Is the solder paste file necessary for through-hole components?

Question

I have designed a PCB. There are only through hole components on the top layer, and only surface mount components on the bottom layer.

Is TOP SOLDER PASTE file necessary to send to the PCB fabricator, the same as bottom solder paste, or is it enough to only send the bottom solder paste file, since I only have SMD components on the bottom?

Also please explain, in general, in which situations do we have to send SOLDER PASTE file to the fabricator?

Thank you very much for your time.

Answer 1

Paste layers are used to fabric stencils for screen printing solder paste onto the boards.

Both the fabrication of a stencil and using it are distinct tasks you have to pay for. While some PCB manufacturers may also offer stencil manufacture, it is a distinct service. Further, to fabricate a useful stencil you need to specify the material, dimensions and in theory mechanical interface with the stencil printing machine.

So no, you don't need to include a paste layer when ordering PC boards.

And when having boards assembled, you would not include a paste layer for any side of the board that you did not want to print with solder paste - paying to run a blank piece of stainless steel through a stencil production line and then paying someone to flip the board to a second side in the paste printer only to squeegee around solder paste while depositing none of it wouldn't really make sense ;-)

For through hole components you need a different fabrication process anyway, such as wave soldering or selective soldering. Talk to your assembly house (ie, the vendor who populates the boards, which is not necessarily the one who manufacturers the PCBs) about what services they can provide, what materials those require from you, and what limitations such process imposes on your design.

Answer 2

Empty paste stencils are just blank, so generally the fabrication drawing/file would state that there are is no requirement for a (topside) solder paste stencil.

It's generally not a good idea to use a solder mask as a stencil mask, for several reasons:

1. You may put solder where you don't want any, such as test points, wire entry points, etc.
2. Paste stencil size are in general not the same as solder mask sizes (they are usually smaller). In cases of thermal pads the stencil area is generally broken up to prevent scooping of the paste during application, and to optimize the amount (most manufacturers provide this information in their mechanical drawing specs).
3. As the designer, it's your responsibility, not the fabricator's, to provide the fabrication documents and standards. The fabricator can be responsible for manufacturing the final stencil and frame to fit their process flow.
   4. If you're talking about sending the actual solder paste (not the stencil mask) it is unusual for the fabricator to request it, unless it's some kind of specialized mix. Most pastes require refrigeration to prevent degradation and are almost always shipped in cold packs (if from a reputable supplier). If it's a common formulation, a request like that would raise flags for me.