Altium: Where can I get reliable PCB footprint and schematic symbols? - Page 1
Forum section: electronics / general

author: matrixofdynamism
author_rank: Regular Contributor
timestamp: April 27, 2023, 04:08:35 pm
content: There are a lot of places on the internet to get schematic symbol and PCB foot prints. I just wish to know from the experts, what is the most reliable source of ready-made PCB footprint and schematic symbols for use with the Altium Designer?

author: ajb
author_rank: Super Contributor
timestamp: April 27, 2023, 06:06:00 pm
content: I'd recommend making them yourself for the most part, especially if they're for professional/production design work. That allows you to a) not have to rely on anyone else getting them right, b) make sure everything is consistent in terms of layer usage, line widths, pad styles, etc etc, c) prepare for when you can't find a ready made footprint or symbol for the part you want to use, and d) forces you to really look at the part drawings/datasheet and take the time to understand the part before using it. Take a bit of time to set up your library templates and primitive defaults up front, and once you get the hang of it the whole process isn't too bad. I'll also take a moment here to evangelize about dblibs, which make reusing footprints and symbols very easy and are generally very efficient when it comes to library management.For standard IC footprints I had been using PCB Library Expert, but that's no longer free. Altium's built-in footprint generator has improved, so I'll likely use that going forward. I'll occasionally use Wurth Electronik's PCB libraries because they've been fairly consistent and reliable, but still end up tweaking them a bit for consistency with my existing library.

author: asmi
author_rank: Super Contributor
timestamp: April 27, 2023, 07:25:45 pm
content: Yep, want something done good - do it yourself. This is especially so for schematics symbols, because the same component can be drawn a multitude of ways depending on your preferences or your company standards and best practices.

author: thm_w
author_rank: Super Contributor
timestamp: April 27, 2023, 09:38:30 pm
content: You made this same thread last year and got answers then:https://www.eevblog.com/forum/altium/where-can-i-find-reliable-libraries/https://www.eevblog.com/forum/altium/improper-import-of-schematic-symbol-or-footprint-from-ultra-librarian/

author: VK3DRB
author_rank: Super Contributor
timestamp: April 29, 2023, 01:27:52 pm
content: Consider doing your own. I tend to do them myself because they are better than almost all the public domain footprints.For example, I always use small filled triangles as pin 1 markers because they are superior to round circles. A triangle points to the pin 1, it is clearly distinguishable from vias, fly vomit or a spec of dust, it is much more discernible even when it is tiny for those with marginal eyesight, and reduces ambiguity in a dense circuit layout. I see no justification why many engineers prefer the antiquated circles, other than the "that's the way we always have done it" mentality or lack of experience maybe.Another thing is I use rounded rectangles for pads on QFICs, TSSOPs, QFN's etc because sharp corners can promote the growth of dendrites when not conformally coated. I also find often the component manufacturer's recommended footprint is not great, so I tend to adjust them as appropriate. I generally follow QPC standards, but often deviate for good reasons.Speaking of footprints, large QFICs should be oriented at 45 degrees to how the paste will be squeegeed onto the footprint. This is to increase yields by reducing voids caused by paste starvation due to paste that might be a bit old or other reasons. I have done this in many products, including very high volume products (ie: >100,000 build quantities) with great results.I always aim to use the component's correct 3D model. I never use extruded 3D models in Altium. Besides the obvious, another advantage is the 3D model double checks my pin spacing, size and location. For 3D models, the manufacturer's website is the first port of call, followed by Octopart, 3D Content Central, SnapEDA etc. For some components, I have had to email the manufacturer to get the 3D model, but that is rare. I have had to make my own step files on occasion, but I avoid it because of the time it takes because and I am no proficient at complicated mechanical CAD.

author: mengfei
author_rank: Regular Contributor
timestamp: June 25, 2023, 08:19:02 am
content: add to altiumhttps://www.samacsys.com/pcb-part-libraries/orhttps://www.snapeda.com/altium-libraries/orhttps://altiumlibrary.com/GetStartedYour Welcome

author: free_electron
author_rank: Super Contributor
timestamp: June 27, 2023, 09:41:56 pm
content: try the celestial altium libraryhttps://github.com/issus/altium-library

author: tszaboo
author_rank: Super Contributor
timestamp: June 27, 2023, 10:08:59 pm
content: Quote from: free_electron on June 27, 2023, 09:41:56 pmThat looks really nice, I'll definetly take a closer look at it.OP: The other good source of components is built right into Altium. You have to do a "Manufacturer part search" on one of the panels.