KB: Combine OrCAD Schematic Import and PADS/Allegro PCB import into single Project

Altium Designer Altium Designer
Starting in version: 18 Up to Current
[Why] Create a single project linking imported OrCAD Schematic Project and imported PADS/Allegro PCB Project [What] Place all imported files in one project folder along with *.prjpcb and add them all within the project opened [How] Copy the pcbdoc imported from PADS/Allegro to the project folder imported from OrCAD. WIth the project opened, right click in Projects panel and invoke 'Add Existing to Project...' to specify the pcbdoc.

Solution Details

The import process is a two stage process.

1st - Schematic:

2nd - PCB:


Importing the OrCAD .DSN file will create a project with the schematics.
Importing the PADS .ASC or the OrCAD .MAX/Allegro .BRD files will create a project with the PCB.

Copy the PCB out of the imported PCB project folder and paste into the imported project folder that contains the Schematics.

With the Schematic Project open in Altium; add the PCB file to the schematic project by right clicking on the Project in the Project Panel and selecting 'Add Existing to Project...' then selecting the PCB you have copied and pasted from the imported PCB project folder.


After adding the PCB from one imported project into the other imported project with the schematics; save the project and make sure the component links are matched by their designators.

With your PCB open and in focus:
Execute Project>>Component Links..

Match all components by their designators by ensuring that the 'Designator' checkbox is enabled at the bottom of the dialog and then clicking the 'Add Pairs Matched By >>' button so that all components are then displayed in the Matched Components List followed by clicking the 'Perform Update' button.

Then create a .PcbLib from the PCB

Design>>Make PCB Library


Save the .PcbLib file and save the project. .PcbLib should be automatically added to the project
With the PCB still open and in Focus:
Execute Design>>Import Changes From [Project Name] to see what changes would be made in the ECO and that all is intact as desired.

Ideally there would be no changes and all is in order though in most cases there may be some differences that will need to be investigated to ensure all is intact with the design.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Was this article helpful?