Quickly adding schematic component values compared to Eagle - Page 1
Forum section: electronics / general

author: euzer
author_rank: Regular Contributor
timestamp: June 17, 2020, 03:15:52 pm
content: Sorry if this has been asked before, but unsure how to search for this specific question.I'm an AD newbie and currently moving from many years on Eagle to AD20. During schematic entry in Eagle I always roughly drop the components to get the circuit for the first pass, net them, then will go back around later and change values, typically for passives, and if required replace the package. The way the component library in AD has been set up for us (each value package combination is a specific component) I have to search and choose a specific value component with a specific package and place that. I find this process very long-winded and slows down getting something representative of what I want on 'paper'. To change a (resistor) value retrospectively I have to delete the component and add a new one from the library, rather than changing a value field in the schematic. There must be a more efficient way of working than doing this?

author: E-Design
author_rank: Regular Contributor
timestamp: June 17, 2020, 03:48:13 pm
content: What I do is make a generic resistor library component where I leave the value and MFG part# blank. And I attach all the footprints I want to it. 0603, 0805 etc..I can quickly drop that into a schematic everywhere I want and just type in the value. It is super fast.Later, once I figured out what I really need, I then can go in and assign a real part number so my BOM for ordering is correct.Of course, as you have seen, the cleanest way is to have each component fully specified in the library. But you don'thaveto do it that way if you want some rapid prototyping.I used to use Eagle years ago, so I am familiar with how quick Eagle can be. I can assure you Altium can be just as quick but I honestly think Altium can be faster to put a schematic together.

author: voltsandjolts
author_rank: Unknown
timestamp: June 17, 2020, 07:58:43 pm
content: This might speed things up a little for you;My library of common Yageo 805 and 603 caps / resistors which all have Farnell and Digi-Key order codes.

author: alexwhittemore
author_rank: Frequent Contributor
timestamp: June 22, 2020, 02:34:27 pm
content: Quote from: voltsandjolts on June 17, 2020, 07:58:43 pmReal Gent, here!I concur with E-Design here. The preferable scenario is that you have a fully-qualified component in your library with the proper value, footprint, and sourcing info ready-to-go. Pending that, I ALSO use a generic component that has the bare minimums (0603 resistor, 1210 unpolarized cap, etc). I'll typically go back through and either replace those with fully qualified components if I have any, OR just use the "manufacturing" panel to find a part number, then "associate manufacturer info and component data" to what's on schematic.THAT SAID, I usually about this differently and actually put in the legwork up front. Rather than spit schematic onto the page then go back and fill it in, I try to make it fully qualified as I go (at least in Altium, where that's much easier than say Eagle or KiCad). That's because, particularly with caps, I want to KNOW that the "0603 10uF cap" I just put down actually exists, and can be purchased, which frequently isn't the case.I find it a little too easy to forget that I "guessed" at the 1uF 0402 or whatever it was, did all the layout on that assumption, THEN realized at the end of layout that I have to go back and change it because I can only find an 0805 of the appropriate parameters. This is doubly true for almost anything other than a resistor or cap - you can't just throw down a "generic" QFN microcontroller and fill it in after the fact. Inductors are ALWYAS a different footprint depending on value and current rating.If you REALLY prefer the Schematic>BOM>Footprints>Netlist>Layout workflow like KiCad really adheres to, I think you can do that with Altium using SchLibs+PCBLibs rather than IntLib or DBLib. But then you give up a lot of time savings and potential BOM headache reduction by doing so, which is why I don't prefer it. I'd way rather specify the component when I'm thinking about what it does and why I put it there.The one counterexample is resistors: I almost always just throw down a generic 0402 or 0603 depending, then fill them back in one by one later from the manufacturing panel. That's not much of a problem, since your chosen value is almost ALWAYS available in whatever package you like, and in stock, unless you've got a specific power rating in mind.