12
\$\begingroup\$

When putting mounting holes for screws on a PCB, should the holes be plated or unplated?

I've read plating the holes provides better support for the screw and helps prevent the PCB from being damaged, but looking at some PCBs I have around (including the extremely popular Arduino UNO), most of them don't seem to have plated mounting holes.

\$\endgroup\$
  • 4
    \$\begingroup\$ Non-plated through holes can add an extra step to PCB fabrication. \$\endgroup\$ – Scott Seidman Jun 19 '14 at 14:43
12
\$\begingroup\$

If the screw is used to ground the board (for example, PC motherboards) then plated is the way to go- this one has the top, bottom and internal ground plane tied together with many small vias radially around the hole. There is no thermal relief on the vias. The vias ensure that even if the hole plating is damaged by the screw thread, the top and bottom pads are solidly connected to the ground plane.

enter image description here

Otherwise it doesn't matter much, though if you don't have any other unplated holes in the board, as Scott Seidman says, it can add cost to the board. Whether there is a pad or not (and the finish on the pad after assembly) may affect what kind of lockwasher or screw you choose to use on the PCB, since solder has a tendency to cold flow.

If the board is multilayer, there should be a large clearance between non-connected internal planes and (particularly) an unplated hole, because the thread can damage the internal surface (and sometimes people do things like drilling out holes that don't quite match the mating surface), and you don't want the screw shorting to (say) an internal power plane.

\$\endgroup\$
6
\$\begingroup\$

I don't see why a plated hole should provide better support or protection. A mounting hole should be a bit bigger than the screw that it will fit, the coating material of the hole's internals does not matter at all.

As Scott says non plated holes could add an extra step: think of it, you etch your pcb, drill all the holes, plate them and you are good to go. If you want to have non plated holes you need to make another drill run after the plating, and that can be quite time and money expensive.

So here's my guess: some PCB manufacturers use different drilling machines for different hole sizes: the tiny, through-hole like holes are drilled with one machine while the bigger, some five to ten mm holes are drilled on another. If you drill the bigger holes after the plating you don't add a step at all and you save coating material, which is good. Now that's why your arduino has non plated mounting holes.

All that said, that applies only if with plating you mean plating. If we are speaking of the pads around a mounting hole now that's a completely different story.

\$\endgroup\$
  • \$\begingroup\$ Can you explain what the "different story" is regarding the pads around a mounting hole? I have a very similar doubt but regarding the copper pads ("annular ring" is another name for the same thing I believe) surrounding the hole on the top and bottom layers rather than the plating inside the hole on the inner layers. \$\endgroup\$ – scuba Aug 25 '17 at 15:10
  • \$\begingroup\$ @scuba for the pads you do not need the deposition extra step since copper is already on the PCB. \$\endgroup\$ – Vladimir Cravero Aug 26 '17 at 16:01
6
\$\begingroup\$

A few of things to consider:

  • The plating thickness is not something that the board house can control to super tight tolerances, but 0.001" is a good rule of thumb. You're not going to get any extra support there.
  • You should be calling out finished hole sizes in your design. Since the plating thickness varies, you can end up with tighter mounting holes than you spec'd. Plan accordingly.
  • If you're relying on the plating to make a connection to an internal ground plane, and an assembler over torques a screw, you run the risk of damaging the plating and breaking that plane connection. This is only an issue if tolerances are not carefully considered.
  • As an aside, some board houses do not like to plate holes that do not have traces going to them. We had some boards with Tag Connect headers, and the guide holes were plated. Until the footprint was fixed, we got a phone call on that one every time.
\$\endgroup\$
5
\$\begingroup\$

For the small chance that the PCB builder may mistakingly not-plate all the holes (disaster city) I'd make all the holes plated. Plus what @scottseidman said as a comment - it's an extra process.

I'd also add this - "should all mounting holes be connected to local PCB 0V?" - some will benefit and some won't of course. I attach them and put little 0603 pads to link them to the ground plane then this covers all eventualities. This mainly applies to circuits inside metal boxes but also, when bench testing it gives a nice copper area to join 0V wires from inputs etc.

\$\endgroup\$
1
\$\begingroup\$

I've read many advantages/reasons on different forums about these mounting holes with vias but I did not see the reason that I am using them for.

With plated mounting holes, if the board is going through a wavesolder machine during the assembly process, all these holes need to be masked with a piece of kapton tape to prevent the solder to get into these holes.

Using non-plated mounting hole with vias eliminates the placing/removing kapton tape step assuming that these non-plated mounting holes have their bottom pad covered with soldermask.

This was suggested to me many years ago from a board assembler contractor. Since then, that's how I make my mounting holes.

New contributor
Yvon Hache is a new contributor to this site. Take care in asking for clarification, commenting, and answering. Check out our Code of Conduct.
\$\endgroup\$

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.