Connect with us

Via pads in mid-layers

Discussion in 'CAD' started by David, Mar 15, 2005.

Scroll to continue with content
  1. David

    David Guest

    In a multi-layer pcb, if I have a via going from the top layer to the
    bottom layer, is it necessary to have a full pad on the inner layers, or
    just on the layers where there is a connection to the via? For higher
    density cards, reducing or removing the anular ring in inner layers (or
    even the top or bottom layers, if there is no connection) would free a lot
    of routing space.

    David
     
  2. Uwe Bonnes

    Uwe Bonnes Guest

    The anular ring in the inner layers and the space around it gives the needed
    alignment accuracy for the board manufacture. A smaller/no ring needs
    higher accuracy meaning a higher price. Talk to the choosen manufacturer if
    the premium is worth the freed routing space.
     
  3. nospam

    nospam Guest

    It won't free a 'lot' of space. You still have to leave clearance around
    the hole and the hole size you specified is the finished plated size so the
    hole is bigger than you think.

    There is also a slight problem that without a pad there is more possibility
    of a crevice being left between layers when the board is laminated and when
    plating holes there is a possibility the crevice will be plated creating an
    internal short. The closer you have tracks to the holes the more likely
    this is.

    Pads on outer layers provide an anchor for the through hole plating. Plated
    holes are barely bonded to the inside of the hole, they are held in place
    mechanically by their shape. Without pads there is the possibility of
    getting resist down the holes which means they may be partially plated
    and/or partially etched, if the problem goes deep enough you may loose
    connections to inner layers.
     
  4. Hello David,
    our PCB manufacturer removes the unconnected pads in the inner layers,
    because there is no advantage for them in the process.
    No, you can't route closer when you remove the unused pads.
    You must be aware that the drill size is about 4mil more than the
    finished hole size and there are also tolerances of the drill position.

    Summary: You don't get any clearance advantage when you remove these pads.

    Best Regards,
    Helmut
     
  5. David

    David Guest

    Thanks to all who answered - it seems there is nothing significant to be
    gained by removing the inner layer pads myself.

    mvh.,

    David
     
  6. Reiterating what some of the other folks have said...

    1. It doesn't give you any routing space, unless you had a greatly
    oversized pad to start with, because you have to allow clearance for
    the (oversize) drill and drill tolerance.

    2. The fab folks like to remove unconnected inner-layer pads because
    it simplifies their optical inspection and processes, and thus
    improves the fab yield a tiny bit. (And its just a quick one-button
    click on the CAM system to do it.)

    3. You *don't* want to remove pads if you have thick inner-layer
    copper (e.g., 2 oz copper power planes), and/or thin dielectric (2-3
    mil). Removing the pads can lead to 'resin starvation' in that area,
    resulting in voids and shorts between planes. (And I've got the
    burned boards to prove it.)

    4. Some folks want the pads to stay because it supposedly helps to
    'anchor' the barrel of the via. (Other folks say 'taint so; take your
    pick.)

    5. If you are way up there in the regions where signal integrity is
    an issue, removing pads can affect (improve) the capacitance and
    inductance of the via, but you have to do 3D field modeling to make
    any use of that.

    6. If, for whatever reason, you have decided that you want the pads
    to stay, you must explicity say so in the fab instructions. Some
    fabricators will routinely remove them if not told differently.
    Likewise, if you want them removed, you also should say so, or just
    remove them yourself.

    Gary Crowell CID
    Micron Technology
     
  7. Hello Gary,
    your comment in point 3. sounds new to me. It seems I should
    ask my board manufacturer about that.
    There is one thing about inner pads I have in mind. They told me
    that unconnected pads may not hold good enough on the core material
    during drilling. They also automatically create tear drops when an
    inner pad is conencted.

    Thanks for your comments. I will keep it in my library.

    Best Regards,
    Helmut
     
  8. Helmut,
    The comment about the inner pad on a core not adhering very
    well during drilling, that would have to be only for a buried
    via. One that is drilled while the core is still not laminated
    within the stackup. If it is a regular via through the stackup,
    it would of course be completely supported top and bottom between
    pieces of laminate, can't get more secure than that!
    Gary's point 3 is valid but at the extremes. Just think, you
    have a heavy plane area and then a large void area, what will
    fill and bond between the two void areas while the other Cu plane
    areas are setting the final thickness between the two laminate
    layers. The prepreg epoxy will flow into that area but possibly
    not quite enough to fully, completely, fill and bond it 100%.
    Same for very thin prepregs that will have trouble filling the
    gap to start with.
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-