Reduce clutter and confusion in schematics. Any tips?  - Page 1
Forum section: electronics / projects

author: FotatoPotato
author_rank: Regular Contributor
timestamp: September 26, 2018, 04:27:52 am
content: Hi all,So I’m currently working on a pretty large, multi page schematic for a 4 channel high power linear power supply, based off of Dave’s uSupply tutorial series. I recently switched from eagle to Altium Designer 18 and so far I’m loving it. The only problem is that my schematics are getting petty messy and borderline unreadable. Do you guys have any tips for cleaning up a schematic and making it more presentable?Thanks

author: Richard Crowley
author_rank: Super Contributor
timestamp: September 26, 2018, 04:40:47 am
content: You can take many valuable cues from large, complex schematics posted online for free study.Two prime tips I would offer1) Make named, "bubble" connections to common power, ground, etc. buses or nodes. vs drawing them endlessly threaded throughout the schematic. There are common symbols for connection to ground And there are even several types of ground symbols if you have separate analog vs. digital ground etc.2) Separate the schematic into logical blocks and label the input and output nodes which connect to like-named nodes in other blocks of the circuit Avoid taking this to the point of breaking the circuit up into small chunks that don't really make sense "out of context".

author: DaJMasta
author_rank: Super Contributor
timestamp: September 26, 2018, 05:09:19 am
content: Logical blocks is good, using several sheets is good, using larger (not letter, but legal sized) sheets is good to space things out. Depending on the part libraries you're using, you can also sometimes find parts that have a better layout of pins for your schematic or that are just physically smaller.Don't know if this is the bubble connection thing mentioned above, but use ports for attachments between different parts of circuit that are straightforward or are far away/on a different sheet. You can make them for any signal line, but you can make power ports for all your rails and you can define buses to bundle several connections into a single port.Maybe look around for some more complicated schematics, perhaps a service manual for a piece of test equipment that has them, and see what techniques they use. Generally with spacing, organizing parts, labels, and using multiple sheets, you can get it to be very readable, and all of this is supported in altium.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 26, 2018, 02:01:25 pm
content: I once wrote up a set of rules,https://www.seventransistorlabs.com/tmoranwms/Elec_Circuit_Rules.htmlalthough the original purpose isn't of much use to me anymore (it's been a long time since I used Paint for schematics!), many are applicable in any system.A few are more stylistic and I don't even do things that way anymore, but it's a good starting point.Regarding multi-sheet and hierarchical design, try to keep minimal connections between sheets. That means organizing sub-circuits by sheet, so the dense connections within the sub-circuit are shown on the sheet, and the signals in and out of it are connected with Off-Sheet Connectors or Ports.Avoid using net names (or other objects, but net labels are the worst offender) to connect nets arbitrarily. It's unavoidable in a multi-sheet design, but that's no excuse for a confusing, disorganized layout using them!Tim

author: FotatoPotato
author_rank: Regular Contributor
timestamp: September 26, 2018, 02:11:48 pm
content: Thanks for all of the info guys, this helps a lot! With regards to signals connecting between sheets I have that mostly covered. Each sheet is sort of “self contained” in the sense that all the connections except the input and miscellaneous voltage rales are only in that specific sheet, so there is no interconnection between any of the sheets except the AC-DC sheet that has the voltage rails on it. But even then, I’m just using the GND and rail symbols so I don’t think that will be a problem. It’s more just a issue of, lots of connections crossing each other and going all over the place in each sheet and it makes it look like a rats nest. I think the fact that I was doing this at 2am didn’t help eitherThanks again, the help is much appreciated

author: ajb
author_rank: Super Contributor
timestamp: September 26, 2018, 02:58:58 pm
content: Complicated schematics often need to be spread out so you can better see what's going on and more easily start to disentangle things. Sometimes you need to bump up a sheet size or three to have more room to rearrange things (the fact that you can't move objects off of the sheet in Altium is really annoying), and then once you find a cleaner way of laying things out you can tighten everything back up and shrink the sheet size.Personally, I hate Alitum's default graphical style. It's hideous, and the component sizes are excessive, which forces some awkward layouts. I made my own symbol library with everything a consistent size, a mostly grayscale color scheme, and a monospace font. It makes it a lot easier to create schematics that are compact but legible and (in my opinion) substantially improves the visual appeal of the schematics.Sometimes you can clean up schematics by using graphical buses, especially when a bunch of signals have to run from one side of the schematic to another. In this situation, you use net labels to establish connectivity between the two parts of the schematic, and the bus wire just provides the visual guide, showing where those signals go.Harnesses are also quite nice for handling collections of signals, especially between sheets.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 26, 2018, 03:26:06 pm
content: https://www.seventransistorlabs.com/Images/555%20Boost.pdfHere's a nice clean example of my current style, including custom libraries (because, yep, the built in libraries are ugly as sin), uniform spacing around components, and correctly positioned component labels. (Pet peeve: Altium's default label positioning is uncontrollable and seemingly intentionally off center. Ugh...). The placement rule I use here is, DC flows vertically, signal flows horizontally, at least one grid space around every component/label and wire (two preferred, for example the feedback wire at the bottom). Minimum turns/bends/junctions, junctions made in tees only. Labels centered above or below horizontal components or justified beside vertical components, where possible.I've also adopted a color scheme, light blue for discretes, light yellow for integrated parts. Keeps things interesting without making a printing problem (say for B&W output).This could be crammed together a lot tighter if more arbitrary positioning were used (5 grid, say?), but it would be far less readable. I've got a whole sheet to work with in this case, no big deal.It does get a bit interesting when cramming a lot onto a single sheet. A job earlier this year really pushed that; I just barely crammed two channels onto a single sheet without it getting too ugly. Any more than that and I would've split it up. (At least that two-channel design has an obvious split. It can be difficult to divide more integrated circuits onto sheets though. You may simply give up and use a larger sheet size in that case -- it'll still view electronically just fine, and should still print fine, most especially if you have a multi-size printer.)Oh and, yeah, this latter example would be infinitely more useful with a visual example, but... unless the customer wants to release it for public viewing, I'd rather not...Tim

author: SiliconWizard
author_rank: Super Contributor
timestamp: September 26, 2018, 05:34:13 pm
content: Quote from: T3sl4co1l on September 26, 2018, 03:26:06 pmNot bad really.Close to publishing quality. I don't particularly care for the yellowish background for ICs that Altium seems to be fond of, but other than that, I like it.