I hereby certify that I am not simply asking someone else to design a footprint for me.
I’m getting queried by the fab about the 0201 paste aperture. I’ve used this footprint before but had some tombstone issues. Now I’m wondering if there’s an issue within the library. I don’t have the IPC or other standards but from some quick searches it seems there’s no consensus on the matter - some say it should have smaller aperture than the copper exposed, others say they should match.
It all seems to depend on stencil thickness too, which doesn’t appear to be consistently discussed in conjunction with aperture size.
Does anyone know the best way to resolve this, perhaps with the librarians? Is this the sort of thing to raise on Gitlab?
It’s beyond the scope of KiCad application or libraries to know the optimal aperture for specific situation. The libraries (the generic footprints like 0201) are already made according to industry standards. I suggest you look into the datasheet of the actual part you (they) use and create a footprint according to that. 0201 is so small that small absolute changes are large relatively, and the exact dimensions are the more important the smaller the part is.
Thanks for your reply. I’m not looking for specific situations. I’m interested in the general solution. The fact that more than one of us is experiencing queries from fabs means I think it’s worth asking about the KiCad implementation. The linked topic which I included in my OP shows that the difference between paste/stencil aperture and soldermask aperture only happens at 0201 and below. I am reassured that industry standards are the basis for the KiCad libraries but it would be helpful if the specifics can be confirmed for this apparent difference. E.g. confirm that IPC standard X guidance recommends Y% paste to pad area for stencils of Z thickness in 0201 passives, or other ratios, or something.
Don’t know much about the specifics of the aperture sizes but have used the Kicad default footprints down to 0201 sizes and they have never been a problem. A lot depends also on how good the production lines pasting is when you get down to that size, which is why I avoid them if I can.
I have asked. I was expecting more consensus or discussion than I have found so far in (an admittedly brief look at) public forums, ideally referring to a standard. Although I appreciate such a standard would be a generalisation. For example, Worthington Assembly publish an “ideal 0201" footprint dimension but it doesn’t look anything like the KiCad library. I have no doubt that the KiCad library is referenced from a standard but when you add in the variables of stencil thickness, aspect ratio and ratio of pad area, things seem less clear.
Do you really need to use 0201 size components?
As part of our business is PCB assembly we see a lot of boards that come through from 3rd party designers with 0402 components on that could quite easily be 0603 or even 0805. Using the biggest size possible (we use 0805 as standard) improves reliability on production and ease of inspection.
I honestly try not to but this is a dense arrangement of passives around an IC which has a strong vendor recommendation to keep distances short or risk significantly undermining the IC’s performance.
IMO this implies that it’s going to be process-dependent, which precludes a standard one-size-fits-all solution. I’d frankly tailor the paste aperture to the needs of the PCBA depending on their unique process configuration.
KiCad libraries are intended to be a good first start and are generally targeted to “just work” for the 90% user as far as possible.
Generally, this means that the components you find in the stock libraries are IPC Density Level B (medium) and designed for roughly 0.1 to 0.15mm stencil thicknesses. 0201s and smaller are specialist components that often require thinner stencils and finer paste (level 4, say). These are not 90% user parts.
When working with specialist parts, for good results you must talk to your board manufacturer and assembler and ask them what they want to do. No one library can get it right for everyone, as each manufacturer will have their own suggestions based on the dozens of parameters that affect these parts at the time you place the order.
The above issue (thanks cpresser!) and the links therein explain what the thinking was here 8 years ago, but that was based on a 25-year old PDF based on a single lab’s equipment, and things may have moved on. The venerable IPC SM-782A ends at 0402, and I don’t know that there is a more modern equivalent to look at. “Best practice” for PCB manufacture is a field full of hearsay and a horrible mishmash of guesswork, assumptions and bad and/or old documents.
So if you have a more up-to-date and verifiably sensible piece of guidance from active production, please do let us know!
For example, it could be that the “most done thing” these days for tiny parts is to just copy the copper size and let the manufacturer fiddle with the apertures in their CAM tooling rather than try to preempt them.
@johnbeard Thanks for confirming what the bases of the current library are, or what they are likely to be. I agree with you and others in this thread that a fab / manufacturer will have opinion on it - Perfect 0201 Footprint — Worthington Assembly Inc. is a somewhat frustrating example in that they only share the part they want their customers to know - the footprint (which does look quite different in proportion to the KiCad one but I don’t infer too much from that in isolation). And then they keep secret (as per their prerogative) the other key parameters around stencil, paste and application procedure.
I have asked my fab, who are making the stencil, what they recommend but they haven’t answered yet. In the meantime, I’ll stick with as-is until an evidenced alternative is suggested. I have hand assembled around 10 boards with approx 30 qty 0201 components each using this footprint. At one stage I had some tombstoning issues and it is obviously hard to populate the components but I have wondered whether I could get better adhesion of the part to the pad when placing if there were more paste on it. I use SMD291SNL10T5 (the 10 stands for the volume in the syringe, so if you want different quantities, look for alternative values in that field) with a 0.1mm stencil normally. I hope that helps others who might read this while making their own decisions in future. We definitely would be enriched by more discussion of these combined footprint/stencil/paste/process topics for finer parts.