# Sheet metal

The SHEET METAL tab builds parts from a sheet of constant thickness under a **sheet metal rule**
(thickness, bend radius, K-factor), set in **Sheet Metal Rules** (`sheet.manage_rules`).

- **Flange** (`sheet.flange`): a base flange from a sketch profile, a contour flange from an open
  sketch, or an edge flange from a part edge.
- **Hem** (`sheet.hem`) and **Fold** (`sheet.fold`) along a sketch line.
- **Unfold / Refold** (`sheet.unfold`, `sheet.refold`) for working on the flat part.
- **Convert** (`sheet.convert`) turns a solid of constant thickness into sheet metal.
- **Create Flat Pattern** (`sheet.flat_pattern`) shows the flat part with its bend lines and a
  bend table, and exports it as DXF or a bend-table CSV through the save picker.

Bends follow the rule's K-factor, so flat lengths match what a press brake will make. The
oracle checks these against parts built in Fusion.

For a shop drawing or spreadsheet, `sheet.export_bend_table` returns CSV by default; choose
`format: "json"` for structured data. It includes the sheet rule, thickness, bend angles,
radii, allowances and flat centre-line coordinates. Lengths use millimetres and angles use
degrees. Supply `path` to save it, or omit `path` to receive the content through the command
response. `body` defaults to the last sheet body. Exporting does not add a timeline entry or
consume an undo step.

```json
{"command":"sheet.export_bend_table","params":{"format":"csv","path":"bracket-bends.csv"}}
{"command":"sheet.export_dxf","params":{"path":"bracket-flat.dxf"}}
```

DXF cutout geometry preserves lines, circles and circular arcs; other curves are sampled
adaptively. The `OUTLINE`, `BEND_UP` and `BEND_DOWN` layers separate cuts from bend centres.

Base-flange profiles keep their interior holes. Through cuts that cross a sheet edge become
notches in the flat outline; overlapping and repeated cuts remove their combined area once.
The flat preview, DXF and unfolded solid use the same material boundaries. Lines and circular
arcs remain exact; other profile curves use a 0.001 mm chord tolerance.

Cuts can leave separate material pieces, including the centre of a ring cut. These pieces
remain one logical sheet group through Unfold / Refold and export as separate flat outlines.
Large profiles that exceed the geometry processing budget report an error instead of
exporting a partial outline.

Parallel, untapered extrude cuts also preserve shallow pockets through Unfold / Refold.
The pocket floor and side walls remain solid geometry; overlapping cuts from opposite sides
become a through hole wherever they remove the whole thickness. Flat-pattern JSON lists
`pockets` with their side, depth and bottom/top thickness coordinates in millimetres.
DXF pocket boundaries use `POCKET_BOTTOM_Z…_TO_…_MM`, `POCKET_TOP_Z…_TO_…_MM`, or
`POCKET_INTERNAL_Z…_TO_…_MM` layers. These are machining operations, so do not treat every
pocket layer as a through-cut contour when importing the drawing into a CAM tool.

Extrude Intersect on a straight base or an unfolded sheet retains the exact planar material,
including interior holes and detached islands. A completely empty intersection removes the
sheet and its metadata together. Pocket profiles can move with planar panels when forming,
but a pocket crossing a bend zone cannot yet be refolded. Machining folded bend material,
tapered sheet cuts and other unsupported 3D sheet Cut/Intersect operations report an error before changing
the design; they cannot silently restore removed material during a later sheet rebuild.