Contact our corporate or local offices directly.
[Why] Import Allegro files to Altium [What] To import the files, Altium Designer ultimately needs the ASCII versions. Binary versions need to go through a conversion process that requires a local installation of extracta.exe that is installed as part of Allegro to convert the *.brd file to the Allegro ASCII *.alg file that Altium needs for the import. [How] use extracta.exe to convert binary *.brd to ASCII *.alg. File » Import Wizard and select 'Allegro Design Files' to convert to Altium *.pcbdocStarting in Version: 18.0
OrCAD is a proprietary software tool suite used primarily for Electronic Design Automation (EDA) developed by Cadence Design Systems, Inc. The name OrCAD is a portmanteau, reflection of the software's origin and the company's focus: Oregon (Oregon, United States) + CAD (Computer-Aided Design). OrCAD is part of the Allegro platform.
In addition to this knowledge article, please review this documentation:
Altium Designer supports the import of Allegro's native binary (*.brd) and ASCII (*.alg) files from Allegro (up to version 17.2). To import the files, Altium Designer ultimately needs the ASCII versions. Binary versions need to go through a conversion process that requires a local installation of extracta.exe that is installed as part of Allegro to convert the *.brd file to the Allegro ASCII *.alg file that Altium needs for the import. As this utility is part of the Allegro tools, Altium is unable to redistribute this file, or the DLLs required to run it. Therefore, the conversion requires a machine with Allegro installed. If that is not available, you can inquire with one of our service bureau members. Here's a link:
Try using Allegro as a search word to reduce the list size, then double check that Services provided includes Allegro.
If both programs are installed and licensed on the same machine, then Altium Designer can automatically use Allegro's utilities to convert the *.brd file into *.alg, and then into an Altium Designer file. You will still need to configure the Path System Environment Variable as described below (just after the next screen shot.)
Note that extracta.exe is tied to a valid Allegro license so when it expires you will no longer be able to import the *.brd file. Altium can import the Allegro ASCII *.alg file without having an installation of Allegro on your machine.
Allegro is installed in the C drive as shown in below:
After Installation, configure the Path System Environment Variable by following steps below (Alternately, you could use the Windows Control Panel ► System and Security ► System dialog to get to the same Settings screen.):
In Windows File Explorer right-click on This PC and select Properties
In the settings window that opens, scroll down in the right panel until you can click on Advanced system settings.
(You may see this dialog instead)
In the System Properties dialog that opens, select ‘Environment Variables…’ in the lower right corner
Select the ‘Path’ variable in the System Variables section and then click ‘Edit’ (Warning, do not use the delete button)
Select ‘New’ in the Edit environment variable dialog and add only the paths indicated in the red box shown in this image (do not make any other changes to the path):
If you accidentally delete your path (it has happened), you can recover the information from a Command prompt: CMD> echo %PATH% then copying the displayed entries back into the Path variable. - This option will not be available after you re-boot.
Back at the System Variables section click ‘New’
Add 'CDSROOT' System Variable with a Value of C:\Cadence\SPB_17.2 (or whatever version you have)
in the dialog like this:
Select OK on each dialog to close and then Restart your PC. Then, you can skip ahead to the import instructions "Import Allegro file using the Altium Import Wizard", below (look for the dark screen shots from the import Wizard.)
If Allegro is installed on a different computer, or you get a message that:
"Cadence Allegro extracta.exe has timed out, unable to continue translation"
You may be able to convert a *.brd file (native Allegro binary) into a *.alg file (ASCII file used by the Altium Designer Allegro importer) to avoid the timeout converting from *.brd to *.alg. You can also run extracta.exe from the command prompt and examine the log file that is created using the following steps. This method of manually converting to the ASCII file first has been successful even when the wizard has failed on a machine with Allegro installed. It can be performed on a single machine if Allegro is installed and the system variables have been set (see the section just after the first screen shot at the start of this article.)
1. Copy the Allegro binary PCB design file (PCBName.brd) and these two Altium Designer utility files from the computer that has Altium installed, into a working folder of a computer that has Extracta.exe installed as described above.
Note: There was an issue with the version of Allegro2Altium.bat that came with AD20 that was fixed with the release of AD20.1.7 and newer.
2. Open a command prompt (start button ► cmd) and use the change directory command to get into your working folder. Example: cd C:\Documents\Files\Test
3. Once in the right directory, type in the command: Allegro2Altium PCBName.brd
4. The batch file invokes the Cadence-installed Allegro extracta.exe utility, using the AllegroExportViews.txt to direct the ASCII data extraction.
This produces an ASCII "PCBName.brd.alg" file. Now in Altium Designer, you should be able to import the "PCBName.brd.alg" file with no problem.
Note: At the time, an extract.log file will also appear in the directory. This may be useful if any errors occur when using the Cadence Allegro/OrCAD utilities.
5. Copy the new *.alg file(s) to the computer running Altium Designer.
6. Follow the steps below to use the import wizard. If it still times out, the file might be too large for the conversion to ASCII.
Import Allegro file using the Altium Import Wizard
Here's documentation on the Import Wizard:
Contact our corporate or local offices directly.