To support the need to load and work with Cadence® Allegro™ Design files, Altium NEXUS’s Import Wizard includes the capability to import Allegro PCB designs in binary (
*.brd - check the import prerequisites), ASCII (
*.alg) forms (which are translated to Altium NEXUS PCB files (
*.PcbDoc)), and Allegro footprint files (*.dra) (which are translated into Altium NEXUS PCB library files (*.PcbLib).
The Allegro PCB files (up to version 17.2) are translated to Altium NEXUS PCB files by the Wizard’s Allegro importer, which is included as an Altium NEXUS platform extension.
If the Allegro Design Files option is not available in the Import Wizard, that indicates that the Importer extension was not added during the initial installation of Altium NEXUS. The extension can be enabled in the Configure Platform page in the Extension & Updates view. Select Extensions and Updates from the Configuration menu ( show image ), click the Configure button under the view’s Installed tab and then check the Allegro option in the Importers\Exporters section.
The Altium NEXUS Import Wizard can directly import Allegro ASCII format PCB files (
*.alg) and Allegro footprint files (*.dra). To import a binary Allegro PCB file (
*.brd), the file must be translated from binary to ASCII. The binary-to-ASCII translation is performed by the Cadence utility called Extracta, a configurable command-line utility that is capable of extracting and translating data from the binary PCB file, with the extraction process controlled by a Command file that details the data required to be extracted. Learn more about Extracta.
Extracta will only extract data from Allegro binary (
*.brd) PCB files whose version is the same as, or lower, than the version of Extracta being used. To check the version of Extracta, open a Windows Command prompt and enter
If Altium NEXUS is installed on the same PC as Cadence Allegro, the extraction process can be handled automatically by the Altium NEXUS Import Wizard. The process of running the Wizard is outlined below. Note that the Wizard also performs file version checking, Allegro files up to 17.2 are currently supported by the Wizard.
If Extracta.exe is not installed on the same PC as Altium NEXUS, you can manually run the extraction process on the PC where the Extracta utility is installed. Altium NEXUS runs the extraction process using the following batch file and extraction command file:
To manually extract the ASCII board data:
<Altium_Designer_Installation_Folder>\Systemfolder, to a known location on the PC that has Allegro installed.
*.brd) file that you want to convert, into the same folder.
your_file.brd is the name of the binary file you want to convert. Surround the filename with double quotes if the filename contains spaces, for example
Allegro2Altium "your file.brd".
your_file.brd.alg) in the folder. Copy this ASCII board file back to the PC where it can be imported into Altium NEXUS using the Import Wizard.
Main page: Import Wizard
The Allegro PCB design file importer is available through Altium NEXUS's Import Wizard (File » Import Wizard), where the option is selected in the wizard's Select Type of Files to Import page – choose the Allegro Design Files option. When adding files to the import file list, use the file browser's filter drop-down menu to choose between binary (
*.brd) or ASCII (
*.alg) Allegro files.
If you attempt to import a binary Allegro Design File (
*.brd) using the Import Wizard and you do not have Allegro installed locally, the import process is suspended and a warning dialog is displayed. In this case, import an ASCII version of the design file that has been created through the Allegro ASCII file extraction process (as outlined above).
To complete the file import and translation process, follow through the remaining pages of the Import Wizard to customize and finish the conversion of the Allegro Design Files into Altium NEXUS design files. See the Allegro Design Files entry on the Import Wizard page for more information on the Wizard's import steps.