STEP files for sheet metal bend review

A bracket arrives as a 6.4 MB STEP file. It looks correct in the viewer, the bend radii are tidy, and the drawing says 2 mm CRCA. The review finds that bend 7 has a 6 mm flange and bend 12 needs the punch to enter a channel 34 mm deep. Neither is formable on the tool the quote assumed, and both would have been visible in ten minutes if anyone had measured the model instead of looking at it.

STEP files for sheet metal bend review are a geometry handover, not a manufacturing instruction. The file states where the metal ends up; it does not state which way each bend runs, what K-factor produced the flat length, or whether the tool can reach. Those three things have to be derived or supplied, and the review is the step where they are checked.

This matters most on parts with more than four bends, where the error compounds. The bending and welded assemblies hub collects the related guides on tooling, tolerance and the flat pattern.

What a STEP file carries, and what it leaves out

A STEP file is an ISO 10303 exchange file. AP214 (ISO 10303-214, now superseded by AP242) carries the core geometry for mechanical design; AP242 (ISO 10303-242) adds managed model-based 3D engineering, which includes semantic PMI, tolerances and annotations. Both describe the boundary representation: faces, edges, vertices and the surfaces between them.

What neither format guarantees is sheet metal intent. A folded solid exported from a modeller is a solid with thin walls and filleted corners. The bend line exists only as a pair of tangent edges, and the direction of the bend is not recorded unless the exporter writes a bend table, a flat pattern body or PMI. Open the same file in two CAD systems and one will show 14 bends while the other shows 13, because a pair of near-tangent faces was interpreted differently.

The practical consequence is that the supplier rebuilds the sheet metal feature tree from the geometry. That is normal and it is fast, but it means the review has to be explicit about what was assumed. If the model was mounted at nominal thickness and the coil runs 0.08 mm light, the derived flat pattern will be short by roughly 0.1 mm per bend.

Export settings decide how much of the geometry survives. Most modellers write B-rep surfaces exactly and tessellate only for display, so a well-exported STEP measures to 0.001 mm. A model exported through a viewer or a mesh converter arrives as facets, and a 2 mm fillet then measures as a chain of flat triangles that no bend review can use. The tell is file size against complexity: a simple bracket that arrives at 40 MB is usually mesh, and a 300-face enclosure that arrives at 900 kB is usually exact.

Units are the other silent fault. A model built in inches and exported without conversion reads 25.4 times too large, and a 2 mm sheet becomes 50.8 mm. The review catches it immediately because the thickness check fails, but a part exported at 0.1 scale slips through and quotes as a miniature. Confirm the unit line before measuring anything.

A STEP file also carries no material. The colour may be grey, and grey is not a grade. Material, thickness, coating and the tolerance class belong on the drawing or in the accompanying PDF, and a model without them cannot be quoted.

What a sheet metal bend review checks on the formed model

The thickness check is the one most often skipped. Measure at the four corners and the centre of a large face. A model built from nominal 2.0 mm sheet that reads 1.94 mm at one corner has a face offset error, and the flat pattern derived from it will be out at every bend on that face. The tolerance for a modelled wall is ±0.05 mm; anything looser is a modelling fault, not a material condition.

The bend relief check matters on parts with a bend that terminates inside a face rather than at an edge. Without a relief, the material at the end of the bend tears or draws a wrinkle into the flat face. The relief needs to be at least as wide as the thickness and as deep as the thickness plus the inside radius. A 2 mm sheet on a 2 mm radius needs a 2 mm × 4 mm relief, and it is a two-minute change in the model.

Reading radius and flange length off the model

Bend radius is measured on the inside of the bend, from the model's cylindrical face, and it has to match a tool that exists. A model with a 1.4 mm inside radius in 2 mm steel is asking for a radius tighter than the material will take without cracking, and no standard punch produces it. The default is 1.0 × thickness for mild steel, 1.0–1.5 × thickness for CRCA depending on temper, and 1.0 × thickness for 304 stainless with the bend line across the rolling direction.

Flange length is measured from the bend line to the free edge, on the outside of the flange, and it has to clear the die shoulder. On a V-die with an 8 × thickness opening, the minimum flange is roughly V/2 + t, which works out at about 5 × thickness. For 2 mm sheet on a 16 mm V-die that is 10 mm, and a 2 mm inside radius does not change it. Below that the flange drops into the die opening and the bend collapses.

A short flange is not always a defect. It can be formed with a narrower die, which raises tonnage and marking, or with a special punch that reaches past the die shoulder. The review should flag it with the tool that will be used, not reject it outright. The minimum flange guide covers the tool options.

When the flat pattern and the formed model disagree

The flat pattern is a function of the bend allowance, and the bend allowance is a function of the K-factor. For a 90° bend:

BA = π × (R + K × t) × θ / 180

With R = 2 mm, t = 2 mm, K = 0.44 and θ = 90°, the allowance is π × (2 + 0.88) / 2 = 4.52 mm. The setback is (R + t) × tan(45°) = 4.00 mm, so the bend deduction is 2 × 4.00 − 4.52 = 3.48 mm. A CAD system using K = 0.50 returns an allowance of 4.71 mm and a deduction of 3.29 mm. Across eight bends the two flat patterns differ by 1.5 mm, which is enough to fail a hole pattern that spans the part.

That is why the formed model should control. The formed geometry is what the customer measured and what the assembly needs. The flat pattern is a manufacturing derivation, and it changes with the tool and the material batch. When a DXF flat pattern arrives with a STEP, the review compares the two, and any difference is resolved in favour of the formed model unless the customer says otherwise in writing.

Where STEP beats DXF, and where it does not

For bend review, STEP wins. A DXF flat pattern shows the developed shape and the bend lines as annotations, but it cannot show whether two flanges collide in three dimensions, whether the punch clears a return flange, or whether a hole lands on the bend radius after forming. Those are the failures that stop a tool, and they only appear in the formed model.

DXF wins for the cut file. The laser nests from a 2D profile, and a DXF with clean closed contours, correct layer assignment and no duplicate entities cuts faster and with fewer dross problems than a profile sliced out of a STEP. The DXF preparation checklist lists the layer and contour rules the nesting software expects.

The strongest submission is both: the formed STEP as the controlling geometry, the DXF as the cutting intent, and a drawing that states material, thickness, finish and the dimensions that matter at assembly. When the two disagree, the review says so before the tool is set, not after the first 50 parts.

How Ganesh reviews a bend model

Ganesh accepts PDF, DXF, DWG and STEP. A STEP intake runs the checks above in the order listed, because a scale error invalidates every later measurement. The model is opened at 1:1, the body count is confirmed, thickness is measured at five points, and each bend is recorded with its radius, flange length, direction and the tool that will form it.

The flat pattern is then derived from the formed model using the bend allowance for the grade and thickness, and checked against any DXF supplied. The bend allowance calculator is used for the arithmetic on single bends, and the result is written into the setup sheet so the brake operator and the inspector work from the same number.

Forming runs on the 200 T, 5-axis CNC press brake with a 4,450 mm bed, Delem control and capacity to 10 mm. Anything with a bend longer than 4,450 mm is split or referred back, because the tool cannot span it. The bending capability sets out the tooling range, and the bend allowance guide explains the K-factor values used per grade.

Ganesh has manufactured sheet metal since 1992 across five units in Mumbai (Vasai) and Nagpur, with ISO 9001:2015 and ISO 14001:2015 certification. PPAP and first article inspection are available, and a first article for a bent part reports flange lengths, included angles and the hole pattern after forming.

What to send with the model

• The STEP file, AP242 if your CAD exports it, at 1:1 in millimetres.
• The drawing revision that the model matches, with material, thickness, finish and the tolerance class.
• The bend-critical dimensions, marked on the drawing, so the review knows which flange cannot move.
• Any proven bend table for the grade, if the flat pattern matters to your assembly.
• The DXF flat pattern if you have one, labelled as derived or controlling.
• The assembly the part fits into, or at least the mating part number, so the review can check tool access in context.

The K-factor explainer covers how the allowance changes with grade and radius, which is the usual source of a flat-pattern disagreement.

When a STEP-only submission is the wrong route

A STEP file on its own is not enough when the part is defined by tolerances rather than by geometry. A welded bracket with a 0.5 mm flatness callout on a machined face, a part with a datum scheme that does not follow the model origin, or a component that must match a customer's checking fixture all need the drawing, and often the fixture definition, before a route can be quoted.

It is also the wrong route when the model is a surface model rather than a solid, when the file was exported from a viewer rather than the native CAD, or when the revision in the file name does not match the revision on the drawing. In each case the review stops and asks, because guessing costs more than the day it takes to get the right file.

Send the formed model, the drawing revision and the bend-critical dimensions. The engineering team will return the flat pattern, the tool plan and a list of any feature that cannot be formed as drawn, with the change that would fix it.