Question about the library - Page 1
Forum section: electronics / general

author: Deridex
author_rank: Regular Contributor
timestamp: October 08, 2017, 08:13:22 am
content: Hello there,The company i work at, used eagle so far.But now we start to use altium because of the increasing project-sizes and some other eagle-specific problems.So my job in the next time is to set the new lybrarie up. We do not want to import our eagle library, because it's faulty at some points and it's somewhat chaotic.So my question to you guys is now:Looking at your own library, what thing would you avoid in the future?orwhat decision do you regret when i t comes down to the library?Thanks in advance for the info

author: Fire Doger
author_rank: Regular Contributor
timestamp: October 09, 2017, 02:32:38 pm
content: Set up some rules. For ex. Mechanical 13 3D models. Mechanical 29 documentation etc.Use a standard grid for silkscreen (It looks pretty on placement)Add "verified" value to components and update it after production to know that footprint is 100% correct.Use the most precise 3D models, may save a lot of time on placement and collision errors.Some supplier links makes loading laggy.If your pcbs are so dense that you can't fit printable designators you can place a text '.designator' and use a mechanical layer for documentation.Use (custom) templates where you can, they save you a lot of time and results are great (graphics, titles,index, design notes, bom, draftsman if you like it)You will figure out soon what works best for you.Just don't make wrong footprints or wrong supplier links.I like how feranec makes them, I think he has some tips about them in YouTube.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 09, 2017, 03:00:55 pm
content: Import is okay, by the way. You have the wonderful opportunity to review and qualify every component, and set a consistent design style. Complex and nice footprints can be saved. Poor ones can be corrected. Bad ones can be skipped.Imports are always on weird layers, and bring a lot of fluff that you don't need. Like, Eagle imports might bring separate "cream" (paste) and component outline and body layers, and so on, along for the ride. Several of those you'll want to either delete (paste is automatically derived from the pads), reassign (component outline --> Mechanical 13), or clean up (avoid silkscreen on pads, use clean lines and arcs?). Some of this can be done en masse: with the Filter and Inspector panels, you can select objects in all footprints in the library and change them all at once.Follow a naming convention. You can have separate library files for classes of components, drawn along whatever lines you like: manufacturer (AD's built in libraries do this), component type (passives, ICs, connectors..), or a monolithic, catch-all library.Naming is the most notable change I've made, in my personal library, over the last, hmm, I've been using AD for 7 years I think? I had also gone through and made some graphical changes. I don't have such a large library that I can't remember all what's in it, but having parts and footprints categorized by purpose makes it much easier to find them. I used to name things by generic (e.g. "R0805" for SMT chip resistor) or part number ("CMS1" for a certain SMT choke), now I've added categories ("IND_CMS1", "CAPAE63X60", "SOIC-8", etc.).Oh, and don't use underscores everywhere. Or ALLCAPS. It's terribly ugly. The 1990s are over. No one needs short file names, caps, space-free names, or anything like that. You are free to make your files smooth and presentable!(Okay, a quirk in my system, I maintain ALL_CAPS and underscores in footprints. I think footprints are still one of the informational backwaters in the world, unfortunately. To be fair, ALLCAPS looks better in stroke font, and is still traditional on mechanical drawings. My component libraries are easier reading though, like "Ind FB 1206 390R 2A", which is short and descriptive.)Tim

author: free_electron
author_rank: Super Contributor
timestamp: October 09, 2017, 03:39:27 pm
content: on the Schematic side :-Draw everything ON-grid.- name symbols properly- for generic symbols (npn , pnp) use a format likeTRANSISTOR-NPN-1B-2C-3ETRANSISTOR-PMOS-1G-2D-3D-4D-5S-6S-7S-8SIC-GENERIC-7404IC-GENERIC-555The first one is npn transistor with pin 1 base ,2 collector and 3 emitter.Make the pin permutations as you need themSecond on is a mosfet in 8 pin SO package- for other parts use a format likeIC-AD-AD693IC-TI-TPS76033-SOT23IC-TI-TPS76033-DFN10First on is a ad693. it only comes in one packagesecond one is available in multiple packages so you add on the package nameon the PCB : define first a set of standard layers.a mechanical layer for the 3d modela courtyard layeran outline layera comment layermake sure to leave an empty layer between them so you can set up automatic mirroring in the PCB editor when you swap parts from top to bottom layername the footprints according to IPC7351 and in the description give the 'human names'for example:SO127P490-14N SO-14 narrow bodyRESC1206N : Resistor, Chip, 1206Make an integrated library that now points to the correct symbol and correct footprint and attach all the relevant data in the integrated library. This allows you to re-use symbols and footprints.The easiest way is to create a microsoft access (or other ODBC ) database and simply create tables. One for resistors, one for caps, one for ic's etc. You bind Altium to the database.If you add information to a part ( like a digikey or mouser or whatever link ) Altium will write directly to the database .you get nice categorised libraries without needing to compile them.your entire parts library is a set of PCBlib gils, SCHlib files and a mdb file.shove those in version control and done.

author: Ice-Tea
author_rank: Super Contributor
timestamp: October 09, 2017, 04:54:21 pm
content: Some things others may or may not agree with:- I use the manufacturer part# (minus options like reel/tube/whatever) as unique identifier. If needed, I add alternatives as parameters. Like this, you avoid confusion about suitable replacements: nothing is a suitable replacement untill it is deliberatly added. Per example, if you make a components C_POL_100uF_16V_D this leaves the door open to any number of "matches". Or will become ambiguous if you have more than one match.- Stick to pin-numbers in footprints. Don't do B,G,D or anything. It doesn't work.- Add supplier parameters. Your board house will thank you.In my own experience, if you mount a library that is on a server, it will make it dog slow. Have server with the libraries on if you must and duplicate locally. And manage permissions.

author: Deridex
author_rank: Regular Contributor
timestamp: October 09, 2017, 04:57:19 pm
content: Quote from: Fire Doger on October 09, 2017, 02:32:38 pmThanks for the info, i will look up feranec at youtube. The other stuff you mentioned makes sense alsoQuote from: T3sl4co1l on October 09, 2017, 03:00:55 pmThe actual plan is to look through the actual eagle library and create the actual used components in the new altium-library.We consider the new library as a big chance to fix the errors that have been done till now. But if we just import, we won't have the 3D-Models etc.You guys made some good points and i will see if i can make it happen that way.Thanks !PS: Till now im used to ALLCAP_WITH_UNDERLINES. Let's see if i can get rid of this habbit

author: Ice-Tea
author_rank: Super Contributor
timestamp: October 09, 2017, 04:59:57 pm
content: Forgot to mention, I assume I may get blasted for this, but I have always liked the description on DigiKey. Quite often, I just copy it as the description for my components. It has the advantage that you immediately have consistent descriptions without thinking about it.