Stats

  • Locked Locked
  • Replies 5
  • Subscribers 164
  • Views 7756
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

back annotate from allegro(pcb) to orcad(schematic)

pakistan

Hi all, 

can I back annotate net from allegro(ver16.0) brd file to orcad schematic.
I have a connector in layout which I can rout as "best rout" but it is very difficult and lengthy process to rout in pcb and then assign ports in schematic manually.
Before allegro we use Pcad. In Pcad we can do it by generating netlist from pcb after best rout and then we compare both netlists and after comparing an ECO file generated, by loading this ECO file in schematic, ports automatically placed according to routing in the pcb layout.
is there any way like this in allegro to rout in pcb then load it in schematic which will reflect accurate pcb routing.
Thanks & Regards

Tanveer

  • pakistan

    actually I have allegro ver16.0 and allegro capture cis ver16.0.

    what is the procedure you follow if you have option to rout according to ease of routing. please let me know the simplest method of doing that sort of thing

     

    Thank & Regards

    Tanveer

  • oldmouldy

    I guess that you mean that connector pins have been swapped inthe PCB to aid routing the PCB? This can be transfered back to the schematic through back annotation. The easiest way is to open Capture, pick the DSN file in the Project Window and then use Tools>Back Annotate, pick PCB Editor tab, specify the netlist directory and BRD file, check Update Schematic and OK to run the Back Annotate. IF you have any reason to believe that the files might not be correctly related, ensure that you have a backup copy of the DSN and BRD files before running Back Annotatation.

  • pakistan
    Hi, Thanks oldmouldy for your prompt reply.I want to confirm one thing when we swap pin in connector as per our routing ease without updating schematic first, we have DRC errors on these pins. Should we ignore them during routing? In my understanding this procedure shold be done after completion of routing, Am I right?

    Thanks & Regards

    Tanveer
  • oldmouldy

    The parts need to be setup to enable pin swapping in the PCB, otherwiae you will be attempting to route the PCB differnetly from the netlist. Use Place>Swap> Components, Functions, Pins as required. Unless you use the Place>Swap functions the loaded netlist will not be changed correctly and the changes will not be back annotated. See Chapter 14 of the Capture USers Guide, cap_ug.pdf in the doc\cap_ug directory within the product installation.

  • pakistan
    Hi oldmouldy,

    Thanks for your guidance. It is working. Now I am able to do back annotation. Thanks again dear, you are a nice person.

    Best Regards

    Tanveer
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.