Flat pattern for sheet metal: what the CAD flat must contain

A flat pattern arrives as a DXF with the outline, the holes and nothing else. The part is cut, bent, and comes back 4 mm long across a chain of three bends. The CAD flat was geometrically correct as an unfolded surface and completely wrong as a manufacturing instruction, because the bend deduction it used was the software default and the shop's tooling does not produce that default.

Flat pattern for sheet metal is the hand-off between design and the laser. Everything the shop needs to make the part without asking a question has to be on it, and the first item is not the outline. It is the bend data: which lines bend, in which direction, at what radius, and by how much the material shortens.

The numbers below are worked at 2 mm CRCA with a 2 mm inside radius, which is the most common combination we see, and they show how a 0.08 change in K-factor becomes a millimetre on the finished part.

What must a flat pattern contain?

A flat pattern must contain eight things: true developed geometry at 1:1, bend lines with direction and radius, the bend allowance or deduction used, bend and corner reliefs, a datum, material and thickness, grain direction, and a revision that matches the drawing.

Take them in order of what goes wrong when they are missing.

Developed geometry. The outline is the part unfolded through the neutral axis, not the outside profile flattened. If the CAD unfolds on the outside surface, every flange comes out long by the bend deduction, and the error is systematic, so every part is wrong in the same direction.

Bend lines. A line with no direction is half a bend. Up and down matter on a box, because two bends in the same direction give a channel and two in opposite directions give a Z, and the flat is the same shape for both.

Bend data. The inside radius per bend and the K-factor or bend deduction table. This is the item most often left off, and the one that turns a correct flat into a part that does not fit.

Reliefs. A bend that stops inside the outline tears at its end unless there is a notch. A three-way corner buckles unless there is a corner relief.

Datum. The same datum as the formed drawing, marked on the flat, so the inspector measures the flat and the formed part from the same feature.

Material and thickness. Including the tolerance on thickness, because a 2.0 mm sheet that arrives at 1.85 mm develops differently.

Grain direction. For aluminium and for any part that will be bent on a tight radius, the rolling direction decides whether the bend cracks.

Revision. A flat that does not carry the drawing revision is the one that gets cut after the design changed.

The bend deduction, worked at 2 mm

The bend allowance is the length of the neutral axis through the bend:

BA = θ × (R + K × t)

For a 90° bend, θ is 1.5708 rad. With R 2 mm, t 2 mm and K 0.42:

BA = 1.5708 × (2 + 0.84) = 4.461 mm

The bend deduction is what you subtract from the sum of the outside dimensions:

BD = 2 × (R + t) − BA

BD = 2 × 4 − 4.461 = 3.539 mm

Two flanges each dimensioned 100 mm outside therefore develop to:

100 + 100 − 3.539 = 196.461 mm

Not 200 mm, and not 196 mm. The 3.5 mm difference is the material that goes into the radius, and it is the number the laser needs before it cuts.

Now change K to 0.50, which is the value many CAD packages use as a default for mild steel:

BA = 1.5708 × (2 + 1.0) = 4.712 mm

BD = 8 − 4.712 = 3.288 mm

Flat length = 196.712 mm

The difference is 0.25 mm on one bend. On a four-bend part, if every bend is in the same chain, that is 1.0 mm, which is twice the ±0.5 mm we hold on formed features and enough to fail a fit.

K is not a constant. It changes with the ratio of inside radius to thickness, and it changes with the tooling and the material. The values below are starting points for mild steel air bending, and the only value that counts is the one measured on the first article.

Reliefs: the geometry that keeps a bend from tearing

A bend relief is a notch at the end of a bend line that lets the material flow instead of tearing. Two dimensions matter:

• Width: at least the material thickness, and never less than 1 mm. On 2 mm sheet, 2 mm.
• Depth: at least R + t beyond the bend line, so the relief clears the tooling. On 2 mm with a 2 mm radius, 4 mm.

The relief is cut in the flat, so it appears in the developed outline, and it is the feature most often omitted when a designer models a part as a solid and asks the software to unfold it. The software will produce a flat with a sharp internal corner at the end of the bend, the laser will cut it, and the part will tear on the first hit, or worse, on the tenth part when the tooling has warmed.

Corner relief at a three-way intersection needs to be larger, because three bends meeting at a point all pull material towards the same corner. A relief radius of 1.5 × t is the working minimum: 3 mm on 2 mm sheet. The relief also gives the brake punch somewhere to sit when the second bend is formed, which is a forming requirement as much as a tearing one.

Grain direction and material

Rolled sheet has a direction. Bending across the rolling direction uses the material's ductility; bending along it concentrates strain at the inclusion lines and cracks earlier. For 5052 aluminium the difference is visible at tight radii, and for 304 stainless it shows as orange-peel on the outside of the bend.

Mark the rolling direction on the flat with a note and an arrow. For a part with one critical bend, orient that bend line across the grain. For a part with bends in both directions, the flat cannot satisfy both, and the design has to accept a larger radius on the bend that runs along the grain. The minimum bend radius guide gives the values by material and temper.

Thickness tolerance belongs here too. IS 513 sheet is supplied to a thickness tolerance, and a 2.0 mm nominal that measures 1.85 mm changes the bend allowance by about 0.10 mm per bend and the bend deduction by about 0.20 mm per bend. On a part with a tight developed length, specify the actual thickness range and develop from the middle of it.

Coating, masking and the flat

The flat is the pre-coat geometry. Powder coating at 60 to 90 µm per face adds 0.12 to 0.18 mm to any dimension measured across two coated faces, and it closes holes by twice the coating thickness.

Two consequences for the flat:

1. A hole that takes a locating pin or a close-fit fastener needs either a mask or 0.15 mm added to its diameter in the flat. Masking is cleaner, because it keeps the hole round and the edge protected.
2. An overall dimension that fits into an opening, such as a 482.6 mm rack panel, has to be developed with the coating in mind. A panel cut at 482.6 mm and coated on both ends measures 482.75 mm over the coating and will not enter the rails.

The powder coating on laser-cut edges covers how the cut edge takes the coat; the flat pattern point is that the coating is a post-cut operation and the flat has to leave room for it.

What Ganesh runs

We cut from DXF, DWG, STEP and PDF. A STEP of the formed part is the cleaner input, because we develop the flat against the tooling we will actually use: the punch radius, the die opening and the measured K-factor for the material and thickness. A DXF flat is accepted when it carries the bend deduction that produced it, and it is checked against the formed model before the laser runs.

Cutting is on the 12 kW fibre laser with the 40 ft × 16 ft bed, so a 3,000 mm developed blank comes off in one setup, with ±0.2 mm position on the flat. Forming is on the 200 T, 4,450 mm, 5-axis brake with Delem control, to ±0.5° and ±0.5 mm on formed features, and the long bed means a part that would otherwise be formed in two hits keeps one bend deduction instead of two. Welding, pretreatment and coating follow where the part needs them, and first article inspection reports the developed length, the flange heights and the bend angles.

The bending capability page lists the machine and tool set, and the design and CAD hub collects the bend allowance and datum rules that go with this one.

What to put on the flat pattern drawing

1. Overall developed length and width, with a tolerance of ±0.3 mm.
2. Every bend line as a line on its own layer, numbered, with up or down direction.
3. Inside radius per bend, and the punch radius if it is fixed by tooling.
4. Bend allowance and bend deduction per bend, or a table with the K-factor and the thickness it was calculated from.
5. Bend relief width and depth, and corner relief radius, as dimensions rather than a note.
6. Datum features marked, matching the formed drawing.
7. Material grade, thickness and tolerance, plus the rolling direction arrow.
8. Coating specification and every masked feature, so the flat is cut knowing what happens after.
9. Revision and the drawing number it was developed from.
10. Dimensions and the bend table indicated to ISO 129-1, so the flat reads the same way as the formed drawing.

When the CAD flat is the wrong deliverable

For a stamped or deep-drawn part, the blank is not a CAD unfold. It is developed in the tool room against the die, with draw beads, blank holder force and material flow, and a flat pattern from a CAD package will be wrong by enough to scrap the first tryout. Send the formed part and let the tool room develop the blank.

A flat is also the wrong deliverable when the part has a hem, a joggle or a bend that requires a special tool, because those features change the developed length in ways a standard K-factor does not capture.

Send the STEP with the bend radii, or the DXF with the deduction stated, and note the material, thickness, finish and annual quantity. The flat can be checked against the tooling before the first blank is cut: request a quote, or read the bend allowance guide and the DXF preparation checklist before you export the file.