SolidCraft is mostly known for sketching and solid modelling, but it also includes a sheet metal workspace. This page covers what is there, how to make a simple bracket, how to get a flat pattern out, and where the limits are. Everything below comes from SolidCraft's own documentation.
What sheet metal features does SolidCraft have?
The SHEET METAL tab builds parts from a sheet of constant thickness. According to the docs, its tools are:
| Tool | What it does |
|---|---|
| Sheet Metal Rules | Sets thickness, bend radius and K-factor, plus relief and gap values |
| Flange | A base flange from a sketch profile, a contour flange from an open sketch, or an edge flange from a part edge |
| Hem | A hem along a sketch line |
| Fold | A bend along a sketch line |
| Unfold / Refold | Flatten the part to work on it, then fold it back |
| Convert to Sheet Metal | Turns a plate, solid or shelled body into sheet metal |
| Perforate | Makes a field of holes |
| Create Flat Pattern | Shows the flat part with bend lines and a bend table, and exports it |
The feature list in docs/features.md counts twelve sheet metal commands, including the DXF and bend-table exports.
How do sheet metal rules work?
Everything starts with a rule: thickness, bend radius and K-factor, set in Sheet Metal Rules. Bends follow the K-factor, so flat lengths should match what a press brake makes. For converted solids the docs give the bend deduction as 2·(R + T)·tan(θ/2) − θ·(R + K·T).
The rule also holds:
- Gap between flanges that meet at a corner.
- Bend relief width and depth, cut beside a bend that ends at an inside corner.
- Corner relief shape:
notch(default),tear,roundorrectangular, with a size.
A single edge-flange feature can override the corner relief for its own corners, and each edge in one feature can have its own angle and height.
How do I make a simple bracket?
This walkthrough follows the documented workflow. Menu names may differ slightly between versions, so use the tool names above as a guide.
- Set the rule. Open Sheet Metal Rules and make a rule such as 2 mm thickness, 1 mm bend radius and a K-factor of 0.5, and set it active.
- Sketch the base. Sketch a rectangle on a plane, for example the bracket's flat plate.
- Add a base flange. Use Flange with the sketch profile. This makes the flat sheet at the rule's thickness.
- Bend up a leg. Use Flange again, as an edge flange, pick one edge of the plate, then set the height and angle (for example 90 degrees and 20 mm).
- Add holes. Sketch on a flat face of the sheet, which the docs say is supported on the base or a flange, then cut. Through holes become round cut-outs in the flat pattern. Hole and Box or Cylinder cuts work square to a panel.
- Check the flat pattern. Run Create Flat Pattern to see the flat part with bend lines and a bend table.
- Change a parameter. Edit the thickness or flange angle and the part rebuilds, as in the rest of SolidCraft.
For the general workflow of sketching and extruding first, see the SolidCraft tutorial.
How do I export the flat pattern?
Create Flat Pattern shows the flat part and exports it through the save picker. From a script, CLI or the MCP server, the documented commands are:
{"command":"sheet.export_bend_table","params":{"format":"csv","path":"bracket-bends.csv"}}
{"command":"sheet.export_dxf","params":{"path":"bracket-flat.dxf"}}
The DXF is an AutoCAD 2000 drawing in millimetres, made for laser-cutting nesting or CAM software. Each kind of line has its own layer:
| Layer | Holds |
|---|---|
OUTLINE |
Outer contour of each piece |
CUT |
Holes, slots and loose pieces |
BEND_UP, BEND_DOWN |
Bend centre lines, dashed, by direction |
ETCH |
Letters to mark, not cut |
BEND_NOTES |
Optional notes such as bend number, direction, angle and radius |
POCKET_... |
Shallow pockets, a layer for each depth |
The bend table lists the rule, thickness, bend angles, radii, allowances and flat centre-line coordinates. Round holes are written as true circles, not chords. Pocket layers are machining operations, so do not treat them as through-cuts when you import into CAM software.
Can I convert an existing part to sheet metal?
Yes. Convert takes a plate of constant thickness, or a solid or shelled body when you pick the fixed face and the sharp edges that become bends. A STEP part imported with bends modelled as cylinders can also be converted; the docs say the bend then uses the rule's radius and K-factor, not the modelled radius. See SolidCraft STEP files for importing.
What are the limits?
- Not converted yet: curved faces other than bends (rolled sheet), and bends that close a ring.
- Holes and engravings that reach into a bend, or a pocket deeper than half the thickness, need cutting after converting.
- Slanted holes, holes drilled into the sheet edge, countersinks and drill points are refused on sheet metal.
- Corners that cannot be closed stay open and the feature reports a warning.
- Unsupported cuts report an error rather than changing the design.
- No drawings or CAM. The roadmap defers both, so take the DXF to nesting or CAM software.
SolidCraft is a young project, so compare the flat pattern with your fabricator's own bend rules before cutting material. If you want the app first, see the SolidCraft download page.