During PCB design & manufacture it is common to remove the via annular rings on internal layers where the via is not connected to anything, so called non-functional pad removal.

Would it be feasible to remove a non-functional pad on an outer layer? Would this introduce any manufacturing or reliability problems?

enter image description here

As a real-world example, I have a 4-layer PCB design with two outer signal layers, and two inner power layers. A BGA chip on the top layer connects to a power layer through a via, and this via takes unnecessary space on the bottom signal layer. Could this pad be removed to reclaim space for better clearance or routing density on the bottom layer?

  • \$\begingroup\$ I have don’t see any problem , maybe harder than to solder fill fully if desired. \$\endgroup\$ – Tony Stewart Sunnyskyguy EE75 Oct 10 '18 at 11:40

No, you can't eliminate the outer-layer pads on vias. As described here, the final etching step occurs after the plating step. The outer pads serve the very important function of protecting the plating inside the via from the final etch.

Specifically, the plating step is normally done through a mask, so that only the traces and pads on the outer surfaces are built up with plating — first copper, then a thin layer of tin. Then the photomask is removed, and the tin itself serves as the mask for the final etching step that removes the unwanted original (unplated) copper on the outer layers.

A via can be plated only if the electrolyte can flow through it. If you omit the surface pad, then the hole will be partially or completely covered by photomask on that side, limiting or stopping the flow of electrolyte. Furthermore, even if plating is successful, once the photomask is stripped for the etching step, the exposed edges of the plated copper inside the hole will be undercut by the etching process, seriously affecting the reliability of the via.

  • \$\begingroup\$ Could you elaborate a bit? How would the pads protect the plating when there is a "big" hole through the center of the pad? \$\endgroup\$ – Andrzej Szombierski Oct 11 '18 at 10:55
  • \$\begingroup\$ See edit above. \$\endgroup\$ – Dave Tweed Oct 11 '18 at 11:50

What you want is called a buried via. They can be made by more advanced PCB fabricators, but they charge a considerable premium for them.

  • \$\begingroup\$ Actually, in this case it would be a "blind via". Also a premium feature. \$\endgroup\$ – Dave Tweed Oct 10 '18 at 13:40
  • \$\begingroup\$ @DaveTweed No, they're buried vias. One end of a blind via is accessible from the suface of the PCB. A buried via, as the name suggests, is buried on both sides. \$\endgroup\$ – dzereb Oct 11 '18 at 7:40
  • \$\begingroup\$ A blind or buried via omits the hole on some layers. I meant only to omit the copper. \$\endgroup\$ – Andrzej Szombierski Oct 11 '18 at 10:45
  • 1
    \$\begingroup\$ @dzereb: The OP wants a via that connects the BGA on the surface to an inner power plane, without coming out the other side. That's a blind via. \$\endgroup\$ – Dave Tweed Oct 11 '18 at 11:37

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.