[SCH Symbols] Connecting Hidden Pins To Shown Pins  - Page 1
Forum section: electronics / general

author: Pseudobyte
author_rank: Frequent Contributor
timestamp: July 07, 2017, 02:30:15 pm
content: First off, I just wanted to say that I am loving this community.I am wondering if it is possible to connect a hidden pin on a schematic symbol to a shown pin. Is there some sort of net naming convention that I can use internally as to avoid issues when the component is placed into a schematic. The main issue being that the supply rail or GND or what have you isn't named as you did in your symbol. I bring this up because I would rather not have to place symbols for power MOSFET packages that have 8 pins with 4 Drain pins and 3 source pins. I want transistor symbols that only show 3 pins!In writing this post I also found the answer to my problem. There isn't one.Apparently one solution is to stack pins on top of one another, but who wants to do that.This seems like a terrible fail on Altium's part. Feature request?

author: voltsandjolts
author_rank: Unknown
timestamp: July 07, 2017, 02:49:19 pm
content: Hiding pins just leads to trouble IMHOShowing all pins might not be pretty but it will be correct.

author: Pseudobyte
author_rank: Frequent Contributor
timestamp: July 07, 2017, 03:03:26 pm
content: I don't think it would be an issue if you could connect them explicitly to other pins in your symbol, but alas you cannot. I understand the problems it will cause as it currently functions. But it would be nice to draw actual 3 pin schematic symbols instead of the monstrosity that you would create with 8 pins hanging out. Perhaps you are correct in that it is still likely you will make mistakes and it is safer to show everything. From an engineering perspective I think it makes a lot of sense to collapse it to it's three basic pins. From a layout perspective I see the risks and concerns for hiding pins. It's a horse a piece I suppose.

author: kony
author_rank: Regular Contributor
timestamp: July 07, 2017, 04:46:57 pm
content: Simple answer.Don't do that.Each physical pin on PCB has to be matching 1:1 its schematic representation, or you are asking for a big trouble long term (not just debug, servicing or returing to old design after few years as well). For simple semiconductors just refactor the symbol with required n drain or source pins - takes literally seconds, same with the schematic entry (not to mention you are likely to reuse schematic snippets over and over again). For larger devices you are doing CSV import of the pins very likely anyhow.

author: ajb
author_rank: Super Contributor
timestamp: July 10, 2017, 11:39:16 am
content: If you give all of the corresponding pads the same designator, then a single schematic pin will connect all of them. Of course this means that your PCB symbol must be created to suit the component; a generic footprint won't work.

author: julianhigginson
author_rank: Frequent Contributor
timestamp: July 11, 2017, 10:46:53 am
content: I can imagine a single pin with multiple pin numbers beside it (say 1,2,3) would do the job and not kill anyone. But that'd be a new feature in altium, and who knows what else it would break. better to just stick with 3 pins doing the same thing in a schematic... here's something I did recently for a part that's 2 mosfets mashed together in 1 nine-pin (well, 8 pins plus a gnd pad) package ... I don't feel good about it, but it works...though this thread made me think about it... (maybe i should read threads here more often...)I can go in and edit each pin and set the pin number position to have each number away from the others (spacing of 6 seems to work for me) Then set the length of ALL those pins to be at a multiple of 10 longer than the biggest pin number position, and then stack all the pins of the same net on top of each other.. making sure the electrical snap point of each is in the same position...I can then lay all the pins together and I expect that in the schematic they will all get connected together as one. The weird visual thing here is that of course your multi pin will get a junction placed on it when it's simply connecting to a single wire...et voilàit's a shame that I can't have commas in there to separate the pins... that said, anyone looking at this part drawing and the part datasheet and losing their mind over not being able to find pin 1234 and pin 678 on a 3.3mm square 8 pin SON with ground pad, is going to be having plenty of other problems with any schematic they are given..

author: ajb
author_rank: Super Contributor
timestamp: July 11, 2017, 05:17:00 pm
content: Quote from: julianhigginson on July 11, 2017, 10:46:53 amYou could just hide the designators entirely and place a string that says "1,2,3" or whatever. I have a vague memory of seeing this method in an Altium doc somewhere. Of course this means that the displayed numbers are no longer tied to the pin designators, but since the pin numbers are defined in the lib, that shouldn't matter unless you're changing pin numbers in the schematic sheet or something.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 11, 2017, 10:48:41 pm
content: 1. Show all pins.This is the most specific, leaving nothing ambiguous or, God forbid, hidden, on the schematic.Remember, the schematic is a document. A language. It conveys information. Hide as little as possible! Do not make it a challenge for the reader to figure out what you're doing!2. Use a normal symbol, and a modified footprint (renumber pads so they get set to the same net).This requires duplicates of some footprints, but is one of the slickest compromises between what-you-say and what-you-do. It's not at all unreasonable for SOT-89 and SOT-223 parts (where the tab is almost always physically connected, at the surface or in the lead frame).3. Hide pins and connect them up manually.This is the greatest risk for making a mistake, in the first place just because it's tiresome to do in Altium, and subsequently because you need to set each pin on each copy of each part that this is done on. It's so bad, I suspect it's a case of: "well, we'llallow youto screw this up, but you're doing it at your own peril."4. Set the pins to multiple pads in the footprint editor. (Lie)Sadly, Altium does not have this feature. It's been requested basically since AD came out. Others have it (even Multisim / Ultiboard has one-to-many pin mapping). Still, nothing... (Well, unless they're addressing it in v17 or 18, I don't know. Seems doubtful.)5. Set the hidden pins to additional nets.This isn't directly applicable, but on a related note: you can set hidden pins to an arbitrary net name, then place that net name on the schematic elsewhere (with a Net Label) and connect to it, or apply a class or rule or whatever.Tim

author: ajb
author_rank: Super Contributor
timestamp: July 13, 2017, 04:59:10 pm
content: Quote from: T3sl4co1l on July 11, 2017, 10:48:41 pmBy coincidence (or perhaps because of this thread?) someone has just observed that this is by far the most popular feature request on BugCrunch:https://bugcrunch.live.altium.com/#Bug/317