200 T Press Brake Bending for Industrial Parts

A 200 T press brake will bend 10 mm steel. It will not bend 10 mm steel over 4,450 mm with an 80 mm die, because that job needs 2,765 kN and the machine is rated at 1,962 kN. The rating is a force at the tool, and the drawing is a thickness and a length; the two are connected by a formula most drawings never mention.

200 T press brake bending is therefore a load calculation before it is a machine capability. A part is approved as "10 mm, fits the 200 T" and then the first-off comes out short at one end, or the die has to be opened up and the inside radius no longer meets the drawing. Both outcomes are predictable from three numbers: die opening, bend length and material strength.

The bending and welded assemblies hub collects the rest of this cluster. This page converts the 200 T rating into bend lengths you can design against, and sets out what the 4,450 mm bed and the 5-axis control actually change.

What 200 T press brake bending actually limits

The rating limits force, not thickness. 200 tonne-force is 1,962 kN, applied over the contact area between punch and workpiece. Air bending — the normal production method, where the punch does not bottom in the die — needs a force that follows this relationship:

F = 1.42 × σb × t² × L ÷ (1,000 × V)

where F is in kN, σb is the tensile strength in MPa, t is thickness in mm, L is bend length in mm and V is the V-die opening in mm. The 1.42 factor accounts for the geometry of a standard V-die and the friction in the bend.

Two things fall out of it. Load rises with the square of thickness, so doubling thickness quadruples the force at the same die opening. And load rises with bend length, so the same thickness over twice the length needs twice the tonnage.

A 6 mm CRCA part, 2,000 mm long, in a 48 mm die at 350 MPa tensile:

F = 1.42 × 350 × 36 × 2,000 ÷ (1,000 × 48) = 745 kN, or 76 tonne-force.

That is comfortable. Now take the same 6 mm on the full 4,450 mm bed: 745 × (4,450 ÷ 2,000) = 1,658 kN, or 169 tonne-force. Still inside the rating, but the margin has gone from 62% to 15%.

Tonnage by thickness on the 200 T brake

The table uses a die opening of 8 × thickness, 350 MPa tensile strength and air bending. The maximum length column is 1,962 kN divided by the load per metre, capped at the 4,450 mm bed.

The bed is 4,450 mm with a Delem control, and the machine is rated to 10 mm thickness. Read the last two rows as a warning rather than a limit: the thickness is inside the rating and the length is not.

Why 10 mm needs a wider die, not a bigger machine

At 10 mm and 4,450 mm, an 80 mm die needs 2,765 kN, which is 41% over the rating. Opening the die to 120 mm changes the load per metre to:

1.42 × 350 × 100 × 1,000 ÷ (1,000 × 120) = 414 kN/m

Over 4,450 mm that is 1,843 kN, or 188 tonne-force. The part fits, at 94% of the machine rating and with an inside radius of 120 × 0.156 = 18.7 mm.

The alternative is to bottom or coin the bend, which forces the punch into the material to set the angle and radius. Coining needs roughly three to five times the air-bend force, which puts 10 mm at full length far outside the machine. On this brake, 10 mm is an air-bending thickness.

That leaves the designer with a choice that has nothing to do with tonnage. Accept the large radius the wide die produces, redesign the part so the bend is shorter than 3,160 mm, or change the material to something with lower tensile strength. A 10 mm part with an R10 callout at full bed length is not manufacturable on a 200 T brake, and it is better to say so at quotation than to discover it at try-out.

A 6 mm base frame checked both ways

A genset base frame with two 2,400 mm bends in 6 mm CRCA is a typical industrial part, and it shows how the radius decision moves the tonnage.

At a 48 mm die the inside radius is 7.5 mm and the load per metre is 373 kN/m. Over 2,400 mm that is 895 kN, or 91 tonne-force per bend, run one bend at a time. The machine is using 46% of its rating, which leaves room for a material batch at the top of its tensile range.

The drawing says R6. To get R6 in air bending the die opening has to be about 6 ÷ 0.156 = 38 mm, and at 38 mm the load per metre rises to 471 kN/m, or 1,130 kN over 2,400 mm — 115 tonne-force. Tightening the radius by 1.5 mm costs 26% more load. It still fits, and it is the right answer if R6 is functional. If R6 was simply copied from a thinner part, it is 24 tonne-force bought for nothing.

The flat pattern follows from the radius: with R6, t6 and K = 0.42, the bend allowance is 1.5708 × (6 + 2.52) = 13.38 mm and the bend deduction is 2 × 12 − 13.38 = 10.62 mm. Cut the blank to the flange lengths minus 10.62 mm at each bend, not to the outside dimensions.

Springback, crown and the 4,450 mm bed

Three errors show up on formed parts, and they have different fixes.

Springback is the elastic recovery when the punch lifts. Mild steel and CRCA recover about 0.5–2° on a 90° bend; stainless and aluminium recover more. At the same R/t the recovery is independent of thickness, so a gauge change moves the angle only through the radius and die opening it brings with it. The control compensates from the material table, but the table is an assumption until the first-off confirms it.

Crown error is geometric. Under load the ram deflects upward and the bed deflects downward, so the gap is widest at the centre of a long tool and the material there gets less penetration. Without compensation, a 3,000 mm bend loses 1–2° between the ends and the middle. The fix is a crowned bed or a control that applies a load-dependent curve, which is what the Delem control on this machine does using the material and thickness in the program.

Twist is a handling problem. A long, narrow part bends out of plane if it is not supported at both ends, and the twist does not show on a single-end angle check. Measure both ends and the middle of every long first-off; the inspection method is set out in bending tolerances and inspection.

What the 5-axis control changes

A 5-axis brake controls Y1 and Y2 (the two ram ends), the back-gauge X, R and Z axes, and crowning; the ram itself moves in depth only. The control uses that combination to correct the angle while the punch is still in contact with the material. In practice it means the machine can compensate for a material batch that springs back differently from the table, without the operator re-hitting the part.

For the designer, the useful consequence is that angle-critical parts with several bends become a single setup rather than a sequence of corrections. For a buyer, the consequence is that a part which needed hand correction on an older brake can be quoted as a repeatable operation. The machine does not change what geometry is possible; it changes how much of the tolerance band the process consumes.

Bend sequence and tool access

Load is only half of what a machine has to do with a part. The other half is whether the punch can reach each bend in an order that does not collide with a flange already formed.

Three rules cover most sequences. Bend the longest flange first, so the part keeps a stiff section for as long as possible. Bend toward the outside and finish on the inside, because a flange formed early blocks the punch path on a later bend if it points the wrong way. And keep all flanges that point the same direction in one setup, so the part is turned once rather than three times.

On a 4,450 mm bed the sequence interacts with handling as well. A 4,000 mm panel needs support at both ends throughout the stroke; without it, the panel sags and the bend picks up a twist that no angle correction fixes. That is a reason to plan support at the quotation stage, not only tonnage.

Working out the flat pattern

A bend is specified by its inside radius and its angle, and the blank is cut to a flat length that assumes a bend allowance. Get the allowance wrong and the flange comes out short or long by a fraction of a millimetre per bend, which compounds over a part with four bends.

For a 90° bend, the bend allowance is:

BA = π × (R + K × t) ÷ 2

with R the inside radius, t the thickness and K the neutral-axis factor, typically 0.33–0.5 for cold-rolled steel depending on the R/t ratio.

A 3 mm part with a 6 mm inside radius and K = 0.42:

BA = 3.1416 × (6 + 1.26) ÷ 2 = 11.40 mm

The bend deduction is 2 × (R + t) − BA = 2 × 9 − 11.40 = 6.60 mm, so the flat length is flange A plus flange B minus 6.60 mm. The full method, including the R/t dependence of K, is in how to calculate bend allowance, and the bend allowance calculator does the arithmetic for a multi-bend part.

What to put on the drawing

Seven fields cover the whole bending decision:

1. Material grade and actual thickness, because tensile strength drives tonnage.
2. Inside radius at every bend, not the outside radius.
3. Bend length and the overall developed length, so the load can be checked.
4. Flange lengths, so the minimum flange rule and tool access can be confirmed.
5. Bend sequence or a note that the supplier may choose it.
6. Critical angles and which face is the datum.
7. Whether surface marks from the punch are acceptable on the outside face.

Field four catches more redesigns than the rest. A flange shorter than the die opening plus the punch radius cannot be formed in a standard tool, and the fix is a different tool or a longer flange. Minimum flange length for press brake parts gives the numbers.

The brake, the bed and the tool room

The 200 T, 5-axis CNC press brake has a 4,450 mm bed and a Delem control, and it forms to 10 mm. It sits alongside mechanical presses from 20 T to 300 T, so a part that moves from prototype bending to a formed tool does not leave the plant, and a 250 T punching capacity handles the pierced features that would otherwise be a second operation.

Bent parts usually become welded assemblies here: three CLOOS robotic MIG cells and more than 30 manual MIG, MAG, spot and SPM stations, with fixtures designed and built in-house. That matters because a bent frame that fits at bending can still move at welding, and the genset parts route shows how base frames and canopy panels are sequenced. Typical sheet metal tolerance is ±0.5 mm, tighter on critical features by agreement.

When this is the wrong route

The brake is the wrong route above 10 mm thickness, and above 4,450 mm in bend length. A 12 mm part needs a larger machine or a different process; a 5,000 mm bend needs a splice, because the tool cannot form a bend it does not cover.

It is also the wrong route at volume. A part with three bends at 30,000 pieces a year belongs in a press tool, where the forming happens in the stroke rather than in three handling operations. And it is the wrong route for a box with return flanges on all four sides if the flanges are deep, because the punch cannot enter the box without colliding; that part needs a different bend sequence or a fabricated corner, and the box bending guide covers the geometry.

When the part fits, send the drawing with the seven fields above. We will confirm the die opening, the tonnage at each bend and the flat pattern before the first blank is cut, so the first-off is a confirmation rather than a discovery.