Overview
Native Trace provides import paths for supported schematic and PCB formats. Import is a migration step, not a promise of lossless round-trip exchange or live synchronization with the source tool.
Work on a copy. Preserve source projects, linked libraries, models, and variant definitions before starting. The available importer and file types depend on the build and host.
Import and Save a Copy
- Identify whether you are importing a complete project, schematic, board, or library.
- Open the corresponding native project/editor import action. In the Full interface, editor import actions are under File → Import where provided.
- Select the supported source file; for a project import, keep its referenced sheets, board, and libraries accessible.
- Review reported missing dependencies, unsupported items, or conversion warnings.
- Save the converted design in a separate destination.
- Reopen that saved copy and check connectivity, libraries, footprints, rules, layers, and variants before editing further.
Native Trace projects retain .kicad_pro project settings, .trace_sch/.trace_pcb designs, and paired .xo drawings. These are not disposable intermediates. Keep them together; use Export to KiCad… where supported when you need KiCad files, not renaming or deleting native files.
gEDA / Lepton EDA
Use the available schematic importer for supported gEDA/Lepton .sch files. A .sch extension alone does not identify every legacy schematic format.
What Gets Imported
Review imported symbols, attributes, wires, labels, buses, and graphics. Check electrical connections independently of the preserved drawing.
Symbol Resolution
Resolve any missing or placeholder symbols to the intended library entry. Verify pin numbering, names, and electrical types; a fallback rectangle does not establish pinout correctness.
RC/Config File Parsing
Keep source library/configuration files available where the importer uses them. Inspect any unresolved custom symbols; do not assume every source library path transfers to the new installation.
Cadence Allegro
The native PCB importer supports Allegro board data, including supported v18+ files. Confirm the selected file is accepted by your installed build.
What Gets Imported
Review footprints, padstacks, tracks, vias, copper areas, text, outline, layers, and translated rules. Complex pad/zone and constraint semantics can differ between tools; refill and inspect rather than assuming all geometry and intent survived.
v18+ Binary Format
Support for an Allegro board version does not imply OrCAD Capture schematic import. This path is PCB import, not complete Cadence-project conversion.
Mentor PADS
Use supported PADS ASCII exports, not an arbitrary PADS binary project.
What Gets Imported
Native schematic and PCB importers have separate supported inputs. Review symbol/footprint mapping, connections, hierarchy where applicable, and board geometry.
Supported Formats
Export the appropriate ASCII design from PADS, then choose the PADS importer in the corresponding native editor. Check the file filter and warnings for your build.
Altium Designer
Use the supported native project or editor import path for Altium project, schematic, board, and library files. This is different from using Trace Plugin to assist an open Altium project in Altium itself.
What Gets Imported
Review sheets, symbols, wires, labels, board geometry, layer mapping, and library associations. Project variant definitions can be read from .PrjPcb; inspect the resulting variants and component assignments.
Accepted File Extensions
The supported path recognizes Altium files such as .PrjPcb, .SchDoc, and .PcbDoc, with the appropriate importer. Use its file filter rather than renaming the extension to imitate another format.
General Import Tips
Compare the saved import with the source:
- Component references, units, pin-to-net mapping, labels, and sheet interfaces.
- Exact footprints, pad numbers, slots/custom shapes, orientation, and 3D links.
- Outline, cutouts, layer stack, tracks, vias, zone fills, and keepouts.
- Net classes/custom rules and fitted-variant/BOM behavior.
Run ERC and DRC for their configured checks. A clean result does not prove lossless conversion, equivalent behavior, or manufacturer acceptance.
Mechanical Exchange
Use DXF for supported 2D reference geometry and STEP for supported model/export workflows. Check units, origin, rotation, side, and actual geometry in the receiving CAD tool.
Native IDF export is available where exposed by the installed build. Do not infer IDX import, bidirectional exchange, or every mechanical format from IDF/STEP support. See Exporting Designs.
If Import Is Incomplete
Retain the original and converted copy. Resolve missing libraries/models and inspect unsupported items before continuing. A failed conversion is not a safe reason to overwrite the source or delete .kicad_pro/.xo.
For unsupported formats, export a supported interchange format from the source tool or contact support with the file type, build, and bounded error—not private design files by default.
Requesting New Importers
Ask in the community or email hello@buildwithtrace.com with the tool and format you need.