9
\$\begingroup\$

I've routed plenty of through-hole boards, but I have no experience with SMD routing techniques, and even the look of the board feels a bit ‘alien’ to me.

Any tips for placing/routing prototype PCBs with SMD components, for someone who can already route with through-hole components? I'll be hand-soldering as well, so I'm sticking to SOIC, 1206, and the like.

Ideally, I'd like tips on how to place for reasonable density, whether to use one or both sides of the board for components, etc.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ There is, of course, David Jones' PCB Design Tutorial, which I never before read in the context of SMD. Going through it now, and Enlightenment Shall Be Had! \$\endgroup\$ – Alexios Jan 11 '12 at 17:31
  • 2
    \$\begingroup\$ IMHO the most important thing to do (after getting a good soldering station) is to pick up a stereo microscope. They're fairly cheap off eBay. Not only is it easier to see what you're doing, they significantly reduce eye strain. \$\endgroup\$ – darron Jan 12 '12 at 0:09
8
\$\begingroup\$

Let me start with your last question, I would highly recommend NOT soldering components on both sides unless you have a really good reason to. I have made a few boards with double sided soldering and it became more of a pain then anything.

As for the routing itself, my answer here might help you out some, but I will elaborate some for your specific circumstances.

Part density can become an issue when you are hand soldering, but it is difficult to give exact numbers as everyone will be different with how comfortable they will be soldering and what parts it is. As a minimum you will probably need 2 soldering iron tips width apart. This will give you the room to get the iron in to work on one part while not hitting the other. You might also want to take into account the angle that you like holding your soldering iron at as you won't want to be resting your iron on another IC. If you have a shakier hand then you might want to see how much your hand shakes and space your parts at least as far as the tip of the iron moves as you are shaking.

I would also avoid running traces between legs of SMD components. A lot of people will do it just because it passes DRC, but if you are hand soldering with no soldermask, it becomes very easy to accidentally bridge to the trace.

It is also helpful, but not required, to bring your traces out straight from any ICs and then after a little room branch them to the direction they need to go. This will help you line up your IC properly as well as to be able to get the solder in place easily.

And finally, going from through hole to SMD, you will find that many of the tricks that you can use with through hole just wont work with SMD. Things like having no vias because you are using a through whole component to jump to the back side, instead you might have to go back to your schematic and change things around to limit the number of vias used. Also you can usually run traces under through hole items, but this may complicate things more with surface mount.

Overall, just practice and you will pick up tricks just like I am sure you have picked up tricks with through hole.

\$\endgroup\$
8
  • 4
    \$\begingroup\$ I agree, but want to point out that some of what Kellenjb objects to is only if you don't have a solder mask for some reason. Personally I think life is too short for hasseling with boards without solder mask, but that's your business. With solder mask you don't have to worry about traces between IC pads, under parts, or leaving pads at strange angles as long as the DRC passes. SMD routing is generally easier because the parts only clutter up one layer, not all layers like thru hole. Also, sticking to 1206 is overkill and will limit part availability. Don't worry about 0805 packages. \$\endgroup\$ – Olin Lathrop Jan 11 '12 at 17:00
  • \$\begingroup\$ @OlinLathrop Yes very good points, I agree with all of them, but I am assuming he will be hand etching or milling with no solder mask. For any boards I make personally, I always get a solder mask, but I know not everyone cares to pay for it. \$\endgroup\$ – Kellenjb Jan 11 '12 at 17:13
  • \$\begingroup\$ Thanks for the answer! I absolutely must have soldermasks for all the reasons that soldermasks are used, and it'd be great to be able to go through SOIC pads, but I don't seem to have enough clearance with 8mil traces (the Olimex minimum). Also, I worry about soldermask alignment tolerances at those scales. \$\endgroup\$ – Alexios Jan 11 '12 at 17:14
  • 1
    \$\begingroup\$ @Alexios Ah, well my comments still hold true, but you can ease up on the restrictions where I worry about bridges. \$\endgroup\$ – Kellenjb Jan 11 '12 at 17:18
  • \$\begingroup\$ @Kellenjb Agreed! Though I worry about bridges too, and with me having little SMD soldering experience, I'd like to avoid as many pitfalls as I can. Can't be too careful, right? \$\endgroup\$ – Alexios Jan 11 '12 at 17:20

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.