solder paste vs. through-hole ?

Richard Chávez rjchavezb at
Sat Jul 14 13:12:02 EDT 2012


I have used several PCB design CADs and I have never seen solder paste on
through-hole pads.

The reason of this is that the solder paste would end up filling the holes
after reflow making it difficult to place the THT components as you
mentioned in your analysis.

About the DNP SMT components, people let this parts with solder paste
basically because if you ever decide to place them in future productions
you don't have to make a new stencil.

So, my suggestion is NEVER place solder paste on THT components and ALWAYS
use solder paste on SMT components pads.


Richard Chavez.

2012/7/13 Werner Almesberger <werner at>

> When looking at the M1r4 gerbers, I noticed that all the copper
> rings around through-hole components were bare metal (copper
> plus - implicitly - surface finish), without solder paste on
> them.
> This surprised me a bit because it had never noticed seeing
> no solder paste on such areas. But then, I may just have missed
> it.
> The question of whether we should put solder paste on copper
> used for through-hole components matters not only for M1r4 but
> also in general for our footprint library since footprint
> definitions also specify whether (and where) to place solder
> paste.
> KiCad lets one edit pad characteristics manually, including
> addition or removal of solder paste, but that's dirty work and
> mistakes are easy to overlook. (When working on the Front/Back
> layers, pads looks the same with or without solder paste. You
> can check the solder paste by explicitly selecting the SoldP_*
> layers.)
> I thought a bit about possible benefits and problems of putting
> solder paste on through-hole pins and came up with the following
> list:
> a) may improve solderability in later process steps,
> b) may conflict with later solderability,
> c) may protect pads,
> d) increased consumption of solder paste,
> e) may increase risk of solder spilling or plugging,
> f) may affect long-term solderability.
> When mixing SMT and through-hole components, the fabrication
> process should be roughly like this:
> 1) start with the bare PCB,
> 2) apply solder paste,
> 3) place the SMT components,
> 4) heat the PCB to melt the solder paste, then let it cool down,
> 5) place the through-hole components,
> 6) solder the through-hole components (either manually or with
>    some type of wave soldering)
> Now, a) and b) would affect what happens at step 6: if the
> solder from the solder paste (solid after step 4) is compatible
> with the solder used for the through-hole components, this
> should improve solderability. If not, it may decrease
> solderability or produce lower quality solder joints.
> In general, I would assume that the materials are chosen such
> that they're compatible.
> Since copper oxidizes when exposed to air and the oxide is very
> difficult to solder, industrially produced PCBs have a surface
> finish that protects the copper.
> The characteristics of common surface finishes can vary quite a
> bit. Here is a nice overview:
> HASL (tin) and ENIG (gold) are the most common choices but we
> may also want to consider IAg (silver) and OSP (organic).
> The characteristics of HASL and ENIG shouldn't be affected by
> the SMT soldering step (4), but an organic protective would
> degrade. Silver may have similar issues.
> If the copper is covered by solder paste, the solder would
> therefore take the role of the surface protectant when OSP is
> used. (c)
> I'm not sure if the increased consumption of solder paste (d) is
> much of a concern. I also don't know if there is a real-life
> risk of solder from the solder paste on through-hole rings
> getting in the way, e.g., by filling holes. (e)
> I asked on #qi-hardware and Joerg suggested to always put solder
> paste, to improve solderability. Joachim added that he prefers
> DNP parts and such to just have gold, without solder on them.
> In fact, if solder from the solder paste ages less gracefully
> than, say, ENIG, the pads of DNP components could become
> difficult to solder with time. Again, I'm not sure if this is an
> issue in real life. In general, the effect in this case
> shouldn't be worse than for any other kind of rework.
> Does the above analysis sound reasonable so far ? Are there
> other issues to consider ?
> I wonder if we can come up with a common set of rules for
> solder-pasting the copper for pins of through-hole components.
> Choices would include:
> - always,
> - never,
> - provide footprints with and without solder paste, leaving the
>   choice to
>   - process requirements, or
>   - user preferences.
> If the above analysis is correct, then where would be a strong
> case for always using solder paste if OSP is involved, and all
> other scenarios would tend to slightly favour applying solder
> paste. If this is true, then we could consider an "always use
> solder paste" rule and avoid duplicating a lot of footprints.
> - Werner
> _______________________________________________
> Qi Hardware Discussion List
> Mail to list (members only): discussion at
> Subscribe or Unsubscribe:
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <>

More information about the discussion mailing list