对于使用 OrCAD-Allegro 工具链进行设计的工程师来说，遵守这些准则可减少设计反复次数，提高设计质量，并避免出现软件错误的发生。益处多多！

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 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
- 2 -
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 or
>-
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 any
problems are detected, you must correct them in the design file and
generate the board file again until an empty swap file is generated.

专栏文章内容及配图由作者撰写发布，仅供工程师学习之用，如有侵权或者其他违规问题，请联系本站处理。 联系我们