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 17.4) 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.
Import Prerequisites
The Altium Designer Import Wizard can directly import Allegro ASCII format PCB files (*.alg). To import a binary Allegro PCB (*.brd) or footprint (*.dra) file, 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 PCB (*.brd) and footprint (*.dra) 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 17.4 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:
Allegro2Altium.batAllegroExportViews.txt
To manually extract the ASCII board data:
- 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.
- Copy the Allegro binary (
*.brd or *.dra) file that you want to convert, into the same folder.
-
Launch a Windows Command Prompt and use the cd command to get into the folder that contains the copied files. Example:
cd C:\Documents\Files\Test
-
Once in the right directory, run the Altium batch file using the Allegro2Altium command. For example:
Allegro2Altium your_file.brd
or
Allegro2Altium your_file.dra
where your_file.brd or your_file.dra 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".
- The process will create an ASCII file (
your_file.brd.alg or your_file.dra.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.
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
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).
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.
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.
Import Wizard - Allegro Design Files
Allegro Design Files
The
Import Wizard handles both Allegro PCB Design files (
*.brd) and Allegro ASCII Extract files (
*.alg). To translate Allegro PCB Design files (
*.brd) you must have a licensed installation of the appropriate version of the Allegro PCB Editor (up to version 17.4 is supported by the Import Wizard). Learn more about
Allegro Import.
Selecting the Files to Import
Click Add to choose which Allegro design files to import. You can delete a selected file by clicking Remove.
Selecting the Constraint Files to Import
Click Add to choose which Allegro *.DCFX constraint files to import. You can delete a selected file by clicking Remove.
Note that the constraint file(s) include the board design rules, so must be included to correctly import the board(s). Constraint files can be exported from the Allegro Constraint Manager.
Analyzing Files
Click Add to choose which Allegro footprint files (*.dra) to import. You can delete a selected file by clicking Remove.
Setting the Reporting Options
Use the Reporting Options page to set up general log reporting options. A Log Report in ASCII file format (*.LOG) is generated for each translated Allegro PCB file. This log is saved in the \Imported sub folder of your original Allegro files. Open the Log Report after translation in a text editor to examine the details.
Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.
Setting PCB Specific Options
This page of the Wizard is used to specify options specific to the PCB import process.
Select the desired Polygon Connect Options: either Use direct connect for default polygon connect style or Use relief connect for default polygon connect style.
Select the Plane Connect Options: either Use direct connect for default plane connect style or Use relief connect for default plane connect style.
Enable the Import Auto-Generated Copper Pour Cutouts option in the Import Auto-Generated Objects Options region to import the voids that are auto-generated in the Allegro PCB Editor as cutouts when the file is translated.
Enable the Optimize Clearance Rules option to use optimization for the clearance rules.
Editing the Layer Mapping
This page of the Wizard is used to review and edit the layer mapping for each Allegro PCB. Default mapping is provided by the Wizard to build the layer mapping for each PCB. Layer mapping can be customized for each of your designs to be imported. You may wish to import multiple Allegro PCB designs and map the same Allegro layer to the same Altium Designer layer. You can set your layer mapping once and use this layer mapping for all of your files to be imported. The advantage of importing in this manner is that batch layer management can save time when importing multiple designs. The disadvantage to using this is that Default Layer Mapping is not always intelligent with differing structures in designs, and therefore, some manual changes may be required.
The Allegro Layer Name, Allegro Layer Type, Altium Layer Type, and Altium Layer Name are listed in the grid region. Click on the 
icon on the right-hand side of each region to filter the displayed list of that region.
If desired, you can edit the layer mapping for any or all Allegro Import PCB designs or library files on this page of the Wizard. To group by a column, drag the column header into the area at the top of the table specified.
Right-clicking in the grid region provides you with a sub-menu where you can:
- Load Layer Mapping – select to open the Load Configuration dialog to load the desired mapping files.
- Save Layer Mapping – select to open the Choose File to Save Layer Mapping dialog and choose the path in which to save the layer mapping.
Specifying the Output Directory
Use this page of the Wizard to review the output project structure and specify the output directory in which to import the files. Use the Browse Folder icon to search for and choose the Project Output Directory.
Click Menu to access options to edit the project structure:
-
Create Project – click to open the Create Project dialog to add a project.
Use the Create Project dialog to add a new project.
- Rename Project – click to rename the selected project. This option is available only when a
*.PrjPcb file is selected.
- Remove Selected Projects – click to remove the selected project from the PCB Projects structure.
- Reset Structure to Default – click to reset the PCB Projects structure to the defaults.
- Add Designs to Project – click to add a design(s) to the project. This option is available only when a
*.PrjPcb file is selected.
-
Remove Selected Designs - click to remove the selected design files.
Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.
Closing the Wizard
The Allegro Import Wizard has completed. Click Finish to close the Wizard.
Imported Allegro files:
Allegro files translate as follows:
- Allegro Binary PCB Design files (
*.brd) translate to Altium Designer PCB files (*.PcbDoc).
- Allegro ASCII Extract files (
*.alg) translate to Altium Designer PCB files (*.PcbDoc).
- Allegro footprint files (
*.dra) translate to Altium Designer PCB library files (*.PcbLib).
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®.
Notes
- Check out the detailed Knowledgebase article on importing Allegro files into Altium Designer.
- In Altium Designer, 3D STEP models are stored inside a 3D Body Object, which is placed in the PCB footprint.
- The Allegro Importer supports importing custom pad stacks defined in an Allegro board design. Import of such a design will create custom pad shapes in Altium Designer. In addition, where thermal tie legs are defined as part of the custom pad stack in Allegro, these will be imported as custom thermal relief connections.
Документация Altium Designer
...
Advanced Design Environment Topics in Altium Designer
Взаимодействие с другими системами проектирования