Im very new here and just had a quick question to ask for anybody who may be able to help!
Im working with a large BGA package and I have vias in between pads. For the end result I would like to have a few select pads tented on the top layer as to not bridge to the BGA pads when assembling, but have those same select vias “un-tented” on the bottom layer as I am making an adaptive flex pcb to solder to those vias.
I have tried a few different options such as plated through hole, but im not sure thats something that can be tented on one side only. Any help would be appreciated! Thank you!
KiCad has existed for quite some years (I think 20+) and as many open source projects development was quite slow in the beginning. Since around 2015 or thereabouts the development pace has been increasing steadily. Almost all the “Big” things have been implemented (“Big” things missing are an integrated autorouter and database based parts management), but there are still a bunch of “missing” and less-developed “small issues” in KiCad.
For via’s you currently have a choice during Gerber generation whether you want them tented or not.
For THT pads you have more choice. You can turn individual layers on or off. So you can for example create a hole in the bottom soldermask layer, but not in the top soldermask and the top layer will be tented.
For about one or two years KiCad has a limited pad stack in which pads of a via can be turned on or off for coper layers. A full pad stack in which the size of the pads can also be set individually is being expected for KiCad V7, maybe later. So that would be 2023 or so.
There is also a significant other difference between pads and via’s. Vials can just be placed anywhere on the PCB, but pads have to be part of a footprint, and connections to pads in footprints have to be part of the schematic.
When considering these limitations, it can be done, but it’s a workaround and a bit of a nuisance for the time being. The workflow would be:
Create a footprint library (Footprints like to be stored in a library very much).
Create a footprint in it for a single THT pad.
Create a schematic symbol for it. (Similar to a one pin connector, test pin, or someting like that).
Add these symbols to the schematic wherever you need them.
During the normal Schematic Editor / Tools / Update PCB from Schematic F8 the footprints will be added to the PCB.
from my EDA philosophy, I have to disprove of all the options suggested by paulvdh. In my opinion, the attributes of vias, is purely a layout decision and has nothing to do with the schematic and the attributes of vias, belong to the via, and are not an independent footprint. Also I don’t like doing anything in gerber. gerber IMO is the output format.
Therefore, what I use, and what might possibly suit your own layout philosophy better is the following.
Design your board with regular tented vias throughout.
Now address all the vias for which you need mask openings and copy paste dedicated filled circles in the B.Mask or F.Mask layers (or both) according exactly to your aperture needs.
This sounds a little clumsy but is actually incredibly quick. Just prepare the Mask layout circle once, and then quickly Crtl-V-click it to all the vias where you really need it.
Whether vias can and will be tented depends on the PCB manufacturer. Nearly every manufacturer will run automated edits when importing your data to adapt it to their process capabilities, removing solder mask from vias is somewhat common. Talk to your board house if you need tenting, the limits depend on their solder mask process, some manufacturer don’t support tenting at all and will remove the solder mask from every via, some will tent vias up to a certain size. Some manufacturers might charge extra fees.
You can tell kicad to remove vias from the solder mask when exporting the design to gerber files:
You can achieve your desired result by running the gerber export for all layers except one of the mask layers with one setting, toggle the setting and export the other mask layer.
