Home > Community > Forums > PCB Design > How to connect vias to specific layers

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: *

 How to connect vias to specific layers 

Last post Mon, Dec 16 2013 6:37 AM by Mike Veal. 9 replies.
Started by tmd63 26 Sep 2013 06:39 AM. Topic has 9 replies and 2107 views
Page 1 of 1 (10 items)
Sort Posts:
  • Thu, Sep 26 2013 6:39 AM

    • tmd63
    • Top 200 Contributor
    • Joined on Mon, Jul 23 2012
    • Stonehouse, Gloucestershire
    • Posts 39
    • Points 855
    How to connect vias to specific layers Reply

     I have a design which has 7 layers. The top layer has only short stubs.

    There are two layers for traces but they are sensitive signals and there is a solid ground plane above and below these two layers. I have connected these two planes at one point near the incoming supply. I also have a single ground plane as layer 7 which is noisy.

    How do I connect a number of ground signals from Layer 1 to Layer 7 WITHOUT connecting to the other two ground planes, which would inject noise onto these planes? 

    When I try using the normal vias, they connect all planes from 1 to 7 and also 2 and 5, I just need layers 1 and 7 connected but they need to connect at the supply (one via connecting layers 1, 2, 5 and 7).

    The impossible we do straight away. Miracles take a little longer.
    • Post Points: 80
  • Thu, Sep 26 2013 7:09 AM

    • chads108
    • Top 50 Contributor
    • Joined on Thu, Mar 29 2012
    • Plano, TX
    • Posts 185
    • Points 3,255
    Re: How to connect vias to specific layers Reply

    You can do this one of two ways.

    First  method is to attach the no shape connect property to the individual vias you are working with and then manually connect them with clines to the layers you want them to connect to.

    Second method would be to void an area, or put a route keepout, around the vias on the layers you do not want them to connect to.

    • Post Points: 5
  • Thu, Sep 26 2013 8:28 PM

    • redwire
    • Top 10 Contributor
    • Joined on Thu, Jul 17 2008
    • Allen, TX
    • Posts 878
    • Points 13,525
    Re: How to connect vias to specific layers Reply

     Have you talked to your fabricator about a 7 layer design?  Most PCBs are fabricated with an even balance of copper layers for cost reasons.  I would suggest adding an 8th layer or making sure your design is at the proper cost target before doing an odd stackup count.

    • Post Points: 20
  • Fri, Sep 27 2013 12:36 AM

    • tmd63
    • Top 200 Contributor
    • Joined on Mon, Jul 23 2012
    • Stonehouse, Gloucestershire
    • Posts 39
    • Points 855
    Re: How to connect vias to specific layers Reply

    My design is not a standard Glass Fibre/Epoxy design and yes, it is standard for my design fabrication to use odd and even layer counts.

     #Chads108, Is there any way of adding the route keepout to a via (maybe give it a new name to separate the new via) instead of doing it for each via in the design?

    The impossible we do straight away. Miracles take a little longer.
    • Post Points: 5
  • Fri, Nov 15 2013 7:55 AM

    • ericchen
    • Not Ranked
    • Joined on Tue, Nov 5 2013
    • Posts 4
    • Points 35
    Re: How to connect vias to specific layers Reply
    and you can use the constain manager;
    • Post Points: 20
  • Thu, Dec 12 2013 1:19 AM

    • Khurram
    • Top 200 Contributor
    • Joined on Sat, May 16 2009
    • Karachi, Pakistan
    • Posts 41
    • Points 715
    Re: How to connect vias to specific layers Reply
     Now I think Cadence should introduce a property (something like “No_shape_Connet_exldue_layers”) which will allow shapes to connect vias on some particular layers while disconnect them on remaining because other methods are time consuming and not reliable.

    Thanks

    Khurram
    • Post Points: 5
  • Fri, Dec 13 2013 1:29 PM

    • ScottCad
    • Top 50 Contributor
    • Joined on Sat, May 26 2012
    • Roswell, GA
    • Posts 176
    • Points 2,775
    Re: How to connect vias to specific layers Reply

    Hello, You can do what you need by using voids on the inner layers but this is kind of a manual way of  doing things.

    A better way to handle these grounds is at the schematic level and pass the net information to the PCB editor.

    On your schematic consider using different grounds "net names" example gnd, agnd, gnd1, gnd2 etc. The advantage is a plane in the pcb editor with the same net name will be a "Connect" and planes that do not have the same net name will have no connection to a via or pin.

    From what you write it sounds like all your ground planes have the same net name ? hence the issue.

    Thanks Scott 

    • Post Points: 20
  • Fri, Dec 13 2013 1:43 PM

    Re: How to connect vias to specific layers Reply

    I've seen the requirement of a signal via (50 ohms) with ground vias adjacent to it.  Ground via spacing was critical to the impedance.    As a bonus, ground vias could only be connected to planes adjacent to the signal layer (ATE fixture.)

    Would be a lot easier if we could add voids to the padstack.  In the meantime, vias as netlist components?  Painful but safe solution...

     (Flashback to the early 90's when PCAD couldn't verify a netlist connection to a negative plane.  This was our safety net.) 

    • Post Points: 20
  • Fri, Dec 13 2013 5:47 PM

    • ScottCad
    • Top 50 Contributor
    • Joined on Sat, May 26 2012
    • Roswell, GA
    • Posts 176
    • Points 2,775
    Re: How to connect vias to specific layers Reply

    Gosh PCAD like voids... Man I rember those days..I dont believe the voids were needed in padstacks from ver 6 on as
    memory recalls as they made a bunch of good changes to the program back then.

    Dont think vias as netlist components is viable.. EZ way is just break up your planes and associate those planes with specific nets.
    Then it does not matter what via is used. On a multi-layer design with positive inner planes the vias wont need voids if the net
    assigned to the via is different than the net assigned to the plane. The plane will get automaticly cleared for the via...

    In Allegro I think it is better to use positive planes, easier to see connectivity.

    In the old days people used negative planes to reduce the size of the artwork gerber output and also to speed up re-draws. Mainly the
    redraw speed of the graphics.. We got better graphics cards and faster PC's now so even on a large board a positive plane is a non issue..

    That ATE test fixture sounded fun :)

    Thanks Scott

    • Post Points: 5
  • Mon, Dec 16 2013 6:37 AM

    • Mike Veal
    • Top 500 Contributor
    • Joined on Mon, Jul 14 2008
    • Posts 29
    • Points 565
    Re: How to connect vias to specific layers Reply

    ScottCad wrote the following post at 12-13-2013 9:29 PM:

    Hello, You can do what you need by using voids on the inner layers but this is kind of a manual way of  doing things.

    A better way to handle these grounds is at the schematic level and pass the net information to the PCB editor.

    On your schematic consider using different grounds "net names" example gnd, agnd, gnd1, gnd2 etc. The advantage is a plane in the pcb editor with the same net name will be a "Connect" and planes that do not have the same net name will have no connection to a via or pin.

    From what you write it sounds like all your ground planes have the same net name ? hence the issue.

    Thanks Scott 

     

     ^^^ This is the solution.

     Label your two grounds with differentnet names in the schematic. GND and AGND for example. Connect them with zero ohm resistors at the one point you want them to join.

     

    Be very careful that you have a return path for the current to get into the GND pins of the chips at each end of the net.

     

    • Post Points: 5
Page 1 of 1 (10 items)
Sort Posts:
Started by tmd63 at 26 Sep 2013 06:39 AM. Topic has 9 replies.