumulated error in the flange-to-flange dimension, and it appears gradually enough that nobody notices until an assembly stops fitting.

Die shoulders wear the same way. A rounded shoulder increases the natural radius and reduces the marking, which sounds acceptable until the radius callout is tight.

The controls are simple: measure the tip radius at every tool service, record it against the part number, regrind or replace at the limit, and re-prove the bend table after either. Store punches and dies on racks, tip-up, with the segment stack kept together; a die dropped on a concrete floor is a die with a new shoulder radius.

How Ganesh sets up a repeat bend programme

Bending runs on the 200 T, 5-axis CNC press brake with a 4,450 mm bed, Delem control and capacity to 10 mm, described in full under sheet metal bending. The control carries a material table per grade, so the springback correction for CRCA and for 304 are separate entries rather than one compromise value.

For a repeat part, the tool set, segment stack, die opening, ram depth per bend and the proved bend table are recorded against the part number and kept together between runs. Blanks arrive from the 12 kW fibre laser with its 40 ft × 16 ft bed, cut to the flat developed from the bend allowance at the actual material and radius, so the flange that reaches the die shoulder is the flange the bend table was proved on. Formed parts then go through seven-tank pretreatment and the 18 ft × 14 ft powder booth.

Ganesh has manufactured sheet metal since 1992 across five units in Mumbai (Vasai) and Nagpur, holds ISO 9001:2015 and ISO 14001:2015, and works to ±0.5 mm typical on formed sheet metal, tighter on critical features by agreement. PPAP and first article inspection are available, and the first article for a repeat bend part includes the angle at each bend and the flange lengths measured from the same datum the drawing uses.

What to put on the drawing

• Material grade, thickness and the thickness tolerance the tonnage was checked against.
• Inside radius per bend, in millimetres, and whether it is critical.
• All flange lengths, including the return flanges that drive the punch choice.
• The inner wall height on box and channel parts, which drives the segment length.
• Bend sequence, if the part can only be formed in one order.
• Angle tolerance and the measuring method; ISO 2768-1 applies only where the drawing calls no individual tolerance.
• Surface faces that must not be marked by the die shoulder.
• Quantity per release and the variants in the family, so the tool set can be scoped once.

The long-bed bending post covers what a 4,450 mm bed changes about part design, and the minimum flange rules set out the geometry that decides whether a return flange can be formed at all.

The bending and welding assemblies hub carries the rest of this cluster, including tonnage selection and bend tolerances.

When a press brake tool is the wrong answer

A dedicated brake tool stops being the answer in three cases. The first is thickness: above 10 mm the brake is out of scope, and the part belongs on a press or with a heavier machine. The second is length: a bend longer than 4,450 mm cannot be made in one hit, and splicing a bend into two is a design decision, not a tooling one.

The third is geometry that a brake cannot make at all. A hem, a curl, a louvre or a form that needs a shaped punch and die is a press tool, not a brake tool, and it is quoted as tooling separate from the piece price. Ganesh does not build press-brake tooling in-house; the tool room builds press tools, progressive dies and welding and checking fixtures, which is where a dedicated form tool belongs.

Send the drawing with the flange lengths, the inside radii and the quantity per release. The engineering team will return the die opening, the punch tip, the segment stack and the tonnage check against the 200 T brake, so the tool set is agreed before the first blank is cut. The press tonnage calculator gives the same number in a few seconds if the part is still being designed.