I found that I can disable these errors through a checkbox in the footprint’s “Clearance and override settings”. However, I am not sure if this is the type of error that I can just ignore, without resulting in a faulty PCB. I plan to upload the Gerber/Drill/BOM/CPL files to one of these online services and have them do the PCB manufacturing and assembly.
My question is, can I simply ignore this error without issue? And if not, what kind of changes to do I need to make to the KiCAD settings or to the footprint itself?
Any assistance on this matter is highly appreciated
From your description I’m not sure if you have understood the issue correctly. Solder bridge is always unintended unless you manually solder two separate copper features together, jumping over the gap with tin on purpose. Maskless areas which leave the gap between two nets without mask are usually either unintended or necessary only because the manufacturer doesn’t make very narrow mask strip.
Bridge and bridging are difficult words here because they can mean almost opposite things. It can mean either the narrow mask strip which bridges two larger mask areas together, or the area without mask where two copper features near each other are left without protection.
Thanks for the tip! Reducing the soldermask expansion for the fine-pitched parts from 0.102 to 0.075mm results in mask being added between the pads. I am not sure if the solder masks are mandatory for this package (because else why would someone design the footprint this way…), but it does solve the errors. I will check with the fab house if they can support this setting
For (in my opinion) typical requirements of 3 mils soldermask expansion and 3 mils minimum soldermask width you are able to have soldermask between pads if distance between them is 9 mils or more. 9 mils = 0.2286mm. For parts with 0.5mm pitch you have a chance to have enough distance between pads. For parts with 0.4mm pitch you will not get bigger distance than 0.2mm what is not enough. In such case you use single long openings in mask for the whole pad rows. The effect of soldermask apertures bridging have the effect very close to intentionally placed common openings for pad rows.
Thank a lot for the recommendations. I guess I now got a better understanding of it.
Unfortunately I cannot achieve 3 mils for both the aperture and solder mask.
That is because the distance between the pads is 0.2 mm (7.874 mills).
Setting the expansion to 3 mils leaves only 1.87 mils for the mask width.
I now set the expansion to 0.05mm (~2 mills (*EDITED*)), leaving a mask with width of 0.1mm (~3.874mils).
While this expansion is below the 3mils you recommended, the fab house states to support expansions of >= 0.038mm, and mask bridge of >= 0.1mm. So I guess this configuration now fulfils the requirements.
The deviation in calculations is too large to be the result of rounding errors.
So they accept 0.4mm pitch with 0.22mm pads.
The problem source is the precision of mask being placed at PCB. If you use 0.05mm expansion and then mask is shifted by 0.075mm you will get mask on one pad edge. The effect will be that stencil will be not able to fit tightly to the pad and paste will be pushed around pad what then will result with short circuit.
If there is such risk the better is to not have mask between pads.
In past (10+ years ago) I was using single big opening. Recently I was told that I can go below 3/3mils specification but I reduced both (more expansion and less width).
