Best practices for Capture-Allegro

Best practices for preparing a library for Capture-Allegro PCB Editor flow
 Limit part and pin names to 31 characters
 Use upper case characters for part/symbol names, part references designators, and pin names
 Do not use special characters to assign part names, references designators, and pin names
 Do not use duplicate pin names for pins other than power pins
 For multiple power pins with the same pin names, do not make some pins visible and other invisible
 Do not use "0" as a pin number
Best practices for Capture design for Allegro PCB Editor
 While defining a net list alias or a net name
 Keep the maximum length of a net name or alias up to 31 characters
 Do not use lower case or special characters in a net name
 Avoid using "Power Pins Visible" property at design level
 Use net to connect pins
 Leave room for assigning a net name. Pin-to-pin connection changes the net name when a user moves a component
 Run the Capture DRC command before generating Allegro PCB Editor netlist
 Set path for Allegro PCB Editor footprint before running Netrev
Best practices for smooth back annotation
 Do not change design name, hierarchical block names, or reference designators in Capture after board files creation
 Do not edit a part from schematic in Capture after board file creation
 Do not replace cache as it changes the Source library name and part name, in capture
 Do not change the values of component definition properties in capture after board files creation
 Do not change Design file/root schematic/hierarchical block names in Capture after board file creation
 Do not add or delete components to or from the schematic design immediately after the board file creation. Add or delete components after finishing the back annotation process

Do not add any additional components in Allegro PCB Editor. Instead, add components in Capture and take them to Allegro PCB Editor
 Do not add, rename, or delete a net in Allegro PCB Editor
 Do not change the format for reference designators for parts in Allegro PCB Editor as <Alphabet(s)><Numeric><Alphabet(s)> or
><Alphabet(s)>-<Alphabet(s)>
 Run Allegro PCB Editor Dbdoctor before running Back annotation by selecting the Database Check command from the Tools menu in Allegro PCB Editor Make backups of the original design before updating the design with the swap information in Capture Back annotate the design immediately after making the board file.
Though it does not a mandatory step, back annotating the design before placing components helps avoid problems in back-annotation at a later stage.
If back annotation at this stage generates an empty swap file, you can proceed with placing and routing the board file. In case and problems are detected, you must correct them in the design file and generate the board file again until an empty swap file is generated.