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
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