Via pads in mid-layers

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

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.

"David" schrieb im Newsbeitrag news: snipped-for-privacy@westcontrol.removethis.com...

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

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

mvh.,

David

Reiterat1. 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.

1. 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.)
2. 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.)
3. 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.)
4. 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.
5. 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

"Gary Crowell / VCP" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

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

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.