The typical workflow in PCB design is one where schematics lead the entire design. They define the electrical connections between parts that will later be reflected in the physical layout. While the design specifications, including footprint assignments, do start in the schematics, there are some instances where one would work directly in the PCB layout to make changes to footprints without starting in the schematic.
Why would we go directly to the PCB layout to swap footprints instead of always starting from the schematic? There are a few good reasons for this:
- Footprints are being important and swapped for mechanical floorplanning purposes
- A design variant is being created with a slightly different footprint
- A part is out of stock and it requires a pin-compatible replacement
If you decide to go this route before annotating the schematics, here’s how you can make footprint changes directly in BRD files in Allegro PCB Editor.
Simple Footprint Swaps in the PCB Editor
Before beginning any footprint swaps in the PCB Editor, you will need to enable logic modification. To do this, navigate to Setup/User Preferences in the top menu. The User Preferences Editor will appear and from here you can enable logic editing. Search for the string logic_edit in the Search bar at the bottom, and enable the checkbox that appears for the logic_edit_enabled preference.
Click OK to close the window. You can now edit the netlist logic that was used to define your electrical connections in the PCB. This will be used in the following sections to create a dummy part from the library and then modify its net connections.
Replacement From Library
When replacing a component from the library, we first need to find the part that we want to modify by reference designator. Suppose we have a design and we want to swap component C135 for a different footprint (same reference designator and net connections). The fastest way to do this without going back to the schematic is to use the Logic/Part Logic option in the top menu.
This opens the Parts List dialog where we perform the following:
- Search for the component you want to swap by reference designator
- Select the matching entry from the search results
- Select the new component data you want to use:
- For a component library entry in TXT format, use the Physical Devices option
- To select a footprint in the system library, use the Physical Packages option
- Select the component data and hit OK
- Click the Modify button in the Parts List dialog to save the modified component
- Click OK to go back to the PCB layout
After clicking OK, the footprint assignment for that reference designator will be updated and the new footprint should appear in the PCB layout. In some cases, you may need to manually place the component again using the Place/Manually… option.
Replacement From Another BRD File
If you want to place a footprint from another PCB layout, you will first need to export the footprint from the other design. Once this is done, you can add it to your library on your local machine in the system folder, or you can keep the footprint in the project folder. No matter where you want to store the footprint, you can first assign the footprint to a library part, then follow the library replacement route shown above.
You could also create a “dummy” part and place it in the PCB layout with the replacement footprint from the library. The existing part with the old footprint can then be deleted, and the original reference designator can be assigned to the new component in the Part Logic dialog shown above. The dummy part will be created from a part that already exists in your library, so your library should already contain the footprint you want to use.
Assign Nets and Complete Routing
Once the new footprints are imported and reference designators are assigned, it’s time to assign nets to the pads on the new component. For small components, like a resistor package or a small IC, this just takes about a minute if the nets are not already assigned. To assign the nets, select the Logic/Net Logic option from the top menu. From this list of nets in the design, select a net you want to assign and click a pin on the component. Continue this until all the pins have nets assigned to them, just make sure to watch for the pin numbering in the new footprint!
Now that nets are assigned, you can place the component and complete the routing as normal. This completes the design update beginning from the PCB layout. If you ever decide to make the changes permanent, you can go back to the schematic and back-annotate with the different footprint assignments, as well as new part number assignments if they were changed.
No matter how you need to edit or build your PCB layout and libraries, you can take full control over your design data package using the best set of PCB design features in Allegro PCB Designer from Cadence. Only Cadence offers a comprehensive set of circuit, IC, and PCB design tools for any application and any level of complexity.