I need my pads for connectors to be plated so that the pins from the connectors can be soldered. But the bottom side cannot have copper pad/annular ring. I have made the pads as shown in the figure below. Bottom pad size is same as the hole size and the hole is Plated.

Is this the proper way? Will there be risk that the holes will be unplated my the manufacturer?

enter image description here

  • 1
    \$\begingroup\$ Only your fab house can tell you that. \$\endgroup\$ May 20, 2015 at 11:21
  • 2
    \$\begingroup\$ There is normally a minimum annular ring spec from the board house- say it is 0.006". Zero (or negative) is less than whatever it is, so at the very least it will cause a DRC error. You will have to ask, as Ignacio suggests. \$\endgroup\$ May 20, 2015 at 11:38

3 Answers 3


Well as comments have said only your fab house can tell you for sure. You should try to keep a close relationship with them as they're basically your partner in all your designs :)

Now this question just happened to come up for me as well a few months ago on a really dense board. I use Via Systems when in the US, a very large and capable manufacturer. I asked them a similar question, could I make vias that only had an annular ring on one layer. Their reply was no don't do that, we can't plate the via properly that way.

Your shop may tell you it's ok but I would expect they won't like it. There's always surface mount connectors. Or and you'd have to ask about this to but I imagine you could just not plate those vias and only route to the top layer where the pad is. There really wouldn't be much holding the connectors on the board at that point and I'd look at mechanically securing them to the board. Maybe epoxy or screws or something like that.


Will there be risk that the holes will be unplated my the manufacturer?

Yes. Most PCB plating operations occur after drilling and before etching. A board with copper on both sides drilled for all the holes requiring plating. Then a conductive solution is sprayed (or dipped) such that all the holes now have a conductive surface - this is the activator. Using electrolytic plating, copper is plated - this thickens the existing copper on the sides, and puts copper over the activator inside the holes. The holes are now plated.

The PCB then gets cleaned and an etching mask is applied that will protect the copper that is to be left on the board.

In theory the mask could be applied just at the hole, and thus leave you with the finish you want - no annular ring.

However, there's always a degree of mis-registration in this process, and it's possible to end up with a damaged plating in the hole if the mask isn't placed precisely.

This is why most PCB fabricators specify a "minimum annular ring".

You'll need to have a discussion with your PCB fabricator about this.

If you can live with a small annular ring, then the minimum may be sufficient. If you cannot have any annular ring, the PCB fabricator will likely be able to make your board with special instructions and an additional cost.

I'd start by carefully examining exactly what you need when you say, "bottom side cannot have copper pad/annular ring" because there's always a little error in everything, and I have a hard time believing you're using a standard component and it doesn't allow an annular ring.

There are probably other solutions as well, but without a better description of the part and how it's meant to be attached, it'll be hard to resolve this for you.


I think you have to provide a convincing reason why you think you cannot have pads on the bottom of the board. If you have pads on the top side among the connector pins there is certainly no reason that it is not possible to have pads on the bottom side too.

Through hole connectors are generally soldered from the bottom side and would certainly be done that way at a production fabrication shop. Hand soldering from the bottom without pads would be tricky at best and likely unreliable. I suspect that wave soldering would also tend to be unreliable without pads.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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