Werner,

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.

Regards,

Richard Chavez.

2012/7/13 Werner Almesberger <werner@almesberger.net>
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:
http://www.trianglecircuits.com/lead-free-finishes.html

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@lists.en.qi-hardware.com
Subscribe or Unsubscribe: http://lists.en.qi-hardware.com/mailman/listinfo/discussion