Key takeaways
- A 200 T brake at an 8 × t die opening holds 8.2 m of 3 mm CRCA but only 4.1 m of 6 mm and 1.84 m of 10 mm stainless, so tonnage alone never tells you the maximum part size.
- Minimum flange on an 8 × t die is V/2 + t, about five thicknesses; a 3 mm part cannot carry a flange shorter than 15 mm without a different tool.
- Setup count divided by batch size is the most quoted and least explained line in a bending quotation; a 15 minute tool change is 18 s per part at 50 pieces and 0.18 s at 5,000.
- A stored bend programme with the grade, thickness and springback correction is what makes a repeat order land on the first article; without it, every release is proved again.
- A press brake is the wrong purchase when the section is constant over kilometres of length, or when annual volume justifies a formed tool.
Most CNC press brake bending quotations are compared on two numbers: the tonnage of the machine and the price per piece. Neither predicts whether the part will arrive right. A 200 T brake and a 100 T brake will produce an identical 90° bracket from 2 mm CRCA, and the difference between a good and a bad quote for the same part is usually in the tooling inventory, the stored programme and how the supplier allocates setup — not in the machine badge.
This guide is about buying the operation rather than the equipment. It sets out what a specification actually limits, how to work out whether your part fits a given machine, and which questions expose a route that nobody has measured. The bending and welded assemblies hub carries the sister articles on tooling, distortion and tolerance that this guide deliberately leaves out.
The tonnage number is a force rating, not a thickness rating
The force needed to air-bend a length of sheet depends on the material, the thickness squared and the bend length:
F (kN/m) = 1.42 × σb (MPa) × t² × 1000 / (1000 × V)
with V the die opening in millimetres. Set V = 8t, which is the normal starting point, and the expression collapses to F = 1.42 × σb × t / 8 kN per metre. For 450 MPa CRCA that is about 8.1 tonnes-force per millimetre of thickness per metre of bend.
The useful consequence is that the maximum bend length is not one number. It is whatever is smaller: the bed length, or the rated tonnage divided by force per metre. Buyers who ask "what thickness can you bend?" get a number that is true only for a short part, and then discover that a 3 m length of the same thickness is refused.
The table that actually limits your part
| Thickness and material | Force at an 8 × t die | Longest bend on a 200 T brake | Ganesh limit or note |
|---|---|---|---|
| 2 mm CRCA, 450 MPa | 16.3 t/m | Bed-limited at 4,450 mm | Full 4,450 mm bed used; no special tool required |
| 3 mm CRCA | 24.4 t/m | Bed-limited at 4,450 mm | 4,450 mm bed, Delem control, standard 25 mm V-die |
| 4 mm CRCA | 32.6 t/m | Bed-limited at 4,450 mm | Comfortable margin on a 200 T rating |
| 6 mm CRCA | 48.8 t/m | 4,100 mm | Tonnage starts to limit before the bed does |
| 8 mm CRCA | 65.1 t/m | 3,070 mm | A full-length 8 mm panel is a different machine or a different design |
| 10 mm CRCA | 81.4 t/m | 2,460 mm | Ganesh bends to 10 mm; the 10 mm length limit is real |
| 3 mm 304, 600 MPa | 32.6 t/m | Bed-limited at 4,450 mm | Full bed needs 145 t of the 200 T rating |
| 4 mm 304 | 43.4 t/m | 4,450 mm at 193 t | 97% of rating; acceptable as a one-off, not as a repeat setup |
| 10 mm 304 | 108.6 t/m | 1,840 mm | Stainless penalty is the strength ratio, about one third |
The 4 mm stainless row is the one worth reading twice. It fits, technically, and a machine run at 97% of rated tonnage deflects enough that the angle in the middle of a long part will not match the ends. The honest answer for a full-length 4 mm stainless channel is a formed section or a design that uses a shorter bend.
What the machine specification leaves out
A specification sheet tells you about the machine. It does not tell you about the bend.
Tool inventory. A brake with one 88° punch and three V-dies is a different supplier from one with a full gooseneck, acute and segmented set. Acute punches reach return flanges a standard punch cannot; segmented tooling lets a short bend be made without a full-length set-up; a gooseneck clears an upstand on a return. Ask for the V widths available, not just the tonnage.
Crowning. Long bends go hollow in the middle unless the bed is crowned or shimmed. Ask whether crowning is hydraulic, mechanical or absent, because a supplier without it will hold ±1° at the ends and miss the middle.
The control and what it stores. A Delem control stores the part programme — material, thickness, angle, springback correction and sequence. That is what allows the second order to land where the first article landed. A supplier who re-programs by hand from a drawing every release is proving the part again every time, and the variation shows up as a batch that differs from the approved sample.
The 5-axis punch. A tilting punch swings clear of an upstand that would obstruct a fixed punch body. For box sections deeper than roughly the punch height, the machine either has 5-axis capability or the part is bent in a sequence with a special tool. This is the specification line most often left out of a quotation and most often discovered on the drawing review afterwards.
How the floor handles the length. A 4,450 mm panel in 3 mm steel weighs about 105 kg for every metre of width. Two operators lifting it from the middle will bow it; a panel bowed during handling reads a twist that is not in the metal. Ask how long parts are moved, and where they are stored.
Minimum flange, hole-to-bend and the geometry nobody quotes
Two geometric limits decide whether a bend is possible at all, and both are functions of the die.
The minimum flange on a V-die is half the die opening plus the thickness, because the flange has to rest on both die shoulders before the punch descends. On an 8 × t die that is 4t + t = 5t. For 3 mm sheet, a 15 mm flange. Below that the part tips into the die, the angle is unpredictable, and the operator compensates by feel.
The hole-to-bend distance is the second limit. The owning rule is R + V/2 + t: the deformation zone reaches out from the bend line by the inside radius plus half the die opening plus the thickness. An M8 hole in 3 mm sheet with a 3 mm inside radius on a 24 mm die therefore needs 3 + 12 + 3 = 18 mm of clear distance. Anything closer is either moved or cut after forming, and the hole-to-bend distance article works through the rule in full.
Both are cheap to check at the drawing review and expensive to find at first article. If a design cannot meet them, the answers are a narrower die, a different sequence, or a change to the part — and the third is usually the cheapest.
Worked flat length, and why the bend deduction matters to a buyer
The flat length is the number everything else depends on: the blank size, the nesting, the material cost and the hole positions before forming.
For a 3 mm CRCA part with an inside radius of 3 mm and two outside dimensions of 50 mm and 40 mm meeting at 90°, with K = 0.33:
Bend allowance = (π/180) × 90 × (3 + 0.33 × 3) = 1.5708 × 3.99 = 6.27 mm. Outside setback on each side = (R + t) × tan(45°) = 6.00 mm, so 12.00 mm in total. Bend deduction = 12.00 − 6.27 = 5.73 mm. Flat length = 50 + 40 − 5.73 = 84.27 mm.
Change K to 0.35 — a plausible difference between two shops' tables for the same grade — and the bend allowance becomes 1.5708 × 4.05 = 6.36 mm, the deduction 5.64 mm, and the flat length 84.36 mm. Nine hundredths of a millimetre on one bend. Over six bends it is over half a millimetre, which is the scale at which a hole pattern stops lining up.
That is why a buyer should ask which K-factor the supplier uses and whether it was proved on the grade being quoted, rather than accepting "we use standard values". The press tonnage calculator reproduces the force numbers in the table above.
Setup, batch size and the real cost structure
A bending price is material, machine time, setup allocation, secondary operations, inspection and packing. Material and machine time are broadly comparable between competent shops. Setup allocation is not.
Consider a part with six bends and two tool changes. Tool change plus first-off approval is, say, 30 minutes of machine time. At 50 pieces that is 36 seconds of setup per part. At 5,000 pieces it is 0.36 seconds. The same physical operation is priced two orders of magnitude apart, and neither supplier is wrong.
Two questions resolve it. First: how many setups does this part need, and what is in each? A supplier who can answer in tool widths and bend sequence has reviewed the part. Second: how is setup charged at low volume — absorbed, charged once per release, or amortised into the piece price? A quote that shows setup separately lets you compare like with like and lets you decide whether a design change that removes one setup is worth making.
The quotation comparison article sets out the full line structure to ask for.
How Ganesh Multitech runs CNC press brake bending
Bending is done on the 200 T, 5-axis CNC press brake with a 4,450 mm bed, Delem control and a 10 mm maximum thickness. The Delem programme holds the material, thickness, angle, springback correction and bend sequence for each part, so a repeat release starts from the approved setup rather than from a drawing and an operator's judgement.
Sheet arrives from a 12 kW fibre laser with a 40 ft × 16 ft bed, which means a 4,000 mm blank is cut in one piece and the brake locates against an edge whose quality is classified under ISO 9013. That combination is what makes a long enclosure side or a rack upright a single-hit bend instead of a spliced one. Ganesh holds ±0.5 mm as a typical sheet metal tolerance, with tighter tolerance on critical features by agreement.
The full machine list and materials sit on the sheet metal bending capability page. Ganesh has manufactured sheet metal since 1992 across five units in Mumbai (Vasai) and Nagpur, under ISO 9001:2015 and ISO 14001:2015, with PPAP and first article inspection available. The 200 T press brake article covers what that class of machine changes about part design, and press brake tool selection covers the tooling side.
Eight questions to ask before you compare two quotes
- What tonnage and bed length will be used, and what is the longest bend at my thickness in my material?
- Which die opening, and therefore what is my minimum flange?
- How many setups does the part need, and what is in each?
- Is the punch 5-axis capable, and does the part need it?
- Which K-factor and bend table, and was it proved on this grade?
- Is the machine crowned, and what angle variation is expected across the length?
- What gauge and method will be used to check the angle at first article?
- What is stored in the programme, so the next release is the same as this one?
A supplier who can answer all eight has done the review. A supplier who answers four has quoted a machine.
When a press brake is the wrong answer
It is the wrong process when the profile is constant over a long run — a roll-formed section holds a cleaner surface and a lower piece price above a few thousand metres a year. It is the wrong process when the shape is a drawn cup or a housing, where the forming is a press and tool question. And it is the wrong process when the annual volume and the tolerance both point at a dedicated tool, which the forming route comparison works through with the crossover arithmetic.
Ganesh does not roll-form, and does not claim a 10 mm bend across a 4,450 mm bed — the tonnage table shows why that is arithmetically impossible. Stating the real limit is more useful than a capability line that fails at the drawing review.
Send the drawing with the material, thickness, flange lengths, annual quantity and whether a tool already exists, or request a quotation with the pack attached. The review comes back with the die opening, the force per metre, the length limit and the setup count, which is everything needed to compare two bending quotes on the same basis.
Frequently asked questions
What tonnage press brake do I need for 3 mm steel?
On an 8 × t die opening, 3 mm CRCA at 450 MPa needs about 24.4 tonnes-force per metre, so a 200 T machine holds roughly 8 m. The bed limits a 4,450 mm part before the tonnage does. At 6 mm the same machine only holds 4.1 m, and the tonnage becomes the limit.
What is the shortest flange a press brake can bend?
About five thicknesses on an 8 × t die, because the flange has to span the die shoulders plus the thickness: V/2 + t. For 3 mm that is 15 mm. A shorter flange needs a narrower die, a special punch, or a design change.
How much does a 5-axis press brake matter compared with a 3-axis machine?
It matters for box sections and return flanges. A tilting punch lets the tool swing clear of an upstand that would collide with a fixed punch body, which is the difference between forming a 150 mm deep channel in one setup and not forming it at all.
Why are two bending quotes for the same part so far apart?
Usually setup allocation, not machine rate. A part with six bends and two tool changes carries roughly 30 minutes of setup; across 50 pieces that is 36 s per part, and across 5,000 pieces it is 0.36 s. Both suppliers can be honest and the totals still differ.
Do I need to supply a flat pattern with the drawing?
No, but supply the K-factor or bend allowance basis if you have proved one. Otherwise the supplier computes the flat from their own table, and the first article confirms it. A 0.02 error in K costs 0.094 mm of flat length per bend at 3 mm.
Can a press brake replace a stamping tool?
Below a few thousand pieces a year, usually yes for simple parts, because there is no tooling to amortise. Above that, or where the part needs a drawn shape, a coined feature or a tolerance that only a tool can repeat, pressing wins. The crossover is a quantity question, not a machine question.
Sources
- ISO 2768-1:1989 — General tolerances, Part 1: linear and angular dimensions without individual tolerance indications · 3 Nov 2026
- ISO 9013:2017 — Thermal cutting, classification of thermal cuts, geometrical product specification and quality tolerances · 3 Nov 2026
- ISO 129-1:2018 — Technical product documentation, presentation of dimensions and tolerances · 3 Nov 2026
Send the part and the quantity per release
Give us the drawing, material, thickness, flange lengths and annual volume. The review returns the tonnage, the die opening, the setup count and the length limit for your part.
Request a quote