Stats

  • Locked Locked
  • Replies 4
  • Subscribers 165
  • Views 14831
  • 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

How to link a spiral inductor to its symbol in schematic

Leron

Dear All,

in my schematic I have an inductor. This inductor does not have a corresponding component for PCB because I want to realize it as a spiral printed on the PCB.

I am wondering how can I create a PCB footprint that is in principle just a piece of metal on the etch/top layer but with two pins in order to have the netlist and the brd to be correlty created.

Any suggestion?

Thanks a lot

Francesco

Parents
  • steve

    Make a footprint (filename.dra) of the spiral track that simply contains two pins (for the connect points). You can make the pins just a small smd dot pad (say 0.2mm) and make sure it is just a TOP pin with no mask or paste). Place these at the connect points of the spiral winding. When the part is placed you only have to wire to the spiral,

  • Leron
    in reply to steve

    Hi Steve,

    thanks.

    does this mean that everytime I use the inductor I have to design it on the PCB? I am worried that connecting with spiral etch the pins in the .dra will result into an error since the two pins will result as electrically shorted.

    Francesco

  • steve
    in reply to Leron

    No, design it as a symbol and then once it is in the board the copper will take on the netname of one of the pins and you will see a DRC error. Use the NET_SHORT property on the pins (Edit Properties then select the Pin) which has a value of netname1:netname2, this means you can effectively short the two nets together.

Reply
  • steve
    in reply to Leron

    No, design it as a symbol and then once it is in the board the copper will take on the netname of one of the pins and you will see a DRC error. Use the NET_SHORT property on the pins (Edit Properties then select the Pin) which has a value of netname1:netname2, this means you can effectively short the two nets together.

Children
  • Leron
    in reply to steve

    It works.... thanks a lot!!!!!

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.