This page describes the process and requirements for importing Allegro PCB designs. It also describes a mechanism for importing designs to create Library content (Parts and footprints).
Cadence Allegro PCB designs can be imported into Pulsonix using the Cadence supplied extracta.exe program which produces an ASCII version of the Allegro design. You must have Allegro installed on your system for this to work. Allegro is the PCB design tool of later versions of the OrCAD design suite.
Important Notes:
- This is a licensed option in Pulsonix and you will require the Allegro Importer option to be activated for this process.
- You must have the Allegro design application (program) on the machine you are attempting to import the files from.
- 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 V16.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.
Importing Allegro Designs (and Designs as Libraries)
Prerequisites for running the Allegro Importer
Allegro cannot export ASCII files of libraries, it can only save native PCB designs (.brd).
In order to import Allegro files (designs or libraries), the Allegro extracta program must be on the same machine that you have Pulsonix installed on. This is a one off process so after the conversion, it can be removed.
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 open 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.
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