What I mean is I want it to be as simple as possible for potential contributors. I don't want to require them to read the IPC-7351 documents.
So from what I understand, C says: Everything at 0.15, except BGA which is 0.25 for <0.3mm, 0.5 for <0.5mm, and then progressive from 0.5mm to 1mm. Right? Since, I believe, we don't have any CGA in our libraries, I say we just don't write it until it happens. On Mon, Sep 15, 2014 at 5:52 PM, Lorenzo Marcantonio < [email protected]> wrote: > On Mon, Sep 15, 2014 at 02:10:39PM -0400, Carl Poirier wrote: > > I want to avoid exceptions as much as possible. Thus, I suggest we put > all > > LGA, CGA and BGA at 0.5. Is QFN also at 0.15? > > Is not an exception thing, it is the rule which is 'proportional', like > annulus size for THT... and also slightly changes with every 7351 revision. > > In B revision (the current published one) the 0.15 applies to chips > smaller than 0603, SODFL and SOTFL, BGA have 1 mm, aluminum cap (and > crystal cans) have 0.5; everything else uses 0.25 > > The newer unpublished C revision (which is the one implemented by all > the current calculators) instead changes *all* the chips, DFN and QFN > (all the 'no-leads' in practice, with or without pullback) to 0.15 and > add the progressive scaling (not all the calculator do this) from 1 to > 0.5 mm (0.5 for balls up to 0.5mm, 0.25 for balls up to 0.3mm). CGA have > bigger allowance (who uses CGA anyway?:P) The official (more or less > since it's unpublished anyway!) nominal courtyard excess for BGA however > is still 0.5. > > However the default for C revision (seems that it will be merged into > the new CM-770) goes from nominal to least... so the 'new defaults' > will be more for people building cellphones than industrial equipment. > Also they change many roundings from 0.05 mm to 0.01 mm. > > For manufacturing yield I still prefer the old B revision tables, > nominal sizes and 0.05 mm rounding. I don't know how is the default > library in kicad parametrized (i.e. how did you calculate the pad sizes? > which clearance and process tolerances?) but for general purpose non-HDI > boards (usually 0.2 or 0.15 clearance) it's easier to use. I'd say that > when you consistently place 0402 parts with 0.1 clearance the least > spacing could be considered. I usually do most of the work with 0.2 > clearance (0.15 costs more :D). When you have to fan out modern BGAs > however > it's usually mandatory the 0.1 clearance (except when you have *really* > a lot of pins to the power plane and you can fan out the remainder on > the signal layer). > > Of course when *you* have to replace the component when necessary it's > wise to leave a bit more of space :P when you do a cellphone who cares, > it's mostly a throw-away board (maybe the gods of reworking can touch > these) > > By the way, current default parametrization for the IPC calculators is > 0.15 clearance (0.2 against thermal slug); rounding is quite > complicated, depending on what you are rounding it goes from 0.01mm to > 0.1mm. > > Also take care that this is only the 'excess courtyard'; the full > courtyard depends on manufacturing process parameters, mainly placement > tolerance (usually ±0.1mm but some processes also use ±0.2 or ±0.05...). > The rule of thumb is to place components so that the courtyards don't > "touch", i.e. with at least 0.05mm between courtyard lines. > > As usual you give the gerbers to the fabricator and he tells you what > has to be changed; last week I had to move stuff from the border due to > the width of the depanelizer blade :P also ceramics near the edges are > prone to cracking and many other things that can't be standardized > anyway. > > PS: you don't gain a lot having a smaller courtyard on QFNs... while the > package is smaller and there are no leads, usually there is a thermal > slug so you have to fan out on the outside! QFPs instead can fan out > (and have routes) even under the body... > > -- > Lorenzo Marcantonio > Logos Srl > > -- > Mailing list: https://launchpad.net/~kicad-lib-committers > Post to : [email protected] > Unsubscribe : https://launchpad.net/~kicad-lib-committers > More help : https://help.launchpad.net/ListHelp >
-- Mailing list: https://launchpad.net/~kicad-lib-committers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-lib-committers More help : https://help.launchpad.net/ListHelp
