Exporting creates deliverables; it does not publish a Workspaces revision, submit an order, or certify manufacturing readiness.
Before You Export
Open the intended project, save the schematic/board, and select the fitted variant. Refill zones, run the relevant ERC/DRC checks, and resolve required findings.
Keep .kicad_pro, .trace_sch/.trace_pcb, and paired .xo files as the native project. Use a separate output destination and verify build and host support for the chosen format.
Gerber Files
- Open the native PCB Plot dialog (under File → Plot in the Full interface).
- Select Gerber and the required copper, mask, silkscreen, paste, and outline layers.
- Check units, origin, format, output folder, and any variant selector.
- Plot the files and generate the required drill files using the available drill controls.
- Open them in a Gerber/drill viewer and inspect outline/cutouts, copper, masks, holes, and layer alignment.
Use the manufacturer's requested options; do not assume every preset matches its current process.
Where Files Are Saved
Check the output path in each export dialog or command and confirm that new files exist there. Prefer separate revision/variant folders so stale artifacts cannot be mistaken for the current export. A successful export message is not a readback check.
Bill of Materials
Use the supported schematic BOM export, typically CSV with selected fields. Review references, quantities, values, footprints, exact manufacturer part numbers, and fitted status. Do not assume Excel or interactive HTML output is available in every build.
The BOM and board position files must describe the same assembly. Check excluded/not-fitted references and deliberate no-BOM items in the actual output.
Pick and Place
Export component positions using the native fabrication output controls where available. Check X/Y origin, units, rotation convention, top/bottom side, references, and included components with the assembler.
Coordinate conventions are not universal; a correctly written file can still need assembler-specific mapping or rotation corrections.
3D Models
Use the available STEP/3D exporter for mechanical comparison and the offered visualization formats where supported. Inspect outline, thickness, fitted components, missing models, offsets, and orientation in the receiving application.
A rendered model does not certify tolerance, thermal fit, tool access, or assembly clearance.
PDF Documentation
Use schematic or PCB plotting/printing controls for the required sheets and layers. Verify page size, scale, labels, revision, variant, and readable line/text output. A drawing does not replace fabrication or assembly data.
Manufacturer Presets
If a preset is available, check its layer list, units, drill handling, origin, and naming against the manufacturer's current instructions. Export presets and manufacturer DRC presets are different settings.
One-Click Manufacturing
A compatible native Send to Manufacturer flow can submit files to supported partners after review. It is separate from export; see Manufacturing for measured board facts, quoting, assembly, and confirmation.
Trace Plugin's fabrication ZIP contains Gerbers/drills and excludes position/assembly files. Prepare and review assembly files separately in the supported host workflow; a companion export is not an implemented native one-click order flow.
Design Rule Export
Preserve the active custom-rule file and relevant board/net-class/stackup documentation when sharing requirements. A rule file is not a complete manufacturing specification or proof that exported geometry complies.
KiCad Project Export
In a compatible native project manager, use Export to KiCad… and choose a separate destination. Cancel an overwrite warning if the destination contains work you need to retain.
Open the exported KiCad project and verify the schematic hierarchy, board, library paths, models, rules, and variants. Keep the native original; export is not a guarantee of lossless bidirectional round-trip behavior.
Other Manufacturing Formats
Native exporters can provide IPC-2581 and ODB++ where supported. Confirm the required version/options and that the receiving manufacturer accepts them. Inspect the actual package, layers, outline, references, and assembly contents rather than assuming equivalence to another export format.
Mechanical Exchange
Use supported DXF for 2D geometry, STEP for 3D exchange, and native IDF export where available. Check units, origin, rotation, cutouts, board thickness, and component/model inclusion.
These paths do not establish IDX import or automatic bidirectional mechanical synchronization. Verify what the installed controls and receiving tool actually support.
Command-Line Exports
Use the native trace-cli bundled with the Trace app. Install Trace and sign in to the desktop first, then consult the installed command's help and CLI reference. Check the format and variant options for each export; do not copy one subcommand's flags into another.
If Export Fails or Looks Wrong
Read the specific output, dependency, variant, or file-access error. Check the intended project and destination, not just an older file with the same name. Correct the missing input or setting and export again into a separate folder.
Inspect the actual artifacts and retain the source design. Do not rename .trace_* to KiCad extensions, delete .xo, or discard .kicad_pro to work around an export failure.