Home > Community > Forums > PCB Design > Footprint with overlapping pads

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Footprint with overlapping pads 

Last post 02-20-2014 1:09 PM by PCBdesigner100. 5 replies.
Started by PCBdesigner100 19 Feb 2014 02:58 PM. Topic has 5 replies and 1460 views
Page 1 of 1 (6 items)
Sort Posts:
  • 02-19-2014 2:58 PM

    Footprint with overlapping pads Reply

    I have a two terminal component which goes inside the PCB and its two terminals are connected at top and bottom layer of the PCB.

    I am facing problem to create the foot print for this. I need to have overlapping pads which connects to different nets. How is it possible?

    I created one pin with only top pad and drill. Another one with bottom pad and drill. When I place them at same point to create the complete footprint, it shows DRC (pin to pin spacing violation) error. I dont have any other clue.

    Please let me know if anyone have any suggestion.

    Thanks. 

    • Post Points: 20
  • 02-19-2014 5:18 PM

    • Randy R
    • Top 50 Contributor
    • Joined on 07-16-2008
    • Dupont, WA
    • Posts 192
    • Points 3,025
    Re: Footprint with overlapping pads Reply

    I'm not sure what your part terminals look like and if the pins are surface mount or through, but here's a couple of possiblities:

    If it's a single pin going through the board, you can add the NET_SHORT property to the pin.

    If there are two surface mount pins, create two single layer pads (no drill) and if needed add the NET_SHORT property to via(s) that connect the two pads.

     Hope this helps.

    Good Day, R².
    • Post Points: 20
  • 02-19-2014 6:46 PM

    Re: Footprint with overlapping pads Reply

    Thanks Randy. However I am looking for something else. I might not have been clear in last post.

    I will make it more clear. The component,  let say is a plastic screw with nuts on both side. Both nuts need to connect different nets. That means the footprint is actually a through hole pin only..with pads on both side connected to different nets. So the hole is a non-plated one.

    I hope I have explained it now. Please let me know if you have any way to do this footprint.

     Thanks. 

    • Post Points: 20
  • 02-20-2014 6:12 AM

    • chads108
    • Top 50 Contributor
    • Joined on 03-29-2012
    • Plano, TX
    • Posts 162
    • Points 2,755
    Re: Footprint with overlapping pads Reply

    I have dealt with this before and I believe what you need to do here is build your footprint using the non-plated hole you require and draw circular shapes on the top and bottom etch to represent the pads.  Place small surface mount pin inside the shape on top and bottom as the actual pin that the net gets assigned to in the schematic.  Once the netlist is read in, the shape will assume the net of the pin in the shape. 

    • Post Points: 20
  • 02-20-2014 8:54 AM

    Re: Footprint with overlapping pads Reply
    Thanks a lot. This trick helped me.
    • Post Points: 5
  • 02-20-2014 1:09 PM

    Re: Footprint with overlapping pads Reply
    Eventually, there I found another way to do it. One pin with non plated drill and bottom pad only. Second pin is one layer pin with only top pad. These to work fine in overlapped position without inducing DRC error! Two pins can be assigned two different nets.
    • Post Points: 5
Page 1 of 1 (6 items)
Sort Posts:
Started by PCBdesigner100 at 19 Feb 2014 02:58 PM. Topic has 5 replies.