Tht + smd

[JohnsonMiller]

I am not an expert at assembly topics, wondering how is the assembly process when THT parts are existing along with SMD parts? A board like iMX6 OpenRex SBC
Board for SMD parts needs to pass through the oven two times, one pass for parts placed on top and second for the bottom, to be cooked two times indeed!
What about THT parts? Hand soldering does not make sense. Is it a robot for sodering?!
And reflow soldering can damage or relocate SMD parts on the bottom side.
Any suggestion?

[WhoKnewKnows]

There are a variety of strategies. It depends on the construction of the PCBA.

A typical scenario is to have SMT components on top and bottom, with TH components inserted on the top side, so TH leads soldered on the bottom. In this scenario, Top SMT components can be placed on solder paste and adhesive, then through the reflow oven.

If the SMT stuff on the bottom side is chip components only, they can be placed in adhesive only, then TH components loaded, then a trip through the wave solder can solder the bottom SMT and TH components simultaneously. Then wash, then 2nd operations, then testing, and so on.

That's just one way to do it.

[qdrives]

Depending on components, layout, quantity TH parts, component options (PIP/THR), quantity products and labor cost, you can do Pin-in-Paste (Through Hole Reflow) wave soldering, selective wave, robot soldering and manual soldering.
I have done many designs that have SMD components on both side and through hole on the top (even one that has through hole on both sides). Some were hand soldered and others were wave soldered.
The design I am currently working on is still a bit unknown, but definitely not wave solder (it could be selective wave).

[robertferanec]

I have see some boards soldered in wave (with no smt on bottom) and I have seen boards with TH components soldered by hand. I have not seen how it it is done with smt on bottom with many through hole components or for very high quantity production with through holes.

[qdrives]

robertferanec what is high quantity? The boards that I designed with SMD wave soldered are produced in quantities of about 1000/year.
On the bottom are resistors, capacitors and discrete components (0603, 1206 and SOT23). No IC. Orientation is important, as is spacing (shadow effect). Special footprint with larger pads.
The components are only glued. Soldering comes from the wave.
Fot the TH components - see part of the board in the photo. I do not have a photo of the bottom, sorry.

[JohnsonMiller]

Thank you guys for your valuable comments,
qdrives , regarding this statement:" The components are only glued. Soldering comes from the wave."
Do we need to supply data for a special stencil to apply glue? What about footprints, do we need to consider glue in component mechanicals? Like adding a special mechanical layer, or adding an opening for glue. Applying glue is probably like applying the paste, correct?

[WhoKnewKnows]

Altium refers to this as glue points or glue dots if you care to have a look at the Altium web site. In the PCB document, there's a mechanical layer pair that's just for specifying glue for components. It can be applied by a stencil, or dispensed by an XY robot (slower, but saves the cost of a stencil).

[qdrives]

JohnsonMiller I wanted to put the glue data into my design, but in all cases, the assembly company wanted to do it themselves.

As far as I know, glue can be added like a stencil, but probably more often applied with dispensing as this allows both stencil for solder paste and glue on the same side (for selective wave and two sided assembly). They may also want to do it themselves because of the production variations (similar to below side note on paste mask)

My experiences with wave soldering SMD components:
- Special pad sizes (bigger)
- Use 0603 or bigger
- SOT23 3 pin is ok
- SC88 (SOT232 5 or 6 pins) has a short on average 5% of the parts (not boards, but parts). So do not use it.
- Have the pads to the side compared to the wave.
- Note the board direction for wave soldering. This is also required if TH connectors need solder thieves (>= 2mm pitch)


As a side note, most engineers also just have the paste mask identical to the pad size and do not specify the stencil thickness nor the solder paste. I thick even very few know there are different stencil thicknesses, and those that know, know it because they either purchased them or looked at them for purchase.
However, stencil thickness, shape (smaller, larger or broken into smaller pieces) and paste type all have influence on the production quality.
My current design is the first I do where these considerations are taken more into account. Mostly because one of the components is very critical about it.
By putting the details into my design, changing EMS should not result in a different product quality result.