Hello Lorenzo.
> Better to use the minus-dash, especially if you want to use the > underscore for subscripts. Of course. I was unprecise. Yes, i mean the minus dash like this one: "-". > I actually use all caps, but if the library > code is sane, everything should work. You think about the BZR4646 Problem at eeschema? There is a Python3 skript to convert the schematics. Look at http://www.mikrocontroller.net/wikifiles/3/33/PyKiCad-CaseSensitiveLibCure_RevC_21Mar2014.zip But read the readme file. > Stick with the dot. Since Win95 there is no trouble using it inside the > name. Comma works too, just decide (AFAIK the period is the most used > around). Of course, but personally, i am mistrustful. I am a hobby paranoiac. ;O) > > Can be done only for footprints with S-expressions.Where is the problem? > > All the new footprints are sexp based and you can > regenerate them from the collection boead without issues. You and i, but there many people who are stuck to older kicad versions for a while. > > 7. Naming should be done from the general to the special. Like > > "Transistor_TO-220_HorizontalInLine_FromSolderSide.kicad_mod" or > > "Transistor_TO-220_HorizontalInLine_Standard.kicad_mod" or > > "Transistor_TO-220_Vertical_Standard.kicad_mod" as an example. > > Need a naming convention for that. Yes! And there is also the possibility of staggering the pins in different ways, like TO220-5. At least perhaps i would not be sensefull to create an official library for any possible case, but there should be EXIST A NAME for it, if it should occure sometimes. > FromSolderSide doesn't exist, BTW. > Everything must be drawn from component side looking down. > Any other way to do it would be foolish. Yes. But for this you need a special footprint, if you not only mount from the solder side, but also have special positions, like a TO220 mounted from the solderside with the heatsink away from the board, so you can place the board upon a heatsink an attaching the TO220 to this heatsink. The special footprint will show you this X-raying through the board, perhaps with a dashed silkscreen outline on the top silkscreenlayer or a "normal" outline at the solder side silkscreen. > Mostly needed for hor/ver mounting *and* for > pin variants (123 vs EBC vs GSD) So special remarks like EBC or GSD should be omitted. To seldom in use. Who this needs, can easily create this by themself. I would only distribute the numbering from documents regarding only the housing without connection to any special device. Everybody has to look for his used devices, wether they fit to this footprint. If somebody needs often needs such a spechial footprint, he can easily create this by themself. At my beginning of making KiCad modules, i was stuck to the Eagle thinking, too. But then i noticed the advantage of having small libraries for housings only, not for each device, like eagle. Maybe, if you youse the same devices very very often (like BC846 as an example) > > Wave/THT are process variants, should kept in *different* libraries with > the same name. Same for packages designed for 8mil process vs designed > for smaller processed (yes, they change depending on the process limits, > too:D) I think more about "finding fast in library". My thinking ist more like "Diode > Standard > SMD > Housing Type. but of course, your way is also ok. > > > But there is also an other abroach to name footprints. Starting with the > > housing name. Like "TO220-2" for diodes or "TO220-3" for douple diodes > > or transistors, triacs ec. More special differences are the same like > > above. > > Right:D 123, EBC, GSD, AnK, A1KA2, and so on... No. Omitt this EBC GSD or so thing. You would get very big labyrinthic librarys. > Part 1, section 1.8. I have the italian edition so I don't know the > original title. It contains the rules for cad systems, I wrote about > that a wole ago. Thank you. > > > And origins should be at the symmetrical center of the symbol. This is, > > because in this case, the symbols will not jump around wild, if you turn > > them (around the origin). It is more easily to place them. > > Placing the origin to the symmetrical center of a point symmetric symbol > > (like an ordinary resistor) is quite easy, but if you have a symbol, > > which is only symmetrical, the origin should lie upon this symmetrical > > axis, but its exact position is not so easy to determine. So i suggest > > for practical purposes, place the origin upon the symmetrical axis > > somewhere near where you would expect the barycentre, if this symbol > > where a real objekt. > > Don't sweat too much over that. "More or less in the middle" for > schematic is a good enough specification. Yes, "More or less in the middle" is ok, but tell the people why. And at last generally pin 1 as anchor is a bad Idea. > PCB modules OTOH have rules, > if you want to follow them (already wrote about these, too) > Other components would benefit from the 'demorgan' option: opamps with > + and - swapped to keep the power supplies in order (V+ on top, V- on > bottom), for example. Other ones would benefit from *multiple* pin > positioning. How many typical configuration does a 555 have ?:P I thougt about: For a small schematic i prefare to have the 555 black box with all pin positions at the right position. So it will be fast to recognize the pins at the real IC for error hunting. if i do not have the pinning in mind. Also it is no problem to show the V+ and V- in the black box. Showing V+ and V- is also important if i use different isolated V+s and V-s.... But in a big schematic, without different V+s and V-s i would perhaps show the V+ and V- pins in a partial component, to reduce the complexity of the schematic. > > Another policy decision: power supplies. Some people use them on the 'A' > component, some other use a locked part just for that, to do a sheet > with supplies and bypass banks. Really no standard here. De morgan is seldom used here, because there are no more big locical gates boards around anymore. Only one or to logical ICs besides the controllers, and there is no need for demorgan. Personally i prefere a special partial component for the power supply. > > Hidden power pins: IMHO worth absolutely *nothing*, just don't use them > :D reason: more often than not (except on doing a pure logic board) > there are many supply rails. On pure logic board too, often you need > a ferrite/inductor to filter the supply so you need to pull out the > supply anyway. And having the pin gives a way to show what bypass cap > goes were. I agree! > > The "Value Text field" is for the Value of the component. Like "1k5" for > > 1500 Ohm or "1k5/0,5W/RM10" for a 1500 Ohm, 0,5 Watt resistor for Grid > > RM10. It should be prefilled with the name of the symbol, like > > What do you mean 'grid RM10'? Remember that designators and values go > into the BOM, too. I'd use "1K5/0W5" for that (but manually typed, it > makes no sense to type the *whole* E192 series (given that some people > only use E12 or E96...) It was just an example. :D But i think that the "Value Text field" should be prefilled with the name of the symbol for symbols and the name of the footprint for footprints. > > "T....". Why not using the offical way (if it exists), and whom like it > > an another way, could change the reference by its own. > > Read above. There are at least two official designator tables, add to it > the IPC one (never seen it in use) and the regional one. Of course. "T" is an ancient german regional code. IPC is realy strange. Especially for footprint naming.......to clumsy for practical work. > Troublesome thing here: I'd say follow the IPC calculated pattern from > the JEDEC sizes for standard packages. A SO-8 suggested by TI could be > bad for soldering a SO-8 from another manufacturer. So the SO-8 package > should be drawn from the MS-12 (IIRC) sizes and then computed using the > IPC rules on the target technology. IPC calculations would be the best. But in former cases, where no IPC calculation existet yet, but different manufacturers, this was my prefered way. > > Of course special packages (like the flat IR mosfets) have to follow the > manufacturer pattern. IXYS is starting with such packages, too. But i have to look further, wether they match with the IR types in some way. They are more like "flat packs" as far as i can see. > I put as a suffix the pin ordering (in relation to the standard > ordering), so while usually you use a TO92-EBC a swapped part could be > TO92-CBE. In fact TO92 transistor existed in all six permutation, some > time ago :P Yes. As i started makin KiCad footprints, i started with TO92. :D and soon i discovered, that it has no sense to make footprint in all permutations. But just inverted could be an exeption. > > For footprints, it is even more crucial to set the origin to the > > symmetrical center, like it is for symbols. They will not only jump > > paround at turning, they also would produce pick and place files for smd > > with a nasty offset. I think, this will fit IPC-7351, despite i do not > > own an exemplar for looking. > > Yes, IPC7351B has a rule for the origin. See previous posts. > > > Of course, but where will you append the reason exact. Not in the name, > > i think, i think more in a commit? > > I'd keep these technology variants in different libs. No. I thought about "where do you specify this reason"? Not where do you store this footprint. :D With best regards: Bernd Wiebus -- 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
