0
\$\begingroup\$

I currently have a 2 layer FR4 board that is basically a microcontroller with a motor attached to it. There are some discrete switches and connectors as well.

Most of the components are SMT components (0805 being the smallest). There are some through hole LEDs and connectors.

For a single layer (one side) board would I have to replace my SMT components to through hole ?

For a single layer (one side) board would a decent board house still be able to do 10 mil traces or are there new rules for single layer boards ? ( I understand that I should contact the board house directly to find out their capabilities)

Any other useful gotchas (or questions I have failed to ask) would be appreciated from your own experience when doing a conversio, design or increasing manufacturing yield.

\$\endgroup\$
  • 1
    \$\begingroup\$ If you're trying to keep costs down, like you said in your earlier question, then using just one place and solder operation is likely cheaper than two. So you should prefer either all SMD, or all through-hole, rather than mixed. \$\endgroup\$ – The Photon Dec 24 '16 at 19:07
  • \$\begingroup\$ Depends if you are "having it made" or hand-soldering it - if you are assembling it yourself there's little penalty for mixing (indeed, that was the way some SMDs first started being common in the market - extra components on the "solder side" of through hole boards.) Or it could be made except for the through-hole parts and those added yourself later. \$\endgroup\$ – Ecnerwal Dec 24 '16 at 19:13
  • \$\begingroup\$ @ThePhoton good point. \$\endgroup\$ – efox29 Dec 24 '16 at 19:30
  • 1
    \$\begingroup\$ For the cheapest single-sided punched boards, 100% test is certainly not standard, so you might want to use relaxed rules to result in higher yield. The best advice I can give is to take apart products which are made in volume and follow the examples. \$\endgroup\$ – Spehro Pefhany Dec 25 '16 at 9:19
  • \$\begingroup\$ @SpehroPefhany Good idea. \$\endgroup\$ – efox29 Dec 26 '16 at 0:18
3
\$\begingroup\$

I've designed around 8 or so single sided mixed SMD/through hole PCBs (most with microcontrollers, one with some radio modules, and a couple with a low speed gate drive).

If you're doing anything that requires a really good ground plane you should probably stick with the two layer board at a minimum. Expect to put a lot of effort into getting your ground planes to be continuous with a single plane of copper. I've heard it said that single sided designs without jumpers are a kind of holy grail for PCB design. The ratsnest on your pcb design tool is actually a very good indicator whether or not your design will be easy to route on one side. Part layout and grounding will be your most difficult challenge with these designs. You'll want to actually trace out the likely path your ground currents will take (or use something like Hyperlynx PI if you have access to that kind of tool).

That said, I've successfully mixed through hole and smd components to give myself a two sided board with one layer of copper (through hole on top, smd on solder side). These board were all milled rather than etched and didn't have any solder mask. In fact, I tried my hardest to only go with single sided boards because the people who operated the milling service I was using were not so great at aligning the two sides (and the through holes weren't plated). I guess that's the price to pay for $0.07 per in^2. If you're going with a standard board house, their two sided rules (trace width, hole size, etc) should apply all the same. From their perspective, a single sided board should be the same as a double sided board unless they're doing something wonky.

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

Assuming low enough speed that this method is acceptable, remember that you can jump over things with through hole components (sometimes leaving the leads longer than stock bend to facilitate that), and that you can (and will often need to) use jumper wires when you hit an otherwise insoluble in one layer solution.

\$\endgroup\$
0
\$\begingroup\$

You can mix through-hole and SMD. Some prototype PCB manufacturers only support SMD, to keep costs down, so make sure to check. The rules for a two-layer vs. four-layer should be similar enough that you won't need to worry unless doing a tricky or complex design.

If the design is relatively simple, not super high-speed, and no RF, the layout should be easy. Be generous with your ground and power lines; a ground plane would be best. Make sure you have a few power decoupling capacitors near the micro. It's handy to try going up-down on one layer, and left-right on the other layer, with your traces. Keep as many traces on one side as you can, which leaves the other free for that big juicy ground plane.

And otherwise, read and study everything you can!

\$\endgroup\$
  • \$\begingroup\$ I think there might have been some confusion with my wording. I edited my question. Sorry! \$\endgroup\$ – efox29 Dec 24 '16 at 18:33
  • \$\begingroup\$ Ah, you only want to use one side, I see. Well, the advice mostly holds the same, you can mix component types just fine. But if you are paying a contract assembly house to do it, they may not be able to or it may cost more. You can do it by hand just fine, start with the SMD. You'll need to pay a bit more attention to routing ground and power traces. Specifically, try not to make any loops with your ground lines, or you can get weird behaviour. Look up "star grounding". And, if routing becomes really challenging, don't be afraid to install some jumper wires on the top. \$\endgroup\$ – Aaron Kondziela Dec 24 '16 at 18:36

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.