My suggestion would be to follow the naming convention of Tom Hausherr's library tool ("Library Expert"):
Please don't use this incomprehensibly verbose convention. Library Expert is
fantastic and gets so many things right, but this isn't one of them. It solves the easy problems for you, and makes the harder part of the problem worse, keeping you reliant on Library Expert for help.
When you're assigning footprints to components, there are two things to check:
- Have I selected the right footprint for this component?
- Is that footprint drawn correctly?
So for your 0603 resistor, problem 1 is making sure that you pick an 0603 footprint instead of 0402 or 0306 or 0805 or whatever. Then problem 2 is making sure your 0603 footprint in your library is good for actually soldering an 0603-sized part to. #2 is more difficult: drawing good footprints can sometimes take a while. And they must be maintained, for example when library standards change. In contrast, #1 is really easy: just read the datasheet and pick out the correct footprint from your library. The rub is that you must do operation #2 once per footprint you draw; you probably have dozens to hundreds of footprints. But #1 applies per
component, and you have thousands to tens of thousands of those!
Library expert makes #2 super easy: it draws perfect footprints perfectly well. It makes #1 very difficult, because it assigns stupid names that cannot be quickly audited. If you are using a SOT23-5 op-amp from TI, with TI package code DBV, and I see that the assigned footprint is "
JEDEC MO-178 AA (SOT23-5)", I'm happy! If I see "
TI DBV-5", I'm also happy! If I see that footprint "
SOT23-5P95_280X145L45X40" has been assigned, I... have no idea if that's right. I mean, sure, it looks approximately correct, but those are the worst to audit... is 280 correct? 145? I don't know. Time to spend some quality time with TI's drawing, I guess
.
So it's relatively easy to check that footprints named this way are drawn according to their names. It's quite difficult to check that they are assigned properly to parts, and because that is the more common task, I strongly dislike this approach to library organization. Instead I prefer:
- Draw as many footprints as possible to standards (JEDEC, JEITA, EIA, ... ). Qualify manufacturer packages as equivalent to these standards, which is usually quick and easy (and we have a database that saves the association), and then you can use one standard footprint to replace a dozen or more manufacturer footprints. Name them as suggested above: by the standard and by the common name: "JEDEC MO-178 AA (SOT23-5)".
- When official standards do not exist (or are practically unobtainable, like EIA passive sizes) and defacto standards exist, take a few minutes to define a GENERIC footprint that covers 95+% of the market and use as above. Example naming: "GENERIC SOT-89" or "CHIP RES EIA 0603/1608M".
- Nonstandard or oddball parts are, if reused at all, usually only reused within one manufacturer. So draw them up as manufacturer-specific, and index them by manufacturer: "TI DBV0005A" so the next time you're stuck using a DBV0005A from TI you know you've already got it covered. This also works fine if you don't recognize something as standard... it's just a footprint tailored to one vendor. Nothing wrong with that.
The actual
drawing of the parts can be handled by Library Expert... I just never use its names, because I cannot audit them as being correct to apply to parts. My goal is to draw as few footprints as possible, of as high a quality as possible, and use them as often as I can. This way, if you change op-amp vendors but keep the same part, you won't be stuck with a silly tool telling you the footprint ought to change by a few microns!