4
\$\begingroup\$

I have a design with huge push buttons (with 6 TH holes.)

There's a few of them so they do take up quite a bit of space mechanically from the top.

I was thinking of placing the majority of the SMT part on the other side (same side where the TH would be soldered.) This way I could place the SMT directly underneath the buttons and with some clearance to its pins.

I was told that this is a bad idea from a manufacturing point of view since there are two processes: one reflow for the SMT and then a solder bath for the pins. The solder bath may cause problems for the SMT.

For this prototype space is not really an issue and so I will take his advice and lay out the SMTs on the same side. But for the next revision, is this something I can consider? I suspect I won't have this much space next time around.

\$\endgroup\$
2
  • \$\begingroup\$ The question is not clear. Post a picture. \$\endgroup\$ Apr 21, 2021 at 10:21
  • \$\begingroup\$ @EnricoMigliore: The question is perfectly clear. This is a common concern when using mixed SMT and through hole parts. \$\endgroup\$
    – JRE
    Apr 21, 2021 at 10:36

2 Answers 2

3
\$\begingroup\$

With only 6 TH parts, your supplier will propose you 2 solutions:

  1. Manual soldering of those 6 TH components

  2. Automatic selective soldering of those 6 TH components

Nobody will use wave soldering for only 6 TH parts, unless you have to assemble more than 10k boards per lot.


There's actually a third method called "pot soldering" for small volume PCB assembly.

SMT parts placed on the bottom must be masked with solder wave pallets.

enter image description here


If you have more than 10k boards to assemble, your supplier will call you in order to define the best soldering strategy.


You can solder SMT parts with a solder wave. They do it all the time when they have to assemble more than 100k boards per month.

Just one process: a wave that solders SMT and THT parts at once.

White goods PCBA are assembled this way especially in China.


Not all SMT packages though can be wave soldered.

That means that the PCB designer must carefully select the right SMT package.

BGAs for example can't be wave soldered.


The footprint of SMT packages for wave soldering must be carefully designed.

See the red circles in the picture:

enter image description here

\$\endgroup\$
3
  • \$\begingroup\$ Each TH part has 6 pins. There are about 7 of them per board. So 42 TH pins per pcb. \$\endgroup\$
    – Hasman404
    Apr 21, 2021 at 14:37
  • \$\begingroup\$ Got it. I reviewed my answer. \$\endgroup\$ Apr 21, 2021 at 14:49
  • \$\begingroup\$ 100k can be somewhat of an exaggeration. If you only have small chip components (0603 chips, SOT-23 etc), it's not much of a challenge for the assembler to do this. As soon as you have something like the SOIC parts in your image, it becomes much more difficult. WRT selective wave solder, talking to your assembler during PCB design stage can reduce tears later on. Basically they will want a healthy clearance between exposed pins and neighbouring SMT parts. \$\endgroup\$
    – Barleyman
    Apr 27, 2022 at 10:00
2
\$\begingroup\$

In general you can't place anything on the solder side in case wave soldering is used (watch Youtube videos of how its done and you'll see why). And wave soldering is the default way to solder through-hole components.

With SMD reflow soldering you can place components on both sides since that process uses an oven. The components are then glued on one side. This makes assembly more expensive too, so it's a last resort when board space is tight.

Various use-cases:

  • You have only through-hole components single-side. Wave soldering is used, relatively cheap assembly process.

  • You have only SMD components single-side. Reflow soldering is used, cheapest assembly process.

  • You have only SMD components but use both sides. Reflow soldering is used, somewhat expensive assembly process.

  • You have a majority of SMD components but some through-hole. Reflow soldering is used and through-hole components are soldered by hand which is somewhat expensive.

    In some cases certain through-hole components can be used during reflow, in which case they are called "through-hole reflow" (THR) or "pin in paste". This is somewhat new still and you need to check with the assembly contractor before designing in such components.

  • You have a majority of through-hole components but some SMD. Again likely hand soldering, though the contractor might have some tricks to combine the two, check with them before designing.

\$\endgroup\$
5
  • 1
    \$\begingroup\$ The way I've seen TH and SMD combined was SMD on the top side reflowed, then SMD on the bottom side glued in place, TH parts placed, wave solder the bottom side. \$\endgroup\$
    – JRE
    Apr 21, 2021 at 10:55
  • \$\begingroup\$ This is incorrect, you very much can wave solder SMT parts. But you must use \$\endgroup\$
    – Barleyman
    Apr 27, 2022 at 9:40
  • \$\begingroup\$ But not just any old SMT component and willy-nilly. You must use special (larger) pads and gaps and be mindful of solder migration and solder wave shadows. Small 2-pin chip components are safe enough as well as SOT-23 style packages. They should be arranged perpendicular to the travel of the solder wave and there should be enough gap in the direction of travel to allow the wave to "reset". TH pins especially need a healthy gap to the nearest SMT pad. \$\endgroup\$
    – Barleyman
    Apr 27, 2022 at 9:46
  • \$\begingroup\$ @Barleyman What would be the point of that? Wave soldering just for the heck of it doesn't fill a purpose. It seems it would only be useful in some very special scenario where you have the majority of components as through-hole, you need to mix in a few simple SMD and for some reason need to place those on the solder side. That's a strange, highly specialized case. \$\endgroup\$
    – Lundin
    Apr 27, 2022 at 9:51
  • \$\begingroup\$ Nothing strange about it at all. You can do everything in one go if your chip components can be wave soldered together with the TH parts. Whether or not this makes sense depends on the board complexity and volumes as Enrico explains in his answer. You should really talk to the assembler to figure out the most cost effective way. \$\endgroup\$
    – Barleyman
    Apr 27, 2022 at 9:57

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.