Altium Designer Documentation

Importing a Design from Allegro into Altium Designer

Created: September 1, 2021 | Updated: September 1, 2021

To support the need to load and work with Cadence® Allegro Design files, Altium Designer’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 Designer PCB files (*.PcbDoc)), and Allegro footprint files (*.dra) (which are translated into Altium Designer PCB library files (*.PcbLib).

The Allegro PCB files (up to version 17.2) are translated to Altium Designer PCB files by the Wizard’s Allegro importer, which is included as an Altium Designer platform extension.

Enabling the Importer

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 Designer. 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 Allegro Importer must be enabled in the Altium Designer's Platform Configuration.The Allegro Importer must be enabled in the Altium Designer's Platform Configuration.

Import Prerequisites

The Altium Designer 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.

Supported Binary File Versions

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 Extracta -version.

Note: If this command fails it may be that Extracta.exe does not have the correct Windows Path defined, refer to this Altium Knowledge Base article for detailed information on configuring the Path System Environment Variable for Extracta.

Importing when Allegro is on the same PC as Altium Designer

If Altium Designer is installed on the same PC as Cadence Allegro, the extraction process can be handled automatically by the Altium Designer 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.

Importing when Allegro is not on the same PC as Altium Designer

If Extracta.exe is not installed on the same PC as Altium Designer, you can manually run the extraction process on the PC where the Extracta utility is installed. Altium Designer runs the extraction process using the following batch file and extraction command file:

  1. Allegro2Altium.bat
  2. AllegroExportViews.txt

To manually extract the ASCII board data:

  1. Copy the two files detailed above from the <Altium_Designer_Installation_Folder>\System folder, to a known location on the PC that has Allegro installed.
  2. Copy the Allegro binary (*.brd) file that you want to convert, into the same folder.
  3. Launch a Windows Command Prompt, and run the Altium batch file using the command:

Allegro2Altium your_file.brd  
where 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".

  1. The process will create an ASCII file (your_file.brd.alg) in the folder. Copy this ASCII board file back to the PC where it can be imported into Altium Designer using the Import Wizard.

The ASCII Allegro design conversion process is controlled by the special Allegro2Altium batch file.The ASCII Allegro design conversion process is controlled by the special Allegro2Altium batch file.

In a standard Allegro installation, the proprietary extracta.exe translation program is added as a system environment path and is therefore accessible from all locations. The Allegro2Altium batch file and the pending conversion process will fail if this program cannot be accessed. Refer to the Altium Knowledge Base article for detailed information on configuring the Path System Environment Variable for Extracta if the program cannot be accessed.

Accessing and Running the Importer

Main page: Import Wizard

The Allegro PCB design file importer is available through Altium Designer'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.

Select either binary or ASCII Allegro design files for import. Allegro must be installed on the local machine to import binary Allegro files (*.brd).Select either binary or ASCII Allegro design files for import. Allegro must be installed on the local machine to import binary Allegro files (*.brd).

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 Designer design files. See the Allegro Design Files entry on the Import Wizard page for more information on the Wizard's import steps.

Note that the Import Wizard offers a default Layer Mapping setup, which can be modified and saved as a *.ini file. The mapping is used by the Import Wizard to build the layer mapping for each PCB in the imported design, so during the import of several PCB files, a saved mapping configuration file can be loaded and applied to individual (or all) PCB files.

An imported and converted Allegro PCB design shown in 3D mode Altium Designer's PCB editor. Allegro design for Hercules Development Kit courtesy of Texas Instruments®.An imported and converted Allegro PCB design shown in 3D mode Altium Designer's PCB editor. Allegro design for Hercules Development Kit courtesy of Texas Instruments®.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: