Stats

  • Locked Locked
  • Replies 5
  • Subscribers 165
  • Views 13796
  • 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

Through via on trace does not generate DRC error.

esemper1

Hello all,

 I had  a few B/V vias on my design and decided to swapp them out for through vias to lower manufacturing cost. The problem is that some of the BB vias that were placed under a trace are not generating DRCs after being converter to through vias. These now go through the traces and therefore cut the traces in secgements. How can I have PCB editor 16.5 generate DRCs for these?

Here is what I have tried: Dtabase check, Deleting all BB vias and leaving only my through vias, refreshing all padstacks, rechecking for DRCs.

  • steve

     How did you "swap" the BB Vias out ?

  • esemper1

    Steve,

    I used the Edit > Replace function. I also replaced some with the Via swap function. However, now i cant tell wich vias were replaced with what funciton.

  • steve

     I'm assuming you mean Tools - Padstack - Replace or hover RMB - Replace padstack. The DRC's just activate straight away when I do this. Are all the DRC's turned on ? Are the Spacing rules set correctly ? Have you use Unused Pad Supression ? If so are the Hole To DRC's enabled ? Can you run a DB Doctor ? Are you running the latest hotfix ?

    Sorry for all the questions just trying to get to the bottom of your issue. 

  • esemper1

    Steve,

     I deactivated the Unsed pad supression. Now I have many DRCs because all the anular ring of all vias was reinstated which helps me spot where i have a via on a trace. I have more DRCs than I needed now but I can easily slide the vias further away from the traces. Can I get rid of all those DRCs and re-supress all un-used pads again?

  • steve

     Yes - clear the DRC's using Slide as you would normally then once you are finished just enable the Pad Supression again. It's that simple.

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.