Flow overview
In the Allegro X ecosystem, the schematic (Allegro X Design Entry CIS, successor to OrCAD Capture CIS) and the layout (Allegro X PCB Editor) exchange data through an Allegro-format netlist. This path produces three text files — pstchip.dat, pstxprt.dat and pstxnet.dat — describing parts, instances and connections. PCB Editor reads them and creates or updates the board database (.brd).
- Libraries: symbol (
.olb), footprint (.dra/.psm) and padstacks (.pad). - Annotated and checked schematic.
- Netlist and board creation/update.
- Placement, routing, verification and manufacturing outputs.
- Back-annotation of changes to the schematic.
1. The library causes most errors
Every symbol needs the PCB Footprint property filled with the exact footprint name (no extension). PCB Editor looks for that name in the directories set under Setup > User Preferences > Paths > Library, in the psmpath (footprints) and padpath (padstacks) variables.
Classic error: symbol pin numbers do not match the footprint (e.g., a symbol pin “A1” against footprint pin “1”, or a thermal pad with no matching pin). The netlist is generated, but the board import fails. Always check pin numbers on both sides.
When the library is managed by CIS (Component Information System), parts come from an ODBC-linked database with fields such as internal part number, manufacturer, MPN, footprint and lifecycle status. This reduces typing and keeps the bill of materials (BOM) consistent.
2. Prepare the schematic
- Tools > Annotate — assigns unique reference designators (R1, C1, U1…).
- Tools > Design Rules Check — flags floating pins, single-node nets, duplicate references and missing properties.
- Review power nets and off-page connectors: identical names join nets across pages.
3. Generate the netlist and create the board
In Tools > Create Netlist, PCB tab, enable the option to create or update the PCB Editor board (the so-called netrev). You can start from a board template (with outline, stackup and rules already defined) or update an existing .brd. By default the netlist files go to an allegro folder next to the project.
If the board already exists, PCB Editor can also import the logic through File > Import > Logic.
Tip: always read the netrev.lst generated by the import. It tells you exactly which footprints were not found and which pins did not match.
4. First steps in layout
- Define the board outline and keepout areas.
- Set up the stackup in Setup > Cross-section before routing (see the stackup article).
- Use Place > Quickplace to bring all components next to the board, then Place > Manually to place them by functional block.
- Enable cross-probing between schematic and layout to select a component on one side and see it highlighted on the other.
5. Engineering changes (ECO) and back-annotation
Pin/gate swaps and renumbering done on the board go back to the schematic through Tools > Back Annotate in Capture. Schematic changes go to the board by re-running the netlist with the option to update the .brd. Keep one direction at a time and version your files before each synchronization.
References and further reading
- EMA Design Automation — netlisting lesson in OrCAD Capture
- Cadence Community — Allegro X Capture CIS forum
- Cadence Community — Allegro X PCB Editor forum
Original text for educational purposes. Menus and commands may vary between Allegro X versions; check the Cadence documentation for your version.