Home > Community > Forums > PCB Design > Should you have pads on the power and gnd layers in stackup

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: *

 Should you have pads on the power and gnd layers in stackup 

Last post Wed, May 9 2007 8:23 AM by archive. 4 replies.
Started by archive 09 May 2007 08:23 AM. Topic has 4 replies and 874 views
Page 1 of 1 (5 items)
Sort Posts:
  • Wed, May 9 2007 8:23 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    Should you have pads on the power and gnd layers in stackup Reply

    Hi,
    I am wondering if you need pads defined in the power and ground planes in my stackup.  I do have them defined in my routing layers, but are there any reasons to or not to have them for the power and ground planes.  Currently, I just have thermals and an antipad defined for them.

    Thanks


    Originally posted in cdnusers.org by cadencesks
    • Post Points: 0
  • Wed, May 9 2007 8:46 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Should you have pads on the power and gnd layers in stackup Reply

    On dedicated power and ground planes it is best to only have anti-pads instead of donuts (Anti-pad & Regular pad). This is really a fabrication concern due to the fact that plane layers tend to shift around during the fabrication process and you don't want the vendor to control regular pad drill breakout on a layer that does not require a connection. One added benefit of just using an anti-pad on power and ground layers is increased plane clearance because your isolation will be between the plated thru hole wall and not the end of the pad. The same would go for inner signal layers where it is best to suppress the Regular pad on a layer that does not require a connection.

    My two cents,
    Mike Catrambone
    UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Post Points: 0
  • Wed, May 9 2007 9:05 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Should you have pads on the power and gnd layers in stackup Reply

    Thanks Mike,
    that makes sense.

    What do you think about mounting holes? I was thinking that i would only need to use a pad on the top and bottom layers. I don't want to increase my capacitance or inductance by adding pads on the inner layers, but if I did that may add strength to the board. I also would not define thermal or anti pads.

    Thanks,
    Louis


    Originally posted in cdnusers.org by cadencesks
    • Post Points: 0
  • Wed, May 9 2007 9:24 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Should you have pads on the power and gnd layers in stackup Reply

    I have constructed mount holes in many ways, pads on all layers of the board, pads on just on top and bottom and no pads at all. It really depends on the type of hardware used in the mounting hole and its application. For example, if you using a #6 or #8 screw with an external or internal tooth lock washer you may want to have a nice copper pad for it to rest on so it does not tear up the bare laminate. Also there is always concern with the compression zone around the mounting hole causing issues on inner layers and if there are pads on every layer from the mounting hole it will help strengthen the area as you indicated.

    Now if this mounting holes needs to be connected to a Ground plane then I would strongly suggest using vias or pins around the mounting hole to ensure the connection to the Ground plane remains reliable, most design today use this technique and you may already. If you just use a plated thru mounting hole then you risk fracturing the hole wall and breaking the connection the Ground plane which could lead reliability problems.

    Mike Catrambone
    UTStarcom, Inc.


    Originally posted in cdnusers.org by mcatramb91
    • Post Points: 0
  • Wed, May 9 2007 11:20 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,950
    RE: Should you have pads on the power and gnd layers in stackup Reply

    Ok,
    thank you for the helping me clear up my confusion.
    Louis


    Originally posted in cdnusers.org by cadencesks
    • Post Points: 0
Page 1 of 1 (5 items)
Sort Posts:
Started by archive at 09 May 2007 08:23 AM. Topic has 4 replies.