Actions
Forum Thread Details
  • State Not Answered
  • Replies 4 replies
  • Subscribers 181 subscribers
  • Views 887 views
  • Users 0 members are here
Related

Why does Eagle not have a "standard" way to link Analogue and Digital grounds

Former Member

The common practice is to keep the analogue and digital grounds seperate and then link them at 1 point. Many  people that have tried to do this over the years have used various work arounds to do this in a "safe" manner without getting DRC errors. Other people have done things that generated DRC errors and then approved them like create a part that has overlapping pads. In either case, the search gives the impression that the Eagle PCB does not have a standard built in method to allow this. Why?

  • 0

    Possibly because there are many ways to do it which for most people are good enough. Approving one DRC error isn't the end of the world. If I have separate grounds I usually create the star point for AGND and 0VD connections with a resistor jumper so I can easily disconnect during debug or fit other components if there are issues. However, with good design practices, partitioning grounds often isn't necessary and can lead to it's own signal integrity issues for any signals having to cross the boundary between the separate grounds.

     

    Mentor Graphics in their DxDesigner have a horrible way using net aliases to alias one global net to another. Until a couple of years ago this totally broke when you had a design with hierarchy, so basically for anything but small designs it was broken. I don't know what Cadence or Altium do for this. If you have suggestions for how this could work then maybe pop it into the suggestions forum.

     

    Best Regards,

     

    Rachael

  • 0 in reply to rachaelp

    In KIcad, the idea for a "net tie" is to use a graphic element (instead of

    a trace) between 2 pads. Can Eagle use the same concept?

     

    https://forum.kicad.info/t/protip-2-net-tie/1112

     

    Rick

    --

    Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

     

  • 0 in reply to rick_b

    On 5/08/2016 7:45 a.m., Rick Brown wrote:

    In KIcad, the idea for a "net tie" is to use a graphic element (instead of

    a trace) between 2 pads. Can Eagle use the same concept?

     

    https://forum.kicad.info/t/protip-2-net-tie/1112

     

    Rick

     

    Sure can,

    Create a user defined layer

    On that layer use a wire to overlap the two different grounds at the

    connection point.

    When you make your gerbers, include that user defined layer with the

    copper layers for that side of the board.

     

    HTH

    Warren

     

     

  • 0

    Am 04.08.2016 um 12:29 schrieb curiousengineer:

    The common practice is to keep the analogue and digital grounds seperate and then link them at 1 point. Many  people that have tried to do this over the years have used various work arounds to do this in a "safe" manner without getting DRC errors. Other people have done things that generated DRC errors and then approved them like create a part that has overlapping pads. In either case, the search gives the impression that the Eagle PCB does not have a standard built in method to allow this. Why?

     

    --

    To view any images and attachments in this post, visit:

    https://www.element14.com/community/message/203062

     

     

    Check the "supply-dummy.lbr".

    It contains a dual gnd device but using additional layer 53/54, so watch it.

     

    --

    Mit freundlichen Grüßen / With best regards

     

    Joern Paschedag