Stats

  • Locked Locked
  • Replies 4
  • Subscribers 167
  • Views 1339
  • 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

Loads of ratsnests after changing component/footprint.

StepscanDarcy

New week, new problem.   The community here on these forums has been amazing at helping me with any issues I've run into so far.  I've completed the changes on one board already!   Now, i'm onto the second board, and I'm just adding one of the same components as last time, but to a different board.    I went about it the exact same way as last time, only this time it's created loads of ratsnest in places that are not near the new connector.   I don't think this happened on the last board, and takes what should be a one afternoon job, and is going to turn it into a few weeks (for someone like me).   Did I do something wrong this time? Or did I just get lucky last time.


What I did:
-updated footprint of old connector in ORCAD Capture by creating the footprint in pcb designer.(same number of pins)

-create netlist from newly saved .dsn file.

-open new .brd that was generated in PCB Designer.

This created LOADS of ratsnest.   I then opened the original .brd file in pcb designer and selected everything in general edit mode and selected "unfix".   I remade the netslist now, and there are still all sorts of new ratsnests, but not as many as the previous export.   

  • StepscanDarcy

    I also can't create a fanout.   I created a fan out on 4 of this same part on a different board. 

    And moving a via can change its net?  I take a via designated to say the fpga, and I move it over a few millimeters to line up with its pin on the connector, and it changes it to a 2.5v via.....I am lost with this program.  It seems to be playing by its own rules haha.


  • redwire
    in reply to StepscanDarcy

    Let me tackle the via question/comment first since it's easier.  Some of your other questions are easier answered if I were to see the board/schematic.

    Via move:  If you used the "move" command then you might encounter another net where you land which Allegro wants to connect to based on how the layers are set up.  Vias are designed to connect to anything that matches their layer connectivity.

    However, if you need to force a via to change its current location and stay connected, use the Route->Slide command and then in the "Options" sub window, change the "Bubble" option to "OFF".  When you drag the via you will see it stay connected.  With this method when you're done you might have to clean up some DRCs.

    Another setting in Slide is Bubble->Shove which will plow straight through to the new location and push everything out of its way.

    I tend to use "shove", then "hug", then "off" knowing how each one reacts.

    And of course use the right mouse options when doing any of these commands to look for snap options that might be useful (e.g. Snap to via, Snap to pin, Snap to line....etc)

    Lastly, look at the copy command as well.  Depending on what you're doing it's sometimes easier to copy then delete.... Be sure to look at the checkbox "Retain net of vias" when copying

  • Ummer

    If number of pins are same then place the updated footprint in the the psm path and use place - > update symbols -> in package symbols select the desired footprints, check ignore fixed property and  update pad stack from library.

    [Note - before updating go to Place->manually and in advanced settings uncheck database and check library]

  • CadAce2K

    You also might try Tools/Derive Connectivity after you've read the new netlist in. Sometimes it will re-connect the lines it can't figure out correctly. Works for me at times. Worth 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.