Blog · Inventor · 1 Oct 2026 · Last updated 13 Oct 2026 · 8 min read · By Stefano B.

How to make an iLogic flat pattern from a STEP solid in Inventor

A bent plate from a STEP file is a dumb solid with no sheet-metal data. The four iLogic lines that turn it into a sheet-metal part and unfold it, the test that tells a real bend from a flat plate, and the flat view that silently draws the folded part instead.

Short answer: set the part's SubType to the sheet-metal GUID, turn off style thickness, set the measured thickness in centimetres, and call Unfold(). Then test the result: Unfold() "succeeds" on flat plates too, and Inventor draws the folded part without a word if there is no flat pattern.

Test Z bracket, 6 mm plate with two bends, as it comes from a STEP file: front view dimensioned outside to outside: bottom flange 114, web 134, top flange 94, overall (202), thickness 6 and inside radius R8. A plain solid with no sheet-metal data and no flat pattern.
From this: a bent plate from STEP is just a solid.
Flat pattern of the same Z bracket, 319.4 x 150 mm, dimensioned from edge to bend line to bend line to edge (88.36, 122.71, 108.36), with the two bend lines in orange, one bend down and one bend up, from the IV_BEND and IV_BEND_DOWN layers of the flat pattern DXF.
To this: the flat pattern, 319.4 × 150 mm, after the four lines below.

The code blocks on this page were run as an iLogic rule in Inventor 2025, copied from this page, on a test bracket and a flat test plate. The images come from the same test bracket we drew for it in Inventor 2025 (Z shape, 6 mm plate, 8 mm inside radius, 150 mm wide), saved as STEP and run through the code on this page. Views and flat pattern are exported to DXF and redrawn; the empty template border and title block are removed, except in the third image, which shows the sheet as Inventor drew it.

This came up on the Autodesk forum more than once: batch flat pattern, bending drawings for all parts in an assembly and convert to sheet metal and set the thickness. This page is the long answer.

The recipe

In an iLogic rule, these lines go first. They are the ones we added to run the blocks on this page:

Dim oPart As PartDocument = ThisDoc.Document
Dim oApp As Inventor.Application = ThisApplication
Dim thicknessCm As Double = 0.6
Dim isBent As Boolean = True
Dim sDxfPath As String = "C:\Temp\flat.dxf"

Then:

oPart.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}"   ' becomes a sheet-metal part
Dim oSM As SheetMetalComponentDefinition = oPart.ComponentDefinition
oSM.UseSheetMetalStyleThickness = False
oSM.Thickness.Value = thicknessCm                            ' measured, in cm
oSM.Unfold()
Try : oSM.FlatPattern.ExitEdit() : Catch : End Try            ' back to the folded model

What to change:

Run it on a copy of the body in a new part, never on the client's file: splitting a STEP multi-body into part files.

Where to paste it: open the part, Manage > iLogic > Add Rule, give the rule a name, paste the blocks in order, click Save & Run. For the DXF, add the line from Flat pattern DXF below at the end. To start the same rule from a script instead: run an iLogic rule from outside Inventor and drive Inventor from the terminal.

There is no thickness in the STEP

A STEP solid has no thickness property. It has to be measured. Volume divided by the largest planar face works only on flat plates: on our flat test plate it gave exactly 6 mm, on the bent test bracket 18.14 mm for a 6 mm plate. In our process the thickness from the job's parts list wins, and it is checked against the drawing.

Is it really bent? Compare the bodies

Unfold() returns without error on a flat plate. To know whether the part is bent, compare the folded body with the flat body. If they are identical, it was never bent:

Dim oColl As ObjectCollection = oApp.TransientObjects.CreateObjectCollection()
oColl.Add(oSM.SurfaceBodies.Item(1))
oColl.Add(oSM.FlatPattern.SurfaceBodies.Item(1))
Dim oIdent As ObjectCollection = oApp.TransientBRep.GetIdenticalBodies(oColl)
If oIdent.Count > 0 Then isBent = False

Do not rely on HasFlatPattern = True. It is true after any unfold.

A flat test plate 200 x 120 x 6 converted to sheet metal: Unfold() gives no error, HasFlatPattern is True, and GetIdenticalBodies on the folded and flat bodies returns 1, so the part was never bent.
A flat plate unfolds without complaint. Only the body comparison says it was never bent.

Another way to find bends in the geometry: a bend is a pair of coaxial cylinders whose radii differ by the thickness. On our test bracket the bends are radii 8 and 14 on a 6 mm plate. We did not run this check on the test parts, and a curved slot can give the same pair of radii: treat it as a hint, not a proof. This would miss a bend stored as a B-spline: see Inventor skips a bend.

Which V-die gives that radius

The inside radius on the drawing is set by the press brake, not by Inventor. In air bending the inside radius comes out at about 16% of the V-die opening. So draw the radius your shop's die gives, and use the same radius in the model. For mild steel (Rm 420 N/mm²), Bystronic's bending table gives:

Plate Recommended V-die Inside radius Min. flange Force per metre
2 mm V12 R2 10 mm 235 kN
3 mm V24 R3.5 17.5 mm 240 kN
4 mm V32 R5 25 mm 315 kN
5 mm V40 R6 31 mm 430 kN
6 mm V50 R8 36 mm 450 kN
10 mm V100 R15.5 71 mm 600 kN

The rule behind it: V = 6 × t up to 2.5 mm, 8 × t from 3 to 8 mm, 10 × t at 9-10 mm, 12 × t above 12 mm (V50 is the nearest die to 8 × 6 = 48). The force grows with the strength of the steel: S355 MC, at 550 N/mm² in the same catalogue, needs about 1.3 times the force in the table. Check the table of your own die maker before you draw.

Our test bracket uses the 6 mm row: V50 die, R8 inside radius, both flanges longer than 36 mm. The flat length also depends on the K-factor of that die. We used Inventor's default, 0.44: for the real flat, set your shop's value in the sheet-metal style.

Flat pattern DXF

oSM.DataIO.WriteDataToFile("FLAT PATTERN DXF?AcadVersion=R12", sDxfPath)

The flat view in the drawing

Add the base view with SheetMetalFoldedModel = False in the options. Three traps:

Drawing view requested as flat pattern but drawn as the folded Z bracket, 202 x 134 mm instead of 319.4 x 150 mm, with no error. Here the cause was a second, unconverted copy of the same STEP open in Inventor.
Asked for the flat view, got the folded part, and no error.
Two flat pattern views of the test bracket: with kTopViewOrientation the flat pattern is seen edge-on, 319.4 x 6 mm; with the default orientation it is 319.4 x 150 mm.
Same flat pattern, two orientations: one of them is edge-on.

Enum values from VBScript

From VBScript, or from Python with late binding, use the numeric values. Read them from the interop assembly (Autodesk.Inventor.Interop.dll), do not guess them. In Inventor 2025: planar surface 5890, cylinder 5891, kTopViewOrientation 10754, kFrontViewOrientation 10764.

Do and don't

Do

Don't

Questions people ask

What about rolled or curved plates? They are not bent plates. They need their own treatment and usually a person's decision.

References