Import Allegro PCB files into Altium Designer

ArmSoM provides Allegro hardware designs. Download the matching product and PCB revision from Hardware resources. Work on a copy; retain the original as your reference.

Choose a workflow

Files / tools available	Workflow
.brd + licensed Allegro/Extracta	Convert locally or on another Allegro workstation
.alg + Altium	Import the ASCII file directly
.brd + Altium only	Obtain an .alg conversion first

PCB import does not recreate the schematic from a PDF.

Convert when necessary

On the licensed Allegro workstation, put the board and Altium's System/Allegro2Altium.bat in a working folder. Before AD 26.1, also include matching AllegroExportViews.txt and AllegroPackageExportViews.txt. In Command Prompt run:

Allegro2Altium.bat "board.brd"

Copy the resulting board.brd.alg to the Altium workstation. Check extract.log on failure. Extracta must support the source file version; the official importer documentation currently lists support through Allegro 17.4. See conversion prerequisites and troubleshooting.

Import and review

1. Enable Altium's Allegro importer.
2. Select File → Import Wizard → Allegro Design Files.
3. Add .alg, or .brd when licensed Allegro is available locally.
4. Include .DCFX constraints if supplied; review layer mapping and output location.
5. Finish and inspect the generated .PcbDoc and translation log.

Compare board outline, holes, layers, pad numbers and critical connections against the original. Before manufacturing, review constraints and run design-rule checks; opening successfully is not manufacturing validation.

See Altium's import guide. This workflow has not been conversion-tested on every ArmSoM design; compatibility depends on file and tool versions.