5
\$\begingroup\$

I'm making my first two layer PCB and have am unsure of whether it's ok to connect a trace to a pad on the top layer (if the pad is on the bottom layer, that is). Here's a picture to show what I'm talking about:

enter image description here

Is the method shown on the right allowed?

\$\endgroup\$
  • 3
    \$\begingroup\$ You say your pad is on the bottom layer, but yet what you show is a thru hole pad that is on all layers. \$\endgroup\$ – Olin Lathrop Jan 19 '12 at 22:32
  • \$\begingroup\$ I'm glad you pointed this out because earlier today I was trying to determine whether the pads were on the top or bottom layer and never did figure it out :-) I guess that, along with the other answers given, answers my question. Kind of a different question, but is a pad on all layers what is typically used instead of just having the pad on the bottom layer? \$\endgroup\$ – Nate Jan 20 '12 at 0:33
  • 1
    \$\begingroup\$ Typically the top side of the board is considered the component side, so pads would be on the top layer only. You can put components on the bottom, but that adds manufacturing complexity and cost, so you only do it when small size is a high priority. Some parts that take mechanical stress may be thru hole, in which case the pads are on all layers. \$\endgroup\$ – Olin Lathrop Jan 20 '12 at 13:33
  • 1
    \$\begingroup\$ If you are going to have your holes plated through, some vendors will insist on having a pad on both sides. The "capture" pad improves reliability by preventing the plated-on copper peeling away from the hole walls, as I understand it. \$\endgroup\$ – The Photon Jan 20 '12 at 16:58
8
\$\begingroup\$

Yes, that is fine. As long as its a plated through-hole (PTH), copper touches both top and bottom layers.

Obviously, if that is a surface mount pad you can only connect it to the same side as the pad itself.

\$\endgroup\$
  • 5
    \$\begingroup\$ It is also OK without PTH if you are going to solder the top and bottom. However, I wouldn't recommend this as it has come back to bite me a few times when I leave a header off or don't solder both sides or whatever might happen. \$\endgroup\$ – Kellenjb Jan 19 '12 at 21:02
4
\$\begingroup\$

It's fine, and it's also a good practice because you save an useless vias, so pads and holes that in addition would have to be made conductive, with a wire or with a metal fill.

So when you design your circuit, besides trying to use in the wisest way your two layers, try to use as much as possible the holes for the pins of the components, to pass traces from one layer to the other.

Plus, if the design is complicated, you can get a hint from the Manhattan tecnique, that is trying to split the traces in vertical and horizontal, and use one layer for one type and the other for the other one, as much as possible...so you have the less chance to have crossing lines in one layer.

The counterpart is that in that case you have to solder also the upper pad of the board; if you pay attention, there's no problem but you have to be more careful to avoid damaging the component. And also, if you find a mistake, the desoldering process becomes more complicated too.

\$\endgroup\$
3
\$\begingroup\$

If it's a through hole pad (which it looks like) then it's on all layers, so top/bottom/middle are all acceptable.

If it were a surface mount pad on the top layer then you obviously can't connect a trace running on the bottom layer directly to it, you would need a via to switch layers.

Just in case you are planning to etch your own board, you need to remember that your pads will not be PTH (plated through hole) so although you will have an annular ring on both top and bottom layers, they will not be electrically connected.
In these cases people often use the lead of whatever part goes ito the pad, and solder it both on the bottom and the top to connect the two.

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

Others already have indicated that for through hole pads the pad is on both top and bottom layer, so you can connect the trace on any layer you like. On some components like PTH electrolytic capacitors you can't solder on the top side, and if the holes aren't PTH (Plated Through Hole, like on a DIY board) I make the connection on the bottom. Just in case the solder won't flow along the wire and to the top pad.

By default all pads on the different layers will have the same shape and size, but your EDA software should allow you to use different pads for different layers. Typically I would use smaller pads for inner layers, as they don't have to be soldered and smaller pads make routing easier.

\$\endgroup\$
  • \$\begingroup\$ Using a via can sometimes make rework/mods easier, if the bottom-side trace between the via and the pad is more accessible than the trace would be otherwise. Further, if the part gets replaced so many times that the pad comes off the board and tries to pull a trace with it, having a via right next to the pad can facilitate repair. Of course, one wouldn't expect such situations to arise with a production board (a production board where one part was replaced that much should typically be junked) but sometimes prototypes can require parts to be swapped out dozens of times. \$\endgroup\$ – supercat Apr 9 '12 at 15:10
0
\$\begingroup\$

I think it depends. If you component is going to be on the top layer, and you have no pad on the bottom layer, then you may not be able to solder the component on, at least if the component is seated close to the board (in the usual way), as in below, where an electrolytic cap is supposed to be soldered to the pad.

enter image description here

If the component is small, or needs to have long leads then this isn't a problem. Also if the component is seated on the bottom side, then top pads are not a problem, and even good: since placing components on the bottom side with bottom pads creates the same kind of problems as soldering components on the top side to top pads.

\$\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.