# 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. Tests check flat lengths against hand-computed bend allowances. Where the edge flanges of one feature meet at a corner of the base, their panels are closed toward each other at any bend angle: each end is cut square to the sheet, on a line in the flat chosen so that the edges nearest each other (on the inner faces) run parallel, the rule's **gap** apart, either side of the plane halfway between the flanges. Flanges at 72° get slanted ends in the flat; corners that aren't square close the same way, and at 90° it is the corner the rule always gave. A corner that can't be closed (a gap under 0.01 mm, flanges bending opposite ways, ends that would overlap in the flat pattern) stays open, and the flange feature reports a warning saying where. A flange added by a later feature leaves the corner as it was: the earlier flange keeps its length and the new one ends at its bend. The flanges of one edge flange feature can each have an angle and a height of their own. An entry of `edges` is a point `[x, y, z]`, which takes the feature's `height` and `angle`, or an object `{"point": [x, y, z], "angle": "105 deg", "height": "30 mm"}` whose `angle` and `height` (either one, or both) replace them for that edge. They are expressions like the feature's own, so parameters work, and each is a feature input of its own (`Edge angle`, `Edge height`) after `Height` and `Angle`. The corners between such flanges close like those between equal ones: the ends run toward each other the rule's gap apart, either side of the plane halfway between the two flanges, and a taller flange's end keeps that line up to its own tip. This is how to close a corner between flanges at different angles, because flanges of separate features don't close toward each other. In the Flange dialog, picking more than one edge shows a row per edge with an angle and a height box; an empty box takes the value above. ```json {"command":"sheet.flange","params":{"edges":[[60,0,2],{"point":[120,45,2],"angle":"90 deg"}, {"point":[60,90,2],"angle":"105 deg","height":"30 mm"},{"point":[0,45,2],"angle":"120 deg","height":"25 mm"}], "height":38.6,"angle":"75 deg"}} ``` 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 material inside both the current tool footprint and its depth interval, including interior holes, detached islands and earlier pockets. A shallow intersection records the removed layers above and below the retained material as top and bottom pockets. The sheet rule keeps the original stock gauge; the remaining solid can be thinner. A completely empty intersection removes the sheet and its metadata together. DXF records pocket depth in its layer names; importing that DXF as ordinary sketch geometry does not reconstruct the machining depths automatically. Each positive retained or removed depth layer must meet the kernel's 0.000001 mm extrusion resolution; smaller layers report an error rather than being rounded away. To Object can retain a tool that trims to a straight prism, using its actual trimmed footprint. A curved tool with varying depth is refused before changing sheet geometry. 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. A sketch can be drawn on a flat face of the sheet: the base or a flange, on either side. Pick the face (or give `sketch.create` the point `plane: {face: [x, y, z]}`) and the sketch attaches to that panel instead of to a certified source face. It keeps the face's name, `sheet:::` (the panel is `base` or the flange's feature tag), and finds the face again whenever the sheet is rebuilt: after a parameter change such as the thickness or a flange angle, through Unfold / Refold, after the file is reopened and when the body is renamed. Sketch coordinates are the flat pattern's, so a point drawn on a flange lies where the flat pattern and its DXF have it, and on the bottom face y runs the other way, as seen from below. When the face is gone (its flange is suppressed or deleted) the sketch reports a lost attachment instead of moving to another face; **Redefine Sketch Plane** attaches it to another face. `fixed: true` still freezes the picked plane in space.