K-factor in CAD for sheet metal: why model and brake disagree

A hat channel cut from a 386.1 mm blank came off the brake 1.46 mm over the developed length. The blank matched the CAD flat exactly. The model had used K = 0.44 with a 2 mm inside radius, and the brake ran a 16 mm V die, which puts the inside radius at about 2.56 mm on 2 mm CRCA. Four bends at roughly 0.37 mm each account for the whole error.

Nothing was machined wrong and nobody misread the drawing. The model described a process the shop was not running. That is the normal failure mode for the K-factor in CAD: the number is treated as a material constant when it is a record of a tooling decision that has not been made yet.

Why does the CAD flat pattern disagree with the brake?

The model calculates the flat from an assumed inside radius and an assumed neutral axis position. The brake produces a radius from the die opening, the material's yield strength and the amount of springback it has to overcome. Two of the three inputs to the bend calculation are guesses in CAD and measurements at the machine.

The geometry is fixed. For a bend of angle θ in radians:

BA = θ × (R + Kt)

where R is the inside radius, t is the thickness and K is the neutral axis offset as a fraction of thickness. The bend deduction for a single bend is:

BD = 2 × (R + t) × tan(θ/2) − BA

For a 90° bend this simplifies to BD = 2(R + t) − 1.5708(R + Kt). The flat length is the sum of the outside flange lengths minus one bend deduction per bend.

K enters only through the second term. That is why a K error alone is small: moving K from 0.44 to 0.33 on 2 mm sheet changes the deduction by 0.53 mm. A radius error is larger, because R appears in both terms and because the die that produces the radius also changes the tonnage. When both move together, as they do when the model assumes a 2 mm radius and the shop runs a 16 mm die, the deduction moves 0.37 mm per bend.

Where the K-factor in CAD comes from

Most sheet metal CAD tools ship a default between 0.40 and 0.50, or a bend table keyed to material and thickness. The default is a compromise value that produces a usable flat for a mid-range die. It is not a measurement of your process.

The real range is narrower than the arguments suggest. On mild steel, K runs from about 0.33 at R/t = 0.5 to 0.50 at R/t = 5, because a tight bend forces the neutral axis towards the inside surface and a generous bend lets it sit near mid-thickness. On 2 mm CRCA that is a radius range from 1 mm to 10 mm.

The radius itself is a tooling output. In air bending, the punch does not coin the inside radius into the sheet unless the punch radius is larger than the natural radius. For mild steel the natural inside radius is roughly 0.16V, where V is the die opening. A 16 mm die gives about 2.56 mm, a 24 mm die about 3.84 mm, and no amount of CAD editing changes either. A drawing that specifies R2 while the shop runs a 24 mm die has specified something the process will not produce without a matching punch radius and enough tonnage to coin.

This is also why the same part quoted by two suppliers can produce two different flats from the same model: they run different die sets, both legitimate, and neither has told the customer which deduction they used.

The practical fix is to key the bend table to the die rather than to the thickness. A table entry that reads "2 mm CRCA: BD 3.48" is wrong the moment the die changes. An entry that reads "2 mm CRCA, 16 mm V, R 2.56, K 0.40: BD 3.84" can be checked against the machine with one coupon. Most CAD tools allow several rows per thickness in a gauge table, selected by the operation instead of by the material.

Bend deduction by die opening for 2 mm CRCA

The table below is calculated for 2 mm CRCA at 450 MPa tensile, 90° air bends, with the natural radius taken as 0.16V and K read from the R/t curve. The force column is the tonnage per metre at that die opening, and the Ganesh column compares it with the 200 T brake across the 4,450 mm bed.

The tonnage figures use F = 1.42 × σb × t² / V in kN per metre, with σb in MPa, t and V in mm. They are the reason the die cannot simply be swapped to chase a radius: the 8 mm die needs three times the force of the 24 mm die for the same bend.

A four-bend channel, recalculated

Take a hat channel in 2 mm CRCA with outside legs of 40, 60, 200, 60 and 40 mm, formed on a 16 mm V die with four 90° bends.

The sum of the outside legs is 400 mm. At the brake, with R = 2.56 and K = 0.40, each bend deducts 3.84 mm, so the blank is 400 − 15.37 = 384.63 mm.

The CAD model with R2 and K = 0.44 deducts 3.48 mm per bend and produces 400 − 13.90 = 386.10 mm. The blank is 1.47 mm longer than the process can absorb, and each of the four legs comes out about 0.37 mm long. On a channel that carries a hole pattern at each end, the holes land 0.37 mm outside the mating face, and the welder closes the gap with force.

Now run the same CAD blank through a 24 mm die. The deduction at that die is 4.30 mm, so the correct blank is 382.80 mm. The 386.10 mm blank is 3.3 mm long, and the part is 3.3 mm over the outside envelope. Same model, same material, same machine, different die, three times the error.

The second case is the one that catches experienced buyers, because the model looks more conservative. A larger die is not a smaller error; it is a different deduction.

A coupon removes the argument. Cut a 100 mm × 100 mm blank, form one 90° bend on the die you intend to run, measure both outside flanges and the inside radius, then back out the deduction as BD = A + B − flat. One coupon per material, thickness and die pins the table for the life of the job, and it takes less time than a single concession.

What the model gets wrong when the die changes

Four things move when a job changes die, and only one of them is K.

The radius moves first. Natural radius scales with the die opening, so the bend deduction follows it. A model that stores one radius per thickness cannot represent two die sets.

Springback moves the angle, not the deduction. A 90° bend on 2 mm CRCA springs back 1–2° depending on the die and the punch radius. The brake compensates by over-bending, which changes the developed length slightly and changes the position of every feature on the flange. CAD usually models the finished angle and ignores the over-bend entirely.

The bend table revision drifts. A bend table saved with the template is copied between projects and edited by whoever is in a hurry. Two models of the same part in the same company can carry different deductions. The drawing needs to state which revision was used.

Imported models carry the customer's assumption. A STEP file from an OEM contains geometry, not a process. The bend radii in it are whatever the OEM's CAD default produced. Developing a flat from that model without checking the radii is how a first article becomes a concession.

What Ganesh runs

Bending is on a 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, forming up to 10 mm. The bed length is relevant here because long parts are formed in one setup rather than repositioned, which removes a class of cumulative error between hits. Tooling comes from the in-house tool room, and the die opening is recorded per job so the flat can be calculated from the die that will actually run.

Cutting is a 12 kW fibre laser with a 40 ft × 16 ft bed, with 6 kW and 3 kW support machines, so a 3,000 mm blank and its bend marks come off in one setup. Welding is three CLOOS robotic MIG cells and more than 30 manual MIG, spot and SPM stations, with fixtures designed and built in-house. Coating runs through seven-tank pretreatment, an 18 ft × 14 ft powder booth and a curing oven, with DFT and cross-hatch adhesion checks.

Typical sheet metal tolerance is ±0.5 mm, tighter on critical features by agreement, and PPAP with first article inspection is available. The bending capability page lists the machine and tool set. The K-factor measurement procedure covers how to back-calculate K from a formed coupon when you need your own number rather than a table.

What to put on the drawing

• Material grade, nominal thickness and the measured thickness range of the coil or sheet.
• Inside radius per bend, and whether it is fixed by the punch or left natural.
• The V die opening the flat was calculated against.
• The bend deduction or the K value used, with a bend table revision identifier.
• Outside flange lengths, not only overall dimensions, so the deduction can be checked.
• A note on which dimensions are critical after forming, with the tolerance on each.
• Bend sequence where a flange would collide with the punch.
• Whether the flat pattern is released for manufacture or for reference only.

The last item prevents most disputes. A flat marked "reference" tells the supplier to develop their own and return it for approval. A flat marked "manufacture" makes the customer responsible for the deduction, which is a decision worth taking deliberately.

When the CAD flat is the wrong deliverable

If the part is welded into an assembly and the assembly is machined or checked after welding, the flat is not the controlling document. The welded assembly drawing and its datum scheme are. Sending a flat with a tight developed length invites the supplier to optimise a dimension that the weld will move anyway.

If the design needs a radius below the material's minimum, no K value rescues it. A 0.5 mm inside radius on 3 mm CRCA will crack or orange-peel regardless of the deduction. The minimum bend radius by material gives the floor, and the bend allowance calculation shows the full arithmetic if you want to reproduce the numbers above.

We do not run 3D five-axis laser trimming or tube laser cutting, so a formed part that needs a hole only reachable after bending is outside the route here. We also do not develop flats against a die set we do not own; if the drawing names a die, it has to be one we can load on the 200 T brake.

Send the model, the material and the die you intend to run to request a quote. We will return the flat we would cut, the bend deduction per bend and the first article plan, so the model and the brake start from the same number. More design rules sit in the design and CAD hub, and the STEP file review notes cover what to check before the model leaves your desk.