Solder Mask Expansion Query

[retrosolutions]

I am finalising a PCB for a production run instead of hand soldering and have a question:

If i select a footprint for a SMD resistor from the defaults provided in kicad i get something like this.

However, the footprint i am using which if i remebder correctly i brought across from EasyEDA has a defined solder mask expansion

So the question is should it or should it not be there?

[fred4u]

If the Expansion value is set to 0, KiCad will use default values for netclass.
Footprint can also have individual value defined, which overrides these defaults.

[paulvdh]

It’s a bit complicated. For most “regular” work it’s probably best to use not solder mask expansion. At least some PCB manufacturers apply their own solder mask expansion settings for making the solder mask based on their own “experience”. And they may or may not tell you this in their settings and capabilities. The amount of solder deposited on a pad also depends on the thickness of the solder stencil. For very fine pitch parts, you may need a thinner solder stencil, and you can (partially) compensate for this by using a larger mask expansion for the pads that do need more solder.

Because it’s hard to figure out what your PCB manufacturer does exactly with your stencil, it’s difficult to make predictions. If you order solder stencils from different sources, the hole sizes can vary. (and stencil thickness, material, quality, etc) But stencils are not very expensive. The easiest path is probably to just try it out, and make a modification if it does not work out very well (or in extreme cases order a new stencil).

If it was my PCB, I would replace all the easyeda footprints with standard KiCad footprints, because:

1. I know the KiCad footprint libraries are quite good, and the easyeda libraries are unknown to me.
2. The rounded corners have some advantages (also an IPC recommendation).
3. Your PCB will have more uniform measurements, sizes, which makes it easier to compare solder-ability and such from different projects.

If you’ve made a bunch of projects, ordered stencils for them too and made PCB’s then you gain some experience and know what works for you. Working form a uniform set of libraries for your parts helps with getting more consistent (and thus predictable) results.

[Piotr]

@retrosolutions

So the question is should it or should it not be there?

My opinion.
Solder mask expansion depends on technology accuracy so generally should be the same for the whole PCB. So the best would be to have it set to 0 in all (standard) footprints and to one value for the PCB. I set it to 0.075mm for PCB.
In fine pitch footprints (below 0.5mm raster) I set mask expansion in footprint definition.

For many years I had set solder paste clearance to 0 and thought it is used that way.
But when I used KiCad rounded pads I got info from my manufacturer that he has no software tool to modify them as needed so I got from him info what I should set for it. But a day later when I had it done and send him corrected file he said that he got the right tool so he did what he wanted himself.
I think it is the best way as it is he who knows how to modify stencil openings depending on stencil he orders and it is he who will assemble PCB.