This page describes the process and requirements for Exporting and then Importing Allegro PCB designs. In order for Allegro designs to be imported, they must first be exported in ASCII format. Allegro is the PCB design tool of later versions of the OrCAD design suite.
This page also describes a mechanism for importing Allegro designs to create Library content (Parts and footprints).
There are two mechanisms for exporting Allegro designs in ASCII format:
- Process 1, where both Allegro and Pulsonix reside on the same PC.
- Process 2, where Allegro resides on one PC and Pulsonix on another machine.
The Extracta Program
Cadence Allegro PCB designs can be imported into Pulsonix once the Cadence supplied extracta.exe program has been run, this produces an ASCII version of the Allegro design.
Important Notes:
- This is a licensed option in Pulsonix and you will require the Allegro Importer option to be activated for this import process.
- Parts and Footprint libraries cannot be directly imported but designs can be imported to create library content for Parts and footprints. Schematic symbol library content can be imported and added from the corresponding OrCAD or Allegro Schematic designs or libraries.
Supported versions of Allegro
Allegro Versions up to V17.x are supported. Later versions may be supported but please contact your local sales office for confirmation.
For Allegro Schematic Capture designs and libraries, see the OrCAD page.
Process 1 - Exporting Allegro Designs from the same PC as Pulsonix
Prerequisites for running the Allegro Importer
Allegro cannot export ASCII files of libraries, it can only save native PCB designs (.brd).
The Extracta.exe program is supplied with Allegro but is run outside of their PCB environment but still as part of their supplied program suite. In this process (1), Pulsonix calls this program in order to export an ASCII file that can then be read in. In this instance, both Allegro and Pulsonix must reside on the same machine. This is a one off process so after the conversion, it can be removed, unless you need to import more than one design.
Locating the Extracta.exe program
The path must be set to the location of the extracta.exe file supplied with OrCAD/Allegro.
To do this, from within Pulsonix go to the Options General option. click the Browse button on the Allegro Extract File Path section and browse to the extracta.exe program location. This is likely to be in the tools\pcb\bin sub folder of your Allegro or OrCAD installation.
Once you have defined the path to the extracta.exe you can now import the Allegro files from within Pulsonix, as explained below.
Importing Allegro PCB Designs into Pulsonix
In Pulsonix, use Open from the File menu and browse to the Allegro board file (.brd) location. Select the design and press Open to start the import process. You will be asked to provide a Part Technology files. choose the one required or select None.
Use Layer Mapping
If you have selected a Technology file, you can also select Use Layer Mapping which will allow you to map the Allegro layers to the Pulsonix layers specified in the Technology. When checked, the Layer Mapping dialog will be activated before the import starts. If this check box is not selected, then the Allegro layers and names will be used. These can be edited in the Layers dialog in the Technology once imported.
Process 2 - Exporting Allegro Designs from a different PC to Pulsonix
The Extracta.exe program is supplied with an Allegro installation but is run outside of their PCB environment but still as part of their supplied program suite. In this process (2), it can be run on another machine to that of Pulsonix and used to export an ASCII file that can then be read in.
This alternative mechanism enables files generated on another machine using the Allegro Extracta.exe program to be loaded into Pulsonix. In order to extract the data required there are a number of actions required:
-
Locate the AllegroToPulsonix.bat and the AllegroTranslate.txt control file supplied with your installed Pulsonix (usually C:\Program Files\Pulsonix 14.0\SysUtils\
-
Copy AllegroToPulsonix.bat and the AllegroTranslate.txt control file to the machine that has Allegro installed. Copy to an accessible folder (i.e. not the Programs folder containing Allegro). For example, create a folder called C:\Temp\
-
Copy the Allegro PCB design file (.brd) that you wish to convert, into the same folder as the batch file.
-
Launch a Windows command shell (type CMD in the Windows Start menu and press <Enter>).
-
In the command shell, navigate to the folder that contains the batch file (i.e. cd C:\Temp\ )
-
Run the AllegroToPulsonix.bat using the following command in the command window:
AllegroToPulsonix design\_name.brd <Enter>
-
Note, normal command shell rules apply, for example, if you have spacing in your filename, you will need to enclose these in quotes “design name.brd”
-
Running the batch file will create an ASCII file of your design with the .alg extension (i.e. design\_name.alg).
-
Copy the resultant .alg file back to where Pulsonix can read it in.
-
In Pulsonix, select the Open dialog on the File menu, there is a new file type. Allegro PCB ASCII File (\*.alg). Select your .alg design file for import.
-
The Pulsonix import filter will now run the Allegro import option.
External Resources
If you require an Allegro design in ASCII format, you can provide the AllegroToPulsonix.bat and the AllegroTranslate.txt control file to the person performing the extraction. The batch files does not require Pulsonix in order to be run. Once run, the resultant .alg file will be provided back to you for import.
Importing Allegro PCB Designs to Create Libraries in Pulsonix
If you wish to import your Allegro Parts and Footprints, as with importing Allegro PCB designs, you must have the path to the extracta program defined (see above under Prerequisites).
You cannot import Allegro Parts or Footprint libraries directly as there is no ASCII export mechanism available in Allegro. However, you can rebuild libraries from your Allegro PCB designs. You can do this iteratively for each design and build-up one complete library over time, or you can create individual libraries on a per-design basis. You may also wish to import many Allegro PCB designs in one go to create a new library.
Once the extracta program has been set up, create library content by dragging (using Windows Explorer) your Allegro PCB design or designs and dropping them onto the open Library Manager Parts tab or Library Manager PCB Footprints tab. Multiple designs can be dragged and dropped at the same time using multiple select (Ctrl and Shift key selections).
You can also use the Import button on either dialog to import the designs but drag and drop is much quicker. However, the two mechanisms are different, although the result is the same. The drag and drop method will use the Save Items To Library dialog where both Parts and Footprints can be imported from selections and libraries chosen. The Import method is more of a batch process but does allow duplicates to be overwritten or ignored.
Related Topics
Options General | Open | Layer Mapping | Libraries Parts | Libraries PCB Footprints | Save Items To Library | OrCAD Import