Stats

  • State Not Answered
  • Replies 3
  • Subscribers 162
  • Views 12890
  • Members are here 0
More Content

Copying circuits from one pcb design to another

HSID

I am using Allegro PCB editor 17.4. Is there a way to copy a circuit from one pcb design to another.

I know I can make a reuse within the design and place a copy of that reuse in the same pcb design. 


But can you copy from one design to another.

If you can, do the ref designators need to be the same. 

Are there any setup involved.

Thanks

  • 0

    Well it can be done but it is not as simple as just cut and paste. If you have an existing circuit you can create a sub drawing of the etch and export it for re-use.

    The process is basically this. Update your schematic so that it includes the new components and a netlist can be generated. To copy the etch of your existing
    circuit. Go to Export "Sub Drawing" Draw a box around the area you need and when everything is highlighted click somewhere in the box and a dialog box will
    pop up that allows you to save the file somewhere on your drive.

    These particular files are called .clip files so before you begin update your clippath under user preferences to point to the folder you want to save the files to.

    To pull the file back in you use import sub drawing.

    When you create the sub drawing under options you can preserve the net name of various things such as shapes. This might be useful if you have copper pours
    in your design etc. You can also export the pcb footprints but it is best not to include them because your new netlist will have them. The basic idea is you only want the
    etch. The etch wont have any net names so basically it is kind of dumb graphics.

    When you import your new netlist you will have the components with their net and pinning info available for placement. The idea is to overlay the footprints on the
    etch. The etch will then take on the net info.

    It is a good idea after you create the sub drawing to import it and remove anything that you may not need and then export it again so it can be used.

    When all is complete your schematic will match your board.

    All the best.

  • 0

    Are you asking if you can use Place Replicate (.mdd file) in a different pcb design than it was created? You can do this but stack-up will need to be the same (i.e. same number of layers and same layer naming) then just copy .mdd file to the location of new pcb design, and Place Replicate Apply the same way as in current design.

    Hopefully this is helpful.

    Cameron

  • 0 in reply to camdal894

    Thank you for the info, I will give this a try.

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.